F405 & F411 versions of the BluePill

The only devices which would fit on such a small board are the F411, which does not provide substantially more processing power than the F103, as its clock speed is only 100Mhz.

The F411 is worse than the F103 for signal acquisition, as it only has 1 ADC (the F103C has 2)

The F405 is a much better processor, but is is not available in a package that would fit on the Blue Pill form factor without using a 4 layer board.
But 4 layer boards as many times more expensive than 2 layers – some PCB plants seem to change 10 times as much for 4 layers.

The other option is to use a BGA version of the F4xx, but these parts are hard to source as they have minimum order quantities of several thousand (probably 1 reel)

And… As has been pointed out by Chris Micro, you can buy a Teensy 3.6 for $19 USD, which is also on a very small form factor, and outperforms most STM32F4 MCU’s

Hence I’m going to park this, as its not worth the time and effort.

_______________________________ Original post ______________________________________

Following form a discussion with @lkcl about creating a STM32 board which is mechanically compatible with the Arduino Due,
http://stm32duino.com/viewtopic.php?f=9&t=2630
the possibility was raised of getting a F4 version of the Blue Pill made by a Chinese manufacturing house.

As the STM32Stamp Eagle design files were published several years ago. ( http://eleccelerator.com/stm32f4stamp-breakout-board/ )

I’ve taken these files and run them though the Eagle2KiCad converter and put the resultant files on Github

https://github.com/rogerclarkmelbourne/ … ill_Boards

In the F405Pill folder

The current status of the files is that the PCB fails DRC because it looks like some vias are not connecting to the filled GND zone on the bottom layer.
I’ve not had chance to figure out why this is happening, and I think perhaps all the via’s to GND may need to be replaced.

So far I’ve made one change to the schematic, as it looks like the USB D+ was missing the 1.5k pullup to 3.3V that is required by the USB Spec and important if the board has to re-enumerate the USB.

Although the PCB looks good, its wide than the Blue Pill which is a problem on breadboards as there is only 1 row of pins available on each side.

Which makes me wonder if it would be possible to rotate the F405 by 45 deg and perhaps use a 4 layer board for routing – as it would be impossible to route on a 2 layer. However I’m not sure if this would help or worth the additional cost.

The other thing which seems to be making the board wider is are the decoupling caps, and the power LED and its series resistor.
I think that if the LED and resistor are moved, and all the tracks re-routed, the width could be reduced a bit e.g. probably by 0.1 inch at least

If a power LED is needed at all, I’m sure it can be positioned elsewhere

One other omission, seems to be the 32khz crystal. I think there is space on the board for this, and I presume as its low frequency, that the tracks to the crystal don’t need to be ultra short.

F405Pill.pdf

(84.56 KiB) Downloaded 81 times

But i’ve also got a bluepill with an F411 on it, and there are also compatible F401, F410, F412 & F413 for it (especially the F413 is ridiculous. 1.5Mb flash, 320kb RAM, and tons of peripherals (but of course you’re still limited to the 36 IO pins…)

the soldering is a PITA, as these are QFN chips, but if you’ve got a hot air station, it’s doable.
And the only other thing you need to do, is put a capacitor on pin 22 (PB11), as on the 4 series it’s an extra capacitor for the internal voltage regulator, and not PB11 (which isn’t present..)

see thread here: viewtopic.php?f=39&t=1658

little extra not (initially?) mentioned in that thread: the bluepill is the only good board to do this on. The maple mini’s pads don’t fit the QFN chips, andn the blackpill is REALLY annoying since it has smd caps right next to the stm32, so changing the stm32 also means you’ll be removing the caps, and then have to get them back on >_<.

bluepill411.jpg (16.88 KiB) Viewed 3953 times

Thanks

I think perhaps the 41x on the BluePill form factor would be better than the F405 on the larger form factor, as there are plenty of larger F4 boards around.

I just looked on AliExpress, and the F411 is available for $4, no one seems to sell the F413 etc

I’ll have a go at entering what we have for the BluePill schematic into KiCad and post to a different repo

http://wiki.stm32duino.com/images/c/c1/ … ematic.pdf

I was just looking at the schematic symbol in KiCad and I could not find an VDDA (analog supply for ADC I presume) but the 411 doesnt seem have that

Re: ADC’s
Umm. Thats not so good.

Perhaps the F405 is a better option after all, as I can’t see any of the 64 pin F4’s that have more than 1 ADC (but its really hard to see from STM’s product selector as it doesnt list the actual number of ADC’s in the selector table)

[zoomx – Fri Sep 29, 2017 8:00 am] –
Two suggestions:
1) a reset circuit Maple Mini like or better
2) Power led with solder pad that you can cut to disable for low power.

Reset circuit I think can be a PFET, I think thats what the Seeed Studio Maple clone uses, I’ll try to find their schematis

Re: Power LED

Is it even necessary ?

Also
Boot1 is not really needed, it can be permanently pulled low.
Perhaps it can double as USB DISCONNECT

SIngle transistor USB reset

BTW. I think STM have a single NPN transistor reset circuit on some of their Nucleo’s now.

I’ll see if I can find that… Though I think a PNP may be a better

[RogerClark – Fri Sep 29, 2017 8:12 am] –
@racemaniac

I was just looking at the schematic symbol in KiCad and I could not find an VDDA (analog supply for ADC I presume) but the 411 doesnt seem have that

Re: ADC’s
Umm. Thats not so good.

Perhaps the F405 is a better option after all, as I can’t see any of the 64 pin F4’s that have more than 1 ADC (but its really hard to see from STM’s product selector as it doesnt list the actual number of ADC’s in the selector table)

All the chips have advantages & disadvantages ^^
I’m happy with the f411 for my projects, but it indeed depends on what you need

might also one day have a go at drawing out a compact board for a bigger f4 chip with more pins .

[RogerClark – Fri Sep 29, 2017 8:14 am] –
Re: Power LED

Is it even necessary ?

No but in other post I read of it’s presence. If present it’s better ti have a pad to cut.
All low power projects start with cuttin or desoldering the power led, Arduino pro mini and ESP01, for example. TI Launchpads use jumpers but I believe that a simple cutting pad does the work in a cheap board.

OK. That should be easy, just have a track thats easy to cut…

Re: USB enumeration

Rick. So… You’re saying that we don’t need a USB re-enumeration circuit or external 1.5k pullup as its all under SW control ?

https://github.com/rogerclarkmelbourne/ … r/F411Pill

All I’ve done so far is to enter the schematic.

Its currently throwing a load of DRC errors, but this not not unusual for MCUs which have loads of pins, some of which aren’t used.
But I”ll need to double check if any of the errors are valid

I wonder if it may be worth making it 22 pins per side or perhaps 24 pins per side as I think there are more GPIO’s available on the F411 than can be fitted on the 2 x 20 pin connectors.

BTW.

I don’t see any point in having Boot1 on a jump link, as loading into RAM is virtually useless. I guess I could route to a pad in case someone really wants to pull it high, but jump links cost money, and waste space

[RogerClark – Fri Sep 29, 2017 4:54 am] –

The current status of the files is that the PCB fails DRC because it looks like some vias are not connecting to the filled GND zone on the bottom layer.

after seeing what kind of damage KiCAD can do (long story…), is it ok in Eagle’s DRC?

Which makes me wonder if it would be possible to rotate the F405 by 45 deg and perhaps use a 4 layer board for routing – as it would be impossible to route on a 2 layer. However I’m not sure if this would help or worth the additional cost.

yehhh 2-layer boards particularly ones with only 12mil clearance and tracks, and 12/24-mil VIAs, are extraordinarily low-cost and can be prototyped in 24-48 hours. 4-layer… yyyeah… not worth it.

One other omission, seems to be the 32khz crystal. I think there is space on the board for this, and I presume as its low frequency, that the tracks to the crystal don’t need to be ultra short.

some clean GND tracks surrounding them, and treating XIN and XOUT effectively as diff-pairs… and definitely no VIAs… should be fine.

l.

[racemaniac – Fri Sep 29, 2017 6:15 am] –
the soldering is a PITA, as these are QFN chips, but if you’ve got a hot air station, it’s doable.

the intention for this design is to make use of shenzhen-based component sourcing and assembly, so that people who are in the West can get decent pricing. also as it’s an open board anyone would be able to do assembly themselves (and prototypes too). sigh yes QFNs are a pain…

[zoomx – Fri Sep 29, 2017 9:36 am] –

[RogerClark – Fri Sep 29, 2017 8:14 am] –
Re: Power LED

Is it even necessary ?

No but in other post I read of its presence. If present it’s better ti have a pad to cut.
All low power projects start with cuttin or desoldering the power led, Arduino pro mini and ESP01, for example. TI Launchpads use jumpers but I believe that a simple cutting pad does the work in a cheap board.

are the 32.768 khz XTAL lines likewise potentially useable as GPIO? i remember that being the case on the 072. question is, would people _want_ to use them as GPIO?

[lkcl – Fri Sep 29, 2017 11:27 am] –

[RogerClark – Fri Sep 29, 2017 4:54 am] –

The current status of the files is that the PCB fails DRC because it looks like some vias are not connecting to the filled GND zone on the bottom layer.

after seeing what kind of damage KiCAD can do (long story…), is it ok in Eagle’s DRC?

As a KiCad user, i’m now wondering what you’re talking about XD

[lkcl – Fri Sep 29, 2017 11:27 am] –

Which makes me wonder if it would be possible to rotate the F405 by 45 deg and perhaps use a 4 layer board for routing – as it would be impossible to route on a 2 layer. However I’m not sure if this would help or worth the additional cost.

yehhh 2-layer boards particularly ones with only 12mil clearance and tracks, and 12/24-mil VIAs, are extraordinarily low-cost and can be prototyped in 24-48 hours. 4-layer… yyyeah… not worth it.

12 mil clearance & tracks seems quite big for something bluepill sized.
i’ve been working 6/6 mil with 24 mil vias, and i think that’s what services like elecrow/dirtypcb/…. support, so also dirtcheap if you go 2 layers. (maybe for some it’s 25 or 27 mil for the vias, not sure, the one i used was ok with 24 mil)

USB disconnect: the MapleMini’s version seems to me the best (2 transistors) as it toggles the 1k5 resistor only if the 5V USB is present. The versions with a single pnp or pfet do not have this option..

Boot1: I am using it (PB2 on BPill) for USB disconnect (pfet). It works fine..

32Khz clock: the RTC’s PC15/14 (BPill) are special pins with lower fanout (see datasheet). The wires to the 32KHz resonator shall be kept short and off the other signals as it is “low” power, thus prone to catch noise.. I think these wires have to have GND guard ring around them..

ADC: mind the agnd/gnd, avcc/vcc topic

[RogerClark – Fri Sep 29, 2017 10:22 am] –
Re: USB enumeration
Rick. So… You’re saying that we don’t need a USB re-enumeration circuit or external 1.5k pullup as its all under SW control ?

It seems that way, based on information in the reference manual
RM0090 wrote:
34.3.2 Full-speed OTG PHY
The embedded full-speed OTG PHY is controlled by the OTG FS core and conveys USB
control & data signals through the full-speed subset of the UTMI+ Bus (UTMIFS). It provides
the physical support to USB connectivity.

The full-speed OTG PHY includes the following components:
• FS/LS transceiver module used by both host and device. It directly drives transmission
and reception on the single-ended USB lines.
• integrated ID pull-up resistor used to sample the ID line for A/B device identification.
• DP/DM integrated pull-up and pull-down resistors controlled by the OTG_FS core
depending on the current role of the device. As a peripheral, it enables the DP pull-up
resistor to signal full-speed peripheral connections as soon as VBUS is sensed to be at
a valid level (B-session valid). In host mode, pull-down resistors are enabled on both
DP/DM. Pull-up and pull-down resistors are dynamically switched when the device’s
role is changed via the host negotiation protocol (HNP).
• Pull-up/pull-down resistor ECN circuit. The DP pull-up consists of 2 resistors controlled
separately from the OTG_FS as per the resistor Engineering Change Notice applied to
USB Rev2.0. The dynamic trimming of the DP pull-up strength allows for better noise
rejection and Tx/Rx signal quality.
• VBUS sensing comparators with hysteresis used to detect VBUS Valid, A-B Session
Valid and session-end voltage thresholds. They are used to drive the session request
protocol (SRP), detect valid startup and end-of-session conditions, and constantly
monitor the VBUS supply during USB operations.
• VBUS pulsing method circuit used to charge/discharge VBUS through resistors during
the SRP (weak drive).

however all these boards won’t outdo the conventional blue pill or maple mini which slots nicely on a breadboard
that in part as r* and v* chips has lots of pins and if one wants all the pins it would be pretty tough to fit that nicely on a breadboard

Thanks for the links.

I think that breadboard compatibility is quite important, and boards with double rows of pins close to each other are generally hard to use unless you design your own PCB motherboard for your project to use them

The STM32STAMP F405 board is not too bad but its not hardware compatible with the motherboards that people are building to use the BluePill

I think I will try to stick to the BluePill form fator, but this may only be possible if I use a F41x device.

I would consider using a BGA decice, but As far as I can tell they are not any smaller than either the QFLP packages that the F41x or F40x are available in.

Rick.

I will remove the pullup resistor, and add the 32khz osc crystal etc

[racemaniac – Fri Sep 29, 2017 11:58 am] –
As a KiCad user, i’m now wondering what you’re talking about XD

yyeahh… to be honest, if you’ve never tried doing 400 to 600 pin BGA packages on 6 to 8 layer boards, you’ll do absolutely fine. however if you’ve used a proper CAD package which has Design Rules – and i mean *decent* Design Rules… KiCAD is a hell of a shock.

12 mil clearance & tracks seems quite big for something bluepill sized.
i’ve been working 6/6 mil with 24 mil vias, and i think that’s what services like elecrow/dirtypcb/…. support, so also dirtcheap if you go 2 layers. (maybe for some it’s 25 or 27 mil for the vias, not sure, the one i used was ok with 24 mil)

i’ve used eurocircuit’s lowest-possible prototyping service and was really impressed (quality and price). the default rules are… chunky though good for a 5x7in PCB with only 100-150 components on it. yeah i didn’t realise the bluepill form-factor is really quite tiny, isn’t it? 6 mil should be absolutely fine. if going below 12mil drill hole sizes i’ll have to ask mike’s advice on what’s cheapest.

CPU clock speed is listed at 100Mhz, which is not a lot faster than the F103, albeit my be more effecinet per clock, and has FPU

I think I should concentrate on the F405, and try to make it fit the Blue Pill form factor ( though this may be impossible)

I will need to see what physical size the BGA package is, but its got loads of pins ( 176 I think), so its not going to be that small.

So perhaps the Blue Pill form factor is unachieveable

BTW.
Re: KiCad

I have not had the luxury of using something like Altium so for me, KiCad stacks up very well compared with my 2 year old copy of Eagle ( commercial basic version)

[lkcl – Fri Sep 29, 2017 8:57 pm] –

[racemaniac – Fri Sep 29, 2017 11:58 am] –
As a KiCad user, i’m now wondering what you’re talking about XD

yyeahh… to be honest, if you’ve never tried doing 400 to 600 pin BGA packages on 6 to 8 layer boards, you’ll do absolutely fine. however if you’ve used a proper CAD package which has Design Rules – and i mean *decent* Design Rules… KiCAD is a hell of a shock.

i have indeed noticed there are a lot of issues with the kicad DRC ^^’
if i look at eagle cad design rule files, there already seem quite some more settings available than what kicad has.
And seeing the push & shove router sometimes still causing violations, or seeing violations reported that don’t seem to make sense, i can imagine that for complex pcb’s, it quickly becomes hell ^^’

The F405RG on its own costs nearly $6 and to squeeze it onto the Blue Pill size board, would require a 4 layer board, with components on both sides of the board (the Blue Pill already has components on both sides, but is a 2 layer board.

So overall, it would probably end up costing at least as much as the larger F405 boards i.e around $10 more than the Blue Pill

I’ll probably put some designs on GitHub for people to check, but I doubt its worth getting a quote to get them manufactured.

https://www.pjrc.com/store/teensy36.html

[ChrisMicro – Sat Sep 30, 2017 3:49 am] –
Is the performance in the range of a teensy 3.6?

https://www.pjrc.com/store/teensy36.html

No. Only the expensive F4’s have run at 180Mhz.

I think the price for the Teensy 3.6 would be virtually impossible to complete with.

Its not worth taking this any further as its uneconomic.

I’ve updated the first post and marked this as closed…

[RogerClark – Sat Sep 30, 2017 2:25 am] –
I’m coming to the conclusion, that to get a F405 or F407 onto a form factor which is the same width as the Blue Pill, would probably result in a board costing more than people are willing to pay.

The F405RG on its own costs nearly $6 and to squeeze it onto the Blue Pill size board, would require a 4 layer board, with components on both sides of the board (the Blue Pill already has components on both sides, but is a 2 layer board.

https://world.taobao.com/search/search. … TM32F405RG

this is the china-equivalent of ebay so volume pricing may be lower: general offers are around the $3 to $4 mark. does that help?

[lkcl – Sat Sep 30, 2017 7:14 am] –

[RogerClark – Sat Sep 30, 2017 2:25 am] –
I’m coming to the conclusion, that to get a F405 or F407 onto a form factor which is the same width as the Blue Pill, would probably result in a board costing more than people are willing to pay.

The F405RG on its own costs nearly $6 and to squeeze it onto the Blue Pill size board, would require a 4 layer board, with components on both sides of the board (the Blue Pill already has components on both sides, but is a 2 layer board.

https://world.taobao.com/search/search. … TM32F405RG

this is the china-equivalent of ebay so volume pricing may be lower: general offers are around the $3 to $4 mark. does that help?

Thanks, but the problem is that the 405 simply won’t fit in the Blue Pill form factor

[RogerClark – Sat Sep 30, 2017 7:21 am] –

Thanks, but the problem is that the 405 simply won’t fit in the Blue Pill form factor

…. won’t fit *at all*… or are you endeavouring to maintain pin-compatibility with the blue pill? the reason i ask it, it was pretty clear from looking at the mega2560 arduino reference design that the entire pinout was designed around… the mega2560. tracks go dead straight, in clear, clean groups, no vias whatsoever. when it came to the 417 (and also the sam3x) the difference is astounding: i’m lucky to have been able to complete the routing *at all*. several areas are a bit… dicey.

so the question in my mind is: are you endeavouring to keep pin-compatibility, because if so yes that would be near-impossible. howeverrr… if creating something that’s pretty much just a break-out board – redefining the pinouts but simply keeping the size – i would be hugely surprised if that didn’t work. and… i’d like this to work

looking at my breadboards <edit>with a BP plugged in</edit>, one side has 2 holes open, the other 3, i suspect most people could live with 2 + 2.
just checked, had to rummage to find a BP
minor fly in the ointment, there is good width outside the BP headers to accommodate the silk screen identifiers.
that almost covers inside hole of the pair, using a slightly longer pin length would ease that a lot though.
a really nasty one, use an even long length header and enough force to bend in to fit such that it would be 3 + 3 holes available, or even 4 + 4, if only slight bend desired, increase pcb width by 0.3″ with 2 + 2 holes to use
ok, that’s a tad too far!

something i do with the wide mounting versions of ESP8266 is using 2 breadboards from the SAME source, they are not all created with equal spacing of the locking tabs, or push/pull wire into/from hole resistance; is to reassemble them with a single power bus between the big body parts of the breadboards. P power strip, B main body.
normal is P-B-P-P-B-P, mine P-B-P-B-P, maybe even P-B-P-P-B-P – too wide for ESP8266 – i tried.
be honest, who’s only bought one breadboard ?

stephen

I could not get a viable routing solution on a 2 later board.

I think it would probably work on a 4 layer board, but the cost of a 4 layer board means no one would buy it, as there would be plenty of cheaper F4 boards which were a different / larger form factor on 2 layers boards.

And as Chris pointed out, the Teensy 3.6 is faster than any F4 MCU I could fit on the Blue Pill form factor and is only $19.

So if anyone wants good performance on a Blue Pill form factor their best option would be to buy a Teensy 3.6

I reason people use the STM32 is because the F103 is dirt cheap and significantly faster than the ATMega328.

If they want more performance and dont need good ADC or DMA etc, then they should probably be looking at the ESP32

[RogerClark – Sun Oct 01, 2017 11:10 am] –
And as Chris pointed out, the Teensy 3.6 is faster than any F4 MCU I could fit on the Blue Pill form factor and is only $19.

30$
19.80$ is the Teensy 3.2 price .

lots of questions

ideally the size would be small enough to fit 2 of them on a 5x5cm pcb (then at dirtypcb you can have 20 of these boards manufactured for <20$ including slow shipping)

.. I just pointed out that there is the Teensy 3.6 and its performance should be compared to a new BluePill-replacement. I didn’t mention the price.
But I think Paul Stoffregen ( the developer ) put really a lot of effort in his software so he really deserves to make some money with his products.
I was thinking of porting some of his software to the STM32 but I decided not to do it for this reason.

[racemaniac – Mon Oct 02, 2017 2:29 pm] –
i’m going to give it a try to make a 2 layer pcb with a 405 on it, and not too large. lets see how (im?)possible this is.
Do i try to break out all pins, or only certain pins? what would the requirements be?
for myself i’d break out the major ports (i2s (= also spi), i2c, uart, …), and whichever other pins are convenient for the format.
i’d try to put an micro sd slot on the pcb (but thus not expose the sdio pins otherwise).
32khz crystal for rtc required or just a nice to have? (how many people actually use it?)

lots of questions

ideally the size would be small enough to fit 2 of them on a 5x5cm pcb (then at dirtypcb you can have 20 of these boards manufactured for <20$ including slow shipping)

I tried to maintain pin compatibility.

It may not be completely impossible on 2 layers, but I think the routing may have to be like a bowl of spaghetti.

The F404 footprint that comes as part of KiCad has a keep-out area under most of the middle of the PCB footprint that does make it impossible to route.
I tried editing the footprint and made the keep-out area smaller so that I could have 2 rows of vias around the inside, but this was not enough to allow it to route.

If the entire middle of the MCU was covered in vias it may help.

Also, if the board extended out beyond the width of the pins it would help, but it would then not fit in a breadboard and have much room to plug pins in around the edge.

I put the files on github in case anyone wants to try this for themselves.

BluepillF4.zip

(176.87 KiB) Downloaded 15 times

[RogerClark – Thu Oct 05, 2017 8:38 pm] –
can you post pngs of the top and bottom layers?

you mean like this? (front & back copper layers)

BluepillF405-F.png (20.92 KiB) Viewed 637 times

I think your tracks are several times smaller than the ones I tried to use.

Edit

Looking at your schematic, I can’t see the two 22R USB protection resistors or the 1.5k pullup

Did I miss something?

Edit.

The 1.5k is not needed but I’m not sure about the 22R

You have vias that partially cover pads for the F405 (I think this may be OK but in most cases the vias could be moved so that they don’t do that)

There seems to be a track shorting power and ground between pins 63 and 64?

Looking at a BluePill I think it has a lot more decoupling capacitors than on your board.

[RogerClark – Thu Oct 05, 2017 10:44 pm] –
Are you using a custom DRC ?

You have vias that partially cover pads for the F405 (I think this may be OK but in most cases the vias could be moved so that they don’t do that)

There seems to be a track shorting power and ground between pins 63 and 64?

Looking at a BluePill I think it has a lot more decoupling capacitors than on your board.

the KiCad DRC doesn’t mind vias partially covering pads.
I often do it, but always make sure the drill isn’t too close to the pad (as that’s what causes issues). Heard plenty of advice of preventing the via be in a pad, but slightly touching it?
the board has 6/6 mil tracks/spacing, and 24 mil vias (although reading up on the dirty pcb specs, might have to be 25 mil, but it’s just a quick change)
and there are no shorts. you’re looking at a track leaving pin 64 horizontally i think, there is no short between 63 & 64 (the top plane fill is 3v3, the bottom plane fill is ground)
And i think all required caps etc… are there. but you can have a look at the schematic in the kicad project. it’s just a first try, but seems to be very possible, and i wouldn’t mind using such a board

i indeed left out the resistors, not sure which is and isn’t needed. Adding them is easy. I tried finding more information about it, but it’s pretty unclear >_<. I think the schematic i found for one of the f4 discovery boards had no resistors at all for the usb.

i’m also wondering if it’s not useful to also connect the ID line to the f4, then it can also be usb host.

[ChrisMicro – Fri Oct 06, 2017 5:49 am] –
Long lives the closed thread

it looks like a fun project
wouldn’t mind having some of those boards made, and assembling them myself, they seem like fun little things

might also give it a go to make a more advanced board, not pin compatble, but having a micro sd slot and also breaking out some other pins .

anyone got a clue about what is and isn’t needed in the usb circuits?
checked the f407 discovery board schematic, and it’s got the 22 ohm resistors in series, but it also has this special chip for noise suppresion on usb connected to the line, that also has other resistors in parallel to that, and has some pull up & down resistors >_<

i could always just copy the usb design of the bluepill, it’s not hard adding those resistors below the usb plug.

BluepillF4v1.0.zip

(194.62 KiB) Downloaded 21 times

BluepillF405-F.Cu.png (78.61 KiB) Viewed 797 times

looks good…

Re:Capacitors

The Blue Pill 3.3v rail is quite noisy. I am not sure if the F4 would have the same problems, but if there is space for additional caps, it may be worth adding some more.

I will need to check if the F405 has an analog Vdd input, because if it does, you should have a separate 3.3V reg for that, like the Maple Mini does. The Maple Mini also has a analog Ground input, which is fed though a ferrite core inductor.

The Teensy breaks some pins to pads as its form factor does not have enough through hole pins for all the possible GPIO.

I wonder if there is any space to do the same

[RogerClark – Sun Oct 08, 2017 8:55 pm] –
Re:Capacitors

Yes ! Strongly suggested for any kind of design …

I think its essential to have these separated from the digital Vdd and Vss, as its a major cause of complain with the Blue Pill as it causes poor ADC performance

From what I recall the Maple mini has these but its also a 4 layer PCB. However I know 4 later PCB’s are 10 time the price of 2 layer, so this would need to be achieved on 2 layers.

I know that its more practical to load code into RAM on a F4 than it is on a F1 (assuming thats the function of Boot1 on a F4, like it is on a F1).
Or you could put a small solder pad as well as the resistor in case someone really wants to pull Boot1

AFIK, there is a BluePill variant with just the Boot0 jump link.

Regarding the header etc… i also find it overkill. I’d prefer a board with just a pulldown on those pins, and a small pad for if you want to pull them up for those few times you need that.

I’ve also started designing an F4 board that is not pin compatible with a bluepill, but similar in size, and more functionality.
differences:
– the pins a bit further apart (but the board equally wide)
– the board a bit shorter (<5cm)
– a micro sd slot available
– all pins not used by usb/microsd broken out
– als the id pin of the usb connected (so we could be a usb host?)
– no 32k crystal (but maybe i’ll add pads for the capacitors so you can put the crystal between the pins where it should be, and add the capacitors to the pcb).
i’ll also try to give it a dedicated analog supply .

@victor_pv started work on a bootloader for the F4, and its partially working except its not compatible with the existing F1 DFU drivers and we don’t have a way to reset the F4 from the Serial yet etc etc

However I’m sure it would be possible to have bootloader upload for the F4 is we had time to write it
Its just not high priority for anyone

[RogerClark – Mon Oct 09, 2017 9:00 am] –
Some people seem to have Boot0 permanently pulled high during development so that it goes into USB DFU mode for upload.

@victor_pv started work on a bootloader for the F4, and its partially working except its not compatible with the existing F1 DFU drivers and we don’t have a way to reset the F4 from the Serial yet etc etc

However I’m sure it would be possible to have bootloader upload for the F4 is we had time to write it
Its just not high priority for anyone

would a default pulldown of the pins, with a header to connect the pin to vcc also be good? (or is there a reason they’re always using a pull up/down rather than directly connecting it).
the bluepill design feels a bit overkill for me .

the purpose of the board is different: this one contains all someone could need during a project (tft, sdio, rotary encoder, pushbuttons, leds, ecc)
the schematics is quite complete, there are a few notes around. I never started to draw the board since i didn’t had time

to make this i have been taking ideas from maple mini, olimex, nucleo boards, f405 stamp and a few others
features of the board: usb otg, separate analog/digital, Vbat, tft, rotary encoder, sdio, ecc

i wouldn’t be able to work on it until the new year

Boot1 is also a GPIO pin, so should not be directly connected to GND in case someone accidentally set the pin to High, as it would damage the MCU and potentially affect it booting correctly.
Hence the weak 100k pulldown that gets used.

IMHO Boot0 still needs to be a jumper or potentially a button, but soldering to pads is a pain and can end up lifting tracks off the board if you have to resolder it multiple times.

They will be slightly more expensive, and more difficult to source. They are pretty common on things like hard drives, modern motherboards, set top boxes and the like, so they aren’t that rare.

https://world.taobao.com/item/553628950 … =12#detail

That board does seem to have the F405 on it, however it must be wider and longer than the Blue Pill, because the only way to get the F405 to fit on the Blue Pill form factor (0.6inch between rows of pins), is to not have the MCU at a 45 deg angle

It seems to have 25 pins down each side, rather than the 20 on the Blue Pill

The price is also quite high (around $15), especially since that a TaoBao price not an inflated AliExpress or eBay price

I think that @racemaniac has done an excellent job fitting the F405 onto the BluePill form factor (assuming his design actually works), and I suspect it would be possible to get it made for under $15 if someone has the right contacts in China

not sure what i’ll do with the boot jumpers, i can probably keep them as is, but i find it a bit overkill for the functionality it provides.

i’ve also been looking into the separate analog power supply, how would you guys see that? you’ve got the 3v3, 5v & gnd pin next to the SWD header, my current idea is to separate them from the rest of the board (also removes that stupid trace i have to do all around the board to get the 5V there), and make that the analog supply.
this does however mean that:
– the only other 5V supply is the usb, so there is no direct pin anymore to connect the 5v to? (maybe put one next to the usb)
– unless you actually have a separate supply, the analog supply will be unpowered unless you connect those pins to something.

but if we really want a completely separate supply, the above is the only option i think. or do we still want to share the 5v & gnd lines between both, and only separate the 3v3 (and give it a separate ground & 3v3 line to the microcontroller with extra decoupling caps for less noise)?

I used part of the maple mini schematic when I investigated if I thought it was possible to produce this board.

Basically, VDD_A needs its own regulator and VSS_A needs a ferrite inductor in series with it.

Looking at the board layout, there is space for the regulator and also probably for the ferrite inductor on the back of the board under the processor, but I don’t know how hard it is to get 5V into that location.

GND would be OK, becuase the processor already has lots of GND pins.

I have tried to open kicad PCB file but there seem to be a some short length of stubs of tracks that don’t seem to go anywhere, which seems strange..

e.g. There is a track on the top / front layer from pin 64 of the F405 , almost tracked to a pad on the back (green) but not via’ed

And there is a separate via, overlaying that pad but not linked to pin 64

unattached_tracks.png (112.65 KiB) Viewed 398 times

*edit, checked on my current version of the board (already made some other changes after i posted that version), and it’s okay there .

-option one: a 100k pulldown on it, and a pad connected to it where you can connect it to vcc
-option two: a 100k pulldown, and a 10k pullup with a pad to connect to vcc (as mentioned, boot1 is also an IO, you can’t then short it by connecting it to vcc externally, and putting it to 0 programmatically).
(and for both options, i could also offer vcc pin next to that pin, so not putting the jumper means it’s low, putting it on, means it’s high).
<manager talk> what would be the minimal viable product? </manager talk>
the second option is probably the safest, will work, and if i offer it as a normal pth, you can put a pin on it to connect via a wire to vcc, or solder a wire to it (and remove/solder it back a few times, pth pads aren’t too sensitive).

boot pin proposals.jpg (50.31 KiB) Viewed 369 times

IMHO … Pulling Boot0 directly to Vcc youself using a wire would not be a serious risk.

I presume you will pull Boot1 low all the time via 100k and not have a jumper.

However I womder if its too minimal if you dont have a pin for Vcc next to the pin for Boot0

Or perhaps a smd push button takes even less space, as its only on one side of the board.

[RogerClark – Tue Oct 10, 2017 6:07 am] –
I think that @racemaniac has done an excellent job fitting the F405 onto the BluePill form factor (assuming his design actually works), and I suspect it would be possible to get it made for under $15 if someone has the right contacts in China

yep i can do that. i’ll need the following:

* clear and complete BOM in TSV format, with a digikey column (helps my friend to make sure his suppliers have got exactly the right part. they don’t buy *from* digikey… they just use the website to make sure the spec’s absolutely correct)
* gerbers including drill-drawing, silk screen, solder mask and paste mask.
* board spec (1.6mm, FR4?), also let me know the min track-to-track, min clearance, and min via drill size.
* how many.

[RogerClark – Tue Oct 10, 2017 6:07 am] –

The price is also quite high (around $15), especially since that a TaoBao price not an inflated AliExpress or eBay price

Right, the price doesn’t compare, that’s why I didn’t save it the first time I saw that board, had to look for the link again.
Hopefully between racemaniac and lkcl something can come out that fits the bill.

[RogerClark – Tue Oct 10, 2017 6:07 am] – I think that @racemaniac has done an excellent job fitting the F405 onto the BluePill form factor (assuming his design actually works), and I suspect it would be possible to get it made for under $15 if someone has the right contacts in China

btw, thanks for the compliment
i’m pretty sure this board will work (i’ve already made a few iterations of pretty similar lightsaber pcb’s for myself). However, how stable these will be, how to best prevent noise, … i’m still very new to this, so not sure how qualitative all those aspects will be .
But i’m enjoying learning KiCad and making boards like this, so this is a fun project. Once we’ve come to a final design, i’m going to have some produced at dirtypcb’s, and i’ll assemble some for myself to have a look how well these perform (and you guys can give me things to test).

And i’m always all ears for suggestions on things i should mind on the pcb, or how to do certain things better .

I also noticed that you are using the same regulator footprint as on the BluePill.

From what I can remember, some people complained that those regulators had a habit or turning into firecrackers, but I suppose thats mainly just the current rating.

I looked on my Maple Mini clone and it uses a 3 pad footprint, rather than a 5 pad on the Blue Pill regulator, but I think the overall amount of space consumed on the PCB would be very similar if not exactly the same

[racemaniac – Wed Oct 11, 2017 8:17 pm] –
i’m pretty sure this board will work (i’ve already made a few iterations of pretty similar lightsaber pcb’s for myself). However, how stable these will be, how to best prevent noise, … i’m still very new to this, so not sure how qualitative all those aspects will be .
But i’m enjoying learning KiCad and making boards like this, so this is a fun project. Once we’ve come to a final design, i’m going to have some produced at dirtypcb’s, and i’ll assemble some for myself to have a look how well these perform (and you guys can give me things to test).

And i’m always all ears for suggestions on things i should mind on the pcb, or how to do certain things better .

it really is exciting, isn’t it? you design something on a computer, and then it comes back as a *real thing* that you spent time on. amazing feeling. anyway. yes. if you’re going to do some prototype assembly in the west it would be better to wait until you have a stable board before asking my friend’s factory in shenzhen to do a quote.

it’s one of the things that i’ve learned, it’s very important not to waste people’s time in shenzhen asking them to run around the markets and suppliers for what can often amount to a few *days* worth of their time… and then they don’t actually receive any money from you. that just pisses them off, and if you’ve asked *someone else* to ask on their behalf (such as my friend, the factory owner), if you do it too many times then *their* reputation goes into the “time-waster” bucket as well.

with things like eurocircuits or other “online” PCB factories (eurocircuits has an absolutely fantastic web site btw), much of the “checking” – the factory rules, DRC compliance and so on – can be done by the web site’s back-end. which is awesome. in china they just don’t have anything like that, it’s all done manually.

so… let’s wait until you have a “final” board design, before getting quotes for 10, 50, 100, 1000, if that’s ok?

It looks like one of the companies I know in China may barter some of my programming effort for building some prototype boards for me if I want.

Nothing definite, but it may be a way to get some prototypes for virtually nothing (apart from my time)

[RogerClark – Thu Oct 12, 2017 12:35 am] –
BTW

I also noticed that you are using the same regulator footprint as on the BluePill.

From what I can remember, some people complained that those regulators had a habit or turning into firecrackers, but I suppose thats mainly just the current rating.

I looked on my Maple Mini clone and it uses a 3 pad footprint, rather than a 5 pad on the Blue Pill regulator, but I think the overall amount of space consumed on the PCB would be very similar if not exactly the same

it’s also a 5 pin regulator, but not the same one as the bluepill. The one i’m using is this: AP2112K
i think it’s affordable, and seems pretty ideal for something bluepill like. up to 600mA output current, very low drop off voltage (350mV @600mA, and lowers pretty much linearly with the voltage, so should also be good enough to run this board on Lion cells without having too much of a voltage drop .

[RogerClark – Thu Oct 12, 2017 5:19 am] –
Guys

It looks like one of the companies I know in China may barter some of my programming effort for building some prototype boards for me if I want.

Nothing definite, but it may be a way to get some prototypes for virtually nothing (apart from my time)

very cool. let me know if they’re reluctant to spend the time doing component sourcing: i have two contacts who can help there. they’d both need paying, but…

Its all dependant on whether their client decides to give them the dev work, and at the moment I’m not convinced that would definitely happen.

[lkcl – Thu Oct 12, 2017 1:24 am] –
so… let’s wait until you have a “final” board design, before getting quotes for 10, 50, 100, 1000, if that’s ok?

… btw racemaniac, just to clarify: i’ve seen various hints that if you happen to have the wrong kicad libraries (or the wrong version or just a different version of kicad) you get a completely different output, and of course you can’t see my screen so wouldn’t be able to check. so when i said “when you’re ready send me the gerbers” that was not me being “lazy” (why would i ask you to send me the gerbers when this is an open project and i could just… download the source and generate them myself, right?) it was so that after all the verification and checking that you’ll be doing, you can *guarantee* – because gerbers are a one-way fixed output – that what you send me will be what you get from the factory. does that make sense?

I’ll double check what error I got, but from what I remember the schematic editor seemed to have problems with 2 of the symbols and potentially did some replacements

I think potentially the F405 symbol was different, as the one you are using looks nothing like the one that is in the STM32 libraries supplied with KiCad.

When I updated you schematic to add another regulator for Vdd_A, when I read the updated netlist into the PCB editor, it seemed to replace the footprint of the F405 as if it was a completely new component, and I had to move the footprint into the correct location on the PCB, where you had previously routed all the tracks

So I would be a bit concerned about generating gerbers without double checking what was happening with the footprints

[RogerClark – Fri Oct 13, 2017 5:25 am] –
@racemaniac

I’ll double check what error I got, but from what I remember the schematic editor seemed to have problems with 2 of the symbols and potentially did some replacements

I think potentially the F405 symbol was different, as the one you are using looks nothing like the one that is in the STM32 libraries supplied with KiCad.

When I updated you schematic to add another regulator for Vdd_A, when I read the updated netlist into the PCB editor, it seemed to replace the footprint of the F405 as if it was a completely new component, and I had to move the footprint into the correct location on the PCB, where you had previously routed all the tracks

So I would be a bit concerned about generating gerbers without double checking what was happening with the footprints

Ah, in the schematic i’m indeed using custom libraries. i usually just quickly make my own lib when needing a component, it’s often faster than hunting down an “official” one
but for the pcb i think the files are completely self describing, so that one should show correctly i think?

but i still find it strange, i thought that was the entire purpose of the BluepillF405-cache.lib : the project stores the versions of the libs it uses in there, and no matter if later on they changed or got removed, it’s in that cache file?
ah well, typical open source stuff i guess XD

On KiCad, if you open a project for viewing it will use cached library data, even if it warns about missing libraries (behaviour may depend on version). However, if you modify the project KiCad may reload data from locally installed libraries, which are usually different to the original ones used.

I had a quick look at the recent zip version, it looked ok. If you have a final version, I could order some boards and hand assemble some prototypes.

[RogerClark – Fri Oct 13, 2017 5:25 am] –
@racemaniac

I’ll double check what error I got, but from what I remember the schematic editor seemed to have problems with 2 of the symbols and potentially did some replacements

The 2 missing schematic symbols I think are ok, KiCad finds them in the cache lib (worked for me anyways).

When I updated you schematic to add another regulator for Vdd_A, when I read the updated netlist into the PCB editor, it seemed to replace the footprint of the F405 as if it was a completely new component, and I had to move the footprint into the correct location on the PCB, where you had previously routed all the tracks

So I would be a bit concerned about generating gerbers without double checking what was happening with the footprints

There is a small discrepancy, in the schematic the F405 is “U1”, in the PCB it is called “STM32”. I would rename the footprint in the PCB, then it should match the netlist.

[bobc – Fri Oct 13, 2017 11:21 am] –

When I updated you schematic to add another regulator for Vdd_A, when I read the updated netlist into the PCB editor, it seemed to replace the footprint of the F405 as if it was a completely new component, and I had to move the footprint into the correct location on the PCB, where you had previously routed all the tracks

So I would be a bit concerned about generating gerbers without double checking what was happening with the footprints

There is a small discrepancy, in the schematic the F405 is “U1”, in the PCB it is called “STM32”. I would rename the footprint in the PCB, then it should match the netlist.

indeed ^^’ (did it to have the nice STM32 label on the pcb) (could have also just hidden the reference and added it as text XD, or also renamed the reference in the schematic XD)

[bobc – Fri Oct 13, 2017 11:37 am] –
Would it help if I put together a BOM with Digikey part numbers?

can indeed also be helpful
pretty early in this post i already put aliexpress links of the more uncommon components i was using (voltage regulator, usb connector, …)
Digikey parts can also be useful (although for things like the usb connector i hope it’s some fairly standard thing XD. it’s micro usb connector i bought of aliexpress and that seems to be easy to find. made my own custom footprint for it that seems to work well)

[bobc – Fri Oct 13, 2017 12:20 pm] –
Ok, I looked up those links, the reset button I can’t view (account not authorized). For USB Micro, it’s a bit difficult to work with no brand/no part number and the footprints vary a lot. I will probably replace that with something I can order locally.

oops
here’s a correct link for the button: https://www.aliexpress.com/item/50pcs-3 … 05991.html
chose that one because i had it on hand, and doesn’t require too much space on the pcb, but if there’s a better one to use, that always possible

[bobc – Fri Oct 13, 2017 12:20 pm] –
Ok, I looked up those links, the reset button I can’t view (account not authorized). For USB Micro, it’s a bit difficult to work with no brand/no part number and the footprints vary a lot. I will probably replace that with something I can order locally.

just… don’t get caught out by using stuff that’s *only* available on digikey. sometimes parts end up being ordered like… 10 years ago by a huge customer, digikey stocks 100,000 of them, then it goes EOL and the *only* place left *in the world* with the parts is… digikey. or avnet etc. etc. it may sound mad but my friend mike has often had people design stuff in the US, sending him a BOM and gerbers and expecting him to be able to just… find everything. he has to explain to them that some parts have to be *imported back in to China*!!

as a general rule though if it’s a very common part, chances are that there will be multiple suppliers, and the vendors know what’s compatible and who to get it from without you needing to specify exactly which random china supplier happens to have it. if you just put in the digikey P/Ns my friend’s suppliers use it to cross-reference and look up a suitable identical part. you would be absolutely amazed: some of them memorise 5 to 10,000 parts including a full current price-list. incredible.

[racemaniac – Fri Oct 13, 2017 12:24 pm] –

[bobc – Fri Oct 13, 2017 12:20 pm] –
Ok, I looked up those links, the reset button I can’t view (account not authorized). For USB Micro, it’s a bit difficult to work with no brand/no part number and the footprints vary a lot. I will probably replace that with something I can order locally.

oops
here’s a correct link for the button: https://www.aliexpress.com/item/50pcs-3 … 05991.html
chose that one because i had it on hand, and doesn’t require too much space on the pcb, but if there’s a better one to use, that always possible

sigh no datasheet, no manufacturer, no part number. pain in the ass to source and find. that would require a trip to Huaqiang Rd markets, to show someone there the photos and ask them to identify it.

bottom line: don’t do it. use something that’s got a part number and manufacturer, like this one:

SKHMQKE010. ALPS Tactile Switch 6.2×6.5×3.1mm SMT

http://www.alps.com/prod/info/E/HTML/Ta … KE010.html
http://eu.mouser.com/ProductDetail/ALPS/SKHMQKE010/

[bobc – Fri Oct 13, 2017 11:37 am] –
Would it help if I put together a BOM with Digikey part numbers?

YES. or farnell / mouser in a pinch. the sourcing rule is:

* find it on digikey, avnet, farnell or mouser first (doesn’t really matter which)
* check the datasheet for suitability
* then go to aliexpress and taobao and search for the part number.
* if it’s got dozens of suppliers of that EXACT part, without there being piss-take prices, it’s good.

if instead you do the following i will NOT help you, because i know it will require several WEEKS of pissing about and possibly actually having to go personally down to the Huaqiang Rd markets, which will mean i have to apply for a 5-day Shenzhen visa, pay for a flight to HK and so on.

* make random arbitrary searches on aliexpress
* don’t provide part numbers, manufacturers, or datasheets

basically whilst the Futian District market suppliers may actually have the full datasheets, their internet access is so piss-poor that they maintain them in an offline fashion ONLY, storing them on laptops and PCs in the tiny 1.2 x 1.5m booths that they actually have to climb over the half-inch thick reinforced glass counters to get in and out of.

so if you want their help you have to email them (in chinese), or you have to go down there personally and show them pictures or actual parts. i apologise but knowing how long that would take, i’m not going to do it (or pay someone else to do it). so please, KEEP THE BOM TO DIGIKEY / MOUSER / FARNELL parts ONLY then check their availability / pricing on aliexpress / taobao, ok? learned that one a long, long time ago.

[lkcl – Fri Oct 13, 2017 1:09 pm] –

[racemaniac – Fri Oct 13, 2017 12:24 pm] –

[bobc – Fri Oct 13, 2017 12:20 pm] –
Ok, I looked up those links, the reset button I can’t view (account not authorized). For USB Micro, it’s a bit difficult to work with no brand/no part number and the footprints vary a lot. I will probably replace that with something I can order locally.

oops
here’s a correct link for the button: https://www.aliexpress.com/item/50pcs-3 … 05991.html
chose that one because i had it on hand, and doesn’t require too much space on the pcb, but if there’s a better one to use, that always possible

sigh no datasheet, no manufacturer, no part number. pain in the ass to source and find. that would require a trip to Huaqiang Rd markets, to show someone there the photos and ask them to identify it.

bottom line: don’t do it. use something that’s got a part number and manufacturer, like this one:

SKHMQKE010. ALPS Tactile Switch 6.2×6.5×3.1mm SMT

http://www.alps.com/prod/info/E/HTML/Ta … KE010.html
http://eu.mouser.com/ProductDetail/ALPS/SKHMQKE010/

It depends on what your requirements are . For me those are parts i see tons of on aliexpress, and making my own footprint in KiCad once i have one of them isn’t much work (scan it in, put the pads & holes in the right places, and add a few lines to show its size), so that’s why i went for those .

Depending on who wants to make these boards, it can indeed be required to change those components to something they can easily source, but for my requirements, those were good parts .

but indeed, trying to find those items on digikey will be hard >_<. but it’s only the button & usb connector that will be annoying in that respect, all the other things are standard, so we can always in a later stage change those to whatever fits our requirements .

[racemaniac – Fri Oct 13, 2017 1:23 pm] –

but indeed, trying to find those items on digikey will be hard >_<. but it’s only the button & usb connector that will be annoying in that respect, all the other things are standard, so we can always in a later stage change those to whatever fits our requirements .

the requirement is to give the BOM and gerbers to a Shenzhen factory, who will then contact Futian district vendors and have all the parts found and ordered in about 3 days flat. if they have to go randomly searching on aliexpress they’ll simply walk away as they have absolutely no time whatsoever for that sort of thing, given that the profit margins and quantities are really really small.

so – please, follow the sourcing advice that i gave in the previous message, ok?

[lkcl – Fri Oct 13, 2017 1:45 pm] –

[racemaniac – Fri Oct 13, 2017 1:23 pm] –

but indeed, trying to find those items on digikey will be hard >_<. but it’s only the button & usb connector that will be annoying in that respect, all the other things are standard, so we can always in a later stage change those to whatever fits our requirements .

the requirement is to give the BOM and gerbers to a Shenzhen factory, who will then contact Futian district vendors and have all the parts found and ordered in about 3 days flat. if they have to go randomly searching on aliexpress they’ll simply walk away as they have absolutely no time whatsoever for that sort of thing, given that the profit margins and quantities are really really small.

so – please, follow the sourcing advice that i gave in the previous message, ok?

If one of you guys has experience with making a good selection of button/usb connector, go for it, i’ll use it in the design (both are ideally sturdy and not too big ).
And wouldn’t just blindly picking something from digikey/… be bad? ideally we’d know what the guy in shenzen can easily and cheaply source, and use that . not some obscure digikey item that he might not even be able to find.

[racemaniac – Fri Oct 13, 2017 2:04 pm] –
If one of you guys has experience with making a good selection of button/usb connector, go for it, i’ll use it in the design (both are ideally sturdy and not too big ).
And wouldn’t just blindly picking something from digikey/… be bad? ideally we’d know what the guy in shenzen can easily and cheaply source, and use that . not some obscure digikey item that he might not even be able to find.

that’s why i said, (1) check on digikey and mouser and farnell FIRST (2) THEN check on aliexpress and taobao SECOND.

the reason is very very simple: aliexpress and taobao suppliers completely fail to provide datasheets and proper references, but they’re a good indicator of availability and pricing.

so you use BOTH… but treat aliexpress and taobao as “unreliable”.

BluepillF4v1.0b.zip

(207.58 KiB) Downloaded 10 times

[lkcl – Sat Oct 14, 2017 10:43 am] –
Untitled1.jpg

are you able to separate these (vertically), moving them apart so that GND can flood-fill between them? i fuss about things like that.

… hang on… those traces go from red to green with nothing in between! you can move the bottom two to green! or… are you using that jump so as to get GND in there? you should be able to get GND in through the use of some stitching VIAs instead – some above the middle red trace and some below. then you could move both those two green traces to *above* the third (top) red one….

it’s the fill that goes around them that’s important, and indeed, the ground has to go between them to get to the top ground pin of the stm32

[lkcl – Sat Oct 14, 2017 10:41 am] –

[racemaniac – Sat Oct 14, 2017 5:40 am] –
Ok, i’ll use that one
I’ve become convinced that there is no intersection between the connectors i see on aliexpress and those i see on digikey XD. i found 1 set of connectors that were very close, nearly identical footprints, but you could physically see on the foto’s that they weren’t identical >_<.

*sigh* yehhh that’s why it’s safer to find a mass-produced (common) part. if it’s not actually amphenol it’ll be a cloned-version-of-an-amphenol part… good enough

you’ve got a part number and a manufacturer for that reset switch in the BOM, right? (or… does anyone else know who makes it? google image search?)

yup, this is the reset switch: https://www.digikey.be/product-detail/e … ND/2747186
same one as the bluepill i think, and easy to find both on digikey & aliexpress

[lkcl – Sat Oct 14, 2017 10:38 am] –
looks really neat and tidy for such a damn small board that’s only 2 layer. dang.

some suggested mods which will fill in those white areas. red dots are VIAs on the green area, green dots are VIAs on the red area, i made them opposite colours so they stand out. rerouting (blotch, blotch, hand-drawn GIMP…) shown which works around the proposed VIAs. 3 green, 5 red just so you have an exact tally. obviously i don’t know if they’ll actually work, you’ll have to check that. can i also suggest putting some stitching VIAs along the bottom outer edge. you can’t put any on the top edge because there’s tracks running along the top.

only other thing: this isn’t 480mbit/sec USB, is it? the fact that the USB traces aren’t diff-pairs has me concerned. if it’s only USB 1.1 speeds (12mbits/sec) it should be fine, but if it’s USB2 480mbit/sec then that’s going to be radiating noise like buggery, even if they are really short tracks.

copper layers (1).png

i’ll have a look at your routing suggestions, but the places where there is no fill, is usually also places where it doesn’t really matter. if there’s no pin needing the gnd/3v3 near there, going out of your way to get the fill there is kind of stupid ^^’
and it’s indeed just slow usb. for high speed usb it’s a lot more pins & an extra chip to get to those high speeds.

[lkcl – Sat Oct 14, 2017 10:38 am] –
some suggested mods which will fill in those white areas. red dots are VIAs on the green area, green dots are VIAs on the red area, i made them opposite colours so they stand out. rerouting (blotch, blotch, hand-drawn GIMP…) shown which works around the proposed VIAs. 3 green, 5 red just so you have an exact tally. obviously i don’t know if they’ll actually work, you’ll have to check that. can i also suggest putting some stitching VIAs along the bottom outer edge. you can’t put any on the top edge because there’s tracks running along the top.

The top & bottom fill are different, the top is 3v3, the bottom is ground (so both have a nice connection trough the entire board. I think that what you’re proposing would be if both were the same? then you can indeed stitch them together to form an even better ground plane across the board.

i’m making some more improvements to the routing so it’s all even tidier
also added two more capacitors as the 3v3 pins without ground next to them of the stm32 didn’t have their decoupling cap yet

[racemaniac – Sat Oct 14, 2017 11:36 am] –
yup, this is the reset switch: https://www.digikey.be/product-detail/e … ND/2747186
same one as the bluepill i think, and easy to find both on digikey & aliexpress

aaaawesooome. that makes the difference between a straightforward buying stint (about 2-4 days) and a whole lot of arseing about, email back and forth with lots of translation into chinese in the mix.

[racemaniac – Sat Oct 14, 2017 12:45 pm] –

[lkcl – Sat Oct 14, 2017 10:38 am] –

The top & bottom fill are different, the top is 3v3, the bottom is ground (so both have a nice connection trough the entire board. I think that what you’re proposing would be if both were the same? then you can indeed stitch them together to form an even better ground plane across the board.

ahh ok – yehyeh what i proposed was if they were both GND.

one more thing i’m not sure about if we need to specify something is the ferrite bead connecting analog ground with the normal ground. I know 0603 size beads exist, i currently use a 0603 capacitor footprint for that, but don’t know much about the specs of such beads.
I saw the original maple mini also uses a small smd one (probably also 0603), anyone know if/what we should specify for it?

copper layers.png (107.53 KiB) Viewed 170 times

• Not sure I am looking at the latest schematic, but make sure you have PA12 as USB D+ (not PA11!)

• I think the pullup on D+ (R8) is not needed on F405, since there is a pullup internal to the CPU. I would leave the footprint for other devices, but mark it “no fit” for F405.

• If R8 is required, it should pull up to 3.3V, not 5V.

[bobc – Sat Oct 14, 2017 3:00 pm] –
Looks good Some notes:

• Not sure I am looking at the latest schematic, but make sure you have PA12 as USB D+ (not PA11!)

• I think the pullup on D+ (R8) is not needed on F405, since there is a pullup internal to the CPU. I would leave the footprint for other devices, but mark it “no fit” for F405.

• If R8 is required, it should pull up to 3.3V, not 5V.

thanks for checking everything out, will be correcting those errors . took the 5V pull up from the bluepill schematic, but i guess that’s wrong then ^^’

BluepillF4v1.0d.zip

(184.66 KiB) Downloaded 13 times

[racemaniac – Sat Oct 14, 2017 3:56 pm] –
And here is a first go at the BOM:
BluepillF405 BOM.xlsx
I hope xlsx is not a problem for you guys to open?

software libre developer here…. 25 years experience of reverse-engineering and working with embedded systems: i have a tendency to automatically reject proprietary or even non-proprietary file-formats that add a thousand percent or greater overhead, and require applications ten to a hundred thousand times larger than the actual data being viewed. if there’s a choice between “install source code of some program” and “install some f***witt multi-megabyte GUI gunk just for viewing a damn file”… which do you ya think i’m gonna choose?

also: google the “father sylveste response” regarding presenting people with the unsolicited assumption that you have – or wish to use – vast amounts of computing resources for document viewing and editing. father sylveste is (was?) a jesuit priest who wrote an extremely respectful way of making people aware of the full implications behind *assuming* that sending people arbitrary and proprietary binary-formatted documents is good for the recipient *or the sender*.

short version: gimme TSV or TXT, dude…

[lkcl – Sat Oct 14, 2017 5:00 pm] –

[racemaniac – Sat Oct 14, 2017 3:56 pm] –
And here is a first go at the BOM:
BluepillF405 BOM.xlsx
I hope xlsx is not a problem for you guys to open?

software libre developer here…. 25 years experience of reverse-engineering and working with embedded systems: i have a tendency to automatically reject proprietary or even non-proprietary file-formats that add a thousand percent or greater overhead, and require applications ten to a hundred thousand times larger than the actual data being viewed. if there’s a choice between “install source code of some program” and “install some f***witt multi-megabyte GUI gunk just for viewing a damn file”… which do you ya think i’m gonna choose?

also: google the “father sylveste response” regarding presenting people with the unsolicited assumption that you have – or wish to use – vast amounts of computing resources for document viewing and editing. father sylveste is (was?) a jesuit priest who wrote an extremely respectful way of making people aware of the full implications behind *assuming* that sending people arbitrary and proprietary binary-formatted documents is good for the recipient *or the sender*.

short version: gimme TSV or TXT, dude…

as an excel developer i know the basic openxml format of xlsx is open and well documented ^^. (there are some legacy old excel support things in there the libre community complains about, but those are only used in in old documents)
but i’ll provide a csv

here you go:

BluepillF405 BOM.csv

(1.87 KiB) Downloaded 142 times

I think @rikkimball also posted about the USB D+ pullup not being required.

I checked the F4STAMP schematic, and its not present that board, but I think we need to check a few more F4 schematic to be absolutely sure

@racemaniac

Was it impossible to route a pin for the USB OTG ?

Pull-up/pull-down resistor ECN circuit. The DP pull-up consists of 2 resistors controlled
separately from the OTG_FS as per the resistor Engineering Change Notice applied to
USB Rev2.0. The dynamic trimming of the DP pull-up strength allows for better noise
rejection and Tx/Rx signal quality

So it has the pull up resistor, and it controls it by itself.

Another interesting thing, is that pin PA9 can be configured as VBUS monitoring, to detect whether the USB cable is connected or disconnected.
No idea if all the pins are broken out, but if PA9 is not and will be unused, then it would good to connect it to VBUS.

Section 34.5.2 decribes how to control the DP pull-up:
Soft disconnect
The powered state can be exited by software with the soft disconnect feature. The DP pullup
resistor is removed by setting the soft disconnect bit in the device control register (SDIS
bit in OTG_FS_DCTL), causing a device disconnect detection interrupt on the host side
even though the USB cable was not really removed from the host port.

[racemaniac – Sat Oct 14, 2017 5:13 pm] –
as an excel developer i know the basic openxml format of xlsx is open and well documented ^^. (there are some legacy old excel support things in there the libre community complains about, but those are only used in in old documents)
but i’ll provide a csv

here you go: BluepillF405 BOM.csv

star. ok looks pretty simple, doesn’t it. for when that goes to the factory are you able to “group” them so there’s a QTY column and a column listing the references?

11; C1 C2 C3 C4…. ; SMD Capacitor 0.1uF 0603;
4; C5 C6 C10 C11; SMD Capacitor 20pF 0603;
etc. etc.

the ferrite bead, not for any particular reason, i happen to be using this one for an audio circuit, it’s quite beefy for an 0603: 1.2A, and it presents 330 ohms @ 100mhz and has a DCR of under 150mOhm (0.15 ohms).

https://www.digikey.com/product-detail/ … ND/1948327

if anyone else feels that spec’s not appropriate for this task do say so. i’m using an MH2029-300Y (3A rating, 300ohm @ 100mhz) in the stl47o but it’s an 0805.

soo… could someone confirm that this is the right procedure:

* look at the datasheet, get its capacitance value
* subtract 10pF (for the pins/traces inherent capacitance)
* because the capacitors are in series to GND, you use the formula 1/(1/C + 1/C) which happens to equal 2 * C

therefore the complete formula for the xtal capacitors is: (DATASHEET VALUE – 10) * 2

is that correct? so for the 8mhz XTAL it’s 20pF so you need (20-10) * 2 = 20pF

but for the 32.768kHz XTAL it’s 12.5pF so you need (12.5pF – 10) * 2 = 5pF

does that look right? did i miss anything?

[lkcl – Sun Oct 15, 2017 1:37 am] –
btw… the crystals… reading the datasheets, they mention that you should assume 10pF capacitance on pins and traces, and that you have to match the capacitance of the *crystal*, is that right?

soo… could someone confirm that this is the right procedure:

* look at the datasheet, get its capacitance value
* subtract 10pF (for the pins/traces inherent capacitance)
* because the capacitors are in series to GND, you use the formula 1/(1/C + 1/C) which happens to equal 2 * C

therefore the complete formula for the xtal capacitors is: (DATASHEET VALUE – 10) * 2

is that correct? so for the 8mhz XTAL it’s 20pF so you need (20-10) * 2 = 20pF

but for the 32.768kHz XTAL it’s 12.5pF so you need (12.5pF – 10) * 2 = 5pF

does that look right? did i miss anything?

what do we do, reduce the capacitors, or ask for a 32khz crystal that is also 20pF? (they also exists, the blueprint schematic has 20pF capacitors on both crystals, so maybe they have one like that. But looking on aliexpress, they seem to all be 12.5pF)

[RogerClark – Sat Oct 14, 2017 8:21 pm] –
@bobc

I think @rikkimball also posted about the USB D+ pullup not being required.

I checked the F4STAMP schematic, and its not present that board, but I think we need to check a few more F4 schematic to be absolutely sure

@racemaniac

Was it impossible to route a pin for the USB OTG ?

shouldn’t be hard, i assume it’s just connecting PA10 to the ident pin? nothing special?

I thought victor said PA9, but perhaps this is not the same thing (and I didnt check the datasheet)

[RogerClark – Sun Oct 15, 2017 7:13 am] –
PA9 or PA10 ??

I thought victor said PA9, but perhaps this is not the same thing (and I didnt check the datasheet)

usb.jpg (12.51 KiB) Viewed 240 times

I wonder what Victor was referring to, or if it was just a typo.

PA10 can be used for ID detection, PA9 for VBUS detection. To support USB host, you need something to switch +5V onto VBUS, which ideally should also provide overcurrent protection.

I note on their design, ST use 20 pF on the 8MHz xtal, and 6.8pF on the 32.768kHz (MC306-G-06Q-32.768, manufacturer JFVNY). I’ve never heard of JFVNY, and couldn’t find a datasheet, so that doesn’t help much!

Edit: found datasheet here http://en.jfvny.com/downloadRepository/ … 9728fd.pdf I know some people try to account for stray capacitance, but I’m not sure if guessing the value without actually measuring it is a good idea. Some people use 5pF as a rule of thumb. I’ve never seen any real measurements which actually show the oscillator is more stable with the “right” value of load capacitor, it’s always a paper exercise. I suspect this is one of those “folklore” things that people like to do but actually has no measureable benefit.

[bobc – Sun Oct 15, 2017 7:42 am] –
I’m using the STMF4DISCOVERY as a reference circuit, http://www.st.com/en/evaluation-tools/s … overy.html

PA10 can be used for ID detection, PA9 for VBUS detection. To support USB host, you need something to switch +5V onto VBUS, which ideally should also provide overcurrent protection.

I note on their design, ST use 20 pF on the 8MHz xtal, and 6.8pF on the 32.768kHz (MC306-G-06Q-32.768, manufacturer JFVNY). I’ve never heard of JFVNY, and couldn’t find a datasheet, so that doesn’t help much!

mc-306 is what i’m using for footprint now, i’ll switch the values to 6.8pF
and for the VBUS, if anybody has an idea on how to implement that, i’m all ears . (preferably not taking up too much space XD)

[racemaniac – Sun Oct 15, 2017 5:39 am] –
what do we do, reduce the capacitors, or ask for a 32khz crystal that is also 20pF? (they also exists, the blueprint schematic has 20pF capacitors on both crystals, so maybe they have one like that. But looking on aliexpress, they seem to all be 12.5pF)

stick with those, then, if they’re commonly available (means lower-prices) and reduce the capacitors to 5pF. does that sound like a good strategy?

[lkcl – Sun Oct 15, 2017 10:25 am] –

[racemaniac – Sun Oct 15, 2017 5:39 am] –
what do we do, reduce the capacitors, or ask for a 32khz crystal that is also 20pF? (they also exists, the blueprint schematic has 20pF capacitors on both crystals, so maybe they have one like that. But looking on aliexpress, they seem to all be 12.5pF)

stick with those, then, if they’re commonly available (means lower-prices) and reduce the capacitors to 5pF. does that sound like a good strategy?

yup, that’s a deal

And just to make things complicated: i made a second design of a bluepill sized F4 board, but with more features rather than pin compatibility

[bobc – Sun Oct 15, 2017 7:42 am] –
I’m using the STMF4DISCOVERY as a reference circuit, http://www.st.com/en/evaluation-tools/s … overy.html

PA10 can be used for ID detection, PA9 for VBUS detection. To support USB host, you need something to switch +5V onto VBUS, which ideally should also provide overcurrent protection.

i typically use the SY6280 for that, but it’s a SOT23-5 and requires 5 components (resistor-divider for the current, 2 4.7uF and 1 0.1uF capacitors). that’s starting to get quite a lot already.

what you can do is use it like a controllable diode with built-in overcurrent protection.

the other circuit i’ve seen is the one on the arduino and the due, which uses an LM385D. westfw on arduino.cc helped track down an SOT23-5 variant (single Op-Amp) which does the job as well: you put the 3v3 on one of the op-amp inputs (Minus) and VBUS on the other (Plus), then wire the output of the Op-Amp directly to a MOSFET. which you also have to have space for (SOT23-3). actually… just looking at the Due Reference Design they just have *two* MOSFETs, one for USBVCC with the gate wired straight to GND, and the other gate connected to that op-amp. it’s 10 components total. one SOT23-5 (op-amp), three SOT23-3 (MOSFETs and transistor) plus discretes.

it starts to get… well… that’s a lot of extra components for such a small – and busy – board space.

my feeling is: the op-amp, transistor etc. could all be replaced with the SY6280, you probably *already have* 4.7uF power-in/out capacitors in place… and you could keep the trick of having the MOSFET with its gate wired to GND to act as a one-way power “diode”.

Some people use 5pF as a rule of thumb. I’ve never seen any real measurements which actually show the oscillator is more stable with the “right” value of load capacitor, it’s always a paper exercise. I suspect this is one of those “folklore” things that people like to do but actually has no measureable benefit.

ST’s application note, referenced in their various MCU datasheets, explains it well. AN4555 page 24/25 has the formula, and then also mentions how to reduce “stray” capacitance which can be anywhere between 2pF and 7pF, and depends on the board layout *for the decoupling capacitors*… not the *crystal* capacitor layout.

it’s complicated in other words.

nom, nom, nom… shuffle…. XTAL to left of F405 goes over by 0.5mm…. F405 goes over by 1mm…. 4-pin header moves left by 1.5mm but without breaking the power/gnd plane that’s going round it….

… that would definitely give you enough room near the USB connector to drop in a SY6280, the resistor-divider and an SOT23-3 MOSFET. datasheet’s easy to find, google “SY6280 datasheet”.

you *might* be able to get away with just moving the 4-pin header over by abouuuut… 0.5mm and not have to move the F405 or the XTAL.

How much current are we expecting this board to draw? the ap2112 is great for operating from a battery, and for low currents, but indeed, it will never stay alive at its 600mA max @5V without proper cooling. probably safe (but hot) up to 200mA @ 5V, but probably not much more. What are our requirements there? do we need to upgrade to an lm1117 (but which has a higher voltage drop, so less suited for battery operation) (basically the same as the AMS1117 i think, also huge voltage drop…).

how much power are we expecting this board to be used for? as is also mentioned in the thread, we can try connecting some of its pins to a plane to provide extra cooling (but which pins would be best >_<)?

*edit*
i’ve just made a test setup with my maple mini that i upgraded with a ap2112. according to my keweisi usb power tester it’s currently getting 270mA @4.6V, and it seems to be holding up pretty well (it’s hot but not burning hot).
According to the datasheet @ those conditions it should be about 63°C (180° per watt without external cooling), i don’t have a thermometer to measure but that seems realistic.
does that seem like a usable voltage regulator for our board, or is it too weak & fragile?

[racemaniac – Sun Oct 15, 2017 12:41 pm] –
How much current are we expecting this board to draw?

the SY6280 copes with switching up to.. 1.5A i think.

F405 moving: disconnect the most immediate tracks then redo them.

[lkcl – Sun Oct 15, 2017 1:07 pm] –

[racemaniac – Sun Oct 15, 2017 12:41 pm] –
How much current are we expecting this board to draw?

the SY6280 copes with switching up to.. 1.5A i think.

F405 moving: disconnect the most immediate tracks then redo them.

i mean the 3v3 part. just read the documentation of the F405, and it’s rated to draw at most 240mA, + 10mA for the 2 leds, we should be able to handle 250mA.
I think that’s well within reach of a single ap2112 @ 5V. it’ll probably go to 70-80 °C, but that’s acceptable i think as a worst case scenario?

I domder what happens to the USB If serial1 is used.

Does it affect the host PC Serial USB driver etc

[RogerClark – Sun Oct 15, 2017 5:32 pm] –
I just remembered PA10 is part of Serial1

I domder what happens to the USB If serial1 is used.

Does it affect the host PC Serial USB driver etc

hmmm… just looking at the datasheet, OTG_FS_ID (PA10) and OTG_HS_ID (PB12) are both “weak pullup” resistors. oh! i think…. i think there’s actually 2 sets of USB OTG interfaces/pins, one set on PA (FS) and one on PB (HS). but you can’t do DFU firmware-flashing through the PB set, only PA11/PA12.

honestly… i feel: if PA10/11 was previously dedicated to USART1_RX, if it doesn’t interfere with interoperability with the bluepull pinouts (i.e. if PA10 can be dedicated to OTG_FS_ID and there’s another couple spare pins with alternative functions as UART TX/RX) i’d say don’t worry about it.

alternative functions for USART1_TX are also on PB7, so if PB7’s not being used that could do the job.

or, USART3 is on PC10/PC11 and also PB10/PB11.

if there’s a priority consideration to use PA10/PA11 for UART-style DFU boot-loading i’d suggest not worrying about that, as USB DFU can take care of that. leave PA10/PA11/PA12 as dedicated to USB, defintely don’t try sharing it.

i’ll try to see if there’s a PDF schematic published somewhere. roger we really need a wiki page for this project, which can keep/manage static links. forums are great for instantaneous narrow-time-window-of-opportunity communication… as long as you keep up-to-date with the discussion…. but they’re a bitch for actually finding useful information. …. remember the AOL “me-too” posting syndrome?

[racemaniac – Sun Oct 15, 2017 1:17 pm] –
i mean the 3v3 part. just read the documentation of the F405, and it’s rated to draw at most 240mA, + 10mA for the 2 leds, we should be able to handle 250mA.
I think that’s well within reach of a single ap2112 @ 5V. it’ll probably go to 70-80 °C, but that’s acceptable i think as a worst case scenario?

bit high! personally i like staying well below rated currrents if possible….

couple of circuits for you. VBUSDET is on a resistor-divider bridge: it’s a cheap way to not need the op-amp. from the arduino circuit you can substitute the MOSFET and the transistor and the op-amp with the SY6280. keep the MOSFET-with-the-gate-to-GND as the power-in-with-a-builtin-diode. aand… you’re done. third picture is from DOCID022152 page 187 en.DM00037051.pdf, stm32f405xx/407 datasheet.

Untitled1.jpg (26.42 KiB) Viewed 264 times

okaaay sooOoo…. PC6 and PC7 are spare. they also have TIM function as well as USART6_TX and USART6_RX. however it looks like you’d also need CTS… and there isn’t a USART6_CTS/RTS – not on the 64-pin variant anyway.

honestly…. looking at the original bluepill, they also wired up PA10-PA12 directly to *both* USB *and* the pin-header…. presumably because of the low pin-count…

i think… it’s basically far too complicated to try dedicating pins to UART and pins to USB, do exactly what they did, but put OTG onto the USB header as well… and *as long as* there is no extra components on PA10 (no pullup/pulldown), as long as you rely on the 405’s internal capabilities to implement the OTG_ID pullup/down functionality, you should be fine.

basically if anyone *really wants* to use PA9/PA10 for TX/RX they’ll just have to live with the fact that they can’t do that and have OTG functionality at the same time. they’re getting the *additional possibility* of OTG functionality when compared to the original BluePill, which didn’t have that at all.

But as the main reason for using the BluePill form factor is so that people could use this as a drop in replacement for existing projects which could use more speed / performance. I think its important to keep PA9 and PA10 connected as Serial (USART 1)

I don’t think it matters if USB OTG does not work while using USART 1, but ideally the normal USB connection to a PC (or Mac etc) should still work when PA9 and PA10 (USART 1) are in use.

[racemaniac – Sun Oct 15, 2017 1:17 pm] –

[lkcl – Sun Oct 15, 2017 1:07 pm] –

[racemaniac – Sun Oct 15, 2017 12:41 pm] –
How much current are we expecting this board to draw?

the SY6280 copes with switching up to.. 1.5A i think.

F405 moving: disconnect the most immediate tracks then redo them.

i mean the 3v3 part. just read the documentation of the F405, and it’s rated to draw at most 240mA, + 10mA for the 2 leds, we should be able to handle 250mA.
I think that’s well within reach of a single ap2112 @ 5V. it’ll probably go to 70-80 °C, but that’s acceptable i think as a worst case scenario?

RT9166-33GVL is rated for 300mA. and the RT9166A is even rated for 600 (in a SOT23-3 package!) pricing on taobao is mad – RMB 1 to RMB 0.25 https://s.taobao.com/search?q=RT9166-33GVL

https://www.digikey.com/product-detail/ … ND/2546644

http://www.richtek.com/assets/product_f … 66A-23.pdf

buuut… hmmm. 300mA @ 3.3v = 1 watt and that completely exceeds the rating of 0.4W for the SOT23-3 package. whoops. do you have room for a SOT-223?

hmm just checking the AP2112k-3.3 pricing on taobao and i think it beats the RT96166 by quite a margin. there’s also a 600mA version of it (the 3.3trg1).

*hand-waving*… the AP2112k-TRG1 should be fine. he said.

*edit*
maybe this one is the winner
and damn i hate how hard these things are to find on aliexpress. Unless i fully type “AP2114HA”, it shows nothing. AP2114 gives me no results what so ever >_<.

[racemaniac – Mon Oct 16, 2017 6:48 am] –
someone else mentioned the ap2114d, which is a lot more expensive i’m afraid (on aliexpress only 1 dealer, selling per 5, @ 0.6€ a piece), but seems the perfect fit for all we can want

aliexpress remember is targetted at selling abroad. taobao is the internal-to-china-version-of-ebay. use that to check instead ok? like this:

https://s.taobao.com/search?q=AP2114HA-3.3TRG1

so… plenty of suppliers on that one.

max rating is 1A, it’s in a proper package with heatsink you can connect to a plane on the board. i’ll have to see if i can make room for it on the board, but i think it’s possible. it will probably make our BOM 0.5$ more expensive, but then we have a voltage regulator that can handle all reasonable cases. for the analog section we can then stick to the ap2112, it’s more than enough for there .
and then we still have nice voltage regulators that have a very low voltage drop, so battery operation remains an option .

https://s.taobao.com/search?q=RT9166A-33GG

RMB 0.40 dang. but only the one supplier.

https://s.taobao.com/search?q=AP2114D-3.3TRG1

lots of suppliers. RMB 1.50, RMB 2, looks like a good choice.

i think really the TO-252 package is what’s needed: it can clearly handle the current properly and dissipate the heat.

[RogerClark – Mon Oct 16, 2017 4:14 am] –
I didnt expect USB and OTG USB to work at the same time

But as the main reason for using the BluePill form factor is so that people could use this as a drop in replacement for existing projects which could use more speed / performance. I think its important to keep PA9 and PA10 connected as Serial (USART 1)

I don’t think it matters if USB OTG does not work while using USART 1, but ideally the normal USB connection to a PC (or Mac etc) should still work when PA9 and PA10 (USART 1) are in use.

well, that should be possible to do as a software option, switching off the OTG_ID alternate function and using PA9 for TX/RX.

hmmm…. i think i see what you’re saying: you anticipate that if you use PA9/10 for UART that the signals jumping about would interfere with USB devicees when the F405 is operating in Host Mode?

okaay…

https://www.maximintegrated.com/en/app- … vp/id/1822

and https://en.wikipedia.org/wiki/USB_On-Th … icro_plugs

the wikipedia page helps identify that A is the host, B is the client. B is floating, A has to be at GND. sooOoo… for any type of “standard” USB2 / USB1.1 device (keyboard, mouse, WIFI dongle) the floating ID pin would be… not a problem.

but… from the maxim site…. it looks like the Host Negotiation Protocol is used at *initial* connect time to decide which one should be host and which client – this is on OTG-based PHYs not USB1/2-based client-only PHYs.

not comfortable with it but… it looks ok to me.

*edit*
tomorrow & thursday i’ll probably have some time to make more changes to the board
this weekend i’ll be on a weekend out, so i won’t be doing anything for this project next weekend .

BluepillF405AP2114.jpg (64.07 KiB) Viewed 248 times

[racemaniac – Mon Oct 16, 2017 7:03 pm] –
I’ve taken a quick go at putting the AP2114 on the board.
I ended up going for the AP2114HA (which is in SOT223 package) first had a look at the sot252 one, but damn is it huge O_O. The 2114HA is a bit smaller (but still WAY bigger than the ap2112 i had), and luckily has GND on its tab (there are 2 versions: the AP2114H & AP2114HA, their pinout differs, and the H has VOUT on its tab).

yeah i always wondered why they do that, always annoyed me that they’re different… then i realised it’s for the trick that you’re using, on 2-layer boards, which i’d never seen before (nice to learn something new) – sandwich between a 3.3v plane on one side and GND on the other. neat. so…. the different types would be for putting on the most suitable side of the PCB. huh. how about that.

And looking at its size, i think it’s big enough, and has a bit ground plane around it to help it cool a bit.BluepillF405AP2114.jpg

size doesn’t matter (hur-hur), it’s the degrees-per-watt figure in the datasheet. you’re looking to do arouuund 250mW @ 3.3v, that’s 8.825 watts. now multiply that by the degrees-per-watt figure for the package…

datasheet:
https://www.diodes.com/assets/Datasheets/AP2114.pdf

there’s two figures for SO-223, one is ambient thermal resistance – 128C/W so we have a figure of 105 degrees that’s on page 7, then another one on page 8 which is 50.9C/Watt (giving a 41.25 degree rise). i don’t know how to interpret these, which one takes precedence, does anyone know?

AP21114HA-3.3TRG1 https://s.taobao.com/search?q=AP2114HA-3.3TRG1 around… RMB 1 which is quite a jump. we’re talking $0.15 instead of $0.05 to $0.07

… still…

[lkcl – Tue Oct 17, 2017 3:17 am] –
size doesn’t matter (hur-hur), it’s the degrees-per-watt figure in the datasheet. you’re looking to do arouuund 250mW @ 3.3v, that’s 8.825 watts. now multiply that by the degrees-per-watt figure for the package…

datasheet:
https://www.diodes.com/assets/Datasheets/AP2114.pdf

there’s two figures for SO-223, one is ambient thermal resistance – 128C/W so we have a figure of 105 degrees that’s on page 7, then another one on page 8 which is 50.9C/Watt (giving a 41.25 degree rise). i don’t know how to interpret these, which one takes precedence, does anyone know?

You’re completely messing up your units, calculations and numbers XD

i assume you mean 250mA @ 3.3v. and that would deliver 0.825W to the microcontroller, but would require the regulator to dissipate 0.425W (1.7V voltage drop * 250mA) (assuming 5V input)
So for the ambient resistance that would result in 54.4°C rise
For the thermal resistance to case it would be 21.6°C rise

Since we don’t have that much copper to put against it and dissipate the heat, we’ll probably be in between there, between 30 & 40 degrees or so.
Seems reasonable?

[racemaniac – Tue Oct 17, 2017 6:13 am] –
You’re completely messing up your units, calculations and numbers XD

wark-wark, fail….

i assume you mean 250mA @ 3.3v. and that would deliver 0.825W to the microcontroller, but would require the regulator to dissipate 0.425W (1.7V voltage drop * 250mA) (assuming 5V input)

ohhh…. cool! so… it’s how much power it has to get *rid* of in order to… okaaay i get it.

So for the ambient resistance that would result in 54.4°C rise
For the thermal resistance to case it would be 21.6°C rise

Since we don’t have that much copper to put against it and dissipate the heat, we’ll probably be in between there, between 30 & 40 degrees or so.
Seems reasonable?

yeah i’d say so. 25+40=65C. 60C is tolerable for humans to touch: it’s just outside that… so people won’t get tooo badly burned if they push it to the limit.

[lkcl – Tue Oct 17, 2017 4:14 am] –
AP2112K-3.3trg1 https://s.taobao.com/search?q=ap2112k-3.3trg1 is around RMB 0.36 to 0.50 estimated

AP21114HA-3.3TRG1 https://s.taobao.com/search?q=AP2114HA-3.3TRG1 around… RMB 1 which is quite a jump. we’re talking $0.15 instead of $0.05 to $0.07

How does AMS1117-3.3 compare? Seems to be very commonly used on the cheap modules. Can’t really understand what I am looking at on Taobao…

[bobc – Tue Oct 17, 2017 11:31 am] –

[lkcl – Tue Oct 17, 2017 4:14 am] –
AP2112K-3.3trg1 https://s.taobao.com/search?q=ap2112k-3.3trg1 is around RMB 0.36 to 0.50 estimated

AP21114HA-3.3TRG1 https://s.taobao.com/search?q=AP2114HA-3.3TRG1 around… RMB 1 which is quite a jump. we’re talking $0.15 instead of $0.05 to $0.07

How does AMS1117-3.3 compare? Seems to be very commonly used on the cheap modules. Can’t really understand what I am looking at on Taobao…

it’s got a huge voltage drop, so for 5v operation it is ok and very cheap, but for connecting your board directly to a lithium battery, it’s a disaster …
that’s why i ended up going for the AP voltage regulators on my projects. i’m making things i want to connect to a battery, and not first have to boost the voltage to 5V… And there have already been discussions on this forum about this, since others are facing the same problem. That’s why i’d prefer the AP2114, but indeed, quality has its price ^^’

IMHO if you want to run from Lipo, you should use an external power management board which also handles not totally discharging the Lipo

I think you are in danger of over speccing and making the price uncompetative

[RogerClark – Tue Oct 17, 2017 7:35 pm] –
Do both regulators have the same package / footprint?

IMHO if you want to run from Lipo, you should use an external power management board which also handles not totally discharging the Lipo

I think you are in danger of over speccing and making the price uncompetative

i usually use batteries with built in protection, so that’s solved on the battery side . (or with these voltage regulators, you can probably also get away with 3 NiMh batteries, iso 4)
and the one i chose is not pin compatible with the ams1117… if however we would go for the other one, the AP2114H (with vout on the tab), that one is pin compatible.
but atm, we’re apparantly at about 0.20$ for the regulators, and that’s the only part where we’re going for something fancy, i think that’s bearable? or is it too much?
atm the idea is a cheap & small ap2112 for the analog supply, and the beefier ap2114 for the main supply.
i can try to go for the one that is pin compatible with the cheaper ams1117, but i’ll have to see how i get that to work with the fact that the regulator fits best on the side of the ground plane ^^’

OK.

I’m not trying to go ultra cheap, but from what I’ve seen, the members of the forum are very price sensitive.

I guess we need to have a total BOM cost and work out the percentage of cost for each item, to see if any particular item is substantial part of the overall cost and if so, whether that part can be exchanged for a cheaper alternative

[bobc – Tue Oct 17, 2017 11:31 am] –
How does AMS1117-3.3 compare? Seems to be very commonly used on the cheap modules. Can’t really understand what I am looking at on Taobao…

it’s ebay for china. so.. you know the summary page on ebay? that’s what you’re looking at. so, you apply the same general tricks: ignore anything too low (suspicious), ignore anything too high, and reject any part that has too few sellers. then take the average of the remaining parts, and divide by (appx) 6.5 to get USD.

that way you get a rough idea +/- 20% of how much a part will cost if bought in the markets in shenzhen.

[RogerClark – Tue Oct 17, 2017 11:05 pm] –
@racemanic

OK.

I’m not trying to go ultra cheap, but from what I’ve seen, the members of the forum are very price sensitive.

I guess we need to have a total BOM cost and work out the percentage of cost for each item, to see if any particular item is substantial part of the overall cost and if so, whether that part can be exchanged for a cheaper alternative

ok so let’s start that:

• https://s.taobao.com/search?q=STM32f405RGT6 $3 to $4
• https://s.taobao.com/search?q=HC-49USX $0.03 so insignificant
• https://s.taobao.com/search?q=32.768k+mc-306 mc-306 $0.04 or thereabouts: also insignificant
• https://s.taobao.com/search?q=10118194-0001LF USB $0.30
• https://s.taobao.com/search?q=RS-187R05A2-DS-MT-RT reset switch $0.15

then we have either:

• https://s.taobao.com/search?q=AP2112K-3.3TRG1 AP2112K $0.04 or
• https://s.taobao.com/search?q=AP2114HA-3.3TRG1 AP21114HA-3.3TRG1 $0.07

so the processor is by far and above the most significant cost, by a long, long margin. even the SY6280 which would give protected USB-OTG power is only around the $0.07 mark https://s.taobao.com/search?q=SY6280

we’re talking a difference in the BOM of around 1%, absolute maximum 2%, due to the relatively high price of the F405. i also looked up the STM32f411RCT6 but there was too much variation to be able to make an estimate.

[racemaniac – Wed Oct 18, 2017 8:07 am] –
thanks for the nice breakdown
the 2114 it is then .
can someone summarize the consensus on what to do for usb otg (if there is one)? haven’t had much time to read it all in detail, and tomorrow i’ll probably have some time to work on the board .

jumping in (corrections / oversight appreciated) i think using a MOSFET-gated-to-ground (just as in the Due schematic) and the SY6280 for enable/disableable power-protection will give you OTG power control with the minimum component count. you’ll have to jump back a few pages to find the schematic images i posted (gaahhh i really don’t like this aspect of forums – roger, we need that wiki page, man!)

this one: http://stm32duino.com/viewtopic.php?f=1 … 140#p35772

also the USB ID line is only checked at plug-in time and for USB2-only-client devices it’s not even relevant. so i think you’re good to go, just don’t put any extra components on it (no resistors, no capacitors, nothing) then it can double up as one of the UART lines.

The hazard I see is that if a cable is plugged into the pill, it could have the ID connected to ground. If you set that GPIO to output 1, it will be sinking straight to ground and will likely burn out. Therefore I suggest all that is needed is a current limiting resistor, e.g. 10k, to allow the GPIO port to be shared.

[bobc – Wed Oct 18, 2017 11:22 am] –
There seems to be some confusion about the ID pin and how it is used. The purpose of the ID pin to identify a “host” when two *devices* are connected together. The ID pin is grounded at one end inside the cable, the ID pin is never driven by the CPU. A PC is always a host, the USB A connector does not have an ID pin.

The hazard I see is that if a cable is plugged into the pill, it could have the ID connected to ground. If you set that GPIO to output 1, it will be sinking straight to ground and will likely burn out. Therefore I suggest all that is needed is a current limiting resistor, e.g. 10k, to allow the GPIO port to be shared.

the reference design in the appendix doesn’t have any such resistor.

the datasheet DocID022152 page 115 section 5.3.6 table 48 shows that PA10 and PB12 have a 10k pull-up and 10k pull-down resistor on-board the IC.

if we suggest that there should be 10k resistors on the ID pin, then by the same logic *all* pins should have 10k resistors on them… because all pins could be used as outputs and “accidentally grounded”.

so, this case should be covered in the instructions: a large warning “do not switch the ID pin to an output and then also plug in a USB OTG device”.

honestly i feel that once you start treating people as unable to read instructions, it never ends. 20 years ago i knew someone who worked for SCO (before they went bad). he taught me a lovely quote: “if you make something idiot-proof, only idiots will use it”.

put a resistor in series and then you can never use that pin for anything other than purposes for which a 10k resistor happens not to interfere.

[racemaniac – Wed Oct 18, 2017 11:52 am] –
Can someone maybe draw me a schema on how we now want to hook it up? i’m getting lost ^^’

again: look at the diagrams i sent in the link to the earlier discussion. here is the link again. diagram 3 in this link http://stm32duino.com/viewtopic.php?f=1 … 140#p35772

that diagram is straight out of the appendix in the datasheet. page 187, figure 95, document ID DocID022152 Rev 8, filename en.DM00037051.

[lkcl – Wed Oct 18, 2017 12:05 pm] –

[racemaniac – Wed Oct 18, 2017 11:52 am] –
Can someone maybe draw me a schema on how we now want to hook it up? i’m getting lost ^^’

again: look at the diagrams i sent in the link to the earlier discussion. here is the link again. diagram 3 in this link http://stm32duino.com/viewtopic.php?f=1 … 140#p35772

that diagram is straight out of the appendix in the datasheet. page 187, figure 95, document ID DocID022152 Rev 8, filename en.DM00037051.

that diagram isn’t quite clear to me, what is the current limiter switch? (is that the SY6280?), and so i’ll have to use an extra pin for this voltage switch (one that is not part of the usb pins of the f4?)
concerning the resistor on ID pin: if i put the resistor between the pad & the usb port (and not between the f4 and the pad), we have best of both worlds . no shorts when doing something wrong, and the pad not having the resistor messing with it .

[racemaniac – Wed Oct 18, 2017 12:50 pm] –

[lkcl – Wed Oct 18, 2017 12:05 pm] –

[racemaniac – Wed Oct 18, 2017 11:52 am] –
Can someone maybe draw me a schema on how we now want to hook it up? i’m getting lost ^^’

again: look at the diagrams i sent in the link to the earlier discussion. here is the link again. diagram 3 in this link http://stm32duino.com/viewtopic.php?f=1 … 140#p35772

that diagram is straight out of the appendix in the datasheet. page 187, figure 95, document ID DocID022152 Rev 8, filename en.DM00037051.

that diagram isn’t quite clear to me,

you wire up the USB and ID direct. no resistors.

what is the current limiter switch? (is that the SY6280?),

yyup. and the 5V regulator thingy is just the MOSFET-that-has-the-gate-tied-to-GND. it’s being used, in effect, as a diode, stopping power getting back up the line. the absolute last thing you want is a current bun-fight between two 5V supplies.

you could just use a schottky diode instead but if you do try to find one with the absolute lowest possible voltage drop. the MOSFET’s probably being used (effectively) as a diode because its voltage drop is (i presume) very low?

and so i’ll have to use an extra pin for this voltage switch (one that is not part of the usb pins of the f4?)

yyup.

concerning the resistor on ID pin: if i put the resistor between the pad & the usb port (and not between the f4 and the pad), we have best of both worlds . no shorts when doing something wrong, and the pad not having the resistor messing with it .

i don’t think it’s a good idea to do anything other than follow the reference design. i do not think it is a good idea to assume that the users need to be… molly-coddled is a good word to use.

i repeat: if you expect that people will damage one particular output and are going to “protect” it with a 10k resistor, you MUST now put a 10k resistor on EVERY single pin…. just in case they quotes might damage the board quotes. this is treating users like idiots, because it’s making the board “idiot-proof”. don’t do it. if they ignore the instructions and blow up the processor, they can buy another board and not make the same mistake again.

again, i repeat: you don’t know the consequences on people’s designs of forcing them to have a 10k resistor in series with that pin. some shields may simply… fail to work properly because the supplied current is insufficient to drive the 10k resistor high/low/whatever. if they use it as an analog output (PWM-driven) you could end up *changing* the output compared to the original BluePill because there’s an extra 10k resistor in the circuit that the shield didn’t anticipate being there, which alters the RC circuit in unpredictable ways.

don’t do it.

so ignoring the CARD_VCC 10k pullup, you can see they’ve put a 1k in series with the USB_ID line. that’s *between the F4 and the USB connector* *NOT* repeat *NOT* between the pinheader and the F4.

i’ll try to find some other schematics just to make absolutely sure.

Untitled1.jpg (60.19 KiB) Viewed 187 times

Untitled1.jpg (28.61 KiB) Viewed 187 times

[lkcl – Wed Oct 18, 2017 1:18 pm] –

again, i repeat: you don’t know the consequences on people’s designs of forcing them to have a 10k resistor in series with that pin. some shields may simply… fail to work properly because the supplied current is insufficient to drive the 10k resistor high/low/whatever. if they use it as an analog output (PWM-driven) you could end up *changing* the output compared to the original BluePill because there’s an extra 10k resistor in the circuit that the shield didn’t anticipate being there, which alters the RC circuit in unpredictable ways.

don’t do it.

Sorry, your argumentative style is simply illogical and idiotic. I made a simple and practical suggestion and you’ve gone into some sort of mental meltdown. Clearly, a non-idiot can simply remove the resistor if they don’t need it, but even a non-idiot will find it harder to replace the CPU if they burn out a pin.

I’m out – good luck.

If nothing is connected in the USB connector (so USB ID PIN is floating), then the 1k is not going anywhere, and should not cause any trouble.

If the Datasheet calls for it, it should be used. If it doesn’t call for it, but can be used without affecting anything, I would think is better to use it (if the pin is in a header so a user may decide to use it for something else). It’s not about protecting every single pin, but just 1 pin that has a higher risk of being shorted to ground.

If that pin is not routed to any header, only to the OTG USB ID pin, the I think we should just go with what the datasheet calls for and not think on it anymore. There is no point protecting the pin if it’s not available in a header to be used as GPIO.

[bobc – Wed Oct 18, 2017 3:43 pm] –

[lkcl – Wed Oct 18, 2017 1:18 pm] –

again, i repeat: you don’t know the consequences on people’s designs of forcing them to have a 10k resistor in series with that pin. some shields may simply… fail to work properly because the supplied current is insufficient to drive the 10k resistor high/low/whatever. if they use it as an analog output (PWM-driven) you could end up *changing* the output compared to the original BluePill because there’s an extra 10k resistor in the circuit that the shield didn’t anticipate being there, which alters the RC circuit in unpredictable ways.

don’t do it.

Sorry, your argumentative style is simply illogical and idiotic. I made a simple and practical suggestion and you’ve gone into some sort of mental meltdown. Clearly, a non-idiot can simply remove the resistor if they don’t need it, but even a non-idiot will find it harder to replace the CPU if they burn out a pin.

I’m out – good luck.

he’s indeed having a bit too much of a meltdown ^^’
but don’t leave the discussion, any feedback is useful, let’s not get discouraged because of this

[bobc – Wed Oct 18, 2017 3:43 pm] –

Sorry, your argumentative style is simply illogical and idiotic. I made a simple and practical suggestion and you’ve gone into some sort of mental meltdown. Clearly, a non-idiot can simply remove the resistor if they don’t need it, but even a non-idiot will find it harder to replace the CPU if they burn out a pin.

I’m out – good luck.

ok, your choice. i’ll assuming you won’t be reading this thread any more. very strange, because he should have seen the follow-up messages which indicated that i realised i’d made a mistake, and double-checked with some other schematics that i have here which show that adding in a series resistor is quite common.

so, would it be reasonable to assume that the users of this board would be happy to remove an 0402 component from a board? what if they want to put it back on again, later? so no – i wouldn’t have thought so. i know from experience that 0402 components are exceptionally hard to hand-solder, if you want to put them back on, and even taking them off in the first place risks damaging or losing them: they tend to stick to the soldering iron tip and need to be removed very very quickly with tweezers.

so, the logic behind not putting the resistor in series between the F4 and the header stands: it changes the characteristics of the pin, such that existing shields with which this board – deliberately named the BluePillF4 and deliberately made to be pin-compatible so as to save people on the cost of having develop or buy yet another set of incompatible shields – may fail to work.

i don’t see anything illogical or idiotic about that: if there is i have no problem with people saying so (publicly).

[victor_pv – Wed Oct 18, 2017 3:59 pm] –
Regarding the 1k resistor, if it’s planned between the USB ID pin and the header pad, then it would not affect if the user doesn’t use USB on the go.
Something like (where the dashes is the electrical connection):
USB ID PIN——1k——header_pin——MCU PIN.

yehyeh, that’s it: that would do it. i didn’t quite understand what racemaster was referring to initially: your ascii art makes it clear that we’re talking about the same thing.

If that pin is not routed to any header, only to the OTG USB ID pin, the I think we should just go with what the datasheet calls for and not think on it anymore. There is no point protecting the pin if it’s not available in a header to be used as GPIO.

http://wiki.stm32duino.com/index.php?title=Blue_Pill pinout’s towards the bottom.

i did the analysis a couple days ago: for pin-compatibility / interoperability with pre-existing bluepill shields there is no other option but to use this particular pin as GPIO.

right at the beginning of the thread (somewhere on page 3 or 4) i asked roger if pin-compatibility was strictly necessary: he said it was because there is a huge range of pre-existing bluepill shields and it would be pain (costly) to force people to make more to yet another non-interoperable shield standard.

[racemaniac – Thu Oct 19, 2017 3:28 pm] –
@22R & 1k5 resistors: not sure for the 22r, but i see something like that used in most cases, the 1k5 is not needed for the F4, but if we leave it in, the board is also compatible with an F1 which does need it

ok – so NC for F4. note recorded to that effect in schematic page?

@mosfet: the one i chose is slightly worse in specs (bit higher on resistance), but also a bit smaller, all in all very very similar .

nice.

@sy6280 resistor, the formula is A=6800/Rset (ohm) . so for 0.5A it’s 13.6K . i thought a bit extra would be nice, but i’ve seen schematics going for a value close to 13.6k

doh!

@divider bridge: do i bring it to for example PC8, or to the dedicated pin for it on the stm32f4 (PA9). It will then basically result in a weak pullup on the TX of the serial line we wish to not compromise, not sure how well u(s)art can cope with that.
otherwise i can do it to pc8 and then we have to manage it ourselves, not have the peripheral do it for us. (or do it via a jumper… but we’re already running short on space >_<)

yeah i didn’t realise in the reference / appendix they just have PA9 wired directly to VBUS. if that’s what they’re doing then… it *should* be listed as a 5v-tolerant pin…. that means looking up table 6 (page 46…) “FT” means “five tolerant”… aand yes, age 55 PA9 is 5v-tolerant.

ok so it’s fine. direct-wired, no resistor-divider bridge. PA9 can be used as OTG_FS_VBUS detect.

Or a Wiki page, Roger? We are up to 20 pages for this thread, and it is getting tedious to find a piece of information!

Putting the files in github would be the best solution

I can put the latest version from @racemaniac in that repo, but he has not posted updates files for several days

Please provide PDFs/GIFs along with CAD files, so that one can see the result on mobile devices without Kicad…

BluepillF4v1.0e.zip

(215.72 KiB) Downloaded 15 times

In case its easier for people to manage this via github, I’ve added @racemaniacs board to my existing github repo

https://github.com/rogerclarkmelbourne/ … ill_Boards

I removed my abandoned attempts, and I’ve renamed the KiCad version of the STM32Stamp board, back to its original name.

Here are the Schematics and PCB files in PDF.

BluepillF4_3D_Top.png (188.53 KiB) Viewed 147 times

I’ll add those files to the repo

Edit.

Those files should now be in the repo

I just put them in the root of the repo.

PS. I think we need a BOM CSV file so that we can calculate the price etc

No point doing gerbers yet, as the design is not stable

Whats the best way to resolve this when I open the schematic ??

missing_libs.png (6.74 KiB) Viewed 143 times

I noticed on the Teensy 3.6 that it has SMD pads on the bottom, because the MCU has more GPIOs etc than there are though holes on the PCB

Looking at the PCB layout, there may be scope to do the same thing for some of the unused pins

[Squonk42 – Thu Oct 19, 2017 10:22 pm] –
Yes, but this is just bending the pins for through-hole, the main body should be OK.

OK

I tried to download that file, but there is a whole load of license conditions which I’m not sure may preclude us from adding it to an open source project

It may not look so pretty, but its probably easier to knock up something in OpenSCAD

[RogerClark – Thu Oct 19, 2017 10:25 pm] –

[Squonk42 – Thu Oct 19, 2017 10:22 pm] –
Yes, but this is just bending the pins for through-hole, the main body should be OK.

OK

I tried to download that file, but there is a whole load of license conditions which I’m not sure may preclude us from adding it to an open source project

It may not look so pretty, but its probably easier to knock up something in OpenSCAD

As it is my own work, I will send you this 3D model under a compatible licence of your choice, let me know the more appropriate.

I wall’have to figure out how to convert it to a format that Kicad can read using free tools like Blender or Openscad

Do you know which formats are supported by Kicad?

It seems that KiCad does not support all types of VRML but that the version exported by FreeCAD works OK.
Also Wings3D can export in the correct type of VRML

But as I was creating my models in OpenSCAD, the best way I found was to open the SCAD file in FreeCAD, then export to WRL

(Note. FreeCAD seems to have 2 copies of the SCAD object when it imports, so I had to select the second “group” e.g. “group11” before I could export.)

I downloaded that model and imported the DAE file into FreeCAD, then selected all the objects and exported as WRL, and loaded that into KiCAD, but it seems to not have any colour information, so it was all the same colour as the PCB (green)

The scale was also quite different, and I had to set it to 0.005 to be roughly correct. But this seems a very strange scale factor e.g. I could understand if it was 0.001 for mm instead of metres, or perhaps 0.0025 for mm to inches etc (or perhaps the reciprocal of that value)

But 0.005 seems strange.

I am not an expert in FreeCAD, I only used it to export from OpenSCAD to VRML, for KiCad and it seemed to retain the colours defined in OpenSCAD, but this doesnt seem to apply to Collada format.

FreeCAD does not seem to support importing Sketchup files

To set the colours you could use Wings3D but its a pain to have to select each object in the model and set its colour

What format was the model originally created in ? Sketchup ?

[RogerClark – Thu Oct 19, 2017 7:52 pm] –
I am. not sure a wiki page would help

from experience of 20+ years collaborating in public i know that it helps enormously… but only if there’s someone actually prepared and motivated to use and maintain it… which because of seeing how amazingly effective they are, year after year, project after project, i most certainly am.

for example: when doing the reverse-engineering of the HTC BlueAngel and other smartphones, we used the wiki to house notes, discussions and so on.

already i’ve been forced into repeatedly giving people back-links to schematic diagrams… which i cannot even find myself and am forced to click, click, click, page back, page back.

those diagrams should *be on the wiki*, where i would bookmark it as a pinned tab, and would reasonably expect people to have it open as well, next to the tab for this [throw-away-style, completely impossible-to-find-anything except the most absolute and immediate latest replies] discussion.

forums are great for communicating in an immediate fashion but for actual information, which people clearly can’t be expected to keep in their heads, they’re worse than useless.

a wiki – which is a STATIC real-time editable document – makes up for that.

Putting the files in github would be the best solution

… which as an ethical software libre advocate i can’t contribute to. for reasons why, see https://directory.fsf.org/wiki/Collecti … placements and https://www.gnu.org/philosophy/who-does … ve.en.html

also: putting the *source* code online is not what is primarily needed here. we need *discussion* documents, research links, links to the datasheets, links to schematic reference diagrams and so on.

yes sure github has a wiki feature… but i cannot use it. so i will be forced into typing out “can someone please put this on the wiki”, “can someone please upload this image to the wiki”, “can someone please put this research link on the wiki” and after about the fourth time people will get really tired of that and will stop replying.

… been at this a long time, roger

It looks like the Collada format is loosing color information.

Anyway, there isn’t much color in it: the body is a kind of mate greyish tin metal, there is a black plastic inner body with gold contacts + SMD pins.

[racemaniac – Fri Oct 20, 2017 9:18 am] –
what i am wondering though is on github or so how we’ll handle the pcb project, unlike code it’s something that doesn’t lend itself to easy merging ^^’
or will i keep doing all the changes to the pcb?

Only put it in github so people could access the latest version from the same place all the time.

To save people having to scroll backwards from the last post, to the last time you attached a zip

I don’t know of a way to do co-operative development of PCB’s or Schematics

[RogerClark – Thu Oct 19, 2017 10:15 pm] –
Missing libs ??

Same here…

[lkcl – Thu Oct 19, 2017 2:56 pm] –
they use a FDN340P if that helps

Nice, but FDN304P is better

[racemaniac – Thu Oct 19, 2017 3:28 pm] –
@mosfet: the one i chose is slightly worse in specs (bit higher on resistance), but also a bit smaller

And where to buy??
2y ago I ordered a couple of IRLML6402, they do work outstanding for me, cheap and widely available.
Last year I got another tip: DMP1045U, harder to find but maybe one of the best possibilities ATM.

Why, the hell, did you change the microUBB printout?
I’ve lying a couple around here, no one matches your new one (

[RogerClark – Fri Oct 20, 2017 9:58 am] –

[racemaniac – Fri Oct 20, 2017 9:18 am] –
what i am wondering though is on github or so how we’ll handle the pcb project, unlike code it’s something that doesn’t lend itself to easy merging ^^’
or will i keep doing all the changes to the pcb?

Only put it in github so people could access the latest version from the same place all the time.

To save people having to scroll backwards from the last post, to the last time you attached a zip

which helps with schematics and PCB files… but does nothing to help with the research of parts, research, publication and discussion of reference designs and so on. for all of that we are still forced to repeatedly cross-reference back to older posts. forum software is a total failure when it comes to collaborative development, roger. it’s perfect for simple real-time (unimportant) discussions. the most extreme case i ever heard was a reference telling people to look for a schematic on page *746* of a 1,000-page discussion.

I don’t know of a way to do co-operative development of PCB’s or Schematics

there was one project i heard of which was an online PCB editor, in theory it would be possible to contribute/collaborate.

kicad helps inasmuch as you can split schematics into multiple pages and use git pull to merge them in. i spoke to the developers a long time ago and got them to remove the ridiculous practice of putting (and modifying) timestamps into the text output every time you hit “save”. it was massively interfering with collaborative development.

PCBs… no. you just have to manually hand off to another person, ask them to do mods, and refrain from editing until they’re finished. in theory, as kicad is a text-based file format you could merge changes but i wouldn’t want to try it.

[bianchifan – Fri Oct 20, 2017 11:12 am] –

[RogerClark – Thu Oct 19, 2017 10:15 pm] –
Missing libs ??

Same here…

[lkcl – Thu Oct 19, 2017 2:56 pm] –
they use a FDN340P if that helps

Nice, but FDN304P is better

[racemaniac – Thu Oct 19, 2017 3:28 pm] –
@mosfet: the one i chose is slightly worse in specs (bit higher on resistance), but also a bit smaller

And where to buy??
2y ago I ordered a couple of IRLML6402, they do work outstanding for me, cheap and widely available.
Last year I got another tip: DMP1045U, harder to find but maybe one of the best possibilities ATM.

Why, the hell, did you change the microUBB printout?
I’ve lying a couple around here, no one matches your new one (

the point was to have a micro usb socket that could be easily sourced, so they went for that one, but indeed, i can’t find it on aliexpress either, so that part also annoys me a bit ^^’
but i do understand that as it currently is, it’ll be easier to have actually produced by someone.

However, this socket takes up a bit more space than the one i used originally, so once we’re done, i can make a second version of the files with parts easily found on aliexpress/ebay, and those can be used for people who want to make their own boards
and now i’m really leaving for the weekend, see y’all on monday

Look at this one, only 0.06 RMB:
https://item.taobao.com/item.htm?id=531741597795

EDIT: It is a clone of this Molex connector:
http://www.molex.com/pdm_docs/sd/476420001_sd.pdf

You can find the 3D model here:
http://www.molex.com/molex/products/dat … ECTORS.xml

[Squonk42 – Fri Oct 20, 2017 1:47 pm] –
A mid-mount micro USB socket like the one used in the Bluepill would be the best, it makes the overall board thinner and it has 4 large TH legs that prevent tearing it apart from PCB when plugging/unplugging the cable.

Look at this one, only 0.06 RMB:
https://item.taobao.com/item.htm?id=531741597795

EDIT: It is a clone of this Molex connector:
http://www.molex.com/pdm_docs/sd/476420001_sd.pdf

You can find the 3D model here:
http://www.molex.com/molex/products/dat … ECTORS.xml

excellent – it’s really important to find datasheets / part numbers for all components… *and* also then check that there’s dozens of suppliers with that exact part on taobao. you can’t do it the other way round (or… it’s hell to try): the market vendors don’t care about datasheets.. or if they do they have them on internet-disconnected personal laptops, no website, and the best you can do to contact them is email them, call them or use QQ. all of which requires that you speak mandarin.

so… good find, sqonk42, that’s saved a lot of hassle, finding the molex part number.

why?

well… in 2 days time when racemaster comes back, there will be about… 2 or 3 more pages of discussion. he won’t see any of that… so what we will be forced to do is: *remember* that the part is there, and do page-back, page-back, page-back, scroll, scroll, scroll… and eventually, if we’re really lucky, not miss it, and be able to refer him to it.

however… if there was a wiki, which he’d bookmarked, we could just say “go look at the wiki reference section we added an excellent USB mid-mount connector”

wiki pages are *really important*. i would set one up however im doing so it makes my personal web server resources a permanent part of the stm32duino infrastructure, which i don’t feel is appropriate for me to do.

You may try Miraheze.

[lkcl – Fri Oct 20, 2017 4:03 pm] –
[edit] – just as a safety check i took most of the chinese characters, the 5P etc. etc. and dropped them into a search: it came up with 2 pages of vendors selling parts that look exactly like this one, which isn’t quite enough to be “safe” that they’re not all rip-off merchants. however as it’s a molex clone it’s probably okay.

Yes, here is the corresponding query:
https://s.taobao.com/search?q=USB+5PIN% … =price-asc

According to Google, “USB 5PIN沉板 MICRO 5P MK5P 沉板 0.8mm母座 四脚插 USB插座” translates into “USB 5PIN sink board MICRO 5P MK5P sink board 0.8mm female four feet plug USB socket”, where “sink board” probably means “mid-mount” and “four feet plug” means “4 Through Hole Solder Tabs”.

2D drawing and 3D STEP files here:
http://www.alps.com/prod/info/E/HTML/Ta … CE010.html

It can be found for 0.10 RMB on TaoBao from many vendors:
https://s.taobao.com/search?q=SKSGACE01 … =price-asc

It could be interesting too to replace the tall and bulky BOOT header & jumpers by an additional similar button for BOOT0, much like the dual-button solution used on NodeMCU boards for RESET/FLASH (page 6):
https://github.com/nodemcu/nodemcu-devk … T_V1.0.PDF

[Squonk42 – Fri Oct 20, 2017 9:17 pm] –
Regarding the reset button switch: I used the ultra-small (3.5 mm L x 2.7 mm W x 1.4 mm H) ALPS SKSGACE010 in some of my existing designs:

2D drawing and 3D STEP files here:
http://www.alps.com/prod/info/E/HTML/Ta … CE010.html

It can be found for 0.10 RMB on TaoBao from many vendors:
https://s.taobao.com/search?q=SKSGACE01 … =price-asc

It could be interesting too to replace the tall and bulky BOOT header & jumpers by an additional similar button for BOOT0, much like the dual-button solution used on NodeMCU boards for RESET/FLASH (page 6):
https://github.com/nodemcu/nodemcu-devk … T_V1.0.PDF

Just a thought, but if Boot0 was a button, perhaps we could also run a track to an unused GPIO pin, so in normal operation it doubled as a USER button.
(though potentially glitches on the GPIO pin at boot time could cause problems

[RogerClark – Fri Oct 20, 2017 10:33 pm] – Just a thought, but if Boot0 was a button, perhaps we could also run a track to an unused GPIO pin, so in normal operation it doubled as a USER button.
(though potentially glitches on the GPIO pin at boot time could cause problems

IIRC, this was the option used in the Maple Mini, where the BOOT0 switch was also connected to PB8:
https://github.com/leaflabs/maplemini/b … lemini.pdf

I forgot that…

[RogerClark – Sat Oct 21, 2017 8:01 pm] –
Thanks…

I forgot that…

Yes, but this means that it was a good idea

So we may keep it!

Another subject, MicroSD, which is a superior feature of the F405: look at this beauty:
http://www.molex.com/molex/products/dat … SOCKET.xml
… Only 11.95 mm wide, meaning that it fits between the BP rows of pins… May be worth to provide the footprint on PCB bottom side (at least if there is still space), although they are not even expensive on TaoBao:
https://s.taobao.com/search?q=104031&ty … =price-asc

Roger, can you do that and bookmark posts like the one with the usb part in the first post? that’s easy and effective, without consuming much time.

I’m not sure what yoi mean by Bookmark..

Re:wiki

Its a refernce not a dev space

stephen

[victor_pv – Sat Oct 21, 2017 8:39 pm] –
Guys, without creating any wiki, is really easy for the OP to modify the first post and add links to the relevant posts in the thread.

Roger, can you do that and bookmark posts like the one with the usb part in the first post? that’s easy and effective, without consuming much time.

that places the burden of maintaining the references onto the OP (in this case, roger). do you think he would be ok to make 4 to 5 edits per week, as everyone asks him, “please can you update the 1st post to put this research on it? please can you put this on the 1st post roger? please can you upload this image onto the 1st post roger?” how long do you think he would tolerate doing that, and do you feel that it’s acceptable to flood an *ALREADY* overloaded forum with 1980s-style AOL “metoo” postings?

also: will roger be up at the same time that i am? i am on GMT+7 (Taiwan), i presume that there are also people in the US and also EU timezones.

the point of a wiki page is that it is collaborative: no one person becomes a critical bottleneck.

[zmemw16 – Sun Oct 22, 2017 1:05 am] –
i wonder maybe if it’s time for a hardware-snippets category ?
threads titled for the component ?

stephen

let’s think that through. how could several people contribute to – edit – posts within that hardware-snippets category? they can’t, can they? not unless the username and password of the account used to make the posts is published – publicly – and i doubt very much whether that would be acceptable.

so what would happen would be that anyone spotting a mistake or wishing to contribute a similar circuit would be forced to post underneath. if the OP is no longer a member of the forum, the information becomes out-of-date, or extremely fragmented.

bottom line: *there is no substitute for a wiki*. forums have an extremely good purpose, but they cause people to lose critical information. wikis are good at recording and researching “static” information, but they are absolutely useless for having lengthy and detailed conversations.

the COMBINATION of the two is what makes a successful collaborative project.

[RogerClark – Sat Oct 21, 2017 8:54 pm] –
Re:wiki

Its a refernce not a dev space

ah, you mean: you want to maintain the stm32duino wiki *as* a static reference, maintained, controlled and reviewed only by a few people to provide specific information? that’s a good resource to have.

unfortunately, though, as you can see from this current discussion, where people are extremely heavily inconvenienced by not being able to record *active* research, having to constantly refer to back-links time and time again, the forum alone is not enough, and neither is a (restricted, static, edited-after-the-fact wiki, no matter how good that resource genuinely is)

this is an example of how, back in 2003, we used a wiki (and irc) to collaborate and communicate over 3 different timezones:

https://forum.xda-developers.com/wiki/H … l/Research

that one we organised very well, splitting it into different pages.

a page where we took a different approach (single-page) is here:

https://forum.xda-developers.com/wiki/H … l/Research

basically we used it to record all of the pictures *as we were going along*. someone would publish and upload a photo of the PCB, then someone else would do the research to find datasheets.

can you see how incredibly useful that would be to have here?

can you see how staggeringly-less hassle it would be to no longer force everybody to rummage through 24 (and increasing) pages to find the exact same information?

[victor_pv – Sun Oct 22, 2017 2:07 pm] –
Roger perhaps a new section in the Wiki for this board, which hopefully will be a reality soon and need a page in the wiki anyway, could have that “research” section?

ok, so just so you know, people, it’s potentially quite a lot of extra administrative / sysadmin work for roger: the wiki’s not set up to permit new logins, so that just slams spammers out cold. very simple, very effective. allowing people accounts that need approval doesn’t shut out spammers: it just… adds to the administrative burden for roger as the spammers will just keep trying anyway. allowing people to have arbitrary accounts (without a sysadmin check) means it risks automated spam-attacks / automated spam-editing. they’re not even personal: regular internet port-scanning takes place by the mafia (in several countries), etc. etc. and as it’s wikimedia the attack scripts literally roll out automatically. this is why i use non-popular web software such as ikiwiki.

the advantage however would be a huge reduction in stress levels of everyone on the forum, as well as an administrative reduction in the development of the “static” reference information (added post-fact) as the “research” material *actually morphs into* reference information (as you can see from those xda-developers examples i worked on over a decade ago), completely saving you (roger) the job of doing it entirely by yourself without any assistance.

[racemaniac – Tue Oct 24, 2017 7:49 am] –
can’t we discuss it on the wiki, and only allow logins the way it is now?

interesting suggestion… from experience i’ve seen repeated evidence that complex discussions quickly become absolute hell-on-earth for different reasons when using a wiki as a “discussion forum”. each type of online collaborative tool has different strengths and weaknesses.

wikis are great for developing and researching information, that, once finished becomes the “reference guide”, but you try and actually maintain a conversation? you can’t find *anything* because it’s all jammed into one non-linear page, where people are perfectly allowed to just… arbitrarily insert responses anywhere into the document. even if everybody follows the “rules”, after even a few hours absolutely nobody can find anything.

forums are great for having linear conversations online, as if people were in the same physical room, but spread out over time. there’s even a way to “catch up” on the discussion by going back a few messages, you can embed images and so on and there’s no special software needed. but if you actually want to develop something complex, absolutely nobody but the world’s geniuses can hold that much information in their heads, and using the forum *alone* everyone feels like they’re desperately treading water on a ladder that’s constantly sinking into the depths of the ocean, drowning them in messages and information.

mailing lists – particularly with archives – are a great way to do the same job as forums except that they have the advantage of contributors being able to go “offline” at their own discretion. many highly technical collaborators still do this, and they take in vast quantities of messages per day and can keep up-to-date very very quickly with literally dozens of simultaneous conversations across a huge number of lists. however it requires quite strict communications discipline (outlined in “mailing list netiquette” documents) that… most forum users are incapable of understanding, respecting or following… to the detriment of absolutely every technical contributor on that list. so the admin sometimes has to get quite strict about enforcing the netiquette.

irc is great for keeping people in touch in real-time, the problem being they actually have to be *in* real-time i.e. on the same time-zone. when working with xda-developers community members, we found that with the addition of a “bot” that logs everything and publishes it online every 24 hrs (just in case our individual internet connectivity went down) we could leave IRC running 24×7 (or in case of a disconnection refer back to the bot logs) and thus actually have a conversation spread out over 36-72 hours. but if we had tried that *without* the wiki to record detailed notes it would have been a total nightmare.

anyway: it really is down to you, roger, also what you feel comfortable with setting up (and maintaining) i have the ability to set up online resources (i run my own server) but as i mentioned before, it would not be appropriate for me to set up “unofficial” wikis / other online document collaboration tools for users of this forum to use, as they would quickly become part of the infrastructure here: the very first URL/link posted and that’s it, it’s no longer “unofficial”. why? well, if i decide i needed the space on my server the records would be… lost, and any references / archive links here in this forum would be terminated as dead-ends. that would be… bad

and for the discussions, the thread is becoming a bit hard. we’re discussing usb, extra pads for the pins, the usb connectors, the voltage regulators all at the same time >_<
it’s becoming a bit much for 1 thread (imo)

[zmemw16 – Tue Oct 24, 2017 8:26 pm] –
isn’t this about how this forum was started, when it was originally created from an excessively large thread ?
lessons learnt ?
srp

XD
indeed XD
a (temporary) forum subsection so we could split this up in several threads would also work

[racemaniac – Tue Oct 24, 2017 7:41 pm] –
not sure if you know there already is a wiki: http://wiki.stm32duino.com

roger has locked it so that nobody can create an account. only authorised people who already have login details are permitted to edit pages.

[racemaniac – Wed Oct 25, 2017 8:40 am] –
concerning the usb connector: i know of the mid mounted ones, but is the board being a tiny bit thinner that much of an advantage? it also takes away space to route the usb traces/place its resistors, and a usb micro connector is already pretty thin.
it’s a nice to have, but not sure if it’s worth it since pcb area is already short in supply as it is ^^’
(and even more so if we want to offer smd pads for the pins currently not broken out)

Not only thinner, but stronger: the micro USB connectors are supposed to withstand more plug/unplug cycles than mini USB ones, which in turns support more cycles than the original USB type B (the square, bulky one). However, being SMD with tiny dimensions make them very easy to break away with some traces from the PCB if you are too rude or don’t pull/push straight.

This was a major cause of failure on early Red/Blue Pill boards with such micro USB SMD connectors.

Having 4 harpoon-like TH legs does make them much more reliable in this regard, which is IMHO a great feature for a prototype board.

[Squonk42 – Wed Oct 25, 2017 7:31 pm] –

[racemaniac – Wed Oct 25, 2017 8:40 am] –
concerning the usb connector: i know of the mid mounted ones, but is the board being a tiny bit thinner that much of an advantage? it also takes away space to route the usb traces/place its resistors, and a usb micro connector is already pretty thin.
it’s a nice to have, but not sure if it’s worth it since pcb area is already short in supply as it is ^^’
(and even more so if we want to offer smd pads for the pins currently not broken out)

Not only thinner, but stronger: the micro USB connectors are supposed to withstand more plug/unplug cycles than mini USB ones, which in turns support more cycles than the original USB type B (the square, bulky one). However, being SMD with tiny dimensions make them very easy to break away with some traces from the PCB if you are too rude or don’t pull/push straight.

This was a major cause of failure on early Red/Blue Pill boards with such micro USB SMD connectors.

Having 4 harpoon-like TH legs does make them much more reliable in this regard, which is IMHO a great feature for a prototype board.

we’re now using an on top one that has 4 legs trough the pcb, so i would assume it’s about as rugged as the mid mounted ones with 4 pins trough the pcb?
and concerning the thickness of the board, i just realised the crystal we’re using is probably about as high as the usb connector XD

[racemaniac – Wed Oct 25, 2017 8:14 pm] –
we’re now using an on top one that has 4 legs trough the pcb, so i would assume it’s about as rugged as the mid mounted ones with 4 pins trough the pcb?

Well, not quite… There are all-SMD ones that are only for occasional plug/unplug cycles. Then you have the ones with 2 or 4 legs through PCB, that are stronger but that should normally be surrounded (and guided) by the enclosure. Then the harpoon-type that is lower-profile and wider legs (and thus has less lever to tear it off the PCB): this is the heavy-duty one that will resists many cycles without guidance.

[racemaniac – Wed Oct 25, 2017 8:14 pm] – and concerning the thickness of the board, i just realised the crystal we’re using is probably about as high as the usb connector XD

… Then I suggest to change it for a lower-profile one
A quick search on Taobao will give you the price for some common 8MHz crystals:
https://s.taobao.com/search?q=8m+%E6%97 … =price-asc
Here are some interesting smaller (5.0 mm x 3.2 mm x 1.2 mm) SMD alternatives:
https://item.taobao.com/item.htm?spm=a2 … t=4#detail
https://item.taobao.com/item.htm?spm=a2 … t=4#detail
https://item.taobao.com/item.htm?spm=a2 … t=4#detail

Or even smaller ones (3.2 mm x 2.5 mm x 0.8 mm):
https://s.taobao.com/search?q=3225+8+mh … =price-asc
https://item.taobao.com/item.htm?spm=a2 … t=4#detail
https://item.taobao.com/item.htm?spm=a2 … t=4#detail
https://item.taobao.com/item.htm?spm=a2 … t=4#detail

As you can see, there is not much a difference in price compared to the bulky HC-49USX ones, they are all ranging from 0.08RMB to 0.25RMB, i.e. from $0.01 to $0.04.

The 32k crystal can probably be replaced by a smaller one too, with not much price increase:
https://item.taobao.com/item.htm?spm=a2 … t=4#detail

For cheaper PCBA, we should avoid using through hole components that are not reflow or wave-solderable (headers, TH crystal…), as they will be assembled by hand at an additional cost.

And if possible, we should try to avoid putting components on both sides: this will also increase to PCBA cost. Check the Teensy board for a good example:

As for the micro USB connector and crystals, these are all design choices, but if you choose to stick with original crystals, you should then keep the original connector too

Or decide to change everything at once!

If not one of these solutions, it should only be because of lack of real estate on the board.

[Squonk42 – Thu Oct 26, 2017 7:59 am] –
Yes, the Teensy is a 4-layer board with BGA components, but it is also $30…

As for the micro USB connector and crystals, these are all design choices, but if you choose to stick with original crystals, you should then keep the original connector too

well no, it’s all choices XD
i chose to stick close on items that didn’t make much difference for me, and for the usb connector chose somethign more practical :p.

but i’d love to hear some other voices about this. For me it’s all the same which components we use, so far i tried to stay close to the original bluepill, but if we’d prefer a smaller smd crystal & stuff like that, why not .
about getting everything on 1 layer, i could give it a rough try this weekend how feasible that is (but the answer is probably not at all on 2 layers ^^’)

I think it is possible to achieve single-sided component load with smaller but not much more expensive parts, that will partly be gained back by a cheaper PCBA.

On the original Bluepill, the crystals, RESET button and BOOT header are HUGE and TALL: this is probably a good way to get more real-estate to move the components back on the top side.

It is also possible to switch to 0402 passives instead of 0603, except for the ones that could be removed/changed by user.

And on such a small board, having a VCC and a GND layer is not the best thing, given the few VCC required connections: it is usually better to have 2 GND planes with via stitching, and route VCC as (large) traces.

For deliverable, I think it is acceptable to provide both headers and SWD headers unsoldered, especially if we burn the bootloader into the chip, this could save some hand-soldering steps during manufacturing.

C4, C7, C8, C9, C17, C18 and C19 can be placed not far away from their respective pin. Of course, this will require some trace shuffling…

So if you’ve got good sources for choosing for those design decisions, i’d love to hear them, it’s hard finding good information on this stuff, and i love all the feedback i’m getting hear as it’s a great chance to learn .

I design PCBs for more than 25 years professionally, using several ECAD systems. I already did simple boards like these, or much more involved boards with RF routing, matched length, antennas, high speed circuits, etc.

I posted links to an equivalent board I did with EagleCAD 6 years ago as a training while I was learning Eagle, so you can judge.

PCB design and manufacturing is not a science, it is a technology, so don’t expect clear cut answers to your questions. Most of what you will get will be based on past experience and not on rules engraved in stone.

The single-sided load for components should be obvious: when using reflow oven soldering, you will need to perform 2 operations, or to glue the components using epoxy on the bottom side, or they will just fall off… This means twice the time in the factory, this will of course cost more.

Wave soldering will have the same problem, plus the additional restrictions on the footprints that depend on the wave direction, so nobody is using it for small SMDs, it is now almost used for TH component only boards.

As for Through-Hole reflow processing (known as Paste-In-Hole), it is rather complex to set up, so Chinese PCBA factories are generally soldering them by hand after reflow soldering (cheaper), adding an extra steps and of course, costs.

As for power/ground planes, you are right, it is usually good to have the largest possible power supply plane to have an equipotential voltage that can be distributed all over the board, same for ground.

However, there is no definitive rule here: it is good to have both planes, and as large as possible, but without trace cutting these planes in half, as this almost destroys all the benefit of it. For this reason as well as for better EMC handling, it is even thus better to use 4 layer boards and have both planes in the inner layers without internal traces. For high-speed differential signals like PCI @ 2.5/5 Gbit/s, it is almost mandatory to put these signals into inner layers with stackups containing a minimum of 8 layers, or route them on the external layers and shielding everything externally.

But for small boards with only 2 layers like these, the most important is to have the largest possible ground surface as it is impossible to have a good full ground plane without trace on 2 layers, mainly for better EMC, ESD evacuation and ease of layout. A good way to do it is to use 2 under-optimal (e.g. with traces) ground planes and stitch them for the best equipotentiality. There are not many high-power components to feed on such a board, so a star or bus-like power supply distribution is OK, and the only thing to really take care of is to properly filter the analog power supply using a ferrite bead at a single point of connection with the digital supply, unless you have high-power analog needs that will dissipate too much power in it.

As for good sources, you can start by reading the IPC-7351 standard (“Generic Requirements for Surface Mount Design and Land Pattern Standard”), continue by reading all other IPC standards, as well as browsing the ARRL Handbook, among other things.

Then, with around 10 years of practice, you will start to forge your own rules

BTW, I found advises from @lkcl for handling manufacturing to a Chinese company very close to my own experience in order to avoid problems!

[Squonk42 – Sat Oct 28, 2017 1:19 pm] –
To be treated as a self-proclaimed expert is a little bit vexing, I hope it was not intentional.

i thought i worded it as well as possible not to say you are a random self proclaimed expert XD (just that it’s hard to find good info since people indicating they know it all continue to contradict eachother whenever you read discussions on how to do grounding, where to put bypass caps, … >_<).
But did want to know where you got your info from, as i’m still learning all this, and want to know where all the suggestions are coming from (and if they’ve been tried & proven, or just personal preference ).

And that the 2 layer components requires more work is indeed obvious, but seeing a bottom price bluepill board have it (and knowing that things that once were expensive no longer are), that’s then part of the question . is it worth it going single side components if the cost difference is maybe negligible these days? (also a problem with engineering, it’s not because it obvious that it’s the best way to go. As a programmer i know the dangers of premature optimization XD)

i’m certainly taking into account your suggestions, and indeed, it’s probably also partially an art, not an exact science (as is a lot of engineering). it’s just hard to find good references on good practices with everyone saying their solution is best for different reasons ^^’.

And thanks for the nice reply . Sorry if i vexed you, but if i don’t at least ask these questions it becomes really hard to filter all the input (since it’s usually 1 person offloading all their suggestions, and noone confirming or agreeing with anything ^^’)

Concerning the SMD components, i also prefer smd crystals over the through hole ones . so i’ll have a look at updating that too (assuming noone has a good reason to stick to the bigger ones (easier to replace etc… is that required?)), it’s more compact, and if it’s another step less, the better.

[Squonk42 – Sat Oct 28, 2017 1:19 pm] –
I design PCBs for more than 25 years professionally, using several ECAD systems…

Hi Squonk42,
your post is really very interesting! I found some confirmations to some my “thoughts” about PCB design…
Thanks a lot for sharing!

[racemaniac – Sat Oct 28, 2017 7:48 am] –
@Squonk
Can you also back up your ideas with some facts (that all the components on a single side is that much cheaper to produce,

it’s that much cheaper to produce. think about it: the board has to go twice through a pick-and-place machine, twice with the squeegee to wipe solder paste across the stainless steel laser-cut mask… which you now have to pay for two of them not one…

but there’s quite a lot of downward-force applied: they put pins underneath along regular intervals to support the PCB to stop it bending: the 2nd time they have to b extra-careful about where to put those… because now there’s components on the board!

nut the 2nd time they can’t use the standard technique (just bake the board), they have to use something different (i forget what it is) but basically if tthey stick the board in a standard cheap oven the components on the other side will fall off! so the heating profile has to be.. different, i.e. more costly, i don’t know the precise details, but it stops the 1st set of components falling off.

all that has to have extra care *not* just “it’s twice as long therefore it’s twice the cost”, where instead for single-sided, you chuck it in the squeeger, chuck it in the pick-and-place, chuck it in the oven and it’s done.

racemaster if you want to learn more, look up “factoryforall.com”, that’s tully, he worked on the openmoko and decided to stay in shenzhen, set up his own factory and bought his own equipment, actually he would be a great person to use for manufacturing this board. his website’s extremely informative and very entertaining at the same time. say hi from me if you contact him.

[lkcl – Sat Oct 28, 2017 8:38 pm] –

[racemaniac – Sat Oct 28, 2017 7:48 am] –
@Squonk
Can you also back up your ideas with some facts (that all the components on a single side is that much cheaper to produce,

it’s that much cheaper to produce. think about it: the board has to go twice through a pick-and-place machine, twice with the squeegee to wipe solder paste across the stainless steel laser-cut mask… which you now have to pay for two of them not one…

but there’s quite a lot of downward-force applied: they put pins underneath along regular intervals to support the PCB to stop it bending: the 2nd time they have to b extra-careful about where to put those… because now there’s components on the board!

nut the 2nd time they can’t use the standard technique (just bake the board), they have to use something different (i forget what it is) but basically if tthey stick the board in a standard cheap oven the components on the other side will fall off! so the heating profile has to be.. different, i.e. more costly, i don’t know the precise details, but it stops the 1st set of components falling off.

all that has to have extra care *not* just “it’s twice as long therefore it’s twice the cost”, where instead for single-sided, you chuck it in the squeeger, chuck it in the pick-and-place, chuck it in the oven and it’s done.

racemaster if you want to learn more, look up “factoryforall.com”, that’s tully, he worked on the openmoko and decided to stay in shenzhen, set up his own factory and bought his own equipment, actually he would be a great person to use for manufacturing this board. his website’s extremely informative and very entertaining at the same time. say hi from me if you contact him.

i know why it *should* make a huge difference, but i’m wondering if it really *does* make such a difference if dirt cheap boards have components on both sides .
but i’m atm giving it a go routing it with all components on 1 side, lets see if that works out

makes me think of something i recently read on hackaday: back in the days you had to pay per via, so via optimization was important. now if they’re not too small, it doesn’t really matter anymore . it also makes sense that wearing out their drills should cost extra, but it doesn’t (anymore).

[lkcl – Sat Oct 28, 2017 8:38 pm] – racemaster if you want to learn more, look up “factoryforall.com”, that’s tully, he worked on the openmoko and decided to stay in shenzhen, set up his own factory and bought his own equipment, actually he would be a great person to use for manufacturing this board. his website’s extremely informative and very entertaining at the same time. say hi from me if you contact him.

Oh yes, I forgot about him!

Yes, very informative website indeed!

Here are some more resources specifically on PCBA from PCBCart:
https://www.pcbcart.com/article/content … ction.html
https://www.pcbcart.com/article/content … ocess.html

e.g. “What are Fiducials?” on this page http://www.factoryforall.com/pcba-fabrication

[lkcl – Sat Oct 28, 2017 8:38 pm] – it’s that much cheaper to produce. think about it: the board has to go twice through a pick-and-place machine, twice with the squeegee to wipe solder paste across the stainless steel laser-cut mask… which you now have to pay for two of them not one…

I do not have any skills in automated PCB produvtion and it doesn’t interest me in any way, but..
Why the hell are mostly all dirt cheap Arduino/STM Pills 2component sided?
Why have the cheapest Arduino clones gigantic crystals?
Or other way round..why is my only 1sided Uno clone (Robotdyn – excellent quality) not the cheapest?

And yes, I’m wondering about the main crystal on my blue pills.. all soldered manually

I guess if the size of the caps is halved etc, and more expensive small SMD crystal(s) are used it may be possible, but I wonder if the overall cost would be increased by needing to use a fab house that could build with ultra small SMD components etc.

Also the regulators need a big heat sink area of the PCB and I’m not sure thats possible on the top of the board

[racemaniac – Sat Oct 28, 2017 9:15 pm] – i know why it *should* make a huge difference, but i’m wondering if it really *does* make such a difference if dirt cheap boards have components on both sides .
but i’m atm giving it a go routing it with all components on 1 side, lets see if that works out

It does take more steps, please check http://www.surfacemountprocess.com/comp … limit.html:

In the Bluepill case, bottom side is side B with only small resistors, caps and small LDO, all without epoxy glue as they are small, then the big components (MCU, 32kHz crystal, micro USB, button and fragile plastic LEDs) on top side (A).

The jumper blocks, 8 MHz crystal and SWD header are then manually soldered (you can tell because of the flux residue around the pins on the bottom side, they don’t even care to clean it).

Add 2 rows of 20-pin headers along with the board and seal it in an anti-static bag.

The original Bluepill board was designed and manufactured by VCC-GND, the price is 18.90RMB ($2.84). But you can find dirt cheap clones down to 7.35RMB ($1.11), when the cheapest STM32F103C8T6 chip you can find is at 7.00RMB… As you can see, the price is very subjective! It depends if you get new or used (possibly defective or untested) parts, non-RoHS process, (non-)testing, grey shift assembly and/or bad working conditions, etc.

If you want to stay with decent assembly conditions, RoHS (you have to!) and (mostly) controlled part origin, then you will find that everything has a price. The manufacturer may not say so, but in the end, they will charge you more

[racemaniac – Sat Oct 28, 2017 9:15 pm] – makes me think of something i recently read on hackaday: back in the days you had to pay per via, so via optimization was important. now if they’re not too small, it doesn’t really matter anymore . it also makes sense that wearing out their drills should cost extra, but it doesn’t (anymore).

Chinese PCB manufacturers no longer charge for more vias, as they found that it is almost proportional to the board area. You can play with online PCB quoting forms like SeeedStudio Fusion to see what really matters today.

As for the 32 kHz crystal, we can either leave the bulky SMD MC-306 one, or replace it by a smaller FC-135 package with known CL (12.5pF)

The BOOT header will have to be replaced by a tactile button, like in the Mapple Mini. The smallest and cheapest I know is the ALPS SKSGACE010, also used in the NodeMCU board. Like the Mapple Mini, you can also connect it to a GPIO (PB8) through a 0R to get a free USER button…

The DMP2160UW PMOS is a good idea to get a low-drop diode.

The SY6280 is good and very cheap. A TPD3S0x4 combined USB Current Limit Switch and D+/D– ESD Protection like in the Teensy 3.6 would be nice to have, but too expensive. For a dev board where you can touch all chips with your fingers, ESD is not really a concern (you do wear a wrist ESD strap, don’t you? ).

Please don’t use a precious PC9 pin for the USB switch enable pin: it is part of the few pins that can provide SDIO interface functionality, so we would better use a dumb pin like PC0 or PC1 for this purpose. My idea would be to add an optional MicroSD socket on the (now flat) bottom side routed like the MicroPython board. Refer to my previous post you may have missed. Now, you know why I insist on having all components on top .

I think that both SDIO and I2S could be very interesting additions to the standard STM32F103C8T6 Bluepill, meaning that PD2 and PC8-12 should be used for the optional onboard SDIO connector, and PC6-7 for the only available I2S MCK pins as TH pads…

Don’t forget that STM32F103RBT6 are almost pin-to-pin compatible with STM32F405RGT6 64LQFP package and cost the same price as the STM32F103C8T6… Provided we take care of the VCAP pins (replace 2u2 caps by 0R for F103) and add an optional USB pull-up on PA12. We may then have 2 versions of the board sharing the same PCB, one with F103, one with F405.

Optionally run the SPI to the SDIO socket? Maybe too many troubles, but would be nice to have for F103.

BTW, pin 1 of bottom edge header should be VBAT (i.e., on the SWD header side, not near the micro USB connector).

btw, before i take a “wrong” micro sd slot, which one would you guys recommend?

You prove that it is possible to keep the same form factor with only minimal changes. Now with more involved component selection and single-side PCB routing, we could keep the price reasonable and pack as much feature as possible.

We can use 6 mils/6 mils/0.3mm PCB manufacturing at no additional cost, this is considered in China as the “PCB prototype quality”, like you can find at most online PCB vendors (see SeedStudio above), so it is reasonable to go down to these specs.

We should seriously consider if we keep the original PCB dimensions of 2.1″ x 0.9″ (53.24mm x 22.86 mm), or if we reduce it a tad to match the recommended 50 mm used by most of the cheap PCB houses… This may perhaps help reduce the cost, or at least it will reduce it for those willing to DIY, because we could panelize 2 of them in a 50 mm x 50 mm square.

Keeping 0603 parts for small resistors and caps <= 100nF is a choice: do we go for 0402 or do we keep the ability to perform DIY soldering with minimum soldering skills? This won’t save a lot of real estate, but this may help greatly to place parts in a more optimal way.

For the crystals, the most difficult is to find parts with a specified CL, which is seldom the case on TaoBao or Aliexpress.

Regarding the microSD socket, look at 104031-0811 from Molex. Only 11.95 mm wide, meaning that it fits between the BP rows of pins… And you can find it cheap on TaoBao from many vendors.

USBugSmall.png (126.82 KiB) Viewed 186 times

I think it works because it looks like the limits set from copper to board edge is not so strict (some manufacturers do not specify it) and depends on the PCB feed direction: the PCB are moved between 2 parallel rails that are either ~6 cm (5 + 2 * 0.5 mm) or ~11 cm (10 + 2 * 0.5 mm) apart:

This is why prototypes services are so strict on dimensions (5 cm or 10 cm), they don’t want to set up the rails for each new board! Then the other dimension is set to 5 cm or 10 cm too, probably for convenience during storage.

Our edge connectors are 20 x 0.1″ = 2″ =5.08 cm long, so when you round them to 5 cm, you cut their last copper pads at the extremities by only 0.04 mm (1.6 mil) each, and as we are cutting perpendicular to the rails above, it should be OK.

BTW, should we keep the PCB area outside the 2 rows of header with silkscreen pin legend or not? They end up wasting 1 breadboard hole on each side of the PCB…

I had the opposite idea about the length…

If there is not enough space on the top of the PCB it could probably be increased by 2 or perhas 3mm at each end, as its unlikely that anyone who has built a board that houses the Blue Pill would have squeezed it in that tightly.

I dont think placement of the SWD connector is critical, and you could drop the Vcc and Gnd pins on that header, as both those connections are available elsewhere.

@squonk42

Thanks for the heads up about the SDIO pins etc.

SDIO and I2S are important as they are not available on the F103C8

Re:resistor size that allows hand soldering.

I don’t think this is necessary

Removing even the smallest SMD resistirs isnt that hard using a soldering iron, as in my experience they seem to stick to the solder and flux and just come away from the board when you remove the iron.

I cant think of any circumstances when people would want to replace resistors

Re:Pads for unised MCU GPIO pins on the bottom of the board.

Hakimg back to the Teensy… We could do this if no components were on the bottom of the board

Re:regulator

I thought there were heat dissipation issues unless the regulator was on the back of the board where there was a lot of copper to dissipate the heat ??

[RogerClark – Sun Oct 29, 2017 9:21 am] –
Looking at the last design posted by @racemaniac in the PCB 3D viewer, I think its going to be a tough job to get all the components onto the top of the PCB.

I guess if the size of the caps is halved etc, and more expensive small SMD crystal(s) are used it may be possible, but I wonder if the overall cost would be increased by needing to use a fab house that could build with ultra small SMD components etc.

Also the regulators need a big heat sink area of the PCB and I’m not sure thats possible on the top of the board

It is possible using small crystals and buttons, still using huge 0603 passives (sorry, still using EagleCAD):

BluePillF4.png (55.59 KiB) Viewed 168 times

[RogerClark – Sun Oct 29, 2017 9:32 pm] – Re: PCB length

I had the opposite idea about the length…

If there is not enough space on the top of the PCB it could probably be increased by 2 or perhas 3mm at each end, as its unlikely that anyone who has built a board that houses the Blue Pill would have squeezed it in that tightly.

Well, I agree we could extend the board in length, the 5 cm limit comes from the cheap prototype PCB houses that use this as a billing threshold.

[RogerClark – Sun Oct 29, 2017 9:32 pm] –
I dont think placement of the SWD connector is critical, and you could drop the Vcc and Gnd pins on that header, as both those connections are available elsewhere.

Yes, good idea, just right next to the SWD connector!

[RogerClark – Sun Oct 29, 2017 9:32 pm] – @squonk42

Thanks for the heads up about the SDIO pins etc.

SDIO and I2S are important as they are not available on the F103C8

Yes, and even better: if we use PC10 for SDIO_D2, PC11 for SDIO_D3/CD and PC12 for SDIO_CK, they just happen to match USART3_TX, USART3_RX and USART3_CK, respectively on the STM32F103Rx, this means that we could possibly drive the SD Card in SPI for the 103!

[RogerClark – Sun Oct 29, 2017 9:32 pm] – @squonk42
Re:resistor size that allows hand soldering.

I don’t think this is necessary

Removing even the smallest SMD resistirs isnt that hard using a soldering iron, as in my experience they seem to stick to the solder and flux and just come away from the board when you remove the iron.

I cant think of any circumstances when people would want to replace resistors

OK, then we will move down to 0402 for all passives except caps > 100n.

[RogerClark – Sun Oct 29, 2017 9:32 pm] – Re:Pads for unised MCU GPIO pins on the bottom of the board.

Hakimg back to the Teensy… We could do this if no components were on the bottom of the board

Yes

[RogerClark – Sun Oct 29, 2017 9:32 pm] –
Re:regulator

I thought there were heat dissipation issues unless the regulator was on the back of the board where there was a lot of copper to dissipate the heat ??

The AP2114AH in SOT223 package has a Tja of 128°C/W without heatsink, and the STM32F405 has a max current draw of 450mA. When powered from 5V, the heat dissipated will be (5V – 3.3V) * 0.45A = 0.4W, or a 52°C rise in temperature above ambient, all with a drop-out voltage that will allow for powering from a LiPo battery (450mV DO @ 1A), even less dissipated heat when powered from battery. We cannot feed a nuclear power plant, but we have some room for powering external stuff before frying the LDO.

OTOH, I benefit from my existing part library!

Here is my current schematic for open discussion.

BluePill F4 Schematics.pdf

(58.07 KiB) Downloaded 30 times

Plus, you don’t have to put the buttons on the USB side like the original, you can move them on the SWD side if necessary (see my part placement above).

Breaking out the analog VCC/GND on header is a good thing, but it breaks the compatibility with existing Bluepill boards, @RogerClark: what do you think?

In my schematics, I just dropped the LDO providing the analog power supply: this is a luxury IMHO. Better have a good ferrite bead between +3V3 and +3V3A only to filter high-frequency noise, and have (as much as possible on such a small board) separate GND and GNDA only connected at a single point, which is the normal way to handle analog/digital coexistence. Adding a ferrite bead between GNDs is not necessarily a good thing for small signals, as it will create a voltage offset between GNDs that depend on ground currents, better put a trace only.

But you could add another pin (through hole) somewhere else, or just a pad on the underside etc

*edit*
after thinking about it a bit more, aren’t both options incompatible?
If i don’t put the analog 3v3 on the standard header, anyone feeding their bluepill via the standard header and doing something analog is out of luck, since the analog part won’t be powered at all.
at least for my solution, if you provide power via both 3v3 pins, the entire board is powered. now i don’t have any bluepill shields/projects that rely on this, so not sure what people who expect pin compatibility are expecting, but i think my solution also has some merits.

the only other option would be a jumper to connect 3v3a with 3v3 (or a small solder bridge you can make, a jumper would be a bit big), and then just keep the regular 3v3 on both pins.

Yes. I guess it would be possible to use one of the Vcc’s as analog Vcc.

Are you using a really small regulator for analog Vcc, or is it roughly equivalent to the cheap regulator on the Blue Pill ?

What advantage is there to having the analog vcc available for external circuits?
Lower noise than the main regulated output ?

I suspect people may use the Vcc pins to power a lot of things and existing designs may link them in their PCB, or assume they are connected together internally.

[RogerClark – Mon Oct 30, 2017 9:59 am] –
@racemaniac

Yes. I guess it would be possible to use one of the Vcc’s as analog Vcc.

Are you using a really small regulator for analog Vcc, or is it roughly equivalent to the cheap regulator on the Blue Pill ?

What advantage is there to having the analog vcc available for external circuits?
Lower noise than the main regulated output ?

I suspect people may use the Vcc pins to power a lot of things and existing designs may link them in their PCB, or assume they are connected together internally.

for analog i’m using the small ap2112 (the one i originally used for the non analog part too, but that was found to be too light).

and there is no very specific reason to have the analog 3v3 also available on the pin headers (other than it at least being reachable/connectable if you’re not using a 5v supply).

it seems we’ve found another design decision to make:
– keep the original pins (both just 3v3, the analog supply then maybe on other pins) -> not quite a fan of this honestly. taking up quite some extra space for this…
– my solution of having the 3v3a & gnda on the pins next to the programming header -> probably also not ideal, depends on how the original bluepills are used (if they power via both 3v3 pins, it’s compatible (as both grounds are tied together via a ferrite bead), otherwise they’d have to make sure to power the other 3v3 pin too)
– keeping the original pins, but offering a jumper/solder bridge that can be made to tie the 3v3 to 3v3a -> very compatible, but it’s less elegant if you want to provide your own analog 3v3 rail (you can connect your 3v3a to the appropriate pin of the jumper/solder bridge, but the analog ground isn’t really broken out in this case…)
– probably some other options i’m not seeing yet ^^’

each choice has its advantages & disadvantages, kepping 100% compatibility is impossible if we now have a separate analog 3v3, so we’ll have to pick our compromise .

From AN2586 “Getting started with STM32F10xxx hardware development”:
Power supply schemes
The circuit is powered by a stabilized power supply, VDD.
● Caution:
– If the ADC is used, the VDD range is limited to 2.4 V to 3.6 V
– If the ADC is not used, the VDD range is 2.0 V to 3.6 V
● The VDD pins must be connected to VDD with external decoupling capacitors (one
100 nF Ceramic capacitor for each VDD pin + one Tantalum or Ceramic capacitor (min.
4.7 µF typ.10 µF).
● The VBAT pin can be connected to the external battery (1.8 V < VBAT < 3.6 V). If no
external battery is used, it is recommended to connect this pin to VDD with a 100 nF
external ceramic decoupling capacitor.
● The VDDA pin must be connected to two external decoupling capacitors (100 nF
Ceramic + 1 µF Tantalum or Ceramic).
● The VREF+ pin can be connected to the VDDA external power supply. If a separate,
external reference voltage is applied on VREF+, a 100 nF and a 1 µF capacitors must be
connected on this pin. In all cases, VREF+ must be kept between 2.4 V and VDDA.
● Additional precautions can be taken to filter analog noise:
– VDDA can be connected to VDD through a ferrite bead.
– The VREF+ pin can be connected to VDDA through a resistor (typ. 47 Ω).

Well beyond what a small ferrite choke could clean up.

The amplifier was for a HB100 doppler radar module, and I have since found a better design for the amplifier which uses its own regulator to minimise the noise.

IMHO, I think before the analog Vcc regulator was removed, we would need to make sure its definitely not needed, by doing some practical validation on real hardware.

Decoupling Insertion Loss.png (36.85 KiB) Viewed 354 times

[Squonk42 – Sun Oct 29, 2017 12:47 pm] –
Regarding the microSD socket, look at 104031-0811 from Molex. Only 11.95 mm wide, meaning that it fits between the BP rows of pins… And you can find it cheap on TaoBao from many vendors.

no. not that one. it’s more expensive and not as ubiquitous in the futian district. molex is also known for being way overpriced.

use the one known as “TF Card”, push-push, with the footprint below:

Untitled.jpg (17.41 KiB) Viewed 350 times

I also consider it as a not mounted option with only a provision for the footprint by default.

Now if you can find a cheaper one having width < 500 mils (12.7 mm), I take it

EDIT: maybe this one or these simpler no push-push ones will do, difficult to tell, there are no dimensions. If someone can ask the vendors for a 2D drawing…

104031-0811.png (20.19 KiB) Viewed 336 times

A 600ohm Ferrite Bead does not have 600ohm “resistance”. That “600ohm” is “impedance – mostly an inductive reactance” at some frequency (ie 100MHz). Ferrite beads have got 0.0xx ohm DC resistance typically..
Even with 600ohm/100MHz impedance and the ADC’s bandwidth (could be ~1MHz) the FB will not have any significant impact on the 1LSB variation (as the FB’s impedance at 1MHz would be maybe 2-5ohm)..

PS: there are smd “inductors” and smd “feritte beads” available.

The inductors are rated in uH or nH, while FBs in “ohms” (an impedance at 100MHz).

Use FBs only, as the “inductors” have got large DC resistance (0.x to ~ohms) and low self-resonance (~1-100MHz) such they will ring…

Also you want to use an FB with rather lower impedance (ie 30-100ohm) as the larger values will peak as well (they do self-resonate at >=200MHz)..

The consensus, was this is not needed on the F4

Re: USB 22ohm resistors.

i think this is best practice, but optional, depending on space on the PCB

Re: Regulator for analog Vcc

I presume that Leaflabs had a good reason for using the second regulator. I suspect, its potentially cheaper and takes less space on the PCB than the passive components you would need instead

Re: 50 mm long board and components in bottom of board

I think with too many constraints, the board is going to take months to design and may never get produced.

Perhaps move as many as possible to the top without wasting hours of time and potentially adding conflicts to the PCB

[RogerClark – Tue Oct 31, 2017 8:17 pm] –
Re: USB pullup

The consensus, was this is not needed on the F4

Yes, but if you make a provision for it, along with replacing the 2x VCAP capacitors by 0R shunts, the board is then compatible with all LQFP64 STM32s, including L4s, and including the SD Card connector through SPI… I think it is really worth the pain!

[RogerClark – Tue Oct 31, 2017 8:17 pm] –
Re: USB 22ohm resistors.

i think this is best practice, but optional, depending on space on the PCB

Agreed, this is usually a provision for CEM certification by replacing with a CMC or adapting the values to get a better eye-diagram for USB certification. Not needed, but we may keep it if we have enough real estate on the board.

[RogerClark – Tue Oct 31, 2017 8:17 pm] –
Re: Regulator for analog Vcc

I presume that Leaflabs had a good reason for using the second regulator. I suspect, its potentially cheaper and takes less space on the PCB than the passive components you would need instead

Not sure, as the regulator will need at least 2x caps anyway (1x at the input, 1x at the output), and you still need at least a decoupling cap near STM32’s AVDD pin, so it is necessarily more expensive, takes more space, and dissipates more power than a passive solution. Probably Leaflabs did not think much when doing this, and just used a bazooka to kill a fly. BTW, the Mapple is the only small dev board I have seen that used a second LDO for analog supply

[RogerClark – Tue Oct 31, 2017 8:17 pm] –
Re: 50 mm long board and components in bottom of board

I think with too many constraints, the board is going to take months to design and may never get produced.

Perhaps move as many as possible to the top without wasting hours of time and potentially adding conflicts to the PCB

If the 50 mm constraint only applies to small PCB prototypes and not to the intended manufacturer, then we should get rid of it, as well as using only 0603 passive components and move down to 0402 alltogether, as this won’t be more expensive and save us some space on the board.

As for double-sided component load, it will be more expensive than single-sided, but the question is how much for the intended manufacturer again. If not too much, then we should only try to make room on the bottom side for the optional SD Card connector. This connector may be too big to be soldered economically on the bottom side, though…

Maybe we should ask the manufacturer for the price difference? If honest, they will tell us, otherwise, they will just take the max price and tell us it is the same price

As for additional pins to break out, a clever solution is to use a second row of 2.54mm holes offset by 1.27mm, like the LicheePi Zero (btw, look at their TF Card connector! It is a Molex 47309-2851, it fits between the 2 header rows):

[RogerClark – Tue Oct 31, 2017 8:17 pm] – ] Re: Regulator for analog Vcc

I presume that Leaflabs had a good reason for using the second regulator. I suspect, its potentially cheaper and takes less space on the PCB than the passive components you would need instead

Not sure, as the regulator will need at least 2x caps anyway (1x at the input, 1x at the output), and you still need at least a decoupling cap near STM32’s AVDD pin, so it is necessarily more expensive, takes more space, and dissipates more power than a passive solution. Probably Leaflabs did not think much when doing this, and just used a bazooka to kill a fly. BTW, the Mapple is the only small dev board I have seen that used a second LDO for analog supply

The LeafLab Maple Mini was a 4 layer PCB with an analog ground plane and a separate digital ground plane. The separate voltage regulator for the analog likely was a decision made to enhance the overall low-noise floor. Most of us have come to think of the Maple Mini being the 2-layer knockoff from China.

Ray

@squonk42

I forgot about F103R compatibility.

I think this needs to be a secondary consideration, as the primary focus as F4

The MCU is on the underside of the board, along with 8Mhz crystal (in a SMD package) and the regulator and the USB reset transistors

The top has the buttons, LEDS, USB socket and other passive components.

So…

My guess is that the cost of putting components on both sides of the boards can’t be a big factor to these companies, otherwise they’d have spent a bit more time on the design and put all the components on one side.

BTW. The original LeafLabs Maple mini has components on both sides of the board as well

(there is photo of the bottom of the Maple mini on Leaflabs site)

[RogerClark – Tue Oct 31, 2017 8:17 pm] – Re: 50 mm long board and components in bottom of board

I think with too many constraints, the board is going to take months to design and may never get produced.

Perhaps move as many as possible to the top without wasting hours of time and potentially adding conflicts to the PCB

tbh, personally i still prefer the bluepill solution: big things on 1 side, small things on the other.
It’s the reason why the bluepill has been the board i’ve been putting other mcu’s on. the maple mini’s pads don’t allow a qfn to fit, and the blackpill has small caps right next to the mcu, so changing the mcu means you’ll also be removing the caps, and is just annoying extra work .
if we want to allow for people to change crystals/mcu/… easily, making sure there are no tiny caps/resistors right next to them makes a lot of sense .

OK, then it is a completely different story and much more understandable, thank you Ray! Low-cost was then not the primary concern like for us here. 4-layer is more expensive.

Re: Components on both sides of the PCB
It looks like it is a cheap option, so let’s go for it!

However, I agree with @racemaniac to put all large components (what about the SD Card connector?) on top and small ones on the bottom. Plus, because of the package size, we don’t have much space to sprinkle the decoupling caps around it, putting them below the chip would be much better and also easier for replacing the chip. For crystals, this is may be different, as vias should be avoided if possible on the clock traces.

Re: F103R compatibility
Not only F103R, but all STM32 MCUs featuring the simple USB Device peripheral in LQFP64 package:
STM32L052R6 STM32L052R8 STM32L053R6 STM32L053R8 STM32L063R8 STM32L072RB STM32L072RZ STM32L073RB STM32L073RZ STM32L083RZ STM32L100R8 STM32L100R8-A STM32L100RB STM32L100RB-A STM32L100RC STM32L151R6 STM32L151R6-A STM32L151R8 STM32L151R8-A STM32L151RB STM32L151RB-A STM32L151RC STM32L151RC-A STM32L151RD STM32L151RE STM32L152R6 STM32L152R6-A STM32L152R8 STM32L152R8-A STM32L152RB STM32L152RB-A STM32L152RC STM32L152RC-A STM32L152RD STM32L152RE STM32L162RC STM32L162RC-A STM32L162RD STM32L162RE STM32L433RB STM32L433RC STM32L443RC STM32L452RC STM32L452RE STM32L462RE STM32F070RB STM32F072R8 STM32F072RB STM32F078RB STM32F102R4 STM32F102R6 STM32F102R8 STM32F102RB STM32F103R4 STM32F103R6 STM32F103R8 STM32F103RB STM32F103RC STM32F103RD STM32F103RE STM32F103RF STM32F103RG STM32F302R6 STM32F302R8 STM32F302RB STM32F302RC STM32F302RD STM32F302RE STM32F303R6 STM32F303R8 STM32F303RB STM32F303RC STM32F303RD STM32F303RE STM32F373R8 STM32F373RB STM32F373RC
This is a long dropped-compatibility list for just a small 0402 pull-up resistor, don’t you think?

Now, I agree that the Maple Mini dual transistor disconnect feature is probably a bit of overkill.

[racemaniac – Wed Nov 01, 2017 10:30 am] –
Concerning the dual supply: if we don’t go for a dual supply, can someone draw me a schematic of what we would replace it by?

See my post above: a simple PI filter with 1µF cap, 470R ferrite bead and 100nF close to the AVDD pin:

I will try to experiment this filter on a real BluePill 3.3 pin tomorrow

Other subject, I found this simple (no push-push) narrow (12.2 mm) and cheap (0.17RMB = $0.03) SD Card connector on Taobao:
https://item.taobao.com/item.htm?spm=a2 … t=4#detail

Do we need to keep the PCB overhang on the outside of the header rows? On one hand, it is convenient to silkscreen to pin name, but OTOH, it makes the board wider by 2 pins on a breadboard…

Re: VBUS valid sensing for HNP SRP

In the STM32F4 Reference Manual RM0090, page 1254, section 34.6.2, there is a mention about connecting PA9 as a VBUS sensing for HNP/SRP: googling around, I found that both SRP (Session Request Protocol) and HNP (Host Negotiation Protocol) are 2 USB OTG protocols, but does anybody knows if these are required for proper USB operation or not?

Having to connect PA9 to VBUS would be rather inconvenient, as it also has the USART1_TX function used by the ROM bootloader…

[racemaniac – Fri Oct 20, 2017 11:28 am] – ..but i do understand that as it currently is, it’ll be easier to have actually produced by someone.

Ok, seems to be my fault, I just read the first post carefully again… now I understand all those fuckin’ Taobao links better

Nevertheless, i found some KiCad projects in here, so why not combine both, elec freak who like to solder and designs ready for production?
Resourcing for the needed component should be the problem of the producing factory(ies), normally they should know where to buy

When I must read all that stuff regarding two or multilayer, SDcard and so on..plz keep in mind the header: f4 versions of “the BluePill”!
The “BluePill” has no SD card, has two layers, 2-sided components, not the smallest.. in short: its cheap, its cheaper, its cheapest – that’s all!

[ChrisMicro – Sun Oct 29, 2017 9:01 am] –
This one ? RobotDyn?

No, as I wrote UNO
the predecessor of this one
from times when they started selling on ALI – with free shippin’ that time;)

[bianchifan – Fri Nov 03, 2017 10:20 am] – Resourcing for the needed component should be the problem of the producing factory(ies), normally they should know where to buy

Yes, but defining exactly what to buy is the designer’s problem
And to get the cheapest solution, you need to compare different sources!

[bianchifan – Fri Nov 03, 2017 10:20 am] – When I must read all that stuff regarding two or multilayer, SDcard and so on..plz keep in mind the header: f4 versions of “the BluePill”!
The “BluePill” has no SD card, has two layers, 2-sided components, not the smallest.. in short: its cheap, its cheaper, its cheapest – that’s all!

Yes, but the BluePill has some well known flaws:

• wrong USB pull-up resistor
• Bad analog power supply / ground, resulting in poor ADC performance
• Useless BOOT1 header & jumper
• BOOT0 header & jumper are huge, could be more practical to have a second button instead

Now if you go from STM32F103 to STM32F405, you got more problems:

• larger package: 10×10 LQFP64 vs. 7×7 LQFP48, doesn’t fit so easily!
• Power consumption: 240 mA vs. 50 mA max, so you need a beefier voltage regulator (at least 600 mA) to be useful, with low drop-out voltage (< 250 mV) for the board to allow powering from a 3.7V LiPo battery

Now, besides more processing power, single-precision FPU, more Flash and RAM memory, the STM32F405 also brings in some nice features:

• USB OTG: but if you want to implement Host mode, you need to provide an USB load switch
• SDIO: you need at least to break out these pins, or provide an optional SDIO socket
• I2S: here, too, you need at least to break out the additional pins
• More GPIOs: break out if possible

… All this on a 2-layer, 2-sided components, same form-factor board at the cheapest possible price: this is exactly where we are at, by weighting carefully each component and each decision together

However I am not sure on the setup for the pick and place machines.

Probably best to speak to a company who already manufactures a similar board.
Robot Dyn have replied to 2 of my emails about their Black Pill board, so perhaps if we placed a large enough order they may be interested.
Basically its all about the money. I can get boards hand soldered in China, but they charged around $10 each , and that was for a less complex board

[racemaniac – Fri Nov 03, 2017 4:03 pm] –
btw, concerning the buttons
Squonk, i like the small buttons you linked… but can’t find them anywhere on aliexpress or ebay (okay, i could find them from 1 seller at a ridiculously high price more than 1€ a piece)
Can we maybe find some buttons that are small enough and that can easily be sourced by those wanting to make their own boards?

I usually buy them from Mouser, but they are also available at other online distributors.

[RogerClark – Fri Nov 03, 2017 7:34 pm] –
Perhaps the best solution with the components is to initially supply them to the manufacturer

However I am not sure on the setup for the pick and place machines.

Probably best to speak to a company who already manufactures a similar board.
Robot Dyn have replied to 2 of my emails about their Black Pill board, so perhaps if we placed a large enough order they may be interested.
Basically its all about the money. I can get boards hand soldered in China, but they charged around $10 each , and that was for a less complex board

IMHO, the best approach is to first design a board with a careful part selection, so they can be sourced cheap both from China (TaoBao is a good way to check for the best deals) and from either global online distributors or AliExpress/eBay.

The idea is to correct the BluePill flaws, take into account interesting features in more powerful chips like the F405, but without adding to the bill or over-engineering.

Then get the PCB done and assemble some prototypes by hand by as many volunteers in this forum as possible to debug the design and correct hardware bugs.

And eventually, we could approach some manufacturers with gerber and BOM files, and ask them for the cost of sourcing, PCBA, bootloader flashing, storage and shipment from AliExpress/eBay/Amazon direct from China. Maybe charge a small extra fee to pay your server and electricity bill, Roger

[Squonk42 – Fri Nov 03, 2017 9:26 pm] –

[racemaniac – Fri Nov 03, 2017 4:03 pm] –
btw, concerning the buttons
Squonk, i like the small buttons you linked… but can’t find them anywhere on aliexpress or ebay (okay, i could find them from 1 seller at a ridiculously high price more than 1€ a piece)
Can we maybe find some buttons that are small enough and that can easily be sourced by those wanting to make their own boards?

I usually buy them from Mouser, but they are also available at other online distributors.

that’s great, but i’m from europe ^^’
buying from the likes of mouser/digikey/… is pretty expensive in shipping fees for me ^^’

but after looking i actually found 1 aliexpress seller selling it at a good price: aliexpress link
Besides the measurements, isntead of giving the part number in the description, it’s the name of the photo -_- (thanks google for finding that)

[racemaniac – Sat Nov 04, 2017 6:47 am] –

[Squonk42 – Fri Nov 03, 2017 9:26 pm] –
I usually buy them from Mouser, but they are also available at other online distributors.

that’s great, but i’m from europe ^^’
buying from the likes of mouser/digikey/… is pretty expensive in shipping fees for me ^^’

Me too

[racemaniac – Sat Nov 04, 2017 6:47 am] – but after looking i actually found 1 aliexpress seller selling it at a good price: aliexpress link
Besides the measurements, isntead of giving the part number in the description, it’s the name of the photo -_- (thanks google for finding that)

Thank you for sharing the link. We are lucky, this button is used in BMW/Mercedes car keyfobs!

so.

that’s one possible outlet and he has several westerners visiting him because he’s known to either have stuff in stock, or he and his brother can order it for you. i think he’s a really good person to know. so! once this board is up and running i’ll make sure he gets some to sell.

[racemaniac – Tue Nov 28, 2017 7:04 am] –
woow, nice!
you’re routing that in 2 layers? XD

Thanks!

Yes, 2 layers, 6 mils trace width / 6 mils spacing, 6 mils annular ring and 12 mils (~0.3 mm) min holes, passed DRC/ERC!

[Pito – Tue Nov 28, 2017 8:12 am] –
How many free holes along the edges you get when you insert it into a solderless breadboard?

It is the same form factor and pinout as the “original” BluePill, i.e. 2.1″ x 0.9″.

[Squonk42 – Tue Nov 28, 2017 8:17 am] –

[racemaniac – Tue Nov 28, 2017 7:04 am] –
woow, nice!
you’re routing that in 2 layers? XD

Thanks!

Yes, 2 layers, 6 mils trace width / 6 mils spacing, 6 mils annular ring and 12 mils (~0.3 mm) min holes, passed DRC/ERC!

that’s then 24mil vias?
i think most cheap services specify 25/27 mil vias with 12 mil drill (although, a service like dirtypcb probably will just build it like that, some others may actually refuse it from what i heard)
i’m very curious to see how you routed all that XD. (and glad someone else is helping out, i’ve got too many electronics projects happening ^^’. it’s becoming a fulltime job)

[racemaniac – Tue Nov 28, 2017 9:12 am] –
that’s then 24mil vias?
i think most cheap services specify 25/27 mil vias with 12 mil drill (although, a service like dirtypcb probably will just build it like that, some others may actually refuse it from what i heard)
i’m very curious to see how you routed all that XD. (and glad someone else is helping out, i’ve got too many electronics projects happening ^^’. it’s becoming a fulltime job)

I used SeeedStudio Fusion PCB Service with these specs, 0.3 mm min hole + 6 mils OAR, $15.05 for 10 panels of 5 PCBs (fitted on 10 cm x 10 cm):
http://support.seeedstudio.com/knowledg … cification

[Squonk42 – Tue Nov 28, 2017 12:41 pm] –
@RogerClark: I cannot attach the 877 KB ZIP file to a post, how may I proceed?

weren’t the files already being committed to the github repo? maybe create a pull request to the stm32duino github

[Squonk42 – Tue Nov 28, 2017 12:41 pm] –
@RogerClark: I cannot attach the 877 KB ZIP file to a post, how may I proceed?

Share over google drive?

The hosting has space limits which I am already pushing up against and I do not want to have to spend more on hosting this site.

(I know I could move hosts etc, but this is not the only site i run in this hosting plan and it would take days to move it all and reconfigure )

As this is my first design using KiCAD, please accept my mistakes!

The design uses only 0603 passive SMT components, and I routed the board on 2 layers using 6 mils trace width / 6 mils spacing, 6 mils annular ring and 12 mils (~0.3 mm) min holes constraints and passed DRC/ERC.

It should have most of the features discussed previously in this thread, plus some more:

Form factor:

• same form factor as “original” BluePill: 2.1″ x 0.9″ (53.34 mm x 22.86 mm)
• same pinout, except for corner +3.3V, replaced by backward-compatible +3.3VA (Analog power supply)

Power supply:

• ultra low-drop, high current (1A) AP2115HA-3.3TRG1 LDO, compatible with standard 1117 LDO pinout, but should work with +3.7V LiPo batteries
• optional AP2112K3.3-TRG1 LDO for Analog power supply or cheaper CLC filter with ferrite bead

LEDs:

• 1 green LED for POWER
• 1 red LED connected to PC13

Buttons:

• 1 miniature RESET switch button
• 1 miniature BOOT0 switch button, can be tied to PB8 using a shunt resistor (default, like Maple Mini)

SWD header: like BluePill
SDIO:

• connected to SDIO peripheral on STM32 devices featuring it
• should map nicely to simple SPI on other STM32s (to be tested!)
• SDIO connector is optional, mounted on PCB bottom side, ultra simple push-pull plastic connector for cheapest price

USB:

• Micro USB type B connector “harpoon-style” for preventing it from tearing off the PCB
• USB OTG for STM32 devices supporting it: ID pin input on PA10, USB overvoltage / overcurrent protection using a SY6280 with enable pin on PC4
• 1.5k USB pull up for STM32s only supporting USB Device mode
• 5V / VUSB reverse protection using a DMP2160UW-7 MOSFET as a low drop-out diode

Expansion:

• 2x 20 pin 2.54 pitch headers, backwards compatible with BluePill pinout
• one +3.3V replaced by +3.3VA (Analog power supply)

MCU:

• Supports STM32F405RGT6 or any STM32FxxxRyyy (all LQFP64 packages)!
• Breaks out all GPIOs on pin headers, except PC0-PC3 and PC5-PC7 as test points. PC4 is used for VBUS_EN and PC8-PC12 are used for internal SDIO connector
• 8 MHz crystal
• 32 kHz crystal

There are some options available:

• Separate Analog power supply using an LDO or a CLC ferrite bead Pi filter (mount ether U2 or L1 but not both)
• Connect BOOT0 button as USER button on PB8 (mount R5 or not)
• SDIO connector on bottom PCB side (mount C16/J4/R12 or not)
• Overvoltage / overcurrent protection for USB OTG (mount U4/R7R11//R13 or not)
• USB D+ 1.5k pull-up resistor for USB Device-only devices (mount R6 or not)
• VCAP_1 and VCAP_2 capacitors for internal 1.25V regulator or shunt resistors to short to GND for devices without internal LDO (replace C11/C14 by 0R)

TODO:

• I still have a problem in the board outline near the USB connector cutout: when entering the 3D view, I get an error message giving some XY coordinates, but I can’t find what is wrong, any help appreciated!
• add teardrops on vias for smoother junction with traces (remove some stress on the copper foil, prevents delamination)
• panelization

Wishlist:

• add a combined 6-axis accelerometer / gyroscope somewhere on the bottom PCB size on an SPI or I2C bus to get a fully working flight controller board!
• add an RGB LED?

Of course, any help / suggestion is welcome!

I’ve pushed it to my repo

https://github.com/rogerclarkmelbourne/ … ill_Boards

in a separate folder

https://github.com/rogerclarkmelbourne/ … r/Squonk42

I loaded the schematic and the PCB and did not get any errors except when using the 3D viewer (this may just be a problem with one of the 3D symbols)

I have not had time to look in detail at the PCB etc

[Squonk42 – Tue Nov 28, 2017 9:22 pm] –
TODO:
[*]add teardrops on vias for smoother junction with traces (remove some stress on the copper foil, prevents delamination)[/*] [*]panelization[/*] [/list]

Concerning the teardrops, are you sure that you need to do that? i’m not sure if it was posted here, but i once saw a nice video @ a chinese pcb factory, where they went through the entire pcb production process, and one of the topics was teardrops, and the message was: don’t add them yourself, it’s one of the things we do to your file before processing it (but ofcourse not sure if that includes the cheap ones we use).

And what do you want to do with panelization? if you want to make a nice panel connected via mousebites, i know i found a nice program to do this (on the gerbers, not on the KiCad files).

concerning your 3d view problems: probably some artifacts of the conversion from eaglecad? in the 3d view you also see this strange thing floating quite a distance from the board.
when i have some time i’ll have a look inside the pcb file itself, it’s a fairly readable format, maybe we can just find the offending items like that

[racemaniac – Wed Nov 29, 2017 7:09 am] – Concerning the teardrops, are you sure that you need to do that? i’m not sure if it was posted here, but i once saw a nice video @ a chinese pcb factory, where they went through the entire pcb production process, and one of the topics was teardrops, and the message was: don’t add them yourself, it’s one of the things we do to your file before processing it (but ofcourse not sure if that includes the cheap ones we use).

All the cheap PCB shops I have used don’t add them by themselves, this is why I consider this!

[racemaniac – Wed Nov 29, 2017 7:09 am] – And what do you want to do with panelization? if you want to make a nice panel connected via mousebites, i know i found a nice program to do this (on the gerbers, not on the KiCad files).

Please let me know the program, I am interested in it!

BluePillF4 Schematics.pdf

BluePillF4 Schematics

(254 KiB) Downloaded 28 times

[Squonk42 – Wed Nov 29, 2017 7:30 am] –

[racemaniac – Wed Nov 29, 2017 7:09 am] – Concerning the teardrops, are you sure that you need to do that? i’m not sure if it was posted here, but i once saw a nice video @ a chinese pcb factory, where they went through the entire pcb production process, and one of the topics was teardrops, and the message was: don’t add them yourself, it’s one of the things we do to your file before processing it (but ofcourse not sure if that includes the cheap ones we use).

All the cheap PCB shops I have used don’t add them by themselves, this is why I consider this!

[racemaniac – Wed Nov 29, 2017 7:09 am] – And what do you want to do with panelization? if you want to make a nice panel connected via mousebites, i know i found a nice program to do this (on the gerbers, not on the KiCad files).

Please let me know the program, I am interested in it!

the pcb panelizer:
http://blog.thisisnotrocketscience.nl/p … panelizer/

[Squonk42 – Wed Nov 29, 2017 1:47 pm] –
Do you remember where on the board you spotted this problem?

centrally underneath the stm32 i think the bottom plane had this very tiny strand of fill between the traces.
but it’s just a property of the fill zone, it’s currently configured to 1 mil.
setting it to a reasonable value probably won’t cause a DRC issue, but better to be safe than sorry .

Are those the test points the ones under the MCU?
If so, could you perhaps separate them a tinny bit more from each other (the ones that are the closest to each other) and perhaps align them?
If someone needs to use them and has to handsolder, having a bit more clearance between them will help, not everyone has a steady hand.

with the attached file, KiCad no longer complains about your edge (and correctly renders the cutout), and the floating island when you zoom way out is also removed .

something else i just noticed: are the holes for the pads for the usb ports correct? the holes seem a bit small.

I am just learning KiCAD

No, you are right, the holes for the USB connector are not correct, they are supposed to be oval, and I just found the way to do it in the footprint editor, so it is fixed now!

I integrated your changes and fixed these issues:

• Integrated changes from @racemaniac for fixing the edge layer issue
• Removed Ref/Value for U3 (STM32) on PCB top
• Fixed Top & Bottom GND zones minimum width to 6 mils
• Added some missing GND tracks between thermal pads due to previous change
• Fixed pads for J5 (micro USB) to be oval instead of round

I created a pull request for Roger: https://github.com/rogerclarkmelbourne/ … rds/pull/1

Keep searching for problems!

I’ve merged the PR

BTW.

@victor_pv has some credit with AllPCB and has offered to get some PCB’s made when the design is stable

We need to make a clean BOM that should allow sourcing through very different suppliers: Taobao, Aliexpress, eBay, Mouser or Digi-Key…

Right now, I ordered all the parts from Aliexpress and have some early PCBs done in EagleCAD on their way (this was before the AllPCB crazyness!) to validate the design.

Once it is done, we will have to investigate on how to manufacture the boards at the lowest possible cost. I may have a way to do this right from Mainland China, but if someone has some hints, it is welcome!

We should think about the easiest way to put the bootloader in it without any soldered header from a bare chip (pogo pins), as well as a sketch that will exercise all components and GPIOs like toggling one pin at a time and verifying by reading all of them that only the single expected externally loopbacked pin is changing.

btw, what do you think of KiCad? it’s great that you made the effort of doing it in KiCad, makes it a lot easier for others to view the files .

But I appreciate the fact that it is free (both as in beer and speech…), and I like the 3D view very much!

I chose to use Kicad to make the design easy to use for everybody, even if it required much more efforts on my side.

[Squonk42 – Thu Nov 30, 2017 10:23 am] –
There are good and bad things in Kicad: I would complain about the strange workflow for linking footprints to parts, and I cannot understand why the netlist is not automatically updated when you change the schematic…

But I appreciate the fact that it is free (both as in beer and speech…), and I like the 3D view very much!

I chose to use Kicad to make the design easy to use for everybody, even if it required much more efforts on my side.

the linking footprints to parts i kind of like (but it’s indeed different from EagleCad)
the automatically updating netlist (and even a bidirectional link between netlist & pcb) is one of the big improvements expected for KiCad 5.0 .

And your effort is greatly appreciated

Thanks for taking the extra time to create it in KiCad

I agree it is different from Eagle, but one good thing is that it does not have any layers or size limitation like the free and the basic version of Eagle have.

The linking of components to footprints seems to be getting stronger, as I have noticed some parts automatically link.

But for things like a resistor, I can understand why this is specified in the output for PCB, as really the footprint of an item is not related to its generic symbol in the schematic.

[RogerClark – Thu Nov 30, 2017 10:34 am] –
@Squonk42

Thanks for taking the extra time to create it in KiCad
The linking of components to footprints seems to be getting stronger, as I have noticed some parts automatically link.

Indeed, a library component can specify a footprint, and the linker will then automatically use that one (but you can then still change it if you want)

I used several ECAD systems, and in this regard, Kicad is really… odd! Up to now, I was using EagleCAD for hobby, but it is no longer a good option, and Kicad is the only serious alternative.

I kind of disagree with you Roger regarding the resistors: even in the schematic, You may have a default package for the whole design, but you may need to take care of the resistor power rating (and thus its actual package) way before you route the board, so there is no absolutely “generic” part IMHO.

I like very much the way parts are handled in Altium…

[Squonk42 – Tue Nov 28, 2017 9:22 pm] –
Wishlist:

• add a combined 6-axis accelerometer / gyroscope somewhere on the bottom PCB size on an SPI or I2C bus to get a fully working flight controller board!
• add an RGB LED?

Of course, any help / suggestion is welcome!

Concerning the accelerometer:
would indeed be a VERY nice to have XD. room for an mpu or adxl would be nice. btw, immediatly go 9 axis, it’s not as if those are any bigger than the 6 axis variants these days. And i2c is probably easier to fit than an spi one (less connections needed), and good enough as communication channel. You’ll need to connect 1 extra pin though for the interrupt (so you can poll when new data is ready iso continuously).
but that’s probably going to be *really* hard to fit XD.

the rgb led would also be nice, was a bit surprised when googling that they exist in 0603 or 0805 sizes O_O
might actually be feasible XD (but maybe total overkill too :p)

[racemaniac – Thu Nov 30, 2017 3:09 pm] –
Concerning the accelerometer:
would indeed be a VERY nice to have XD. room for an mpu or adxl would be nice. btw, immediatly go 9 axis, it’s not as if those are any bigger than the 6 axis variants these days. And i2c is probably easier to fit than an spi one (less connections needed), and good enough as communication channel. You’ll need to connect 1 extra pin though for the interrupt (so you can poll when new data is ready iso continuously).

but that’s probably going to be *really* hard to fit XD.

I had this idea because most flight controllers now use either an F3 or F4 (some use F7) STM32s and are in the $25 price range. However, most of them are 6-axis only (accelero + gyro, no compass), most of them is good old MPU6000.

As for I2C, I agree that it is simpler (SDA, SCL + IRQ), but you are then limited to 4K looptime / 4 K gyro sampling rate, whereas with SPI, you co go up to 8K/8K at the expense of 2 additional signals. I will check what is available on our BluePill board near the SWD connector (the only free area on top side is between the 2 buttons and not too crowded, just the SWDCLK/SWDIO signals right now) or maybe on the bottom side.

Yes, I agree that IRQ is a must-have!

[racemaniac – Thu Nov 30, 2017 3:09 pm] –
the rgb led would also be nice, was a bit surprised when googling that they exist in 0603 or 0805 sizes O_O
might actually be feasible XD (but maybe total overkill too :p)

As for the LED, the current one on PC13 is a 0603, so fitting an RGB one is just a matter of bringing 2 more signals (if possible PWM) and 2 more resistors, so not a big deal. Price is not very expensive either.

Both features may just be optional to reduce the cost, but could be populated by the user if required, or bought mounted at higher price.

[racemaniac – Fri Dec 01, 2017 6:53 pm] –
it’s probably a bit late for this XD
but for 32khz crystal i’d expected you’d go for one of these: https://www.aliexpress.com/item/10pcs-F … 31870.html
They are even smaller than the ones you chose, and the ones of the link i just gave, you can also properly see its specifications

The FC-12M are smaller, but they are also more expensive, and the one you linked has a shipping cost of $46.86 to France via EMS And what you see in the picture is not necessarily what you get, so having 12.5pF / 20 ppm on the bag pictured here doesn’t mean much.

The FC-135 is cheaper and still has a reasonable size. But of course, we can still change the design!

[Squonk42 – Fri Dec 01, 2017 9:08 pm] –

[racemaniac – Fri Dec 01, 2017 6:53 pm] –
it’s probably a bit late for this XD
but for 32khz crystal i’d expected you’d go for one of these: https://www.aliexpress.com/item/10pcs-F … 31870.html
They are even smaller than the ones you chose, and the ones of the link i just gave, you can also properly see its specifications

The FC-12M are smaller, but they are also more expensive, and the one you linked has a shipping cost of $46.86 to France via EMS And what you see in the picture is not necessarily what you get, so having 12.5pF / 20 ppm on the bag pictured here doesn’t mean much.

The FC-135 is cheaper and still has a reasonable size. But of course, we can still change the design!

strange, for me it’s a 1$ shipping cost on that one XD

[racemaniac – Fri Dec 01, 2017 7:07 pm] –
Ok, had a tiny bit of time to have a very quick look at the pcb

Found 1 error in the schema: on the AP2112k, you put the 3v3 as vin, not the 5V (so its vout will currently be a bit lowere than 3.3v)
Also when using the ap2112k configuration, we would connect its ground via a ferrite bead to the common ground.

And now i’m gone again (and have a thing to go to for the entire weekend, so no electronics time this weekend )

Good catch!

Ok, bringing the +5V in the AP2112 vicinity does not seem too difficult: just re-route the NRST signal around the PC5 pad on the bottom side and follow the VBUS_EN signal to the header pin. This would free the outer bottom overhang side to route the +5V between the PA1-PA2 pins instead of +3V3.

The ferrite bead between AGND and GND looks more tricky… I see a solution by moving the R4 resistor connected to BOOT0 between the 2 button switches (or if we get a smaller 32kHz crystal, this could free some space too…), shifting down the 2x 8MHz crystal capacitors to make room for the ferrite bead, what do you think?

However, I see no way to route the AGND to a header pin.

[racemaniac – Fri Dec 01, 2017 9:18 pm] –

[Squonk42 – Fri Dec 01, 2017 9:08 pm] –

[racemaniac – Fri Dec 01, 2017 6:53 pm] –
it’s probably a bit late for this XD
but for 32khz crystal i’d expected you’d go for one of these: https://www.aliexpress.com/item/10pcs-F … 31870.html
They are even smaller than the ones you chose, and the ones of the link i just gave, you can also properly see its specifications

The FC-12M are smaller, but they are also more expensive, and the one you linked has a shipping cost of $46.86 to France via EMS And what you see in the picture is not necessarily what you get, so having 12.5pF / 20 ppm on the bag pictured here doesn’t mean much.

The FC-135 is cheaper and still has a reasonable size. But of course, we can still change the design!

strange, for me it’s a 1$ shipping cost on that one XD

FC-12M.png (172.75 KiB) Viewed 202 times

[Squonk42 – Thu Nov 30, 2017 6:21 am] –

Once it is done, we will have to investigate on how to manufacture the boards at the lowest possible cost. I may have a way to do this right from Mainland China, but if someone has some hints, it is welcome!

email me at [email protected] and i can put you in touch with my contact who has a factory in north-east shenzhen. he can easily handle this board, assembly included. if it’s ok we’ll talk before-hand before cc’ing him in, to get the exact info needed so that it minimises the number of questions and avoids time-wasting for him.

background: mike majored in economics, speaks very good english, is extremely conscientious and took over his father’s factory about 3 years ago. he is *ridiculously* busy and goes out of his way to help me. i consider myself extremely lucky to know him, and if i get even the *slightest* hint that he’s been messed about i’ll put my foot down hard as i won’t have *my* reputation with him affected. hence why it’s best to get “all ducks in row” in advance, know exactly how many samples, have the BOM in TSV file-format, digikey P/Ns all listed on everythig, gerbers pre-vetted (no panelisation, his sources handle that) etc. etc.

bottom line: he’ll give you an extremely competitive and FAIR quote, won’t f*** you over because you happen to be a foreigner and therefore automatically qualify for “massive price-hikes” and he’ll do everything he can to make sure you get a decent service.

[lkcl – Fri Dec 01, 2017 9:50 pm] –

[Squonk42 – Thu Nov 30, 2017 6:21 am] –

Once it is done, we will have to investigate on how to manufacture the boards at the lowest possible cost. I may have a way to do this right from Mainland China, but if someone has some hints, it is welcome!

email me at [email protected] and i can put you in touch with my contact who has a factory in north-east shenzhen. he can easily handle this board, assembly included. if it’s ok we’ll talk before-hand before cc’ing him in, to get the exact info needed so that it minimises the number of questions and avoids time-wasting for him.

background: mike majored in economics, speaks very good english, is extremely conscientious and took over his father’s factory about 3 years ago. he is *ridiculously* busy and goes out of his way to help me. i consider myself extremely lucky to know him, and if i get even the *slightest* hint that he’s been messed about i’ll put my foot down hard as i won’t have *my* reputation with him affected. hence why it’s best to get “all ducks in row” in advance, know exactly how many samples, have the BOM in TSV file-format, digikey P/Ns all listed on everythig, gerbers pre-vetted (no panelisation, his sources handle that) etc. etc.

bottom line: he’ll give you an extremely competitive and FAIR quote, won’t f*** you over because you happen to be a foreigner and therefore automatically qualify for “massive price-hikes” and he’ll do everything he can to make sure you get a decent service.

Thank you very much Luke for this proposal, it seems like a very interesting solution!

I think we need to make the prototype work 100% first thing, then establish a clean BOM before going to ask the factory.

[Squonk42 – Fri Dec 01, 2017 9:20 pm] –

[racemaniac – Fri Dec 01, 2017 7:07 pm] –
Ok, had a tiny bit of time to have a very quick look at the pcb

Found 1 error in the schema: on the AP2112k, you put the 3v3 as vin, not the 5V (so its vout will currently be a bit lowere than 3.3v)
Also when using the ap2112k configuration, we would connect its ground via a ferrite bead to the common ground.

And now i’m gone again (and have a thing to go to for the entire weekend, so no electronics time this weekend )

Good catch!

Ok, bringing the +5V in the AP2112 vicinity does not seem too difficult: just re-route the NRST signal around the PC5 pad on the bottom side and follow the VBUS_EN signal to the header pin. This would free the outer bottom overhang side to route the +5V between the PA1-PA2 pins instead of +3V3.

The ferrite bead between AGND and GND looks more tricky… I see a solution by moving the R4 resistor connected to BOOT0 between the 2 button switches (or if we get a smaller 32kHz crystal, this could free some space too…), shifting down the 2x 8MHz crystal capacitors to make room for the ferrite bead, what do you think?

However, I see no way to route the AGND to a header pin.

don’t think it’s really needed to put the AGND on the header (or A3V3). In the end we decided that people just want to get the 3v3 from the header, not be able to supply it. as we already give a good voltage regulator that will make 3v3 out of anything slightly above 3v3
and anyhow, AGND and GND are still connected, so it won’t matter that much i think

But I noticed in @racemaniacs list of parts from Aliexpress, a STM32F103RB

I presume this was to save costs during testing

However this board factor would also fit the F103RCT and even the RET RGT

These are better devices as they have DAC and I think they have SDIO

The only problem is that I can’t find any RCT versions on Aliexpress, but Taobao has loads.

I have been stung in the past buying from Taobao as you need to use a third party agent to reship the package etc, and they charged a massive additional shipping change on some boards,

But in this case it looks lower risk, so may be worth considering

[RogerClark – Sat Dec 02, 2017 8:10 pm] –
I have been stung in the past buying from Taobao as you need to use a third party agent to reship the package etc, and they charged a massive additional shipping change on some boards,

But in this case it looks lower risk, so may be worth considering

I used a while back a forwarding agent, and is much cheaper. You buy on your own, and ship t them (google translate, learn Chinese, find a friend who speaks Chinese…). So you pay no commission on the purchases or the local shipping. Then once all your purchases arrive to the shipping agent, you pay them to ship it to you.
I did a test order fairly small, but even for such small order (perhaps $50 total), it came to be cheaper than buying thru an agent, even that same agent.
You need to make sure you are buying what you want, which can be tricky. So I think is a good option for buying in larger quantities from a company you already trust in Taobao but does not ship to the USA.

Now, for ordering 3 or 4 MCUs for a prototype, is probably not worth the hassle. For ordering 50 for a small run, may be worth it.
But to produce 50 boards, we may be starting to get at the volume that could be assembled for a good price by a company.

About features, 103RCT has 3 SPI, 2 DACs and SDIO. We have a beta version of the SDIO working. I haven’t fully tested cause I didn’t have a board with the connector in it (using dupont wires with 4 bits high speed was nasty). I have such a board now, and when I get a chance will work a bit further on the SDIO. 1 bit mode was working fine.

[RogerClark – Sat Dec 02, 2017 8:10 pm] –
Just a thought.

But I noticed in @racemaniacs list of parts from Aliexpress, a STM32F103RB

I presume this was to save costs during testing

However this board factor would also fit the F103RCT and even the RET RGT

These are better devices as they have DAC and I think they have SDIO

The only problem is that I can’t find any RCT versions on Aliexpress, but Taobao has loads.

I have been stung in the past buying from Taobao as you need to use a third party agent to reship the package etc, and they charged a massive additional shipping change on some boards,

But in this case it looks lower risk, so may be worth considering

If you refer to my Aliexpress list of parts, I chose the STM32F103RB as the cheapest one to replace the LQFP48 STM32F103C8T6 or STM32F103CBT6.

Having an LQFP64 package opens the door to a lot more chips, from F0 or L4 to F7.

regarding the pcb (noticed it before, but forgot to mention it)
make sure to adjust your solder mask clearance. By default KiCad now puts it to 6 mil, which is risky on small boards like this ^^’
In pcbnew, go to the Dimensions menu->pads mask clearance. And i usually just put it to 0
Maybe 1 or 2 mil is better, but haven’t had issues with it (and if you put it to 0, the manufacturer can easily change it themselves before processing the board)

tiny remark regarding the pcb: the thicker trace for vbat is probably a waste of space ^^. vbat would see very little current (it’s for the low power stand by things), so giving it a wider trace is a bit overkill XD

and as mentioned before, maybe just don’t bother putting the a3v3/agnd on the pin header. it’ll also save you some space, and if you want to route PA9 to vbus, the extra space may be welcome ^^

And small thing i noticed (but not sure if it’s good or not XD): your big value capacitors on the sd card / voltage regulator out. I think it’s a wise choice, and wonder what motivated you to choose those values . On my lightsaber boards i notice how much noise the SD card can cause, so giving it a bigger capacitor may be a wise choice (same for the voltage regulator, put a bigger value there and focus on the bigger spikes). Currently i’m trending to a big & a small one, but on my boards i have a bit more room XD.

[racemaniac – Mon Dec 04, 2017 5:33 pm] –
had a bit more time, this time went over your schematic once more, noticed one more missing feature:
PA9 is VBUS sense (seeing if VBUS is powered or not), so the plan was connecting it to VBUS (via a voltage divider so we lower the voltage to ~3v3 -> not entirely sure that’s needed, maybe the pin is 5V tolerant?).
but it’s ofcourse another trace towards the usb pluf you have to get on there ^^’

It is not a bug, it is a feature

Well, actually, this pin is headache: PA9 is the ROM bootloader TX pin, also UART1_TX, but can be a GPIO too…

If we permanently connect PA9 to VBUS, we break the compatibility with the BluePill: imagine one existing setup where PA9 is not connected to 5V, you get a short… Of course, we could put yet another series resistor to avoid such case, but a better idea would be to break out VBUS to a header in place of a 5V pin and connect PA9 to it externally.

[racemaniac – Mon Dec 04, 2017 6:11 pm] –
Ok, done doing a basic review of it all now, my remarks:

Thank you for spending your time on it!

[racemaniac – Mon Dec 04, 2017 6:11 pm] –
regarding the pcb (noticed it before, but forgot to mention it)
make sure to adjust your solder mask clearance. By default KiCad now puts it to 6 mil, which is risky on small boards like this ^^’
In pcbnew, go to the Dimensions menu->pads mask clearance. And i usually just put it to 0
Maybe 1 or 2 mil is better, but haven’t had issues with it (and if you put it to 0, the manufacturer can easily change it themselves before processing the board)

Oh, thank you! I was actually looking for this setting. I was once bitten hard by this problem, the PCB manufacturer doubling my own solder mask clearance, leading to an unsolderable PCB… I will set it to zero and let the factory do it.

[racemaniac – Mon Dec 04, 2017 6:11 pm] –
tiny remark regarding the pcb: the thicker trace for vbat is probably a waste of space ^^. vbat would see very little current (it’s for the low power stand by things), so giving it a wider trace is a bit overkill XD

Yeah, I just used the same trace width for all power rails, but here it is clearly oversize

[racemaniac – Mon Dec 04, 2017 6:11 pm] –
And small thing i noticed (but not sure if it’s good or not XD): your big value capacitors on the sd card / voltage regulator out. I think it’s a wise choice, and wonder what motivated you to choose those values . On my lightsaber boards i notice how much noise the SD card can cause, so giving it a bigger capacitor may be a wise choice (same for the voltage regulator, put a bigger value there and focus on the bigger spikes). Currently i’m trending to a big & a small one, but on my boards i have a bit more room XD.

Experience Toggling 4 bits synchronously, plus command and clock is just terrible for the power rail, unless you put a large enough power reservoir close to it. Adding a 100nF in parallel would be nice, but I am quite limited by real estate here…

Do you think I should put larger capacitor values there?

[Squonk42 – Tue Dec 05, 2017 1:07 pm] –

[racemaniac – Mon Dec 04, 2017 6:11 pm] –
And small thing i noticed (but not sure if it’s good or not XD): your big value capacitors on the sd card / voltage regulator out. I think it’s a wise choice, and wonder what motivated you to choose those values . On my lightsaber boards i notice how much noise the SD card can cause, so giving it a bigger capacitor may be a wise choice (same for the voltage regulator, put a bigger value there and focus on the bigger spikes). Currently i’m trending to a big & a small one, but on my boards i have a bit more room XD.

Experience Toggling 4 bits synchronously, plus command and clock is just terrible for the power rail, unless you put a large enough power reservoir close to it. Adding a 100nF in parallel would be nice, but I am quite limited by real estate here…

Do you think I should put larger capacitor values there?

don’t have enough experience yet to advise either way XD.
we’re indeed short on space, so lets give it a try like this, we’ll see where it gets

and indeed, it has 4 communication channels etc… but even on a macro scale it’s noticable.
on my current saber boards, i didn’t properly put capacitors on the entire DAC section, and now i’ve got noise from the SD card based on how often i access it. if for example i’m doing 200 block reads per second there’ll be a clear 200hz tone out of the speaker ^^ (luckily at a pretty low volume). (new version is underway from china that i hope fixes this issue XD)
i hope the capacitors you chose will do enough to prevent both high & low frequency noise from the sd card .

regarding the vbus feature: doesn’t sound too bad as an idea indeed . ideally we would know if the voltage divider is needed or not, and if it is, offer a vbus pad that has the divider on it already, if not, the 5v pin is indeed acceptable.

BTW, VBUS is connected to our 5V (actually down to ~+3.5V) power supply input through the MOSFET mounted as a diode, so I wonder how come the VBUS would disappear without the STM32 being shut down at the same time.

[Squonk42 – Tue Dec 05, 2017 2:00 pm] –
According to the STM32F405xx, STM32F407xx datasheet, PA9 is 5V tolerant, so no voltage divider required (“FT” I/O structure)!

BTW, VBUS is connected to our 5V (actually down to ~+3.5V) power supply input through the MOSFET mounted as a diode, so I wonder how come the VBUS would disappear without the STM32 being shut down at the same time.

isn’t the mosfet as a diode meant for powering the board via usb?
it’s a diode from vbus -> 5V, not the other way around (if it is, we have to fix that ^^)
the goal is that if we power it via usb, that the entire board is powered, but if you power the board via the 5V supply, then the vbus only gets powered if the SY6280 is enabled (as it’s current limiting, so we don’t risk damaging the board with whatever is connected to the usb port).

DMP2160UW.png (11.81 KiB) Viewed 347 times

Here is a short TODO list:

• Add teardrops => Check https://github.com/svofski/kicad-teardrops
• Panelization => Check pcb-panelizer ( http://blog.thisisnotrocketscience.nl/p … panelizer/)
• Fix fill area minimum width => Fixed Top & Bottom GND zones minimum width to 6 mils
• Added some missing GND tracks between thermal pads due to previous change
• Problem with PCB edges in 3D view => Fixed by @racemaniac
• USB connector holes are too small => Fixed pads for J5 (micro USB) to be oval instead of round
• Remove Ref/Value for U3 (STM32) on PCB top => OK
• Option: Add an IMU somewhere on the bottom PCB size on an SPI or I2C bus to get a fully working flight controller board! i am thinking of an Invensense MPU6000 hooked to an SPI bus in order to get 8ksps performance
• Option: Add an RGB LED => 0603?
• Power AP2112 from +5V, not from +3.3V
• Add ferrite bead between GND and AGND
• Replace 32kHz crystal by smaller FC-12M, may be required for previous item
• Option: Add MCP73831 LiPo battery charger (would require an ideal diode like D3/FET2/R6 in the Olimexino ATMega32U4 schematics)
• Add pad/pin for VBUS for external PA9 VBUS_SENSE feature (USB Host) => Added a series resistor between VBUS and PA9 to avoid short-circuits
• Adjust solder mask clearance to 0
• Make VBAT trace thinner
• Provide footprint for parallel capacitor near SDCard and voltage regulators
• Fix MOSFET direction => replace by an SS12 Schottky diode
• Added PWR_FLAG to schematic to remove ERC warnings
• Replaced NC by real Kicad ones to remove ERC warnings
• Cleaned up Expansion connector labels in schematic
• Cleaned up traces for PA13-14 and PC13-15
• Changed micro USB connector to BSC-Elec U02-BFD3111B0-009
• Option: add an SPI Flash chip as an alternative to SDCard connector (overlapping footprints)
• Add optional shunt resistors to route a single bit SPI bus to the SDCard connector for devices without SDIO interface => NOT POSSIBLE, too tight!

All volunteers welcome!

[Squonk42 – Wed Dec 06, 2017 7:58 am] –
Please look at the Arduino Due schematic and TI AN above.

I can see the schematic, but i want to understand why it is so XD
Otherwise i’ll keep making the same mistake >_<

What is the purpose of the FET Q1

Which direction is it supposed to prevent. e.g. USB -> 5V pin , or 5V pin to USB

It definitely won’t stop 5V pin -> USB because of the internal diode as show in the symbol.

[Squonk42 – Wed Dec 06, 2017 9:02 am] –
Exactly, the idea is to allow USB to power the +5V, but not the opposite direction (we want to control VUSB using the SY6280 USB load switch), so the MOSFET body diode should be USB => +5V, like in the Arduino Due schematic and TI’s AN.

but since we’re also pulling the gate low, won’t it also conduct the other way around anyway?
Is it then maybe this that we want to create:
https://electronics.stackexchange.com/q … ransistors
but that’s then with 3 transistors >_<

I presume we are not simply using a diode on the 5V input, because you don’t want the 0.5V drop across the diode ?

AFIK the Maple mini just uses a diode for this.

What else uses the 5V input ? that really requires 5V, and not 3.3V from the regulator.

Even if the diode dropped 0.5V that would still be 4.5V on the input to the regulator, and I thought that would be enough voltage for some regulators to output 3.3V ??

In the Arduino Due schematic, there is one that is polarized by a comparator circuit. How the MOSFET bottom circuit works is still a mystery.

Max current is 1A with the AP2114, and this may be used by external components in addition to the STM32F405 current consumption. But if we use a Schottky diode, the drop is only 0.3V, not 0.6V, so the max power dissipation is the diode is 0.6W. A 4mm x 2mm (vs. 3 mm x 2.5 mm for the MOSFET) diode such as an PMEG3010ER or MBRM130LT1G could handle that…

EDIT: well, maybe not: Taj is 220°C/W, so for 0.6W, this is a 132°C temperature rise… with a max Tj of 150°C, you blow the diode @1A above 18°C! It can only stand up to 0.5A @ 40°C.

Just read thru TI note, so it’s for reverse current protection, not short circuit. I wonder why it needs that on the USC2 power source, is not like you can reverse a USB cable… But on the other hand, it also blocks current flowing from the load to the USB port, so that port can be used to power the board, but the board will not power something connected to that port.
Makes sense in the DUE since that’s not the native port. In our case since we can use the USB port as host and connect a slave, we don’t want that circuit or would prevent us from powering a slave.
Am I right?

[victor_pv – Wed Dec 06, 2017 2:42 pm] –
Perhaps the bottom FET is just short circuit protection?
If the drain voltage was equal to the gate (so drain shorted to gate, which is ground), the FET would stay closed, and the internal diode is reversed, so there is no current flowing to the short.

Just read thru TI note, so it’s for reverse current protection, not short circuit. I wonder why it needs that on the USC2 power source, is not like you can reverse a USB cable… But on the other hand, it also blocks current flowing from the load to the USB port, so that port can be used to power the board, but the board will not power something connected to that port.
Makes sense in the DUE since that’s not the native port. In our case since we can use the USB port as host and connect a slave, we don’t want that circuit or would prevent us from powering a slave.
Am I right?

For a MOSFET to pass/block, what matters is the Vgs compared to its threshold value (negative for a P-type).

But you are probably right for the Due. In our case, we cannot use this solution, and I cannot find a single-component solution to implement this protection, except for a Schottky diode that will heat the birds!

[Squonk42 – Wed Dec 06, 2017 3:06 pm] –

[victor_pv – Wed Dec 06, 2017 2:42 pm] –
Perhaps the bottom FET is just short circuit protection?
If the drain voltage was equal to the gate (so drain shorted to gate, which is ground), the FET would stay closed, and the internal diode is reversed, so there is no current flowing to the short.

Just read thru TI note, so it’s for reverse current protection, not short circuit. I wonder why it needs that on the USC2 power source, is not like you can reverse a USB cable… But on the other hand, it also blocks current flowing from the load to the USB port, so that port can be used to power the board, but the board will not power something connected to that port.
Makes sense in the DUE since that’s not the native port. In our case since we can use the USB port as host and connect a slave, we don’t want that circuit or would prevent us from powering a slave.
Am I right?

For a MOSFET to pass/block, what matters is the Vgs compared to its threshold value (negative for a P-type).

But you are probably right for the Due. In our case, we cannot use this solution, and I cannot find a single-component solution to implement this protection, except for a Schottky diode that will heat the birds!

Maybe a diode like this: https://www.vishay.com/docs/88746/ss12.pdf
(also easily & cheaply found on aliexpress)
or a bit bigger & certainly capable of 1A: https://www.vishay.com/docs/88712/s2a.pdf

I’m trying to understand, so correct me if I’m wrong, but we want to achieve this:
-Power the board from USB.
-Power a slave device from the board usb
-Prevent current flowing back to the USB port if the USB has some voltage, but the board +5 voltage is higher.

Something like this, but single component:
http://www.linear.com/product/LTC4160

Actually reading thru that, is achieves multiple functions. Current limiter, battery charger, and switching regulator. Perhaps is worth it since it would replace multiple components.

[racemaniac – Wed Dec 06, 2017 3:11 pm] –
Maybe a diode like this: https://www.vishay.com/docs/88746/ss12.pdf
(also easily & cheaply found on aliexpress)
or a bit bigger & certainly capable of 1A: https://www.vishay.com/docs/88712/s2a.pdf

The first one has a Vf of 0.5V and is already 4 mm x 2.54 mm but may be acceptable with Tja of 88°C/W (44°C rise), the second has Vf of 1.15V and is even larger, so no way.

The MAX40200 ideal diode would match perfectly, but it is not cheap and cannot be found on Aliexpress:

MAX40200.png (10.37 KiB) Viewed 134 times

Can do power management + battery charging, and works with USB OTG, but cheapest cost seems around $1, and still needs a few external components.

[victor_pv – Wed Dec 06, 2017 3:12 pm] –
Something like this, but single component:
http://www.linear.com/product/LTC4160

Actually reading thru that, is achieves multiple functions. Current limiter, battery charger, and switching regulator. Perhaps is worth it since it would replace multiple components.

This component is $0.30 on Taobao, plus power inductor, MOSFET and other components: probably too expensive and too large. All PMIC will have the same problems.

I am trying to understand how FET2 works in this schematic:
https://www.olimex.com/Products/Duino/A … rev_A3.pdf

[Squonk42 – Wed Dec 06, 2017 3:29 pm] –

[racemaniac – Wed Dec 06, 2017 3:11 pm] –
Maybe a diode like this: https://www.vishay.com/docs/88746/ss12.pdf
(also easily & cheaply found on aliexpress)
or a bit bigger & certainly capable of 1A: https://www.vishay.com/docs/88712/s2a.pdf

The first one has a Vf of 0.5V and is already 4 mm x 2.54 mm but may be acceptable with Tja of 88°C/W (44°C rise), the second has Vf of 1.15V and is even larger, so no way.

The MAX40200 ideal diode would match perfectly, but it is not cheap and cannot be found on Aliexpress:
MAX40200.png

Indeed, the bigger ones are too much, but those SS12 diodes may be an option? and they’re indeed big, but if we can get some traces between its pads, it might work out? And it’s also a cheap & easy to find diode, so ideal for the kind of board we’re making.

[Squonk42 – Wed Dec 06, 2017 3:45 pm] –
I am trying to understand how FET2 works in this schematic:
https://www.olimex.com/Products/Duino/A … rev_A3.pdf

Seems like this circuit, this has the explanation on how it works. Called Q1 here:
https://behindthesciences.com/electroni … y-circuit/

The FET is basically just acting like a diode ( if it’s connected correctly ), and will handle the expected current.

But the issue is that sometimes the battery is allowed to feed the USB for OTG operation.

So can we connect the gate to a GPIO, and require software control for then using the battery connection ?
Possibly not, as for some time during startup the GPIO may not be the correct value?

Or alternatively, just directly connect VBAT , and users need to use their brains and not connect USB and battery at the same time. perhaps make the track very thin, to act like a fuse, so if the user does this, it burn the track but not the board..

Or use a jump link.

Looking on AliExpress there seems to be multiple vendors

Its 1A 20V

Edit.

I am changing my copy of the schematic now.

I’ve had to include the diodes library, but I guess now its in the schematic, I need to move the symbol into the board’s custom lib.

I don’t normally bother on components like diodes etc which are common, and only use custom libs for parts not available in KiCads default libs, but I can to manually add it to the boards on library, if we are happy with that diode

Edit.

Its a bit of a pain to do, but I’ve added a 1N5817 to the BluePill lib (in my local copy)

The diode prevents the +5V pin feeding the USB VBus

SS12 diodes are extremely common, even on Aliexpress:
https://www.aliexpress.com/item/sku/32830718059.html

However I don’t know what package the SS12 uses

SS12 are extremely standard SMD power diodes, they use an “SMA” (also called “DO-214AC”) package, plenty of them on Digi-Key:
https://www.digikey.com/products/en/dis … 280?k=ss12

AFAICT, it corresponds to the “D_SMA” footprint in the “Diodes_SMD” footprint library in Kicad. But in general I prefer to use my old trusted footprints rather than using an existing one that I have not checked against the real thing. One thing that makes me suspect problems is the “D_SMA_Handsoldering” variant…

I’ll change the name of the library symbol from 1N5812 to SS12 (its the same visual symbol) , and use the D_SMA footprint

[Squonk42 – Thu Dec 07, 2017 9:35 pm] –
AFAICT, it corresponds to the “D_SMA” footprint in the “Diodes_SMD” footprint library in Kicad. But in general I prefer to use my old trusted footprints rather than using an existing one that I have not checked against the real thing. One thing that makes me suspect problems is the “D_SMA_Handsoldering” variant…

KiCad has a lot of handsoldering variants for smd components. I assume it’s just some bigger pads so you can more easily solder them with your soldering iron. I always use the regular pads as i use solder paste & stencil (and since space is tight XD)

I presumed the same thing about “hand soldering” versions, but never took the time to look

I do recall selecting them sometimes when I know the board is actually going to be hand soldered, i.e I did some boards for a small company and they didnt have their SMD reflow setup to start with, so as there was plenty of room on the PCB they wanted everything to be big SMD e.g. 1206 sizes for R and C and LEDs, so that they could be hand soldered.

[RogerClark – Thu Dec 07, 2017 9:53 pm] –
@racemanic

I presumed the same thing about “hand soldering” versions, but never took the time to look

I do recall selecting them sometimes when I know the board is actually going to be hand soldered, i.e I did some boards for a small company and they didnt have their SMD reflow setup to start with, so as there was plenty of room on the PCB they wanted everything to be big SMD e.g. 1206 sizes for R and C and LEDs, so that they could be hand soldered.

just did a quick check with the SMA diode footprint: it’s indeed pads that extend beyond the diode so it can easily be soldered with an iron.

Of course, these PCBs have the +3.3V voltage problem on the Analog LDO input, and the MOSFET problem too

If the intention is to make them easy to hand solder, I think using the hand solder version of the footprint would be a good idea, but if we are just making a few of them for prototyping until we are happy, and we all feel confortable with hand solder/skillet/reflow, then better use the real version of the pads that would would send to a factory, so no last minute mistakes because we replace a hand solder version for a normal solder version later on.

One more thing, why is the SY6280 in to +5V and out to VBUS? in that configuration, the board can power the USB, but the USB can’t power the board. Did I miss something? Ok I see the SY6280 is not provided to power the board, but to power the USB port,controlled by PC9.

The consensus was just to use a Schottky diode, so I was updating my copy of the files, but so far I’ve only had time to update the schematic, and I need to rename the schematic symbol to a SS12 as I didnt see a SS12 in the kicad diodes lib (but I will double check)
I’ve not looked at the PCB yet, but it should be OK as it replaces the 3 pads on the fet, with 2 pads

I had to move one resistor a bit, and move a few tracks.

Hopefully what I’ve done is OK, but if not we can revert to the previous version.

BTW There is now more space near the diode, so we may be able to move other things to this space

I didnt change anything else, though I noticed some of the tracks could be cleaned up a bit, as they seemed to have unnecessary small kinks in them.

Please download it and let me know if I’ve stuffed up or not
PS. DRC seems OK (no errors) and I looked in the 3D viewer and there seemed to be enough space between the diode and the regulator

[victor_pv – Fri Dec 08, 2017 2:01 am] –
I just found the perfect component for the job, MAX40200, but is not worth it, can’t find it in aliexpress, and in mourser costs $0.5.

I mentioned it in a previous post, but it is too exotic and expensive.

And we don’t have the room to fit the additional dual transistor and 2 more resistors to have a current mirror like the RPi, so either we put an Ss12 Schottky diode or we put nothing like the origial Bluepill.

I will check Roger’s additions.

Regarding the track clean up, this may be intentional in order to accomodate for the teardrops (smooth junction between track and pad to remove stress caused by etchint sharp corners), I had to turn some segments to pass DRC. But of course, it may happen that I forgot to optimize some tracks too!

For the teardrops, you have to duplicate the PCB just before generating the gerber files and run an automatic script that will add them with no way back, then panelize the result, hopefully with the tool found by @racemaniac to get the result above (this was in EagleCAD).

I moved R1 a bit, but in hindsight, I can now move it back to the left a bit.

I initially tried to have D3 closer to the regulator and needed to move R1 but looking in the 3D view they looked unnecessarily close

So I moved the track from PA11 to USB DM, to allow D3 to move even further away from the regulator if necessary.

I also moved the tracks and vias on PB12 and PB13 to make more room for D3

PA11 and P12 tracks can be moved down even more as could PB12 and PB13 if we needed space next to D3 for anything else

Arggghh.

I just noticed a stub of the 3.3V track, sticking out. I’ll remove it …

diode.jpg (198.16 KiB) Viewed 151 times

OK.

I’ll need to check why that track is there. I didnt add it and I can’t see what it would have been connecting to

Edit

I checked and I’ve somehow lost 5V pad which was at the end of that track.

I’ll reinstate the track and that pad

BTW.

I can’t see why VCAP1 and PB2 tracks are routing around something, which I can’t see

VCAP1_PB2.png (47.93 KiB) Viewed 141 times

I’ve removed U1 not Q1

Apologies

I’ll try to fix it now

[RogerClark – Fri Dec 08, 2017 10:08 am] –
I screwed up big time

I’ve removed U1 not Q1

Apologies

I’ll try to fix it now

lol, that happens
it’s great to see us working together towards this . i was hoping someone else would pick up the pcb development, so this weekend i can focus on writing software for my saber boards
i’ve got multiple simultaneous files streaming from an sd card working pretty well (still some last bugs/details to finish, and somewhere in the future do yet another rewrite as i’m now finally coming close to an API i like, and a feature set that makes sense for what i’m trying to do ).
got my board playing 4 48khz stereo wavs from the sd card, and mixing them together .

I should have some time this WE to browse through the TODO list.

I’ve reverted back to before I started

I’m going to need to move a lot of components

I think I’ll need to move the group of components (R’s and C’s etc) next to pins for B11,B10,B1 to the right

move_components.png (49.25 KiB) Viewed 235 times

Or do we need a 1A diode. Will a 500mA one do ?

If I push U4 and a load of the components next to it, to the right, there isnt really enough room, and one of the resistors has to be moved completely out the way, and at the moment I can’t see a good place for it.

And its getting too late for me to do any more today.

So I suspect you guys will have it done before I wake up tomorrow

add_SS12_diode.png (107.92 KiB) Viewed 233 times

[RogerClark – Fri Dec 08, 2017 11:17 am] –
Can we get the same spec diode in a smaller package, as is a real squeeze getting the it to fit

Or do we need a 1A diode. Will a 500mA one do ?

This is questionable! We chose the main LDO to be able to deliver 1A, as the STM32F405 already sinks 450 mA max itself; we added some room to power external components as well (SDIO…).

However, the USB 2.0 spec only allows delivering 500 mA, and this is even conditioned by a proper negotiation beforehand, otherwise, it is limited to 100 mA. Despite this limitation, there are a lot of wall adapters with an USB A socket that can deliver more than that, and it is easy to find a USB A to micro USB B cable to power the board over the micro USB B socket.

There are some smaller 1A Schottky diodes, but they are not as common and rather expensive: https://toshiba.semicon-storage.com/inf … e=CUS10S30

So, do we limit the power supply from the USB to 500 mA? If yes, this one may be interesting:
http://www.onsemi.com/pub/Collateral/MBR0520LT1-D.PDF
https://www.aliexpress.com/item/sku/1985290956.html

[Squonk42 – Fri Dec 08, 2017 12:55 pm] –

[RogerClark – Fri Dec 08, 2017 11:17 am] –
Can we get the same spec diode in a smaller package, as is a real squeeze getting the it to fit

Or do we need a 1A diode. Will a 500mA one do ?

This is questionable! We chose the main LDO to be able to deliver 1A, as the STM32F405 already sinks 450 mA max itself; we added some room to power external components as well (SDIO…).

However, the USB 2.0 spec only allows delivering 500 mA, and this is even conditioned by a proper negotiation beforehand, otherwise, it is limited to 100 mA. Despite this limitation, there are a lot of wall adapters with an USB A socket that can deliver more than that, and it is easy to find a USB A to micro USB B cable to power the board over the micro USB B socket.

There are some smaller 1A Schottky diodes, but they are not as common and rather expensive: https://toshiba.semicon-storage.com/inf … e=CUS10S30

So, do we limit the power supply from the USB to 500 mA? If yes, this one may be interesting:
http://www.onsemi.com/pub/Collateral/MBR0520LT1-D.PDF
https://www.aliexpress.com/item/sku/1985290956.html

how about this one:
https://www.aliexpress.com/item/100PCS- … eLevelAB=0
http://www.mouser.com/ds/2/258/B5817W-B … 276623.pdf

Same package as the 0.5A you’re mentioning, but also 1A (and bit lower votlage drop)

[racemaniac – Fri Dec 08, 2017 1:35 pm] – how about this one:
https://www.aliexpress.com/item/100PCS- … eLevelAB=0
http://www.mouser.com/ds/2/258/B5817W-B … 276623.pdf

Same package as the 0.5A you’re mentioning, but also 1A (and bit lower votlage drop)

There is something I don’t understand in the datasheet: max dissipation is 250mW, however Vf is max 0.45V x 1A = 450mW to dissipate.. Tj 25°C !?!

[Squonk42 – Fri Dec 08, 2017 1:48 pm] –

[racemaniac – Fri Dec 08, 2017 1:35 pm] – how about this one:
https://www.aliexpress.com/item/100PCS- … eLevelAB=0
http://www.mouser.com/ds/2/258/B5817W-B … 276623.pdf

Same package as the 0.5A you’re mentioning, but also 1A (and bit lower votlage drop)

There is something I don’t understand in the datasheet: max dissipation is 250mW, however Vf is max 0.45V x 1A = 450mW to dissipate.. Tj 25°C !?!

hmm, indeed pretty strange >_<
also don’t get it O_o

I am not sure why this diode is so much bigger than the FET it replaced.

I know that the FET was in the circuit the wrong way around, but is there no way to get a FET to behave like this diode ?
( to achieve the same functionality in a smaller package)

[RogerClark – Fri Dec 08, 2017 8:04 pm] –
I think it can be made to fit, but virtually all the other components between the USB connector and the MCU probably need to be moved, and a load of tracks rerouted.

I am not sure why this diode is so much bigger than the FET it replaced.

I know that the FET was in the circuit the wrong way around, but is there no way to get a FET to behave like this diode ?
( to achieve the same functionality in a smaller package)

because the diode has a voltage drop that is WAY higher than the fet . it has to dissipate way more heat, so it’s bigger…

We must respect the component courtyards: for example it is forbidden to put components in the corner of the STM32 as some pick&place machine may grab the chip by the corners or use a suction cup on the top. And the U1 (LDO) needs the largest possible copper area below it in order to dissipate the heat. It will be thus difficult to move much of the components around.

The diode is bigger because it needs to dissipate more heat: when there is current (up to 1A) flowing in the non-blocking direction, a Schottky (metal-silicon junction) diode has a forward voltage (Vf) ranging from 0.2-0.3 to 0.5V (vs. 0.6V for an NP silicon diode), resulting in a power of 1A x 0.6V = 0.6W to dissipate in heat. Then, the thermal resistance of the package (in °C/W, the smallest package, the highest resistance value) then gives you what will be the increase in temperature for this power, that you need to add to the ambient temperature to get junction temperature, which must never exceed a maximum value (generally 150°C).

Unlike the diode, a MOSFET when unblocked will feature a drain/source resistance (Rdson) of a few tens of milliohms (75 to 160 mhoms for the DMP2160UW-7), resulting in a power of 0.160 mohms x 1A x 1A = 0.16W, almost 4x less, so the package can be much smaller for a FET.

The MOSFET was not only the wrong way around to let current flow from Vusb to +5V, but it was actually always on, whatever the current direction. Mounting a MOSFET with its gate connected to ground is only useful to prevent a reverse battery connection to a circuit only sinking current, NOT to replace a diode between 2 voltage supplies like we did.

For the MOSFET to be used as an “ideal diode” (because of its low voltage drop of 0.16 mohms x 1A = 0.16V), the gate must be controlled by a circuit that will depend on the relative polarity on both sides of the diode. It can be achieved using an op amp like in the Arduino Due (see IC1B in the Arduino Due schematic), a current mirror like in the RPi B+, or using an exotic and rather expensive MAX40200 ideal diode integrating the MOSFET and the comparator.

Is this just to keep it 100% compatible with the BluePill ?

Is it just protection if someone powers via 5V and connects USB?

I think this may just have to be a limitation, that it’s not practical to have the protection diode on the board, as there is simply not enough space.

One other alternative could be 2 x 0.5A diodes, as perhaps they is space for 2 smaller diodes in different locations.

However my vote would be not to have the diode at all

[RogerClark – Fri Dec 08, 2017 9:16 pm] –
Is it really such a major problem if 5V is connected directly from the USB to that pin?

Is this just to keep it 100% compatible with the BluePill ?

Is it just protection if someone powers via 5V and connects USB?

I think this may just have to be a limitation, that it’s not practical to have the protection diode on the board, as there is simply not enough space.

One other alternative could be 2 x 0.5A diodes, as perhaps they is space for 2 smaller diodes in different locations.

However my vote would be not to have the diode at all

if we ditch the diode, we also ditch the other other current limiter, and then the issue is that as usb host you can’t accept a powered device. That is a tradeoff we can choose for, but it’s a limitation (but would indeed save us a TON of boardspace)

If people really like the board and think its worth the extra money for the expensive MAX40200, then it would not be that hard to produce boards with that on it.

But for now, I think we need to move forward..

1N5819HW.png (119.29 KiB) Viewed 149 times

Here is what KiCad is showing for the regulator U4 and the diode

D_SMA_footprint.png (7.06 KiB) Viewed 146 times

1N5819HW is also a 1A Shottky diode able to withstand the required power and is easy to find on Aliexpress:
https://www.diodes.com/assets/Datasheets/ds30217.pdf

OK.

A smaller package can probably me made to fit.

And I am pretty confident that if I replace the 32kHz crystal by a smaller FC-12M package as suggested by @racemaniac, I will be able to fit the ferrite bead between GND and AGND, which should cover most of the problems we found so far.

Then, we have all the options as footprints only (battery charger, IMU, RGB LED…)!

Just in case I’m missing something with KiCad.

Can you guys confirm that the footprint dragging doesnt work in OpenGL mode, but the interactive Push / Shove (of tracks) feature only works in OpenGL mode.

So if i want drag a track I need to switch to OpenGL to take advantage of the Push/Shove but if I want to drag a component and keep the track segments attached by simple rubber banding, this only works in “Canvas” view mode ??

PS. I’m using the latest stable version (4.0.7) not the “nightly” builds (I’ve heard that the nightly’s are much more advanced than the stable, but normally the Stable is good enough for me)

Thanks.

Hopefully in the next version they will unify things, as its not ideal having to switch in and out of OpenGL mode

This means that for reliable operation, the bootloader should have stable levels on USART1_RX (PA10), USART3_RX (PB11 and PC11), CAN2_RX (PB5) pins during boot, in addition to BOOT0 being high and BOOT1 (PB2 pin) being low, which is the case when the BOOT0/USER button is pressed.

This is confirmed by a remark in the MicroPython board schematic:USB DFU requires stable levels on PA10, PB5, PB11 & PC11. PB2 must be low during boot.

Even if the pins were randomly toggling with noise it would only be a 1 in 256 times that the data would match the pattern.

And in reality I don’t think the input pins randomly toggle, unless you attach a long length of wire to them to pickup noise, and in most cases that would pick up mains hum of 50 or 60 Hz

e.g.
With the RobotDyn Black Pill boards that I received the other day, they did not send jump links, so I did not solder the boot0 or boot1 pins. I just flashed the bootloader via STLink and they worked fine even with boot0 technically floating.

The Maple mini does not pull boot1 low but unless you stick your finger on that pin, it’s possible to reflash just by pulling boot0 high.

I need to test this hypothesis, but I suspect the pins have a tendency to float low.

1. add extra components to pull those pins low, which may affect their usage for other functions (if the pull down is too weak, it may not have an an effect other than if the pins are floating, if the pull down is strong, then it may affect other uses.
2. leave then like they are, in the particular conditions they may affect usb dfu bootloader

My vote goes for the second option, since I believe the conditions in which may cause the bootloader to not get to the USB port, would be only if there is something in serial sending that character, and in that case the pull downs would not help, since I would expect whatever serial device is in the other end to be stronger than the pull downs, otherwise your serial functionality is compromised. I don’t think something else other than serial will cause it to randomly get the special character.
If it happens, then the stlink pins are available, and if not, we can load our own bootloader that goes straight to USB and that’s it. There is code from STM that Roger and me tested a couple of months back. If we need to, we can work on that to make it funtions the way we want. We could even add sdio support to upload boards with a bin in the sdcard.

I will then implement solution #2 (not care about it) since 1) I think this situation is unlikely and can be fixed by a simple retry and 2) it is easier, since there is nothing to do!

Uploading a board from a bin file on the sdcard would be great!

I fixed all problems in the TODO list, it just needs more cleanup (more trace shufflîng, 3D models for new 32kHz crystal and Schottky diode, etc.).

I checked the board and it does not have a pulldown on PA9 or PA10

I also checked the STM32 Stamp schematic (there is a copy in my repo in the STM32F4Stamp folder) and that board does not have a pulldown on PA9 or PA10 (it can however use PA10 to connect to the serial port, I presume to signal OTG) if a jump link is installed

I think the micropython team are being over-cautious.

BTW. I find using the built in DFU hard to use, as its unclear whether code can reboot/reset the MCU into its internal DFU mode, so you would have to keep boot0 high, and press the reset button each time

(It may be possible to jump to the bootloader but I don’t think anyone has proved they can do that)

I know Victor has written a DFU bootloader, based on STM’s example code, and they would initially be the best thing to use (apart from STLink)
However because both the internal DFU bootloader and the one from ST’M’s code, use DFUSe, it is not compatible with the F103 DFU drivers or DFU-Util, so if I get time I want to investigate porting the existing F1 bootloader to F4
I know its possible, but the code to do it seems to have been lost.

[RogerClark – Mon Dec 11, 2017 6:32 am] –
I’ve tested DFU upload on one F4 board, and it seemed to work every time.

I checked the board and it does not have a pulldown on PA9 or PA10

I also checked the STM32 Stamp schematic (there is a copy in my repo in the STM32F4Stamp folder) and that board does not have a pulldown on PA9 or PA10 (it can however use PA10 to connect to the serial port, I presume to signal OTG) if a jump link is installed

I think the micropython team are being over-cautious.

BTW. I find using the built in DFU hard to use, as its unclear whether code can reboot/reset the MCU into its internal DFU mode, so you would have to keep boot0 high, and press the reset button each time

(It may be possible to jump to the bootloader but I don’t think anyone has proved they can do that)

I know Victor has written a DFU bootloader, based on STM’s example code, and they would initially be the best thing to use (apart from STLink)
However because both the internal DFU bootloader and the one from ST’M’s code, use DFUSe, it is not compatible with the F103 DFU drivers or DFU-Util, so if I get time I want to investigate porting the existing F1 bootloader to F4
I know its possible, but the code to do it seems to have been lost.

OK, thank you Roger for testing, I also think that this is over-engineering.

In AN2606, Table 3, there is a memory location, maybe it is just a matter of jumping there?

Yes. I think in theory it can be done. But I”ve read various posts on various forums where people seem to be having trouble doing that

Seems to be straightforward, have not tested it thought, but should be easy to test. I’ll try when I get a second.

@Roger you are giving me too much credit, I barely modified a few things. It’s mostly the code from STM, which Chriss Bar had already taken and done a few modifications.
I am sure we can modify it to be 100% compatible with our bootloader, alt modes and all. But if we can reliably use the hardware one, then no need for it and saves a few KB of flash, and the same BIN would be valid no matter what method is used for upload (serial, dfu, stlink…)

Re: F4 DFU bootloader

You managed to get it working more than I did

Re: Using the old bootloader. From the code snippets I’ve seen, I don’t think that too many changes are needed to get the old bootloader to work on the F4 and like you say, its smaller and can use all the existing binaries and drivers.

So perhaps if I get time over Christmas I’ll setup system workbench, or True Studio etc, and see if I can port it.

I think the register addresses for the GPIO are different (and also for the USB controls), and I know the GPIO clock settings etc will be different.
But the GPIO stuff should be easy to crib from the LibMaple F4 core.

The USB code in the LibMaple F4 code is a lot different from the F1, but I don’t know if there is a good reason for this.

Anyway, getting the bootloader LED flashing on the F4 would a be a good start !

[RogerClark – Tue Dec 12, 2017 4:36 am] –

I think the register addresses for the GPIO are different (and also for the USB controls), and I know the GPIO clock settings etc will be different.
But the GPIO stuff should be easy to crib from the LibMaple F4 core.

I believe you are right about GPIO, just the base addresses are different, but same registers and flags in the same offsets, so should work just changing the base address.
Not sure about USB, haven’t looked, but flash is different too, larger pages and a mix of smaller and larger pages in the same device, but for writing to the flash perhaps you can reuse the parts from the STM code.

I had not considered the flash writing part of the code. It’s strange that the flash page size changes depending on where the flash page is.
On the F103 the page size is bigger on the devices with more flash, I remember looking into this, but can’t remember whether it was for the bootloader or the core.

Its something like 1k on the Low Density MCU’s and 2k on the medium and possibly 4k on the High density.

But all pages in the same MCU will be the same size.

Having different sizes at different locations in the flash is a pain, as it would make the code a bit larger as it needs a case or if statement to handle it , in several places

So I’d probably need to look elsewhere for savings in code size, as it only just sits in 8k at the moment

I am redoing it in Kicad, but I am much slower as I don’t know the software well enough, but I am still learning

Right now I have the symbols, footprint and 3D models for the FC-12M 32 kHz crystal and the SOD-123 diode, I routed the diode, but still need to apply the other remaining changes.

I am doing it on my spare time, not easy before X-Mas!

However, it perfectly matches the one on the original Bluepill! I asked the vendor for a drawing, and will modify the footprint to be compatible with both.

I will share the Kicad files are soon as they are stable enough (hopefully before the end of this WE), before adding any option.

I eventually found a drawing that is a bitmap capture of the datasheet (I am still interested in it):

image.jpeg (138.84 KiB) Viewed 214 times

EDIT: This one shows a lightly different design but the footprint seems to match with the one you posted:
https://www.aliexpress.com/item/50pcs-M … 19250.html

[Squonk42 – Thu Dec 14, 2017 2:41 pm] –
I think it is possible to design a single footprint that will work with all of them: the 5 USB pins have a standard pitch (but their footprint length may be 1.10 or 1.15 mm), there may be a “lip” at the front or it can be flat like for the Chinese ones, the biggest differences are regarding the legs, but by designing large and long enough oval holes, I am pretty confident we can accommodate a lot of different “harpoon” style models.

XD
exactly what i was thinking (but didn’t want to give you even more work XD)

BTW. I noticed that Eagle are now advertising it now supports Push And Shove routing, but KiCad has had that for ages ( in OpenGL disolay mode)

I also happened to notice a video by Dave ( EEVBlog) about how Autodesk have consistently changed what they said they would do in terms of licensing and prices, since buying Eagle, and their prices and licensing model seem to get worse every day.

What clinched it for me, was finding I can’t use the version of Eagle which I upgraded to, without signing in to Autodesk to use it, despite paying for a perpetual license for the previous version.

If I had realised the “update” removed its ability to operate without signing in, I would never have updated.So I now have a non functional copy of Eagle installed, and would have to find my original installer file, and remove the new copy and reinstall the old copy etc etc. which is never worth the time and effort.

I started to migrate away from Eagle, as soon as Autodesk bought it, so don’t have any recent boards designed using it.
And for my older boards, they were never very complex and I would take the opportunity to do them again from scratch in KiCad, and fix the problems most of them have e.g. replace component footprints with more readily available parts

When i have some time i’ll assemble one, and give them a try .
As the noise on the ADC is one of the things we want to get better than the existing bluepills, does anybody have ideas of good testcases?

[racemaniac – Fri Dec 15, 2017 1:15 pm] –
As the noise on the ADC is one of the things we want to get better than the existing bluepills, does anybody have ideas of good testcases?

Pigoscope may be good code to visualize the noise. See what shows when floating, and when connected to known value with large resistors.
Since at the same time it reads ADC with DMA it may be using serialUSB or the SPI ports it may be getting some noise generated in the same board.

Here is a list of their micro USB connectors: https://bsc-elec.en.alibaba.com/product … ector.html

The one that is perfectly matching the Bluepill one is their model 008 (please notice the shell shape around the 5 USB pins):

BSC008.jpg (70.93 KiB) Viewed 255 times

[victor_pv – Fri Dec 15, 2017 1:45 pm] –

[racemaniac – Fri Dec 15, 2017 1:15 pm] –
As the noise on the ADC is one of the things we want to get better than the existing bluepills, does anybody have ideas of good testcases?

Pigoscope may be good code to visualize the noise. See what shows when floating, and when connected to known value with large resistors.
Since at the same time it reads ADC with DMA it may be using serialUSB or the SPI ports it may be getting some noise generated in the same board.

Anyone up for documenting how & what to test, and to do a testrun on the bluepill? (and to figure out how we can get a similar test running on the F4, or would the pigoscope code be compatible?)

There was an initial version without DMA, that for the purposes of measuring the adc noise should still work, and may run straight in an F4.

The current one may work in F3 MCUs though, since they are so close to the F1, or may work with just slight modifications.

What MCUs are you guys planning to put in these boards? just F405 and F411?

[victor_pv – Sun Dec 17, 2017 3:11 pm] –
I think you are right Roger. Perhaps with a few modifications it can work though.

There was an initial version without DMA, that for the purposes of measuring the adc noise should still work, and may run straight in an F4.

The current one may work in F3 MCUs though, since they are so close to the F1, or may work with just slight modifications.

What MCUs are you guys planning to put in these boards? just F405 and F411?

just f405 atm

The 3D model for the micro USB connector is still the old Molex one, but the footprint is the one for the BSC Model 010 above (the one I bought from Aliexpress). If there are 3D modeler experts, I can provide the datasheet

Please let me know if you spot some errors! I tried my best not to break things, but who knows…

I merged the PR

[RogerClark – Sun Dec 17, 2017 9:05 pm] –
i think the option of using something like a F103RE or F103RG etc would be interesting as all the F1 core would work, plus it has DAC and SDIO, and this board would have better ADC noise performance

great idea
why didn’t i think of that XD

I thought the F103RB was just like a F103CB in a different package, so it has more pins
It does not have extra features like DAC and SDIO

But it would run the Pig-O-Scope firmware

R8 would be the cheapest, as its just a C8 in a bigger package ( so just has more pins available)

I have end of year deadlines and some bugs to fix before friday

i may have time later in the week.

[Squonk42 – Mon Dec 18, 2017 8:19 pm] –
Yes, but I was looking for the cheapest STM32F103C8T6 replacement in an LQFP64 package!

The R8/RB miss the SDIO, so you won’t be able to test the SD card.
In that regard the RET6 seems to be the best size/price balance, cost about the same as the RC, but has 512KB of flash and 64KB of RAM.
In the other hand, all the RC/VC that have fallen in my hands were rebadged RE/VE and had the 512KB of flash and 64KB of RAM.

[victor_pv – Tue Dec 19, 2017 4:01 am] – The R8/RB miss the SDIO, so you won’t be able to test the SD card.

Apparently, ST is that clever that they designed the SDIO to be on SPI pins… This means that we should be able to drive the SDCard in single SPI mode on devices without SDIO peripheral.

This is indeed something I want to test and one of the reasons I bought some STM32F103C8T6 in the first place!

[Squonk42 – Tue Dec 19, 2017 5:38 am] –
Apparently, ST is that clever that they designed the SDIO to be on SPI pins… This means that we should be able to drive the SDCard in single SPI mode on devices without SDIO peripheral.

That is not what I see on the stm32f1ret datasheet.
I see SDIO in the following pins:
PC8
PC9
PC10
PC11
PC12
PD2

On the F1, none of them seem to be shared with any SPI port, even remapped.

On the F405 there is an SPI3 listed in those pins, but the mapping between SPI and SDIO does not match the SDCard usage.
For example:
CLK line is the same pin in SDIO or SPI mode for an SDCard, but in the F405 SPI3 CLK is pin PC10, while SDIO CK is pin PC12.

In SDIO Mode CMD line corresponds to Datain In SPI mode. But in the F405, MOSI (data in for the card) is in pin PC12, but SDIO CMD is pin PD12.

So the pins do not correspond. Either the board is wired to use SPI, or is wired for SDIO, but I do not see the way to have a set of traces match both uses, even in 1 bit mode.
Please correct me if I am wrong. These are the documents I used as reference:
405RGT datasheet: https://cdn.sparkfun.com/datasheets/Wid … 05RGT6.pdf
103RET datasheet: http://www.st.com/content/ccc/resource/ … 191185.pdf

I don’t know where I got this impression that it was compatible.

I merged the pull request as soon as I got the notification email

[victor_pv – Wed Dec 20, 2017 11:52 pm] –
Squonk, is this the final one, or are you stil thinking on adding something else?

How about we all first have a good look at it to do a last check for errors/improvements, and then we’ll have some of these produced .

[racemaniac – Thu Dec 21, 2017 1:01 am] –
How about we all first have a good look at it to do a last check for errors/improvements, and then we’ll have some of these produced .

I’m inpatient , but my question was more directed at the whole design, whether it has all components and features he wanted, or he is still working on adding things, not if the PCB design was final.

[RogerClark – Thu Dec 21, 2017 12:51 am] –
Looks amazing

I merged the pull request as soon as I got the notification email

Indeed, I saw it accepted before I finished posting here!

• Add teardrops => Check https://github.com/svofski/kicad-teardrops
• Panelization => Check pcb-panelizer ( http://blog.thisisnotrocketscience.nl/p … panelizer/)
• Option: Add an IMU somewhere on the bottom PCB size on an SPI or I2C bus to get a fully working flight controller board! i am thinking of an Invensense MPU6000 hooked to an SPI bus in order to get 8ksps performance
• Option: Add an RGB LED => 0603?
• Option: Add MCP73831 LiPo battery charger (would require an ideal diode like D3/FET2/R6 in the Olimexino ATMega32U4 schematics)
• Add pad/pin for VBUS for external PA9 VBUS_SENSE feature (USB Host) => Added a series resistor between VBUS and PA9 to avoid short-circuits
• Provide footprint for parallel capacitor near SDCard and voltage regulators
• Option: add an SPI Flash chip as an alternative to SDCard connector (overlapping footprints)
• Add optional shunt resistors to route a single bit SPI bus to the SDCard connector for devices without SDIO interface => NOT POSSIBLE, too tight!

The first 2 items are required steps to launch the final PCBs, but not strictly required for prototypes.
Many of the remaining items are options that need to be discussed/prioritized ar’least to see what will be included in the first version.

But as @racemaniac pointed out, there must be a previous check on the current design for possible improvments/errors.

And of course, this is a collaborative design and all input is welcomed!

Unfortunately, PA4-7 is crammed on the pins closest north of the STM32 on the BluePill board, and this is the same situation south of the STM32 for PA15+PB3-5 pins, so these signals are difficult to use for onboard chips such as SPI Flash or IMU. PB9-10+PC2-3 is spread all over the board, so not usable either.

This only leaves the possibility to use SPI1 on PB12-15, because the corresponding pins are located at the bottom left of the board and are close to each other. But the free PCB space in this region is tight, unless the SDCard connector is not mounted. This means that this SPI1 pin configuration may be suitable for an SPI Flash chip as an alternative to mounting the SDCard connector, which sounds reasonable. Of course, this is subject to being able to add the SPI Flash footprint on bottom side, as an alternative footprint to the SDCard connector.

This also rules out the SPI bus interface mentioned before for the IMU. The IMU can however be controlled using I2C with a limited 4ksps rate and located between or beneath the 2 button switches, where there is still some room. This sample rate is not ridiculous, most of the current flight controllers are still limited to 4ksps, only the latest ones switched to SPI and chips that can handle 8 or 16ksps.

What do you think?

I’d stick with the board as it currently is.

From my previous post, it seems obvious that routing an SPI bus to the built-in SDCard connector is utopia.

However, adding a pad/pin for VBUS for external PA9 VBUS_SENSE (USB Host) may be an interesting feature: we may re-purpose one of the 2 GND pins near the micro USB connector to output VBUS through a 0R shunt, to be mounted only when the USB Host feature is required.

It may also be possible to add parallel decoupling capacitors on the SDCard and the U1 LDO.

As the current micro USB connector is a little bit shorter than the previous Molex part, this leave some (little) room for adding a 0603 footprint close to VBUS, and it seems relatively easy to route the PA9 signal close to it.

The point is that it is now possible to perform this connection onboard instead of externally, like proposed previously: if we add a series 560 ohm resistor between VBUS and PA9 like the micropython board, this prevents short-circuits if PA9 is driven low (i ~= 9 mA, P ~= 44 mW). PA9 is 5V-tolerant, so no voltage divider is required, and if strict compatibility with the original Bluepill is required, one can unsolder this resistor to disconnect the signals, but at least, there is no risk for a blue smoke. And there is no real need to breakout the VBUS signal otherwise.

I think it is also possible to remove the R12 pull-up resistor on SDIO_D3 and replace it with a second parallel 100 nF (unmounted?) capacitor across SDCard voltage supply for better decoupling if required. The reason for the R12 resistor is unclear, I probably just took the micropython board as an example, but in their case it is only used for fixing the voltage level at boot time for securing the ROM bootloader, which seems not to cause particular problems based on our experience.

[Squonk42 – Sat Dec 23, 2017 1:02 pm] –
I looked further at the PA9/VBUS_SENSE to VBUS connection for the USB Host feature.

As the current micro USB connector is a little bit shorter than the previous Molex part, this leave some (little) room for adding a 0603 footprint close to VBUS, and it seems relatively easy to route the PA9 signal close to it.

The point is that it is now possible to perform this connection onboard instead of externally, like proposed previously: if we add a series 560 ohm resistor between VBUS and PA9 like the micropython board, this prevents short-circuits if PA9 is driven low (i ~= 9 mA, P ~= 44 mW). PA9 is 5V-tolerant, so no voltage divider is required, and if strict compatibility with the original Bluepill is required, one can unsolder this resistor to disconnect the signals, but at least, there is no risk for a blue smoke. And there is no real need to breakout the VBUS signal otherwise.

I think it is also possible to remove the R12 pull-up resistor on SDIO_D3 and replace it with a second parallel 100 nF (unmounted?) capacitor across SDCard voltage supply for better decoupling if required. The reason for the R12 resistor is unclear, I probably just took the micropython board as an example, but in their case it is only used for fixing the voltage level at boot time for securing the ROM bootloader, which seems not to cause particular problems based on our experience.

hadn’t noticed the pullup on the d3 line yet, indeed, best to remove it.
when using the sd card, just enable the internal pullups of the stm32 on the datalines, and it’ll be fine

What do you think about the series resistor between VBUS and PA9?

[Squonk42 – Sat Dec 23, 2017 1:24 pm] –
OK, I will do that!

What do you think about the series resistor between VBUS and PA9?

i think it’s also ok, but i’m a bit too tired & with my mind elsewhere to think it through XD

• Add teardrops => Check https://github.com/svofski/kicad-teardrops
• Panelization => Check pcb-panelizer ( http://blog.thisisnotrocketscience.nl/p … panelizer/)
• Option: Add an IMU somewhere on the bottom PCB size on an SPI or I2C bus to get a fully working flight controller board! i am thinking of an Invensense MPU6000 hooked to an SPI bus in order to get 8ksps performance I2C bus, as no SPI bus is available easily onboard with the real estate for the chip
• Option: Add an RGB LED => 0603?
• Option: Add MCP73831 LiPo battery charger (would require an ideal diode like D3/FET2/R6 in the Olimexino ATMega32U4 schematics)
• Option: add an SPI Flash chip as an alternative to SDCard connector (overlapping footprints)

And here is a 3D view of the result:

Stm32F405 board sold in Taobao.com

The header, USB connector and button switch looks cheap, but the price isn’t: 99 RMB is $15, and that is on Taobao…

I don’t know yet how much our BluePill F4 will cost, but I hope to keep the price between $5 and $10. Of course, this depends on volume and if we find someone to build it in Mainland China or not.

[Squonk42 – Sat Dec 23, 2017 1:02 pm] –
I think it is also possible to remove the R12 pull-up resistor on SDIO_D3 and replace it with a second parallel 100 nF (unmounted?) capacitor across SDCard voltage supply for better decoupling if required. The reason for the R12 resistor is unclear, I probably just took the micropython board as an example, but in their case it is only used for fixing the voltage level at boot time for securing the ROM bootloader, which seems not to cause particular problems based on our experience.

If I remember right, SDIO_D3 also has a function as SDCard detect when no card detect switch exists. I’m trying to find all the information, from what I remember there is a pull up of 1M or so internally in the sdcard, that can be disconnected with a command.
No idea why would need a resistor in series, but may have something to do with it, and likely carried from another board design.
If I can find more information on this, which should be somewhere in the internet, I’ll post it.

There is some mention about that pull up here:
https://www.sdcard.org/cht/downloads/pl … E1_100.pdf

Found a bit more infor, it’s 50K and pull up, page 20:
http://datasheet.octopart.com/IP4052CX2 … 555750.pdf

There are some circuits showing a 570K pull down externally. My guess is that’s used to ensure the line is down while a card is not connected, so card detection can effectively detect when one is connected and the line is pulled up.
Having a external pull-up would negate the card detection feature completely, so I can only guess that R12 is not related to card detection at all, and likely as Squonk thought is used for boot.

1M sdcard detect.JPG (37.49 KiB) Viewed 337 times

This rules out R12 pull-up completely. In the micropython schematic, it is clearly part of their scheme to fix the voltage of input pins used by the ROM bootloader.

I am a little bit nervous with pull-up/down values in Mohms: because of their high resistance value, they are very sensitive to ESD, as a small current will be enough to cause a significant voltage glitch. OTOH, if Olimex is using this trick for ages…

[Squonk42 – Sun Dec 24, 2017 4:57 pm] –
I am a little bit nervous with pull-up/down values in Mohms: because of their high resistance value, they are very sensitive to ESD, as a small current will be enough to cause a significant voltage glitch. OTOH, if Olimex is using this trick for ages…

STM had ESD protection in the SDCard pins int heir 3d printer board, with one of their chips for specifically that purpose (ESD protection for SDcard ports). It’s an option, but would add another footprint to route in the PCB and another part to the BOM.
The second link I added shows a 470K pull down, still pretty high, but half of the Megaohm ones

[Squonk42 – Sun Dec 24, 2017 4:57 pm] –
Thank to both of you for looking at it!

This rules out R12 pull-up completely. In the micropython schematic, it is clearly part of their scheme to fix the voltage of input pins used by the ROM bootloader.

I am a little bit nervous with pull-up/down values in Mohms: because of their high resistance value, they are very sensitive to ESD, as a small current will be enough to cause a significant voltage glitch. OTOH, if Olimex is using this trick for ages…

Normally the pins need a pull-up ( if we use those of the stm32 it’s 40k I think). The default pull-up of 200k is probably chosen to not affect the real pullups too much when put in parallel with them. When we put a pulldown for card detection, it’ll make a voltage divider with the 200k pull-up, so anything below 400k will cause the resulting voltage to be too close to VCC/2 (or even below it) when the card is inserted, so it’s logical to choose something big like 1M

PS: many sources say the internal sdcard DAT3 pullup is ~50k. Some specs say it is 10k-90k Min-Max. Some 50k +/- 20%.
There is the ACMD42 command which switches the pullup on/off when required..
PPS: The latest SD Physical Layer Simplified Specification v6.0 (page 11) says “At power up this line has a 50k pull up enabled in the card”.

[victor_pv – Sun Dec 24, 2017 7:06 pm] –

[Squonk42 – Sun Dec 24, 2017 4:57 pm] –
I am a little bit nervous with pull-up/down values in Mohms: because of their high resistance value, they are very sensitive to ESD, as a small current will be enough to cause a significant voltage glitch. OTOH, if Olimex is using this trick for ages…

STM had ESD protection in the SDCard pins int heir 3d printer board, with one of their chips for specifically that purpose (ESD protection for SDcard ports). It’s an option, but would add another footprint to route in the PCB and another part to the BOM.
The second link I added shows a 470K pull down, still pretty high, but half of the Megaohm ones

ESD protections are mandatory in an end-user product on all connectors, buttons, LEDS, etc. that are accessible externally in order to comply with EMC rules. In this case, TVS protection diodes must be used, such as PRTR5V0U2X for the USB connector, dual PRTR5V0U4D for the SDCard connector, and individual 0603 bidirectional ESD TVS diodes on buttons and LEDs. Products featuring high resistance values are also subject to a more subtle ESD problem, where this resistor is acting as an antenna for ESD surface currents on the enclosure (thus my fear, not counting for additional thermal noise).

But for a prototype board like this, the whole PCB is exposed anyway, so you are supposed to use them in an ESD-safe environment only (you always wear your ESD wrist strap, do you? ), and there is thus an exemption for this kind of products. This is why there are no ESD protections at all on our BluePill f4 board, this would add to the BOM cost without adding much effective protection anyway.

Note that this may cause a problem if this board is naively integrated as-is in an end-user product, though…

Please note also that for a bullet-proof EMC USB design, we would need to add a common-mode choke on USB data lines to avoid common-mode noise pollution, ferrite beads on on power USB power supply to filter out high-frequency noise, and high-voltage (500V) capacitor with parallel 1M resistor between shield protective Earth and ground in order to achieve proper GND level alignment upon cable insertion… Not implemented here for the same reason as above!

[Pito – Mon Dec 25, 2017 11:45 am] –
I am a little bit nervous with pull-up/down values in Mohms: because of their high resistance value, they are very sensitive to ESD, as a small current will be enough to cause a significant voltage glitch.
No problem with 1M pulldown as it is active only during “card detect read of the DAT3”. When the card is not inserted you have to read 0, thus the parasitic pullup resistances shall be kept high at that line.
The only source of voltage at the 1M when sdcard not inserted, imho, is the reverse current of the high-side clamp diode (pin’s built-in ESD protection) which could be something around 100mV max (Ir=100nA worst case).
Otherwise there could be the stm32’s pullup (say 40k || 200k 50k) active as Victor wrote (that eliminates the 1M “sensitivity”).

PS: many sources say the internal sdcard DAT3 pullup is ~50k. Some specs say it is 10k-90k Min-Max. Some 50k +/- 20%.
There is the ACMD42 command which switches the pullup on/off when required..
PPS: The latest SD Physical Layer Simplified Specification v6.0 (page 11) says “At power up this line has a 50k pull up enabled in the card”.

There is not much room to add a new 0603 footprint near the SDIO_D3 signal. Do you think that this “SDCard Detect” feature is required and if so, should we sacrifice one the 2 decoupling capacitors on the SCard connector to get it on board?

[Squonk42 – Mon Dec 25, 2017 4:08 pm] –

[Pito – Mon Dec 25, 2017 11:45 am] –
I am a little bit nervous with pull-up/down values in Mohms: because of their high resistance value, they are very sensitive to ESD, as a small current will be enough to cause a significant voltage glitch.
No problem with 1M pulldown as it is active only during “card detect read of the DAT3”. When the card is not inserted you have to read 0, thus the parasitic pullup resistances shall be kept high at that line.
The only source of voltage at the 1M when sdcard not inserted, imho, is the reverse current of the high-side clamp diode (pin’s built-in ESD protection) which could be something around 100mV max (Ir=100nA worst case).
Otherwise there could be the stm32’s pullup (say 40k || 200k 50k) active as Victor wrote (that eliminates the 1M “sensitivity”).

PS: many sources say the internal sdcard DAT3 pullup is ~50k. Some specs say it is 10k-90k Min-Max. Some 50k +/- 20%.
There is the ACMD42 command which switches the pullup on/off when required..
PPS: The latest SD Physical Layer Simplified Specification v6.0 (page 11) says “At power up this line has a 50k pull up enabled in the card”.

There is not much room to add a new 0603 footprint near the SDIO_D3 signal. Do you think that this “SDCard Detect” feature is required and if so, should we sacrifice one the 2 decoupling capacitors on the SCard connector to get it on board?

Not having an sd card detect is quite annoying i think :s. so if possible it would be *really* nice to have.

[racemaniac – Mon Dec 25, 2017 9:29 pm] –

[Squonk42 – Mon Dec 25, 2017 4:08 pm] –

[Pito – Mon Dec 25, 2017 11:45 am] –

No problem with 1M pulldown as it is active only during “card detect read of the DAT3”. When the card is not inserted you have to read 0, thus the parasitic pullup resistances shall be kept high at that line.
The only source of voltage at the 1M when sdcard not inserted, imho, is the reverse current of the high-side clamp diode (pin’s built-in ESD protection) which could be something around 100mV max (Ir=100nA worst case).
Otherwise there could be the stm32’s pullup (say 40k || 200k 50k) active as Victor wrote (that eliminates the 1M “sensitivity”).

PS: many sources say the internal sdcard DAT3 pullup is ~50k. Some specs say it is 10k-90k Min-Max. Some 50k +/- 20%.
There is the ACMD42 command which switches the pullup on/off when required..
PPS: The latest SD Physical Layer Simplified Specification v6.0 (page 11) says “At power up this line has a 50k pull up enabled in the card”.

There is not much room to add a new 0603 footprint near the SDIO_D3 signal. Do you think that this “SDCard Detect” feature is required and if so, should we sacrifice one the 2 decoupling capacitors on the SCard connector to get it on board?

Not having an sd card detect is quite annoying i think :s. so if possible it would be *really* nice to have.

OK, actually, the main LDO U1 and the SD Card connector are very close to each other, so we can remove one decoupling capacitor safely. I will then add the 1M pull-down resistor on SDIO_D3 to get the SDCard detect feature.

I started to add a 1616 (“0603”) RGB LED to replace the red LED D2: it is possible to get a footprint which is compatible with both, so a cheap version will have only the red one, and as an option (more expensive?), we can get an RGB LED by mounting 2 resistors to connect the blue and green cathodes to PA14 and PA13, respectively. These signals are only used for SWD, so it will add some colors during flashing

Unfortunately, AFAICT PA13/PA14 and PC13 do not have PWM capabilities.

An another point is an sdcard possesses a ~uF decoupling capacitor inside, so a hot-insertion of the sdcard could cause a current surge resetting the mcu. Thus powering the sdcards requires a careful design (ie. a separate voltage regulator, LC filter, large capacity low ESR capacitor, etc)..
https://forum.arduino.cc/index.php?topi … msg2214450

[Pito – Tue Dec 26, 2017 10:58 am] –
Not having an sd card detect is quite annoying i think :s. so if possible it would be *really* nice to have.
Btw, the only way how to get an sdcard under full control for ie. a “hot-swapping” or a “recovery” from a crashed sdcard is to have the sdcard’s Vcc power switchable on/off (ie. via a high-side pmosfet, etc.).. And the OS/core must support that option as well..

An another point is an sdcard possesses a ~uF decoupling capacitor inside, so a hot-insertion of the sdcard could cause a current surge resetting the mcu. Thus powering the sdcards requires a careful design (ie. a separate voltage regulator, LC filter, large capacity low ESR capacitor, etc)..
https://forum.arduino.cc/index.php?topi … msg2214450

Ooh, thanks for the extra info, was wondering about the first (what to do when an sd card crashes, if you could resolve it via software)
it’s odd that you can’t >_<…
And i already ran into the sd card resetting the mcu on my lightsaber boards, but if we put a 4.7uF capacitor across it (as in the current design), isn’t that already enough?

Well, we can’t afford to have a PM for the SDCard only, unfortunately.

As for the inrush current, the AP2114 looks like it has a 40mV dip @1A using the same 4.7µF caps that we use here, so I hope it will be good enough not to reset the STM32. We may have to test and adjust the capacitor values/types.

• Add teardrops => Check https://github.com/svofski/kicad-teardrops
• Panelization => Check pcb-panelizer ( http://blog.thisisnotrocketscience.nl/p … panelizer/)
• Option: Add an IMU somewhere on the bottom PCB size on an SPI or I2C bus to get a fully working flight controller board! i am thinking of an Invensense MPU6000 hooked to an SPI bus in order to get 8ksps performance I2C bus, as no SPI bus is available easily onboard with the real estate for the chip
• Option: Add MCP73831 LiPo battery charger (would require an ideal diode like D3/FET2/R6 in the Olimexino ATMega32U4 schematics)
• Option: add an SPI Flash/FRAM chip as an alternative to SDCard connector (overlapping footprints)

And here is a 3D view of the result:

[racemaniac – Wed Dec 27, 2017 7:23 am] –
btw, maybe time to do an update of the BOM?

I created a pull request with updated BOM (BOM files were in .gitignore ). I added the PDF files for schematic and layout at the same time.

I think I can fit the same inductor as Olimex (LQW2BASR47J00L) which is a relatively large 0805 footprint, but I cannot add more capacitors than the 4.7µF 6.3V X7R 0603 already installed. We can replace it with a 10µF with same other characteristics if required. Do you think we should be OK with this setup?

We have the AP2114HA-3.3TRG1 LDO D1 nearby with its 2 output capacitors C8 (4.7µF 6.3V X7R 0603) and C18 (100nF 50V X7R 0603), then the inductor above in series with the SDIO_VDD, then C&6 (another 4.7µF 6.3V X7R 0603), all in a tight space. We can change the values or put a ferrite bead and experiment, I guess.

Many of the SDIO Card interface I have seen on dev boards (some much larger than our BluePill) do not provide such a luxurious filtering, probably because they don’t consider hot swapping the card.

On a layout point of view, there won’t be much more I will be able to stuff in there, so I will release a new version with the additional 0805 footprint in series with the SDCard power supply, we will have to test.

Unfortunately, I don’t have an Olimex F407 board available to test for the Vdd transient

The another option is a “ferrite bead” – they are rated in ohms, like 22..1000ohm (an wideband impedance) but for >=1A currents (Rs=0.0xxohm).
For example:
https://eu.mouser.com/Passive-Component … _/N-bw7pa/
https://eu.mouser.com/productdetail/mur … 5UCw%3D%3D
http://www.mouser.com/ds/2/281/c51e-794816.pdf
They are easily to get in 0603 as well.

Anyhow, the best way to design that luxurious filtering is to measure how it works in situ..

PS: if it fits leave the 0805 pads there and you may experiment with the best type of inductor/FB.
Worst case you may deploy a 0ohm resistor there when the luxurious LC would not be required.

SDCArd Inductor.png (56.31 KiB) Viewed 234 times

1) If what you are talking about are the traces circled in red, this is normal: it is part of my attempts to add teardrops to the board. If the trace goes straight, the teardrop will trigger a DRC violation because it is to close to the nearby trace.

As for the one circled in green, I will drag the trace, no problem!

Teardrops.png (71.12 KiB) Viewed 191 times

There are also some problems of coordinate comparisons that are done strictly without systematically applying a tolerance value: these ghosts unconnected value are symptomatic

Let me know if it fixes the problems for you: for me, I no longer get unconnected signals after applying a “Cleanup Tracks and Vias”, nor do I have unconnected signals in the status bar.

I also cleaned up the unnecessary labels in the schematic, and improved the 3D model for the FC-12M crystal.

Let me know if you still experience “Unconnected” wires.

[Squonk42 – Mon Jan 01, 2018 8:40 pm] –
I pushed a new version after checking the generated gerber files with gerbview.

I also cleaned up the unnecessary labels in the schematic, and improved the 3D model for the FC-12M crystal.

Let me know if you still experience “Unconnected” wires.

looks better indeed, nothing indicated as unconnected anymore, and a cleanup of tracks & traces doesn’t remove required traces anymore

Thanks for testing!

I strongly recommend to use FreecAD version 0.17 or later.

– the gnd of ap2112k should be connected to agnd, not gnd
– your alternative to the seperate voltage regulator doesn’t match what you described in your post:

the grounds of the resistors before & after the ferrite bead should have some distance, the resistor after the cap’s ground & the ground of the IC should be as close as possible
this might affect the performance of your alternative to the seperate regulator

I agree on the first remark. On the second one, “apart” is a relative concept, especially on this tiny board

I am thinking or removing the “CLC” solution to keep only the AP212 (with AGND). What do you think?

On another subject, I think it is very feasible to add an optional LiPo charger circuit based on the Microchip MCP73812 and an “ideal diode” like used in the OLIMEXINO-32U4 :

OLIMEXINO-32U4 LiPo Charger.png (110.36 KiB) Viewed 192 times

[Squonk42 – Sat Jan 06, 2018 9:36 am] –
No problem, the more pairs of eyes, the better!

I agree on the first remark. On the second one, “apart” is a relative concept, especially on this tiny board

I am thinking or removing the “CLC” solution to keep only the AP212 (with AGND). What do you think?

On another subject, I think it is very feasible to add an optional LiPo charger circuit based on the Microchip MCP73812 and an “ideal diode” like used in the OLIMEXINO-32U4 :
OLIMEXINO-32U4 LiPo Charger.png
It should fit on the bottom of the board, between the right edge and the SWD connector. I still don’t know where I will connect the battery though…

for me only the second regulator is fine. it’ll probably be more reliable than the other option since it’s indeed hard to properly seperate those grounds.
the charger sounds fun, but that ideal diode is probably not a cheap/easy part to get?
and one thing that’s also bothering me a bit when seeing the 3d model: some of the pads on the bottom are underneath the sd card when it’s inserted? not such a huge problem, also since they’re probably pretty hard to move ^^’

[racemaniac – Sat Jan 06, 2018 9:44 am] – for me only the second regulator is fine. it’ll probably be more reliable than the other option since it’s indeed hard to properly seperate those grounds.

What worries me is that in almost all STM32F schematics that I can find, the +3.3VA is only obtained by filtering the +3.3V using a ferrite bead and a couple of 10µF/6/3V + 100nF capacitors. I just feel that using both a separate LDO and an inductor between AGND and GND is a little bit over-engineered.

[racemaniac – Sat Jan 06, 2018 9:44 am] – the charger sounds fun, but that ideal diode is probably not a cheap/easy part to get?

The “ideal diode” here is just the IRLML6402 PMOS and the 1N5819 Schottky diode, along with the 10K resistor to polarize the MOSFET correctly. The IRLML6402 is a very common part, available at all global web distributors, but also on AliExpress and Taobao at a very low price. The 1N5819 Schottky diode is the same that we are already using for the connection between VUSB and +5V, so cheap too.

All components are easy to solder by hand (no QFN…), so they could be added by a motived DYI person afterwards, or sold as an option.

For the battery connection, I think I will only provide a simple 1mm drill TH for VBAT (and rename the existing pin VBAT to VBK to avoid confusion, as it is more for RTC backup), the question is where to put this pad: it is huge

[racemaniac – Sat Jan 06, 2018 9:44 am] – and one thing that’s also bothering me a bit when seeing the 3d model: some of the pads on the bottom are underneath the sd card when it’s inserted? not such a huge problem, also since they’re probably pretty hard to move ^^’

Yes, these are the pads for PC6/PC7. But these signals are quite important, as they are the only way to get the I2S2_MCK/I2S3_MCK signals.

I will see what I can do: it looks like I can route PC7 under the PC6/SDIO_D2/SDIO_D3 traces, then use a via to cross the SDIO bus and have the PC7 pad close to the other ones. For PC6, I can probably move up the PB15/PB14 pads to route a trace on top between SDO_D0 and PB15, then have the PC6 pad close to the other ones.

BluePillF4 PC6-7.png (154.8 KiB) Viewed 194 times

[Pito – Sat Jan 06, 2018 2:14 pm] –
Can you reuse the Vcc/Gnd pins from the SWD header for the battery as well
a) You do not need battery connected when doing programming via SWD..
b) You may not need Vcc connected on the Vcc pin while programming..

Yes! So, I added a 0R between the SWD +3.3V pin (now +VBAT) and the +3.3V signal, so:

• it behaves like on the BluePill if there is no LiPo charger circuit, the +3.3V pin on the SWD header is an input that will compete with the LDO output (bad )
• if you have a LiPo charger circuit and no battery connected, just connect the SWD +3.3V power to the +3.3V pin on the header near the NRST pin (still bad )
• better: feed the board from +5V or USB if no battery or no battery charger circuit!
• but if you have a LiPo charger circuit and a battery connected, just don’t connect the pin to anything and use the battery power

On other subjects, I fixed the AGND problem on the analog LDO and separated the GND pads on the capacitors in the CLC filter option: actually, one is now on AGND, the other on GND and much farther apart.

I also have the Olimex LiPo charger circuit routed, I just need to clean up all this mess before committing the changes.

[Squonk42 – Tue Jan 09, 2018 10:04 pm] –

[Pito – Sat Jan 06, 2018 2:14 pm] –
Can you reuse the Vcc/Gnd pins from the SWD header for the battery as well
a) You do not need battery connected when doing programming via SWD..
b) You may not need Vcc connected on the Vcc pin while programming..

Yes! So, I added a 0R between the SWD +3.3V pin (now +VBAT) and the +3.3V signal, so:

• it behaves like on the BluePill if there is no LiPo charger circuit, the +3.3V pin on the SWD header is an input that will compete with the LDO output (bad )
• if you have a LiPo charger circuit and no battery connected, just connect the SWD +3.3V power to the +3.3V pin on the header near the NRST pin (still bad )
• better: feed the board from +5V or USB if no battery or no battery charger circuit!
• but if you have a LiPo charger circuit and a battery connected, just don’t connect the pin to anything and use the battery power

On other subjects, I fixed the AGND problem on the analog LDO and separated the GND pads on the capacitors in the CLC filter option: actually, one is now on AGND, the other on GND and much farther apart.

I also have the Olimex LiPo charger circuit routed, I just need to clean up all this mess before committing the changes.

sounds great

[Pito – Wed Jan 10, 2018 9:57 am] –
Also – for demanding users who are ready to pay $3 more for 4 layers – what would happen if you add 2 layers – GND and VCC? It may help you with routing as well..

Actually, routing is not that bad, there is still some unused space left

The idea is to get an F4 version of the BluePill board, if possible made by a Chinese manufacturing house. IMO, a large part of the success of the BluePill board is because of its cheap price: it’s in the same ball park as the Arduino Pro Mini @$1.72. You can get cheaper boards featuring ATMega 168, ATTiny85 or down to STM8S103F3P6 @$0.66, but you get so much more power with the BluePill…

OTOH, you can get much more powerful chips with a little more money, including ESP8266 and ESP32.

So if there is a sweet spot for an F4 BluePill, it must be at the lowest possible cost, with the benefit of raw CPU power and numerous peripherals with DMA.

Most people here are very concerned about price, so I think we should stick to a 2-layer design only. I admit 4 layers would bring better performance (including for EMC reasons), but then, you can always add the GND and power layers and clean up traces if required for your needs.

• Main thing: I added a LiPo battery charger as an option on the bottom of the board below the SWD connector. It uses the same MCP73812T-420I/OT and ideal diode made up of a PMOS FET transistor and a Schottky diode as Olimex in its OLIMEXINO-32U4 board. The battery has to be connected to the 2 extreme pins on the SWD header,
  as there are other ways to power the board anyway. If the charger option is not installed, a 0R mounted on the board top side makes it strictly compatible with the original Bluepill by connecting it to +3V3
• The GND on the analog LDO is now on AGND
• The alternative (simpler) analog power supply using a CLC filter is now laid out better
• The VBUS_EN pin has been changed from PC4 to PC0, as this pin is less useful for anything else
• The pads on the bottom side of the board for PC1-PC7 are now aligned and no longer below the SDCard, with a nice 1.27 mm pitch

Here is what it looks like:

Please let me know if you find a problem, or just if you want to discuss regarding the board!

[Squonk42 – Sat Jan 13, 2018 9:01 pm] –
I pushed a new version of the BluePill F4 board with the following features:

• Main thing: I added a LiPo battery charger as an option on the bottom of the board below the SWD connector. It uses the same MCP73812T-420I/OT and ideal diode made up of a PMOS FET transistor and a Schottky diode as Olimex in its OLIMEXINO-32U4 board. The battery has to be connected to the 2 extreme pins on the SWD header,
  as there are other ways to power the board anyway. If the charger option is not installed, a 0R mounted on the board top side makes it strictly compatible with the original Bluepill by connecting it to +3V3
• The GND on the analog LDO is now on AGND
• The alternative (simpler) analog power supply using a CLC filter is now laid out better
• The VBUS_EN pin has been changed from PC4 to PC0, as this pin is less useful for anything else
• The pads on the bottom side of the board for PC1-PC7 are now aligned and no longer below the SDCard, with a nice 1.27 mm pitch

Here is what it looks like:

Please let me know if you find a problem, or just if you want to discuss regarding the board!

niiiice XD
one tiny remark though: there’s a silk screen line going trough the pc7 pad (although when plotting the gerbers, you can substract it from the silk screen ).

PS: the PC1-PC7 will become better accessible too. The Q is the usb socket – it could stay as-is, if you ask me..

[racemaniac – Sun Jan 14, 2018 8:43 am] – niiiice XD
one tiny remark though: there’s a silk screen line going trough the pc7 pad (although when plotting the gerbers, you can substract it from the silk screen ).

Fixed:

[Pito – Sun Jan 14, 2018 11:54 am] –
Another option is to have the current bottom the new top.. Sdcard will stay as-is, but leds and buttons have to be placed on the new top.. That could be easy as there is nothing beneath the leds and buttons currently..
Like Maple Mini did..
You must not see the chip, and you will get more place for silk screen messages and logos

PS: the PC1-PC7 will become better accessible too. The Q is the usb socket – it could stay as-is, if you ask me..

that would then break the point of the basic items of the board (the bluepill compatible part) all being on 1 side

[ChrisMicro – Sun Jan 14, 2018 9:24 am] –
Your design looks very nice. Probably it would be useful if the SD-Card Holder would be turned by 180°. It could be easier for a user to exchange the SD-card when the board is built in a housing.

At one point in time, I had the SDCard turned 180°, but I figured out it would not be easy to access it anyway, since the micro-USB plug probably be in the way. And this is no fancy push-push SDCard holder…

But I may be wrong. If this is the case, there is a nice puzzle to solve when reordering the traces below the STM32

EDIT: below you can see what I mean (I just put the SDCard holder on an original BluePill):

With this MCU, the micro USB connector, a (larger but beefier) LDO, 2x (smaller) crystals, 2x buttons (vs. 1x, lower profile), 2x LEDs, the SWD header, 1 additional Schottky diode, 13 resistors (vs. 8), 15 capacitors (vs. 13), 2 inductors (vs. none) and no cumbersome jumper block, this should be in the same $2~$3 ballpark as the original BluePill, but with more buttons for reset, boot selection and custom application usage, a correct USB pull-up resistor, a VUSB/+5V reverse current diode protection and more power… All with a lower profile (flat bottom), as the tallest part besides the SWD header are the LDO and the micro USB connector (< 2 mm). EDIT: and better analog supply too!

Here is the new “BluePill F1”:

As traces and pads on a PCB cost nothing except for the time you spend laying them out, it may be a good opportunity to etch some useful circuit that may be commonly used by developers. This is why I started by adding the LiPo charger circuit above as a nice option

I checked existing STM32 designs for more ideas: ST own Nucleo and Discovery boards, 3rd-party boards like Olimex or Itead, language-oriented Espruino and pyboard boards, and also some more specific boards for flight controllers or autopilots like Pixracer and Paparazzi.

In no particular order, here is a list of possible integration candidate circuits:

• Audio (I2S codec or analog interface to ADC/DAC): probably too big to fit and not of general interest
• 2.4GHz RF module: too big
• LCD/OLED screen: like the NodeMCU+OLED combo
• Micro-joystick (on bottom face?)
• Reset controller chip
• Ethernet: too big
• USB TVS: would be difficult to add as an option, and not required on a bare dev board unless it is integrated into a product
• RS232 buffer
• Bluetooth module: too big
• Coin-cell battery or “Gold Cap” for RTC
• FRAM/Flash SPI chip (SOIC8): tried to fit a footprint as an alternative to the SD Card connector, but this results in turning the nice (small) GND plane below the main LDO to pieces => not good
• MOSFET for power output (buzzer, relay, etc.): how to make it optional?
• Battery voltage resistor divider
• CAN transceiver
• 3, 6 or 9-axis IMU (Inertial Measurement Unit), e.g. accelerometer, gyroscope, magnetometer, pressure sensor (altitude): problem is most of them are soldering iron-unfriendly QFN packages These are used of course in all flight controller or autopilot boards, but also on more general-purpose boards like the ST boards (they sell MEMs…) and pyboard, for example…
• “FrSky Inverter”, e.g. a dual XOR gate to invert the level of UART signals as used by this common R/C protocol
• …

Please let me know what do you think of this, or if you have even more circuits to propose!

I2C FRAM/Flash are 4x to 50x slower than their SPI counterparts, but they may still be useful, you are right. They will then be easier to place in the large empty area below the buttons, and I2C is indeed requiring only 2 signal wires which are easy to find. Maybe a combination of alternative I2C footprints could be nice to have? Like the FRAM/Flash, some I2C sensors, 0.91″ OLED screen, etc?

i think we’re now at a point where it is interesting to order a few boards and build a few prototypes?

This means that we have around 2 weeks to finish the design, or we will only get the boards on mid-March.

I have most of the components available to make a few boards.

If nobody spots more problems in the current version, then the only thing left is to duplicate the PCB to add the teardrops, at least for a better drill to pad tolerance, mechanical and thermal stress. It looks like the board dimensions are too small for www.allpcb.com to do V-cuts, but they accept tab routing and they propose to do it themselves for free, resulting in a total cost including 24h lead time and TNT shipping to France (3-5 days) for 40 pieces @ $20 (60 pieces are only @ $23 !?!). Unfortunately at this price, the boards will be green, not blue, this adds $8 more

We do not take many risks by adding footprints on the bottom side for some I2C or other simple devices like voltage divider, MOSFET, etc. But we have to decide what we want asap, as everything will not fit.

Having microSD card is already a killer feature!

As for extra circuit I vote for 1) Extra (F)RAM 2) CAN transceiver 3) Battery resistor driver

Cheers, Ollie

So, why should someone want to exchange the SD-card?
There are many reasons:
1. The F4 is capable to play MP3 files
2. Someone makes a data logger and wants to transfer the collected 16GB of data by exchanging the SD-card
3. SD-cards are not famous for the life span

[ChrisMicro – Tue Jan 16, 2018 7:26 pm] –
Just one remark to the “SD-card exchange problem”:
To exchange the SD-card on the bottom side when the F4BP is soldered is probably impossible.
<…>

On the surface, your argument is sound. The reality is that I have been playing around with the rPi_Zero-W since they were first available, and it is very, very rare to have to remove the SD card.
Cards today are all wear-leveled and are very tough. A little bit of S/W to manage the filesystem should go a long way to dealing with not needing to remove the card… that is, if using for logging, have an option that spools the file to the serial port of the PC (or USB) and a dialog requesting “Delete?” at the end of the spooling will do necessary housecleaning.
If the board is mounted upside down, small holes in the hosting board or enclosure can be utilized for the buttons. Slap a label over the holes if you want it dust free.

Just thinking out loud.

Ray

Just the SD Card connector on the Teensy is $1.90, our connector is $0.30, although not a fancy push/push type.

Anyway, it is not possible to move the SD Card connector on the other side of our board while keeping the original Bluepill pinout compatibility as we have the SWD header on this side.

We are left to leaving the SD Card in its position, either 1) with the same orientation and card removed “under the belly” which is not possible when mounted on a breadboard, 2) turned 180° but then you have to disconnect the USB plug in order to remove the card, 3) flip the whole board upside down with “above the belly” orientation, but then we need to put the buttons and LEDs on the opposite PCB side, and the micro USB connector will be reversed.

I spent 2 hours to turn the SD Card connector 180°, and I have 2 unrouted wires left (SDIO_D3 pull-down and PB12 signal), so solution 2) may be possible, although not easy…

I’m also interested in grabbing some of these – if they come built

There have been a few people besides Roger that registered to allpcb with the link I posted, so even thought the cost with allpcb went significantly up, we still can get a good bunch of free boards with the credit.

[racemaniac – Wed Jan 17, 2018 9:03 am] –
same here, sd card position is ok for me

+1 or +3
stephen

[Squonk42 – Tue Jan 16, 2018 1:00 pm] –
It looks like the board dimensions are too small for www.allpcb.com to do V-cuts, but they accept tab routing and they propose to do it themselves for free, resulting in a total cost including 24h lead time and TNT shipping to France (3-5 days) for 40 pieces @ $20 (60 pieces are only @ $23 !?!). Unfortunately at this price, the boards will be green, not blue, this adds $8 more

When I do a quote on their system, if I select v-routing for 60 pieces, panel by ALLPCB (so we provide gerbers for a single board and they panelize it), get a quote of $26.
I am setting the dimensions to 16×64 similar to the blue pill.

EDIT: If I just select 60 individual boards, no panel, comes up as $19. Since these are not for industrial production, I would think having the individual boards from the start is just the same as much effort to assemble and reflow as DIY as having them panelized, or anyone sees an advantage on having the panel?

Also, any change to the components in this post?
viewtopic.php?f=19&t=2633&start=360#p37849
Perhaps we should edit Roger’s first post to add the links.

@Squonk42: the big blue traces loop in the middle.. would it work?

[Pito – Wed Jan 17, 2018 5:23 pm] –
or anyone sees an advantage on having the panel?
They do not provide Vcut within a panel when the individual board is less than 80x80mm.. (do select “Panel Separating Way:”)
So the only option is, for example, to buy Single PCB, 60pcs 64x16mm, $19 as of today.
PS: It seems they are steadily increasing the prices, 100×100 5pcs $23 today..

@Squonk42: the big blue traces loop in the middle.. would it work?

You are right about the price increase for 100×100.
About the v-cut, I have no problem selecting it when I select a board that’s 16×64 and set the panel as 6×2, so 6 boards wide (96mm) and 2 high (128mm).
You can’t have vcuts if the whole panel is smaller than 80×80, but the individual boards being smaller is fine as long as the whole panel is larger.

Comparing in PCB shopper for 100×100 5 or 10 pieces EasyEDA is cheaper while also shipping with DHL.
Anyway we have some free credit for AllPCB, still nothing can’t beat free