Community rework of standard maple and maple mini.

LeafLabs Garden » Support » Maple Hardware Support

Community rework of standard maple and maple mini.

(181 posts) (14 voices)

Started 2 years ago by feurig
Latest reply from crenn

« Previous 1…8910…13 Next »

soycamo
Member

@gbulmer You use the leftover X-ray sheets like you would kapton sheets. It's simply reusing existing materials.

Building the Orone-mini-S8A right now... it's in the oven! I see some discrepancies between what @feurig ordered, the BOM I used to make the parts order, and what's in the github repo. WOW that ESD is super small. I think 1206 was a bit overkill -- I think I would prefer 0805. It makes an easier "pull" when applying the solder paste. I'll give a better update once I've finished.

However, I think you did a great job on the repo itself, it was very thorough. I would look into using tags or branches for various versions, but otherwise just cloning the whole thing before I went into the lab worked out great. :D

Posted 2 years ago #
gbulmer
Moderator

soycamo - " You use the leftover X-ray sheets like you would kapton sheets. It's simply reusing existing materials."

Clever! Maybe I'll try local dentists to get some. Folks are usually extremly helpful when I explain I'm try to help kids make things.

Building the Orone-mini-S8A right now... it's in the oven!

BRILLIANT!

WOW that ESD is super small.
Yes. Sorry. I preferred that circuit to Siy's approach. It is a lovely little chip because it contains the USB termination, and ESD protection, without the pull-up resistor. So it is ideal for the STM32F2 and STM32F4 which contains the USB pull-up resistor on-chip. I had hoped the STM32F303 would have that feature too, but sadly not. AFAICT the ESD's only weakness is the small package.

" I think 1206 was a bit overkill -- I think I would prefer 0805. It makes an easier "pull" when applying the solder paste."
I started with 0805, but then went 1206 because my TekWizz chums thought that would be easier to make. Also local schools used 1206 for SMD beginners. So I have visions of 13yo's making their own "iPods" based on STM32F303 Orone-mini :-)

I still have the older design, which is exactly Maple-mini 0.6" header spacing and footprint, except for av+. That uses 0805. I might like to rework to use the ground-on-tab regulator. I might even be able to fit the extra pads on a longer board, but retain the 0.6" header pin spacing. What do you think?

However, I think you did a great job on the repo itself, it was very thorough.
Thank you very much :-)
Folks gave lots of very helpful advice and feedback, so I tried to do an adequate job. I feel it is a good example of the benefit of Open Source hardware.

I would look into using tags or branches for various versions
I was trying to follow a 'form, fit or function' rule for different versions.
So I thought, especially while it is 'in-flight', different pin-outs, different BoM, different track/space needed a different part-number, otherwise it might be a PITA.

If we can settle on a pin-out then I think there are still variants which need unique "part numbers", and hence aren't simply tags on the same branch.

IMHO track/space variation, e.g. 6mil vs 8mil, need to be a different part number because it matters when making the PCB. I also think BoM variation needs a different part number too. When the PCB is distinct for a BoM or manufacturing purpose it seems better to make them explicit part variants with their own part number. Then only use versions/revisions at the git level to track changes to what should then be 'the same thing'.

I like the 43 pin S8D/S8H which puts the LED pin 33, 'Vusb' after the polyfuse, and 'Vx' after the diodes, and USB_DISC on an internal pad. They all seem to be useful. I haven't put USB_DISC in-line with the pin headers because there is no space!

Does anyone want any changes to the pin out, or can I assume this is the pin-out which we are all (mostly) happy with?

I can see there is an argument for putting av+ back on the header, and by my part-numbering rules, that would be a variant. However, I don't think most people would mind which they use because it should have minimal impact on USB-powered form, fit or function.

Posted 2 years ago #
soycamo
Member

@gbulmer
I preferred that circuit to Siy's approach. It is a lovely little chip because it contains the USB termination, and ESD protection, without the pull-up resistor.
We were using this part for the Maple Bacon: STF202 which is slightly bigger than the one you are using but surprisingly similar, though the markings are STILL hard to read. Gosh dang I guess you can't get ESDs any bigger :(

That uses 0805. I might like to rework to use the ground-on-tab regulator. I might even be able to fit the extra pads on a longer board, but retain the 0.6" header pin spacing. What do you think?
I like that idea, I'm just not sure how time-consuming it will be to keep various versions of these boards around (unless that's not a factor).

Does anyone want any changes to the pin out, or can I assume this is the pin-out which we are all (mostly) happy with?
One thing that has bothered me that I wanted to fix on my own board is the USB-connected pins. After @feurig gave a class on using the Maple, a student came by a local gathering to explain that he thought he had bricked his Maple Bacon, only for @feurig to discover that it was because of using the pins connected to USB.
Soooo we should ax those. However, I'd like to hear arguments on keeping the pins around (or maybe making those pins be optional somehow?

Posted 2 years ago #
gbulmer
Moderator

soycamo - Thank you for the comments.

"We were using this part for the Maple Bacon: STF202"
That is the chip Siy uses for USB termination and ESD protection. AFAIK, based on a post be feurig, that is where Maple bacon took that part of its schematic.

For me, the NUF2042XV6 has a few advantages over the STF202.

To make my boards easier to make, I try to restrict them to SMD on one side only. I like this approach a lot (we used it on the OU's SenseBoard, but not fully). This makes DIY SMD simpler. For example, it lets folks use the SMD reflow 'skillet' technique. To make the USB socket connection more robust the USB socket is thru-hole. To get more space for SMD, and more space for user silk screen, the USB socket in on the non-SMD side, along with all of the users silk screen. So thru-hole USB sockets are my favoured approach.

The pinout of the NUF2042XV6 is easy to route to the thru-hole USB socket. The STF202 seems a better fit with SMD USB sockets.

Before doing the mini, I had been playing with a design for a 64pin LQFP STM32F103/STM32F4 board. STM32F2 and STM32F4 have USB pull-up resistors built into the chips full-speed USB peripheral, so I thought they could skip external pull-up resistor circuitry. Hence the NUF2042XV6 seems ideal; the pull-up parts can be omitted for STM32F4, and it should work correctly. However, it is more messy to use the STF202 with STM32F4; either the Vusb input signal can't be connected, and hence Vusb can't be ESD protected, or the on-board R-up mustn't be used. I was trying to minimise hacking on the USB libraries, which I assumed used the on-board R-up (I didn't check) so I chose to use the NUF2042XV6. AFAIK, the only 48pin STM32F4 is the STM32F401, and I haven't even looked to see if it would be easy to modify Orone-mini for it, so it isn't yet an import consideration.

There are a few other USB termination and ESD parts. For example the Semtech EClamp2522P looks perfect, though it is still 1.6mm x 1.6mm. The USB R-up is controlled by a separate pin, and isn't wired directly to Vusb. Unfortunately, the ground connection is a pad under the chip. I am not confident that a newbie (or me) could make that using simple SMD techniques, and I think it'd be awkward to diagnose the defect and fix it. I might change my view if SMD solder paste templates are easy to make.

"One thing that has bothered me that I wanted to fix on my own board is the USB-connected pins. After @feurig gave a class on using the Maple, a student came by a local gathering to explain that he thought he had bricked his Maple Bacon, only for @feurig to discover that it was because of using the pins connected to USB."
Yes that is a serious concern that I share.

"Soooo we should ax those. However, I'd like to hear arguments on keeping the pins around (or maybe making those pins be optional somehow?"
I don't want to remove the USB D+ or D- signals from the pin header because:
1. the Orone-mini is no longer Maple-mini compatible (on the pin-outs they share)
2. If the Orone-mini is used in a design which doesn't use USB, then those two pins can be used as normal I/O. It seems a shame to waste them. It seems like removing those pins penalises the smart to protect the ignorant (or worse), which is not a principle I like to encourage. I would hope the person who made the mistake learned something quite valuable, and that's one of the aims. My 64pin designs don't put USB D+/D- signals on header pins because I/O seems less precious than on the mini, and I am trying to cram into a limited number of pins.

To reduce the problem of the USB pins being used by accident, I am planning changes to the silk screen. The silk screen still needs improving anyway (ADC, PWM), so warning that two pins are USB seems to be a good improvement.

Anyone have an Eagle library part for a 'skull and crossbones" or a "Warning" sign?

I could put solder bridges in the USB D+/D- tracks so that the header pins are normally not connected. However, it is a small board and I'm trying to keep the ground plane as big as practical. Also I believe the USB signals should be simple and direct, with no 'stubs', and bridges with 'optional' tracks would create 'stubs'. So I am less enthusiastic about that than leaving those as they are. I am still open to persuasion.

Posted 2 years ago #
soycamo
Member

@gbulmer
For example the Semtech EClamp2522P looks perfect, though it is still 1.6mm x 1.6mm. The USB R-up is controlled by a separate pin, and isn't wired directly to Vusb. Unfortunately, the ground connection is a pad under the chip. I am not confident that a newbie (or me) could make that using simple SMD techniques, and I think it'd be awkward to diagnose the defect and fix it.
Looking at the footprint, I can see why you would hesitate with this part. I'm willing to give it a shot. If you're cutting soldermasks with a laser cutter, the difference seems negligible. If you're doing SMT by hand... well... :(

I could put solder bridges in the USB D+/D- tracks so that the header pins are normally not connected.
That seems preferable but yeah, that would be a feat. I suppose you could move the solder bridge to the other side? (Pretending that it makes sense electrically, I would.)

Another concern I have related to assembly is the position of the caps near the microcontroller -- I put way too much paste on the board so there were some shorts. My friend and I were able to clean up most of them except for around the microcontroller. It made rework pretty hard. I forked the repo and had started moving things around so I can show you what I think is a more optimal position for the caps, from an "I'm a novice at SMT" perspective.

I'm so happy you found the through-hole USB part.

Again, thanks for all your work!

Posted 2 years ago #
gbulmer
Moderator

soycamo -

For example the Semtech EClamp2522P looks perfect, ... Unfortunately, the ground connection is a pad under the chip. I am not confident that a newbie (or me) could make that using simple SMD techniques, ...
Looking at the footprint, I can see why you would hesitate with this part. I'm willing to give it a shot. If you're cutting soldermasks with a laser cutter, the difference seems negligible. If you're doing SMT by hand... well... :(

To be clear, I don't plan on changing to use EClamp2522P in the near future. I think that 'easy to make solder paste stencils' is a pre-requisite to using chips like that, with pads completely under the body.

I could put solder bridges in the USB D+/D- tracks so that the header pins are normally not connected.
That seems preferable but yeah, that would be a feat. I suppose you could move the solder bridge to the other side? (Pretending that it makes sense electrically, I would.)

Yes, if I did add solder bridges to connect the USB signals to header pins, they would be on the (Eagle) bottom copper, user 'top'.

"Another concern I have related to assembly is the position of the caps near the microcontroller ... It made rework pretty hard. I forked the repo and had started moving things around so I can show you what I think is a more optimal position for the caps, from an "I'm a novice at SMT" perspective."

Excellent point. I'd be very pleased to see that.
It feels like the design is stabilising, so I should also ask Chris Evans to have a hard look. When we did the old Orone board, he said that some caps were too close, and made assembly and rework hard. I'd forgotten about that, so thank you for raising that issue. Maybe making the board a mm or two longer would help create plenty of space?

I'm so happy you found the through-hole USB part.
I am very pleased that you like it too.
I was surprised how time consuming finding it was (carried by 5 of 6 distributors I use). However it feels like time well spent.
I do like 'over-engineered' sockets and connectors; they often take the strain :-)

Posted 2 years ago #
ala42
Member

> I was trying to minimise hacking on the USB libraries, which I assumed used the on-board R-up (I didn't check)
I do not use the chip internal pullup for the F4, as it requires to use PA9 to connect to VBUS, so PA9 can not be used for USART1. My USB port needs an external pullup.

Posted 2 years ago #
siy
Member

@gbulmer, sorry for delays, I was busy with other project and had no time to look here.

siy - Making the solder paste stencil using etching is a good suggestion. However, I am concerned on a few areas:
1. I would prefer to use a technique that is easy for hardware beginners to use without my involvement. I actually think more people have access to laser cutters than to etching equipment (in the UK). I think folks often use pre-coated photoresist which doesn't need developer. AFAIK, dry film photoresist uses a developer. Is that correct?

Well, both photoresists need a developer. Dry film photoresist uses water solution of sodium carbonate (~1% by weight). This one is quite safe by all means (it's widely used for softening water and other purposes, it even registered as food additive E500).
About etching equipment: for this purpose you don't need any special etching equipment other than you need for PCB's (etching solution is the same).
About laser cutters: they are quite rare here and tray with ferric chloride is much more accessible than laser cutter.

2. Might using cans as raw material a bit too challenging for schools? I would be worried that folks would cut themselves. Is there a good way to make handling the can easy and safe?

Cutting cans is quite safe operation. If you think this might present a danger for schools, they can wear gloves before cutting (I'd suggest to do so at least initially).

Using thin aluminium sheet with a nice rounded edge might be okay.

Yes, that definitely better especially because aluminium cans need additional processing before use: paint at both sides of aluminium sheet cut from can need to be removed with fine grained sand paper and to make sheet flat it need to be put into oven with some weight on top of it and then heated to about 220-250 degrees and slowly cooled. So, using ready to use thin aluminium sheet is definitely better. I'm using cans just because they are easy to find here (unlike aluminium sheet of required thinckness).

Posted 2 years ago #
gbulmer
Moderator

ala42 - "I do not use the chip internal pullup for the F4, as it requires to use PA9 to connect to VBUS, ..."
Thank you very much for that pearl of wisdom. That's a valuable improvement in my understanding.

"... so PA9 can not be used for USART1."
The person assigning functions to pins had an "off day" with that. That damages the ability to use USART1 for booting. IMHO that was a poor decision because USART1 is the only common boot peripheral across all the STM32F's :-(

"My USB port needs an external pullup."
Okay.

Conclusion: USB_DISC needs to be available on a pad as a signal to control R-up even on an STM32F4.

Posted 2 years ago #
gbulmer
Moderator

siy - Thank you for sharing the trick needed to flatten aluminium sheets from cans. There are likely a bunch of folks who will try that.

AFAICT most secondary schools in my part of the UK either have a laser cutter, or can get access to a laser cutter at a nearby school.
I don't know if they keep it well-enough aligned to cut stencils, so etching a stencil might be an important alternative.

Posted 2 years ago #
gbulmer
Moderator

I've pushed an update introducing Orone-mini-S8E:
https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0/Orone-mini-S8E-v0r001

1. Added 2pin 0.1" pitch header for USB 'DISC' and ground. This moved the 'DISC' pad off the 0.1" grid, used for all other pads, to find enough space to add the ground pin 0.1" away from it. This is intended to ease manual control of the USB pull-up resistor (R-up), and hence help folks to use the STM32F303's manufactured-in USB bootloader.

This change is physically incompatible with Orone-mini-S8D, and other Orone-mini's. Hence it is a new 'part number'

There are other small changes:
2. Increased clearance between STM32F and decoupling capacitors, responding to soycamo's feedback about assembly problems
3. Added 'usb only' warning to 'User top' (Eagle bottom) silk screen around USB pins, addressing soycamo's (and my) concerns about misuse of USB D+/D- as GPIO via header pins
4. Added 'ain' and 'pwm' identification for header pins on 'User top' (Eagle bottom) silk screen
5. Minor 'tidy-up' of 'User top' (Eagle bottom) silk screen
6. Increased separation between analogue ground (AGND) and other signals, intended to reduce the ADC noise signal, responding to ventosus' helpful ADC noise measurements (of course, this needs to be tested)
7. Updated 'README' to show which Orone-mini designs have been 'superseded', and hence are not likely to be updated and improved.

Posted 2 years ago #
siy
Member

@gbulmer, some time ago I wrote an article (http://we.easyelectronics.ru/evsi/izgotovlenie-trafaretov-dlya-naneseniya-payalnoy-pasty.html) about making stencils from aluminium cans where process described in details (with pictures). This article is in Russian, but I'm going to post (translated, of course) version of this article at Instructables. Can't promise more or less precise time frame because other project (current source for through hole plating) takes almost all my spare time.

Posted 2 years ago #
gbulmer
Moderator

siy - no rush. We'll be experimenting over the summer, and unlikely to try to show anyone this stuff before September.

Posted 2 years ago #
gbulmer
Moderator

I've pushed an update to Orone-mini-S8H:
https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0

This board uses 8mil track and 8mil clearance, hopefully enabling folks to use a wider range of PCB manufacturers than 6mil/6mil.

It includes all of the updates for Orone-mini-S8E:
1. Added 2pin 0.1" pitch header for USB 'DISC' and ground. Unlike Orone-mini-S8E, these pads are on the 0.1" grid, so veroboard could be used to make daughterboards, and have access to all signals. USB 'DISC' and ground pads are 0.1" apart, supporting the use of a 2pin 0.1" pitch header to connect them. This is intended to ease manual control of the USB pull-up resistor (R-up), and hence help folks to use the STM32F303's manufactured-in USB bootloader.
2. Increased clearance between STM32F and decoupling capacitors
3. Added 'usb only' warning to 'User top' (Eagle bottom) silk screen around USB D+/D- pins
4. Added 'ain' and 'pwm' identification for header pins on 'User top' (Eagle bottom) silk screen
5. Minor 'tidy-up' of 'User top' (Eagle bottom) silk screen
6. Increased separation between analogue ground (AGND) and other signals, intended to reduce the ADC noise signal
7. Updated 'README' files

This update also includes an Eagle CAM file, intended to generate Gerber files and drill files for oshpark.com

Finally, there are tiny tweaks to Orone-mini-S8E silk screen.

I think all of the feedback has been incorporated in these new boards. So I think the S8E and S8H variants are ready to be made.
A big 'Thank you' to ventosus and soycamo for making the earlier boards.

I intend to upload the PCB CAD to manufacturers at the weekend, or early next week, unless someone spots a defect. So all comments are gratefully received (before then B-)

Posted 2 years ago #
gbulmer
Moderator

I think I've got an Eagle problem with the silk screen rectangle containing the warning text 'usb only'.

This doesn't seem to be the right way to 'cut' text-shaped holes in the silk screen rectangle. I want some form of highlighted warning on the User silk screen, but AFAICT that approach does not work.

Posted 2 years ago #

RSS feed for this topic

« Previous 1…8910…13 Next »

Reply »

You must log in to post.