Uploaded new Orone-mini-S8C-v0r001 a few minutes ago.
This replaces C1, 100uF and 16V, which was a 1206 case with a 2917 (metric 7343 case), about 7x larger. This should be significantly easier to source and lower cost.
There are new BoMs.
Community rework of standard maple and maple mini.
(181 posts) (14 voices)-
gbulmer
Moderatorbobricius - Interesting suggestions, however part of the goal is to make the boards straightforward to DIY.
AFAIK all uSD sockets are Surface Mount Devices (SMD). The only side with enough space (about 14mm x 21mm, minimum) is the opposite side to the current surface mount components. Putting any Surface Mount Devices on the bottom-layer, which is the 'top' of the board for the user, causes it to be harder to make using DIY SMD techniques. So I am unlikely to do that.
A cr2032 battery is much wider than the pin headers, so it is too big to fit unless it stands vertically. The only vertically mounted cr2032 battery footprint I have is through hole, and it is difficult to see where it might fit. I think it might take a lot of work.
Some of Siy's boards have a battery holder. Have a look at those.
A simple approach for Orone-mini would be to make a 'daughter board' to carry those two parts. The PCB would be a similar size, and it would connect to the Orone-mini pin headers. Once the boards are tested, I might be interested in doing that. I might add a 32KiHz crystal too for the Real Time Clock.
However, my priority is to get the existing Orone-mini boards working first.
Of course, there is nothing preventing you from making those changes.
Posted 2 years ago # -
gbulmer
ModeratorI've committed to github a slightly tweaked version of Orone-mini-S8C.
There are two signals which are not available in Maple-mini's header pins. One controls the user LED. The other controls the USB pull-up resistor (USB Rup).
Orone-mini-S8C adds a thru-hole pad to the USB Rup signal, positioned on the 0.1" grid. I've also moved the user-LED pads to coincide with the 0.1" grid. So anyone making a daughterboard, even from matrixboard or strip board (Veroboard) could get access to those signals. Though you would need to remove the User LED. However, if you want access to the User LED signal, then its probably a good idea to avoid having the User LED drawing power from the pin anyway.
I could have tried to position access to these signals in different places, but one would have required part of the silkscreen text to be smaller, and the other would have cut the underside copper pour into smaller pieces, reducing its effectiveness as a heat sink for the regulator. However those are still options to consider, so I'm interested to know if anyone feels they are of use.
Posted 2 years ago # -
gbulmer
ModeratorI've moved the LEDs around, put the User LED signal (33) onto a pad aligned with the top row of the pin headers (so this could be a 21 pin header if you want to get at it from a breadboard). The signal controlling DISC is not on a pad aligned with the header pins, but is on a pad aligned to the header pins' 0.1" grid, so it is accessible from stripboard/Veroboard.
ventosus commented "have to increase all the annular rings of plated through holes to at least 0.125mm to get the design through the online DRC at eurocircuits.com".
So I have increased the annular rings around pads and vias (defined in the DRC->Restring->Pads Minimum and ->Vias Minimum) from OSPark's minimum 7mil to 10mil (which is slightly larger than 0.125mm x 2). Hopefully this gets through their checks.I think I'm done, unless someone identifies some defects.
Edit: It's at https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0Next stage is get PCBs made.
I am reasonably confident this will pass the Eagle DRU file for OSHPark (after Laen's feedback).
I think it will pass the Design Rules for Seeedstudio, PCBCart, and Spirit Circuits by substituting one of the alternative USB-Mini footprints from the Orone-mini-v0/Library/USB-Mini-Molex.lbr. I intend checking with Spirit Circuits and Seeedstudio.Of course, I'm very interested in feedback.
Posted 2 years ago # -
gbulmer
ModeratorMoved the BoM files to their own directory as all the S8 boards use the same parts https://github.com/gbulmer/openstm32hw/tree/master/Orone-mini-v0/Orone-mini-BoM-v0r001
I did an initial part costing using prices from RS and Future (in the .csv) and parts for an STM32F103CB-based board, or an STM32F303CC would be under £10 (GBP) ex-VAT (without PCB). However, some of the parts come in minimum-order-units of 10, 25, 50 or 100 (didn't record that I'm afraid). So the cost for one board would be more.
EDIT: For anyone thinking of making a PCB in the next couple of days: you might want to wait until the next revision, which I hope to have done by Monday evening (GMT). I am working through the CAM job, aiming to ensure everything looks reasonable.
Posted 2 years ago # -
I have a first running Orone Mini S8A...
Soldering was done with the hot-plate reflow method and after reworking the ESD package with two magnifying lenses in series I even got a working USB connection, put the maple mini bootloader on there via serial and run a sketch to compare the standard deviation of the ADC readout of a hall-effect sensor on Pin 3 to the original maple mini.https://dl.dropboxusercontent.com/u/46882396/orone_bottom.jpg
https://dl.dropboxusercontent.com/u/46882396/orone_top.jpg
https://dl.dropboxusercontent.com/u/46882396/orone_adc.pdfPosted 2 years ago # -
gbulmer
Moderatorventosus - Brilliant! Very helpful pictures too. Thank you very, very much.
Where did you get the board made? Was it eurocircuits.com? What was the annular ring size? I'll try to ensure the board meets it.
What was the problem with the ESD package? Was it just too small or something else?Thank you very much for doing the ADC test too.
Lots of food for thought! I'd very much appreciate feedback!-)
Posted 2 years ago # -
No, I have to thank you for the routing work...
Yes, at eurocircuits.com, I had to increase the via diameter to 40mil. With the 0.5mm drill size, this gave me an annular ring of 0.128mm, this was enough to reach their required minimum of 0.125mm. I also had to use the two-hole version of the USB connector, as they don't accept overlapping holes.
Yes the ESD package is small, but the problem was more a lack of skill ;-) The LQFP48 and the ESD package were my first 0.5mm pitch packages ever and I got too much solder on the pads with my self-cut mylar stencil and some legs bridged as a result which was hard to see on the ESD package as it's legs have rather short wings. I'll just have to get me a decent clock worker lens...
I'll try to do some more tests for all ADC pins and check for connectivity on the SPI, I2C and USART ports in the next days...
Edit: I got the parts from Digi-Key for 16.88€
Posted 2 years ago # -
gbulmer
Moderatorfolks - It might be worth looking at the S8D variant which uses the much larger, and much cheaper capacitor for C1 (at RS, the larger-case capacitor is 30p vs over £3).
Like the more recent board designs, it brings out two extra signals onto the 0.1" grid; signal 33 which drives the LED is at an edge, and 'DISC' which pulls up the USB-resistor can be reached 'in the middle'. So for folks who aren't intending to use the board with USB once its programmed, this could give two extra signals, and one for the rest of us. The LEDs are also at an edge so they should be easier to see if you 'bury' the board inside something. Though the LEDs are small 1.8mm ones. (I should have a look at the board to see if I can find a better place so that 5mm LEDs can be used, but that isn't a priority.)
The ADC results measured by Ventosus is causing me to slightly adjust the ground plane and a few tracks to get better separation of the ADC tracks from the rest of the board, and better ground routing. I don't know that it will make a measurable difference, but there is just enough space to do it, and it seems worth the effort.
I am also about to push a variant made using 8mil/8mil track and space. Laen is happy with 6mil/6mil for OSHPark. However Laen has done some tests on some low-cost PCB makers. Lean found they some problems with their 6mil/6mil capability, and so recommended using coarser 8mil/8mil track and space rules so that low-cost services are able to make the board reliably.
When I have done that board (I will push by this evening - Edit: just got home, unlikely I'll push tonight), I intend to put both the 6mil/6mil and 8mil/8mil through Seeedstudio. So I will have some spare boards when that comes back. The 8mil/8mil board is 0.1" longer than the 6mil/6mil PCB, the same width and same 0.8" pin-header row-spacing.
Posted 2 years ago # -
gbulmer
Moderatorventosus - "I had to increase the via diameter to 40mil. With the 0.5mm drill size, this gave me an annular ring of 0.128mm, this was enough to reach their required minimum of 0.125mm. "
Okay.
Due to your post a few weeks ago, I have made the annular ring 20mil bigger than the drill, which gives a diameter of:
drill = 0.5mm (19.69mil) + 2 x DRC->Restring-Pad-Minimum (10mil, 0.254mm),
= 19.69mil + 20mil = 39.69mil
= 0.5mm + 2x0.254mm = 1.008mm"I also had to use the two-hole version of the USB connector, as they don't accept overlapping holes."
Due to your earlier post, I am now using that footprint by default.
I intend to generate the Gerbers+drill file for a few PCB makers so that folks without Eagle skills can successfully get boards made.
The variation is due to the differing ways PCB manufacturers use to get the board outline.Ventosus, I notice the bottom silk screen is missing. Is that because the eurocircuits service only gives one silk screen, or is it because I didn't provide the CAM file?
Posted 2 years ago # -
gbulmer
ModeratorFeurig/Folks - would you either push your BoM to github, or post on gist or pastebin and post a link here and I'll copy?
I am using a csv file for the BoM, Tab-separated would be okay too; they are portable across spreedsheets apps. Some of the distributors can upload a spreadsheet to fill the shopping trolley/basket, making it easy to create the order.
Posted 2 years ago #
Reply »
You must log in to post.