gbulmer,
I got the Orone Mini S8H boards back from OSH Park today, they look great!
http://imgur.com/2HrJNU5
http://imgur.com/mXYqEl3
I haven't ordered parts yet, but I hope to do the BOM and order today or tomorrow. After that, I'm going to cut a solder mask stencil for it.
gbulmer
Moderator
Adam - Thank you very much for posting the pictures. That is very, very helpful.
Also thanks for getting the S8H variant made. That uses 'slacker' 8mil track/space which should be easier to make and more robust.
I'm thrilled. Those OSHPark boards do look very good.
I have been very impressed by the PCBs I've had made in the past. Also OSHPark are good value for prototypes; I SWAG it'd about $50 + P&P to get 10 panels from Seeedstudio of that quality (gold plated, and non-green solder mask), vs $48 for 12 PCBs from OSHPark including P&P, and you only need spend $12 to get 3 PCBs from OSHPark.
It looks like the user-side silk screen came out reasonably well using OSHParks default Eagle to Gerber processing. Getting that right was one of the main goals of changes on the later revisions.
One thing I can't quite make out from the pictures is are the vias 'tented', i.e. covered with the purple solder mask? Also, does that allow the silkscreen to print reasonably well when it prints over them?
If that is okay, then folks can just submit the Eagle PCB .brd file, and it looks like everything might 'Just Work' (TM:-) !
There is the small problem of joining the two drill holes to form the slots in the PCB for the USB socket lugs. Maybe I should make some with 'un-plated slots' to see how well the socket is attached? It'd be nice to have a PCB with no 'post-processing', i.e. it arrives from the manufacturer and is ready to solder.
I'd like to know if the 1.8mm 'rectangular' LEDs are easy to get from your favoured supplier (I chose to use them to save space, and I have a bunch as they fit on 0.1" pitch veroboard very nicely).
I'd very much like to know how making the solder paste stencil goes, and how well it works.
I have access to laser cutting, and so a solder paste stencil might make the board feasible as a 'second SMD project' (I think its worth doing something less demanding to get the process understood first :-).
Thanks once again for your help and feedback.
It feels like we have several 'release candidates' in this series of boards, with the more recent variants giving a bit of useful support to STM32F303 with its manufactured-in USB bootloader.
I guess one finishing touch is to add the Open Source Hardware logo?
gbulmer,
None of the vias are tented. Maybe they would be if I sent Gerbers processed with your custom CAM job? I'll try that on the next batch.
Since the vias aren't tented, the silkscreen text just prints across the holes. It looks fine to me - I can read everything.
The USB connector attachment "slots" did not come out as slots - they are just plated holes close together:
I haven't looked at the connector, but I'm guessing it won't go into those without some modifications? I have a Proxon Micromot (small electric drill) with some small bits, maybe that will work to drill out the slot?
If we do need slots rather than holes, maybe we can change the board outline? OSH Park says:
"Internal cutouts are allowed and supported. Draw them on your board outline layer."
http://oshpark.com/pricing
As for the rectangular LEDs, I was able to find something close to what you specified:
Green square LED
http://www.digikey.com/product-search/en?x=-1281&y=-71&lang=en&site=us&KeyWords=754-1373-ND
Yellow square LED
http://www.digikey.com/product-search/en?x=-1281&y=-71&lang=en&site=us&KeyWords=754-1376-ND
I picked a yellow LED since I have bad color vision and red is too similar to green for me.
I'm willing to make a change to board outline to get the slots, and run another job with OSH Park... what do you think?
Regarding the solder mask stencil- I read this article recently:
http://pmonta.com/blog/2012/12/25/smt-stencil-cutting/
And so got a Silhouette Cameo stencil cutter:
http://www.amazon.com/Silhouette-Cameo-Starter-Bundle-Cutter/dp/B007R83VKE/
It seemed like the fastest, least expensive way to go. But I haven't tried it yet - probably in the next couple of days. I'll let you know if it works.
Regarding the Open Source Hardware logo, yeah that would be nice to have too. There is an Eagle library for it here:
I'll take a shot at putting it on the back next to the board name.
gbulmer
Moderator
Adam - "None of the vias are tented. Maybe they would be if I sent Gerbers processed with your custom CAM job? I'll try that on the next batch."
Okay, they aren't 'tented'. I can see in the photo the vias are covered with solder mask, but it hasn't covered the hole. So I think the CAD is okay and the CAM is okay; but the solder mask isn't 'stiff' enough to cover the hole.
The vias use 0.5mm drills. I picked that size to increase the number of PCB manufacturers. It could be reduced to 0.4mm, which would be within the OSHPark design rules. A smaller hole should improve the silk screen.
The user-side silk screen that will suffer is on pins "29", "30", "19", "Vin" and one of the "pwm" labels.
I'll have a look to see if I can improve the placement of via or silk screen.
"I haven't looked at the connector, but I'm guessing it won't go into those without some modifications?
Yes. I think a craft knife or scalpel will cut the PCB material between the two holes.
I have a Proxon Micromot (small electric drill) with some small bits, maybe that will work to drill out the slot?
That should work if the bit is small.
"If we do need slots rather than holes, maybe we can change the board outline?"
There is a library for the Molex USB mini socket at github:
https://github.com/gbulmer/openstm32hw/blob/master/Orone-mini-v0/Library/USB-Mini-Molex.lbr
It has three alternative footprints defined for the same USB socket. One has two holes, and is the default, another has slots, and another has overlapping drill holes. Alternative footprints can be substituted on the board. In theory, there should be nothing else to do.
The down-side of slots at OSHPark, and AFAIK most PCB makers, is slots are not plated through. I was concerned that the socket would be better anchored by solder-adhesion with plated drill holes.
"I'm willing to make a change to board outline to get the slots, and run another job with OSH Park... what do you think?"
It would be good to test slots to discover how well the socket is held. However I think you've already helped us all, so please don't worry unless you need more boards.
Those LEDs look fine. I should add alternative part numbers for yellow or amber LEDs to the BoM to give folks flexibility.
Thanks for the link to using the Silhouette Cameo stencil cutter. I haven't seen that before. The results look very good.
I can add the OSH logo. Do you know, does it matter which of the three are used?
Garry,
The user-side silk screen that will suffer is on pins "29", "30", "19", "Vin" and one of the "pwm" labels.
I'll have a look to see if I can improve the placement of via or silk screen.
They're all totally readable on my board, even though they're not tented.
There is a library for the Molex USB mini socket at github:
I'm using that. How do I change from one of the footprints to the other?
Not knowing about the footprints, I did a version of the board (in a git branch) that has overlapping drill holes, and it looks like that will work.
I can add the OSH logo. Do you know, does it matter which of the three are used?
I think whichever you like best-
Garry,
Ok, I figured out how to use the other connector footprint (package) - right click on the symbol on the schematic, choose Package.
I added another 2 drill holes to each "slot" in the overdrill package style to make the slot neater. If I make more boards I'll try this out. I'll also send you a pull request for it.
gbulmer
Moderator
Adam - "I'm using that. How do I change from one of the footprints to the other?"
In Eagles board editor, the icon below 'Add' is 'Replace'.
Select 'Replace', and the part selection dialogue appears as if 'Add' was selected.
Find the right part, "USB-MINIBTH-ODRILL", then click on the USB socket on the board.
You won't see much change, except the holes for the lugs change to three overlapping drill holes.
I believe it obeys the design rules which Laen of OSHpark suggested, but it has not been tested. It should give a slot which is 'finished', and platted through.
Many PCB manufacturers might refuse to do this footprint, hence it isn't the default, but Laen said OSHpark's supplier will do it.
Edit: overlapped with your post.
Garry,
I got email back from Laen who said OSH Park can do slots of any width down to 0.035" wide.
I changed the CAM job to put the milling layer onto the board outline gerber, and it looks like it can mill nice looking slots. I'm going to try this out if I make more boards.
gbulmer
Moderator
Adam - One of the three alternative footprint for the Molex USB-mini socket, in the library on github has milled slots for the socket lugs.
The Molex socket drawing recommends a slot width of 0.7mm (+/-0.05mm)
http://www.molex.com/pdm_docs/sd/565790519_sd.pdf
However, Seeedstudio (and folks using the same PCB service) offer a minimum of 1mm wide slot, so 1mm is the width of the slot in the existing alternative USB-mini footprint. I'm aiming for board CAD which is makable by different manufacturers, so I am reluctant to proliferate board CAD or package footprints. I'd prefer to use the larger design rules, like 1mm width.
However, we could encapsulate the OSHpark specifics into a fourth USB-mini socket footprint within the part library. There is already the overlapping drill holes package for OSHpark so slots is plausible.
I'd like to try the 1mm wide slot though, to understand how well it works. If it works well enough, it would make a reasonable general manufacturable board, ready for use without further finishing.
gbulmer
Moderator
Based on the tests by ventosus:
http://forums.leaflabs.com/topic.php?id=10410&page=7#post-25373
the noise on ADC readings is higher on Orone-mini, which only brings the digital power regulator out to a header pin.
I removed the connection to av+ to avoid damage to the regulator when drawing too much current, usually running above 6V.
Should av+ be put back on the header pins, with the analogue regulator reconnected to av+, to try to get lower noise ADC?
First version of my STM32 stick with OLIMEX UEXT
Overall dimensions much bigger than I initially expect :(
http://sardravce.sk/tuke/smartstickSTM32.brd
http://sardravce.sk/tuke/smartstickSTM32.sch
-no external power (every phone charger have 5V and USB)
-cute shaped design
-two types of 3V regulator
-cr2032 battery bottom
-rgb led
-usb ESD or resistors
Todo:
...I see now little crystal bug
-check uext pinout
-check all :)
-check again
-add labels, silkscreen
-add testpoints for SWD or connector
Here's some pictures of my first try at cutting a solder paste stencil using Peter Monta's gerber2graphtec program and a Cameo Silhouette cutting plotter:
Overview:
http://i.imgur.com/FPpXKo4.jpg
Closeups:
http://i.imgur.com/6ZDHb0T.jpg
http://i.imgur.com/KZyc3nu.jpg
The overview shot looks good - the 1206 pads are square and well cut. But the fine-pitch pads for the STM32 are not looking so good.
These are with default settings, the default cutting knife, and 3M PP2500 (4 mil) film. I'm going to try tuning gerber2graphtec's options so I can get the fine pitch pads to all come out straight. I might need to use a different cutting knife too.
gerber2graphtec: https://github.com/pmonta/gerber2graphtec
gbulmer
Moderator
Adam - I think Chris Evans laser-cut solder paste stencils look better than those. However, I'd certainly like to see how good you can make the stencil with your much lower-cost stencil cutter. That stencil cutter is about 1/20th the cost of the laser cutter, and gets into my price range :-)
You must log in to post.
