That looks pretty good. If I can get it together this weekend I may get some into the next run.
But the reason I am thinking about SFE is that I was going to make a handful of them in case anyone else wanted any... not sure if SFE would be cheaper for that purpose. Better to make some prototypes first, of course.
gbulmer
Moderator
I may have misunderstood the pricing, but, as soon as we want more than one PCB, it appears dorkbotpdx.org wins on price 'hands down'; dorkbotpdx.org make 3 PCBs for the $5/sq inch, BatchPCB charges by the sq. inch, and makes one PCB.
So if the PCB is 1"x1.5", then I believe dorkbotpdx.org is 1.5x$5 = $7.50 for 3 boards, $15 for 6, $22.50 for 9, $30 for 12 (do you see the pattern !-)
for the same 1"x1.5" PCB BatchPCB is $10 setup + 2x$2.50 (I believe BatchPCB round up to the nearest sq inch) = $15 for 1, $20 for 2, $25 for 3, $40 for 6, $55 for 9.
Please do check the prices, I may have misunderstood
i've received my boards from the first dorkbotPDX run that i participated in, and they're quite good.. probably not any better or worse than batchPCB (sparkfun), but i've never ordered boards from them before.. they're certainly no better or worse than any boards i've ordered from elsewhere (alberta printed circuits and sunstone). the boards i sent to pdx were similarly small about 1" x 2".
hmm.. looks like i can't edit my post, but full disclosure, in the run i participated in (oct 25), the boardhouse only sent one copy of the boards, so i received the first of the 3 within reasonable time, and i received an email from laen explaining the situation when the package went out (rather than when it arrived).
i did receive the other two within a week or two (timing was poor, laen was out of town on vacation for a week+).
so, there was a minor glitch, but it was handled openly and effectively.
gbulmer
Moderator
soundcyst - your feedback is really helpful, thank you.
This may sound a bit perverse, but the fact that it went wrong, but was properly handled makes me feel more comfortable about giving dorkbotPDX a try.
I have a little board I need to do, I'll try to get it done in time for the next run.
I made the JTAG adapter circuit on a breadboard to match the diagram, and get the same results as I posted above, here's an excerpt:
Info : JTAG tap: stm32.cpu tap/device found: 0x01b00037 (mfg: 0x01b, part: 0x1b00, ver: 0x0)
Warn : JTAG tap: stm32.cpu UNEXPECTED: 0x01b00037 (mfg: 0x01b, part: 0x1b00, ver: 0x0)
Error: JTAG tap: stm32.cpu expected 1 of 1: 0x3ba00477 (mfg: 0x23b, part: 0xba00, ver: 0x3)I double-checked that the circuit is correct using a multimeter. If I did that right, the only other possible difference is my JTAG adapter, since I'm not using the recommended one.
So, I just ordered the recommened Olimex ARM-USB-OCD adapter from SFE. Hopefully there really is some difference between that and the ARM-USB-TINY that I have, and the new one will work.
Well to make some more progess, despite not having a working adapter to test the circuit, I made a PCB layout for the JTAG adapter schematic that okie posted. Here it is:
https://github.com/adamfeuer/maple/blob/master/jtagadapter/maple-jtagadapter-brd.png
The Eagle board file (.brd) can be found here:
https://github.com/adamfeuer/maple/tree/master/jtagadapter
Or you can just clone my fork of the maple hardware repository using this command:
git clone git://github.com/adamfeuer/maple.git maple-hardware-adamfI replaced the SMT resistors okie put on with through-hole ones, since I didn't want to hand-solder SMT resistors. I also realized I didn't need two Maple-JTAG connectors, one for bottom and one for top - since if I solder the connector the bottom of the adapter board, I can go direct to the bottom of the Maple and the signals will match up.
Note the layout is probably horrible - this is literally my first PCB design. I can use some help - if you are interested in this, will you check out the .brd file to see if the layout looks ok? I followed the Sparkfun tutorial and looked at the layers in gerbv, and they look ok, but I may have made mistakes. I welcome help. You can tell me what to fix, or just clone my repo, fix it, tell me and I'll pull the changes back.
dorkbot is doing a run on December 6 - that's this coming Monday - so if you have changes, let me know by tomorrow afternoon Pacific Time. I want to get this board into their run. I am not sure if they are full, but I will submit it tomorrow evening.
Also let me know if you want a copy of this untested board and I'll make you one. Leaf Labs folks, I'll send you one too (if it works).
gbulmer, thanks for the pointer to dorkbot pdx.
gbulmer,
re: sounding ominous, I didn't mean it that way. I'm just frustrated that I can't get the JTAG adapter to work, and my different adapter is the only other difference between my setup and okie's that I can think of.
All I really want to do is debug this lwip TCP/IP stack I'm trying to port to Maple...!
this is in kicad?
have you double checked that you have the design rules set to match laen's requirements? he posted a .dru file for eagle, but i don't think you can load those in kicad.. for a board like this, the free version of eagle might be a better choice.
the layout looks a bit messy to me, and i'm not really sure what it says in the sparkfun tutorials, but in general, you want to keep things horizontal, vertical, or at 45 degree angles. 90 degree angles can result in manufacturing issues.. mitring the edges helps too.
other than that it looks fine.
gbulmer
Moderator
I find it very helpful to have a schematic with a PCB.
I'll repeat an observation from one of my PCB mentors: you are paying for a copper covered board. Copper is good. Rather than have most of it chemically removed to be disposed of, maybe to leach into the water supply, keep it on the board :-)
As soundcyst said, avoid right angle or tighter corners (including steps in tracks). PCB manufacture is a 'wet chemical process'. Try to think what happens when washing a strangely shaped object. Corners can trap etching chemicals, or be attacked by the chemicals from more than one side. Hence try to avoid sharp corners, and use mitres. Further, sharp corners can radiate electrical noise more strongly than rounded or straight tracks.
Also, set up the design rules; "Design rules are you friend" :-)
They help ensure the geometry of the tracks is within the capabilities of the manufacturing process. The tracks on that board look very, very narrow.
Also, the wider the track, the lower the resistance, and low resistance is good. Unless doing exotic design, it is always better to keep track resistance low.
I assume the picture was generated straight from the CAD, and it hasn't been changed in any way?
Some of the tracks seem to have little steps in them which suggest the parts aren't lined up.
If the CAD actually generates gerbers with those steps, the track corners will not come out as cleanly.
I'd recommend lining up the tops of the row of resistors, and routing with wide, wide tracks.
Also, most (all?) of those resistors are pulling pins to ground/Vcc.
You could save space by using a resistor array, e.g. SIL's:
http://search.digikey.com/scripts/DkSearch/dksus.dll
http://www.rapidonline.com/Electronic-Components/Resistors-Potentiometer/Resistor-Arrays/SIL-Resistor-networks/29581
one type has a shared common for all of the resistors. It might make the PCB smaller. Consider one for R1 to R6, and another for R7 to R9 (this one is less of a win).
Almost all of the signals on the top row of the 20-pin socket are common, joined together, with the actual signals on the lower row, on the opposite side. If either the 8 pin socket moved below (south) the 20-pin, or the 20-pin were rotated through 180 degrees, then the signal pins that need to be connected would have less 'wiring' in between, so it would be easier to connect because tracks can use both layers without obstruction, and easier to understand!
If you could use smaller resistors, e.g. a SIL, and move the socket, the resistors might be moved out of the space between the sockets, so the signals between the two sockets should be more direct. (Of course, there still needs to be some room for headers, so this might not work as well as I hope).
I tend to try to route the same signal on one side initially.
All of the connection between 9 of the pins on the 20-pin socket could be routed on one layer.
All the track between R1 to R6 (north end) could be on one layer.
All the tracks between R7 to R9 (south end) could be on one layer
After that, most of the signals will be on one side, so add a ground plane. That is a 'copper pour' made using a polygon, drawn around the board, connected to ground. Eagle (I think that's what you said you were using) will calculate it so that it doesn't touch any signals. So you could put one on both sides of the board. It will help reduce electrical noise, and reduce the amount of copper etched from the board.
My PCB mentor says that for best results, hatch large areas of copper (yes, I know what he said about removing copper) because this can help get more even etching in manufacture. Not critical, but does look more interesting :-)
I hope my comments don't put you off. I hope they help.
You must log in to post.