BatchPCB-howto

From SPCoast

I use the following workflow to upload and order boards from BatchPCB

First, set up EAGLE and customize it's environment and behavior

1. Obtain the latest version of Cadsoft's Eagle program
2. Download a .dru rules file that encodes BatchPCB's requirements. I use a 10-mil version of SparkFun's DRU file Put a copy of the file (with the .dru extension) in the Eagle program's dru directory (on my Mac, this is at Applications/Eagle/dru/SparkFun10mil.dru )
3. Download a .cam processor definition file that you can use to create "gerber" and "drill" files for BatchPCB. I tweeked the SparkFun one to use additional layers and not generate a mill file, you can download JMP-gerb274x.cam and put it in Eagle's cam directory (Applications/Eagle/cam/JMP-gerb274x.cam)
4. ON MACOS and Linux: I use a homegrown shell script   that will archive old files and collect things for BatchPCB and put it somewhere where you can find it easily - I put it in my $HOME/bin subdirectory and make sure my PATH references it as makeboard.
5. Tell Eagle to use the rules file when autorouting: (Tools)->(DRC), (Load) dru/SparkFun10mil.dru

Second, go over to BatchPCB's website and create an account.

Once you have set up your EAGLE environment and a BatchPCB account, you can focus on creating boards:

1. Create a schematic and associated PCB layout using Eagle Lite (there are many good tutorials on the web - I'll bet you can't tell that I particularly like SparkFun's site :-) I tend to give the files version numbers in their name as well as in text on the board - and increment the version number whenever I actually fab a board, so I have filenames like CANBusProtoboard-1.0.sch
2. When you have a PCB you like (AND HAVE CHECKED by printing 1:1 and making sure all your components fit), use the CAM Processor to generate the files that the Board house needs:
   1. (File) -> (CAM Processor), (File) -> (Open) /Applications/EAGLE/cam/JMP-gerb274x.cam
   2. (Process job)
   3. dismiss the CAM Processor window - it will have created a bunch of files in the directory your schematic and pcb files are in
3. I then use the helper script in a terminal window, giving it the base name of my project, but you can manually make a tar file out of the gerber and drill files and compress it with gzip if you like:
   • plocher@mymac> makeboard CANBusProtoboard-1.0
     This will create a subdirectory with a bunch of files in it:
     • CANBusProtoboard-1.0.GBL  - Gerber Bottom Layer copper traces
     • CANBusProtoboard-1.0.GBO  - Gerber Bottom Silkscreen
     • CANBusProtoboard-1.0.GBS  - Gerber Bottom Soldermask
     • CANBusProtoboard-1.0.GTL  - Gerber Top Layer copper traces
     • CANBusProtoboard-1.0.GTO  - Gerber Top Silkscreen
     • CANBusProtoboard-1.0.GTS  - Gerber Top Soldermask
     • CANBusProtoboard-1.0.TXT  - Excellon Drill File (for all the holes that need to be drilled into your board)
   • the above "gerber and drill" files are collected and gzip'd into
     • CANBusProtoboard-1.0.gerbers.tar.gz
   • while the Eagle files
     • CANBusProtoboard-1.0.sch and
     • CANBusProtoboard-1.0.brd
   • are put in
     • CANBusProtoboard-1.0.eagle.tar
4. You can now use your BatchPCB account to (Upload a New Design). I use the basename of my project, with a version number, for the name of the design, e.g., "CANBus Protoboard 1.0" I then (Browse) to the eagle directory created by the makeboard script, then select the ...gerbers.tar.gz" file. Click (continue) a couple more times and your board design will be uploaded and validated by BatchPCB's automated system.
5. If it passes, you can then order 1 or 100 or more of your board - though I'd recommend you start simple so you don't waste money making coasters :-)
6. Finally, you can upload the ...eagle.tar file to your blog or website so that others can build on your efforts as they explore the world of making their own boards.