Gerber file generation from Cadence Layout Plus (tailored for 4PCB.com)

After completing all steps of board layout including board outline…

Prepare to run the post processor

1. Go to Options -> Post Process Settings
2. Set “Batch Enabled” for all layers that you would like fabricated (typically for a 2 layer board, this is: TOP, BOT, SMT, SMB, SST, SSB, FAB, and SPT, SPB if you would like a solder paste stencil (you’ll need to make sure all of your parts have solder paste outlines defined or else this is useless). Here’s an overview of what each file is:

TOP: Top copper - all copper traces on top layer of board.
BOT: Bottom copper - all copper traces on bottom layer of board.
SMT: Solder mask top - Negative image of where solder mask is applied to top layer of board.
SMB: Solder mask bottom - Negative image of where solder mask is applied to bottom layer of board.
SST: Silk screen top – Screen printing that appears on top layer of board.
SSB: Silk screen bottom – Screen printing that appears on bottom layer of board.
FAB: Fabrication - Board outline and hole info, used strictly for board outline feature.
SPT: Solder paste top – Image of where solder paste should be applied to the top of board, used to make a negative stencil.
SPB: Solder paste bottom – Only needed if surface mount components will be mounted to the bottom of the board, an image of where solder paste should be applied to the bottom of the board, used to make a negative stencil.

Run the Post Processor to Generate Gerber Files

1. Go to Auto -> Run Post Processor. Gerber files and thruhole.tap files are generated. Make sure you save old gerber files before running the post processor if you want to keep them.
2. Your project directory contains all files, arrange by date modified to see the most recent additions of your gerber files.
3. Take files *.TOP, *.BOT, *.SMT, *.SMB, *.SST, *.SSB (if you have silkscreen on the bottom layer), *.FAB, thruhole.TAP, and a text file with file descriptions and zip them all together in one folder.
4. Go to your board house’s website and upload the zip file to their Free DFM (Design for manufacturability) machine. Go through their file ID dialog and board spec page. You should get DFM results back soon (not immediately) if you upload during their business hours. USE THEIR CUSTOMER SERVICE IF NEEDED, it’s good and they don’t mind “stupid” questions.
5. After clearing up all DFM problems, place your order. If you’re using the $33 each section of 4pcb.com, go to 33each.com and upload your zip file there. In the comment section when you are placing your order, write STUDENT to allow a minimum order of 1 board (and you get a McDonald’s gift card with your order too!).
6. If you'd like to make a solder paste stencil, use the *.SPT and *.SPB files (typically just the *.SPT file) to order the stencils. You can also convert the files to DXF's and use one of the LaserCAMM's around to cut out a template. Experience has shown that 0.002" adhesive back mylar film works well. You can order it for cheap from McMaster.com.

-- JohnUlmen - 15 Sep 2008