Jefferson Lab > Engineering > EECAD
Privacy and Security Notice

EECAD Guidelines & Standards

How to generate Gerber data & NC Drill information from PCAD

Generating Drill Data

  1. Go into .Print. and select Drill symbols. Set your symbols by either selecting .Auto. or manually assign the symbols.
  2. Select N/C Drill from the pull down menus; Select Tools, then auto-assign.
  3. Select N/C Drill Format and make sure the following boxes are checked: Inches, ASCII none, Leading.
  4. Verify output directory.(you should not be writing files to the \Program files\P-CAD 2001 directory)
  5. Generate your data.
  6. Open Explorer of File Manager and look for a file located in \Program files\P-CAD 2001 \Utils called drilltab.exe (Drill table generator for your fab drawing). Double click to start it. When it kicks up the results, set layer to FAB and set your text font. It is also recommended that you add a column in your table for tolerance information.( +/-.003 all holes < .055, +/-.004 .055- , .125, +/-.005 .125 > )

Generating Gerber data

  1. Verify your file set up once you select .Gerber out.. Files should be named with the following file extension:
    • .TOP = top side signal layer
    • .BOT = bottom side signal layer
    • .BSS = bottom side silk screen (where applicable)
    • .TSS = top side silk screen
    • .TSM = top side solder mask
    • .BSM = bottom side soldermask (only needed if bottom side pads differ from top side pads)
    • .GND = internal ground plane (where applicable)
    • .PWR = internal power plane (where applicable)
    • .IN1 = internal signal layer (where applicable. Additional internal signal layers should be numbered accordingly)
    • FAB = fabrication drawing that tells the fab house board thickness, ozs. of copper desired, drill information and size of the board.
  2. Select Aperatures, then select Auto Assign
  3. Select Gerber format. Make sure that the following boxes are checked: Inches, 5.3 format, Include Aperature definitions (as RS-274-X mass parameters)
  4. Make sure your output path is your current directory (or whatever directory you want it to go to) and not the \Program files\P-CAD 2001 directory!
  5. Generate your data.
  6. View and verify your data using a Gerber viewer like Camtastic! (supplied via the network)
  7. Create a zip file and copy your gerber and N/C drill files into it. This is what you will send to the board house.

Return to EECAD Guidelines Home