Protel Gerber Export for CSE Protomat

Setting up the rules

1. Electrical->Clearance: Minimum clearance should be 0.2mm
2. Routing->Width:
   • Minimum width should be 0.2mm for all layers. NB: this is very fine and will be difficult for beginners to solder/rework, 0.25mm is easier for most people
   • Maximum can be any width desired.
3. Routing->Routing Via Style:
   • Minimum via pad diameter is 0.7mm
   • Maximum via pad diameter is as large as desired
   • Minimum via hole size is 0.4mm (smaller by special request)
   • Maximum via hole size is as large as desired
4. Manufacturing->Minimum annular ring should be 0.15mm
5. Manufacturing->HoleSize:
   • Minimum hole size should be 0.4mm (smaller by special request)
   • Maximum hole size may be as large as desired
6. Placement->Component clearance
   • Component clearance settings as desired

General PCB design

1. It is generally a good idea to use a seperate layer for the board outline. I use Mechanical Layer 1 with four tracks (for a square PCB). This is then exported as a separate gerber file later on.

Exporting the gerber files

1. Open the PCB file to be manufactured
2. Select File->Fabrication Outputs->Gerber Files from the menu
3. Select the general tab:
   1. Select millimeters
   2. Select 4:3
4. Select the layers tab:
   1. Check "Plot" for the copper layers to export (for a two layer board this will be "Top Layer" and "Bottom Layer")
   2. Check the board outline layer to be exported (e.g. "Mechanical1" or "Keep Out Layer")
   3. Make sure no layers are mirrored
   4. Check the "Include unconnected mid-layer pads" option
   5. Ensure no unwanted mechanical layers will be added in
5. Leave the "Drill Drawing" and "Apertures" tabs at their default settings
6. Select the "Advanced" tab:
   1. Click "Keep leading and trailing zeroes
   2. Click Reference to absolute origin
   3. Un-check Optimize change location commands
7. Click OK. Camtastic should open. Check that it looks reasonable.

Exporting the drill files

1. Open the PCB file to be manufactured (or go back to it using the tabs at the top of the window if it is still open from exporting the gerber files)
2. Select File->Fabrication Outputs->NC Drill Files from the menu
   1. Select "Millimeters"
   2. Select "4:3"
   3. Select "Reference to absolute origin"
   4. Select "Keep leading and trailing zeroes"
   5. Un-check "Optimize change location commands"
   6. Click OK.
3. CAMtastic will appear and a window will open.
4. Click "Units"
   1. Change Integer to "4"
   2. Change Decimal to "3"
   3. Change Units to "Metric"
   4. Change Type to "Absolute"
   5. Change Zero Suppression to "None"
   6. Click OK
5. Click OK

Sending the appropriate files

1. Project outputs for PROJECTNAME/PCBNAME.TXT
2. Project outputs for PROJECTNAME/PCBNAME.GBL
3. Project outputs for PROJECTNAME/PCBNAME.GTL
4. (If you included other copper layers) Project outputs for PROJECTNAME/PCBNAME.G11, etc.
5. (If you included mechanical layer 1) Project outputs for PROJECTNAME/PCBNAME.GM1
6. (If you included the keep out layer) Project outputs for PROJECTNAME/PCBNAME.GM1