Beobot 2.0/Electrical System/PCB manufacturing

From ILabWiki

Create Gerber Files

First, we have to produce the manufacturing file outputs: Gerber files, which encode the following layers:

Top overlay (for labels): *.gto
Top solder mask: *.gts
Top layer (for copper): *.gtl
Bottom overlay (for labels): *.gbo
Bottom solder mask: *.gbs
Bottom layer (for copper): *.gbl

And, if you have inner layers:

VCC inner layer *.gp1
GND inner layer *.gp2

We do this by:

From the *.PcbDoc: File -> Fabrication Output -> Gerber Setup.
Go to layers tab and check the above 6 (or 8) layers like the picture below

Go to the Drill Drawing tab and un-check both the Drill Drawing Plots and the Drill Guide Plots
This procedure will also produce a Camtastic file (*.Cam). Save it as Beobot2_prototype1_CAMtastic.Cam.
From the Camtastic file: File -> Export -> Gerber. Create a folder named "Gerber" and store them there.

Create Drill File

We also have to create a drill files for the holes in the board:

From the *.PcbDoc file:

File -> Fabrication Output -> NC Drill Files.
Change the "Generate Board Edge Rout Paths" to 10 mils.
This procedure will also produce a Camtastic file (*.Cam). Save it as Beobot2_prototype1_CAMtastic2.Cam
From the Camtastic file: File -> Export -> Save Drill ...
Select layer L1. Ok.
From the Write drill menu: save the cam.drl file to the Gerbers folder

Check the files

Zip all 7 (or 9) files to a single Zip file. Name it: beobot2_prototype1.zip We now ready to send the Gerber files to be checked for correctness at freedfm.com

Go to the website.

Fill in your email and upload the Zip file. It will go to another page and it will ask for the following information:

Design File information. The outer layers should be easy to add. There is a table ("Click here to see a table")
For the inner layer VCC and GND: *.gp1 and *.gp2, select inner layer. Make the polarity both negative. Select layer 2 for *.gp1/GND and 3 for *.gp2/5VCC.
Fill in Part Number as B2P1
No on ITAR (for exporting permit to foreign countries, i think).
Solder mask sides: both
Silk screen sides: both
X,Y dimension: 12 by 5 inch.
Fill in other order related info.

Here is a snapshot of the FreeDFM page: