== 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
[[Image:Gerber_Setup.JPG]]
* 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 [http://freedfm.com 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:

[[Image:FreeDFM.JPG]] 

We wait for the results to come back via email.


Back to [[Beobot_2.0/Electrical_System| electrical system]]
[[Category:beobot]]