User Guide

2. Section for the component side (already contained in
GERBER.CAM).Youcreatetheoutputfiles:
name.cmp
Layers:Top,Pads,Vias
3.Solderside(alreadycontainedin gerber.cam):
name.sol
Layers:Bottom,Pads,Vias
4.Silkscreenprint,componentside(alreadycontainedin gerber.cam):
name.plc
Layers:tPlace,Dimension,tNames
5.Silkscreenprint,solderside(alreadycontainedin gerber.cam):
name.pls
Layers:bPlace,Dimension,bNames
6. Supplylayer$GND(new in gerber.cam):
name.ly2
Layers:$GND
7.VCCinnerlayer(new in gerber.cam):
name.l15
Layers:VCC,Pads,Vias
8.Solderstopmask,componentside(alreadycontainedin gerber.cam):
name.stc
Layers:tStop
9.Solderstopmask,solderside(alreadycontainedin gerber.cam):
name.sts
Layers:bStop
10.Soldercreammask,componentside(new in gerber.cam):
name.crc
Layers:tCream
11.Soldercreammask,solderside(new in gerber.cam):
name.crs
Layers:bCream
Check once more whether all the necessary layers for the creation of the
aperture table are active in the first section. The output file generated in
the first section cannot be used. For this reason, the file name.$$$
shouldbedeleted.
Layers that refer to the bottom side of your layout will be generated
mirrored in all predefined job files. If your board house recommends
non-mirroredfiles,pleasedeactivatethisflagoptionforeachsection.
If you want to generate output files for supply layers with one signal (here
$GND),youmustonlyselecttheinnersignallayer.Nopads,novias!
For other inner layers that may contain polygons you have to select addi
-
tional pads and vias layers (as you would also do for the top or bottom
side).
If the Layer Setup defines blind and buried vias, the combination of one
signal layer and the Vias layer shows (according to the via length) only
those vias that belong to this signal layer. If there is only the via layer active
(nosignallayer)theCAMProcessorwilloutputallviasofthelayout.
224
EAGLEManual