Gerber netlist/DRC verification

[randychase]

For those now doing verification for fabrication, please provide the process you use. I have ignored doing this for many years with no problems, but just had a faulty board when the gerbers didn't work out.

[phillipr]

Randy,

We send the ipc netlist script output file with the gerbers.

[Fab Guy]

If you are using Power pcb to compare netlists, and you have a version of CAM350, Use the following procedure.

In Power PCB
Load PCB file
Tools|CAM350
Use defaults, Note location of .CAM file
Create file only, or create and launch.

In CAM 350
Note location of a pin 1 or tooling hole
File|Export|Netlist
IPC-D-356
Note location of saved file
File|New

In Power PCB
File|CAM
Insure Layers are flooded and planes connected in Pour manager.
Choose layers to export, note only electrical and drill are required at this point.
Run, note location of exported layers

IN CAM350
File|Import|Auto Import, choose directory which contains the Gerber files
Run drill script to identify nonplates and correct the actual drill sizes.
Tables|Layers, Label Layers
Info|Query|All, to insure gerbers are at the same location as the IPC netlist.

In CAM350
Utilities|Netlist Extract, accept defaults
File|Import|Netlist
IPC-D-356
Should come back with netlist import done, found no errors.


If you have errors

In CAM350
Such as: Incoming Net GND passes thru nets $Net42 and $Net43! (open)
Info|Find|Net, look for this last net given, in this case $Net43

Such as:Incoming nets 24MHZ and GND both pass thru net $Net41! (short)
Info |Find|Net, look for GND, if too much info, then open .CAM file from Direct CAM and look for both items.

Note: there is no need to jump back and forth, you can direct cam and export gerbers at the same time. Also, if you are a script to generate the IPC file, you dont need to Direct CAM out of Power PCB