How to combine gerber data for different PCBs

[lguancho]

Hi, all. I have gerber files for 5 different PCB, all double-sided design. How can I combine these files into 1 single gerber data. My intention is to save some fabrication setup cost.

Please recommend me a CAM tool that can do this job.

Warmest Regards

lguancho

 

[Frosty]

Any cam tool can do this.

Cam350, Camtastic, GC-CAM.....

You can also do it without CAM tool.

Most packages will allow you to have multiple PCB on the same PCB document, but of course you cannot use any rule checking features as the netlists will be corrupt.

But if you open a new PCB file, create your mechnaical details for your 'panel' then you can copy / paste your seperate PCB into this new PCB docuemnt, add mechanical details for any break outs or scores to split the different PCB after fab.

In this way you can generate one set of gerber files for all PCB at once.

This is actually what you would do in a cam tool anyway, so why use one at all.

Which PCB editor are you use? Are you use any power (negative) planes? If you use planes, it would be better to convert to copper (positive) by using copper pour or place polygon as most times power planes will screw up like this as power planes do not really exist as objects until gerber stage.

:F

 

[lguancho]

Hi, frosty. I am using protel 99se. I have created the 5 PCBs in a single project, the netlists are different files. So, I can actually open a new pcb file, and copy and paste each pcbs into this new pcb file?


Thanks for helping.

lguancho

 

[taring77]

i did try that in PowerPCB its userinterface is friendly but like frosty said perhaps u check the design rules & make sure individual board is okay 1st then u just copy over to 1 pcb and send the gerber files. But do be careful coz the size of file can be big if poured

 

[lollobrigido]

pr0tel D*P 2oo4 with his Cam tastic has good tools for this work. I use it and it's simple.

Lollo

 

[Frosty]

If you are using 99SE.

Make all things and layers visible in PCB or they will not get copy

Open new PCB, PCB Nr. 6, make 1mm active grid

Copy all object from PCB Nr. 1 into place in PCB Nr. 6

When doing this use Eduit,Select,All and then Edit,Copy. Then when ready to past, use Edit,Paste,Special and tick box for to allow Duplicate Designators.

Copy all object from PCB Nr. 1 into place in PCB Nr. 6 using paste special command
Copy all object from PCB Nr. 2 into place in PCB Nr. 6 using paste special command

And so on.

Move your PCB around the PCB Nr. 6 area for best fit, once finish copy all 5 PCB, pick a mechanical layer and draw PCB 'frame' for your panel.

You cannot of course use DRC on PCB Nr. 6 as netlist is not good, you have to make sure 500% all DRC is already OK in PCB Nr. 1 - 5

Good luck

:F