1
\$\begingroup\$

I'm in the process of exporting a PCB design from Altium. At present I'm saving the output as a .cam file. I've sent this file to a fabricator that uses CAM350 v11 and they are getting an error along the lines of "database unrecognized".

Does anyone have experience exporting Gerbers from Altium for import with CAM350?

Should I be using .cam files for output or should I be using individual files per layer?

Is there another way to export Gerbers from Altium that I'm overlooking?

\$\endgroup\$
1
  • \$\begingroup\$ Have you tried Altium support? \$\endgroup\$ Oct 20 '14 at 11:22
5
\$\begingroup\$

A .cam file is Altiums internal CAM editor file type. It's not a gerber file at all.

You need to actually export gerbers, which are one-per layer.

First, export the gerber files (this is all done with the .PcbDoc file open in the editor):
enter image description here

Chose the layers you need. In this case, I have a two layer board, with a top and bottom soldermask and silkscreen. If you are having solderpaste stencils made, you export those here as well.
enter image description here

The configuration here is not critical, I typically use 2:4 notation in imperial units (but I'm in the US, and we use imperial). It just has to match the configuration when you export the NC drills file.
enter image description here

Now, you have to export the corresponding NC drill file. This is the file that dictates where all the holes go.
enter image description here

Again, as long as these settings match the setting used in your gerber files, they'll probably work. I've tried referencing to absolute, and referencing to relative origin, and not had issues with either with multiple board-houses. I generally leave it all as default except the 2:4 units setting. enter image description here

Doing all this will generate the needed gerbers in a sub-directory of your project folder, called 'Project Outputs for {project-name}'.

enter image description here

For a 2 layer board with soldermask+silk on top and bottom, you will have 7 files (top copper, top soldermask, top silk, bottom copper, bottom soldermask, bottom silk, drill).

For a 4 layer board, you have 9 files (the previous seven plus the two inner layers).

Most board houses just want these files. You generally put them in a zip file and send them in however they ask (either a web-form or email. I've seen both).


Note: that when exporting gerbers and the NC drill files, Altium will export the gerber files, and then automatically load them into a CAM editing session. You do not need this cam file. From what I can tell, this is just so you can verify that the export actually exported correctly. I usually don't even bother saving it.

Note 2: You can also export gerbers/NC-drill files via a .OutJob file. I am not documenting that here.

\$\endgroup\$
1
  • \$\begingroup\$ @Brown1 - Hah, no problem. I remember getting started with Altium. Sooooo many buttons! \$\endgroup\$ Oct 20 '14 at 13:31

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.