Export Gerber files to CirQwizard

Hello everyone,

I’m new with kiCAD and I want to print a PCB using a cirqoid machine and the software running is the cirQwizard.
Unfortunately I cannot export the gerber files to the cirQwizard (the software does not find the gerbers when I try to import them).
Maybe it’s a problem with the format generated from kiCAD but I have already tryied to change it without success.

If anyone could help me, it would be perfect.



We need more information. What version of Kicad and what platform? Is the software all on the same machine or are you exporting it to some device and trying to transfer to another machine? The nightly Kicad builds has experimental support for Gerber 2 format and that helped me out on a simple board I was doing. I haven’t heard of anyone having troubles submitting gerbers from Kicad to board houses so I don’t think it is the format because I think gerber is a ‘format’.

Have you successfully used this cirQwizard with gerbers generated by other ECAD programs?

It looks like you can just rename the Gerber files from KiCad with a different extension.

CirqWizard supports 5 files:(assuming a project called “test”)

1, Top copper layer. Copy test-F.Cu.gtl to test.cmp
2. Bottom copper . Copy test-B.Cu.gbl to test.sol
3. Solder paste, top. Copy . Copy test-F.Paste.gtp to test.crc
4. Drills. Copy test.drl to test.drd
5. Board outline. Copy test-Edge.Cuts.gm1 to test.ncl

This assumes you have “Use Protel File extensions” enabled. I would also suggest making sure “Include extended attributes” is off. There may some other options to change, but that should get you further.

For reference, cirqWizard guide for Eagle is at http://cirqwizard.org/docs/gerber.html


If you have an error message saying that CirQwizard can not find files, then @bobc has probably given the answer: your software is expecting certain extensions on the filenames, which don’t agree with KiCAD’s default extensions. Change the filename extensions and your problem should be solved. (In spite of what some may say, the extensions for Gerber filenames were never truly standardized.)

If your software is finding and reading files, but finds fault with the content, there are a few options to try when you plot the Gerber files from KiCAD. One is to omit the Gerber “X2” information. (“X2” is a fairly recent addition to the Gerber standard, and not yet widely supported.) The other option to experiment with is the numerical precision - 5 versus 6 digits after the decimal point. Both of these are selectable in the “Plot” menu for PCBNew.


Thank you very much guys!

Changing the extension, I could open the files without problems! :slight_smile: