Hi guys, I am trying to import the gerber and drill files from here: PCB GERBER files into the KiCad PCB editor.
I proceed as follows: I open all the files in the Gerber Viewer in KiCad. Then I go to the menu File → Export to PCB Editor. Next, I set the export targets as follows:
After opening the file in the KiCad PCB Editor, it seems that all layers have been loaded correctly, except for the B.Cu and F.Cu layers. Instead of these layers, I only see a solid-colored layer without any visible traces or connections. Otherwise, the dimensions and everything else appear to be fine.
Could someone please advise me on how to properly import everything into the KiCad PCB Editor? Thank you very much in advance.
The gerber files use “Negative” polygons to show the openings. The converter doesn’t handle these well, so you end up with a large polygon on the top and bottom layers.
FWIW, the gerber to pcbnew converter is very rough. You will be better off recreating the two layer board in pcbnew
The original PCB layout file (ATU-100_mini_PCB.lay6 or ATU-100_EXT.lay6) appears to be from a program called Sprint Layout 6.0 from Abacom. There is a free viewer available on their website that maybe will produce an image that is easier to trace over.
This may be so-so either way, but probably Seth is right.
The biggest problem is usually re-creating the footprints. It doesn’t make much sense to try to create a KiCad layout from gerbers if you don’t have footprints with which to replace lone pad graphics (and silkscreen lines, texts etc.).
In this design you can delete the one big outer polygon, cutout polygons and polygons which represent those “negative” openings. After that you have the pads and the tracks left (now, after exporting, they are covered by larger polygons). After replacing pads with real footprints – which you have to design separately although it’s possible to copy some items from the board to footprint designs – you have the tracks connecting the footprints, but there aren’t so many tracks here, and you could have just drawn them from scratch.
For the footprints it may be easier to find ready made replacements for example from the KiCad libraries.
Then you just need one zone covering the board. As far as I can see, the largest polygon is the ground zone outline. In the gerbers the holes in the zone seem to be made with negative shapes and then tracks and pads again with positive shapes. That’s a different strategy than what KiCad uses.
So, if you want a design you can edit further, you have to do so much manually and there’s so little you can save from the original that it may be easier to do it from scratch, following only the dimensions from the original.
Here’s some instructions for reverse engineering from gerbers, but it depends on how the gerbers are constructed:
