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:
Thanks for your support. I decided to re-make the PCB but now I and already finished a lot of the work but I have some doubts and questions.
I’m not sure how to recreate some of the copper areas according to the original PCB (see the image with the sections: on the left is the original Gerber, in the middle is my version with footprints, and on the right is without footprints). I assume I need to create those rectangular copper pads using zones, as it seems that footprints alone are not sufficient, as shown in my middle and right images. However, I’m completely unsure about the circular copper areas visible in the original Gerber.
I attempted to create four circular pads using the circle tool and then converted them into zones. This can be seen, for example, with the pads connected to FWD and RVS, but I have no idea if this is the correct approach. When I then tried to create a GND zone in this area, no clearance was generated around these circular pads.
It seems I am missing some basic understanding. Here’s an example from the other side of the board. Around some components, a clearance is generated, but not around the layers, traces, and pads I created myself.
Here’s how I proceeded: I only had Gerber files and drill files available. As described above, I couldn’t successfully import the Cu layers, so I only imported all the other Gerber files and the drill file. I connected everything to a schematic that I redrew from a PDF. I placed the components and started creating traces. I didn’t set clearance anywhere explicitly, but when I check the details in some areas, the clearance is listed as 0.5 mm.
I will try. I am new to the KiCad and just learning while playing with this project. BTW I found now the when I use the circle tool or rectangle tool I can add the the object to any net… good to know.
Instead to add copper circle, rectangle or any geometric shape I suggest you to created a custom footprint SMT pad. Then you will able to add it in your design
I don’t think so. maybe I don’t understand this completely from the images and the explanation, but I think you just have a basic, normal situation with pads and zones. You have for example two rectangular pads at left with “Earth” net (maybe badly named if it’s not connected to our Tellus! “GND” is the standard for the device’s reference ground). You don’t have the zone around them, though. Just create the zone, one large simple rectangular shape with the same outline than the red area in the leftmost image, set it to the same net and fill it. If I understood correctly, you have already tried to do this.
What you need to do to get correct connections is to set the zone’s “Pad connections” property to Solid. Some of the round THT pads, on the other hand, need thermal reliefs – in the image with 4 spokes. Try setting the zone’s property to “Reliefs for PTH” and it may do it automatically so that SMD pads have solid connections and PTH pads have reliefs, I haven’t actually used that. You can find the corresponding property in each footprint and even in each pad, and there you can override the zone’s setting case by case basis. This is what I have used.
