Translate GERBER files

[mxlemming]

Hi,

I have a request, which is probably me being dumb but…

I have a dual board design. There are pins that click into place top to bottom. It would be great if the pins lined up… and they do by my measurements.

But, it would also be very nice if I could load the two GERBERs that are actually being made and overlay them, which would avoid all ambiguity.

I cannot find a translation option. I might be blind or stupid, or it might not be there… Any hints?

David

[RaptorUK]

Why not export one board s a STEP file and create a rudimentary footprint for it and add it’s STEP file.

Then add this footprint to the other board and look in the 3D viewer to check the alignment . . .

[mxlemming]

I also just found I could copy paste the top copper layer of one onto the other and see that way. So I guess in practical terms the question is solved…

[paulvdh]

There are plenty options here.

1. Start with a template, that has outline, mounting holes critical connector locations, and use that template for both projects (probably a bit late now).
2. Generate gerbers from both projects, and then load some layers from those projects in the gerber viewer and lay them on top of each other.
3. The Gerber viewer can create a PCB from a set of gerber files, but that does not give more possibilities in this regard then doing something with the original files in the first place.
4. When the PCB editor is running in Standalone Mode you can use the File / Append Board function to load another PCB. (Make sure you have copies, backups).
5. You can use: PCB Editor / File / Fabrication Outputs / Gerber / Plot Format: SVG, and then in the other project, use PCB Editor / File / Import / Graphics to read your image and put it on a user layer for reference.

These methods can all be used to verify whether things were done correctly, but for designing the thing in the first place, putting both PCB’s in the same location on the canvas makes it easy to directly compare coordinates. Using the “File / Drill origin” and put it on a reference location (for example pin one of the mating connectors) is also a good option. And there are some left over risks that have to be managed. For example when using dual row pin headers, you can either put both connectors on the top of the PCB of each project (such as those “stack through” connectors used in PC104), or put one of the connectors on the bottom, but you have to use Male / Female connectors to prevent mirroring the pin layout.

Doing a manual test with something physical you can touch can also help, such as:

[tutorial] Test fitting Footprints

A small demo to show how I test fit footprints. It’s a combination of a few things to make it work perfectly. The first step is to print a PCB mirrored on a piece of Paper: PcbNew → File → Print → Options Mirror → Print. 2nd step: Take a needle and pre-punch all the mounting holes into the paper. (For the large holes I used a hole punch). 3rd step: Carefully put the connector into the sheet of paper. 4th step: Take a picture or scan the whole contraption with a flatbed scanner. This make…

Also, mating the connectors before and during soldering can help. It reduces the risk of the plastic overheating, because the mating connector absorbs some of the heat. And even if they overheat and some plastic melts, it still keeps the conductors in the right place. It also improves alignment during soldering.

[BlackCoffee]

FYI… Humoring myself…

This may not matter in your case or, perhaps most cases. But, if you move the position of something just slightly, perhaps because you need that ‘ever-so slightly’ changed position, you probably would not visually notice it if overlaying the two files.

However, there is a difference that may matter to you/others… I see users talk about umpteenth decimal places and not considering the average thickness of a human-hair is 0.003inch and they worry about that…

Example: I moved a Track’s Start/End position by 0.01mm and cannot visually see the difference but, it does show up when comparing files in Text-Editor…