KiCad Gerber Viewer - Need How To Align Layers Tutorial

Re: KiCad version 5.1.6-1
Windows 10

This is one of my first attempts to make a multi-board design. I need to align the gerbers, so that the separate boards will align, when assembled.

Previously, I just printed the boards on paper and checked the alignment with a back light. (That does work with my current revision of the boards.) But, it occurred to me that I could check the alignment with the gerber viewer.

I found this tutorial, but in Step #5, the directions say to right-click on the layer to evoke the “Modify Orientation” function. That does not work.
https://docs.oshpark.com/design-tools/gerbv/modify-orientation/

So, I need a tutorial that works with the current version of KiCad. Please and thank you.

First of all gerbv and kicad’s gerber viewer are different programs alltogether. If you want to follow that tutorial then download gerbv: http://gerbv.geda-project.org/

But seeing that you are on Windows and there doesn’t seem to be gerbv build available for win you will probably have to look for alternatives.

What I can suggest is exporting layers you want to overlay into svg and then using a graphical program like inkscape to manipulate them.

1 Like

Thanks, qu1ck! I will leave this thread up, for awhile, to see if anyone else has a suggestion.

I would think that there is some way to go in to KiCad/PCB and change the orientation point of each board to a common point… say the mounting hole in the top, left corner… I don’t feel great, today, and that makes it hard to think, but I will try to keep after it…

If both projects are in kicad then even easier way to do overlay is to just open one project in pcbnew standalone (laucnh pcbnew.exe not kicad.exe) and then append the other board. Then move it as needed, just don’t save the file (or have a backup, in fact always have a backup).

1 Like

I’m thinking I just need to find out how to make the origin of each board a point that is common to all three boards. Meaning, set the origin to be the drilled mounting hole that is in the top, left corner. That hole is common to all three boards.

That is easy too.
Click on your hole or pad that has the hole and you will see it’s position in absolute coordinates:

image

Now say you want it to be (100, 150) for all your boards. Select the whole board and press ctrl-m (move exactly), in the resulting window enter 100 - current x position and 150 - current y position

image

That way kicad will do the math for you. Press ok and the whole board will move so that your hole is now at (100, 150).

Do the same for other boards and now the gerbers should align automatically.

Also there is auxiliary axis origin that you can place on the hole
image
and if you check corresponding box in gerber plotting dialog it should use that origin as gerber origin.

I haven’t used that though so test it yourself.

@qu1ck Thanks for the tip. I found that definitely one needs to check Use Auxiliary Origin when generating plot and drill files. Then the gerbers and drill files of both boards lined up in the viewer.

Now I have to figure out how to flip one of the boards as they are mounted back to back in my design.

Great instructions, qu1ck! Sooo glad you reminded me to make a backup copy. I would add a couple of steps…
Select one item to use as a reference.
Read its coordinates and write down the math formula for where it is going on note paper.
Turn on all Layers and Items. If it is not checked, that layer/item will not be moved.
Change Locked Footprints to be Locked Pads.
Select all items and Move Exactly, by entering the formula that you wrote down.
Save.
Repeat for each board.

I have not finished, but this seems to be working.

Would have changing the gerber axis to use the Auxiliary Origin aligned the gerbers, without having to correct the board files?

It should, but you still have to place the auxiliary origin.

qu1ck, I have finished resetting everything as you instructed and it worked perfectly! Now, I have greater confidence in my layout. Thank you!

1 Like

Recently I had the idea to use (127, 127) mm as a reference position for all my future PCB’s.
That reference position can be a corner of a PCB, pin 1 of a THT connector or other recognizable feature on a PCB.

The reason for this magic number is that it is the lowest common prime between some triangular country in the west and the rest of the world and you can switch between grids (for some common THT connectors, and metric for board outlines and the rest) When done this way, you can add some nice round numbers as references on Dwg.User for CAD purposes etc.

https://sourceforge.net/projects/gerbv/files/

1 Like

I don’t understand the issue.
ASSuming the boards are to be stacked, making the outline’s origin identical should answer your question. Whatever holes that are needed for standoffs should be placed at the same coordinates in all the different PCB’s.