This tutorial was done on Windows. Authors claim it could also be used on Linux by using Mono, but I haven't tried and don't understand a lot about Mono to see what could be done. I am switching to Linux nowadays, so I'd be very grateful to anybody that'd make instructions on how to launch it, however - and I'm sure other fellow Linux-wielding engineers will be grateful, too =)
The tool I'm personally using to panelize boards is GerberPanelizer from ThisIsNotRocketScience.nl. It's a wonderful tool that allows you to panelize PCBs, mainly using tabs&mousebites. There are more tools in the archive, they all seem Gerber-related but I didn't even go through them =)
I'm using KiCad myself, so I'll mainly work with KiCad-made gerbers. The panelizer project page has some tips for Eagle users as well, related to CAM files, so if you're an Eagle user, check it out, it can help with some moments. I'd love to cover Gerber generation for different EDA packages (actually, not), but Internet has plenty of tutorials on those. There's a good online Gerber files viewer (needs gerber ZIPs) which gives out pretty renderings of your board, so you can use it to check your Gerbers - I do that all the time (and KiCad 3D viewer helps, too).
No matter your EDA tool, the workflow is simple - first, you have to have gerber files in separate folders for each project.
Generate gerbers for each project that you want to include on the panel. You should have a couple of separate folders with gerber files - or in case you want to panelize multiples of the same board, just one folder.
Gerber folder requirements:
- Just a folder, named however you like, with Gerber files inside (not zipped up or anything)
- Only one board per folder allowed
- Files can be in ".gbr" format (where extension is the same but filenames differ), judging from the code, but I haven't checked if it works.
- Otherwise, has to have a .gml/.gko file - .gm1 from KiCad isn't suitable yet (but will hopefully be at some point)
The workflow is simple - drag a folder from your file manager onto the view, and the board inside the folder will be added.
To start, open the GerberPanelizer tool. Go to File->New:
You'll get a 10x10cm panel view. If it's not the case, or you want another size, you might change panel parameters in "Panel Properties".
Now, you need to drag a folder with gerbers onto the view. The collapsible list in the right top corner will indicate there's a board and, if you're lucky, it's going to appear on the field, too.
Necessary: leave some distance between adjacent boards: the mill bit that will be milling out the board outline has to have some place to move. Good distance is 2mm and up.
After we placed some boards, we need to place tabs connecting them, and I think it makes sense to do it manually. Hover mouse cursor on the space between the board and press T on keyboard, you're going to get a circle. Move that circle to the place where you want a tab and it'll link two boards. If it won't be able to, the circle outline will be red and it'll give a warning in small text, hopefully.
Too many tabs will make dividing boards hard. Not enough tabs will give a chance of boards breaking off and getting lost after milling. I more or less have one tab per each board in total, there's also "1 tab per 3cm" rule of thumb. This is OK:
Now, once you've rotated, moved and linked all the boards, press the File -> Export Merged Gerbers button, and make a new folder somewhere to store the gerber files in:
That's it, your gerbers are being linked together. In a short time, the tool will automatically open your image viewer software with pictures of back and front of your boards (those pictures will also be saved in the folder with the gerbers taht just got created). Now zip the gerbers up and send them off to fab!