Panelization - using GerberPanelizer on Windows (Linux possible)

A project log for Small PCBs for panelizing + tutorial

Ordering a 10x10 board with only 10x4 taken? Panelize one of these!

aryaArya 05/08/2017 at 23:2826 Comments

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 =)

This is the GitHub issue describing steps to launch it on Linux, half-successfully (thanks to @jlbrian7 for figuring this out)

The tool I'm personally using to panelize boards is GerberPanelizer from 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.

Gerber export tutorial - KiCad (with important Panelizer-specific notes)

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:

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!


rob wrote 09/09/2021 at 20:00 point

Just tried this.    Wow, that panelizer is painful to use, slow and waits for you to get done entering all your data before it crashes.    Has no documentation to speak of, and what else?

The ThisIsNotRocketScience GerberTools is not completely worthless, however.; it serves as an example of how not to release software.

  Are you sure? yes | no

Ken Yap wrote 08/02/2019 at 23:33 point

Sadly the latest release from 2018 doesn't work under Linux for me, only the one named Panelizer posted by somebody in a thread you referenced works.

I also found quirks in the software. For example if position two instances of the same design head to toe by rotating one 180° and then run the packer the rotation (any angle actually) gets cancelled.

Never mind, the tool will only be used once in a while.

C# looks as horrible a language as Java. 😉

  Are you sure? yes | no

Dave's Dev Lab wrote 08/02/2019 at 02:07 point

wow nice new tool! i've been using gerbmerge for some time! it's much more cryptic than this tool!

  Are you sure? yes | no

Arya wrote 08/02/2019 at 22:57 point

This writeup will have its second birthday in a couple of days! ;-P it's probably just that you only saw this now due to the new comments. Do check out this tool, I am very happy with it - I even have a Python script to auto-combine the .pos files!

  Are you sure? yes | no

Ken Yap wrote 08/02/2019 at 00:20 point

Thanks, seems to work well under Linux. I used a precompiled version labelled in that github thread you referenced. Didn't check if anybody packaged a more recent version, just playing around with it before using it in earnest.

I ran it under Linux by going to the directory and

mono GerberPanelizer.exe

then driving the GUI. Naturally mono needs to be installed. I installed the package mono-core and its dependencies on my distro. .gbr format doesn't work but Protel does if you rename .gm1 to .gml. A pity as .gbr extensions are the better standard.

A little experimentation shows that mono needs to be run in the directory with the .exe and other resources so I made a little helper shell script like this:


cd [directory with GerberPanelizer.exe]

exec mono GerberPanelizer.exe

  Are you sure? yes | no

Arya wrote 08/02/2019 at 01:11 point

Very happy to hear that! One small comment from you, one giant leap for me gradually moving from Windows to Linux =)

  Are you sure? yes | no

Ken Yap wrote 08/02/2019 at 01:30 point

I take back the comment about .gbr format working. Seems only the Protel extensions work.

  Are you sure? yes | no

Arya wrote 08/02/2019 at 01:36 point

Got it! I don't think that's Linux-specific, maybe the panelizer just doesn't understand the KiCad format? I would suggest you open an issue on GitHub, of course, look it up there too, maybe someone already figured that one out.

  Are you sure? yes | no

Arya wrote 08/02/2019 at 01:36 point

(I personally never use the .gbr extensions, so I have no idea if they actually work on Windows)

  Are you sure? yes | no

Ken Yap wrote 08/02/2019 at 01:49 point

It's not a Linux or Kicad issue. The problem is the Protel file extension convention was always that, not a standard. I can imagine someone reading a printed copy of Protel documentation wasn't sure if it was .gml or .gm1. Neither is mandated by any standard so it's a WontFix issue for Kicad. The later x2 format with metadata in comments fixed that so the only extension needed is .gbr what is specified in the standard. But Panelizer doesn't understand that format. If not already done Panelizer should regard .gml and .gm1 as equivalent.

  Are you sure? yes | no

Pintoo wrote 07/16/2017 at 22:33 point

Hi Aresnijs, I'm discovering Gerber Panelizer, thank you for your tuto, 

do you know how to deal with the creation of breaks between the gerber files and the 'fill empty area' area ?

I'm using Version 1.0.6257.24941 built on 17/02/2017

  Are you sure? yes | no

Arya wrote 08/03/2017 at 04:16 point

Hi! Sorry for reaching out so late, I didn't get a notification for your reply here =( I have sent in a pull request to fix this issue on GerberPanelizer GitHub, but AFAIK the PR is not merged, and the issue is not yet fixed separately. Meanwhile, I can publish a version I compiled myself, without this problem. 

  Are you sure? yes | no

Seamus de Cleir wrote 09/12/2018 at 19:21 point

Is there a complied version with the fix? I see that the solution still hasn't been used 

  Are you sure? yes | no

Seamus de Cleir wrote 09/12/2018 at 21:31 point

Thanks a million

  Are you sure? yes | no

Dolev Papo wrote 10/13/2019 at 13:44 point

@Arsenijs The file is no longer available. I'm not sure it'll solve my problem, but my problem is that I'm checking 'fill empty area' and hitting OK and the software crashes...maybe little help??

  Are you sure? yes | no

Tom Magnier wrote 06/02/2017 at 06:09 point

I came across this tool but didn't have a chance to play with it at the moment... Seems better than doing the mouse bites by hand :)

About the KiCad origin issue, you might want to export your Gerbers (and drill file) with the "Use auxiliary axis as origin" option. In KiCad you can place that auxiliary origin with one of the buttons in the toolbar.

  Are you sure? yes | no

Arya wrote 06/08/2017 at 02:46 point

Added the instructions for the "auxiliary origin point" thing, hope nobody misses it when following the instructions =)

  Are you sure? yes | no

ZaidPirwani wrote 06/01/2017 at 09:24 point

I needed JUST this... thanks

  Are you sure? yes | no

Arya wrote 06/01/2017 at 11:03 point

If this is useful to you, and you have some small boards that would be useful to others, please do share them on this project =)

  Are you sure? yes | no

leb9049 wrote 05/09/2017 at 05:04 point

@Arsenijs Thanks, this looks good, I'll give it a try on my next board. One of my issues is trying to keep the order# the board house puts on off my actual boards. Have you had any experience with trying to tell them where to put it?

  Are you sure? yes | no

Arya wrote 05/09/2017 at 12:04 point

As far as I know, DirtyPCBs, for example, doesn't care and will put it wherever. Other fabs, however, don't put them at all. I'd say it's very fab-specific, but I'm guessing that if you have part of your board full with silkscreen art and another part is empty, they'll most likely put it on the empty part. 

But then, I don't know if it's not automated =D

  Are you sure? yes | no

drojf wrote 06/02/2017 at 10:14 point

PCBWay actually states this on their website "Attention please! If you don't note not to add pcb order number on board, we will add it on board by default!"

What they do is let you enter an order (eg dimensions, quantity, color etc) without uploading a PCB file. After your order is entered, they give you an order number, e.g. "1234567". Then you can go back and modify your PCB to add the number, "1234567" somewhere on the board (probably would be a good idea to let them know where you put it as a comment). DISCLAIMER: I haven't actually tried this before.

The funny thing about how they charge - it costs extra if you put multiple DIFFERENT designs on one board. However if you put multiple copies of the SAME design on one board, they don't charge extra.

  Are you sure? yes | no

Arya wrote 06/01/2017 at 11:00 point

BTW, I ordered two identical panels from DirtyPCBs, and the order numbers were in different places, even though the gerbers were identical =)

  Are you sure? yes | no

Ken Yap wrote 08/03/2019 at 00:44 point

@Arsenijs All this talk of order# made me look at a board I had made. It took some searching but I found the order number PCBway put in 1 mm lettering under one IC footprint. That size wouldn't bother me at all.

Another fab I used, elecrow, didn't put an order# at all. And they also offer V-cut and mouse bite panelizing for free for identical designs on one board but you have to give the instructions in separate notes.

  Are you sure? yes | no

Arya wrote 05/09/2017 at 00:18 point

@leb9049 Check this tutorial out =)

  Are you sure? yes | no