1. Download The Tools
You probably already have KiCAD. Next, make sure to download GerberPanelizer by This is not Rocket Science (site link) from GitHub. This guide uses the 2018-08-10 snapshot release.2. Export your designs from KiCAD
Your designs have to be completely ready for production before starting this process. Components placed, tracks laid, zones poured etc. It is very “one-way” in that it is impossible to update an already panelized design once it has been exported.
Here’s one of the designs that will be added to the panel.
place
→ grid origin
to do this. I am putting it in the top left hand corner of the board.

Grid origin placed
file
→ plot
to adjust the gerber export settings.
- Make sure
Output directory
is set to an empty directory somewhere on your disk. In this example, it’s set totx-gerbers
. - Check
Use auxiliary axis as origin
- Check
Use Protel filename extensions
- *Optional* Since I’m not using them in this design, I’ve unchecked
F.Paste
andB.Paste
.
Plot
.


.drl
files.
Select file
→ fabrication outputs
→ Drill (.drl) File...
These settings will automatically be set to match the previous export, but make sure the output folder and the drill origin match the previous settings. Mine looked like this:


3. Modify the exported files
This step is weird. You need to change the extension of all.gm1
files to .gko
. For this example, flail-tx-kicad-Edge_Cuts.gm1
needs to be renamed to flail-tx-kicad-Edge_Cuts.gko
as this is what GerberPanelizer expects. Here is my resulting directory:

.gko
file4. Load the designs into Gerber Panelizer
Open up GerberPanelizer, you will be greeted with this screen:
file
→ new
to create a new project. Next, select board placement
→ add gerber folder
and navigate to the output folder from KiCAD. In this example, it was tx-gerbers
.
You should be seeing something like this:

board placement
→ autopack: native
and your design will leap into view:

add instance
.
5. Arrange designs and add tabs
Since you’ve been hittingboard placement
→ autopack: native
after each board add, your designs should be properly arranged at this point. You can manually move the designs by clicking and dragging them, but I’ve found that using the autopack works really really well. Here’s what my design looks like at this point:

breaktabs
→ insert breaktab
, and a small red circle will appear in the top left hand corner of the workspace:



6. Export the panelized design
It’s a good idea to first save the design in GerberPanelizer so you can edit the layout later without having to start from scratch. Once you export the final merged gerber files, they cannot be edited or re-arranged. Selectfile
→save as
to save the project.
Now to export the gerbers.
Again, in GerberPanelizer, select file
→ export merged gerbers
and choose an empty output directory. The directory has to be empty because you typically send a zip archive of all gerbers to the manufacturer to get made, and this zip archive should just include this export. You should see this window pop up:




.zip
file.
7. Verify using GerbView
KiCAD ships with a program called GerbView to inspect gerber files. Open that gerbview and then open your zipped merged output directory withfile
→ open zip archive file
.
There will be an error message which you can ignore.



8. Wrap up
Thanks for reading! Did this guide work for you? Let me know in the comments below this post.Note: This is confirmed to work with KiCAD 4 and 5.
excelent explanation!
You saved me! I am looking for a panelizer for many months and I was not able do put to work this software and your explanation is very clear!
marcelo pessoa
thanks a lot , nice job, very clear explanation
Awesome! The “Use Protel filename extension” solved by problem. Thanks.