1. Download The ToolsYou 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 KiCADYour 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. You’ll want to add a grid origin that is really close to your design. In KiCAD, select
grid originto do this. I am putting it in the top left hand corner of the board. In pcbnew, select
plotto adjust the gerber export settings.
- Make sure
Output directoryis set to an empty directory somewhere on your disk. In this example, it’s set to
Use auxiliary axis as origin
Use Protel filename extensions
- *Optional* Since I’m not using them in this design, I’ve unchecked
Plot. You should be greeted with a directory of files with dissimilar extensions: Next, you need to export the
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: Here is my resulting output directory with all of the files:
3. Modify the exported filesThis step is weird. You need to change the extension of all
.gko. For this example,
flail-tx-kicad-Edge_Cuts.gm1needs to be renamed to
flail-tx-kicad-Edge_Cuts.gkoas this is what GerberPanelizer expects. Here is my resulting directory:
4. Load the designs into Gerber PanelizerOpen up GerberPanelizer, you will be greeted with this screen: Select
newto create a new project. Next, select
add gerber folderand navigate to the output folder from KiCAD. In this example, it was
tx-gerbers. You should be seeing something like this: Where is the board?! Select
autopack: nativeand your design will leap into view: Now, re-do the guide up until this point for however many unique designs you want to add to this panel. If you want to duplicate your design multiple times in the same panel, you can add an instance by right clicking on the instance in the right hand view and then clicking
5. Arrange designs and add tabsSince you’ve been hitting
autopack: nativeafter 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: To join the designs together, you need to add breaktabs. Select
insert breaktab, and a small red circle will appear in the top left hand corner of the workspace: Click and drag the tab between the two designs. Make sure black dots appear on either edge of the design: Continue to add tabs in the same manner until the text turns a bright green color, this lets you know that the boards will be secured. There is no way to automatically add the proper tabs, so make sure you use your best judgement. Now we’re ready to export!
6. Export the panelized designIt’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. Select
save asto save the project. Now to export the gerbers. Again, in GerberPanelizer, select
export merged gerbersand 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: The contents of the merged output directory should look like this: The merged output directory will include several image renderings of your merged designs, this is a great first check to make sure that everything went well. Looks good! However before you send any critical designs off for manufacturing it’s best practice to visually inspect the layers with a gerber viewer. Save the merged output directory as a
7. Verify using GerbViewKiCAD ships with a program called GerbView to inspect gerber files. Open that gerbview and then open your zipped merged output directory with
open zip archive file. There will be an error message which you can ignore. You should see something like this: There’s the design as we expect it, you can uncheck the different layers on the right pane just like in pcbnew to inspect them one by one. I’ve uploaded this design to oshpark (a domestic PCB fab service) to see if their preview also looks correct and again, there are no problems. You’re now ready to send your panelized designs out for manufacturing. Congrats!
8. Wrap upThanks 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.