The panelization process

I have been doing too much PCB design in KICAD for my client from which I used to hand over the process of manufacturing to another designer. Currently am supposed to take the PCB through the whole process until I send the finished and functional product to the client. The manufacturer has raised an issue where I have to push my PCB design to another level before I send it to him and that is the step of panelization. I have red through the internet about this process but I have not come across how it is done in KICAD. Someone help out.

Below is the link of what I have found from the internet:
What is PCB Panelization & Why do we need it? - The Engineering Projects

I have not tried it myself, but I would use KiKit.

1 Like

KICAD does not support panelization directly.
There’s a script plugin KiKit which is intended to define panelization for your boards and output PCB panel.
But even though I deal with assembly house directly, I don’t panelize my boards myself. Instead, I ask PCB house to set up panel according to my needs and do receive physical boards and their panelized gerbers.

IMO if you want to learn how to panelize, learn KiKit.
If you want to get job done, ask your PCB house to panelize boards for you, just like in the linked article.
All I have to do afterwards is the Paste layer that matches the panel. This I do get with the following steps:

  1. Import Panel outline to kicad using Gerber viewer → Export outline to Kicad
  2. Copy original (single board) design to separate folder, like PROJECTxyz_PANEL
  3. Launch PCB Editor in standalone mode, open your board file from above created copy
  4. Group your PCB to make it easier to copy
  5. File > Append board and append the exported panel outline
  6. Copy/paste or create array to put copies of your single PCB at proper locations to match panel spacing
  7. Export your panel’s PASTE layer

In case you have rectangular (didnt tried with other form of edge cuts) board you could try this Plugin:panelize - #14 by poco. This is a simple panelization tool with a simple GUI, way more faster to start than kikit (kikit does not have GUI, as I remember.

Edited, current KiKit does support gui.

1 Like

If you ask PCB house (or assembly house) to do panelization for you I think you should send them Paste layer together with other gerbers and you should get it back panelized exactly as the PCB was panelized.

1 Like

PCBWay does this upon request.
JLCPCB does not, even if requested.
For prototypes and short-batch I mainly use these board houses. For production runs I don’t have to worry about that. Of course I always provide single-board paste layer.

1 Like

KiKit sounds interesting. When I get a break and upgrade to 6.1 I’ll have to check it out.
I pay the contract manufacture to deal with panelization and solder paste mask. They get the full design for just one board, including silkscreen and paste mask. They are the ones that will have to break up the panel. They can choose the configuration of the panel. Otherwise, you have 3 groups trying to communicate with each other.
After you have worked with a contract manufacture (AKA a “stuff house”) enough, they could give you the information so you could do the panelization and possibly save a bit of money on a small run.
The last board I ran was a run of 25. It was $400 fixed price for all production set-up, dealing with the PCB house of their choice, break-apart of the big board, etc. A good deal since a mistake at this level would often cost more than $400.

Agree with responses that you should look at KiKit and learn more about the process. Consider working with your client to go the route I talked about above. Consider if you want to “own”/be responsible for any problems. It is difficult to take on a risk that your are either not aware of or you have not discussed with your client in advance.


Tis one is very helpful. Am loving it. Kikit is becoming something easy to use. Just gone through it in few hours and am getting new and helpful insights. Thanks!

this is a wonderful procedure and I will keep trying it until I get the desired panels.

More of an FYI than a suggestion…

Before we had software (a long, long time ago, because we didn’t have computers) Panelization was done by Milling and PCB fab houses wanted clients to either Layout the panel geometry so they could cut it (they never charged me extra). They provided sizes of the stock material (so client could optimize for cost). They would lay it out for a few dollars more.

I had a lot of success with PCB123 (they also provided free software. They’re still around but, I no nothing about current company…

I retired 20 yrs ago and now make only 1/2 sided hobby boards at home so, I decided to do my own milling (I have CNC mills). But, I stick with this Simple-Minded panelization approach.
Some houses will do V-cuts instead of milling but, the layout process is the same (draw it and make notes on drawing).

Enter Kicad… It’s easy to layout panels in Edge-Cuts. And, even cooler is making a Footprint of Panels. That’s how I do multiples of the same PCB shapes - Make the footprint, change (edit) layers from Dwg to Edge_Cuts. Now, when I need the panels, I just place the Footprint and add my circuit, copy&paste the circuit into the other panels.

EDIT: Before somebody asks/mentions… Yes, the Holes are different for two of the Panels, by design (they get a master circuit)

Example of the Footprint…

1 Like

It does:

1 Like

Ok, edited my post. I found KiKit very hard use, so never practically used that ( during v5). I will give it a try with v6.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.