Panelizing - What are People Doing?


I’ve searched the forum on this topic and come away with the impression that KiCAD really cannot do panels in any straightforward, professional, and non-error-prone way, so this post is not really to ask for KiCAD workarounds but rather to ask what people actually are doing in order to get boards panelized (or panelised). Here’s my history:

In the first batch, I sent gerbers for one individual PCB to Sunstone and told them I needed it panelized so that Screaming Circuits could assemble them. A month or so later my lovely assembled boards came back without further action on my part.

In a subsequent batch, I had the boards made by a Chinese vendor. Again, I sent them the gerbers for the individual PCB and the outside dimensions of the panel that Sunstone had made. The panels came back fine, I sent them off to Screaming for assembly, and again the finished boards came back fine without my having to do anything.

In a still later run I changed to a local assembly house. I gave them the made-in-China panels, and they said “We need gerbers for the panel so we can make the stencil”. I was like “What? I have no idea.” After a few days, they came back and said “Our stencil vendor has agreed that they can make your stencil” as if this was a major project and inconvenience for them.

Now I have some new small boards that need to be panelized. I sent the gerbers off to the same Chinese vendor with a note that they should make the panels 5 x 8 boards or whatever is most convenient for them, and they came back saying “We can’t make your boards without panel drawings”.

This is getting tedious, and I hate feeling like I’m not providing adequate documentation to vendors. Any suggestions for recommended practices (apart from going back to Sunstone/Screaming, whose prices are 3x those of China + local assembly)?


Is there a script to clone PCB on panel for manufacturing?
Print PCB copy one sheet
Kicad panelizing
SKiDL: a Python-based schematic design language
Print PCB copy one sheet

Wait a sec.
Are you interested in the final boards, being assembled (maybe even tested) only or do you care that they need to arrive at your place in a large panel (also assembled and tested I guess)?

  • I buy my panels from China.
  • When the panels arrive I send them and a kit of components to a domestic assembly house.
  • My assembly house is asking for gerber files for the complete panel so that they can make a stencil for solder paste. I do not have gerber files for the complete panel.
  • Also, the Chinese board vendor on one occasion has asked for “panel drawings”, which I don’t have and am not 100% clear on what they want. I don’t see how I can give them a drawing without knowing the details of their process (tab/perf, v-score, etc).

So I am asking what workflow others use for getting panels and panel stencils made.


This looks promising, although the warning about hole misalignment is a bit worrying since this is an Eagle (ugh) -oriented tool.

I would think there’d be a good demand for such a tool, and I for one would be willing to pay money for one that works well and professionally.


I don’t have experience on that level… unfortunately.

Anyhow - to make panel drawings you would need to know the panel size of the boardhouse. It’s a non-starter without that information.

Next piece of info would be the local assembler and what he can work with - as I assume he will make/order a stencil that fits his tools.

And as you found out KiCAD currently isn’t in a position to give you panel designs out-of-the-box, but I could see it done with the array function and manual placement of v-score in one of the Eco layers maybe (if you ignore ratsnests going all over the place and DRC becoming useless) . If you’re going for mousebites you’d need to be smart about what to include in the array (Edge.Cuts) to save manual work with the mouse (and possible errors).

I’m sure one of the more seasoned users will chime in if he’s got some idea/tip what works for him.

PS: cool that they made it open now… last time I’ve seen that tool they had closed alpha/beta testing going on. Will need to check this out at some point :wink:


Hi Julia,
I can tell you how I’m dealing with Panelizing stuff:

  • for the first run, I order panelizing by the PCB manufacturer, and at the time I do specify panel configuration which is worked out with my EMS (single board configuration like 4x4, separation technology (v-score,route), margin size, additional fiducials and tooling holes for the margins),
  • I request the PCB manufacturer to send me back GERBER files for the combined panel (that’s the key here),
  • I prepare stencils for this particular panel design,
  • if for some reason I need other PCB fab to manufacture my boards, I do provide them the working GERBER files of the configured panel instead of just basic board design.
    It would be harder to end up with identical panels, if the panel would be redesigned. You don’t have to change the stencil each time you choose new PCB manufacturer, and you can keep all your manufacturing configuration (like pick&place, AOI etc…).

Btw, I might have mistaken you with someone else, but does your entry mean that Gen16 brain is designed with Kicad?


That’s my process too. If they won’t send back Gerbers, its likely not the place you want to go. After all, you need to do a sanity check if they modify your files to make sure they didn’t mess something up.


Thanks for the great info. Yes, I’m the designer of the Gen-16 system; I used Express PCB for that project, it’s my favorite PCB tool by far for its great intuitive UI but it’s limited in some ways - you have to pay extra for Gerbers, you cannot get centroid data, routing signals on inner layers is difficult, you’re limited to 4 layers, 90-degree rotations, only circular holes, and no npth holes. I think our CM in China copied my layouts into PADS for final production.


Nice to hear you’re the designer of this breakthrough system.
IMHO Kicad seems a way to go. Few years ago I was looking around to find best low-cost EDA package that will allow me to do commercial projects. I chose Kicad and I’m pretty happy with my choice, especially after the project underwent massive improvement thanks to the dev team.
Kicad will not limit you with your projects, and with the features like interactive routing you’re getting close to the top tier EDA experience. Once you’ll learn it’s interface, it becomes a very handy tool. I’m successfully manufacturing Kicad-designed boards, and I don’t feel the need to look for alternative.
One more hint, use some 3rd party GERBER viewer for validation of your production files, just in case you’d find some “hidden feature” of the GERBER engine in your EDA package :wink: I use GERBV (part of GEDA package), and I’m fine with it.


Yeah, Kicad is OK, and generally less user-hostile than most other PCB programs like the absolutely ghastly Eagle. It’s just a shame that it contradicts so many standard (outside of engineering, anyway) UI paradigms; it’s really not necessary, as Express PCB demonstrates. The UI inconsistency between modules is a bit maddening as well, but I guess that’s to be expected from something written by various random people.

I’m enjoying the interactive router and tolerating everything else, although I still swear at it regularly.


So I bought this:

Looks like it will do everything I could ever want, and well, with a pretty nice UI. Note that it’s not a stand-alone, you have to also buy one of their “main” CAM tools. I bought ViewMate Deluxe for $95, total investment was $350 for the package - a lot less than FAB 3000.


I’m glad you found a reasonable commercial solution. I may look into that myself.

If anybody finds this thread looking for a open source/hobby solution I have used gerbmerge multiple times before on kicad and eagle exported gerbers. One of the same or many unique designs are possible. I didn’t write the program, but my fork has some fixed for metric units that are needed to process kicad gerbers. The gerber processor is pretty basic, so it can have trouble with complex fills and slots. Opening and resaving in gerbv to simplify the gerber syntax can help.



So far, I have sent the gerber files to the manufacturer and they made the panel and the stencil.

Then I sent pcb panels and the stencil to the assembler.

But have you tried the “create array” feature in pcbnew opengl mode? I think this feature solves your need for panelised gerbers.



I create my panels using the Append Board feature in Pcbnew. I am using tabs to connect boards together. This means I use a footprint that represents a tab and place it around the board that I have imported, modify the cut lines. Then I use the Create array feature to multiply the boards. As a last step I create the frame for the panel.

The final panel ends up looking something like this:

I wish there was a better system inside KiCad where one could just list some parameters of how the panel should look like. Making it easier to update the boards inside the panel, as well as creating new panels.


Usually if one person who is able to code and needs a feature badly it happens :wink:


You would find some of the PCB fabricators starting to use KiCad internally. Many are currently using dodgy cracks


Yeah I obviously do not need that feature badly enough to implement it yet. But if the block reuse feature gets implemented that the developers are talking about on the mailinglist, the step to panelization will become much smaller. :slight_smile:


Hey esden, thank you so much for posting that image. Your post told me everything I needed to know in order to start panelizing in kicad.

The trick was to create a new footprints for the horizontal and vertical 0.1" tabs with the mousebites.

For the mousebite/tab footprint, I started with a 0.1"x0.1" silkscreen box centered on the origin, so I knew where the margins are for the tab. Then I used 2mil (0.05mm) drills inset from the edge of the “tabs”. After those are set up, I erased the silkscreen and saved the footprint. I’m not sure if I have the drill size and mousebite offset perfect yet, but it’s a start.

(updated with correct mousebite drill specs, 2mil (0.05mm))


I leave panelising to the CM doing the board assembly - I just send them my cad files and I get back fully assembled pcbs.

In fact, I recently asked them if it would be better for me or them to panelise:-
Reply from the CM: “Yes best if you leave the panel design to us so we can optimise design for our systems and also to ensure its cost effective for a fabricator.”

Your CM probably wants tooling holes and panel sizes to suit their machinery - letting them panelise solves all this.


It’s certainly a good idea to talk to your CM about their process requirements, but not all CMs can or want to panelize your boards, especially for free.