Duplicate Layout for second unit?


I’m looking for the best way to copy a layout design. If it were a left/right channel thing, I would copy the channel in a hierarchical sheet and do the Layout twice.

However, in this case, it is really just a second unit that I want to combine on a single PCB. They work complete separately (maybe apart from the power connector). It is up to the user to cut the PCB in half if needed.
If I add a second hierarchical sheet, all labels would be different.

So I tried just copying everything, but I don’t think this is a great solution as I now have hundreds of unconnected nets between the two layouts.

What do you suggest doing?

Say you have a single PCB and want a duplicate of the circuit on a larger PCB.

Simply window-box select the complete PCB, Copy it, Paste it right back into the PCB (or, another PCB file). Draw new Edge_cuts for the full enchalada).

You can set it up into Panels, if desired (different ways to do it…)

Example shows one circuit, copied, pasted and Edge_Cuts redrawn…

Well that’s what I tried. But since I also copy the net information, I get a mess with new “unconnected” connections. See picture above

I saw it but, why copy the Net? The Single PCB contains all the info needed for a Copy

I don’t know why it copies the net information as well. I selected in the Selection Filter all Items and duplicated it exactly as you said…
I mean, what could I do wrong witch simple copy/past? :man_shrugging:

Well… Not related (or, perhaps is related) I upgraded my Mac last week and had odd problems. I thought I worked them out until today.

After upgrading the Mac, I upgraded Kicad to 6.0.4 and thought all was good. That assessment was based on only brief inspection… Today’s efforts lead me to discover problems galore…

Firstly, (not important to you) somehow a complete Duplicate of the HD was made and set to Hidden.

This resulted in Duplication and funkyness of Kicad’s access to the Paths and Files…
Everything was duplicated! Some Apps and Files are opening from a combination of locations…

Example: A Trimmer-Pot that was perfect in previous Kicad 5.0.10) now shows it still linked to good paths and 3d step file but, it (and none of my previous models) show in 3Dview though all looks correct…

New projects created using the models/footrpints/symbols are ok but, not the old stuff…

I guess I can’t help you… (I’m about to stop using technology and go back to Pencil & Paper!)

…following up…

I just made several new PCB files - all 3D, Footprints and Symbols are loading okay!

Thus, so far, it appears the Mac upgrade is the problem. When loading an older Kicad project, some show about half of the 3D models, other half not showing…

I leave it here…

Well thanks buddy, I appreciate!

Regarding the technology. I used much, much worse tools than KiCad in the past. I’m generally quite happy with Kicad and version 6 especially.

If anyone else could give me a hint though concerning the layout duplication problem, that would be great.

The magic word for what you want to do is called panelization.
The problem with it is, that it is not (officially) supported by KiCad (yet).
There are however quite a lot of people who want to make panels and there are several script based approaches and tutorials. KiKit (a plugin installable via KiCad’s plugin & Content manager) also claims to be able to help with it.

In a simple approach, you do it by:

  1. Make a perfect PCB, with just a single instance of your board.
  2. Open the PCB Editor in Standalone Mode
  3. Use PCB Editor / File / Append Board to add a copy of your PCB into this separate instance of the PCB Editor
  4. Modify it, add: Edge.cuts, mouse bites, etc.
  5. Forget about DRC in this stage, it’s utterly broken because of the reason you already noticed.
  6. Have your panel manufactured from that copy of the project.

A simple search will find more (but similar) alternatives:

The plugins and script I mentioned earlier automate part of these tasks. I have however not used them myself and have thus no experience with them.

I did this. The extra rats at the end? So what? Board was done and they don’t show up on the gerbers. Keep two copies if you want. One of the board prior to duplicating it on the other half. I didn’t bother.

Or just start a new project and paste two copies of your original board into this new project.
Same Refs & no ratlines.

Or just hide the ratlines.

Just make sure your original board is absolutely:

It is sub optimal if you can’t verify the final gerbers that you sent for the PCB’s to be manufactured. These days KiCad also has a nag screen that tries to refill zones when you want to create Gerber files, and that could mess up your panel.

This becomes much more of an issue, if you want to add extra hardware, for example a connector fro gang programming or testing the whole panel.

Also, just for completeness:
There is software that can do panelization on a gerber file level, and several PCB manufacturers can make the panel for you for a small extra cost. These usually have some “array function” in which you fill in some numbers for the number of PCB’s you want in your panel.

Ok, I see. panelization…

Not sure though which approach now is best suited for me. I guess the “copy to a new project” seems rater safe.
Quick following up question for this. Do I need to do this in a new project, or can I just create/copy the second PCB file in the same project?

Working with the PCB Editor in Standalone Mode and then using File / Append Board … is the easiest / quickest.

The PCB Editor is in “Standalone Mode” if you open it directly from your file manager, and without an active project.

If you open a project, there is a Save As … in the KiCad project manager, which copies the whole project to another directory, but then you have to manage that extra project, or can have them mixed up.

If you use the Append Board function in the Standalone mode, then you copy the data of a PCB into an empty PCB file and have to enter a filename when you want to save it.

But it does of course never hurt to backup your project before you do anything that could damage it (such as using KiCad functions you are not familiar with). I prefer simple zip files to backup a project (with an date appended in ISO_8601 format. Others use GIT as a backup strategy.

I don’t get it. I had two boards to panelize. First one worked (after a bit of swearing at least).
But the second one still messes with ratsnest.

So the whole point of using PCB editor in standalone mode and Append board is defeated…?

I wonder why it worked for the first board, but for this one it refuses…?

KiCad can not distinguish between net names in the left PCB and net names in the right PCB. For all KiCad knows, the net names are the same, and therefore get merged in a big net.
This is why it is currently not supported.

The only thing the standalone mode adds, is an easy import of multiple PCB’s (can even be from different projects) to make a panel.

The ratsnest does not work when combining multiple PCB’s and this won’t be fixed in short term, because first the underlying problem of the netlist naming must be solved, and this is related to “design blocks” or similar yet-to-be-implemented features.

So for now there is no other option then to disable the ratsnest, and also not re-generate zones when creating gerbers for your panels.

Funny, because now I did it a second time, and now it is working. It still lists unrouted items, but no ratsnest is show between the two boards, despite the fact the ratsnest is not disabled in the view!

Good to know. thanks.

Thanks a lot for everyone’s advice. I think I got the two boards now done .

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