Plugins move footprints

I have a hierarchical design with top sheet that has 10 copies of the bottom sheet. The bottom sheet is a simple circuit with qty 2 of SOT-23-5 packages and 6 SMT resistors.

I place these on the PCB. Then run place footprints by sheet. The plugin only moves some of the components.

Is there a process to make this plugin work? I googled and could not find a definitive tutorial for a design with more than one kind of component.

What you want is Mitja’s Replicate Layout plugin

I do use Replicate Layout. But, the cells need to be far apart. Replicate Layout scrambles the pages in the close spacing that KIcad places them.

At least link the plugin that you are using. And if possible share the project so that someone can replicate your issue.

Thank you for the reply.MoveFootprints.zip (262.3 KB)

Here is the place footprints plugin

The project I created to test this action plugin is attached.

Summoning @MitjaN as a friendly neighborhood expert and author of the plugin.

This thread has a link to a .pdf that explains the “Replicate layout” plugin quite well.

First of all we all appreciate if users seeking help are as verbose as they can be. Then our responses can be more precise. So until you correct me I am going to assume that you are using 5.1.x, and Place footprints with Replicate layout action plugins. But if you are using anything else, then my response might not be correct.

The Place footprints will place only anchor footprints of each hierarchical sheet in linear, circular or matrix layout. The anchor footprints are footprints for the same symbol in all the sheets. So if you want to “copy” footprint positions for all the sheets, there are two options.

If you want linear, circular or matrix layout:

  1. position the footprints for one sheet, you might also want to lay out copper traces, zones and other graphical items for this sheet
  2. select the footprint which will serve as a source(reference) anchor footprint
  3. Run the place footprints action plugin which will place destination anchor footprints
  4. select the footprint which will serve as a source(reference) anchor footprint
  5. Run the Replicate layout action plugin

If you want to lay out sheets differently:

  1. position the footprints for one sheet, you might also want to lay out copper traces, zones and other graphical items for this sheet
  2. Place the destination anchor footprints for other sheets manually. Currently plugin only supports if the destination anchor footprints are on the same layer as source anchor footprint
  3. Select the footprint which will serve as a source(reference) anchor footprint
  4. Run the Replicate layout action plugin

It is unclear to me in which step you have problems, so can you elaborate more on the topic. Have patience and keep in mind that for most of us English is not out primary language so we need more words to get the nuances across.

1 Like

I have just tested the MoveFootprints project with Replicate Layout and the plugin works as expected.

Maybe @briansmith23456 had some different expectations, like https://github.com/ian-ross/kicad-plugins.

Hello MitjaN

It is a pleasure to meet you. Thank you for your patient explanation and instruction.

I just replicated your steps and it works.

My problem was that after running Place Footprints, the footprints appears scrambled. After running Replicate Layout, the sheets are brought back together. I did not realize that both plugins have to be run back-to-back. I was trying the plugins one at a time.

Congratulation for creating these amazingly useful plugins and thank you.

2 Likes

Thanks for the kind words. It is always nice to be appreciated.

Yeah the Place footprints functionality used to be folded into Replicate layout plugin. But I’ve split it into dedicated plugin almost two years ago. For two reasons:

  • This enables Replicate layout to work where anchor footprints are placed manualy. So an kind of arrangement is possible
  • The code for place footprints can also be used to place consequential footprints residing on one schematics page (LED, ring, …)

So if you find any old examples on the web you can easily be confused, and I’ll be the first one to admit, the documentation could (and should) be better.

Hello MitjaN

I have an additional item of feedback.

I used the newest Kicad 5.99 just to see if I liked it. 5.99 is definitely an improvement. The new 5.99 does not work with your plugins.

best regards

This behaviour is known.

Eeschema’s file format has been changed in v5.99

No plugin that reads eeschema files will work until it is rewritten.

A v5.1.x plugin specific for pcbnew may work or not in v5.99

1 Like