Laying out lots of LEDs

[greggj]

Hiya all,

I got about 260 LEDs to lay out in a grid. They are all mixed up when you “populate from schematic” (or whatever the option is called). So unstringing them one by one takes time.
Is there any way to select all object type, say LEDs - and then just get them to be laid out in a grid automatically - without having to resort to scripts?
I can imagine I’m not the only one

I can select individual LEDs in the schematic - and the selection then happens on the PCB . But I can’t select - say - 8 components in schematic and have them be selected in the PCB view. Wonder if that’s just a limitation or a bug.

Using 6.0.10 . Tried the nightly build, but that doesn’t improve things and it crashed on save, so won’t be using it for a while

[Piotr]

@greggj

Is there any way to select all object type, say LEDs - and then just get them to be laid out in a grid automatically - without having to resort to scripts?

As people write here if schematic is divided into subschematics then you can get footprints at PCB divided into groups like schematic is divided. Never tried it myself but I think it can be helpful in your case.

[paulvdh]

You can select a footprint, then right click and select: Special Tools / Create Array, but that function creates new footprints that are not linked to the schematic and I do not understand how that can be used in a meaningful way.

There is also an “Place Footprints” plugin, but I have not used it myself. Is this compatible with your: “without having to resort to scripts?”

Another method is to use the “Replicate Layout” plugin, but this needs a change of the schematic. This works by making a schematic sheet with a row of LEDs and then re-using that sheet for each column. (or swap “row” and “column”, whatever works best for you).
With the replicate layout plugin you can also automate most of the drawing of the PCB tracks.

KiCad-Nightly also has a “Pack and Move Footprints” feature that may help with the initial sorting. With it you should at least be able to separate the LED’s from the rest of the footprints easily.

Post-v6 new features and development news

Now you can quickly separate footprints by functional blocks by selecting them on schematic, then using the new “Pack and Move Footprints” action in the PCB editor. The footprints are grouped by size and sorted by reference, then packed in a square. The initial footprint spread algorithm after updating PCB from schematic was also improved. The placement is more compact, and symbols that are close to each other on the schematic are more likely to have their footprints close on the PC…

[greggj]

The new version (7) has this great option, when you select multiple items in PCB view - and press P - it will arrange them nicely.
I wish devs added bunch of options that would allow me to arrange it in grid of various sizes, spacing , etc. Or is this too late to have a KiCAD v7 request please ?

[greggj]

@paulvdh

There is also an “Place Footprints” plugin, but I have not used it myself. Is this compatible with your: “without having to resort to scripts?”

took me a while to understand how it works, cos its not intuitive at first. But I got it using this plugin.
Thanks!