Making a multi-component footprint from a single one

[kenyapcomau]

So the time has come for me to do this sort of thing: Grouping parts and centering as a group

I want to make a footprint comprising 4 LEDs in series. The main reason is to lock the relative positions of the LEDs, and most important to be able to rotate the combination by arbitrary angles on the board. Rene thinks it’s a hack, but to hell with the BoM since I’m not after automated assembly. Here’s what I have now, not finished.

I did this by copy and paste. Have I done the right thing by numbering them like above so that they will get connected in series later? I noticed that the pads are not Cu entities and read that I should not put copper in footprints.

Another thing I want to do is remove the individual courtyards and replace it by a rectangular one with rounded corners that covers the assembly. Can I just delete the 4 individual courtyards then create a new one?

Finally when I move the REF** I notice from a blue line it’s referenced to pin 1 of the left LED. How can I re-reference it to the centre of the combined footprint?

Kicad 5.1.5 if it matters.

[pedro]

@kenyapcomau

Another thing I want to do is remove the individual courtyards and replace it by a rectangular one with rounded corners that covers the assembly. Can I just delete the 4 individual courtyards then create a new one?

Yes.

@kenyapcomau

Finally when I move the REF** I notice from a blue line it’s referenced to pin 1 of the left LED. How can I re-reference it to the centre of the combined footprint?

With the anchor tool. In the footprint editor, place the anchor between pins 3.

@kenyapcomau

Have I done the right thing by numbering them like above so that they will get connected in series later?

It doesn’t matter, as you are also the final user. I prefer to give each pin a different number and connect the pins in the schematic. But it’s your choice as far you understand your own schematic.

Another thing you need to do is a unique 5-pin (or 8-pin)symbol to match the footprint.

@kenyapcomau

I noticed that the pads are not Cu entities and read that I should not put copper in footprints.

I don’t understand what this means. I can’t figure out a footprint without copper unless you plan to solder the pins “in the air” by pairs.

[kenyapcomau]

@pedro

@kenyapcomau

I noticed that the pads are not Cu entities and read that I should not put copper in footprints.

I don’t understand what this means. I can’t figure out a footprint without copper unless you plan to solder the pins “in the air” by pairs.

In the footprint editor, pad is a primitive as it is an object under Place. Also it’s in the file like this:

(pad 1 thru_hole rect (at -12.7 0) (size 1.8 1.8) (drill 0.9) (layers *.Cu *.Mask))

and presumably the Cu and mask layers etc. are generated when the footprint is placed on the board. Therefore I reason that should not try to connect the pads with copper at this stage but let trace routing take care of it later. Someone also mentioned in a thread not to add copper to footprints.

Ideally I could make the inner pads already connected, then I could dispense with the inner numbers, trace routing, and associate the chain with a diode symbol.

Also I can’t figure out how to draw a courtyard. There is a polygon tool, but there is no selector to make it go on the F.CrtYd layer.

[kenyapcomau]

@kenyapcomau

Also I can’t figure out how to draw a courtyard. There is a polygon tool, but there is no selector to make it go on the F.CrtYd layer.

Never mind I figured this out. I draw the lines and then edit properties to make it go to the F.CrtYd layer.

@kenyapcomau

Ideally I could make the inner pads already connected, then I could dispense with the inner numbers, trace routing, and associate the chain with a diode symbol.

The best I could do is 1. Make the outer cathode pin 1 and the outer anode pin 2, then give the inner connections numbers 3, 4 and 5. Then starting with the LED_ALT symbol, I added 3 hidden pins of type passive and created a new symbol: LED_ALTx4. Hopefully I can then use it on the schematic like a single LED and the ratsnest lines will indicate the inner connections need traces.

This is what I have now:

Now I still have to fix the 3D model, it shows one LED in the middle when I need to show 4.

[pedro]

@kenyapcomau

Therefore I reason that should not try to connect the pads with copper at this stage but let trace routing take care of it later. Someone also mentioned in a thread not to add copper to footprints.

I see, you mean copper tracks into the pcb, not copper pads. I can be done but I don’t recommend it because the tracks will be ignored by the DRC.

[SembazuruCDE]

@kenyapcomau

Never mind I figured this out. I draw the lines and then edit properties to make it go to the F.CrtYd layer.

Or, select the F.CrtYd layer (so the little blue arrow on the left of the layer list now points to the front courtyard layer) and then draw lines. Both techniques work.

[kenyapcomau]

@SembazuruCDE

Or, select the F.CrtYd layer (so the little blue arrow on the left of the layer list now points to the front courtyard layer) and then draw lines. Both techniques work.

Ah, ok I was used to using the dropdown in pcbnew.

[kenyapcomau]

Ok this is what I arrived at.

I think it will work out for fab. One snag was that I had to assign pins to the inner connections so that they could be joined with traces. I could make them invisible but then they might accidentally brush up against a wire and get connected. At least if they are visible and NC, ERC will detect when this happens. What I really need to do is make a new symbol, perhaps an elongated rectangle with a diode symbol on it. Fortunately joining NC pins in pcbnew is not a DRC error.

This is a horrible hack of course because the components aren’t represented in the BoM. It would be nice in some future Kicad version to have a way to create compound components that have the correct inner connections, and a compound footprint, yet contribute correctly to the BoM, with the appropriate coordinates for PnP.