Can you connect a pad in footprint editor?

Again … just did a bunch of reading …

I am trying to connect two pads in the footprint editor.

They are just 3 mm round pads with a 1.5 hole … 4 mm apart.

One post said to overlap the pads … Guess I would make on oval or large or ?

Another post said it could not be done.

Can I join pads?

Screenshot 2023-11-21 115342


1st, Why do it in Footprint?

2nd, Best to do it in PCB with a Track.
If really wanting to do it with Graphic then, draw it on a Cu layer then, Right-Click and convert to track.

Video show drawing a Graphic Line on Front-Cu layer.
Then, deleting it and drawing a Track.
Then, drawing a Line on Cu-Layer and converting it to a Track.

Note: After Creating it from Line to Track, both are overlaid. You can Delete the Line if desired…

You don’t need a Schematic if not wanting one.
Many of my Kicad PCB’s are made from hand-drawn schematic, old-schematic’s…etc. Some are too simple to bother with schematic…

I just place Terminal/Pad/other footprints and hook-up traces (Track).

It can be done, but you must mark the pads as being net ties. Do this in footprint properties (net tie pad groups)

I think the “Keep It Simple” approach is to give the pads to be joined the same number, and run a track in the PCB editor.

Otherwise, I think the preferred way might be to create a custom pad shape. Other methods used to cause issues with DRC, although of course you can ignore those.

BTW, is the idea to create a multipurpose footprint for different sizes of fuse holders? Because it appears the fuse holder corresponding to that part number only has two pins.

There are certain fuse holders that use multiple PTH pads to mount one mechanical part. Making these net-tie pad groups makes sense to me.

Thanks … I was trying to think ahead. I like this particular fuse holder from Wurth Elektronik … UL approved, 30A … but I can see the quantity is limited in the USA compared to say Keystone but who’s product is not UL approved and only rated for 5A.

I was just worried in a year or two I might not be able to get the Wurth so I am just making the PCB fit either one.

I was going to do it with a track but didn’t want to forget so I thought I could just put it in now.


Great to know … I will jot that down in my notes … thanks!

You read my mind … Just as you suspected, I am designing for two different holders in case one goes obsolete or I just can’t get it in a year or two. I like the Wurth (UL approved, 30A) rather than the Keystone (not UL and 5A).

I can do it with a track but didn’t want to forget it so thought I would put it in now.

I can do it with a track but was afraid I would forget it later … just thought it best to do now.

The simplest way is to use pads with the same pad number. If you do this, then KiCad assumes these pads always have to be connected with a track on the PCB, so you can not forget it. It also simplifies the schematic, because there are still just two (different) pin numbers for the schematic.

You can also use “Pad Edit Mode” to add graphic shapes to a pad in the footprint editor. You can add a line to one of the pads to extend it, so it overlaps with another pad.

So, just to make sure I am understanding correctly …

I just went into the footprint editor … I selected the pads … now I have two number 1’s and two number 2’s (pad number under pad properties).

I don’t see any changes in the footprint but are you saying there will be a trace put in when I drop it into the drawing?

When you put the footprint in the PCB, there will ba a rastnet between the 2 pads n°1, and another between the 2 pads n°2.
After that you will have to draw the track.
If you forget to draw the track the DRC checking will complain that a track is misisng.

Of course you need to execute the DRC checking at some point. but it always a thing to do before sending you design in porduction anyway.

OK …found the properties section and found “Net Ties”

In the larger box is written “Pad groups allowed to short different nets:”

I hit the “+” and it is waiting for me to enter something … what do I need to enter?

I did name two terminals as 1 and two as 2 … is this correct?


You don’t need to do the net tie thing if your pads both have the same number.

You don’t need to draw a track in the board either, you can connect the two “1” pads with a graphic line in the footprint editor.

Hi @xtal_01

There is a lot to be learned by exploring Kicad footprints in the Footprint Editor and the PCB Editor. You can see how they are created and the pads numbered, and if you place a fuse on your schematic, link it to a footprint and follow the procedure to have it placed on the PCB, you will see how Kicad deals with connecting tracks.

The below illustration shows at top, a Kicad library fuse and holder footprint. Underneath I modified some pads on a duplicate to show what can easily be achieved with the Pad Editor.

Generally, the simplest method to create footprints is to find a similar footprint in a Kicad Library, “save as” into a Personal Library and then modify that footprint according to the appropriate Date Sheet.

Finally, If you have access to an original PCB, if it lasted 30 years, making similar footprints should see your new PCB last as long without incident also.

I have only been using KiCad for a few days but have been able to do exactly what you say.

I used stock symbols and linked them to stock footprints when I could.

I was able to used a footprint in the system and modify it.

So far so good.

My only question is how to link two pads in the footprint editor.

I know I can do it later but wanted to do it in the editor so I don’t forget.

I gave them both the same number (two number 1 pins and two number 2 pins).

Do I need to do anything else to make sure they link?"


Do I need to do anything else to make sure they link?

Pads with the same number in the footprint will automatically get a ratsnest-connection later in the pcb-editor.
You are then responsible to draw the track for this ratsnest-line.

Indeed. Just try it out. Link a schematic symbol to your footprint, and start routing. DRC will not accept the board as fully routed until you have also drawn the extra wires between the pads.

Awesome … thanks so much!

Slowly coming together.

With some luck I will have all the parts in today or tomorrow (depending on how much the wife make me do to get ready for Thanks Giving tomorrow).

I will give it a try and see what I get.