Membrane pattern cannot be connected

[dol2zang]

In kicad 5.1.7 version, it was not possible to connect with “walk around”, so I connected it when working with “highlight collision”.

However

Even if you change the MODE of “interactive Router settings” in version 6.0.5, the wire is not connected.

Is there a way to connect the membrane pattern wire?

Upload the footprint file

membrane_switch_4.4mm.kicad_mod (1.2 KB)

[paulvdh]

There are two ugly ways to get this done. One way is to combine the Highlight collisions with the option Allow DRC violations:

Another, but similar way is to first draw a track segment, then move it by grabbing an endpoint and placing that endpoint on the pad. KiCad does not do DRC checks during move operations.

These two ways do let you make a connection, but they do not get rid of DRC errors.

The real problem is more work to fix.
In your footprint, you have used graphical items to draw the pads, and this does not work anymore in KiCad V6. The normal way to draw such pads in KiCad V6 is to first draw a pad in the Footprint Editor, then select the pad and press [Ctrl + E] or select Edit pad as Graphic Shapes frop the popup menu.

Doing this makes ads the lines and arcs to the pad itself, so KiCad can also calculate clearance outlines around them. I did this and it works. I can now use this footprint on the PCB, and connect a track to it (without violating DRC). There is another problem though.
You have drawn the “fingers” of this switch very close together, and now KiCad is complaining because the 0.2mm clearance of the net I drew it with is being violated. See the screenshot of the PCB editor with the clearance outlines below.

Some other changes I made:

1. I reduced the pad size from 0.5mm to 0.4mm, so the SMT pad is the same diameter as the fingers and arcs.
2. I turned off the F.Paste and F.Mask layers for both the pads. You probably do not want solder paste on these pads.
3. I removed the circle you drew on F.Mask, and replaced it with an “Aperture Pad”. This is now the only object on F.Mask.
4. Along the editing, the file format seems to have changed a bit (as viewed in a text editor) I’m not entirely sure what happened.

But in the end, the footprint below is almost good. You only have to fix the clearance issue. The pads and the fingers now inherit the clearance from the net they are attached to.

membrane_switch_4.4mm_V2.kicad_mod (1.7 KB)

[dol2zang]

Thanks…very a lot…

It’s been a big help.