BTW, I tried to create a solidregion, but that does allow to set multilayer, but with the odd behaviour of converting it to a cutout ??

Hi! Picture of the footprint mod attempt would be nice, it tells more than a thousand words :-) Regards, Markus Virtanen HW / Electronics Designer

Take for example a single "finger" of the  edge connector pad, numbered "N". Make the card edge section out of two single layer pads,  top and bottom layer. Number them both N. Make them a little longer than required, say by 10%. Place a multi-layer pad of the same width and long enough to accommodate the hole plus overlapping, lengthways, the first single layer pads by that 10% margin. The hole should not overlap the single layer pads. Number this pad N. On the multi-layer pads, set the solder mask expansion to -0.55 times the width of the multi-layer pad. Don't forget the minus sign. Repeat for the required number of pads. Done.

Ok Andy, I get it. Combine a simple outer layer track element with a multilayer pad, and elimitate the soldermask on the pad. Thanks.

"elimitate the soldermask on the **multi-layer** pad." You've got it. :)

Got it to work. Great. Now, I hope the Gerber reflects my design in a way the PCB manufacturer can understand.

There have been a number of posts and issues identified recently about checking Gerbers generated using mm as the canvas units. To avoid any issues: Ensure you do your final DRC checks using the dimensions units that you created the board in to reduce the risk of rounding errors generating false DRC errors. Then switch to inches or mils units before you export the Gerbers. Then check the Gerbers using gerbv.

OK, thanks.

OK, I ended up doing this: For each finger (wire solder pad) i created two single layer pads (as ones used for SMD footprints), one placed on each outer layer. Then a third multiplayer pad (as ones used for through hole mounting) placed further in on the PCB. All 3 pads with the same pad number. The two single layers pads are connected to the multiplayer pad by laying these out with some overlap. Finally I had to remove the paste mask on both single layer pads, and the solder mask on the multilayer pad, all by using a negative expansion value larger than the pad size. This looks like so on the top side, and the bottom side is equal to. Each solder pad now has connection to a different layer on the 4 layer PCB. The vias are closed off to not swallow solder, and the pads are free to receive a edge connector or wires. The paste mask cover the finger pads.