I hereby certify that I am not simply asking someone else to design a footprint for me.
This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.
Hey guys!
First time KiCad user here, and Ive been trying for a few hours to figure out a workaround for merging multiple pads together. A reference image and technical document can be found at the end of this.
Each input pin is connected to a heatsink, however I am struggling to figure out if there is a methodology for merging each of said pins. The resultant footprint throws errors on the pcb layout, which serves as a significant portion of the errors therein. I have tried editing the pads in the fooprint editor as graphic shapes, but have only managed to merge one of them. I have also gone into the symbol editor and changed each of the input pins to be numerically the same. Ive perused stackexchange and this forum for an hour and only found vague answers to the aforementioned, so I thought I would ask for assistance here
Use many pad numbers at footprint (like at your picture) and use the corresponding pins at symbol to connect them at schematic (can be done by placing pin over pin in symbol so at schematic you see one pin.
Give all connected pads the same number and you can have one pin in symbol.
A variant of 2 can probably be to make a complicated shape one pad.
I suppose that if the pins were connected at schematic you should not get errors at PCB.
I have recently made first experiments with it. I think that you can only merge graphic to pad and not pad to pad. So to make complicated pad you should have one pad and several graphic rectangles.
This I don’t understand. You made several symbol pins having the same number. I have never tried it.
Assigning the same number refers to pads not pins.
One way is to change nothing on the footprint at all, but modify the schematic (symbol) instead. If the netlist has pads 5, 6, 7 and 8 connected to the same net, then you won’t get errors.
The Edit Pad as Graphic Shapes is also an option, but normally this has only one pad, and the rest are graphic elements (lines, arcs, rectangles and such).
For this method:
Draw three rectangles, with the shapes of pads 5, 6 and 7.
Replace pads 5, 6, and 7 with those rectangles.
Select pad 8, and press [Ctrl + e] twice. (To enter and exit pad edit mode). At the moment pad edit mode is exited, overlapping graphics will become a part of the pad.
A third and simple method is to simply renumber all overlapping pads to have the same pad number.
When you’re satisfied with the answer / result, then mark the best fitting answer to the original question as the solution. You can do this by clicking on the checkbox in one of the posts.
The goal here is to help other people who are searching this forum for answers, to find their answers quicker.
