I’m trying to create a footprint for this USB micro connected:
http://portal.fciconnect.com/Comergent//fci/drawing/10118194.pdf
There are two pads that are a mix of a rectangle and a circle. There is an arc on one side of the rectangle. How can I recreate this shape in the pad editor? Can I overlap an oval and a circle without breaking any important design rules for manufacturing?
Basically, I just resolved to make a rectangle that covered the same area. I figured having too much space wouldn’t be a bad thing.
I have exactly the same question, but my pad needs to be ‘L’ shaped, what is the proper way to do this please?
Use two rectangular pads.
Just thinking about it, two pads should work. I’ve never done it before, but gerber files are just XY coordinate plots. The distinction of number of pads in the footprint will go away when the production gerbers are submitted to the manufacturer. If it looks like two pads that overlap in the KiCad footprint, it doesn’t matter. It will look like a single, continuous block in the gerber file.
As a side note, I never figured out the half circle. But I also had to create a rectangle with a cut corner. I did this by rotating a square 45 degrees. I filled in the rest of the space with two more rectangles.
This is not exactly a solution to creating a half circle pad but I was trying to do the same thing and settled on using an oval pad and offsetting the drill hole to the edge of the pad. Looks different but does the same thing.
The OPs FCI usb connector can get away with circular holes and pads, this makes the pcb easier to make and more choice of suppliers.
Just make sure to use thermal relief or soldering those tabs will be a problem
The problem with just using two rectangular pads is that you run into issues with the design rules. I get clearance errors with this method. Moreover, it forces you to draw a track between the pads, despite their clear overlap.
I think being able to draw custom pad shapes is necessary. This should definitely be submitted for a suggestion to the developers.
If the two pads have the same pinnumber than kicad connects them internally.
Two overlapping pads withe same pad number should not cause a DRC error.
Custom pads have been a wishlist item for ages, but no trivial to do due to complexity of managing solder mask, DRC and plotting
Yes, the SAME pad number is the important thing to avoid DRC squawks.
I think there are some rules regarding the degree of overlap, before KiCAD will treat overlapping pads as a single pad. I don’t recall whether it’s a percentage of overlap, or one pad must touch the center point of the other pad, or something else. To make an “L” shaped pad, for example, you may need to define two pads to form the main parts of the “L” and another (long and skinny) pad or two for the “connection” between the pads. Yeah, sort of a kluge, but it DOES work.
Dale
I don’t recall whether it’s a percentage of overlap, or one pad must touch the center point of the other pad, or something else.
Perhaps this was the problem. I just made the pads butt up against each other with 0 overlap and 0 gap.
Zero overlap can easily become a gap after rounding errors - very dangerous
I recently posted a footprint for a TO-220 package at Same net pad clearance settings[SOLVED] .
Download the footprint and open it in the Footprint Editor. Delete the large " Pad 2 " that is used for the thermal tab, and you’ll see other pads that overlap it. After studying their properties and parameters for a few minutes you should be able to figure out how overlapping pads work. (If not, come back here with a follow-on question.)
Dale
So I guess that means some zeros are smaller than other zeros, right?
Shall we start a contest to see who has the smallest one? 
Dale
I’m not quite sure how to interpret that post as there were no smileys or winks.
It has nothing to do with rounding zero. Pad 1 with a width of w1 is placed at x1,y1 and pad 2 with a width of w2 is placed at x2,y2 such that the edges of the two pads touch giving a gap of zero. If at any time a process such as DRC for example were to round any of w1,x1,w2,x2, none of which are zero, then you could get lucky and have an overlap or unlucky and have a gap greater than zero.
Not just the KiCad DRC, the fab post processing treats these pads as discrete objects and might create a gap
I had instances where different zoom levels of the gerber viewer showed a gap and no gap… confusing to say the least.
Maybe our “primitive work” with custom pads will gone soon. https://lists.launchpad.net/kicad-developers/msg27617.html
make the paste and soldermask custom size also.
no diffrent from how you make filled zones in pcbnew.
use same mechanism/concept
poly-line