I’m relatively new to EDA software but I’ve made some boards and footprints at this point. The specific issue I am having is relating to big snap in capacitor footprints.
It has 4 pins, 2 of which have positions defined by degrees at the same radius of the positive and negative leads. Does KiCAD have some way for me to best approach doing this? I was hoping SnapEDA or Mouser would get me a footprint for these (I have a few other similar snap ins I’m trying to get footprints for) but it’s been the better part of 2 weeks; at least from Mouser. I just tried SnapEDA a couple of days ago. Still, I’d like to know how I can do this myself for the future.
It’s just Trigonometry . . . you can work out the positions given the angle and the PCD of 22.5mm +/-0.1mm . . . alternatively put 2 pads in 22.5mm away from the 0,0 point one above and one below select them both and rotate 30deg, duplicate the 2 pads and rotate once more by 60deg this time, then delete the surplus pads.
There are probably other ways to do this too . . .
This whole job to make a footprint takes a total of about 4 minutes when you have spent a little time learning how the symbol and footprint editors work.
It really pays to learn and use the Symbol and Footprint Editors. Using these features saves hours of surfing and correspondence.
The simplest way is probably to just draw a circular array of 12 pads and then delete the pads you don’t need and renumber the left overs.
I also had a look at the 3D model for that capacitor. What a horror. The reference is at the top of the capacitor (???) and the pins look so abysmally angular and unrealistic that you can’t really use it for testing your footprint.
To make this:
Open Footprint Editor
Set grid to .25mm X & Y
Change to Polar coordinates.
File > new footprint: fill in the box.
Save: select a personal libray for the footprint.
Place pad (number 1) on the axis.
Edit pad: diameter 5mm hole 2mm.
Right Mouse Button on pad for Select > Positioning Tools > Move Exactly & tick Polar coords.
Fill box: distance 11.25mm angle 270 > OK
Place pad (number 2 and should be same dimension as 1) RMB Positioning Tool > Polar.
Fill box: 11.25mm angle 90
Place Pad (3) on axis, repeat procedure but this time 11.25mm & 30 degrees
Place Pad (4) on axis, repeat procedure but this time 11.25mm & 150 degrees.
Select F.Fab layer, select graphic circle click mouse on axis. Drag away from axis and watch measurement. Stop circle at 20mm radius.
Select F. Silk. Repeat making a circle but this time 20.25mm
Select F.Courtyard Repeat circle but this time 21mm.
Save. Done.
Maybe need to check tolerances for pad holes and circle diameters.
Jmk’s polar coordinates style really looks great. But if you want other options:
Draw a new graphic arc, starting from the center of the footprint (center of the component). Continue horizontally, click when it reaches the wanted radius (11.25mm). Continue down/right; you can see the angle there. Stop at 30deg and click. Then last point is now in the destination. Move a pad there.
KiCad doesn’t snap to items in other layers, so you can change the arc’s layer to F.Cu from the properties. Keep Ctrl pressed while you move the pad so that it snaps to the snapping points of the arc.
