Coax Resistor foot print

I hope you can see the picture. Need a foot print for a two legged resistor. One leg is a bolt for a 144mil hole that needs a large pad for a nut on the back side and a very small pad for the top side. (Through hole, different size pads) The second leg mates with a 800mil pad in the same location with 300 mil of void in the center. (like a surface mount pad)

coax resistor

Do you have a link to the datasheet you could share?

Ring shaped SIMD pads can be made with complex pads.

If you just need a copper ring than it is quite easily done.

  • First place a graphical circle with the correct diameter and width on any layer.
  • Put a circular SMD pad anywhere on this circle (such that the pad is fully covered by the circular line)
  • Select both the graphical circle and the pad.
  • Right click -> Create pad from selected shapes

If you need a complex paste layout then maybe use freecad with stepup as shown in Kicad StepUp: The Sketcher for Footprint generation
If your paste layout is a simple segmentation like in Mounting_Wuerth_WA-SMSI-4.5mm_H1mm_9774010482 then you can use the generator i wrote


I don’t have the data sheet today.
It is a shunt resistor for measuring high current. There are two high current connections and a BNC scope connections. I believe this picture is the part but does not show the large 0.8" washer/flange that the factory added to make it mount on a PCB.

I am going to work my way down your ideas. Thanks.
So far I made a large thick donut around the part of “F. Mask”. This I hope will give me a large area of copper with no mask and no solder paste. (I will put the part in a large copper zone)
Then I will add a SMD pad in the F. Mask area for the second leg.

For the first pin; I might have to have a non plated hole with pad on only the bottom. I tried to make a through hole with different pad size top/bottom but can not. I may have to use the F. Mask idea and a zone fill to get a large pad on the bottom side.

Something like the picture but round flange and much less white insulator.

Thank you for that. It really helps to make a small pad and a shape and connect them together.
I can only post one picture at a time. Here is top side. Large copper donut for the resistor to sit on. Plated hole and small pad. I put a area fill over part of the part just to show it connects and does not fill the center area.
How to make it work.
I made a “O” in silkS and put it at (not 0). Easy to work on if not at zero. Copied the “O” to another location. Changed one to Top Copper and the other to Top Mask. When these are at zero address you get a “O” of bare copper.
Next problem is a Filled Zone will fill the center of the O. I could not find a round Keep Out. From experience, uncommitted copper blocks Filled Zone. I made a circle of copper, thin, and just larger then the inside the O. This blocks the Filled Zone from getting to the inside of the O.
Added a SMD pad inside the O and combined the pad and O together.

The 3D view shows “R1” in a bad spot. While the layout editor shows it outside the copper O. I will have to look at the gerbers to see what really happened.

Bottom side. Large pad. Area fill works.
I made a plated hole with a pad on the back side only. It made this side work but left me with no pad on the top side. Fixed by adding a small “O” of copper to the top side pad.

There may be some things I forget. I tried many different things.

A plated pad might not be a good idea as the drill hit for this pad will be placed in the drill file for plated holes. Unless you want the hole plated (the picture seems to suggest you do not want that)

I really suggest you make a ring pad in the way I explained above. This allows you to add a non-plated hole in the centre which will be more in line of what you show in your picture.

The example board has a plated hole.
I think I will say with a plated hole because the pad will be stronger. There are Gorillas with wrenches.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.