Help creating footprint for SMA clamp

Hi BDC, sorry to read you are struggling with this still. 

The two suggestions I have are to create two pins out of each pad. I have seen this implemented for some high speed connectors. See below image example for a surface bnc type, for which there are two separate shapes overlapping to create this.

The second idea is use the donut type pad design which has a hole inner diameter. This can be placed in the symbol dra but each pin could be surrounded by a static shape already containing the necessary void. These shapes can be assigned to the net. Here is a mock up example I made: 

Before the 'DONUT' pad type existed, we would create a shape symbol with an inner arc connected to an outer arc with line segments spaced 0.02 mils apart...

I can't upload an image, so below is the 'show element' of the shape:

LISTING: 1 element(s)

             < SHAPE >

       class         ETCH

       subclass      TOP

  element is on a dummy net

  Number of connections: 0

  Shape is solid filled

  Area:   0.0118  (sq in)

Exterior boundary: 

  segment:xy (0.01 -12.50) xy (0.01 -62.50) width (0.00) 

  arc seg:xy (0.01 -62.50) xy (-0.01 -62.50) width (0.00) 

    center-xy:  (-0.00 -0.00) radius (62.50)   CCW

  segment:xy (-0.01 -62.50) xy (-0.01 -12.50) width (0.00) 

  arc seg:xy (-0.01 -12.50) xy (0.01 -12.50) width (0.00) 

    center-xy:  (0.00 -0.00) radius (12.50)   CW

  Number of voids: 0

HI.

Hi, There are a couple of methods to design this connector & Considerations. Technically for the connector from a board perspective your going to need three pins for the connections and a route keep out circle that is oversized for the center pin, along with a soldermask area that extends beyond the body of the part and a silkscreen. Since this connector will connect to a ground plane on the board, when you pour the copper the Route Keep Out will keep that pour away from the center pin. The only other thing you need is a 3 pin symbol for the schematic.

The other option when creating the part is to also include the physical etch that represents the part body and this can be done by composing a shape within the PCB Symbol editor. The first option is the easiest of the two. I cant post any pictures of the part I created for you, got a notice about "contacting the administrator"

The datasheet for that connector has some ambiguity. It does not show a dimension for the curve part of the connector body. The center pin
for the through hole pin does not include a recommended drill size. The center pin shows a diameter of 20mil, so assume an 8 mil or 10 mil drill hole. More than likely that thru pin will have to be filled and capped since it mates to the connector. Depending on the frequency of use you may have to consider back drilling the pad so as to preserve the S11 response over frequency. What frequency will the conn be used at and what RF Power level ?

Best regards.