Make a PCB Footprint using a Multilayer pad (numbered 1) created using the Polygon option to create the circular but with a flat sectioned hole. The copper annuals around the pad can then be your ground connection. Add a second smaller multilayer pad (numbered 2) in the same Footprint if you need a connection pad for a wire from the centre pin. Save it with a unique name and a clear Description then, in your schematic, place a 2 pin header and then assign the name of your Footprint to it to pull that footprint into your PCB. Note that depending on your application, a simple wire connection from the centre pin to the PCB may not be a good impedance match to the coaxial cable and connector.

sorry to sound thick but is there a tutorial showing this ?

@2e0oyy, Start here: [https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a](https://easyeda.com/forum/topic/How-to-ask-for-help-and-get-an-answer-71b17a40d15442349eaecbfae083e46a)<br> <br> Then look through here: [https://www.youtube.com/watch?v=MsuR6W-jN5M&list=PLbKMtvtYbdPMZfzGuVTdc0MWKrFvU4nsu](https://www.youtube.com/watch?v=MsuR6W-jN5M&list=PLbKMtvtYbdPMZfzGuVTdc0MWKrFvU4nsu) [https://docs.easyeda.com/en/Videos/Demo-Video/index.html](https://docs.easyeda.com/en/Videos/Demo-Video/index.html)<br> <br>

@andyfierman sorry this is second time i have used this design software. i have been through the videos i started with them and the other tutorial resources. i have tried to research your previous answer which i have been unable to do but i have tried several times i can get a round pad and edit it using polygon tools but still end up with round hole surely this should be a simple thing to do but i guess it is beyond my capabilities. Thank you for attempting to help i think i will have to keep it as a round hole and save myself a headache

@2e0oyy, Oops. My bad. I forgot that the polygon option in the pad tool only affects the copper annulus and not the hole itself. Here are a couple of ways that you can make the shaped hole in the Footprint Editor. **Note:** * These images below are illustrations only. The dimensions shown probably do not match those of your connector. * If the datasheet gives the dimensions of the recommended hole size then use those dimensions. * If the datasheet only gives the the connector body dimensions, you will need to add a small amount to slightly enlarge the hole size. * If you do not have the datasheet then find one. **1) (Preferred)** **Use Arc (Center)** If they are not given in the datasheet then you will have to do some trigonometry on the dimensions of the connector (or if given, the hole specified for the connector) to work out the angles of the end points of the flat section of the connector body with respect to the centre of the circle defining the connector body. Note the radius, R, of the circle defining the connector body (or the hole if given). Set the Canvas Grid and Snap to R (this helps with the construction of the hole shape); Click on the Arc (not the Arc Centre) tool; Click on -R,0 to start the arc; Click on R,0 to end the arc (this creates a semicircle of radius R);  Edit the Start and End angles to the values you have calculated above;  Draw a Track from the Start point to the End point (it should snap to those exact points);  Select the whole arc plus track and set it to the Board Outline Layer;  **2) (Not preferred)** **Use the Solid Region set to Board Cutout:** [https://docs.easyeda.com/en/PCB/Solid-Region/index.html](https://docs.easyeda.com/en/PCB/Solid-Region/index.html) Draw the hole as a series of edited points. **In either case:** Then place a larger diameter round Single Layer pad on each of the top and bottom layers. You can connect the top and bottom pads with vias placed around them if you wish because the hole may not be through plated.