Hello Since this is a two years old problem, then I don't think that I will bring the best solution, but let's try. I suggest you to make a customized footprint matching the dimension of the desired shape and to do this you need to create a new "PCB Lib" : [https://docs.easyeda.com/en/PCBLib/PCBLib-Create/index.html#Create-The-Footprint](https://docs.easyeda.com/en/PCBLib/PCBLib-Create/index.html#Create-The-Footprint)

@palimpalim, Assuming that the hole in the round pad is a hole in the copper of the pad and NOT the PCB: In the Top Layer, create a arc using the Arc Centre tool set to the Centre Point option. When you start drawing the arc it will appear as a circle. You don't have to draw it accurately at this stage so just left click once then draw part of an arc and left click again to end the arc. Then right click to exit drawing the arc. Select the arc and in the right hand panel, set the desired Width, Radius and Center X and Center Y. Set the Start angle to 0 and the end angle to 359.9. Right click on it and select Convert to Pad. You now have a circular Top layer pad with a hole in the copper. This is an annulus. Select it and set the Paste Mask Extension to minus half the width of the annulus. So if the width of the annulus is 0.25mm (i.e. half of 1.65mm diameter -1.15mm diameter), set the Paste Mask Extension to -0.125mm. Setting it to an arbitrary value of less than this, i.e. -1mm is fine. This closes off the paste mask aperture. Now create 4 arcs in the Top Paste Mask layer, of the correct dimensions to leave the 4 gaps when placed in a circle. Using the Two point arc option may be easier. Place them is the required positions. Done.