`Is it possible to make round pads with different diameters for top and bottom?` Not directly but you can try placing a double sided pad (All layers) and then placing a single (Top or Bottom layer only) pad of a larger diameter directly over it. The PCB Design Manager may complain but it should not stop you being able to have the board made. If it works it may be worth making a note of it in the Documentation layer and/or in an email to support when you place the order. Another option may be use the `Hole` tool in the **PCB Tools** pallette to make an unplated hole and then put a single layer copper pad over it on one side of the board and a different sized single layer pad over it on the other side. This does however result in a non-plated through hole (NPTH). `Is it possible to make double sided pad with top side diameter nearly the same as the hole diameter?` Assuming the above trick works, the limitation on the smaller pad diameter (relative to the hole diameter) is that the Pad tool has a minimum annulus of copper, i.e. you cannot set a vanishingly small ring of copper around the hole. I'm not sure what that minimum is but the tool will tell you if the copper diameter is too small with respect to the hole diameter. You can also use the `Solid Region` tool in the **PCB Tools** pallette to make a hole in a copper area but that is not so useful for round holes. https://easyeda.com/Doc/Tutorial/PCB.htm#Solid-Region-in-PCB

I can confirm that it is possible to place a single sided pad over a double sided padded through plated hole *with no Net or DRC errors*. To achieve this, the single sided pad must have: 1. no net name assigned to it (`Net` field must be blank); 2. no hole in it (`Hole` diameter = 0) I have not checked exhaustively but it looks like the minimum value of (Pad diameter - Hole diameter) is about 0.115mm. The width of the resulting copper annulus is therefore half of that value.

I have an existing layout, done in Altium. I am attempting to move it to EasyEDA, since I made some changes to the design and did the schematic in EasyEDA. It has some double sided pads under a metal TO-18 package that sits right on the PCB. Thus, on the layout the pads on top have been made just larger than the holes, to avoid shorting out to the metal package. I need to reproduce that feature. I am guessing I will have to use a gerber editor to get it done then.

I don't see why you would have to use a Gerber editor. The techniques I have described above will allow you to reproduce the pads you want. If the pad annulus under the TO-18 can is too wide then can you not simply make the pads for this device single sided on the bottom only? If they have to have almost zero annulus under the can then clearly they have no tracks to them under the can either so on a double sided PCB, it will not matter if the holes for the device pins are non-plated through with a pad on only the bottom of the board.

Good point. I should have thought of that myself. :-)