Hi
I've been using Eagle fora long time but there are many features of it I do not use - one is the solder restriction layers. Instead, I make a circle in the reference layer to show the clearance I want around a hole or other pad. For mounting holes, I use 0.125", which is 3.175mm. I'm using 4-40 hardware which is about the size of M3 but with coarser threads - it is what's available here.
I drop the hole, then move the reference circle over top of it. The circle has to allow for the bolt head diameter, spacer diameter, nut diameter, PLUS some isolation space to the nearest trace.
I am often designing tube stuff, so voltage clearance is important. I use a conservative guide of 0.12mil/V. if you take the mils (0.001") and divide by 0.12 you get the voltage spacing. For example, a 25mil space between a bolt head and a trace provides 25/0.12=208V of isolation. There are way more aggressive (less conservative) guides than this and I've seen those boards burn.
It used to be that PCBs began as copper-clad fibreglass sheets. These had to be etched and drilled in two steps. Drilling accommodates holes that will be vias AND mounting holes, then the holes needing plating are done as a separate step.. These days, the boards are blank fibreglass, holes are drilled and copper is sprayed on with plated holes plated at that time. I believe drilling of through-holes and plated holes (vias) is one step, but in any case, no board house charges extra for mounting holes.
When you select the Holes icon on the left-hand menu, a drip-down list of hole sizes appears. Scroll down to the size you want. if you do not see the size, choose one anyway and drop it on the board, then go to the Change icon (wrench) and select drill, then scroll to the bottom of that list and type in the diameter you want. Then cursor over the hole on the board and click on it - it will change to the new size. The next holes you drop will be this size, too, unless you select a different size. Alternatively, you can do the Change drill size before dropping any holes, then select the Holes icon and they will be the new size.
With my reference circle, I make one to the side of the board, then move it over the first hole. Then I use the Copy icon to makes copies of it to drop over the other holes. When you drop the holes, use the largest grid possible that positions the holes where you want them to be. My holes are usually on a 0.1" grid where traces may be on a 0.0125" grid. You can move back and forth between different grid sizes as you draw the board outline, drop holes, drop components, and then add traces. The traces will need the finer grid to allow for odd pin centres of components, especially if you mix metric and inch footprints.
Note also, that the "i" (information) icon allows you to click on any hole, component, line, trace or via and see the information about that item. You do not have to enter x-y data to see this info. The information window opens when you click on the item, then you click it off by pressing the "okay" button inside the window. Then cursor to other items and see their info. Select STOP to exit the information mode.
Remember to SAVE frequently - every few steps of whatever you are doing. It is easy to lose hours of work if Eagle crashes.