I have a footprint that requires thermal vias in the thermal pad plus specific paste pattern for the thermal pad (see the picture). This pad generates a bunch of hole near pad DRC errors which just annoys me to no end. Previously I was able to give the pads the same number which would work to bypass this error, however it doesn’t work this time around for some reason. You can see on the picture that I renamed all six paste “pads” with the same name as the thermal pad and the thermal via in the pad, yet it still generates the error. (To make a square paste aperture with rounded corners I had to make a cross with to rectangular pads and put four round pads in the corner). Am I missing something?
Noticed something else. When I match the number of the paste pads to the thermal pad (P$1) I get an additional error on the Unconnected tab. It claims that the pad on the paste layer is not connected 
I think I had a similar error, unresolved. The thermal pad is of type SMD. I then tried to “via stitch” using the “place tracks and vias” tool. It didn’t work. My theory is that the keepout of my vias was large and intersected the edge of the pad. Is that what you are doing, adding the holes as vias after you place the part?
As a workaround, I am trying the technique of adding a grid of through hole, square pads in a grid, in lieu of one thermal pad (as described elsewhere on the net. The problem I have now is that the paste mask doesn’t apply solder to the grid of thermal pads since they are of type TH. It seems like you have defined a pad (as a filled shape) in the paste mask layer??
You didn’t read my post carefully. You can’t place a via on a footprint pad and expect it not to complain about it. The right way to do it is to modify the footprint itself and to place two pads of the same number one on top of another. One would be an SMD pad the other a through-hole one. The key is to have the same pin number for both of them. My problem was that when you add a Paste layer only pad to the mix, then it starts complaining again even if it has the same pin number.
The solution to the problem turned out to be a simple one. Change all the Paste layer pads into Paste + Front Copper pads. Then the DRC detects them as the same net and stops complaining
Well people on IRC thought I should be able to place a via on a footprint pad. But you’re right, I had trouble with it, and defining the holes in the footprint IS a better solution.
I still don’t understand how you implemented a “paste layer only pad”. The properties of a pad include a type and a set of layers. Maybe I missed it, but I don’t see those details in your post.
Anyway, I found that you don’t need a “paste layer only pad” if as you suggest, you place a TH type and and SMD type pad with the same pin number. You can make the SMD pad a little smaller than the TH pad (say 80% coverage.) The SMD pad generates a shape in the paste mask (at least in the Gerbers) and the TH doesn’t. Maybe that’s not an ideal solution because you can’t see it in PCBnew, and it doesn’t have rounded corners.
Make a pad, select paste layer and in copper layer select “None”