How to convert a pin to only drill/hole for connector clamping in an updated footprint?

In your footprint, delete the "X1" and "X2" text on the Package Geometry/Pin_Number layer.  This will change them from pins to mechanical pins.  Mechanical pins don't need corresponding pins in the schematic symbol.

I try to delete these pins, but they seem to be deleted enterely from the footprint. The two cercles have also disappeared, so I would like to let here the cercles as a drills (so as mechanical symbol). I was working on this. I also will try with deleting as you say the text.

thanks Randy, I will tourn back explaining what happened with your suggestion.

I have done what you say, I deleted the text and the pins now are called "mechanical pin". I updated the pcb layout with place/update symbols option but this error is launched:

'CONNVMEST64PACACODADO' symbol starting to refresh: ERROR(SPMHNI-270): 2 pins found in the symbol in the physical design, but missing from library symbol. They are: X2,X1

It seems to still having the two pins x2, x1. But I don't know from where is getting this data. The schematic symbol has no x1, x2 pin, asi you can see.

Thanks to all of you!

I solved this problem following the steps below:

1. I deleted the pins.
2. After this, I went to the "add pin" item from bar menu and then I checked "mechanical" option from "options" right tab.
3. Then I chose the "padstack" that I want to put there. And that's how I had drawn my no electric holes. 

But even doing this way, it gives me errors when I tried to generate netlist and update the board. But I have faced this other issue as follows:

1. This launched that two pins have missmatched because the symbol hasn't two more electric pins. So I tried one more thing, that was to save this footprint with another name, as it was a new footprint.
2. Then I removed the old footprint file from schematic symbols and I linked the new one (the same draw but other name) to this connector symbol from the symbol library, schematic and lib cache.
3. Hence I started the netlist and update pcb board processes and voila. No error.

So, it makes me think that there was some issue with corrupted or mistaken data that was automatically generated in some translation file at the moment of original library translation.

Thanks for all of your suggestions. They still been so helpful.