Yes you can do all three you have asked for. It is to long to type and you will be better served if yuo contact Customer Service Department directly.
For item 1 go to Design Rules - Nets - select Net - select Clearance Icon and you can change Clearance to all items or select only the box intersecting Copper and Pad (true hole) and/or Copper and SMD (surface mount pad) and enter the value for new clearance.
Answer for 2nd
Make changes and repour.
Answer for the 3rd
Change Pad stack from ROUND to OVAL
Select ROUND to Thermals/ OVAL to Flood over.
1) I'm attempting to do a copper pour on the top that acts as a ground plane. Some of the pads on the top layer have 100V so I would like to make sure that I have the proper clearance between the ground plane and the pads to prevent arcing. When I change the clearance values in the Design Rules, it seems that all pads (including the ground pads) on the components adjust to that clearance. I only want the non-ground pads to follow this clearance rule. Any suggestions?
--> You started out correctly, now go to Setup-Design Rules, click on the "Net" button and select the signal(s) you want a tighter clearance to, and set the sopper to pad clearance to what you want. Or, if you have extended rules, set the defaults back to the tighter clearance do a conditional rule for GND (and any other relevant signal) to the surface layer and set the GND to copper clearance to what you want.
--> [added] Or - Put the relevant signals into a class, and set a conditional rule for the top layer to that Class with the pad to copper rule set to the expanded size.
2) How do I remporarily remove my copper pour so that I can make changes to my traces and then repour?
--> SPO if you're using a Split/Mixed plane.
--> PO if you're using a Copper Pour.
3) How do I remove thermals from some pads on my board but not others?
--> A couple of ways, the way Vinay said (using oval/round pads) or select the relevant pads and modify their padstack (set the thermals to what you want) as needed.