If the via is part of a footprint you can change the style by selecting it and choosing an alternative pad style.
Having trouble working out what you mean. Surely, if the thermal is set up in a particular way in the technology form, then pouring copper can only result in that set up applying to all thermals in that area? See my attachment. I really need the two smaller holes to have smaller spokes.
When you referred to thermal via I thought you were needing to untent a via for a via in a thermal pad, hence I was referring you to where I'd written how to have tented and untented vias in the same design.
I normally have vias unisolated from templates and copper pours.
To get around your problem you could change the via to a free pad (insert > free pad) then add the free pad to the required net, then in Setup Technology
1. Create an attribute in the PCB design where the usage is set to "Pad", for example: "thermal_45deg_0.30mm-width".
2. Create a new line style for the new spoke width you want to use, for example: "thermal-relief-spoke_0.30mm".
3. Under Rules - DFM/DFT, and Thermal, click New and create a new rule where: Attribute Name = thermal_45deg_0.30mm-width Match Value = 0 Applies To = Via Spoke Style = "thermal-relief-spoke_0.30mm"
Then Apply and OK to close the Setup Technology dialogue.
In the design select the Free Pad in question using the right click, select Pad Attributes and click New then select the attribute name thermal_45deg_0.30mm-width