You can offset the pocket inward the horizontal distance the v-bit will cut and run a pocketing toolpath on that vector using a small bit for the pocket like a 0.125 end mill and a large area clearance tool like your 0.50 end mill. Then run a pocketing toolpath using the v-bit and use the smaller end mill you used for the other pocket as a large area clearance tool, this gives you the correct relationship between the v-bit and the 0.125 end mill in both pocking toolpaths. Then when you run the toolpaths you run the Clearance pass with the 0.50 end mill, the pocket toolpath with the 0.125 end mill and last run the pocket toolpath using the v-bit. You don't run the Clearance toolpath using the small 0.125 end mill it was only used to get the correct geometry between all the bits.Looking great, as usual!
The only feature change I'd like to see in Aspire is to allow two rough clearance cuts before the final V-cut. Using a big bit does remove a lot of material quickly, but also leaves quite a bit of work for the V-bit to do in the flat parts that the big bit wouldn't fit into. If they allowed a second rough cut, say with a 1/4" or 3/16" bit to remove what the 1/2" bit missed you might save another 10 to 20 percent of cut time.
With a 45 degree bit, the offset to the bottom from the edge will be equal to the depth. Make an offset line, then profile inside it with smaller end mill. Use the rough cut for the 1/2" end mill to clear the rest. Now create another V-carve toolpath using that 1/4" or 3/16" bit as the rough cut but only use the V-bit part to finish off the edge carving. Much less bottom flat work left for that V-bit to do.