Advanced V-Carve -vs- PVC
I recently wrestled with getting a good finish using advanced V-Carve on solid PVC and thought I’d share my results.
A typical Advanced V-Carve path cuts the area pocket first, then engraves the edges, then goes back & picks out the corners. What I found is the Vee-Bit tends to bend or push the material away from the edge as it cuts, leaving a nasty looking web or burr of material
My first thought was, “What if I reverse the order & run the Vee-bit first, and then the area pocket?
It didn’t work & gave very similar results.
So then my next thought was I needed to cut into the bottom corner enough that there is no material to peel off.
Ending up with a shape something like this.
Another thing I didn’t like is the cleanup passes the Vee-bit did in the corners where the area pocket tool wouldn’t reach. (essentially the “rest milling” part of the path). Not too bad on this square example, but on other jobs with sharper corners & narrow areas it could be quite a bit.
So I decided to make my overlap enough to clean up at least a square corner
This calculated out to about a 0.0175” offset for a 1/8” tool.
To accomplish the overlap I created an “undersized” tool in CC. 0.0175 on the radius = 0.035 on the diameter, so subtracting that from 0.125, I get 0.090.
I set up my advanced Vee-Carve like this
Here’s the finished product.
I set my Z height about 0.005” below the top of the stock to allow for surfacing afterward. After the V-Carve I masked the edges & painted it black, then used a surfacing bit to take 0.005” off to return the top surface to white.
And yes, that’s the QR symbol for my home wifi. So if you’re coming over just click on it, you won’t have to ask. 