Fusion 360 has a setting for wear compensation. Does gsender have a place to set this parameter. I ask because my actual hole size is smaller than my programmed hole size and, as I understand it, the wear compensation is a strategy to mitigate the issue.
@Jonathan Not as far as I know. This would be a feature of your CAM software, which gSender is not (that said, gSender can create g-code for surfacing),
The best way to correct this would be to use a caliper to measure your tool diameter, and then enter that diameter in your CAM software’s tool database. You then create the g-code from that.
in Vectric vCarve, you can use offsets for some of the toolpaths. This can be a good strategy for holes or dadoes.
Measuring the bit diameter and entering that into the toolpath setup gets you close, but measuring the kerf created by the tool in the material you’re cutting with a caliper is more precise.
It’s pretty simple in Vectric software. In the toolpath setup click the Edit button and change the bit diameter to the actual kerf width. It does not change the diameter setting in the tool database, only for the toolpath you’re currently working on. Very handy when you’re working with inlays.
Of course you can also change it in the db if you prefer, but be aware that if you swap the bit for a new one it may have a slightly different diameter.
I think measuring the kerf is the way to go. I think it was @TDA, with PreciseBits, that said it was more accurate and that even if your careful your probably doing some damage to the cutting edge of the bit if you measure it with calipers. Measuring the kerf would also compensate for runout, if I’m not mistaken, whereas measuring the bit wouldn’t.
When he said that it made me wonder if using a block to zero was doing damage to the bit on a small scale. But then again a touch block is made of softer material than calipers. What do I know? Microscopic damage is above my pay grade so to speak.
There was another thing that TDA said which made sense but I hadn’t thought of until he said it. If your bit diameter is the same as the shank diameter it’s probably undersized because if a manufacturer buys 1/4" round stock and then cuts and sharpens it some of that 1/4" is going to be lost during sharpening. I haven’t a clue if some manufactures use larger stock and mill the whole thing down to compensate for that.
The OP was not asking about how to measure the holes.
If your hole is undersized from what you have programmed in Fusion then if you change the tool wear in Fusion it should compensate the GCode and therefore make the hole larger. Alternatively, and this is what I do, I just go back to my model and enlarge the hole. You could also do an offset on the hole perimeter and label it as tool offset. Thats basically what the tool wear compensation is doing , But remember the tool compensation will effect the ENTIRE MODEL or atleast whatever you are cutting with that tool.
Grbl does not support tool comp. I know what my bit diameter is by machining a 1 inch circle then measuring. If the circle turns out 1.003 inches. Then your adjustment is HALF that. I go negative with a stock to leave in fusion. For example I use .002 clearance on inlays, so if the 1 inch circle is 1.003, I go negative .0035 inch to give me the right clearance.