Hey all, I am wondering if anyone has a solution for this more elegant than cutting a cross and measuring the width of my cut. My plan so far is to just make a program and cut a piece of scrap two lines per tool one vertical and one horizontal then labeling them with an engraving bit and renaming each of the tools with an approximate diameter.
So here’s an additional thought, If I probe with a pin but I have my cutters set up for precise dimensions are my offsets going to be wrong because I probed with a 1/4" pin when my tool dia is actually .241 for instance?
If that was the case and I probed with the tool instead would I have to probe in-between each cut that has a tool change and split all my programs up?
Additional context. If you have an endmill with an odd number of flutes, it could trigger asymmetrically from left to right, or front to back. Using the BitSetter with a dowel pin is the most precise way to set a zero in the horizontal plane. And you do not need to probe again between cuts. Once your zero is set in X and Y, it’s set for good.
Also, it is generally unnecessary to do the test cut you are suggesting Dean. Most endmills are within a couple thousandths of an inch of their nominal diameter, and your test is going to introduce more variables and have you chasing your proverbial tail.
If you are cutting wood or plastic, sometimes the slot closes up a tiny tiny bit as wood deforms out of the way. Or at a microscopic level, the cutter is ping-ponging back and forth in the slot from vibration. Or there’s a little runout and the cutter is carving out a wider channel than the cutter itself. Your margin for error with your tests is going to be no better than the tolerance of the tool from the factory. You’re likely to just make things worse.
Best practices for maximum precision in your parts is to run a light finishing pass after your main cut. IF after that point you determine there’s a systematic error in your cuts, you can consider endmill diameter variations. But unless you’re sending your parts to Mars, I just would not worry about this right now.
well to a degree right, If I measure my runout at the depth I want my cut to be, check how square my Z axis is and do a little math to .0005 and do the test cut in the material I intend to work with and do a finishing pass I shouldn’t be chasing my tail unless it becomes about machine rigidity correct?
It’s not really about going to Mars as much as it is learning the process.
A finishing pass needs some amount of residual material to cut. You can’t truly really do that in a slot that’s meant to be the identical width of the cutter. And in the real world, depending on whether or not you’re cutting on the inside of a pocket, or the outside of a part, there’s going to be some deflection in the tool, the machine, or the material. There’s lots of factors that affect accuracy, including backlash. And I feel like the way you’re going about this is going to end up attributing too much of the total error in the system to the cutter diameter, and you’re never going to be able to fully escape chasing your own tail.
If you really want to get a good reading on tool diameter, you need to cut out the middle man. Measure the tool directly.
Load a tool in the spindle, put a dial indicator on the shaft. Correct out runout as best you can, raise the spindle, and then measure the high points on the flutes of the cutter. Do some math to figure out the max diameter of the cutting edges.