Programming countersink and chamfer tools

Just wondering how everyone programs a "keo" single flute csink tool. I always have to program short and let the setup person sneak up on the correct diamter of countersink. Looks like there should be a more defined way of doing this. Same thing for chamfer tools.

Thanks,
Tjay

One way would to find the distance from the end to the desired diameter via a comparator (shadowgraph).

Another if you can follow my logic....

Draw a 'Vee' with your cad/cam at the angle of the cutter. The point to be X000, Y000. Draw a vertical centerline ('x'000). Draw a parallel line 1/2 the diameter at the bottom of the cutter. Trim the pointed area of the 'v'. Move the bottom to 000 ( my cad/cam would be 'Y'000.).

Save as a master.

Required diameter divided by 2 becomes the parallel distance from the 'x'000.

Tangency point of this line and the cutter angle becomes the exact 'z' distance form the bottom of the cutter.

Just remember probably there are no 2 c'sinks identical.

Is that helpful?

A single flute countersink probably has an eccentric point. This is difficult to see on a relieved single flute tool, but is easy to see on a 'zero flute' countersink.

This makes setting the tool length offset a bit of a challenge because the sharp point of the tool is not truly the conical zero of the cutting edge. Thus, the setup man is probably always going to have to make an adjustment until you and he agree on how a specific tool cuts.

Set to a datum dia., easy on an optical tool presetter but can be done on an optical comp. Then program off the datum point. Resharpened center drills, blunt drill points and angle variation becomes irrelevant.

start shallow, manually change the program at the machine if you don't have a $20k optical tool presetter.

My best suggestion is to ditch countersinks, if you're running 82 degree hardware, get 82 degree spot drills. A little trick for 82 degree tools is to shoot for 10% more in depth than you'd would with a 90 degree spot drill (which has a 1:2 ratio, theoretically). You'll usually get it within +/-0.010", then adjust accordingly. Out of luck if you're running 100 degree hardware though...

From my experience, single-flute countersinks are pretty useless in CNC. Like HuFlung said, they run eccentic...so they are hard to take into account what they will do. And 6-flutes countersinks are ground flat with a big minor diameter, so it's a crap shot what you'll get in size as well.

Chamfering tools, it's usually trial-and-error with adjusting the minor diameter offset or the depth. I'm always on the big side with the minor diameter so that the tool doesn't gouge the part, so my adjustment's almost always with depth. Corner radius tools are the worst!

seems USA problems are the same as Australia's