Holes circle milled

[foolsh]

why is it holes, circle milled can't get correct to size specification.either i get one whereby the upper part of hole is too big,but bottom part pin gage no-go.one reason i could give is cutter tip part wear out.another reason cutter almost as large as hole,so feedrate is too fast for it to cut.anybody got any suggestions?

[Tom Dorgan from American Precision]

I prefer to keep my cutter to no more than 2/3 of my hole size.. ie.. .375 hole I would use a .25 cutter. You will have to slow down on small holes. What type of machine you have will determine how fast you can cut the circle. My routers will do a .375 hole at 50-60IPM but most machines will not stay round at that speed. I also do depth cuts and make a finish pass at the final depth only. You might want to try making a finish pass at each depth if you are going very deep.

[Guest]

It sounds like your cutter might be atapered a bit.

 

Many carbide manufacturers have a taper spec on their tools, if this an extremely fusst diameter, you could try helix boring to negate the taper of the tool.

 

I have also found that if I need something with no wall taper Robb-Jack endmills are ground straight

 

Feedrate can also affect the hole size. If you are close to the size an small feedrate is going to be necessary.

[crazy^millman]

If you are trying to hold that close of a size I would bore it verse fitting with the endmill. Leave .003 and then bore it and should have no problem.

 

HTH

[doyleg]

If you are using the roughing option in circle mill, it roughs out at the same dia. as the finish cut but without d-comp. This may also be a reason for holes being too big.

[Troy Gossett Indepak Inc.]

+1 for Helix bore I use a small overlap and finish at final depth. You could also try cutting conventionally rather than climbing, the tip of the cutter will be more likely to cut oversize than under so I'd back your comp off and try it again.

[foolsh]

i will try all your suggestions and do a upcut with a small feedrate with multiple depth of cuts.i am also using cutter compensation as i don't want to keep running to the computer to change the program.but i am wondering if cutter compensation could be used,i am using a cutter almost as big as the hole,by the way the hole is dia.2.05(-0.01),i amusing 2 mm cutter.

[?Mark]

That's .0807 hole and .0787 cutter.

 

Ain't going to work like that. You're pretty much flexing your endmill. Try reaming or similar approach.

 

hth

[Colin Gilchrist]

You would need a 1.5 mm or smaller endmill for that hole size.