Why do small endmills always seem to overcut?

mhajicek · Dec 26, 2019

I've noticed over many years and different machines of different makes, that small (say 1/32") endmills often overcut, and I need to raise them about .002" to .003" to make them match up with faces cut by larger (over 1/8") cutters. Today I'm matching a fillet cut with a 1/32" ball with a face cut with a 3/16" bull, and had to raise the ball .003", while every other cut in the program matched with no adjustment. I would say it's thermal growth of the spindle due to higher RPM, except the cut only takes a couple minutes and I'm running 1000PSI TSC. Centrifugal expansion of the CAT40 spindle would seem to work in the opposite direction, letting the holder pull up further (hence the pop on toolchange after.) Have you noticed the same thing, and do you have an explanation? Thanks!

Finegrain · Dec 26, 2019

Contact toolsetter that has a face not exactly coplanar with the mill's X and Y will measure larger diameter tools a bit longer than they should be. Also, IME ball endmills typically don't measure at the theoretical correct place, maybe because of the end grind is not ideal.

Optical toolsetter would not have any not-coplanar error.

Regards.

Mike

CarbideBob · Dec 26, 2019

Three thou seems a lot. How are you setting tool lengths?
Different methods over those years and many machines or the same technique being used?
Something strange going on here so a good thread and very good question.
I'll normally hit 1-3 tenths when matching.
Let's also be aware of surface finish high/low dims with the bigger guy and how we want a blend to happen but this is so huge and way past that.
The bigger tool deflects if well loaded so it becomes a tiny bit shorter but not on this level.
Thermal would not approach this amount. Taper expansion also.
Something is fishy in Denmark.....

Is this error always one sided or does it go the other way for you sometimes even if very rarely?
Bob

litlerob1 · Dec 26, 2019

I'm sure Mike is right, but I have no idea what he means by "Coplanar", or not Coplanar. If it were not Coplanar with Z, (except were talking about "Tiny") I'd understand, but not with X and Y....?

I always assumed it was because it pushed the Collett up a little. But I've noticed it also.

R

mhajicek · Dec 26, 2019

I'm currently running a 2015 Haas VF-3SS 15K RPM with the contact tool setter. I just checked it with an indicator and there is a depression in the middle of the tool probe that would account for about a thou of it, but not the other .002". 5-10 years ago I was programming for four Kitamura HMC's (a 300, two 400's, and a brand new 500 with CAT50 dual contact) and a Quaser VMC, some with contact, some with laser. Same issues with all of them; larger facing cuts and tiny ball endmills were always about .002" mismatched.

CarbideBob · Dec 26, 2019

Is this a small ballnose tool problem? If you go to 1/16 or 1/32 flat end do you have the same error?
One can not pick up the high on a ballnose without rotating on the probe. There is only one standing tall and proud.
Lasers and machine vision basically suck the hind tit at any type of tight measuring here unless very carefully designed for the application.

All that BS about measuring aside, said 3 thou is so simply huge to the point of something here going on the OP is fighting and should not need to comp around or fiddle fart with.

Let's try to make it all go away or define some rules you and the OP can use in the CAM or tool length side.
Bob

mhajicek · Dec 26, 2019

I'm ordering a new contact tip for the toolsetter since I did find a dip in the middle, fixing that can only help. But I do think there's something else going on, either inherent to the CAT spindle type or to the machine geometry in general since I've seen it on several different machines and all the same direction and very similar magnitude.

I haven't tried matching faces with a small flat EM that I recall, so that's up in the air. Good question, I'll have to experiment with that. I don't see why you'd have to spin a ball EM to measure its length though, since it's hitting a 1/2" diameter flat (supposedly anyway) probe face. Diameter, sure.

CarbideBob · Dec 26, 2019

And you think when we swing these edges around to center there is not runout?
Plus the tip is gashed, some edges never make it.
Give the cutting tool guy some room to play and pick up my high spot.
Yes 3 thou is so way outside unless you oriented just so terribly bad on a ballnose tool.
It's a circle with flutes, get into those 45s and and it does not look or check the same. Optical compartor will show you that.
More BS and still this does not solve your problem ....so :willy_nilly:

and you can see all the good I am.
Bob

Larry Dickman · Dec 26, 2019

mhajicek said:
I'm ordering a new contact tip for the toolsetter since I did find a dip in the middle, fixing that can only help. But I do think there's something else going on, either inherent to the CAT spindle type or to the machine geometry in general since I've seen it on several different machines and all the same direction and very similar magnitude.

I haven't tried matching faces with a small flat EM that I recall, so that's up in the air. Good question, I'll have to experiment with that. I don't see why you'd have to spin a ball EM to measure its length though, since it's hitting a 1/2" diameter flat (supposedly anyway) probe face. Diameter, sure.

I haven't had a problem with tool setter dips in a long time. Perhaps they changed the material? But we used to, so we would send them to our tool grinder and have him clean up the face. Lot cheaper than a new one.

mhajicek · Dec 26, 2019

New one's $94 through Productivity. I figure I'll dress the old one to have a spare. Still not seeing how spinning a ball endmill could effect the length touchoff. Sure one flute may be protruding more than the others and there may be a gash cut, but that high point is going to be at or very near the center of that 1/2" probe tip in any orientation. Spinning it will only move it in the X/Y plane (unless my machine were way out of tram), and I'm seeing mismatch in Z. I certainly do spin my indexable cutters and anything larger than the probe tip when setting length.

BROTHERFRANK · Dec 26, 2019

Are you using a Renishaw TS27R type probe that tilts down at an angle while measuring? I am thinking that a small tool will contact at the center and larger tools will contact at a different point on the probe face relative to the pivot point. Can you test by touching off other small tools like drills and spot drills and then touch your tools to a gage block and verify the repeatability? Then check larger tools to gage block and compare?

mhajicek · Dec 26, 2019

BROTHERFRANK said:
Are you using a Renishaw TS27R type probe that tilts down at an angle while measuring? I am thinking that a small tool will contact at the center and larger tools will contact at a different point on the probe face relative to the pivot point. Can you test by touching off other small tools like drills and spot drills and then touch your tools to a gage block and verify the repeatability? Then check larger tools to gage block and compare?

Using one of these:
OTS 3D touch-trigger tool setter

That's a good idea, I'll try that.

EmGo · Dec 26, 2019

I would think it has something to do with the stinky little things bending more ... but trying to imagine in what way, with a ballnose

With a flat bottom, I can see the mill bending a little which would make the leading edge cut lower, but a ball end should not do that ...

Does climb or conventional make any difference ?

mhajicek · Dec 26, 2019

EmanuelGoldstein said:
Does climb or conventional make any difference ?

Not so as I've noticed. Hard to imagine a 1/32" carbide ball stretching .002".

Milland · Dec 26, 2019

Next time you're calling up the small cutter after a large, could you try running it briefly with RPM derated to the same speed (with relative feed correction) as the large? Just needs to be long enough to establish a cut path that can be checked out for height mismatch.

If it's still off then it sounds like some systemic fault in the auto tool touch off, which maybe you've fixed with a new contact.

5 axis Fidia guy · Dec 27, 2019

I am not a Hass guy but I will throw this out there. Back in my Fidia days there were not only heat compensation values, there were elongation values. With the comp off, the spindle at 2k rpm's and at 24k rpm's had about .002 elongation, this is different from the heat values, and it happens instantly, and with every spindle to some degree.(The centrifugal force takes up any clearance in the bearings). Maybe, just maybe this parameter is turned off in the control, or it's not an option. Either way, the only way to get good blends is the set your tool length AT THE OPERATING RPM'S with a laser. This should be standard practice with any machine.

dstryr · Dec 27, 2019

When you picked up the .001 dip in the center what size indicator were you using?
if you dont use the sensor to rotate to find the diameter of larger tools you could always shift the center point over .030 in one direction and test the length measurements?

Easy solution would be to create a seperate measurement program for "smaller" ball endmills and calibrate the lengths with your tool once you adjusted it the .003...
Sometimes we dont always need to find out "why" but just fix things so they are good to go.

lowCountryCamo · Dec 29, 2019

We see the same thing with small radius tip pencil cutters. I always attributed that to smaller tools cut with less pressure so there is no push off. Our situation is with 5 axis trunnions so flex does come into play.

Chris59 · Jan 2, 2020

lowCountryCamo said:
We see the same thing with small radius tip pencil cutters. I always attributed that to smaller tools cut with less pressure so there is no push off. Our situation is with 5 axis trunnions so flex does come into play.

That is what I think too and in combination with the ball grind not making in to the full radius at the very tip.
But I've never seen .002-.003. I usually only have to raise it .0002 to .0005"

G00 Proto · Jan 2, 2020

I always assumed (without actually thinking hard about it), that the higher the RPM the more cutter expansion I had. I guess I don't even spend much time thinking about it any more. For instance, I use a dial toolsetter to set me Z tool heights on mills. Then I'll use the exact same dial to set the Z height of the part. I know from experience that my face mill will "grow" .001, and my small endmills will grow about .0025". I attribute this to the RPMs making the assembly longer, and the smaller tools not having as much push back (plus I think I have some implicit hysteresis on the way I set part Z zero). In your case I wonder if your TSC isn't exacerbating the problem. You have 1000 PSI (holy shit). Lets just say that is pushing against the entire toolholder effective area... that's 556 lbs of force. On a little tool, its gotta pee out a little hole... on a big tool, there is less restriction.

Why do small endmills always seem to overcut?

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Diamond

Titanium

Diamond

Stainless

Diamond

Diamond

Diamond

Diamond

Stainless

Diamond

Stainless

Cast Iron

Hot Rolled

Similar threads