Newb question about holding sizes (CNC lathe)

vettedude · Aug 25, 2014

I work with allot of families of parts.

When i shift from a part in say the 6" range to the 4" range i am usually off on diameters by 0.002-0.005.

What gives? Same tools, same inserts (We use Poly Crystalline Diamond inserts only, i do not believe it is possible to wear the pcd after 30 parts), nothing changing other than the major diameters. I am using tool nose radius offsets, but the parts is the same cross section only a different major diameter. If i change to a different part family the dimensions are off a bit more significant.

Am i missing something or is being off by 0.002" between different parts typical?

I fix the problem by changing the tool compensation, and life is good again.

ewlsey · Aug 25, 2014

Many things could be wrong. A bad ball screw, a bad thrust bearing, incorrect backlash compensation, or incorrect ball screw mapping.

It might be time for some maintenance.

vettedude · Aug 25, 2014

ewlsey said:
Many things could be wrong. A bad ball screw, a bad thrust bearing, incorrect backlash compensation, or incorrect ball screw mapping.

It might be time for some maintenance.

the machine is 6 months old.

jrmach · Aug 25, 2014

cutter height ?

SeymourDumore · Aug 26, 2014

jrmach said:
cutter height ?

Yupp, that is the first thing to check.

And then material, speeds, feeds, features.
Then what is the leftover after the rougher.

Vette, when it comes to turning, that is just the fact of life and don't let anyone tell you otherwise.
If it's a production item, turn the frickin' thing, measure it, throw it away and adjust.
If it's a onesey, set your offsets .01 over, measure, adjust, recut....

I'm sure there will be some schmucks coming to chime in that they have a formula for this and that and they'll get a guaranteed good first part
outta the gate.
All bullshit!

If you can afford a lost part, run it and adjust after.
If you cannot, then adjust, measure, re-adjust, measure again....

hanermo · Aug 26, 2014

Seymore - I agree on your theory bud NOT the numbers.
0.005 == 0.10 mm.
NO WAY is any modern semi ok cnc lathe off by 0.10 mm in diameter.

0.05 mm -maybe. 0.02 mm yes. 0.10 mm - absolutely not.
Unless the material is screwy, plastics maybe ? or the feeds/speeds/inserts etc.
Problem with program maybe ?

Suggest testing with alu or free machining steel (need to have suitable inserts).

If the probelm still repeats, the manufacturer should fix it for free.
Absolutely not acceptable to have a 0.10 mm error in diameter (on a 4" to 6" variation, note !).
Something is wrong somewhere.

sable · Aug 26, 2014

I agree with those who say this is way too much for a 6 month old machine ( what is it ?) .

A trick that a fella showed me was that instead of changing the tool offset to overcome this ,you change the size in the program ,this means that the offset stays the same for every part so when you run a different job the only thing you change is the program ,of course you have to do this if there are significant changes in diameter or the tolerances are tight ( assuming the lathe is not absolutely spot on).

gregormarwick · Aug 26, 2014

What direction is the error? If the centre height is wrong (doesn't really matter in theory whether high or low) then the part will become oversize as you get smaller.

If your parts are going undersize as you get smaller then you can probably rule this out.

I'd like to believe it's not pitch error. 0.1mm over 25mm travel is extreme. So extreme that the ball nut would bind on the screw, unless it was really worn out.

Seymour is absolutely right that this is a fact of life when turning, but your error over such a small travel is too much.

Bobw · Aug 26, 2014

The first thing I thought was tool height when I saw this last night, then I drew it up real quick. From a 2" rad to a 3"rad, a .003 difference
would put your tool about 1/8" too low (or high). That just seems too far off, somebody would have noticed that by now, maybe?

Other thoughts, besides something totally screwed up with the ball screw, or how the machine is moving the ball screw..

Different diameter parts are different lengths, and the head stock is out a bit...

Running proven out programs and the feeds, speeds and possible varying amount of stock left for the finish is causing the difference...
As in things are different in different programs.

Somebody has a micrometer that could really use some calibrating?

DMF_TomB · Aug 26, 2014

measure the X axis or diameter direction with a dial indicator. 1.000 movement should read 2.000 on diameter of DRO
.
i had a lathe that of course their was a calibration check of DRO and it was off. i retested it, put in compensation factor per the procedure in the manual, and retested to confirm i did it correctly.
.
what i found out was a button on control that could turn the compensation factor off and if DRO was switched off the compensation factor was turned off by default. it was no big deal turning it back on. i just was not aware originally what on control indicated the compensation factor was active.
.
a new machine should have it's DRO checked with a dial indicator or gage blocks to confirm 1.0000 of movement reads as 1.0000 (2.0000 on diameter screen).......... maybe it is ok, but checking it should take what a few minutes at most and then you will know if it passes a calibration check.
.
on some machines it is considered normal and expected to check the Digital Readout at least once a year.

Mtndew · Aug 26, 2014

vettedude said:
the machine is 6 months old.

That doesn't necessarily mean that it's not your machine. Although chances are that it isn't.
Have you double checked to see if it's still level? Sometimes they settle after the 1st 6 months.

Try indexing the turret 180 degrees and using a totally different toolholder and see if the problem is identical.

yardbird · Aug 26, 2014

SeymourDumore said:
Yupp, that is the first thing to check.

And then material, speeds, feeds, features.
Then what is the leftover after the rougher.

Vette, when it comes to turning, that is just the fact of life and don't let anyone tell you otherwise.
If it's a production item, turn the frickin' thing, measure it, throw it away and adjust.
If it's a onesey, set your offsets .01 over, measure, adjust, recut....

I'm sure there will be some schmucks coming to chime in that they have a formula for this and that and they'll get a guaranteed good first part
outta the gate.
All bullshit!

If you can afford a lost part, run it and adjust after.
If you cannot, then adjust, measure, re-adjust, measure again....

I agree with this fella. ^^^

If I need the first one on the money I always leave material measure then rerun the finish tool. Thats just the way it is.

Brent

bw_4000 · Aug 26, 2014

Are you sure that the programs are correct?

npok · Aug 26, 2014

Does the variation happen consistently throughout the day? It could just be a matter of the machine moving around as it warms up.

75sv1 · Aug 26, 2014

My take is how far do the parts over hang from the chuck? If more that 1-1/2 ot 2 X the diameter, then I would expect flex in the part from a 6 inch diameter to a 4 inch diameter.

SeymourDumore · Aug 26, 2014

Guys, I'm not sure why some of you think he has a problem with his machine, or that .002 variation from one FAMILY of part to the NEXT
that is 2" ( 50+mm ) smaller/larger is too much.

I may have missed it, but he doesn't seem to complain about not being able hold consistant tolerances, nor that his part varies between different diameters.
All he said was that one part of 6" is correct, but then the next setup - with all else being the same - is off by .002 or so.

I don't know about you guys, but I often get about that much difference running the same material even, and not only on one machine, but
any machine.
Not to say that it is the rule, but when it comes to turning I never expect the first part to be spot on after a setup switchover if the tools remained from the previous setup.

Just think back for a second if you've ever experienced that a roughing cycle on one part but different diameters leaves different amounts for finishing?
In fact that is one of the things I like about the Haas and Mits G71 cycles, as one can define an I and K in addition to the U and W, because that is the only way to have
a consistant amount left for the finish tool.
Short of that, I run a semifinish tool whenever I have to hit something in the 'hood of .0005 total.

toolsteel · Aug 26, 2014

I have ran into this before.......I have always written it off to the center height of the tool not being perfect......there are many things that need to be absolutely perfect for this not to happen. From the insert to the tool, the holder, the turret, the angle of the slant....etc. That doesnt even get into the mechanics of the machine itself (backlash etc). For my own sanity.......I blame it on the fact that the world is imperfect.......most things are not entirely flat, nor entirely round.......Make a note of how the change in diameter affects the part and compensate the correct direction so that worse case scenario you make an offset and re run your finish tool.........BTW.....changing bore sizes by an equally drastic amount will probably have a similar effect.

yardbird · Aug 26, 2014

SeymourDumore said:
Not to say that it is the rule

Well I kinda do. If it cost more in time than material to dial in the first piece. Run one adjust for the next. If not then I wouldn't chance it even tough its kinda a PITA when you were just making good parts. When I make a boat anchor I want it to be for some other reason then I didn't measure and dial it in. I think you made a lot of good points in the entire post.

Brent

Limy Sami · Aug 26, 2014

X 2, and when you're running parts out of PEEK, use Acetal for the set up parts

DefeatingZero · Aug 26, 2014

Just back off all your tools about .010" radial, run the whole thing, adjust the roughers back .010" and finishers to where they need to be to be at size. Then just rerun finishers. Yardbird is right, if it costs less to adjust and rerun then do that, otherwise just make scrap then adjust. it all depends on what your time and materials cost. If you have no room for scrap, be sure to back off and rerun!

Newb question about holding sizes (CNC lathe)

Stainless

Diamond

Stainless

Titanium

Diamond

Titanium

Titanium

Diamond

Diamond

Diamond

Diamond

Titanium

Cast Iron

Aluminum

Hot Rolled

Diamond

Titanium

Titanium

Diamond

Plastic

Similar threads