What's new
What's new

Tool pull out on Threadmill

pitnut

Plastic
Joined
Dec 6, 2022
Hello all,

I am currently working with some 6061 2x2 square stock in a Haas DS30. Right now I am having a problem with my Thread mill (morse 1/4-18 NPT) (https://www.morsecuttingtools.com/catalogue/product/321272) pulling out of its holder. The tool sits in an ER25 collet which is fine, but that is part of an extension that goes into an epinger radial live tooling block and is held by a 3/4" ER32 collet. That extension keeps slipping out of the 3/4" collet.

I have tried retightening it and switching to another collet, both of which didn't help. Right now I'm in the process of adjusting speeds and feeds as I'm worried it was pulling because of too much load on the tool. It was initially programmed at 1000-1200 rpm and 20 IPM (96 SFM and 0.005 IPT) but the Mfg states in aluminum 750-900 SFM is ideal with an IPT of 0.003-0.0045. I tried turning it up (380 sfm and .0037 IPT) but due to my bar sticking out 3.25" I was getting a lot of vibration and noise. I also maxed out my live tool rpm at 380 SFM. I'm at a bit of a loss here as this part has had multiple runs of 200 parts done by others and this is the first time I'm dealing with this issue.

Does anyone have any ideas? I must be overlooking or have done something improperly in the setup as I am quite new and lack experience. I can update with any info or clarify anything I have said.

I don't believe the nut itself is loosening as it's still quite hard to loosen. The tool comes out about .008" after 6 parts. The Shank of the holder is quite smooth too, I'm going to double check its Dia. tomorrow.

Thanks for reading my wall of text.
 
Emuge STRONGLY recommends against using a thread mill in one ER collet, your setup uses 2 er's. It's obviously flexing, increase your rigidity and your issue will go away.
 
Are you cleaning the ER32 of oil and then tightening with a torque wrench?
With a sort of solvent, no just air blast. I will do that. As for the torque wrench, I don't have access to one that would work with this holder. I understand over-torquing can be just as bad if not worse than under-torquing?
 
Emuge STRONGLY recommends against using a thread mill in one ER collet, your setup uses 2 er's. It's obviously flexing, increase your rigidity and your issue will go away.
That makes a lot of sense to me. I am forced to use the collet in the live tool holder but I will try to find a more rigid holder for the TM with a set screw?
 
Last edited:
We have about 30-40 threadmills in service at any given time across all our machines and every single one of them is held in an ER collet chuck. In fact, I can't recall ever using any other type of holder for a threadmill, and I've never had one pull out.

Something is wrong... not enough torque, bad collet, bad collet nut, etc.

The tool sits in an ER25 collet which is fine, but that is part of an extension that goes into an epinger radial live tooling block and is held by a 3/4" ER32 collet. That extension keeps slipping out of the 3/4" collet.

It takes a lot of force to pull a 3/4 tool out of a 3/4 ER32 collet. Torque should be around 100 ft lbs.
 
I understand over-torquing can be just as bad if not worse than under-torquing?
With over torquing, you run the risk of the splitting the collet or damaging the threads.

But "worse" than under torquing? Not a chance. When collets crack, they still work until you disassemble them. When a tool pulls out of an undertorqued assembly, it can potentially damage the machine.
 
With over torquing, you run the risk of the splitting the collet or damaging the threads.

But "worse" than under torquing? Not a chance. When collets crack, they still work until you disassemble them. When a tool pulls out of an undertorqued assembly, it can potentially damage the machine.
I agree completely, most of my thread milling in much smaller than OP but there is no reason a collet setup shouldn't work.

Flex is one thing but pull out is another entirely. I have used 3/4 ER32 to hold endmills that spike my spindle load monitor without pulling out. I am guessing its isn't being tightened enough. I am not a turning center guy so there might be some limitation I am not aware of?

Keep in mind that collets and nuts are consumables and once they are out of life it's time to replace them.
 
I must be missing something or don't understand the dynamics of forces applied by a Thread Mill, but my first thought is it's mostly radial forces with axial forces being counterbalanced by the shape of the dual opposed cutting edge(s), so how is pull out even a problem?

My question... you sure you've got that thing programmed correctly?
 
I am of the feeling something is wrong with that collet or nut or something.

With that said, let me point out that when the "recommendation" is .005ipt on a threadmill, that's a straightline feed, not circular.

feedrate 20ipm when your tool is only going around in a ~.250 diameter circular tool path, you're going to be going way faster than 20ipm at the outer diameter of the hole.

Take a look at this document from harvey tool on calculating internal feedrate factors for threadmills. https://harveyperformance.widen.net/content/cmtvmjvfdu/pdf/SF_822700.pdf?u=1i9tm9

That pdf was for single point tools but the concept is the same. I did very rough estimates and you'd need to cut your feedrate by about 60%. Maybe more. I didn't look up the diameter of a 1/4npt but I estimate it's somewhere in the 1/2" range, and that tool says it's a 3/8 diameter.

That will certainly not help the pullout situation!
 
Just quick update. I swapped my radial drill and thread mill so I could hold the extension with a set screw and flat. The drill went into the ER32 with a different size collet and everything seems to be holding position now.

I think there was something wrong with the collets, they are of unknown age. I find a lot of warped collets/wrong size shanks stuck in toolholders. Going to look into a torque wrench adapter
 
Last edited:
I am of the feeling something is wrong with that collet or nut or something.

With that said, let me point out that when the "recommendation" is .005ipt on a threadmill, that's a straightline feed, not circular.

feedrate 20ipm when your tool is only going around in a ~.250 diameter circular tool path, you're going to be going way faster than 20ipm at the outer diameter of the hole.

Take a look at this document from harvey tool on calculating internal feedrate factors for threadmills. https://harveyperformance.widen.net/content/cmtvmjvfdu/pdf/SF_822700.pdf?u=1i9tm9

That pdf was for single point tools but the concept is the same. I did very rough estimates and you'd need to cut your feedrate by about 60%. Maybe more. I didn't look up the diameter of a 1/4npt but I estimate it's somewhere in the 1/2" range, and that tool says it's a 3/8 diameter.

That will certainly not help the pullout situation!
Using the calculations I ended up with 4.6IPM as opposed to the 14.8IPM, the threads do seem to have less chatter now.
 
I'm pretty sure the radial force at the cutting edge was causing the tool shank to walk, using the small amount of slop provided by a worn or damaged collet (bellmouthed).
 








 
Back
Top