Has anyone made a thread mill?

[Freedommachine]

This is a new one for me. I have to make a replacement adjuster screw for an obsolete piece of equipment. The screw is basically a set screw with a non-standard trapezoidal thread form that looks like this:



It comes out to a 1.5mm pitch but my lathe cannot cut metric threads so thread milling is my only available option.

I picked up 3 feet of 5/8" dia O1 so I should have plenty of attempts to get the tool geometry correct. My plan is to turn the basic thread form on the lathe; cut 4 teeth into it on the mill while holding the tool in a collet block, relieve the backside of the teeth on a bench grinder and then heat treat with oxy/fuel.

What do you guys think?

 

[Vancbiker]

I’d be looking for a favor from a friend with a CNC lathe or an engine lathe with metric change gears. Seems to me that would be easier and faster.

 

[lobust]

TR threads fall into the same trap as ACME, in that they can't be threadmilled unless you can tilt the tool axis perpendicular to the lead angle either with a tilted rotary or 5ax.

If you don't have access to a suitable lathe you have one last course of action:

If you use this calculator http://bilar.co.uk/cgi-bin/change-gear-calculator.pl

You can figure out if any undocumented assortment of your changewheels will get you close enough, or figure out which wheel(s) you would need to add to your set to make it work. If you have or know someone with a 3D printer you can just print up a changewheel to get the job done. Alternatively buy an off the shelf gear and machine the centre to suit.

 

[MwTech Inc]

What do you guys think?

I think you better charge good for this .....
Going to eat up a lot of time fussing around....

 

[Mud]

If you use this calculator http://bilar.co.uk/cgi-bin/change-gear-calculator.pl

Cool calculator. Have any more similar? I'm looking for a way to calculate gear shaper change gears from a known assortment.

 

[lobust]

Cool calculator. Have any more similar? I'm looking for a way to calculate gear shaper change gears from a known assortment.

I found that one just recently via google search when I was trying to figure out how to cut a 4.5mm pitch on my HBM.

I did find some others too but I didn't bookmark them as that one worked really well for my purposes.

 

[Freedommachine]

TR threads fall into the same trap as ACME, in that they can't be threadmilled unless you can tilt the tool axis perpendicular to the lead angle either with a tilted rotary or 5ax.

If you don't have access to a suitable lathe you have one last course of action:

If you use this calculator http://bilar.co.uk/cgi-bin/change-gear-calculator.pl

You can figure out if any undocumented assortment of your changewheels will get you close enough, or figure out which wheel(s) you would need to add to your set to make it work. If you have or know someone with a 3D printer you can just print up a changewheel to get the job done. Alternatively buy an off the shelf gear and machine the centre to suit.

Well, I'm glad I asked before learning the hard way, thank you. Looks like I'll have to find someone who will let me use their lathe.

I really need to just buy one but I'm saving my shekels for a cnc turret lathe.

I think you better charge good for this .....
Going to eat up a lot of time fussing around....

The device is my own so unfortunately it's a government job.

 

[Barbter]

Is there much meat around the female thread so you can tap it bigger and then use a standard screw

 

[MwTech Inc]

following along Barbter's thinking....you could use a thread repair insert like this (90245A035 McMaster)
If part is delicate lose the tangs and lock tite it.
If the wall is thin, chuck it and lose the outside threads and "tig" it in.

 

[Dualkit]

You should list your location in case someone here is close by.

 

[Freedommachine]

Is there much meat around the female thread so you can tap it bigger and then use a standard screw

Nope. It's only half of a female thread, it operates very similar to a toe clamp. This is the part that the trapezoidal threaded set screw engages with.

 

[Freedommachine]

You should list your location in case someone here is close by.

Portage county Ohio.

 

[Dualkit]

Portage county Ohio.

I actually know someone close to you but he isn't one of the favor trading type. If it was me I would make you one on my CNC as long as you were buying the pizza and beer.

 

[Freedommachine]

Finally! I got it done.



I thread milled it.

@lobust Idk who told you it wasn't possible to thread mill trapezoidal threads but it turns out to be a fairly common thing. Acme thread mills are available as an off the shelf item from a few different mfg's

My thread was even more difficult because it's only a 15° pitch angle - half of what an Acme has. I made a thread mill from a broken woodruff key seat cutter by circle grinding a 7.5° angle on either side using a dremel tool mounted on the lathe compound. It won't win any awards but it's in spec and good to go after a little light deburr.

 

[Kustomizer]

Good show Sir!

 

[lobust]

Finally! I got it done.



I thread milled it.

@lobust Idk who told you it wasn't possible to thread mill trapezoidal threads but it turns out to be a fairly common thing. Acme thread mills are available as an off the shelf item from a few different mfg's

My thread was even more difficult because it's only a 15° pitch angle - half of what an Acme has. I made a thread mill from a broken woodruff key seat cutter by circle grinding a 7.5° angle on either side using a dremel tool mounted on the lathe compound. It won't win any awards but it's in spec and good to go after a little light deburr.

First of all, good on you for ignoring me and getting it done!

In my defence, I misunderstood and assumed that you were threadmilling a nut. The form error is MUCH less of an issue when OD threadmilling, although it is very likely still present if you examine closely, especially given your almost parallel flank angle. All the same, if the results are good enough then they are good enough!

Yes, it's true that there are ACME threadmills available off the shelf - but they can only be used for OD threads and perhaps don't state as such, so people mistakenly think they can use them for ID threads...

 

[Jashley73]

In my defence, I misunderstood and assumed that you were threadmilling a nut. The form error is MUCH less of an issue when OD threadmilling, although it is very likely still present if you examine closely, especially given your almost parallel flank angle. All the same, if the results are good enough then they are good enough!

Yes, it's true that there are ACME threadmills available off the shelf - but they can only be used for OD threads and perhaps don't state as such, so people mistakenly think they can use them for ID threads...

Why would it be impossible to thread mill internal, female Acme/Stub-Acme/TR threads? Are you suggesting that the helix-angle is too large, and thus, needs exceptional clearance on the top & bottom flank-faces of the thread mill?



If so - Now you've got me thinking about putting an internal threading tool holder (boring bar) in a rotating boring head, and using a rigid-tap cycle to thread them. Of course you'd have to multi-pass it, but it should be possible. More so if you trigg'd the start points, and altered your R-plane start height for each pass...

 

[lobust]

Why would it be impossible to thread mill internal, female Acme/Stub-Acme/TR threads? Are you suggesting that the helix-angle is too large, and thus, needs exceptional clearance on the top & bottom flank-faces of the thread mill?



If so - Now you've got me thinking about putting an internal threading tool holder (boring bar) in a rotating boring head, and using a rigid-tap cycle to thread them. Of course you'd have to multi-pass it, but it should be possible. More so if you trigg'd the start points, and altered your R-plane start height for each pass...

Yes, there is a fundamental problem in threadmilling in that the axis of the tool and the axis of the threadform are not parallel. Clearance or gouging is a function of flank angle, lead angle, and diameter delta between the tool and the thread. Typical 60 degree threads can tolerate a tool diameter quite close the thread minor without (meaningfully) gouging, but as the flank angle tends towards parallel, the possible cutter diameter tends towards zero. This is true regardless of ID or OD thread, but is obviously a much more significant issue for ID threads.

You can model this up in cad and it becomes very apparent. For any given acme/tr thread, any tool that is large enough to functionally cut it will intersect the thread surface and gouge the flanks.

As for rigid tapping I have considered that before but can’t really see any way that it would work unless you were using a cutting tool that could tolerate being dragged in reverse over the cut surface. HSS would be the only real option…

One method that does work, and that I have actually used successfully in the past, is if you have full rotary axis control of the tool spindle, in which case you can interpolate it in spindle-Z and move the tool away from the part to retract it. Still have to manually offset the tool for every pass though.

Best of all would be if you had a machine capable of U-Z interpolation. I’ve never had a machine that could do that to play with unfortunately!

 

[Litlerob1]

Why would it be impossible to thread mill internal, female Acme/Stub-Acme/TR threads? Are you suggesting that the helix-angle is too large, and thus, needs exceptional clearance on the top & bottom flank-faces of the thread mill?

Picture a Tongue and Groove joint, and trying to fit it at a helix. Acme threads can be very close. As the crest of the Thread diameter increases it gets easier to not gouge the flanks. But depending on QC even 60° threads technically have gouging on the flanks.

R