need to thread a steel round bar 3/4x10 in a turning center to make 3200 parts, help

[SDConcepts]

material is 4130 steel 2" dia bar. will be bar fed into our lathe. whats the best way to cut the 3/4x10 thread? we thought about tapping, but worried about tap life and how repeatable the parts will be after heat treating. and then thought about single pointing it, but need to thread down 1.6" and then starting to worry about tool deflection and having to chase the thread with a tap when done.

trying to do this in one op, so the hole will be blind as well. my current thoughts are osg spiral flute taps so we eject the chips. but looking for other ideas and opinions.

thanks

 

[guest]

5/8" indexable drill, finish bore the minor, single point with a 1/2" shank threading bar. DMin .600 on the bar, .656 minor so no problem.

Threading

1.6" thread depth should be fine, you can always program in a couple thou taper if your spring passes don't get it.

Run it on the upper side of the tolerance, the hole's going to shrink a little in HT unless you are taking a lot off the OD at the same time.

 

[ManualEd]

Tap a few pieces with different H limits on the taps, and HT them.
See which tap size will give you acceptable threads and go from there.

The extra cycle time (and dicking around) for single point threading a coarse thread that deep will far outweigh a few extra taps.

 

[SeymourDumore]

Like ED said, do whatever you have to to find the right process by tapping.
4130 sucks for thread surface, and it sucks 4X for coarse thread.
Blind 3/4-10 @ 1.6 depth is not something I'd want to single point in that garbage.

 

[Dan from Oakland]

It will shrink in heat treat regardless of how much you turn off the outside in my experience. What is your final hardness?

 

[SeymourDumore]

It will shrink in heat treat regardless of how much you turn off the outside in my experience. What is your final hardness?

True, but one can always re-tap afterwards.
Yes, it sucks but if that is what's called for .....

 

[SDConcepts]

will be hardened to 32rc

 

[TDegenhart]

Geometric tapping head with collapsible tap?

Tom

 

[DDoug]

will be hardened to 32rc

Can't get that in pre-hard ?

 

[Larry Dickman]

True, but one can always re-tap afterwards.
Yes, it sucks but if that is what's called for .....

3200 pcs? Ya, that would suck.

Only 32rc, should be fine with a H5

 

[HuFlungDung]

Can't get that in pre-hard ?

Agreed. It would likely machine better and not require re-tapping after HT. The distortion in that length of thread is not really addressed by an oversize tap. Re-tapping 3200 holes = no fun.

 

[TDegenhart]

Ox had a setup on one of his machines to tap and withdraw the tap without reversing the spindle. Gearing that would run the tap in the counterclockwise direction faster than the spindle speed.

Tom

 

[david n]

Definitely go with prehard material if you can.....it will cut 2x's better than annealed material.............................

 

[Gobo]

Pre-hard material and form tap. Drill the largest size hole you can get away with.

 

[Dan from Oakland]

That's exactly why I asked what the hardness spec was. Get your customer to change the material to 4140 HT. 28-32 Rc is pretty much what you get with this material. It will machine much better than annealed and you will save the heat treat cost. With the prehard material, you should be able to single point the thread. In addition, your cutoff tool will be much happier as well due to the better chip control.

Just a comment- form tapping a 3/4- 10 in prehard 4140 is gonna take some serious balls.

 

[triumph406]

I would tap after HT, I tap 28-32Rc 4140 using TiCN coated taps, hold up very well. I'd expect to go thru quite a few if your running 3200 parts

 

[Mtndew]

Either get PHT material (that's what we do), or send the full bars out to heat treat as soon as they come off the steel truck and fully machine the parts afterwards.

 

[Limy Sami]

Geometric tapping head with collapsible tap?

Tom

Agreed it would be a good option as the chasers are easily ground, I had a quick google and it looks like they're no longer made.

 

[Ox]

That's exactly why I asked what the hardness spec was. Get your customer to change the material to 4140 HT. 28-32 Rc is pretty much what you get with this material. It will machine much better than annealed and you will save the heat treat cost. With the prehard material, you should be able to single point the thread. In addition, your cutoff tool will be much happier as well due to the better chip control.

Just a comment- form tapping a 3/4- 10 in prehard 4140 is gonna take some serious balls.

I form tapped 3/4-10 in 304SS. I think that we did that on a 25hp spindle.
The perishables/hole was high, but we gott'r done....


I would prefer a SP FL tap if you can make it work in this material.


----------------------

Think Snow Eh!
Ox

 

[o1bigtenor]

An off the wall idea

material is 4130 steel 2" dia bar. will be bar fed into our lathe. whats the best way to cut the 3/4x10 thread? we thought about tapping, but worried about tap life and how repeatable the parts will be after heat treating. and then thought about single pointing it, but need to thread down 1.6" and then starting to worry about tool deflection and having to chase the thread with a tap when done.

trying to do this in one op, so the hole will be blind as well. my current thoughts are osg spiral flute taps so we eject the chips. but looking for other ideas and opinions.

thanks

IF (huge caveat there) you have a machine that will do it - - - why not thread mill it?
At 3/4" thread you have enough space that the thread mill is stout.
All you need is a program - - - move into the center of the 'hole', spin the bar and the tool moving the tool in an arc so that you don't have full engagement until you are about 2/3rds of the way around the circle and then you rotate the turning tool until all the threads are cut then you feed to the center of the hole retract and you're done.
(I haven't done this but this is common practice on a mill - - - why can't you do it on a lathe with rotary live tooling?)