Formula to change rpm on threading cycle

[Hertz]

Good afternoon. I was wondering if any of you know the formula to be able to change rpms on a thread cycle on a lathe while maintaining start point. I have a thread that has started chattering really bad halfway and i want to change the rpm, but if I do, my threads won't line up. Is there a formula at all to be able to adjust the rpm to a number while keeping the same start?

 

[sinha]

The RPM must remain same in all passes. If changed, the helix would shift.
There is no formula to calculate the shift. One can only determine it experimentally, by giving a shallow cut at the two RPMs, separately, and measure the shift in the helix. The start point would need to be shifted to compensate for the shift in the helices.

 

[Azoth]

I think the reason you can't use G96 or change your rpms once you start single point threading was due to inertia/acceleration delay of the turret.

The machine will wait for a signal for the spindle orientation before feeding in Z so you'd need to know the time required for the machine to accelerate to the feed rate velocity to compensate for how far it lags behind. The faster the spindle speed, the more time the turret has to fall behind. Even if you knew how quickly the turret can accelerate, the time it takes to accelerate could still vary further due to friction/mass of the ways/turret.

I'm a novice though so don't take my word for it. Just no one has been able to answer that question for me so that's my hypothesis.

 

[Nmbmxer]

If you manually write the threading cycle with G32 you could change rpm after however many passes you wanted. You'd have to manually trial & error figure out the new z-start location for the reduced rpm though, just like picking up a thread. I don't think you can change the rpm once it starts feeding for a pass.

 

[Hertz]

Ahh, ok. I figured as much. Just thought maybe someone had ideas. Thanks fellas.

 

[jelrod1]

Ive just stopped it and added a bunch of passes when that happens at the same RPM to get through the part then change it on the next one.

 

[angelw]

I think the reason you can't use G96 or change your rpms once you start single point threading was due to inertia/acceleration delay of the turret.

It has Zero to do with that, its all due to the synchronization between the Spindle RPM and the Axis Motion. As the Threading Tool makes passes at the various diameters, in G96 Mode, the RMP of the Spindle will change due to maintaining Constant Surface Speed at these various diameters.

Regards,

Bill

 

[Nmbmxer]

Once the spindle syncs it’s fine, I’ve had a spindle drive fault out in the middle of a threading pass and it coasted down and didn’t even chip my insert. It’s the acceleration time between where it starts moving (z start) and when it syncs the feedrate to the current spindle speed spindle. The time delay to syncs the motion changes with spindle speed.

 

[SeymourDumore]

Is it just one part, or you want to do this for a production run?
Chatter sucks, but sometimes RPM won't make a damned bit of a difference.
If it is a production run, then perhaps you can change the cycle to a G92 and call the depths explicitly.
I do that on quite a few parts, specially on thin walled ones.
For chatter, I typically finish threading to the nominal minor, then back off .0005 and chase two or three more passes.

 

[angelw]

Once the spindle syncs it’s fine, I’ve had a spindle drive fault out in the middle of a threading pass and it coasted down and didn’t even chip my insert. It’s the acceleration time between where it starts moving (z start) and when it syncs the federate to the current spindle speed spindle. The time delay to syncs the motion changes with spindle speed.

None of the above.
The following is a Cut and Paste directly from a Fanuc Manual. I've highlighted the important bit.

In general, thread cutting is repeated along the same tool path in rough
cutting through finish cutting for a screw. Since thread cutting starts when
the position coder mounted on the spindle outputs a 1–turn signal,
threading is started at a fixed point and the tool path on the workpiece is
unchanged for repeated thread cutting. Note that the spindle speed must
remain constant from rough cutting through finish cutting. If not,
incorrect thread lead will occur.

and also from the Fanuc Manual:

7. Because the constant surface speed control is effective during thread cutting and the spindle speed changes, the correct thread lead may not be cut. Therefore, do not use the constant surface speed control during thread cutting. Instead, use G97.

You can have the Thread Operation Start Point a mile away from the start of the Thread and it makes Zero difference to how the Thread Tracks with varying Spindle Speeds.

What you're actually referring to in your Post, is the Pitch Error due to acceleration at the start of the Thread and to a much lesser degree, due to deceleration at the finish point of the Thread.

 

[angelw]

Good afternoon. I was wondering if any of you know the formula to be able to change rpms on a thread cycle on a lathe while maintaining start point. I have a thread that has started chattering really bad halfway and i want to change the rpm, but if I do, my threads won't line up. Is there a formula at all to be able to adjust the rpm to a number while keeping the same start?

Hello Hertz,
I've not tested this with a late model control, but certainly with a lathe equipped with a FS6T control, the index of the Thread was directly related the Spindle Revs and logically so, since the Threading pass is started based on the 1 Turn Signal output by the Spindle Encoder. Therefore, a Two Start Thread could be cut by either halving, or doubling the Spindle RPM used to cut the first lead, for use to cut the second lead.

Theoretically, if you wanted to re-cut a Thread that had just been cut with, say, 1800 RPM, if you were to halve the the Spindle RPM to 900, by shifting the Z Start Point by half the Thread Lead, the Threading Tool Should track in the same Thread Groove.

Also theoretically, you could extrapolate that out to use whatever the ratio of Spindle RPM change was, to the degree of Z Start Point change, to have the Threading Tool track in the same Thread Groove.

Regards,

Bill

 

[Nmbmxer]

To be fair, when the spindle drive pooped on me it was on a Mazak not a Fanuc.

I read your passage as when the spindle encoder outputs a 1 (after calculating the exact spindle speed) it starts moving from a fixed point, the Z start location. How long it takes to get from stopped to the correct feedrate (and at the end stopped again) is the incomplete thread distance. My old Mazak manual had several pages on how to calculate the number of incomplete threads at the start & end of the threading pass based on acceleration setting parameters and spindle speed.

I don't believe it is trying to have the tool moving at the correct feedrate and the spindle index position meet at an imaginary point at same instant. If it did then spindle speed wouldn't matter. I think that would take a machine with a full C to accomplish.

I've never heard of a multi-start thread cut by doubling/halving the RPM, only by varying the starting Z by a fraction of the pitch.

 

[angelw]

To be fair, when the spindle drive pooped on me it was on a Mazak not a Fanuc.

I read your passage as when the spindle encoder outputs a 1 (after calculating the exact spindle speed) it starts moving from a fixed point, the Z start location. How long it takes to get from stopped to the correct feedrate (and at the end stopped again) is the incomplete thread distance. My old Mazak manual had several pages on how to calculate the number of incomplete threads at the start & end of the threading pass based on acceleration setting parameters and spindle speed.

I don't believe it is trying to have the tool moving at the correct feedrate and the spindle index position meet at an imaginary point at same instant. If it did then spindle speed wouldn't matter. I think that would take a machine with a full C to accomplish.

I've never heard of a multi-start thread cut by doubling/halving the RPM, only by varying the starting Z by a fraction of the pitch.

It may be possible to change the spindle speed and have the Thread cut in the same path if the machine had rigid tapping available on the Main Spindle, but not otherwise. If what you are saying is correct, rigid tapping would be doable on any machine that simply had Thread Cutting available. In Rigid Tapping a different Spindle RPM can be used to extract the tap to that used when cutting the Thread.

I'm not advocating the use of Spindle Speed change to cut a Multi Lead Thread, I was simply pointing out what happens and what has been my observation. When called to a client's work, when he complained that the machine had trashed an expensive, one off part during the Thread Cutting operation, it turned out they had done what you're saying is OK to do and changed the Spindle Revs to re-cut the Thread. They only changed the revs by a hundred or so RPM and therefore the Indexing of the Thread Start was not obvious, but as soon as that was revealed, I explained the situation. To demonstrate the point, I cut a sample thread twice on the same work-piece and halved the RPM between the Thread cutting operations. The Start Index of the two Threading operations were 180degrees apart.

If what you're saying is correct, then the OP should have no trouble using any RPM he wants to recut his thread. Good luck with that!

 

[Vancbiker]

......Therefore, a Two Start Thread could be cut by either halving, or doubling the Spindle RPM used to cut the first lead, for use to cut the second lead.......

While it might be sort of close on the second lead, I very much doubt that it would exactly split the first lead. The time required for the control to receive the one revolution pulse, process that and issue motion command to the servo drives is fixed, not related to spindle speed. I've never tried this to see how close it might be. If I had access to a lathe now I'd give it a try.

 

[angelw]

While it might be sort of close on the second lead, I very much doubt that it would exactly split the first lead. The time required for the control to receive the one revolution pulse, process that and issue motion command to the servo drives is fixed, not related to spindle speed. I've never tried this to see how close it might be. If I had access to a lathe now I'd give it a try.

Hello Kevin,
It was never put to the test and was pursuant to the topic of my previous Post. However, rotating the spindle so that the Start of one Lead lined up with the top of a OD Turning Tool, a line was scribed on the face of the work-piece to split the corresponding start of the second Lead on the other side of the part. If not absolutely exact, it was mighty close.

What I'm saying more broadly and it's generally acknowledged, is that Spindle Revs can't be changed mid stream in a Thread Cutting operation and have the Threading Tool track in the same Thread Groove. Whether this is by explicitly specifying a different, fixed RPM via G97, or the variations in RPM that will occur if Constant Surface Speed Control, G96, were to be used, makes no difference.

I reiterate, if what Nmbmxer is saying is true, the OP should be able to use any RPM he likes to re-cut the Thread; that's just not going to happen.

Regards,

Bill

 

[Nmbmxer]

I reiterate, if what Nmbmxer is saying is true, the OP should be able to use any RPM he likes to re-cut the Thread; that's just not going to happen.

Regards,

Bill

I don’t think you can change the rpm due to timing issues, like was posted before rigid tapping and G76 aren’t the same.

 

[angelw]

I don’t think you can change the rpm due to timing issues, like was posted before rigid tapping and G76 aren’t the same.

Well now you're contradicting what you've stated earlier. The simple fact is, that changing the Spindle Speed will have the Threading Tool cut a different Thread Groove. Whether that change in RPM is due to an explicit change via G97, or via Constant Surface Speed Control and the different diameters the Threading Tool visits during the Threading Operation, is irrelevant.

 

[Vancbiker]

Hi Bill, Totally agree with what you’re saying. Varying spindle speed during single point threading has caught many out and made many scrap parts as folks figured this out. My point about timing was mostly as a warning to folks that might be thinking of trying a double start thread by merely doubling (or halving) the spindle speed. Of course the slower one goes doing this the less error there will be.

My explanation might also help the OP understand why there is no formula possible to accurately calculate a Z shift to accommodate a new spindle speed for recutting a thread.

 

[jhearons]

Buy an Okuma... Actually, I see that Fanuc also offers variable speed threading.

StackPath

What Is Arbitrary Speed Threading?

This CNC function enables an operator to control chatter when repairing threads on components such as oilfield pipes.

www.mmsonline.com

 

[mmurray70]

Such a shame that we have to deal with this bull shit. Maybe one time in history it was an issue, but all the manufacturers could easily have this perfectly synced at any speed with todays technology. Doosan sells this feature as an upgrade. Costs them zero dollars to just include it as a standard feature. What a greedy bunch of crooks we deal with.