Problem- G76 threading, loosing thread lead with RPM change

[JohnnyDon]

I have a 18-T (model A) Fanuc control. Using a G76 threading cycle - it seems that you should be able to start cutting a thread, but then if you are getting chatter or something you should be able to lower the G97 RPM and then cut the thread again and not loose the spindle orientation or the thread lead. Since the feed rate in inches per rev does not change, it seems like you should be able to change the RPM and still not loose the timing. When I try this I wind up cross cutting my original threads.

[HuFlungDung]

I think that is a common problem on any lathe where the spindle drive runs open loop feedback. Although the encoder index provides a start signal, the Z axis and the spindle are not electronically geared together. Therefore the time delay between index detection and initiation of motion may be a constant, which means that changing the rpm will affect the phase angle of the toolpath entry point.

If chatter is bugging me, I usually end up writing out a threading routine in full with G33 (Mitsubishi) so that I can cut alternate flanks of the thread. This decreases contact area and promotes getting the tool edge under the skin to take a cut.

Keep the cuts fairly aggressive in depth, too. You might only have the opportunity to take one or two finish passes with the tool fully engaged before chatter begins again.

Also try the miracle fluid WD40 during threading. It can make quite a difference in chip flow, reducing chatter or delaying the occurance until much later in the threading process. The trick is to be done before 'later' arrives

[JohnnyDon]

thanks for the threading info

[g-codeguy]

I don't have HFD's technical knowledge, but he is definitely right. Changing the RPM will change the pick up point for threading resulting in a cross thread. You can't change the Z-axis starting position either, but you can change the the Z-axis ending position, the amount of the first cut, the thread height, the minimum DOC, the compound infeed, the amount for the last pass if being used, lead out, and of course the number of spring passes. Did I leave anything out?

[JohnnyDon]

Thank you guys for the replies. With your help, we now have a better understanding for future parts.

[jimiscnc]

A very interesting subject. I think there may be a Fanuc Control option that would allow you to change threading RPM and still pick up the same lead.

I know on a Mazak that capability is offered, but it is indeed a s/w option. "thread start point compensation"

FYI

[sinha_nsit]

Fanuc does not recommend rpm change during threading. In fact, one should not use CSS in threading. And, in a threading re-work, the workpiece should not be unclamped, start point of the threading cycle should not be changed, and the same rpm should be used. Otherwise, the tool will start following a different helix. However, if by doing experiments, you can estimate the shift amount in the two helices, you can shift the start point of the threading cycle in the opposite direction, at the changed rpm. This will ensure the same helices at the two rpm's.

G76 should be used to cut only one side of the thread
(e.g., G76 P_ _ 60 Q_ R_)
This will reduce the cutting force, and may help in reducing chatter.