[Paul Zeballos]

Hi, I am running a program with a Thread Cycle (G34) routine in a lathe with a FANUC 18i control. I noticed that the starting point for the thread cycle (I suppose there must be a mark in the spindle to start the thread cycle) changes when I change the RPM in the program. That is a huge problem because I need to machine used pieces (need to seek the original path in the working piece) and work at different speeds.

Hope anyone can help me.

By the way, I writing from Peru so please forgive my english mistakes.

Thank you.

[ChrisW]

Use spindle override to change rpm

It always fails to properly track when changing rpm in program

[fordav11]

Spindle override does not work in a thread cycle the machines goes to 100% of the programmed speed.
In any case the position change is normal when the speed changes (that is why the override is fixed at 100% when threading)
To pick up an old thread use the Z offset on the threading tool. If you are threading to a shoulder the distance you can move the Z offset could be limited to a very small distance so you will need to stop the machine and turn the part a little bit until the tool is more in line then use the Z offset to fine-tune the position. A quick way to roughly line it up is take a threading cut (with the X offset set plus so the tool does not touch). About half way down the threading pass press the emergency stop. The machine will stop immediately. Then release the emergency stop, hold the part, unclamp the chuck and rotate the part so the tool lines up in the thread groove. Take another cut to check and use the Z offset to fine-tune the exact position.
For tapered threads it's a lot more difficult. The newer machines have a special option for thread reworking. Mazaks have had that capability for many years.

[Paul Zeballos]

Thank you fordav11. My case is like you said, I thread to a shoulder. I built a timing flange between the chuck and the working piece to pick up the old threads easily . I really don't have problems on this setup. My problems is: once I find the correct path at a given speed I am forced to use that speed forever. I want to use different speeds for the same piece. I suppose there must be a control parameter to force the threading cycle to start at a desire point in the spindle encoder. Do you have something in mind?

[fordav11]

What you want is impossible.
You can't change the speed part-way through cutting a thread and I don't see any reason why you would need to do that?
The encoder determines the start position based on the speed and uses that as reference while taking cuts.
Pick a speed then once you have your tool lined-up you must use that speed for the entire operation.

[angelw]

Thank you fordav11. My case is like you said, I thread to a shoulder. I built a timing flange between the chuck and the working piece to pick up the old threads easily . I really don't have problems on this setup. My problems is: once I find the correct path at a given speed I am forced to use that speed forever. I want to use different speeds for the same piece. I suppose there must be a control parameter to force the threading cycle to start at a desire point in the spindle encoder. Do you have something in mind?

You can set your threading tool correctly with regards to the Z Zero of the work and therefore the shoulder you run the thread to, but instead of moving the threading tool out of true position via the Z offset, you move the Z start position of the threading operation to synchronize the threading tool with the existing thread. If you determined that you had to move the tool via the Z offset by 0.5mm for example, then you would move the Z start position by that amount to achieve the same result, only the tool will still pull out at the same position relative to the shoulder.

Regards,

Bill

[dlstaufe]

if you're trying to "repair" damaged threads, or pickup an existing thread I would:
-write a finish pass only thread program and use this for alignment as follows
-adjust the common X so the tool is just above the part.
-cycle the thread, watching the alignment.
-adjust the start Z position so the tool appears to be centered in thread.
-cycle the thread alignment program to verify (by eye) you r z start change was accurate
-if so, drop the common x offset half way and repeat the "align by eye" process.
-continue this process, dropping the x common offset a comfortable amount each time until you recut the thread where you want.

I hope this helps