Thread milling

[Hymen]

Anyone ever successfully perform Thread milling on a lathe with only X, Z, and C axes.

 

Using G112 you cannot move the three axis at the same time correct? So this won't work.

 

So I was thinking of turning the live tool and the spindle on, calculate my feed from both, then move in on the x axis and then the Z.

 

Anyone try this? I doubt it will work but for the time and tool life I would save it is worth checking out.

 

The thread is 1/2-28 UNEF in inconel 718.

 

Or if you have suggestions on how I might get around the, G112, 3 axes delima please ad your feed back and I'll test it out.

[Tim Johnson]

Here's how I did a 9/16-18 thread in 20cb3 material. Mazak SQT-18m

 

code:

---

N1250G97G98S1300T0202M201M203

N1260G28H0.

N1270G00X0.C0.Z1.15

N1280G01Z.76F100.M211

N1290X.085F2.6

N1300H378.Z.8183F774.13

N1310X0.F2.6

N1320Z.76C0.F100.

N1330X.09F2.6

N1340H378.Z.8183F774.13

N1350X0.F2.6

N1360G00Z1.15M212

N1370G99G28U0W0T0000M202M205

---

Worked very well...

[Bryan Johnson]

Yes. I have thread milled on a Haas C axis Lathe (no Y), and yes, you can move all 3 (XZC) axis while in G112 mode (on this machine).

[Hymen]

Thanks guys.

I got it to work, although Miyano said it could not be done, but I had to use G107 as I could not get this to work in G112 on this Fanuc controller.

 

And it repeats! Allowing for sizing of the thread. This was the main grey area for me, whether or not I could actually re-start the cycle and not mess up the threads.