Thread milling fanuc murata lathe

[kennyprfc]

Does anyone know a thread milling app to generate a thread mill program for lathe. I tried using the vargus milling app swapping the axis but it doesn't like it.

 

[Mtndew]

Does anyone know a thread milling app to generate a thread mill program for lathe. I tried using the vargus milling app swapping the axis but it doesn't like it.

Then don't use the milling app,use the Vargus lathe threading app.
VARGUS GENius

 

[kennyprfc]

Then don't use the milling app,use the Vargus lathe threading app.
VARGUS GENius

That only has thread turning options not power tool threading

 

[Mtndew]

Oh, I mis-read your original question.
You are thread milling on a lathe.
What alarm does it give you when you try the milling app? Maybe it's a simple G-code fix?

 

[Philabuster]

Does anyone know a thread milling app to generate a thread mill program for lathe. I tried using the vargus milling app swapping the axis but it doesn't like it.

Threadmilling on the lathe is easy the way I do it. Call up milling mode and home C-Axis. Bring the tool to X0, move the tool to bottom of hole depth on Z, G1 X to radial position to cut thread diameter, G1 Z (one thread pitch) C360.0 (feedrate will be in degrees/min), G1 X0, Retract Z from hole. Done.

This is for a multi-tooth threadmill making one revolution of the chuck. If you are using a single point cutter, then multiply 360° by the number of threads and make Z travel farther to match. For 10 revolutions, C3600.

 

[coyoinu]

the milling app probably didn't like it due to the plane selection, working in YZ as you would on the lathe reverses the arcs compared to other planes. change G2 to G3 and vice versa, it'll probably work

 

[kennyprfc]

Oh, I mis-read your original question.
You are thread milling on a lathe.
What alarm does it give you when you try the milling app? Maybe it's a simple G-code fix?

Plane selection alarm. I'm assuming it needs a cide to work in 3 planes we've contacted muratec for info

 

[kennyprfc]

Threadmilling on the lathe is easy the way I do it. Call up milling mode and home C-Axis. Bring the tool to X0, move the tool to bottom of hole depth on Z, G1 X to radial position to cut thread diameter, G1 Z (one thread pitch) C360.0 (feedrate will be in degrees/min), G1 X0, Retract Z from hole. Done.

This is for a multi-tooth threadmill making one revolution of the chuck. If you are using a single point cutter, then multiply 360° by the number of threads and make Z travel farther to match. For 10 revolutions, C3600.

I'll keep this in mind for any centre hole tapping in the future this looks like a nice way to write it . Unfortunately my threads on the outer diameter.

 

[Philabuster]

I'll keep this in mind for any centre hole tapping in the future this looks like a nice way to write it . Unfortunately my threads on the outer diameter.

If the threads are concentric to the centerline, then all you need to do is feed into it from the OD, then rotate C 360° while you move Z one thread pitch.