Threadmill

[Joels]

I was using a 1/4-18 NPT threadmill in some Nitronic 50 material and i was breaking threadmills. To make a long story short what i needed to do was to make several passes with the threadmill to avoid the tool from breaking. Is there a way to get mastercam to do this automatically? i had to keep adjusting the tool dia and reload the program to get this done.

[Mgrenier]

Joel,

 

The third page of the thread mill parameters is for multi-pass. You might want to try and play with those.

 

Hope that helps.

[Joels]

is that for v9.2? i didnt see that page. I think it only has 2 pages.

[Storkman]

No, that is only in MR1 for X

[c-hook]

I have never had any luck using the thread milling feature in MC9.1. I always get some weird looking tool path than in no way resembles what I am trying to accomplish, so I have always just used sub-routines to achieve this, which I think work better anyway because you only have 3 lines of code to deal with in the sub if any adjustments need to be made. Of course I don't think the same approach will work with a pipe thread, considering the taper an all.

[PeterM]

My chief gripe with the Threadmill, and for that matter the circlemill toolpaths in general is not being able to set the entry/exit moves as in contour toolpaths. If that could be added I would consider it a great improvement.

 

_________________________________

Peter Martin

Senior Programmer/Milling supervisor

Preci Mfg

400 Weaver St. Winooski VT

802.655.2414

[mike_f]

what I do in ver.9 is to program my thread mill op. then copy it 2 or 3 times depending on how many rough passes I want, then I go back and change the threads major dia. to get successivly larger for each operation. I usually set a small entry/exit amount usually .02, check start at center, helical entry/exit at top & bottom for a smooth entry and exit. for NPT threads I use a taper angle of 1.7833....HTH

[Guest]

quote:

---

is that for v9.2?

---

V9.2???

 

Wasn't that the last hacked version that was for sale on Ebay?

 

 

 

j/k

[Hardmill]

You need to use contour ramp,

All the control you need and tool comp too.

 

 

PEACE

[Storkman]

quote:

---

All the control you need and tool comp too

---

Leave it to the old guy to answer that.

 

Hey Dude, remember Elvis?

 

[Hardmill]

Hey pinhead, hows it going ??

 

 

PEACE

[mike_f]

the thing with contour ramp though is it doesn't allow you to lead in on a helix, for instance, in lead in lead out you can put in a helix hieght but it will always feed negative in z, if you start at the bottom of a hole that puts your lead in helix in the wrong direction for a right hand thread. the other thing is the taper angle for tapered threads, I don't see a way to do that with contour ramp. If you're using a multi tooth thread mill the angle is built into the cutter, but I still use in to keep my teeth in contact throughout the cut.

[toolall1]

havent thread milled much.but i picked up some good info here thanks

[TFesta]

If you keep ajusting the tool dia. offset why don't you just make 3 or 4 copies of your program with different offset # and away you go.

[mike_f]

you don't need to re-run the same prog. or make multiple copies of your prog. just create a threadmill op., in your op. mngr. copy that operation for as many rough passes as you want. go into the thread mill parameters for each op. and alter the major thread diameter, ex: I threadmill some 3/8 NPT threads in 316 s.s., I take 3 passes, in my 1st op. I set the maj. dia as .63, in the 2nd I set it as .6765 & the 3rd I set as .6865, the tool will now take 3 passes.