emuge npt threadmill and mastercam

[perfecseal mankato]

I am trying to get an emuge 1/8-27 npt threadmill to work with mastercams threadmill cycle.

I contacted emuge and what they said to do in mastercam does not seem to work.

Has anyone else tried this using the threadmill.

I used a circle .399 diam. threadmill diam.= .301

-.302 deep 9 cutting threads and .75" taper /ft.

(all supplied by emuge)

I really do not want to hand write 600 holes

with there cycle, lots of cut n paste.

mastercam mr0304 mill level 3 all up to the current maintenance updates

[Toolfab]

You can use MC to program thread mills (it works better with Tool Fab thread mills tho )

 

Tool Paths, next menu, circle toolpaths, thread mill.

 

Is this a multi-fluted tool or a single blade thread mill?

[crazy^millman]

I would hope you would subprogram the thread cycle then use a point call in Mastercam then use the sub call to do it but like toolfab said a slam dunk with the threadmilling cycle.

 

HTH

[kccadcam]

So,,, Exactly what is is doing wrong??

[perfecseal mankato]

I got it figured out with a tapered pipe thred mill

need to know the tip diameter of the thread mill.

the diameter I was given was at 9 threads up on the thread mill. No wonder why it was not working !!!!

Thanks for all the input.

Toolfab, if I have any more questions I will send you an e-mail

[Toolfab]

word

 

[Metalmuncher]

Perfecsealmankato I can send you a program if you want.I thread most of my holes

[Threept82]

You should'nt need to tell MC any taper because

thats built into the thread mill.

[Toolfab]

Not true three. You have to put the taper into the thread mill page so the interpolation follows the tapered wall. otherwise the thread mill will not make a true thread all the way up the hole.

 

IF the thread mill goes to the bottom of the hole, rolls around 360 degrees and comes up the taper of the thread mill will will "fall" away from the tapered wall. By putting a 1.7889 degree taper value in the thread mill parameter page the thread mill will roll around the hole while keeping 100% engagment between the thread mill and the reamed hole.

 

HTH

 

[Threept82]

On a multi-tooth, solid carbide,

1 complete revolution, Z up the pitch?

[Toolfab]

That is the way that I do it. 360 degress, bottom to top, counter clockwise.

[Threept82]

Me to, but its just a G3X,Y,Z,I,J and feed

I'm use to thread milling with other software. In

MC you need to tell it taper? I've yet to taper

threadmill with MC. Because with a tapered treadmill it should act the same as a regular

straight thread, No?

[Toolfab]

Nope, I will go make some screen shots and show you, give me a few minutes.

 

[Toolfab]

ok, its to small of a difference to show with the toolpath.

 

I will try to splain,

 

If you take a tapered tool, and go to the bottom of the hole then without following the taper up the hole you will loose contact with the thread mill. The thread mill is ground to the NPT spec, the hole is reamed with a pipe reamer, (or should be) those two tapers match, right? right.

 

If the thread mill is pulled straight out, you will get a gap, or clearance that will start between the two tapers as soon as the mill starts retracting if the taper is not put into MC. By putting the taper in the ops page you will get the required code to keep the 2 surfaces in contact before the arc out and the tool completing the thread.

 

Did i explain that ok?

 

[Threept82]

Toolfab.

You win.

I tried it with no taper and again with

.0625 taper. There was a differance of a few ten'ths

I'll be. Thanks I'll remember that and also try it

in the other cam sfotware.

[Toolfab]

Right on, glad I got you there. Its not about winning, but you had me all scared that I was doing it wrong. I was waiting for my customers to call me up all pissed!!!!lmfao

 

[Threept82]

LOL

[Threept82]

Other software doesn’t even have a place for

taper to be given. It should be called StupidCam.

[iowajim62]

3.82 u said

 

quote:

---

It should be called StupidCam.

---

It isn't ?!?!?!?

just had to poke

[Threept82]

It is now. Can you believe Stupidcam is back on

the market?