npt thread

[goooose]

im threading some different npt holes, 1/4, 1/2, 3/4 and 2.

ive read that when the cutter travels up when cutting (even with a tapered t.mill) the arc must increase.

i cant seem to get mc to do this. ive giving the thread taper angle, but it still posts the same as if i left it at 0.

i know the threads are probably good enough....

[gcode]

It depends on what kind of cutter you are using

If you're using an NTP threadmill or NPT

threading insert, the taper is built into the insert. As long as the tool's length of

cut is longer than the depth of the thread,

you want your tool path to just cut a circle.

 

This is controled by the "number of teeth"

setting. Set it to one and post a junk file

you should see a tapered helix running from

the bottom up.

 

This is how you're program it using a single tooth

cutter.

[goooose]

http://www.practicalmachinist.com/vb/showthread.php?t=166346

 

this is what i mean

[gcode]

The taper is built into the cutter.. A circle toolpath is all that is required.

[CNCGUY]

Yes, this is true!!

 

quote:

---

The taper is built into the cutter..

---

However, this is not.

 

quote:

---

A circle toolpath is all that is required.

---

Quote from post in practical machinist. FWIW - I agree!! We cut nptf every day.

 

quote:

---

I threadmill NPT threads all the time, and yes, you DO have to taper the helical move to cut the correct form, even though the threadmill has the taper ground in already.

Obviously, since you are moving upwards as you cut, you also need to move outwards to maintain the correct engagement on the taper.

---

[Murray Mold]

I agree with that also, but I do alot of 1/8" and 1/4" npt for waterlines in molds and moving the cutter straight up works just fine for me.

 

I'm sure if you were doing aerospace stuff you would have to do it on a taper.

 

I've never tried it in MC, but now I'm curious and will give it a try.

[specv]

cnc guy is right, we cut 1/4-18 threads a lot. and in order for the truncation gage and the taper gage to work you need to increase diameter as you go up the thread also needs to be programmed in quadrants. MC will not do this correctly so we use a macro program for our tapered pipe threads.

[CNCGUY]

quote:

---

MC will not do this correctly

---

The only thing we thread mill with is MC.

 

Here's the code for 1/4-18 NPTF in 316 stainless. . .HTH

 

code:

---

N16

T16 M06 H16 (VARDEX 0250-18 NPTF-F THREAD MILL)

G54 G00 G90 X0. Y0.

S4439 M03

M08

G43 Z.63

G01 Z.0044 F75.

G41 D16 X.0556 F3.46

G03 X0. Y.0756 Z.0183 I-.0556 J.0174

Y-.0765 Z.0461 I0. J-.076

Y.0773 Z.0738 I0. J.0769

X-.0573 Y0. Z.0877 I0. J-.0599

G01 G40 X0.

Z.0044 F75.

G41 X.0711 F4.23

G03 X0. Y.0911 Z.0183 I-.0711 J.0178

Y-.0919 Z.0461 I0. J-.0915

Y.0928 Z.0738 I0. J.0923

X-.0728 Y0. Z.0877 I0. J-.075

G01 G40 X0.

G00 Z.63

M09

G53 G00 Z0.

G129 X0. Y0.

M30

---

[Murray Mold]

Okay, I finally got around to trying this in MC

The above link had this info:

"The correction factor to mill perfect NPT threads is .0011" per quadrant and it is true the radius should change constantly to account for the taper form."

So that would mean .0044 per whole circle.

My question is now, in the "Taper Angle" box, what do I put in as a value? Will it be in degrees of angle (2 degrees)or how much bigger at the top than at the bottom (.0044)? I always done these straight up with no problems, but now that I know the correct way, I want to do it correctly.

 

Thanx

[Murray Mold]

Bueller, Frye, Anyone, Anyone.....lol

Seriously, has anyone used this method in MCX3?

 

Would it be 1.7899, or 1.7899/2 or .0044?

 

Thanx again

[CNCGUY]

Taper angle should be 1.78333. That will get the code I posted above. BTW-I am running X2, not X3.

 

HTH

[Murray Mold]

Thanx for the help.

[vulan]

Hi ..

Can anyone help me...i a trying to do NPT thread mill in mc now, and t don't know how i can have the program with G03 posted, what i have is a whole bunch of linear moves ... :-(

Thanks alot

and have a nice day

 

MC X4 MU3

[3R!< W3NG3R]

is the linearize helix box checked? If so, uncheck it and see if that does it for you.

 

Otherwise check the filter settings and the control definition.

[vulan]

Thank you very much for your help Eric, it works !