NPT Thread cutting oversize

[Hertz]

Hey guys, Title says oversize, but I meant undersize. I am trying to cut a 2"-11.5 NPT thread on the lathe and it is cutting about .06 undersize. This is the program I got from Mastercam but I can't see any reason for the undersize thread. Any ideas?

 

T0505

G98

G97S500M03

G0Z.2235M8

X2.6009

G76P010060Q30R0.

G76X2.2326Z-1.P530Q100R-.0374F.08696

G28U0.M9

G0Z10.

 

In Mastercam I have these settings.

[KFrey]

The x value in the G76 line should be the minor diameter at the back end of the tapered thread. I haven't done the math in your case, but try selecting 'Large end of Taper' in the Thread Shape Parameters and see if your X value changes. The post may need to be set up properly for this also.

[Hertz]

T0505

G98

G97S500M03

G0Z.2235

X2.575

G76P010060Q30R0.

G76X2.2067Z-1.P530Q100R-.0374F.08696

G28U0.

G0Z10.

 

No difference really. Still smaller than original.

 

I tried a few different variances but nothing is changing the right way. All changes seem to want to make the cut even deeper.

[Hertz]

Ok I did this. Told it the small side of the taper and entered in the pipe OD as the MD and the thread depth, thus setting the md to 2.269 as it outputted in the post. The thing that baffles me is the numbers are backwards to what they are supposed to be. I mean I am lying to it in the parameters just to get it to output properly.

T0505

G98

G97S500M03

G0Z.2235

X2.6373

G76P010060Q30R0.

G76X2.269Z-1.P530Q100R-.0374F.08696

G28U0.

G0Z10.

 

This looks better but not quite right yet. There is about .037 difference from original.

[Machineguy]

How's your planes set for lathe ? +d +z

For now try changing your "x" tool dimension on you tool page. Canned cycles don't seem to see a comp in the tool table., so adjust the "X" for that tool + .037 to start.

 

Machineguy

[KFrey]

This is what has worked for me in the past:

 

-on the thread shape parameters page, select your thread from the table. the numbers will fill in for you from the small end of taper.

-click on 'Draw Thread' to get the thread shape on your screen and save the geometry. (with small end of taper still selected).

-now select 'Large end of Taper'

-pick the endpoints of the lines representing the large end of the taper for your major and minor diameter.

-post the code with 'Large end of taper' selected.

 

If the Z endpoint that the table gives you isn't what you are looking for, trim the lines that get drawn from 'Draw Thread' to the Z point that you need, and then use those x values for your maj and min diameters.

[Guest MTB Technical Services]

Your thread taper is incorrect.

 

Mastercam has had a bug in G76 since V9.

The default posts don't take the run-in distance into account for the taper so the angle is incorrect.

[Hertz]

Really? That's pretty dumb for them to not fix it since V9. Christ were on X7. And how do you see my taper is incorrect? It says 1.7833 which is the correct taper for an NPT. Unless I don't see something else?

[Guest MTB Technical Services]

The R value in the second line is the radial difference.

It should be positive for ID work and negative for OD work.

Mastercam default posts ignore the run-in distance for G76 tapered threads and they need to include it.

Mastercam calls this the acceleration distance in the Op dialogue..

I know Colin had corrected this for the latest build but I don't believe the update copies the post files.

 

You can contact CNC or your dealer and get the updated default post.

 

You can always use this.

http://www.mtbtech.net/blog/2013/10/01/Free-G76-Thread-Cycle-Generator.aspx

[Hertz]

Ok thanks.

[Hertz]

I generated this code from your program.

 

G00X2.8097Z0.55

G76P011060Q30R0.002

G76X2.3029Z-1.0P534Q100R-0.0483F0.087

G00X2.8097Z0.55

 

Looks ok. The taper value (2nd R) has changed but my first X # looks right.

[Guest MTB Technical Services]

I generated this code from your program.

 

G00X2.8097Z0.55

G76P011060Q30R0.002

G76X2.3029Z-1.0P534Q100R-0.0483F0.087

G00X2.8097Z0.55

 

Looks ok. The taper value (2nd R) has changed but my first X # looks right.

 

If you trig out [1.0 ( Z Depth) + 0.55 ( Run-in distance)]*TAN[1.78333] you'll get 0.048259 or 0.0483 to 4 places.

 

Your original radial taper value was way off.