G71 and NPT Threads

[camhead420]

Hi all,

I got a job with 3\4 -14 npt external threads. What numbers out of the handbook do i use with the G71?
I am using .90371" as a starting dia. , but what would the H be for thread height?

Thanks!

 

[Booze Daily]

I just looked up my code and I'm using .078
Starting X is .906

 

[SeymourDumore]

Hi all,

I got a job with 3\4 -14 npt external threads. What numbers out of the handbook do i use with the G71?
I am using .90371" as a starting dia. , but what would the H be for thread height?

Thanks!

Not enough info on multiple levels!
First, not sure what the G71 cycle is, but guessing it's the equivalent of a Fanuc G76. ( Perhaps Okuma???)
If so then you need to define two different values. One is the Height of the thread, the other is the taper amount.
The Height is defined by P, the taper is by R.
The height (P) is approx .054 for a 14 pitch NPT, but cannot tell you about the taper without more info.
The taper ( R) value is a signed distance from the X-end point to the X-start point.
So, you need to know the Z start and Z end point, and then the X value at each of those points.

 

[camhead420]

Sorry about the info, i had this thrown at me as i was rushing out the door.(no excuse)
It is for an Okuma LB3000, OSP200L control.

 

[bradleyk]

H.12 for Okuma. Also, you don't need a finish point in X...just use an angle command
A178.2167 is a 1°47' taper. The machine will calculate endpoint for you.

X1.15 Z.3
G71 X.892 Z-.71 A178.2167 H.12 D.015 U.003 F1 J14 B50 M33 M73

 

[litlerob1]

G71 X..Z-..I(value difference of X start and X finish, divided by 2) H(Height of thread from root to crest) F(1/14).

R

 

[camhead420]

H.12 for Okuma. Also, you don't need a finish point in X...just use an angle command
A178.2167 is a 1°47' taper. The machine will calculate endpoint for you.

X1.15 Z.3
G71 X.892 Z-.71 A178.2167 H.12 D.015 U.003 F1 J14 B50 M33 M73

B50 ?

 

[litlerob1]

B50 ?

Okuma uses about 90leven different ways to accomplish a task. More than one way to skin a cat, as they say. The B value is arbitrary.

https://www.google.com/url?sa=t&sou...FjAEegQIEhAB&usg=AOvVaw0yF7AKeDPnBV0hkKg4UpVq

 

[camhead420]

Thanks for the link, you are right, many ways to get the job done.
Curious on the m33 zig zag cut mode? trying to picture that.

 

[Booze Daily]

(from the manual)

 

[bradleyk]

The B value is whatever modified flank infeed you want. I use it depending on material. A B50 means the thread insert will follow a path 5° off the flank of the 60° thread...modified flank infeed. The M33 command zig-zags...as in alternating flank infeed with each flank being 5° off the normal 60° flank (60-50=10 ...divided by the two flanks=5°).
If you don't want the zig-zag infeed then use M32.

 

[camhead420]

One other question i have is what do you all do about checking? We are just making it fit the part right now. I see the ring gauge
for sale, does it do depth like the male gauge? That is all i have done is internal NPT threads.
Thanks for the help!

 

[Booze Daily]

If it just has to "work", I usually use a mating part so it screws on about 1/2" or so.
If you are going to use a gage, yes it screws on so that it is flush with the end of the part.

 

[SeymourDumore]

If you are going to use a gage, yes it screws on so that it is flush with the end of the part.

To clarify, the standard NPT gage must be +/- 1 turn from flush.
The double step gage must be within the two steps by hand engagement.