[tap32]

i need help programming internal 1.25-11.5 npt threads!
using okuma lathe
will be using single point thread insert.

could somebody write a code for boring and threading.

thank you for all your help

does anyone have a "cheatsheet" for programming npt threads?

[broby]

Hi Tap32,
Going from memory here...
I do not have the taper angle of an NPT thread to hand but I think it is around 1.57degrees. The easyist way I find to program imperial threads (TPI) is to make sure you are programming an even number of threads per inch using the G71 threading cycle.
In this cycle you program the pitch of the thread by using F50.8 J23 where J represents the number of threads per pitch "F". The value of "J" must be an integer, thus the need to multiply 11.5 by 2 to get a value of 23.
Also, you will need to use a value for the angle of the thread by using "A1.57" in the cycle. Where the value for "A" is the angle of the thread from the centre line of the shaft. (might be half the included angle, can not remember, been too long).
Thus you would end up with a threading cycle something like:
G71 X... Z... H... A1.57 F50.8 J23 B60 M33 M73
Obviously the values for X and Z need to match your final sizes and the value for H is the radial depth of the thread.
Hope some of this helps, alot of this information is from a rusty area of memory!
Cheers
Brian.

[g-codeguy]

Apologize for not posting it sooner. Been swamped the past 3 weeks. Finally got ahead enough to lay this out for you without holding up our machines.

I laid it out using data from the Machinery's Handbook. Don't have any cheat sheets. I save the various pipe thread operations in a separate file once I've programmed them (and varified they are good, natch ), and then modify feeds and speeds for the current material being run.

I included a canned roughing cycle...just in case. You undoubtedly don't have your post set up like ours. As you can see, we use variables for the feedrate and DOC.

I did offset the tapered geometry plus .002. It may not be enough. Every pipe thread I have ever run holding the bore size so that the 6-step plug gage basic tolerance is held winds up being on the maximum once the thread gage goes to the proper depth. I now modify the 1.7833 degree line until the 6-step is on the high limit. That way the threading insert has a little less tool pressure. Chatter is almost always a problem with the size parts we normally run.


FINISH PASS 1/32R INSERT

X1.739Z0
G2X1.6881Z-.0105L.036
G1X1.5093Z-.1
X1.457Z-.9394
Z-?


FINISH PASS 1/64R INSERT

X1.709Z0
G2X1.6793Z-.0062L.021
G1X1.5089Z-.0914
X1.457Z-.9246
Z-?


THREAD

X1.41Z.4
G71X1.6844Z-1.I-.0436B29D.024H.1392F.08696M32M75

The only part we have made with this thread was programmed for Z-.85 instead of Z-1. In case you don't already know, X1.6844 is at Z.4. Modify the variables as you need.


N600 (ROUGH CANNED 1/32R INSERT)
G97S972T0606M3M61
G0X1.375Z.03M8
G96S350
G85N100D=V2U.02W.01F=V3
N100G81
G0X1.7696
G1X1.5093Z-.1001
X1.457Z-.9396
Z-1.3702
X1.375
G80
G0Z1.M9
X8.Z30.
M1

EDIT: 1.457 thru hole is based on using a tapered reamer. Chart shows it to be 1.4567, but I've never seen a case where .003 would make a difference much less .0003