[whiteboy]

Hope someone can help me with this, Haas sure didn't.

I Need to machine proper pocket/bore and then single point a 3/8-18 NPT thread. Part will have a 0.375 hole already drilled through if it matters. Thread depth is to be 0.407 and material is 6061.
Machine is a 2000 SL20.

Have literally beaten head on Machinery's Handbook trying to figure this out, but to no avail.

Before anyone suggests it, I have already checked Haas' website. Their latest lathe books have NO info about cutting ID NPT threads. The threading info they do provide is VERY vague in my opinion. I even called Haas (Lathe Applications) just now and the gentleman that took my call did his best to help me, but he even admitted the numbers he gave me may not work as he had never programmed an ID NPT thread before.

So..... Anybody out there got a good handle on this???

MANY MANY thanks in advance for any help with this.

[Haas_Apps]

Please call me and I am sure we can get you running

Wayne Reilly
805-278-8560

[Geof]

You use G76 with a positive I value for the taper that depends on the Z distance travelled between the start and end of the thread. The taper is 1/16" per inch diameter measure. You should be able to find the ID to bore for the small, furthest in, end of the thread from Machinery's Handbook.

[whiteboy]

Geof,
And how does the I value depend on the Z distance traveled??? Is it a radial value derived from the difference of the Z start and endpoints divided by 2?

As far as Machinerys Handbook (I am using the 25th Edition) giving the the ID to bore for the small, furthest in end of the thread, won't the small diameter on the part in my example be controlled by the taper? As I said, the thread depth from the face of the part is 0.407. If you use the 0.407 value to calculate your thread parameters from, please tell me how.

Thanks for the info.....

[Geof]

You have it partly correct.

The I value is the taper in radial measure, in other words half the difference in the diameter between the two ends of the thread.

If you had a thread 1.0000" long the difference would be 0.0625" but your thread is 0.407" so the difference is 0.407*0.0625 = 0.0254"

This is the taper only for the length of the thread it self, the Z distance travelled by the tool is longer because you have to start a little bit ahead of the part.

If you put your Z offset at the end of the part the threading tool is going to travel to Z-0.407 and probably starting at Z0.200 will give enough space for the machine to get everything up to speed and synchronized, so your total Z travel is 0.607 and the taper will be 0.0379 diameter measure, 0.0190 measured on the radius and this is your I value.

For internal threads the I is positive so it is added to the X diameter at the bottom of the thread; you have it backwards, it is the large diameter that is determined by the I value.