Thread milling

[Boone]

I'm trying to thread mill a 10-32 hole. On all of the thread mills I've used in the past the teeth are the pitch of the thread. On this particular tool, they are .062 apart. I'm not getting the correct pitch in the thread. I used the following:

 

G1Z-.300

G41D3X.117Fxx

G3X.117Y0Z-.2688I-.117J0

G1G40X0

 

What am I doing wrong? Should the distance traveled in Z be 1/2 of the pitch or something?

 

Thanks in advance.

[RobertELee]

You should still be using a .03125 pitch, that shouldn't change.

[Boone]

Well this is an Xactform thread mill. I went to their website and it is definitely the one that they recommend to use for this thread.

[RobertELee]

Yeah, sorry, what I meant was you should still be programming for a .03125 pitch, I looked at the program again and it looks like you are. I guess I miscalculated when I looked at it the first time.

 

What pitch are you getting? I use skip-tooth thread mills all the time and never have a problem.

[Span]

I think you need to make at least 2 revolutions.

[DavidB]

You have tyo program for the pitch in your case 0.03125".

If your getting wrong thread pitch the tool is doing it not MC.

quote:

---

On this particular tool, they are .062 apart

---

You have to use the correct tool for the pitch required.

 

Bet your parts pitch is to coarse!

 

Thread mill info

[Jaz]

Like Span said, if you are using a 'skip tooth' style thread mill you will need to adjust your tool path to make at least two complete revolutions while cutting the threads. So total z travelled should be double (minimum) the pitch of the threads.

[Boone]

Sorry It's been so long. I figured out that I needed to do the 2 revolutions. Thanks for the help folks.