[naytep]

I am trying to threadmill with Gibbs. Gibbs only offers a single point tool, I am using a 1/2 dia 16 pitch (multi groove) thread mill. What am I missining? I am trying to mill 1-1/2" 16. The code (MAZAK FUSION) is giving me Z-062 and a J that it repeats. The values dont change. I have never threadmilled so I am not sure if its correct. Please give some pointers.
thanks
John

[bbern]

That seems correct.
Here's code from my post.

O3894( PROGRAM: THRDMILTST.NCF )
( 1. DIA THREADMILL- .0625 PITCH )
N1G17G80G40
N2T1M6( 1. DIA THREADMILL- .0625 PITCH )
M11
( CS#1 - XY PLANE )
( G54.1P1= X0. Y0. Z0. )
G54.1P1
G90G0X0.Y0.B0.S3000M3
M10
G43Z1.H1M8
Z.3
G91
G1Z-.807F5.
G0X.1556Y.1556
G41G1X-.0077Y.0132D101
G3X-.1479Y.0812Z.007I-.1479J-.0941
Z.0625J-.25
Z.0625J-.25
X-.1479Y-.0812Z.007J-.1753
G40G1X-.0077Y-.0132
G0X.1556Y-.1556
G90Z.3
Z1.
M9
G91G28Z0.
G90
M5
M11
G91G28Y0
G90
M30

[naytep]

How do you handle the multi-thread tooth mills? Gibbs only allows for a single tooth type cutter. Most thread mills have a length of teeth.

[bbern]

I just don't feed all the way out of the hole. I make my start depth at the bottom of the hole and end depth a few turns up from there.Just a few rotations and out.

[SKEETO]

I believe you need to draw the tool geometry in a new workgroup and save it as a formed tool.

[cadman]

You will only need to create a form tool for the threadmill if you need to see it render all of the threads in tool simulation, otherwise just use the threadmill tool palette. Just like bbern said, for a full profile threadmill you only need to make a few turns.

[drewky]

John,
I've been converting lots of our processes over from tapping to threadmilling. Even though we have GibbsCam, I just use any of the numerous spreadsheets or web help sites to generate the code. I have used the programming guidelines for Threadmills USA and was able to get a good thread on the first crack. Good luck!
Mike

[inertialabs]

I just don't feed all the way out of the hole. I make my start depth at the bottom of the hole and end depth a few turns up from there.Just a few rotations and out.

So let me get this straight

If I use the tool path that I am using now for a single point cutter but instead of feeding all the way out of the hole I limit it to 3 turns then come out of the hole

Question when Thread milling a NPT 1/2 - 14 thread in 303 SS with a muilti flute Thread Mill should I use multiple passes or can you go full depth in one pass ?