Thread mill question

[Columbo™]

Did a search for this and came up blank.... so, sorry if this was coverd already.....

 

Is there a way to have mastercam not post out lines N16 and N20.... N16 is one quarter around, N18 is a full 360 and N20 is one quarter around.....

 

I just want the thread mill to engage, go once 360 around and get out..... Thought I was able to do this back in X5 or X6.

 

 

(** .350 THREAD MILL  **)
(GENERATE .5625-12 THREAD 12 PLACES)
N6 G15 H1 G0 G90 G94 X0. Y12.4 B90. S1000 M3 T5 M8
N8 G56 H5 Z10.
N10 Z9.6
N12 G1 Z9. F25.
N14 G41 D5 Y12.2937 F8.
N16 G3 X.1063 Y12.4 Z9.0208 I0. J.1063
N18 X.1063 Y12.4 Z9.1042 I-.1063 J0.
N20 X0. Y12.5063 Z9.125 I-.1063 J0.
N22 G1 G40 Y12.4
N24 G0 Z9.6
N26 Z10.

[GIZMO 21]

Try unchecking your helical entry in lead in/out in the cut parameters.

[Columbo™]

Try unchecking your helical entry in lead in/out in the cut parameters.

 

 

Yea, tried that already..... It makes a quarter turn around WITHOUT moving the Z axis.

[htm01]

Try unchecking your helical entry in lead in/out in the cut parameters.

AND SET ENTRY/EXIT ARC CLEARANCE TO 0.

[GIZMO 21]

Ah, i see what your saying.

[Matthew Hajicek - Singularity]

I think setting your "Entry / exit arc clearance" to zero should give you what you want.  Then it will feed into the cut perpendicularly.

[GIZMO 21]

AND SET ENTRY/EXIT ARC CLEARANCE TO 0.

It still does the 1/4 start.

[Columbo™]

I think setting your "Entry / exit arc clearance" to zero should give you what you want.  Then it will feed into the cut perpendicularly.

 

Still get that quarter turn

 

 

It still does the 1/4 start.

 

YEP

[EX-wccprogrammer]

It appears that the logic for the threadmill cycle adds 1/4 turn lead in and lead out by default.  These arc moves appear in the NCI file, regardless of the settings adjusted in Mastercam.  The only way to get the output that you are looking for is to write a pthreadmill postblock in your post that ignores the lead in and lead out arcs.  This would be relatively easy using a counter to keep track of the arc moves, and forcing the first and last arc to output linear.

 

HTH

[Guest MTB Technical Services]

A straight line entry at the bottom of a hole will NOT give you the correct thread form.

 

You need the 1/4 entry so the thread form is correct.

[Columbo™]

It appears that the logic for the threadmill cycle adds 1/4 turn lead in and lead out by default.  These arc moves appear in the NCI file, regardless of the settings adjusted in Mastercam.  The only way to get the output that you are looking for is to write a pthreadmill postblock in your post that ignores the lead in and lead out arcs.  This would be relatively easy using a counter to keep track of the arc moves, and forcing the first and last arc to output linear.

 

HTH

 

Thank you.... will look into this

 

 

 

 

 

A straight line entry at the bottom of a hole will NOT give you the correct thread form.

 

You need the 1/4 entry so the thread form is correct.

 

We have been doing it this way for years..... Form seems to be fine

[Guest MTB Technical Services]

We have been doing it this way for years..... Form seems to be fine

 

If the thread application is not under pressure, not a problem.

The imperfection won't stop the thread from working.

 

The size of the hob versus the hole minor diameter makes a difference.

 

If you're doing any kind of pressure thread or load bearing that way, you are asking for trouble.

 

A straight line engagement with a hob will distort the thread form at the entry point.

The 1/4 turn is there to allow a radial helix entry that follows the pitch so the thread form

at the point where the thread is fully engaged isn't distorted.

 

This is one of the reasons single-point tooling is used.