Need help with Okuma threading code

[Camgal_59]

Hi all,

 

The post sent to me for our Okuma captain lathe is not creating the correct coding to cut a thread. I've tried several ways of coding per the manual, nothing is working. The tool is not retracting in 'X' before is returns to the 'Z' start.

 

Can anyone show me an example of OD threading code for the Okuma Captain Lathe?

 

[Greg Williams]

Yep,

 

NAT07

N0900 G97 S909 M41 M08

N0901 G00 X108 Z3.638 T070707

N0902 X45

N0903 G71 X32.4 Z-31.213 H2.6 D0.8 U0.06 B60 F2 M22 M73 M32

N0904 G00 X108

N0905 M05 M09

N0906 X500 Z800 T0700

 

 

The G71 command signals the beginning of a thread cutting cycle.

 

The X value is the minor diameter of the thread, the Z value is the termination point of the thread,

 

the B value is the thread angle, the D value is the depth of the first cut (diameter),

 

the U value is the finish allowance (also in diameter),

 

the H value is the thread height (again in diameter), and the

 

F value is the thread lead (the feed rate in inches per minute).

 

The M33 means that there will be a zigzag inffed cutting pattern, and M73 sets the infeed depth to pattern #1. (See manual.)

[Camgal_59]

Greg .. I have to tweak a few sizes [such as 'B' needs to be '0' to cut a straight thread] but otherwise looks likes this works!!

 

THANK YOU!

 

Now, I'll have to play with my post to enable the correct code. The post is putting out this type of code [which didn't work on our machine]:

 

(OD THREAD 1-2MM PITCH INSERT - R166.0G-16VM01-001)

G0 T121212

G97 S200 M03

G0 X.515 Z5.189 M8

G71 X.2617 Z4.8228 A29 H.0533 D.02 U0. F.04921 M32 M75

M9

G0 X20. Z20. T1200

M05

 

BTW: this is for an M8 thread [using english conversion]

[chris m]

Jo, B is the thread angle in the Okuma, not the threading angle, so B60 does cut a straight thread.

 

Below is working code from my Captain for and ID thread [M36, I think]:

 

N900

( T09 )

( THREAD ID )

( C5-R166.4KF-17070-16 )

( R166.0L-16MM01-150 )

G50 S3000

G00 X20. Z20.

T090909

G97 S1752 M03 M08 M42

VNVLX=VZOFX+VTOFX[9]-.02+1.280

VNVLZ=VZOFZ+VTOFZ[9]-.005-1.645

G00 X1.325 Z1.100

Z.100

Z-1.2606

G71 X1.424 Z-1.6391 B60 D.010 U.002 H.0633 M33 M75 M22 F.0591

G00 X1.35 Z.25

M09

G00 X20. Z20.

M01

 

Never really had the desire to screw around with my post for this, I just hand-write threading, so no help there.

[lionel 3362]

I am running into the same problem. We have a okuma OSP7000L. We use a M32, M73 threading cycle but the post is giving me a M32, M75 cycle. How do i get it to give me the cycle I need. Thanks

[crazy^millman]

Most Okuma lathe posts have a mi or mr switch to change the way it outputs the M codes for the threading cycle look in there.

 

HTH

[lionel 3362]

Im sorry im kind of new to this. Would that be located in the control definition?

[lionel 3362]

I found it. Thank you for the help, its much appreciated.