Okuma lathe threading help please

[Scott Lundin Shopware Inc.]

I am Fanuc guy so the Okuma code below in new to me.  After ID threading is complete the threading bar rapids from a Z.118 clearance position to Z-.8739 and then rapids in X and Z right through the part to the home position causing a collision.  What in the code below could cause this?

 

(TOOL - 8 OFFSET - 8)

(ID THREAD - MIN. 1.0 DIA.  INSERT - NTC-3L10I)

( THREAD 1.625-48 )

NAT08

G97 S1173 M3 M42

T080808

M8

G18

G0 Z.118

X1.5055

Z-.8739

G71 X1.6262 Z-1.068 B60 H.0207 D.0066 U.003 F.02083 M33 M75

Z.118

M9

G97 S1173

G0 X10. Z10.

T0800

M5

G0 X20. Y0. Z30.

M5

M02

 

[Reko]

Above the G71 line... there is a Z-.8739

 

You need to start the cycle in front of the bore... Z0.1 would get my vote. The cycle always ends where it started.

 

I see there is a Z0.118 after the cycle... not sure why it ignores that.

[DODGERFAN]

I just posted that thread real quick with my proven post and this is what it looks like. 

 

(*****)
N1 ( TOOL - 102  OFFSET - 102 )
(   ID THREAD - MIN. .25 DIA.    INSERT -  NONE )
(*****)
G0 X10. Z10.
T10302
G97 S200 M03 M41
G0 X1.5024 Z4.0954
G71 X1.6262  Z1.2193 B29 D.009 H.0601 M32 M75 F.0208
G0 X10. Z10.
M05
M02
%
  HTH.

[Reko]

Yes... see the line right above the G71 cycle?

 

G0 X1.5024 Z4.0954

 

That is also where it should finish... then, it goes straight home (G0 X10. Z10.) after the cycle.

 

But in theory... the Z.118 in Scott's example should clear the bore before it goes home too.

[DODGERFAN]

The only thing I can think of is he isn't defining his stock.  His thread is starting inside the bore at Z-.8739, if its not defined properly it would exit thru the material.

[Mick]

Weird. The thread cycle, upon completion, should retract to the start Z position of the thread (in this case Z-.8739), then read the next line (in this case Z.118)

 

We've got three Okuma lathes here, and I have programmed plenty of thread cycles when they move to a Z+ position, then to a Z- position, execute the thread, then retract to a Z+ position, and then home, all with no issues.

[taperlength]

Try adding G0  to the Z.118 right after the G71 line.

[Scott Lundin Shopware Inc.]

Yep, adding the G00 to the Z.118 line after the G71 did the trick.  Thanks to everyone for all the responses.