Okuma NPT threading cycle

[gcode]

One of my contract customers requested a 1/8-27 NPT threading cycle.

It's probably been 20 years since I touched an Okma lathe.

I'm running an old version X Okuma lathe post from InHouse cira 2005..

 

can someone look at this code and tell me if it looks right

 

TIA

 

 

T0707

G97 S1400 M03 M41

G0 X1.5 M08

Z.127

X.6096

G71 X.3339 Z-.264 I.0082 B29 D.016 H.0593 M32 M75 F.037

X1.5

Z.25

G0 X10. Z10.

M05

M02

%

[JerryBenoit]

Well gcode,

 

All the Okuma lathes that I have ran use Fanuc controls. If this is the case a G71 is roughing in Z axis you would need to change that to a G76. Also is this lathe in a dual can cycle mode or singular. Looking at the feed I would carry it out 6 places, granted it probably is not needed being a short length, but I always carry the feed on a feed 6 place unless the decimal terminates before that. Being an O.D. thread you might have the taper value as a negitive, but check the machine manuel if that is correct. I am not sure if the machine has a "B" and "H" value that depends on the machine tool builder, again check the documentation. If you don't have the documentaion ask your customer what the control type is.

 

Hope this helps.

 

Jerry

[T_MALENA]

I think you need a U.005 or so. The control may default to a preset value & take the doc at 50% of that then 50% of that & so on.

[T_MALENA]

Let me clarify a little(I just reread my prev post).

 

gcode the code posted should work, ASSUMING you have a OSP control. However when using M32 & M75 the control takes the finish pass into the doc calculations for the final passes<-- notice passes. Maybe try it & see tool life compared to # of passes. Also try M32 M73. M73 acts similar to M75 but divides your D valud in half each pass until reaching the U finish pass allowance. But at 1400 rpm & that loc shouldn't matter much.

 

G71 X.3339 Z-.264 I.0082 B29 D.016 H.0593 M32 M75 F.037

 

X=final dia. - root

Z=end of thread - unless you add M23 & a L value.

I= the taper - rad value

B= the infeed angle, I do the same with 29 deg.

D=Dia. doc - so 1st doc will be .0080

H=height of thread - in dia.

U=finish pass

M32 infeeds to cut on leading edge of tool (right hand)

M75 adjusts the doc

F=I have no idea what the F is

 

 

HTH

[Goldorak]

 

F=I have no idea what the F is

 

 

F is the feed per revolution (1/27=.037)

[T_MALENA]

I ment that as in W The F

[Goldorak]

the F is the WTF when you set a F20 for a drilling cycle and you forget to change the G95 to a G94....... 20 inches per rev is a pretty fast feed a 4500RPM...