[plast744]

hi i need help on writting the G code for threading 1/2-8 2star acme. i understand that 4 thread per in and 180 degree apart. i can cut first star at 0 degree, but i don't know how to cut the second star at 180 degree cuase i don't know it's there a command for the okuma lathe tell to rotate 180 than cut the second star.

[tex]

Just a guess:

M19 P180

[mark c]

When I've done this on Fanuc controls, I've changed the starting Z value by the pitch of the thread, in other words, first start, Z.1, second start Z.35 etc

Hope this helps

[Zep]

Mark is right , its a two part threading cycle with a shift amount
I used IGF on my Okuma for the thread you asked about and this is the code it generated

NAT05
N0100 G00 X20 Z10
N0101 G97 S800 M42 M03 M08
N0102 X0.55 Z1.1 T050505
N0103 G71 X0.3376 Z0 H0.1624 D0.032 U0.0016 B29 F0.25 M22 M73 M32
N0104 G00 Z1.225
N0105 G71 X0.3376 Z0 H0.1624 D0.032 U0.0016 B29 F0.25 M22 M73 M32
N0106 M05 M09
N0107 G00 X20 Z10 T0500
N0108 M01


please note values will need to be adjusted for your needs but format should be close.

[jessegrnv]

G71 X.5 Z-1.0 B90 D.01 H.1 U.001 F.125 M33
VZSHZ=-.0625
G71 X.5 Z-1.0 B90 D.01 H.1 U.001 F.125 M33
vzshz=0

I run an Okuma Crown with osp7000l controls and this would work on my machine.
vzshz is a variable z shift that moves the offsett what ever you make it equal.(-.0625 should make it 180 degrees from the first thread.)
g71= thread cutting cycle
x=start point of thread
z=end point of thread
b=angle of thread
d= depth of cut
h= thread height
u=depth of cut for finish pass
f=feed
m33=in feed pattern(stagger)
Make sure to set vzshz=0 after you thread or all of your offsets will be set back .0625.

[broby]

If you have the option... try a Q2 value on the end of the G71 cycle and hey presto you have a 2 start thread!

ie... using the code from the above example...
G71 X.5 Z-1.0 B90 D.01 H.1 U.001 F.125 M33 Q2

This works on our machines.
Cheers
Brian.