HAAS ST 25 - G76 Threading Cycle

[A1BERZ]

Hello, I am looking for some advice here. I have been trying to rifle a 3in barrel on a HAAS ST 25 using a G76 threading cycle with a 16in lead.

This is a sample of the code \\

(TOOL - 8 OFFSET - 8)
(3D LATHE TOOL-7 INSERT - INSERT)
G00 T0808
G18
M8
G97 S10 M4
G00 G54 Z.0439
X.344
Z-3.
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 Z.0439
M9
G53 X0.
G53 Z0.
M37
M61
M33
M30

We are having trouble with W-2.6667 that incremental Z move does not work with the tooling we have available it will cause a crash by forcing the tool into the part. We need a way to clock the spindle 60 degrees for each groove of the riffling with out changing the start position of the tool in Z.

Any help or ideas at all would be greatly appreciated looking forward to hearing all of your brilliant ideas.

 

[DouglasJRizzo]

You could start 14." back and roll in.
Some machines have a Phase Synch option and could could reposition along C axis if available.

 

[Booze Daily]

If you have enough Z travel, starting at the front and grooving toward the back would work.
Change your W to a positive number.

 

[A1BERZ]

The tool we are using is designed to pulled from back to front, but if we cant figure anything else out then we will more than likely be redesigning the tool and starting at the front. Thank you very much for your feedback!

 

[angelw]

Hello, I am looking for some advice here. I have been trying to rifle a 3in barrel on a HAAS ST 25 using a G76 threading cycle with a 16in lead.

This is a sample of the code \\

(TOOL - 8 OFFSET - 8)
(3D LATHE TOOL-7 INSERT - INSERT)
G00 T0808
G18
M8
G97 S10 M4
G00 G54 Z.0439
X.344
Z-3.
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 W-2.6667
G76 X.355 Z.05 K.0035 D.0007 A00 E16.
G00 Z.0439
M9
G53 X0.
G53 Z0.
M37
M61
M33
M30

We are having trouble with W-2.6667 that incremental Z move does not work with the tooling we have available it will cause a crash by forcing the tool into the part. We need a way to clock the spindle 60 degrees for each groove of the riffling with out changing the start position of the tool in Z.

Any help or ideas at all would be greatly appreciated looking forward to hearing all of your brilliant ideas.

Hello A1BERZ,
You do this by not changeing your Z Start Point and index the Helical Path with a "Q" address included in the G76 Block. In the first G76 Block, the "Q" address can be specified as Q0, or simply omitted (Q0 is assumed by the control if omitted), second and subsequent G76 Blocks the "Q" address would be incremented by 60 degrees, written without a decimal point, that is, Q0, Q60000, Q120000, Q180000, Q240000 and Q300000.

Regards,

Bill

 

[MaxPrairie]

Hello A1BERZ,
You do this by not changeing your Z Start Point and index the Helical Path with a "Q" address included in the G76 Block. In the first G76 Block, the "Q" address can be specified as Q0, or simply omitted (Q0 is assumed by the control if omitted), second and subsequent G76 Blocks the "Q" address would be incremented by 60 degrees, written without a decimal point, that is, Q0, Q60000, Q120000, Q180000, Q240000 and Q300000.

Regards,

Bill

Yup. Q is what you need. Also how you do multi start threads.

 

[angelw]

Yup. Q is what you need. Also how you do multi start threads.

It's a Multi Start Thread that the OP is cutting; it just happens to have a very long lead.

 

[A1BERZ]

Thank you very much we will be trying this first thing Monday!