Hurco winmax, Programming Manual

Page: 139 / 254

WinMax Lathe NC Programming
704-0115-307
ISNC G Codes
4-25
G32 - Constant Lead Thread Cutting
G32 allows you to perform single edge ID and OD thread cutting. The cutting amount per
depth is held constant, and either straight or tapered threads can be cut using this cycle.
Refer to G78 - Threading Cycle, on page 4 - 64 for information about programming the
more complex, multi-pass Threading Cycle for OD and ID threads.
Default—No
Modal—Yes
Cancels:
• G33 - Threading
• G76 - Multiple Threading Cycle
• G77 - Outer Diameter/Inner Diameter Cutting Cycle
• G78 - Threading Cycle
• G79 - Stock Removal in Facing Cycle
The starting angle is measured in 0.001 degree increments. If no decimal point is
specified the scale factor is 0.001. For example, Q180000 is equivalent to 180.000
degrees.
This cycle can be interrupted. If either the Feed Hold or Interrupt Cycle button is
pressed, the tool will retract to Z start after completing the lead out move for the current
depth of cut. When the Feed Hold button is pressed, cutting will continue until the first
non-thread cutting move.
The feedrate override is fixed at 100% during thread cutting.
When multiple threading commands are issued in sequence, the control will not wait for a
spindle before continuing the next thread command.
Format
G32 X(u) ____ Z(w) ____ F or E ____ Q ____
Parameters
• X(u)—X end point
• Z(u)—Z end point; only used for tapered threading.
• F or E—pitch
• Q—thread starting angle
• X indicates Absolute X and (u) indicates Incremental X.
• Z indicates Absolute Z and (w) indicates Incremental Z.