G32 Thread Cutting (Group 01)

Classic Control - Lathe Operator's Manual

The Online Interactive Operator's Manual is currently available in English only.

A PDF version of the Operator's Manual is available for download in multiple languages. Click the link below to view the Operator's Manual in your language. Click "Continue" to view the online version in English.

Get a translated PDF Download Continue
F - Feedrate in inches (mm) per minute 
Q - Thread Start Angle (optional). See example on the following page.
U/W - X/Z-axis incremental positioning command. (Incremental thread depth values are user specified)
X/Z - X/Z-axis absolute positioning command. (Thread depth values are user specified)
note: Feedrate is equivalent to thread lead. Movement on at least one axis must be specified. Tapered threads have lead in both X and Z. In this case set the feedrate to the larger of the two leads. G99 (Feed per Revolution) must be active.

G32 Definition of Lead (Feedrate): [1] Straight thread, [2] Tapered thread.

G32 differs from other thread cutting cycles in that taper and/or lead can vary continuously throughout the entire thread. In addition, no automatic position return is performed at the end of the threading operation.

At the first line of a G32 block of code, axis feed is synchronized with the rotation signal of the spindle encoder. This synchronization remains in effect for each line in a G32 sequence. It is possible to cancel G32 and recall it without losing the original synchronization. This means multiple passes will exactly follow the previous tool path. (The actual spindle RPM must be exactly the same between passes).

note: Single Block Stop and Feed Hold are deferred until last line of a G32 sequence. Feedrate Override is ignored while G32 is active, Actual Feedrate will always be 100% of programmed feedrate. M23 and M24 have no affect on a G32 operation, the user must program chamfering if needed. G32 must not be used with any G-code Canned Cycles (i.e.: G71). Do Not change spindle RPM during threading.
caution: G32 is Modal. Always cancel G32 with another Group 01 G-code at the end of a threading operation. (Group 01 G-codes: G00, G01, G02, G03, G32, G90, G92, and G94.

Straight-to-Taper-to-Straight Thread Cutting Cycle

note: Example is for reference only. Multiple passes are usually required to cut actual threads.
% o60321 (G32 THREAD CUTTING WITH TAPER) ; (G54 X0 is at the center of rotation) ; (Z0 is on the face of the part) ; (T1 is an OD thread tool) ; (BEGIN PREPARATION BLOCKS) ; T101 (Select tool and offset 1) ; G00 G18 G20 G40 G80 G99 (Safe startup) ; G50 S1000 (Limit spindle to 1000 RPM) ; G97 S500 M03 (CSS off, Spindle on CW) ; N1 G00 G54 X0.25 Z0.1 (Rapid to 1st position) ; M08 (coolant on) ; (BEGIN CUTTING BLOCKS) ; N2 G32 Z-0.26 F0.065 (Straight thread, Lead = .065) ; N3 X0.455 Z-0.585 (Blend to tapered thread) ; N4 Z-0.9425 (Blend back to straight thread) ; N5 X0.655 Z-1.0425 (Pull off at 45 degrees) ; (BEGIN COMPLETION BLOCKS) ; N6 G00 X1.2 M09 (Rapid Retract, Coolant off) ; G53 X0 (X home) ; G53 Z0 M05 (Z home, spindle off) ; M30 (End program) ; %

Be aware: Many service and repair procedures should be done only by authorized personnel. The service technicians at your Haas Factory Outlet (HFO) have the training, experience, and are certified to do these tasks safely and correctly. You should not do machine repair or service procedures unless you are qualified and knowledgeable about the processes.

Danger: Some service procedures can be dangerous or life-threatening. DO NOT attempt a procedure that you do not completely understand. Contact your Haas Factory Outlet (HFO) and schedule a service technician visit if you have any doubts about doing a procedure.

Feedback