THREAD CYCLE – G32 COMMAND

Contrary to its name, G32 in CNC programming isn’t actually a THREAD CYCLE that automates the entire threading process. It’s a modal command, meaning it affects the machine’s behavior until another command overrides it. According to G32 command, straight thread and taper thread of certain lead are cut.
Here’s a breakdown of what G32 does:

  • Synchronized Spindle and Feed: G32 establishes a link between the spindle rotation and the feed rate. As the spindle turns one revolution, the tool feed locks in to maintain a consistent thread pitch. Imagine it like manually turning a lathe where your hand controls the feed while the spindle spins.
  • Precise Control: While G32 dictates the synchronization, you manually program the toolpath for each cutting pass. This gives you granular control over the thread profile, allowing you to create both straight and tapered threads.
  • Special Considerations: G32 bypasses features like feed rate override and single block execution. This ensures consistent thread creation without external interruptions.

G32 THREAD CYCLE Syntax

The exact syntax for G32 can vary depending on the specific CNC machine controller you’re using. However, here’s a general breakdown of the common elements:

G32 Z(w) F or G32 Z(w) X(u) F

  • G32 (This initiates the thread cutting with synchronized movement)
  • F (Feedrate): This defines the thread pitch (distance between threads) by specifying the feedrate per spindle revolution. For example, F.5 would result in a thread with a 0.5 unit pitch for each spindle revolution.
  • Z(w) ; Z-axis position for thread depth
  • Additional Axes (Optional): While G32 focuses on Z-axis movement for thread , some controllers allow you to specify additional axes (like X) for more complex thread geometries.

Here’s an example of a basic G32 command for cutting a thread:

G32 Z-10 F.2 ; Z-axis movement of 10 units, Thread pitch of 0.2 units per spindle revolution

Important points to remember:

Consult your machine’s manual : The specific syntax and supported parameters for G32 might differ between controllers. Always refer to your CNC machine’s manual for the exact implementation.

G32 vs. Canned Cycles : G32 offers more flexibility but requires manual toolpath programming for each pass. For simpler threading operations, some controllers might offer pre-defined “canned threading cycles” that automate the process (G76 Threading cycle).

G32 THREAD CYCLE example program:

Example 1 : straight lead

STRAIGHT LEAD THREAD EXAMPLE

(ABSOLUTE)
G50 T0100
G97 S800 M03
G00 X90.0 Z5.0 T0101 M8
X48.0
G32 Z-71.5 F3.0
G00 X90.0
Z5.0
X46.0
G32 Z-71.5
G00 X90.0
Z5.0
X150.0 Z150.0 T0100
M30

Example 2 : taper lead

TAPER LEAD THREAD EXAMPLE
(ABSOLUTE)(INCREMENTAL)
G50 S800 T0100G50 S800 T0100
G97 S800 M03G97 S800 M03
G00 X90.0 Z5.0 T0101G00 X90.0 Z5.0 T0101
X22.026 :U-67.974
G32 X49.562 Z-71.5 F3.0G32 U27.321 W-76.5 F3.0
G00 X90.0G00 U40.438
Z5.0W76.5
X21.052U-68.948
G32 X48.588 Z-71.5G32 U27.321 W-76.5
G00 X90.0G00 X90.0
Z5.0W76.5
X150.0 Z150.0 T0100X150.0 Z150.0 T0100
M30M30
Program for taper thread

Leave a Reply