G32 CNC Code | Threading | Turning

English CNC Wiki
1

Mastering G32: Single-Point Threading on CNC Lathes

On a CNC lathe, creating threads is a fundamental machining operation. While canned cycles like G76 and G92 provide convenient ways to program standard threads, the G32 G-code offers ultimate control and flexibility. G32 commands single-point threading, where you define every movement of the threading tool. This makes it ideal for:

  • Non-standard thread forms: Threads with unusual profiles or pitches.
  • Tapered threads: Threads where the diameter changes along the length.
  • Multi-start threads: Threads with multiple, intertwined helical grooves.
  • Very fine threads: Where maximum precision is required.
  • Interrupted threads: Threads with gaps or segments.
  • Special materials: Where canned cycles might not be optimal.
  • Maximum Control:

This article provides a comprehensive guide to understanding and using G32 on CNC lathes. We’ll cover:

  • The concept of single-point threading.
  • The G32 syntax and parameters.
  • The critical role of spindle synchronization.
  • How to program multi-pass threading with G32.
  • How to program tapered threads with G32.
  • The starting point and retract considerations.
  • G32 vs. G76 and G92.
  • Control-specific variations (Fanuc, Siemens, Haas, Mazak, Mitsubishi).
  • Troubleshooting tips.
  • The role of CAM software.

Crucial Note: Always consult the programming manuals for your specific CNC control system and machine tool. While G32 is generally standardized for single-point threading, there might be subtle variations in implementation or additional control-specific features.

1. What is Single-Point Threading?

In single-point threading, a single-point threading tool (a tool with a cutting edge shaped to the desired thread profile) is used to cut the thread groove. The tool makes multiple passes, gradually cutting the thread to its full depth. This is in contrast to using a tap or die, which cuts the full thread in a single pass.

Advantages of Single-Point Threading (G32):

  • Maximum Control: You have complete control over every aspect of the threading operation (infeed, speed, depth, etc.).
  • Flexibility: You can cut any thread form, pitch, or lead, including non-standard threads and variable-pitch threads.
  • Precision: With careful programming and setup, you can achieve very high precision.
  • Adaptability: You can easily adjust the threading parameters (e.g., infeed) during the operation if needed.

Disadvantages of Single-Point Threading (G32):

  • More Complex Programming: Requires more programming effort than canned cycles. You need to calculate and program each pass individually.
  • Longer Cycle Times: Multiple passes take longer than a single-pass tapping operation (but are often faster than canned cycles for specialized threads).

2. G32 Syntax (Fanuc and Common Variations)

The basic syntax for G32 on Fanuc and many compatible controls is:

G32 X... Z... F... Q... ;

  • G32: The single-point threading command.
  • X...: The target diameter (or radius, depending on your machine’s settings) at the end of the threading pass. For external threads, this will usually be smaller than the starting diameter. For internal threads, it will be larger.
  • Z...: The target Z-axis position at the end of the threading pass.
  • F...: The lead of the thread. This is the axial distance the tool travels in one revolution of the spindle.
    • Single-Start Threads: For a single-start thread, the lead (F) is equal to the pitch of the thread (the distance between adjacent thread crests).
    • Multi-Start Threads: For a multi-start thread, the lead (F) is equal to the pitch multiplied by the number of starts.
  • Q... (Optional): The start angle of the thread (in degrees), used for multi-start threads. This parameter is control-specific and might not be available on all systems. It’s often specified in milli-degrees (e.g., Q180000 for 180 degrees). Check your manual.

Important: G32 is a modal G-code within its group. It remains active until another motion command from the same group (G00, G01, G02, G03) is programmed. However, best practice dictates repeating the G32 on each threading pass.

3. Spindle Synchronization: The Key to G32

The G32 command relies on precise synchronization between the spindle rotation (C-axis on lathes with live tooling) and the Z-axis movement. The control system uses an encoder on the spindle to track its exact angular position. For every revolution of the spindle, the Z-axis moves by the distance specified by the F word (the lead). This creates the helical path of the thread.

Critical Points:

  • Constant Spindle Speed: The spindle speed must remain constant during the G32 move. Any variation in spindle speed will result in an incorrect thread pitch. Therefore, you typically use G97 (constant RPM mode), not G96 (constant surface speed), when using G32.
  • Accurate Encoder: The spindle encoder must be accurate and functioning correctly.
  • Rigid Machine: The machine must be rigid enough to maintain precise synchronization between the spindle and the Z-axis, even under load.

4. Basic G32 Examples (Single Pass)

Before tackling multi-pass threading, let’s look at some simple, single-pass G32 examples to illustrate the basic syntax and axis movements. These examples assume a Fanuc-style control and standard right-hand external threading.

Example 1: Single-Pass External Thread (Conceptual)

G00 X25.0 Z5.0 ; Rapid to a safe position above the major diameter
G32 X19.0 Z-20.0 F2.0 ; Cut a single pass of a thread with a 2.0mm lead
; Ending at X19.0 (diameter) and Z-20.0
G00 X25.0 ; Rapid retract in X
G00 Z5.0  ; Rapid return to Z start
  • Explanation:
    • G00 X25.0 Z5.0: Rapid to a safe starting position. The X value is larger than the final thread’s major diameter. The Z value is slightly before the start of the thread.
    • G32 X19.0 Z-20.0 F2.0: The G32 command.
      • X19.0: The target diameter for this pass. This is not the final minor diameter; it’s just an intermediate depth.
      • Z-20.0: The target Z position (the end of the thread).
      • F2.0: The lead of the thread (2.0 mm).
    • G00 X25.0: Rapidly retract in X to a safe diameter.
    • G00 Z5.0: Rapidly return to the Z starting position.

Example 2: Single-Pass Internal Thread (Conceptual)

G00 X15.0 Z5.0 ; Rapid to a safe position inside the bore
G32 X21.0 Z-20.0 F1.5 ; Cut a single pass of an internal thread with a 1.5mm lead
; Ending at X21.0 (diameter) and Z-20.0
G00 X15.0 ; Rapid retract in X
G00
  • Explanation:
    • G00 X15.0 Z5.0: Rapid to a safe starting position inside the bore (X is smaller than the final thread’s minor diameter).
    • G32 X21.0 Z-20.0 F1.5: The G32 command.
      • X21.0: The target diameter for this pass (an intermediate value).
      • Z-20.0: The target Z position.
      • F1.5: The lead of the thread (1.5 mm).
    • G00 X15.0: Rapidly retract in X to a safe diameter.
    • G00 Z5.0: Rapidly return to the Z starting position.

5. Multi-Pass Threading with G32

As shown in these single-pass examples, a complete thread usually requires multiple G32 passes. Here’s the multi-pass example.

Example: Multi-Pass External Threading (Fanuc-Style, Conceptual):

Let’s say we want to cut an M20 x 2.5 single-start external thread (20mm major diameter, 2.5mm pitch).

O0001 (G32 Multi-Pass Threading)
G21 G18 G40 G99 ; Metric, XZ plane, cancel comp, feed/rev
T0101 ; Select threading tool
G97 S500 M03 ; Constant RPM (500 RPM), spindle on

; --- First Pass ---
G00 X21.0 Z5.0 ; Rapid to safe start (above major diameter)
G32 X19.5 Z-25.0 F2.5 ; Threading pass 1 (0.5mm depth in radius)
G00 X21.0  ; Rapid retract in X
G00 Z5.0   ; Rapid return to Z start

; --- Second Pass ---
G00 X21.0 Z5.0 ; Rapid to starting position
G32 X19.0 Z-25.0 F2.5 ; Threading pass 2 (0.5mm additional depth)
G00 X21.0  ; Rapid retract in X
G00 Z5.0   ; Rapid return to Z start

; --- Third Pass ---
G00 X21.0 Z5.0 ; Rapid
G32 X18.6 Z-25.0 F2.5 ; Threading pass 3 (0.4mm additional depth)
G00 X21.0
G00 Z5.0

; --- Fourth Pass ---
G00 X21.0 Z5.0; Rapid
G32 X18.2 Z-25.0 F2.5; Threading pass
G00 X21.0;
G00 Z5.0;

; --- Fifth Pass ---
G00 X21.0 Z5.0; Rapid
G32 X18.0 Z-25.0 F2.5; Threading Pass
G00 X21.0;
G00 Z5.0;

; --- "Spring Pass" (Final Pass at Full Depth) ---
G00 X21.0 Z5.0 ; Rapid
G32 X18.0 Z-25.0 F2.5 ; Final threading pass (full depth - no additional infeed)
G00 X21.0  ; Rapid retract in X
G00 Z5.0   ; Rapid return to Z start

G28 U0 W0 ; Home
M30 ; Program end
%

Explanation:

  • Setup: We select the threading tool, set constant RPM mode (G97), and turn the spindle on.
  • Approach: We rapid (G00) to a safe starting position slightly above the major diameter of the thread (X21.0) and a short distance away from the start of the thread in Z (Z5.0).
  • Threading Passes: We use multiple G32 blocks. Each G32 block defines one pass of the threading tool.
    • X: The target diameter for that pass. We gradually decrease the X value for each pass, cutting the thread deeper and deeper. The final pass should be at the minor diameter of the thread.
    • Z: The target Z-axis position (the end of the thread). This is usually the same for all passes.
    • F2.5: The lead of the thread (2.5 mm). This value must be accurate and must remain constant for all passes.
  • Retract: After each G32 pass, we use G00 to retract the tool in X (to a safe diameter) and then return to the Z starting position. This is critical to avoid damaging the thread.
  • Spring Pass: The final pass at X18.0 (the minor diameter) is a spring pass, with no additional infeed.

Calculating Infeed Amounts:

There are several ways to determine the X-axis infeed amounts for each pass:

  • Machining Handbooks: Handbooks often provide recommended infeed values for different materials and thread sizes.
  • CAM Software: CAM software will automatically calculate the infeed amounts based on the tool geometry and desired thread profile.
  • Trial and Error: For non-critical threads, you can use a trial-and-error approach, starting with small infeed amounts and gradually increasing them until the thread is cut to the correct depth.
  • Equal Infeed: A simple approach is to divide the total thread depth by the number of passes.
  • Decreasing Infeed: A more common and often better approach is to use decreasing infeed amounts. The first few passes take larger cuts, and the later passes take smaller cuts. This helps to reduce tool wear and improve surface finish. The example above uses a decreasing infeed.

6. Tapered Threads with G32

To cut a tapered thread with G32, you need to change both the X and Z values in the G32 block for each pass, according to the desired taper angle. The calculations for tapered threads can be complex, and using CAM software is highly recommended. The F value will remain consistent.

7. Starting Point and Retract (Critical for Safety)

  • Starting Point:
    • External Threads: Position the tool slightly above the major diameter in X and a short distance away from the start of the thread in Z.
    • Internal Threads: Position the tool slightly inside the minor diameter in X and a short distance away from the start of the thread in Z.
  • Retract: Immediately after each G32 pass, retract the tool in the X-axis using G00 (rapid) or G01 (feed). This prevents the tool from rubbing against the newly cut thread on the return move. Then, return to the Z starting position using G00.

8. G32 vs. G76 and G92 (Canned Cycles)

  • G32 (Single-Point Threading): Provides maximum control but requires manual programming of each pass.
  • G76 (Multiple Repetitive Threading Cycle): A canned cycle that automates the multi-pass threading process. You specify the thread parameters (major/minor diameter, pitch, infeed angle, etc.), and the control automatically calculates the infeed amounts and generates the multiple passes. Much easier to program for standard threads.
  • G92 (Simple Threading Cycle): An older, simpler threading cycle than G76. It’s still a canned cycle, but offers less control than G76.

When to Use G32:

  • Non-standard thread forms.
  • Tapered threads (where precise control is needed).
  • Multi-start threads (especially with unusual start angles).
  • Interrupted threads.
  • When you need maximum control over the threading process.
  • When a suitable canned cycle is not available.

When to Use G76 (or G92):

  • Standard thread forms.
  • When programming speed and simplicity are priorities.

9. Control-Specific Variations

  • Fanuc: G32 is the standard command for single-point threading. The Q parameter (start angle) is available on many Fanuc controls.
  • Siemens: Siemens controls might use G33 for single-point threading. Siemens also has extensive threading cycles. Consult the Siemens documentation.
  • Haas: Haas lathes use G32 for single-point threading.
  • Mazak: In Mazatrol, threading is typically handled through conversational programming. In EIA/ISO mode, G32 is likely used, but always consult the documentation.
  • Mitsubishi: Check documentation
  • Other Controls: Always consult your documentation.

10. Troubleshooting

  • Incorrect Thread Pitch:
    • Incorrect F Value: The most common error. Make sure the F value matches the lead of the thread (pitch x number of starts).
    • Incorrect Units: Make sure you’re using the correct units (inches or millimeters) for the F value (G20/G21).
    • Spindle Speed Variation: The spindle speed must be constant during the G32 move. Use G97 (constant RPM).
  • Tapered Thread (When It Shouldn’t Be):
    • Make sure you’re only changing the X value (for a straight thread) in subsequent G32 blocks. If you’re unintentionally changing Z, you’ll get a tapered thread.
  • Rough Thread Finish:
    • Incorrect Infeed: Too much infeed per pass.
    • Tool Condition: Use a sharp, appropriate threading tool.
    • Spindle Speed/Feed Rate: Incorrect cutting parameters.
    • Coolant: Ensure proper coolant application.
  • Tool Breakage:
    • Excessive Infeed: Too much infeed per pass.
    • Incorrect Starting Point: Not starting above the major diameter (external) or below the minor diameter (internal).
    • No Retract: Forgetting to retract the tool in X after each pass.
    • Dull Tool:

11. Best Practices

  • Use Decreasing Infeed Amounts: Take larger cuts on the first few passes and smaller cuts on the later passes.
  • Program a Spring Pass: Always include a final pass at the full thread depth with no additional infeed.
  • Use a Safe Starting Point: Position the tool clear of the workpiece before starting the G32 move.
  • Retract Safely: Retract the tool in X after each pass before returning to the Z starting position.
  • Use Constant RPM (G97): Avoid using G96 (Constant Surface Speed) with G32.
  • Verify Spindle Synchronization: Ensure your machine’s spindle encoder is functioning correctly.
  • Use Sufficient Coolant:
  • Start with a Slower Feed Override: When testing a new G32 program, use a reduced feed override.
  • Use Single Block Mode: Run the program in single block mode for the first few passes.
  • Inspect the Thread: Carefully check the thread after cutting.
  • Use CAM Software: For complex or non-standard threads.

12. CAM Software

CAM software can greatly simplify threading operations, especially when using G32. The CAM system will:

  • Allow you to define the thread parameters.
  • Automatically generate the multiple G32 passes, with appropriate infeed amounts and retract moves.
  • Optimize the cutting parameters.
  • Provide simulation to verify the toolpath.

While you can program G32 threading manually, CAM software is highly recommended for all but the simplest threads, and it’s essential for complex or non-standard threads.

13. Frequently Asked Questions (FAQ)

  • Q: What’s the difference between G32, G76, and G92?
    • A: G32 is for single-point threading (manual control over each pass). G76 and G92 are canned cycles that automate multi-pass threading.
  • Q: Can I cut tapered threads with G32?
    • A: Yes, by changing both X and Z in the G32 block.
  • Q: Can I cut multi-start threads with G32?
    • A: Yes, by using the Q parameter (if supported) or by adjusting the Z starting position for each start.
  • Q: Do I need to use cutter compensation (G41/G42) with G32?
    • A: Generally, no. Tool nose radius compensation is typically not used with G32 because you’re programming the toolpath for a specific tool nose radius.
  • What is the best threading method? * A: CAM generated programs are typically best for threading.

14. Conclusion

The G32 G-code provides complete control over the single-point threading process on CNC lathes. It allows you to create a wide variety of thread forms, including non-standard, tapered, and multi-start threads, with high precision. While it requires more programming effort than canned cycles (G76, G92), its flexibility makes it an indispensable tool for experienced CNC machinists. For most standard threading operations, however, a canned cycle (G76 is recommended) or CAM software will be more efficient. Always consult your machine’s and control system’s documentation for specific details and limitations.