G32

Format and notes

G32 X(U)_ Z(W)_ F_ (F is the lead. For multi-start threads, Q_ gives the start angle)

• The feed starts in sync with the spindle's once-per-revolution signal, so the tool enters the same groove however many passes you repeat. You write the infeed, retract and return yourself with G00 (G92 is a single canned cycle that bundles the four moves, and G76 is a multiple repetitive cycle in which the NC even calculates how the infeed is divided)
• F is the lead (the distance advanced per spindle revolution). For a single-start thread it equals the pitch; for a double-start thread it is twice the pitch
• Use it after fixing the spindle speed with G97. Do not change the speed until the thread is finished (a lag between spindle and feed throws off the lead). Do not use constant surface speed (G96) even for a tapered thread
• Feed per revolution (G99) is assumed. In the Siemens ISO dialect, commanding it while still in feed per minute (G94) gives an alarm, and Haas states that G99 is required
• At the start and end of a thread the feed cannot keep up, so the lead is not correct (incomplete thread portions δ1 and δ2). Command the required thread length plus the run-up δ1 and run-out δ2
• During threading, feed override and feed hold (pausing the feed) have no effect, because stopping partway would ruin the thread form (Mitsubishi Electric). If you want to stop, wait until the run of G32 blocks ends
• If you write G32 blocks in a row, the motion does not stop at block boundaries, so you can cut a continuous thread such as “parallel thread to tapered thread”. Used for shapes that G92 and G76 cannot write, and for worms. Do not change F partway or insert M-codes (Siemens ISO dialect)
• Command the lead of a tapered thread along the longer axis direction. If the taper angle is 45° or less, it is the lead in the Z direction (Siemens ISO dialect. Haas says “the larger of the two leads”)
• G32 is modal. Cancel it with G00 when you are done. If you forget, the next “X-only line” (meant as the retract) also moves at the threading feed
• How the decimal point is written for the start angle Q of multi-start threads is the exact opposite depending on the model (the Siemens ISO dialect writes Q180. with a decimal point; Haas writes Q180000 without one)

Example

G97 S600 M03 ;        (constant spindle speed. Do not use G96)
G00 X25. Z5. ;        (5 mm in front of the end face = run-up δ1)
X19.4 ;               (1st infeed)
G32 Z-22. F1.5 ;      (one threading pass. Into the relief groove = δ2)
G00 X25. ;            (retract)
Z5. ;                 (return)
X18.9 ;               (2nd infeed)
G32 Z-22. ;           (F stays at the previous value)
G00 X25. ;
Z5. ;
X18.16 ;              (finish: root diameter ≈ 20 − 2×0.6134×1.5)
G32 Z-22. ;
G00 X25. ;
Z5. ;

An example of an M20×1.5 external thread (G-code system A) written by Kezuriba. For illustration, there are only 3 infeeds. In practice, the thread is divided into 6–10 passes, with each infeed made slightly smaller than the last.

Differences between controls and machines

The same code can be written or assigned differently depending on the CNC control and the machine builder. Always check your machine’s manual.

“One source / reference” rows were confirmed in only one source. “CAM post output / reference” rows show what a CAM post processor outputs and could not be confirmed in the control maker’s own public documents.