The Fastest China Rapid Prototype,Small To Large Batch Manufacturer to Bring Your Ideal Project to Life - Be-Cu Discover Our Top Manufacturing Wiki And Guide in 2024 Eamil us : [email protected]

Thread Machining Commands G32, G92, G76

CNC lathes can process straight threads, taper threads, and face threads, as shown in the figure. The cnc machining method is divided into single-stroke thread cutting, simple thread cutting cycle and thread cutting compound cycle.

(1) Single-Stroke Thread Cutting G32

Command format: G32 X(U)_ Z(W) F___

X(U) and Z(W) in the command are the coordinates of the thread end point, and F is the thread lead. The parameters to be determined before using the G32 command are shown in Figure a. The meanings of each parameter are as follows:

L: thread lead, when machining tapered threads, take the larger thread lead in the X direction and the Z direction;

α: Taper angle of taper thread, if α is zero, it is a straight thread;

δ1, δ2: cut-in amount and cut-out amount. Generally δ1=2~5mm, δ2=(1/4~1/2)δ1.

Example of thread machining: As shown in Figure b, the thread pitch L=3.5mm, the thread height=2mm, the spindle speed N=514r/min, δ1=2mm, δ2=lmm, turning in two times, and the depth of each turning is 1mm. The processing program is:

  • N0 G50 X50.0 Z70.0 Set the workpiece origin at the left end face
  • N2 S514 T0202 M08 M03 Specify the spindle speed 514r/min, adjust the thread turning tool
  • N4 G00 Xl2.0 Z72.0; Rapidly go to the thread turning start point (12.0, 72.0)
  • N6 G32 X41.0 Z29.0 F3.5; Thread turning
  • N8 G00 X50.0; Rapid retraction along the X axis
  • N10 Z72.0; Rapid retraction in the direction of Z axis
  • N12 X10.0; Rapidly go to the starting point of the second thread turning
  • N14 G32 X39.0 Z29.0; Second thread turning
  • N16 G00 X50.0; Rapid retraction along the X axis
  • N18 G30 U0 W0 M09; return to reference point
  • N20 M30; program end

(2) Thread cutting cycle command G92

Thread cutting cycle G92 is a simple thread cycle. This command can cut tapered threads and cylindrical threads. The cycle route is basically the same as the aforementioned single shape canned cycle, except that the subsequent feed of F is changed to the pitch value. Its command format is:

G92 X(U)Z(W)____R____F;

The picture shows the thread cutting cycle diagram.

The tool starts from the cycle starting point A, and performs automatic cycle according to the path A→B→C→D→A. The dotted line in the figure represents the rapid movement of the tool, and the solid line represents the movement at the working speed specified by F. X, Z are the coordinates of the end point of the thread (point C); U, W are the incremental values ​​from the coordinates of the starting point to the end point; R is the difference between the radius of the end point and the radius of the start point of the tapered thread. , when the cylindrical thread R=0, it can be omitted; F is the pitch value. The retraction angle for thread cutting is 45°.

Example of thread machining: machining the thread as shown in Figure b above. The procedure is:

N0 G50 X50.0 Z70.0; Set the workpiece origin at the left end face

N2 S514 T0202 M08 M03; Specify the spindle speed 514r/min,

Adjust the thread turning tool

N4 G00 X12.0 Z72.0; Rapidly go to the starting point of thread turning

(12.0, 72.0)

N6 G92 X41.0 Z29.0 R29.0 F3.5; Thread turning

N8 X39

N10 G30 U20 W20 M09; return to reference point

N12 M30; program end

(3) Multiple cycle command G76 for thread cutting

G76 thread cutting multiple cycle command is simpler than G32 and G92 commands, and only need to specify the relevant parameters once in the program, and the thread machining process will be carried out automatically. The instruction execution process is shown in the figure below, and the instruction format is as follows:

The format of G76 thread cutting command needs to be defined by two commands at the same time, and its format is:

G76 P(m)(r)(a) Q____ R____;

G76 X(U) Z(W) R(i) P(k) Q(Δd ) F(L);

The meaning of the geometric parameters in the formula

The definition of each parameter is as follows:

m: The number of repetitions of fine turning, from 1 to 99, this parameter is a modal quantity.

r: The chamfering value of the thread end, the value can be set between 0.0L and 9.9L, and the coefficient should be an integer multiple of 0.1, which is represented by a two-digit integer between 00 and 99, where L is the thread pitch. This parameter is a modal quantity.

a: Tool angle, which can be selected from six angles of 80°, 60°, 55°, 30°, 29° and 0°, represented by a two-digit integer. This parameter is a modal quantity. m, r and a are specified with address P at the same time, for example: m=2, r=1.2L, a=60°, expressed as P021260.

Q: Minimum turning depth, specified by radius programming. The turning depth in each turning process is (Δd-Δd ), when the calculated depth is less than this limit value, the turning depth is locked at this value. This parameter is a modal quantity.

R: Finishing allowance, specified by radius programming.

This parameter is modal, X(U), Z(W): coordinates of thread end point

i: Thread taper value, specified by radius programming. If R=0 it is straight thread.

k: thread height, specified by radius programming.

Δd: Depth of first turning, specified by radius programming.

L: Pitch.

In the above two instructions, the value after the Q, R, and P addresses should be expressed in the form of no decimal point.

A straight thread on the shaft of the part

G76 thread turning example: the above picture shows a straight thread on the shaft of the part, the thread height is 3.68mm, the thread pitch is 6mm, the chamfering at the end of the thread is 1.1L, the tool nose angle is 60°, the first turning depth is 1.8mm, The minimum turning depth is 0.1mm. The procedure is:

N16 G76 P011160 Q100 R200;

N18 G76 X60.64 Z25.0 P3680 Q1800 F6.0;