CNC machining method for multi-thread
1. Machining multi-thread by changing the initial angle of thread cutting
1 Principle of the method
Machining multi-thread by changing the initial angle of thread cutting is to divide the number of threads along the circumferential direction. After machining each thread, the spindle rotates a certain angle, while the axial position of the starting point remains unchanged, and then the next thread is processed.
2 Application of G32 instruction to process multi-thread
2.1 Instruction format
G32X(U)__Z(W)__F__Q__;
Where:
X, Z——the end point coordinates of the thread when programming in absolute dimension;
U, W——the end point coordinates of the thread when programming in incremental dimension;
F——thread lead (if it is a single thread, it is the thread pitch);
Q——thread starting angle, the value is a non-modal value without a decimal point, that is, the increment is 0.0010;
If the starting angle is 1800, it is expressed as Q180000 (single thread can be specified without specifying, in which case the value is zero);
The range of the starting angle Q is between 0 and 360000. If a value greater than 360000 is specified, it is calculated as 360000 (3600).
2.2 Application examples
Example 1, thread processing program compiled with G32 instruction.
Process analysis:
The part has a double thread M24X3 (P1.5) -6g, with a pitch of 1.5mm and a lead of 3mm. The programming origin is set at the center of the right end face of the workpiece.
Cutting parameter determination:
Check the turning manual to determine the cutting depth (radius value) of 0.974mm, the number of feeds is 4 times, and the cutting depth (diameter value) of each back of the knife is 0.8mm, 0.6mm, 0.4mm, and 0.16mm respectively.
S1 (speed-up feed section length) = 4mm, S2 (speed-down retraction section length) = 2mm.
Assuming the starting angle of the first thread is 00, the starting angle of the second thread is 3600/2=1800
The reference program is as follows:
……；
G00X30.0Z4.0；
X23.2；
G32Z-32.0F3.0Q0； /1st thread, first cut
G00X30.0Z4.0；
X22.6；
G32Z-32.0F3.0Q0； /1st thread, second cut
……；
G00 X30.0Z4.0；
X22.04；
G32Z-32.0F3.0Q0； / 4th cut of the first thread
G00X30.0Z4.0；
X23.2；
G32Z-32.0F3.0Q180000；/ 1st cut of the second thread
G00X30.0Z4.0；
X22.6；
G32Z-32.0F3.0Q180000；/ 2nd cut of the second thread
……；
G00X30.0Z4.0；
X22.04；
G32Z-32.0F3.0Q180000；/ 4th cut of the second thread
G00X30.0；
X100.0Z100.0；
M05；
M30；
2.3 Using G92 command to process multiple threads
2.3.1 Instruction format
G92X(U)__Z(W)__F__Q__;
The meaning of each parameter in the formula is the same as 1.2.1
2.3.2 Application example
Example 2, thread processing program compiled with G92 instruction.
Process analysis:
The part has multiple threads M30X3(P1.5)-6G, with a pitch of 1.5mm and a lead of 3mm. The programming origin is set at the center of the left end face of the workpiece.
Cutting parameter determination (omitted)
The reference program is as follows:
……;
G92X29.2Z18.5F3.0; /Double thread cutting cycle 1, back cutting amount 0.8mm
X29.2Q180000;
X28.6F3.0; /Double thread cutting cycle 2, back cutting amount 0.6mm
X28.6Q180000;
X28.2F3.0; /Double thread cutting cycle 3, back cutting amount 0.4mm
X28.2Q180000;
X28.04F3.0; /Double thread cutting cycle 4, back cutting amount 0.16mm
X28.04Q180000;
M05;
M30;
II. Processing multi-thread by changing the starting point of thread cutting
1 Principle of the method
The method of changing the starting point of thread cutting is used to process multiple threads. When programming, the starting point of the first thread is first determined, and the first thread processing is completed using the thread processing instruction. Before processing the second thread, the starting point of the cutting should be re-determined, and the axial difference from the starting point of the first thread is a pitch P. By analogy, multiple threads can be turned.
Assume that the thread lead is F and the number of threads is n, then the pitch P=F/n. As shown in Figure 3, the axial difference of each thread is a pitch P. If point A is the starting point of the first thread and point B is the starting point of the second thread, then the Z direction value of the starting point of the second thread is the Z direction value of the starting point of the first thread plus a pitch P.
Since the position of the thread cutting starting point changes, while the cutting end point remains unchanged, the cutting length of each thread should be increased or decreased by a pitch when programming to ensure the consistency of the end points of each thread [3].
2 Use G92 command to process multi-thread
2.1 Command format
G92X(U)__Z(W)__F__;
2.2 Application examples
Example 3: Use G92 command to program thread processing.
The part has double-thread M24X3(P1.5), with a pitch of 1.5mm and a lead of 3mm.
The programming origin is set at the center of the right end face of the workpiece.
Reference program:
……
G00X30.0Z4.0; /Starting point of the first thread cycle
G92X23.2Z-22.0F3.0; /1st thread cutting cycle 1, back cutting depth 0.8mm
X22.6; /1st thread cutting cycle 2, back cutting depth 0.6mm
X22.2; /1st thread cutting cycle 3, back cutting depth 0.4 mm
X22.04; /1st thread cutting cycle 4, back cutting depth 0.16 mm
G00X30.0Z5.5; /Determine the starting point of the second thread cycle (the cutting starting point of the second thread is offset by 1 pitch relative to the starting point of the first thread)
G92X23.2Z-22.0F3.0; /2nd thread cutting cycle 1, back cutting depth 0.8mm
X22.6; /2nd thread cutting cycle 2, back cutting depth 0.6 mm
X22.2; /2nd thread cutting cycle 3, back cutting depth 0.4 mm
X22.04; /2nd thread cutting cycle 4, back cutting depth 0.16 mm
X100.0Z100.0;
M05;
M30;
3. Apply G76 command to process multiple threads
3.1 Command format
G76P(m)(r)(a) Q(△dmin)R(d);
G76X(U)__Z(W)__R(i)P(k)Q(△d)F(L);
Where:
m——Number of finishing repetitions (1-99), modal value
r——Chamfering amount, modal value
a——Tool tip angle (thread profile angle), modal value, generally 600
△dmin——Minimum back cutting amount (radius value), modal value
d——Finishing allowance (radius value), modal value
X(U), Z(W)——thread end coordinate value
i——thread taper value (radius difference), if i=0, it is a common cylindrical thread, which can be omitted
k——thread height (radius value)
△d——first back cutting amount (radius value)
L——thread lead
m, r, a are specified by address P at the same time, for example, when m=2, r=1.2L, a=600, it is expressed as P021260
3.2 Application example
Example 4, thread machining program compiled with G76 instruction.
The part has double thread M30X4 (P2.0), pitch is 2.0mm, lead is 4mm, and the programming origin is set at the center of the right end face of the workpiece.
Reference program: (assuming that the actual major diameter of the thread has been processed)
……;
G00X35.0Z3.0S350M03; /1st thread positioning
G76P021260Q100R100;
G76X26.97Z-30.0R0P1510Q200F4.0;
G00Z5.0; /2nd thread positioning (the cutting starting point of the 2nd thread is offset by 1 pitch relative to the starting point of the 1st thread)
G76P021260Q100R100;
G76X26.97Z-30.0R0P1510Q200F4.0;
G28U0W0;
M05;
M30; |
