There are 11 kinds of fixed cycle instructions for hole processing in the FANUC system. Some of them are introduced below.
1) Drilling cycle command G81
The G81 drilling cycle command format is:
G81 G△△ X__ Y__ Z__ R__ F__
X, Y are the position of the hole, Z is the depth of the hole, F is the feed speed (mm/min), and R is the height of the reference plane. G△△ can be G98 and G99. The two modal commands G98 and G99 control whether the tool returns to the initial plane or the reference plane after the hole machining cycle is completed; G98 returns to the initial plane, which is the default mode; G99 returns to the reference plane. When programming, you can use absolute coordinate G90 and relative coordinate G91 programming. It is recommended to use absolute coordinate programming as much as possible.
The action process is as follows:
(1) The drill bit is quickly positioned to the starting point B (X, Y) of the hole processing cycle;
(2) The drill bit moves rapidly along the Z direction to the reference plane R;
(3) Drilling processing;
(4) The drill bit quickly returns to the reference plane R or to the initial plane B.
This command is generally used to process holes whose depth is less than 5 times the diameter. Programming example: The part shown in Figure a requires G81 to be used to process all holes. The CNC machining program is as follows:
picture
N02 T01 M06; Use No. T01 tool (Φ10 drill bit)
N04 G90 S1000 M03; Start the spindle to rotate forward at 1000r/min
N06 G00 X0. Y0. Z30. M08;
N08 G81 G99
N10
N12 Y30; drill hole at (50,30) position
N14 X10; drill holes at (10,30)
N16 G80; cancel drilling cycle
N18 G00 Z30
N20 M30
2) Drilling cycle command G82
The G82 drilling cycle command format is:
G82 G△△ X__ Y__ Z__ R__ P__ F__
In the command, P is the pause time of the drill bit at the bottom of the hole, the unit is ms (millisecond), and the meaning of the other parameters is the same as G81.
This command adds a feed pause action at the bottom of the hole, that is, when the drill bit reaches the bottom of the hole, the tool does not make any feed movement and remains in a rotating state to make the bottom of the hole smoother. G82 is generally used for enlarging and countersunk holes.
The action process is as follows:
(1) The drill bit is quickly positioned to the starting point B (X, Y) of the hole processing cycle;
(2) The drill bit moves rapidly along the Z direction to the reference plane R;
(3) Drilling processing;
(4) The drill bit pauses feeding at the bottom of the hole;
(5) The drill bit quickly returns to the reference plane R or to the initial plane B.
3) High-speed deep hole drilling cycle command G73
For the processing of holes with a depth greater than 5 times the diameter, since it is deep hole processing, which is not conducive to chip removal, interval feeding (feeding in multiple times) is used. The depth of each feed is Q, and the depth of the last feed is ≤ Q , the retraction amount is d (set internally by the system) until the bottom of the hole. See Figure b.
The G73 high-speed deep hole drilling cycle command format is:
G73 G△△ X__ Y__ Z__ R__ Q__ F__
In the command, Q means each feed depth is Q, and the meanings of other parameters are the same as G81.
The action process is as follows:
(1) The drill bit is quickly positioned to the starting point B (X, Y) of the hole processing cycle;
(2) The drill bit moves rapidly along the Z direction to the reference plane R;
(3) Drilling processing, the feed depth is Q;
(4) Retract the tool, the retraction amount is d
(5) Repeat (3) and (4) until the required processing depth
(6) The drill bit quickly returns to the reference plane R or to the initial plane B.
4) Tapping cycle command G84
The G84 thread machining cycle command format is:
G84 G△△ X__ Y__ Z__ R__ F__
The thread tapping process requires a strict proportional relationship between the spindle speed S and the feed speed F. Therefore, the feed speed needs to be calculated based on the spindle speed during programming. The feed speed F = spindle speed × thread pitch. The meaning of the other parameters is the same as G81. The spindle rotates forward when tapping and feeding using G84, and reverse when exiting. What is different from drilling is that the return process after tapping is not a rapid movement, but a reverse exit at the feed speed. Before the instruction is executed, the spindle does not even need to be started. When the instruction is executed, the CNC system will automatically start the spindle forward rotation.
The action process is as follows:
(1) The spindle rotates forward, and the tap is quickly positioned to the starting point B (X, Y) of the thread processing cycle;
(2) The tap moves rapidly along the Z direction to the reference plane R;
(3) Tapping processing;
(4) The spindle is reversed, and the tap is reversed and returned to the reference plane R at the feed speed;
(5) When using the G98 command, the tap quickly returns to the initial plane B.
Programming example: Tapping the 4 holes in Figure 5-34 with a tapping depth of 10mm. The CNC machining program is:
N02 T01 M06; Use No. T02 tool (Φ10 tap. The pitch is 2mm)
N04 G90 S150 M03; Start the spindle to rotate forward 1000r/min
N06 G00 X0. Y0. Z30. M08;
N08 G84 G99 Spindle speed) 150 × (thread pitch) 2 = 300
N10 X50; Tapping at the (50, 10) position (G84 is a modal command until G80 is canceled)
N12 Y30; Tapping at (50,30) position
N14 X10; Tapping at (10,30) position
N16 G80; cancel tapping cycle
N18 G00 Z30
N20 M30
5) Left-hand tapping thread cycle command G74
The G74 thread machining cycle command format is:
G74 G△△ X__ Y__ Z__ R__ F__
The difference from G84 is that the spindle rotates reversely during feed and forward when exiting. The meaning of each parameter is the same as G84.
The action process is as follows:
(1) The spindle is reversed and the tap is quickly positioned to the starting point B (X, Y) of the thread processing cycle;
(2) The tap moves rapidly along the Z direction to the reference plane R;
(3) Tapping processing;
(4) The spindle rotates forward, and the tap returns to the reference plane R at the feed speed;
(5) When using the G98 command, the tap quickly returns to the initial plane B.
6) Boring processing cycle command G85
The G85 boring processing cycle command format is:
G85 G△△ X__ Y__ Z__ R__ F__
The meaning of each parameter is the same as G81.
The action process is as follows:
(1) The boring tool is quickly positioned to the starting point B (X, Y) of the boring processing cycle;
(2) The boring tool quickly moves along the Z direction to the reference plane R;
(3) Boring processing;
(4) The boring tool returns to the reference plane R or the initial plane B at the feed speed;
7) Boring processing cycle command G86
The G86 drilling cycle command format is:
G86 G△△ X__ Y__ Z__ R__ F__
The difference from G85 is that after reaching the bottom of the hole, the spindle stops and exits quickly. The meaning of each parameter is the same as G85.
The action process is as follows:
(1) The boring tool is quickly positioned to the starting point B (X, Y) of the boring processing cycle;
(2) The boring tool quickly moves along the Z direction to the reference plane R;
(3) Boring processing;
(4) The spindle stops and the boring tool quickly returns to the reference plane R or the initial plane B;
8) Boring processing cycle command G89
The G89 boring processing cycle command format is:
G89G△△ X__ Y__ Z__ R__ P__ F__
The difference from G85 is: after reaching the hole bottom position, the feed is paused. P is the pause time (ms), and the meanings of other parameters are the same as G85.
The action process is as follows:
(1) The boring tool is quickly positioned to the starting point B (X, Y) of the boring processing cycle;
(2) The boring tool quickly moves along the Z direction to the reference plane R;
(3) Boring processing;
(4) Feed pause;
(5) The boring tool returns to the reference plane R or the initial plane B at the feed speed;
9) Fine boring cycle command G76
The G76 boring processing cycle command format is:
G76 G△△ X__ Y__ Z__ R__ P__ Q__ F__
The difference from G85 is that G76 has three actions at the bottom of the hole: feed pause, spindle accurate stop (directional stop), reverse offset of the tool along the tool tip by the Q value, and then rapid exit. This ensures that the tool does not scratch the surface of the hole. P is the pause time (ms), Q is the offset value, and the meanings of the other parameters are the same as G85.
The action process is as follows:
(1) The boring tool is quickly positioned to the starting point B (X, Y) of the boring processing cycle;
(2) The boring tool quickly moves along the Z direction to the reference plane R;
(3) Boring processing;
(4) Feed pause, spindle accurate stop, and reverse offset of the tool along the tool tip;
(5) The boring tool quickly exits to the reference plane R or the initial plane B;
10) Back boring cycle command G87
The command format of the G87 back boring processing cycle command is:
G87 G△△ X__ Y__ Z__ R__ Q__ F__
The meaning of each parameter is the same as G76.
The action process is as follows:
(1) The boring tool is quickly positioned to the starting point B (X, Y) of the boring processing cycle;
(2) The spindle stops accurately and the tool offsets in the opposite direction of the tool tip;
(3) Quickly move to the bottom of the hole;
(4) The tool tip shifts back to the processing position in the positive direction, and the spindle rotates forward;
(5) The tool feeds upward to the reference plane R;
(6) The spindle stops accurately, and the tool is offset by the Q value in the opposite direction of the tool tip;
(7) The boring tool quickly exits to the initial plane B;
(8) Offset along the positive direction of the tool tip;
11) Cancel the hole machining cycle command G80
