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 rate (mm/min), and R is the height of the reference plane. G△△ can be G98 and G99, G98 and G99 two modal commands to control whether the tool returns to the initial plane or the reference plane after the hole machining cycle ends; G98 returns to the initial plane, which is the default mode; G99 returns to the reference plane. Absolute coordinate G90 and relative coordinate G91 can be used for programming. It is recommended to use absolute coordinate programming as much as possible.

The action process is as follows:

1) The drill is quickly positioned to the starting point B (X, Y) of the hole machining cycle;

2) The drill bit quickly moves along the Z direction to the reference plane R;

3) Drilling processing;

4) The drill bit quickly retracts to the reference plane R or quickly returns to the initial plane B.

This command is generally used to machine holes with a depth of less than 5 times the diameter. Programming example: The part as shown in Figure a requires all holes to be machined with G81. The NC machining program is as follows:

N02 T01 M06; Use T01 tool (Φ10 drill bit)

N04 G90 S1000 M03; Start the spindle forward rotation 1000r/min

N06 G00 X0. Y0. Z30. M08;

N08 G81 G99 X10. Y10. Z-15. R5 F20; Drill holes at position (10, 10), the depth of the hole is 15mm, the height of the reference plane is 5mm, and the drilling cycle ends and returns to the reference plane

N10 X50; Drill holes at the position (50, 10) (G81 is a modal command, until G80 is cancelled)

N12 Y30; Drill holes at (50,30) position

N14 X10; Drill at (10,30) position

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 instruction, P is the pause time of the drill at the bottom of the hole, the unit is ms (milliseconds), and the other parameters have the same meaning as G81. If you want to learn UG programming, you can add to the QQ group: 304214709 to receive the UG tutorial. Learn UG programming from the beginning

This instruction adds a feed pause action at the bottom of the hole, that is, when the drill is processed to the bottom of the hole, the tool does not feed and keeps rotating to make the bottom of the hole smoother. G82 is generally used for reaming and countersinking.

The action process is as follows:

1) The drill is quickly positioned to the starting point B (X, Y) of the hole machining cycle;

2) The drill bit moves quickly to the reference plane R along the Z direction;

3) Drilling processing;

4) The drill pauses to feed at the bottom of the hole;

5) The drill bit quickly retracts to the reference plane R or quickly retracts to the initial plane B.

3. High-speed deep hole drilling cycle command G73

For the machining of holes with a depth of more than 5 times the diameter, because it is deep hole machining, which is not conducive to chip removal, so the interval feed (multiple feeds) is adopted, the depth of each feed is Q, and the depth of the last feed is ≤Q , The retraction amount is d (set 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 is the depth of each feed, and the meaning of the other parameters is the same as G81.

The action process is as follows:

1) The drill is quickly positioned to the starting point B (X, Y) of the hole machining cycle;

2) The drill bit moves quickly to the reference plane R along the Z direction;

3) Drilling, the feed depth is Q;

4) Withdraw the knife, the amount of withdrawal is d

5) Repeat (3) and (4) until the required processing depth

6) The drill bit quickly retracts to the reference plane R or quickly returns to the initial plane B.

4. Tapping cycle command G84

The G84 thread processing 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, when programming, it is required to calculate the feed speed according to the spindle speed. The feed speed F=spindle speed × thread pitch, and the meaning of other parameters is the same as G81. When using G84 tapping feed, the spindle rotates forward, and when it exits, the spindle rotates backward. The difference from drilling is that the return process after tapping is not a rapid movement, but a reverse exit at the feed rate.

Before the instruction is executed, the spindle may not even 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 machining cycle;

2) The tap moves quickly along the Z direction to the reference plane R;

3) Tapping processing;

4) The spindle reverses, and the tap returns to the reference plane R at the feed rate reversed;

5) When the G98 command is used, the tap quickly returns to the initial plane B.

Programming example: tap the 4 holes in Figure 5-34, the tapping depth is 10mm, the CNC machining program is:

N02 T01 M06; Use T02 tool (Φ10 tap. Pitch is 2mm)

N04 G90 S150 M03; Start spindle forward rotation 1000r/min

N06 G00 X0. Y0. Z30. M08;

N08 G84 G99 X10. Y10. Z-10. R5 F300; Tapping at the position (10, 10), the depth of the thread is 10mm, the height of the reference plane is 5mm, the thread processing cycle ends and returns to the reference plane, the feed rate F=( Spindle speed) 150×(thread pitch) 2=300

N10 X50; Tapping at the position (50, 10) (G84 is a modal command until G80 is cancelled)

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 with G84 is that the spindle rotates in the reverse direction when feeding, and it rotates in the forward direction 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 machining cycle;

2) The tap moves quickly 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 rate when it rotates forward;

5) When the G98 command is used, the tap quickly returns to the initial plane B.

6. Boring machining cycle command G85

The command format of G85 boring machining cycle command 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 machining 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 rate.

7. Boring machining cycle command G86

The G86 drilling cycle command format is:

G86 G△△ X__ Y__ Z__ R__ F__

The difference with G85 is: after reaching the hole bottom position, 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 machining 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 machining cycle command G89

The G89 boring machining cycle command format is:

G89G△△ X__ Y__ Z__ R__ P__ F__

The difference with G85 is: after reaching the hole bottom position, the feed pauses. P is the pause time (ms), the meaning of other parameters 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 machining 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 rate.

9. Fine boring cycle command G76

The G76 boring machining cycle command format is:

G76 G△△ X__ Y__ Z__ R__ P__ Q__ F__

The difference with G85 is: G76 has three actions at the bottom of the hole: feed pause, spindle stop (orientation stop), the reverse offset Q value of the tool along the tool tip, 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 other parameters have the same meaning 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 machining cycle;

2) The boring tool quickly moves along the Z direction to the reference plane R;

3) Boring processing;

4) Feed pause, accurate spindle stop, 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 G87 back boring machining cycle command format 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 machining cycle;

2) The spindle stops exactly and the tool is offset in the opposite direction of the tool tip;

3) Quickly move to the bottom of the hole;

4) The tool nose shifts back to the machining position in the positive direction, and the spindle rotates forward;

5) The tool feeds upwards to the reference plane R;

6) The spindle stops exactly, 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 in the positive direction of the tool nose.