HNC-818. User Manual

12. Fixed Cycle

3. Conduct boring downward at the

speed of F.

4. Move to the point Z at the hole bottom.

5. Exit upward rapidly to the point R (the spindle remains rotation).

6. Exit upward rapidly to the point B in the G98 mode.

Attention

1. The boring axis must be the Z axis.

2. The point Z must be lower than the plane of point R; otherwise, an

alarm will be reported.

3. If the motion amount of Z, Q, and K are zero, the cycle is not

executed.

4. The G85 command data is saved as modal data.

5. Before using the command of G85, use the corresponding M

command to rotate the spindle.

Example

Conduct boring of the holes as shown in the figure below:

%3351

N10 G92 X0 Y0 Z80

N15 M03 S600

N20 G98 G85 G91 X20 Y15 G90 R20 Z-3 L2 F100

183

12. Fixed Cycle

12.1.13 Boring Cycle (G86)

Description

The operation specified by G86 is similar as G81. In the G86 mode, the

spindle stops at the hole bottom and the tool exits rapidly. The command

is used to bore the holes which have low requirement for precision.

Format

(G98/G99) G86 X_ Y_ Z_ R_ F_ L_;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91).

The absolute position of the hole bottom for absolute

programming (G90), or the distance from the hole

bottom to the point R for incremental programming

(G91)

The absolute position of the point R for absolute

programming (G90), or the distance from the point R to

the initial plane for incremental programming (G91).

Cutting feed speed.

The repeat count

(Generally used for multi-hole

machining to simplify programming. It is optional

when L=1.)

Operation procedure

1. The tool moves rapidly to the point B over the hole center.

2. Move rapidly to the point R, close to the workpiece.

3. Conduct boring downward at the speed of F.

4. Reach the hole bottom of point Z.

5. The spindle stops rotation.

6. Exit upward rapidly to the point R (G99) or B (G98).

7. The spindle restores clockwise rotation.

Attention

1. If the movement amount of Z is zero, the command is not executed.

2. The G86 command data is saved as modal data.

185

12. Fixed Cycle

3. The boring axis must be the Z axis.

4. The point Z must be lower than the plane of point R; otherwise, an

alarm will be reported.

Example

Conduct boring of the hole as shown in the figure below:

%3353; Reaming with a reamer

N10 G92 X0 Y0 Z80

N15 G98 G86 G90 X20 Y15 R20 Z-2 F200

N20 X40 Y30

N30 G90 G00 X0 Y0 Z80

N40 M30

186

12. Fixed Cycle

12.1.14 Anti-Boring Cycle(G87)

Description

The instruction is generally used to bore holes which are smaller at the

upper part and larger at the lower part. The hole bottom point Z is

generally above the reference point R, which is different from other

instructions.

Initial point

Offset (I, J)

Positioning point R

Point Z

Point R

Reverse offset (I, J)

Format

(G98/G99) G87X_ Y_ Z_ R_ I_ J_ P_ F_ L_;

Parameter

Description

X Y

The absolute position the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91).

The absolute position of the hole bottom along Z axis

for absolute programming (G90), or the distance from

the hole bottom to the point R for incremental

programming (G91)

The absolute position of the point R along Z axis for

absolute programming (G90), or the distance from the

point R to the initial plane for incremental

programming (G91).

Offset value along X axis.

Offset value along Y axis.

The duration that the tool remains at the hole bottom.

Unit: millisecond.

Cutting feed speed.

The repeat count (Generally used for multi-hole

187

12. Fixed Cycle

Operation procedure

1. The tool moves rapidly to the point B over the hole center.

2. The spindle conducts orientation and stops rotation.

3. The boring tool rapidly moves away from the tool nose with the

distance specified by I or J.

4. Move rapidly to the point R.

5. Move rapidly in the positive direction of the tool nose with the

distance specified by I or J, and the tool moves back to the hole

center specified by X, Y.

6. The spindle rotates in the clockwise direction.

7. Conduct boring upward at the speed of F, to the point Z at the hole

bottom.

8. Remain at the hole bottom for P milliseconds (The spindle remains

rotation).

9. The spindle conducts orientation and stops rotation.

10. The boring tool rapidly moves away from the tool nose with the

distance specified by I or J.

11. Exit upward rapidly to the point B (G98).

12. Move rapidly in the positive direction of the tool nose with the

distance specified by I or J, and the tool moves back to the hole

center point B.

13. The spindle restores the clockwise rotation.

Attention

1. The boring axis must be the Z axis.

2. If the movement amount of Z is zero, the command is not executed.

3. The point Z must be higher than the plane of point R; otherwise, an

alarm will be reported.

4. The G87 command data is saved as modal data.

5. Only G98 can be used for G87.

6. Before using the command of G87, use the corresponding M

command to rotate the spindle.

189

12. Fixed Cycle

12.1.15 Boring Cycle (Manual Boring) (G88)

Description

Before boring, this instruction memories the initial point B or reference

point R. When the boring tool automatically processes to the hole bottom,

the machine stops. You may manually change the operation mode to

"Manual", and move the tool upward to the point B or R, and avoid the

workpiece. Then the operation mode is changed back to the automatic

operation mode. Start the program again, and the tool returns back to the

point B or R. This instruction is generally used for precise boring with

milling machines, without calling the spindle exact stop function.

Return to point

B; spindle CW

Initial point B

Reference point R

Return to point

R; spindle CW

Reference point R

G98

G99

Hole bottom point

Hole bottom

Remains at the hole bottom

point Z

and the spindle stops

Format

G98 (G99) G88 X_ Y_ Z_ R_ P_ F_ L_

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current

tool position to the hole for incremental programming

(G91).

The absolute position of the hole bottom along axis Z

for absolute programming (G90), or the distance from

the hole bottom to the point R for incremental

programming (G91).

The absolute position of the point R along Z axis for

absolute programming (G90), or the distance from the

point R to the initial plane for incremental

programming (G91).

The duration that the tool remains at the hole bottom.

Unit: millisecond.

Boring feed speed.

The repeat count

(Generally used for multi-hole

machining, and therefore X or Y is incremental value.)

191

12. Fixed Cycle

Operation procedure

The tool moves rapidly to the point B over the hole center.

Move rapidly to the point R, close to the workpiece surface.

Conduct boring downward at the speed of F, to the point Z at the

hole bottom.

Remain at the hole bottom for P seconds (The spindle remains

rotation).

The spindle stops rotation.

Manually move the tool until it is over the point R (G99) or B

(G98).

Press Start in the auto operation mode, the tool rapidly moves to

the point R (G99) or B (G98).

The spindle restores the clockwise rotation.

Attention

The boring axis must be the Z axis.

If the movement amount of Z is zero, the command is not executed.

The point Z must be lower than the plane of point R; otherwise, an

alarm will be reported.

The G88 command data is saved as modal data.

If G99 is used, manually move the tool to the place over the point of

If G98 is used, manually move the tool to the place over the point of

Before using the command of G88, use the corresponding M

command to rotate the spindle.

192

12. Fixed Cycle

12.1.16 Boring Cycle (G89)

Description

This operation specified by the command G89 is almost the same as that

of G86. In the G89 mode, the spindle pauses at the hole bottom. Before

specifying G89, use auxiliary function the M command to rotate the

spindle. When the G89 command and M command are specified in the

same block, the system executes the M command while the first

positioning movement is performing , and then conducts the next boring.

If the repeat count L is specified, the system executes the M command

only for the first boring hole.

The operation specified by G89 is as shown below:

Initial plane

Plane of point R

Point R

Point Z

Pause

G89 (G98)

G89 (G99)

This cycle is used for boring.

Format

(G98/G99) G89 X_ Y_ Z_ R_ P_ F_ L;

Parameter

Description

X Y

The absolute position of the hole for absolute

programming (G90), or the distance from the current tool

position to the hole for incremental programming (G91).

The absolute position of the hole bottom for absolute

programming (G90), or the distance from the hole bottom

to the point R for incremental programming (G91).

The absolute position of the point R for absolute

programming (G90), or the distance from the point R to

the initial plane for incremental programming (G91).

The duration that the tool remains at the hole bottom.

Unit: millisecond.

Cutting feed speed.

194

12. Fixed Cycle

Attention

1. The boring axis must be the Z axis.

2. The point Z must be lower than the plane of point R; otherwise, an

alarm will be reported.

3. The G89 command data is saved as modal data.

4. G89 is similar as G86, but with a pause at the hole bottom.

5. If the movement amount of Z is zero, this command is not executed.

6. Before using the command of G89, use the corresponding M

command to rotate the spindle.

Example

M3 S1000; The spindle starts rotation.

G90 G99 G89 X300 Y-250 Z-150 R-120 P1000 F120; Conduct

positioning, and conduct boring for hole 1, return to the point R and then

pauses at the hole bottom for one second

Y-550; Conduct positioning, and conduct boring for hole 2; return

to the point R

Y-750; Conduct positioning, and conduct boring for hole 3; return to the

point R

X1000; Conduct positioning, and conduct boring for hole 4; return to the

point R

Y-550; Conduct positioning, and conduct boring for hole 5; return to the

point R

G98 Y-750; Conduct positioning, and conduct boring for hole 5; return to

the initial plane

G80 G28 G91 X0 Y0 Z0; Cancel boring and return to the reference point

M5; The spindle stops rotation.

196

12. Fixed Cycle

12.1.18 Arc Groove Cycle (Type 1) (G181)

Description

This command is used to process the grooves arranged according to an

arc. The groove width is defined by the tool diameter.

(G98/G99) G181 R_ Z_ N_ K_ X_ Y_ I_ A_ B_ F_ Q_ V_

Format

Parameter

Description

The coordinate value of the reference point R for

absolute programming, or the distance from reference

point R to the initial plane for incremental

programming.

The coordinate value of the groove bottom for absolute

programming, or the incremental value from the

groove bottom to the reference point R for incremental

programming.

The number of grooves (It is optional when N=1)

The length of the groove.

The center of the arc formed by the grooves. The first

axis coordinate of the current plane for absolute

programming, and the incremental value relative to the

start point for incremental programming.

The center of the arc formed by the grooves. The

second axis coordinate of the current plane for absolute

programming, and the incremental value relative to the

start point for incremental programming.

The radius of the arc formed by the grooves.

Start angle (-180 to 180 degrees, positive in the CCW

direction and negative in the CW direction. It is

optional when A=0)

198

12. Fixed Cycle

Incremental angle (It is optional when B=360/N. A

positive B value indicates the milling in the CCW

direction; a negative B value indicates the milling in

the CW direction.

Milling speed.

The maximum feed depth each time (It is optional

when Q= groove depth , cutting to the bottom for a

time).

Tool radius.

Parameter graph

Operation procedure

Select a random start point from which the tool may move to each

groove without any collision.

Go to the reference position R over the near-end of the first groove

from the start point. The near-end indicates the end near to the

center of the arc groove. The groove specified by the start angle A

will be processed firstly.

Feed downward at the milling feed rate to the defined depth, and

then conduct milling back and forth until the bottom is machined.

Conduct deep feed at the groove end.

On the application axis (generally Z axis), exit the tool to the

reference point R. Select the shortest path to rapidly move to the

end of the next groove, and conduct milling back and forth until the

bottom is machined.

After completing the last groove, exit the tool to the initial point B

or the reference point R based on the current modal G98 or G99,

199

12. Fixed Cycle

and then the cycle ends.

N=3

Milling in the

A=180

CCW direction B=-90

Attention

The groove number N must be a non-negative integer. If not, the

negative symbol

(-) will be ignored, and the number will be

rounded.

The maximum feed depth is specified by the value of Q. If the

groove depth is not divisible by Q, the final cut depth will be less

than Q.

The milling direction for each groove is related to the symbol of B.

If the value of B is positive, the system starts the milling from the

first groove to the last in the CCW direction; if the value of B is

negative, the system starts the milling in the CW direction. If B is

not specified, the system will automatically derive B from B=360/N,

and conduct milling in the CCW direction.

The value of K, I, and Q should be non-negative values. If not, the

system will ignore the negative symbol.

Rotate the spindle before executing the cycle. For alarm information,

see section 12.1.26.

200

12. Fixed Cycle

Example

grooves as shown in the figure below: Groove length 30 mm; groove

depth 23 mm; feed depth 6 mm

A-B

90 degrees

degrees

%0526

N10

G54 X0 Y0 Z5

N20

G17 G90

N30

T10

N40

M06

N50

M03 S600

N60

G181 R0 Z-23 N4 K30 X40 Y45 I20 A45 B90 F100 Q6 V5

N70

M30

Conduct

milling

for

four

rectangle

201

12. Fixed Cycle

12.1.19 Arc Groove Cycle (Type 2) (G182)

Description

The instruction is used to process grooves which are arranged in an

annular array. The longitudinal shaft of these grooves turn up radially.

The instruction is different from G181, as the groove width can be

specified by a parameter, but not be defined by the tool diameter.

This cycle can be specified for rough and finish machining.

(G98/G99)G182 R_Z_N_K_W_X_Y_I_A_B_F_ Q_ E_O_H_U_P_C_D_V_

Format

Para

Description

meter

The coordinate value of the reference point R for absolute

programming, or the distance from reference point R to the

initial plane for incremental programming.

The coordinate value of the groove bottom for absolute

programming, or the incremental value from the groove

bottom to the reference point R for incremental

programming.

The number of grooves (It is optional when N=1)

The length of the groove.

The groove width (It is optional when W= tool diameter).

The center of the arc formed by the grooves. The first axis

coordinate of the current plane for absolute programming,

and the incremental value relative to the start point for

incremental programming.

202

12. Fixed Cycle

The center of the arc formed by the grooves. The second

axis coordinate of the current plane for absolute

programming, and the incremental value relative to the

start point for incremental programming.

The radius of the arc formed by the grooves.

Start angle (-180 to 180 degrees, positive in the CCW

direction and negative in the CW direction. It is optional

when A=0)

Incremental angle (It is optional when B=360/N. A positive

B value indicates the milling in the CCW direction; a

negative B value indicates the milling in the CW direction.

Milling speed for rough machining.

The maximum feed depth for rough machining each time(It

is optical when Q=groove depth -the depth of groove

Parameter graph

bottom left for finish machining).

The finish allowance at the edge of the groove(It is optional

when E=0).

The finish allowance in the groove bottom(It is optional

when O=0).

The maximum feed depth for finish machining(It is

optional when H=Q).

Feed speed for finish machining(It is optional when U=F).

Spindle speed for finish machining(It is optional when

P=spindle speed before the cycle or default spindle speed).

The direction for milling each groove (It is optional when

C=3)

0：milling in the same direction with the spindle rotation；

1：milling in the reversed direction with the spindle

rotation； 2：milling in G02 direction； 3：milling in G03

direction

1：rough machining 2：finish machining (It is optional when

D=1).

Tool radius.

203

12. Fixed Cycle

Before entering the cycle mode, you need to use the command to enable

spindle rotation. The system will calculate the reasonable milling

Milling direction

direction based on the spindle rotation direction (M03/M04) and the

command . See the table below:

Milling direction

Execute M03/M04 before the cycle

(Parameter C)

M03 spindle CW

M04 spindle CCW

0: same direction

G03

G02

1: reversed direction

G02

G03

2: in G02 direction

G02

3: in G03 direction

G03

Left blank

G03

Select the start point , a random start point from which the tool may

move to each groove without any collision.

Operation procedure

Go to the reference point R over the first groove. The groove

specified by the start angle A will be processed firstly.

Rough machining (D=1):

Starting at the groove end, the tool conducts milling from the

middle part to the margin and from the groove surface to the finish

allowance in the milling direction specified by C. Each time the tool

feeds at the same point of the groove end until it reaches finish

allowance in the groove bottom.

Finish machining (D=2):

Conduct finish machining for the groove wall and then the groove

bottom. Conduct milling from the middle part to the defined groove

margin in the milling direction specified by the parameter C, and

then back to the the same start position, conduct milling downward

to the groove bottom

204

12. Fixed Cycle

After completing a groove, exits the tool to the reference point R.

Rapidly move to the near-end of the next groove, and repeat step 3

until completing the last groove.

Exits the tool to the initial point B or the reference point R with

G98 or G99, and then the cycle ends.

The tool radius cannot exceed the specified groove width W;

otherwise, an alarm will be reported.

The groove number N must be a non-negative integer. If not, the

Attention

system will ignore the negative symbol, and conduct rounding for

the non-integer.

Q and H both specify the maximum feed depth . If the groove depth

is not divisible by Q or H, the final cut depth will be less than Q or

The milling direction for each groove is specified by the parameter

C. The milling direction between grooves is specified by the

parameter B. If the value of B is positive, the system starts the

milling from the first groove to the last in the CCW direction; if the

value of B is negative, the system starts the milling in the CW

direction. If B is not specified, the system will automatically derives

B from B=360/N, and conduct milling in the CCW direction.

The values of parameter K, W, I, E, O, H and Q should be

non-negative values. If the value is negative, the system will ignore

the negative symbol.

Rotate the spindle Before executing the cycle. The finish allowance

(E) specified for the groove margin cannot exceed half of the

groove width (W/2), and the finish allowance (O) specified for the

groove bottom cannot exceed the groove depth; otherwise, an alarm

will be reported. For more alarm information, see section 12.1.26.

205

12. Fixed Cycle

Example

Conduct milling for four grooves as shown in the figure below:

Groove length 30 mm; groove width 15 mm; groove depth 23 mm; finish

allowance

0.5 mm; milling direction G02; feed depth for rough

machining 6 mm; tool radius: 5 mm

90 degrees

A-B

45°

%0527

N10 G54 G17 G90

N20 T10

N30 M06

N40 M03 S600

N50 G182R5Z-23N4K30X40Y45W15I20A45B90F100Q6E0.5O0.5C2 V5

N60 M30

206

12. Fixed Cycle

12.1.20 Circumference Groove Milling Cycle (G183)

Description

This cycle is used to process circumference grooves distributed in a

circle shape. You may specify roughing, finishing or comprehensive

machining.

(G98/G99)G183R_Z_N_K_W_X_Y_I_A_B_F_ Q_E_O_H_U_P_C_D_V_

Format

Parameter

Description

The coordinate value of the reference point R for

absolute programming, or the distance from reference

point R to the initial plane for incremental

programming.

The coordinate value of the groove bottom for absolute

programming, or the incremental value from the

groove bottom to the reference point R for incremental

programming.

The number of grooves (It is optional when N=1 ).

The angle of groove length (0 to 360 degrees. Unit:

degree).

The width of the groove (It is optional when W= tool

diameter ).

The center of the circle rounded by the grooves. The

first axis coordinate of the current plane for absolute

programming, and the incremental value to the start

point for incremental programming.

207

12. Fixed Cycle

The center of the circle rounded by the grooves. The

second axis coordinate of the current plane for absolute

programming, and the incremental value to the start

point for incremental programming.

The radius of the circle rounded by the grooves.

Start angle (-180 to 180 degrees, positive in the CCW

direction and negative in the CW direction. It is

optional when A=0.)

Incremental angle (It is optional when B=360/N ; a

positive B value indicates the milling in the CCW

direction while a negative B value indicates the milling

in the CW direction.

Milling speed during rough machining.

The maximum feed depth for each time during rough

machining (It is optional when Q= groove depth- finish

ing allowance of the groove bottom).

The finishing allowance of the groove margin (It is

optional when E=0).

The finishing allowance in the groove bottom (It is

optional when O=0).

The feed rate for finish machining (It is optional when

U=F).

The spindle speed for finish machining (It is optional

when P= the spindle speed before cycle ).

The direction for milling each groove (It is optional

when C=3)

0：milling in the same direction with the spindle

rotation； 1：milling in the reversed direction with the

spindle rotation； 2：milling in G02 direction； 3：

milling in G03 direction

Machining type (It is optional when D=1)

1: rough machining;

2: finish machining

Tool radius.

208

12. Fixed Cycle

Parameter graph

Milling direction

Before entering the cycle mode, you need to use the command to enable

spindle rotation. The system will calculate the reasonable milling

direction (M03/M04) based on the spindle rotation and the command .

See the table below:

Milling Direction

Execute M03/M04 before the cycle

(Parameter C)

M03 spindle CW

M04 spindle CCW

0: same direction

G03

G02

1: reversed direction

G02

G03

2: in G02 direction

G02

3: in G03 direction

G03

Left blank

G03

Operation procedure

During the cycle, use G00 to move to the reference plane R.

Conduct milling for the current groove from middle part to the edge.

The operation procedure is similar as that of G182.

After completing a groove, exit the tool to the reference plane and

move to the next groove.

After completing all grooves, exit the tool with the G98 or G99

command, and then the cycle ends.

209

12. Fixed Cycle

Example

Conduct milling for three grooves shown in the figure below:

Circle center: (X60, Y60); radius on the XY plane: 42 mm; groove width:

15 mm; groove length angle: 70 degrees; groove depth: 23 mm; start

angle: 0 degree; incremental angle: 120 degrees; finishing allowance on

the groove contour: 0.5 mm; feed depth: 6 mm; tool radius 5 mm

The spindle speed and feed rate for rough and finish machining are the

same. The finish machining is completed with one cut.

See the figure below:

A-B

70°

120°

%0528

N10 G54 G17 G90

N20 T10

N30 M06

N40 M03 S600

210

12. Fixed Cycle

12.1.21 Rectangular Groove Cycle (G184)

Description

This cycle is used for the rough and finish machining of rectangular

grooves with rounded corners.

Format

(G98/G99)G184R_Z_K_W_X_Y_I_A_F_ Q_E_O_H_U_P_C_D_V_

Parameter

Description

The coordinate value of the reference point R for

absolute programming, or the distance from reference

point R to the initial plane for incremental

programming.

The coordinate value of the groove bottom for absolute

programming, or the incremental value from the

groove bottom to the reference point R for incremental

programming.

The length of the groove.

The width of the groove.

The center of the groove. The first axis coordinate of

the current plane for absolute programming, and the

incremental value to the start point for incremental

programming.

The center of the groove. The second axis coordinate

of the current plane for absolute programming, and the

incremental value to the start point for incremental

programming.

The arc radius of the rounded corner (It can be left

blank or specified to 0 when I=W/2 ).

212

12. Fixed Cycle

The angle formed by the long side of the rectangle

groove and the first positive axis (It is optional when

A=0.).

Milling speed during rough machining.

The maximum feed depth for each time during rough

machining

(It is optional when Q= groove depth-

finishing allowance of the groove bottom).

The finishing allowance of the groove margin (It is

optional when E=0).

The finishing allowance of the groove bottom (It is

optional when O=0).

The maximum feed rate for finish machining (It is

optional when U=Q ).

The feed rate for finish machining (It is optional when

U=F ).

The spindle speed for finish machining (It is optional

when P= the spindle speed before cycle or the default

spindle speed).

The direction for milling each groove (It is optional

when C=3)

0：milling in the same direction with the spindle

rotation； 1：milling in the reversed direction with the

spindle rotation； 2：milling in G02 direction； 3：

milling in G03 direction

Machining type (It is optional when D=1)

1: rough machining

2: finish machining

The tool radius.

213

HNC-818. User Manual - page 7