Content      ..     6      7      8      9     ..

HNC8 Series CNC Controller. Programming Manual (V2.4) - page 8

can be omitted when A=0)

Incremental angle (can be omitted when B=360/N; The negative value indicates the milling of

B

grooves in counterclockwise direction, and the positive value indicates the milling of grooves in

clockwise direction)

F

Milling speed in roughing

Max. feed depth in roughing (can be omitted when Q=groove depth-finishing allowance of

Q

groove bottom)

E

Finishing allowance of groove edge (can be omitted when E=0)

O

Finishing allowance of groove bottom (can be omitted when O=0)

U

Feedrate in finishing (can be omitted when U=F)

Spindle speed in finishing (can be omitted when P=spindle speed or default speed before

P

entering cycle)

Milling direction for grooving (can be omitted when C=3)

C

0：milling in the same direction; 1: milling in the reverse direction; 2: milling in G02 direction;

3: milling in G03 direction

D

Machining type (can be omitted when D=1) 1: roughing; 2: finishing

V

Tool radius

Description



Graphical representation

Milling direction

The spindle must be specified to rotate before entering the cycle. A reasonable milling direction

is calculated based on the spindle rotation direction M3/4 and the milling direction set by the user

before entering the cycle. The selection of the milling direction is shown in the following table:

Milling direction (cycle

Specify M03/M04 before entering cycle

280

parameter C)

M03 spindle rotation CW

M04 spindle rotation CCW

milling in the same

G03

G02

direction

milling in the reverse

G02

G03

direction

2：G02 direction

G02

G02

3：G03 direction

G03(1)

G03

省略 Omitted

G03

G03

Steps

(1) When cycle runs, use G00 to reach the reference level R;

(2) Milling the current groove back and forth from inside to outside, the milling steps are similar to

G182;

(3) After finishing machining a groove, the tool retracts to the reference level and moves to the next

groove;

(4) After processing all grooves, retract the tool with G98/G99 to complete the cycle.

Example

Machining three grooves on a circle with a center of (X60, Y60) and a radius of 42mm in the XY

plane. The groove size: width is 15mm, groove length angle is 70 degrees, groove depth is 23mm,

starting angle is 0 degrees, incremental angle is 120 degrees, the finishing allowance on the groove

contour is 0.5mm, and the depth of each feed is 6mm. The same speed and feed rate are used for

finishing and roughing. The finishing is completed in one cut, and the tool radius is 5mm.

281

%0528

N10 G54 G17 G90

N20 T10

N30 M06

N40 M03 S600

N50 G00 X60 Y60 Z5

N60G183R2Z-23N3K70W15X60Y60I42A70B120F100Q6E0.5O0.5V5

N70 M30

282

16.4.4 Rectangular Pocket Milling Cycle (G184)

Function and Purpose



This cycle is used for rough machining and finishing of rectangular pockets with circular corners.

Command Format

(G98/G99)G184R_Z_K_W_X_Y_I_A_F_ Q_E_O_H_U_P_C_D_V_；

Parameter

Meaning

Coordinates of R point in absolute programming; distance from initial level to R point

R

in incremental programming

Coordinate of pocket bottom in absolute programming; incremental value of pocket

Z

bottom relative to reference point R in incremental programming.

K

Pocket length

W

Pocket width

Center of pocket. Coordinate of the first axis in the current plane in absolute

X

programming; incremental value relative to the starting point in incremental

programming.

Center of pocket. Coordinate of the second axis in the current plane in absolute

Y

programming; incremental value relative to the starting point in incremental

programming.

Radius of circular corners of rectangular pocket (can be omitted or specified as 0 when

I

I=W/2)

The angle between the long side of the rectangular groove and the positive direction of

A

the first axis in the plane (can be omitted when A=0)

F

Milling speed in roughing

283

Max. feed depth in roughing (can be omitted when Q=groove depth-finishing allowance

Q

of groove bottom)

E

Finishing allowance of groove edge (can be omitted when E=0)

O

Finishing allowance of groove bottom (can be omitted when O=0)

H

Max. feed depth in finishing (can be omitted when H=Q)

U

Feedrate in finishing (can be omitted when U=F)

Spindle speed in finishing (can be omitted when P=spindle speed or default speed before

P

entering cycle)

Milling direction (can be omitted when C=3)

C

0：milling in the same direction; 1: milling in the reverse direction; 2: milling in G02

direction; 3: milling in G03 direction

D

Machining type (can be omitted when D=1) 1: roughing; 2: finishing

V

Tool radius

Description



Graphical representation

Milling direction

The spindle must be specified to rotate before entering the cycle. A reasonable milling direction

is calculated based on the spindle rotation direction M3/4 and the milling direction set by the user

before entering the cycle. The selection of the milling direction is shown in the following table:

Milling direction

M03/M04 Specify M03/M04 before entering cycle

(cycle parameter C)

M03 spindle rotation CW

M04 spindle rotation CCW

0：milling in the same

G03

G02

direction

1：milling in the

G02

G03

reverse direction

2：G02 direction

G02

G02

3：G03 direction

G03

G03

284

Omitted

G03

G03

Steps

(1) Position to the starting position of the cycle. This point can be any position, but it must be

ensured that the workpiece can be positioned from this point without collision;

Roughing (D=1)

(2) The midpoint of the edge of the wide side (finishing allowance of the pocket edge is left)is

positioned with G00, and the depth is fed with a feed amount Q. The pocket surface is milled from

the outside to the inside in the milling direction defined by C, and the tool returns to the same

cutting point, feed from the groove surface again to the finishing allowance at the bottom of the

groove.

Finishing（D=2）

(3) The midpoint of the edge of the wide side (finishing allowance of the pocket edge is left)is

positioned with G00, and the depth is fed with an amount H. The pocket surface is milled from

the outside to the inside in the milling direction defined by C, and the tool returns to the same

cutting point, feed from the groove surface again to the finishing allowance at the bottom of the

groove.

(4) After machining, move the tool to the initial level or reference level with G98/G99, and the

cycle ends.

Example

Machine a pocket in the G17 plane with a length of 60mm, a width of 40mm, a corner radius of

8mm, and a depth of 17.5mm. The pocket forms a 0 degree angle with X axis. The finishing

allowance of edge is 0.75mm, and the finishing allowance of bottom is 0.2mm. The pocket center

is X60Y40, the feed depth is 4mm, and the tool radius is 5mm. Only rough machining is

performed, as shown below.

%0526

285

16.4.5 Circular Pocket Milling Cycle (G185)

Function and Purpose



This cycle is used for processing circular pocket. Finishing and roughing are supported.

Command Format

(G98/G99)G185R_Z_X_Y_I_ F_ Q_E_O_H_U_P_C_D_V_；

Parameter

Meaning

Coordinates of R point in absolute programming; distance from reference point B to R

R

point in incremental programming

Coordinate value of pocket bottom in absolute programming; incremental value of

Z

pocket bottom relative to reference point R in incremental programming

Center of pocket. Coordinate of the first axis in the current plane in absolute

X

programming; incremental value relative to the starting point in incremental

programming.

Center of pocket. Coordinate of the second axis in the current plane in absolute

Y

programming; incremental value relative to the starting point in incremental

programming.

I

Radius of pocket

F

Milling speed in roughing

Max. feed depth in roughing (can be omitted when Q=pocket depth-finishing allowance

Q

of pocket bottom)

E

Finishing allowance of pocket edge (can be omitted when E=0)

O

Finishing allowance of pocket bottom (can be omitted when O=0)

H

Max. feed depth in finishing (can be omitted when H=Q)

U

Feedrate in finishing (can be omitted when U=F)

P

Spindle speed in finishing (can be omitted when P=spindle speed or default speed before

287

entering cycle)

Milling direction (can be omitted when C=3)

C

0：milling in the same direction; 1: milling in the reverse direction; 2: milling in G02

direction; 3: milling in G03 direction

D

Machining type (can be omitted when D=1) 1: roughing; 2: finishing

V

Tool radius

Description



Graphical representation

Milling direction

The spindle must be specified to rotate before entering the cycle. A reasonable milling direction

is calculated based on the spindle rotation direction M3/4 and the milling direction set by the user

before entering the cycle. The selection of the milling direction is shown in the following table:

Specify M03/M04 before entering cycle

Milling direction (cycle

M03 spindle rotation

M04 spindle rotation

parameter C)

CW

CCW

0： milling in the same direction

G03

G02

1： milling in the reverse

G02

G03

direction

2： G02 direction

G02

G02

3： G03 direction

G03

G03

Omitted

G03

G03

Steps

(1) Selecting a position as the starting position of the cycle, this position can be random, and it must

be possible to reach to workpiece from this position without collision.

(2) Roughing（D=1）

288

16.4.6 End Face Milling Cycle（G186）

Function and Purpose



This cycle can mill any rectangular end face in finishing and roughing.

Command Format

(G98/G99)G186R_Z_N_W_X_Y_ I_ A_F_Q_J_O_H_K_U_P_C_D_V_

Parameter

Meaning

Coordinates of reference point R in absolute programming; distance from initial level B

R

to R point in incremental programming

Coordinate value of bottom in absolute programming; incremental value of bottom

Z

relative to reference point R in incremental programming

N

Length of the first axis of workpiece

W

Length of the second axis of workpiece

Starting position.

X、Y

Coordinate of the first axis in the current plane in absolute programming; incremental

value relative to the current point in incremental programming.

I

Safety margin in milling direction (can be omitted, I=tool radius)

The angle between the long side of the end face and the positive direction of the first axis

A

in the plane (can be omitted, A=0)

F

Milling speed in roughing

Max. feed depth in roughing (can be omitted, Q=milling depth-finishing allowance of

Q

bottom)

J

Milling width in roughing (can be omitted, J=tool diameter×80%)

O

Finishing allowance of workpiece bottom (can be omitted, O=0）

H

Max. feed depth in finishing (can be omitted, H=Q）

K

Cutting width in finishing (can be omitted, K=tool diameter×80%）

U

Milling speed in finishing (can be omitted, U=F)

Spindle speed in finishing (can be omitted, P=spindle speed or default speed before

P

entering cycle)

Milling direction (can be omitted, C=0)

0: Bidirectional machining of 1^st axis in the selected plane

C

1: Bidirectional machining of 2^nd axis in the selected plane

2: Unidirectional machining of 1^st axis in the selected plane

3: Unidirectional machining of 2^nd axis in the selected plane

Machining type (can be omitted, D=1)

D

1: roughing, 2: finishing

V

Tool radius

290

Description



C=0，D=1, bidirectional machining of X axis

C=1，D=1，unidirectional machining of X axis

C=2，D=1，unidirectional machining of X axis

C=3，D=1，unidirectional machining of Y axis

291

(Note 1) The above table only lists end face milling cycle in G17 plane (rough machining), for

G18/G19 plane and so on, finishing and hybrid machining (D=2) are also similar.

Example

For milling a rectangular end face, the end face dimensions and related process parameters are as

follows:

Initial level 10mm; reference level 2mm, only rough machining is allowed, each milling width

10mm, each feed depth 6mm, total milling depth 11mm, milling starting point (100, 100), end face

size 60mm×40mm, the safety margin in milling direction is 5mm. Bidirectional milling of X axis

is allowed, the processing feedrate of surface is 500mm/min, and the milling tool radius is 5mm.

N10

G54 X0 Y0 Z20

N20

G17 G90

N30

T10

N40

M06

N50

M03 S650

N60

G00 X0 Y0 Z20

N70

G99G186 Z-11 R0 N60 W40 X100 Y100 I5 F500 Q6 J10 V5

N80 M30

Note

1) N, W, I, O, Q, J, H, K are designated as non-negative numbers. If a negative number is input, the

negative sign will be ignored in the cycle;

2) For the feed width (J, K) and feed depth (Q, H), when the feed amount cannot be divisible by it,

the last cut will be smaller than the feed width or depth;

3) The spindle must be commanded to rotate before entering the cycle;

4) Please refer to section 16.4.9 for the alarms generated in this cycle.

292

华中 8 型数控系统编程说明书

16.4.7 Rectangular Boss Milling Cycle (G188)

Function and Purpose



Rectangular boss milling cycle is for processing rectangular bosses of any size in the plane. The

rectangle bosses can have corner arcs. User can choose the type of machining, finishing, rough

machining or hybrid machining.

Command Format

(G98/G99)G188R_Z_N_W_X_Y_J_K_I_ A_F_ Q_E_O_H_U_P_C_D_V_；

Parameter

Meaning

Coordinates of R point in absolute programming; distance from reference point R to

R

initial level in incremental programming

Coordinates of boss bottom in absolute programming; distance from boss bottom to

Z

reference point R in incremental programming

N

Length of boss

W

Width of boss

Center of boss. Coordinate of the first axis in the current plane in absolute programming;

X

incremental value relative to the starting point in incremental programming.

Center of boss. Coordinate of the second axis in the current plane in absolute

Y

programming; incremental value relative to the starting point in incremental

programming.

J

Length of boss blank

K

Width of boss blank

I

Radius of corner of boss (can be omitted, I=W/2）

The angle between the long side of the rectangular boss and the positive direction of the

A

first axis in the plane (can be omitted, A=0)

F

Milling speed in roughing

293

华中 8 型数控系统编程说明书

Max. feed depth in roughing (can be omitted, Q=pocket depth-finishing allowance of

Q

boss bottom)

E

Finishing allowance of boss edge (can be omitted when E=0)

O

Finishing allowance of boss bottom (can be omitted when O=0)

H

Max. feed depth in finishing (can be omitted when H=Q)

U

Feedrate in finishing (can be omitted when U=F)

Spindle speed in finishing (can be omitted when P=spindle speed or default speed before

P

entering cycle)

Milling direction (can be omitted when C=3)

C

0：milling in the same direction; 1: milling in the reverse direction; 2: milling in G02

direction; 3: milling in G03 direction

D

Machining type (can be omitted, D=1) 1: roughing; 2: finishing

Description



Graphical representation

Enter contour, exit contour

Return to the contour

Leave the contour

In order to ensure the smoothness when the tool enters the workpiece, the cycle automatically

adds a semicircle path when entering and exiting the workpiece during execution. The radius is

determined by the cycle parameters, and the direction is opposite to the milling direction. If the

294

华中 8 型数控系统编程说明书

G2 direction is specified for milling, then the semicircle inserted here is in the G3 direction.

Size of boss blank

For the processing of pre-poured workpieces, the blank size of the rectangular boss can also be

considered, which is symmetrical to the boss size, and the center point is also (X, Y).

Milling direction

The spindle must be specified to rotate before entering the cycle. A reasonable milling direction

is calculated based on the spindle rotation direction M3/4 and the milling direction set by the user

before entering the cycle. The selection of the milling direction is shown in the following table:

Milling direction (cycle

Specify M03/M04 before entering cycle

parameter C)

M03 spindle rotation CW

M04 spindle rotation CCW

0： milling in the same direction

G03

G02

1： milling in the reverse

G02

G03

direction

2： G02 direction

G02

G02

3： G03 direction

G03

G03

Omitted

G03

G03

295

Steps

(1) Select a position as the starting position of the cycle. This point needs to be positioned on the

right side of the boss in the positive direction of the first axis in the plane. Note that the semicircle

automatically added needs to be taken into account.

(2) Roughing（D=1）

Move to the reference level above the wide side of the boss with G00, feed an amount, mill the

blank surface to the finishing allowance of the edge based on the milling direction, exit the

workpiece contour, rapid traverse to the starting point with G00, and feed to machine the surface

of boss to the finishing allowance of the bottom.

(3) Finishing（D=2）

Move to the reference level above the wide side of the boss with G00, feed an amount, enter the

workpiece contour to mill the finishing allowance of the edge based on the milling direction, exit

the workpiece contour, rapid traverse to the starting point with G00, and then feed to machine the

mill the bottom to the finishing allowance; and mill the finsihing allowance of the bottom.

(4) After the boss is machined, move the tool to the initial level or reference level with G98/G99,

and the cycle is completed.

Example

Machine the rectangular boss as shown in the figure below, the boss size is 60mm×40mm, the

blank size is 80mm×50mm, and the tool radius is 3mm.

%1019

G17 G54 G90

T10

M06

M03 S650

G98 G188 R2Z-17.5N60W40X80Y60J80K50I15A10F200Q11E2O1V3

296

M30

Note

(1) Please refer to section 16.4.9 for the alarms generated in this cycle;

(2) W, J, K, I, E, O, Q, H are designated as non-negative numbers. If a negative number is specified,

the negative sign will be ignored in the cycle;

(3) The maximum feed depth of finishing and roughing is specified with Q and H respectively.

When the feed amount cannot be divisible by it, the last cut will be smaller than Q or H;

(4) The spindle must be commanded to rotate before entering the cycle;

(6) If the specified wide side is greater than the long side, the wide side and the long side will be

automatically exchanged by the cycle, and the corresponding rotation will be performed to meet

the desired boss position.

16.4.8 Round Boss Milling Cycle (G189)

Function and Purpose



This cycle is to machine the round boss of any size in the plane.

Command Format

(G98/G99)G189R_Z_X_Y_ I_ J_F_ Q_E_O_H_U_P_C_D_V_；

Parameter

Meaning

Coordinates of R point in absolute programming; distance from reference point R to

R

initial level in incremental programming

Coordinates of boss bottom in absolute programming; incremental value of boss bottom

Z

relative to reference point R in incremental programming

Center of boss. Coordinate of the first axis in the current plane in absolute programming;

X

incremental value relative to the starting point in incremental programming.

297

Center of boss. Coordinate of the second axis in the current plane in absolute

Y

programming; incremental value relative to the starting point in incremental

programming.

I

Radius of round boss

J

Radius of blank

F

Milling speed in roughing

Q

Max. feed depth in roughing (can be omitted)

E

Finishing allowance of boss edge (can be omitted, E=0)

O

Finishing allowance of boss bottom (can be omitted, O=0)

H

Max. feed depth in finishing (can be omitted, H=Q)

U

Feedrate in finishing (can be omitted, U=F)

Spindle speed in finishing (can be omitted, P=spindle speed or default speed before

P

entering cycle)

Milling direction (can be omitted, C=3)

C

0：milling in the same direction; 1: milling in the reverse direction; 2: milling in G02

direction; 3: milling in G03 direction

D

Machining type (can be omitted, D=1) 1: roughing; 2: finishing

V

Tool radius

Description



Enter contour, exit contour

Return to the contour

Leave the contour

Like the G188 cycle, this cycle also adds a semi-circle every time the tool horizontally enters or exits

the blank workpiece to ensure the smooth transition of the moving from boss edge to the blank, and

the radius of the semi-circle is automatically calculated by the cycle.

Blank size

Like the G188 cycle, this cycle can also set the size of the blank, and the center point is also (X, Y).

Milling direction

The spindle must be specified to rotate before entering the cycle. A reasonable milling direction is

calculated based on the spindle rotation direction M3/4 and the milling direction set by the user

before entering the cycle. The selection of the milling direction is shown in the following table:

298

Milling direction

Specify M03/M04 before entering cycle

(cycle parameter C)

M03 spindle rotation CW

M04 spindle rotation CCW

0： milling in the

G03

G02

same direction

1： milling in the

G02

G03

reverse direction

2： G02 direction

G02

G02

3： G03 direction

G03

G03

Omitted

G03

G03

Steps

(1) Select a position as the starting position of the cycle. This point needs to be positioned on the

right side of the boss in the positive direction of the first axis in the plane. Note that the semicircle

automatically added by the cycle needs to be taken into account.

(2) Roughing（D=1）

Move to the reference level above the wide side of the boss with G00, feed an amount, mill the blank

surface to the finishing allowance of the edge based on the milling direction, exit the workpiece

contour, rapid traverse to the starting point with G00, and feed to machine the surface of boss to the

finishing allowance of the bottom.

(3) Finishing（D=2）

Move to the reference level above the wide side of the boss with G00, feed an amount, enter the

workpiece contour to mill the finishing allowance of the edge based on the milling direction, exit the

workpiece contour, rapid traverse to the starting point with G00, and then feed to machine the mill

the bottom to the finishing allowance; and mill the finsihing allowance of the bottom.

(4) After the boss is machined, move the tool to the initial level or reference level with G98/G99, and

the cycle is completed.

Example

Machine the round boss as shown in the figure below, the blank radius is 55mm, the feed depth for

each cut is 10mm, and the tool radius is 5mm.

299

%1020

G17 G54 G90

T10

M06

M03 S650

G98G189 R2Z-20X60Y70I25J27.5F200Q10E1O1V5

M30

Note

(1) Please refer to section 16.4.9 for the alarms generated in this cycle.

(2) J, K, I, E, O, Q, H are designated as non-negative numbers. If a negative number is specified, the

negative sign will be ignored in the cycle.

(3) The maximum feed depth for roughing and finishing is specified with Q and H respectively, when

the feed amount cannot be divisible by it, the last cut will be smaller than Q or H;

(4) The spindle must be commanded to rotate before entering the cycle;

300

16.4.9 Milling Cycle Alarm Diagnosis

Function and Purpose



When the milling canned cycle is executed, if the system recognizes an error, an alarm will be

generated and the execution of the current cycle will be interrupted. It will continue after modified

by user.

This section lists the possible alarms that the system may generate during the execution of the

milling cycle, and analyzes the cause of the alarms. User can modify the program based on that

before continuing to execute the cycle.

Description



Alarm No.

Message

Source

Cause and comments

G181

G182

G183

G184

No tool radius V is specified before

800

No tool radius defined

G185

entering cycle.

G186

G188

G189

If R is not specified in this block, and

G181

the R modal value cannot be detected

G182

by the cycle, this alarm will be

G183

generated.

No reference level

G184

801

This parameter is required to specify

defined

G185

the groove depth in increments or

G186

when returning to the R level at the

G188

end of the cycle, so this parameter

G189

should be defined.

G181

G182

G183

The position of groove bottom needs

No groove

bottom

G184

to be defined, otherwise the groove

802

position defined

G185

depth cannot be determined in the

G186

cycle.

G188

G189

G181

If the number of grooves is specified

Number of grooves

803

G182

as 0, an alarm will be generated. The

defined as zero

G183

number of grooves should be specified

301

as an integer larger than 0.

The groove length must be greater

Groove lenth defined too

804

G182

than the groove width, otherwise this

small

alarm will be generated.

G181

G182

If the diameter of the milling cutter

G183

exceeds the groove length defined by

G184

805

Tool radius too large

the cycle, this alarm will be generated.

G185

User can use a milling cutter with a

G186

smaller radius to complete the milling.

G188

G189

If the arc center position is not

G181

No center position

explained in the block, and the cycle

806

G182

defined

fails to detect the modal position, this

G183

alarm will be generated.

If there is no arc radius modal value,

G181

the radius value must be specified in

807

No radius defined

G182

this row, otherwise this alarm will be

G183

generated.

Considering the angle between the

milling cutter radius and

the

grooves, there may be interference

G181

Interference

between

between the machined grooves, which

808

G182

grooves

will affect the contour shape of the

G183

groove. The interference check will be

performed before the cycle, and user

will be prompted in time.

。Due to the improper definition of the

number of grooves and the angle

Number of grooves

G181

between grooves, this alarm will be

809

conflicts

with angle

G182

generated if the number of grooves

increment defined

G183

×angle between grooves>

360

degrees.

G181

G182

G183

The alarm is generated when the

Max. feed depth defined

G184

maximum feed depth Q is greater than

810

too large

G185

the groove depth. If this alarm occurs,

G186

reduce Q.

G188

G189

811

Please command spindle

G181

Before the cycle is executed, the

302

to rotate before entering

G182

current spindle status is detected. This

cycle

G183

alarm will be generated if the spindle

G184

is not rotating.

G185

G186

G188

G189

G184

Center

position

not

If the position of circular pocket center

G185

812

defined

for

circular

or boss center is not defined, this

G188

pocket or boss

alarm will be generated.

G189

Radius position not

If the radius of round pocket or boss is

G185

813

defined

for

circular

not defined, this alarm will be

G189

pocket or boss

generated.

G182

G183

The reserved edge finishing allowance

Finishing allowance of

G184

814

is too large to complete the machining.

edge too large

G185

Please reduce the allowance.

G188

G189

G182

G183

The reserved finishing allowance of

G184

Finishing allowance of

edge is too large to complete the

815

G185

bottom too large

machining. Please reduce the

G186

allowance.

G188

G189

G182

G183

Max.feed

depth

in

G184

When the maximum feed depth H is

816

finishing defined too

G185

larger than the groove depth, this

large

G186

alarm is generated, then reduce H.

G188

G189

For G186, the end face size of the

workpiece to be processed must be

Size of workpiece to be

819

G186

specified, such as the length and the

machined not defined

width, otherwise this alarm will be

issued.

It is necessary to specify the starting

No milling starting

point of milling for face milling cycle

820

G186

position defined

G186, which is generally the lower

left corner of the workpiece in

303

machining plane. If it is not specified,

this alarm will be generated.

A safety margin must be specified for

Safety margin defined too

the face milling cycle for a good

821

G186

small

milling effect, and this value is not less

than the milling tool radius.

The milling width is not larger than

Milling width defined too

822

G186

tool diameter in roughing for face

large in roughing

milling cycle G186.

The milling width is not larger than

Milling width defined too

823

G186

tool diameter in finishing for face

large in finishing

milling cycle G186.

For round boss G189 or rectangular

No blank size defined for

G188

boss G188, the blank size needs to be

824

boss

G189

defined, otherwise this alarm will be

generated.

G181

If the groove length or width is not

G182

specified in this block, and the modal

No length or width

826

G183

value of the groove length is not

defined for pocket or boss

G184

detected by the cycle, this alarm will

G188

be generated.

The circular corner can be defined for

Corner radius defined too

the rectangular groove or rectangular

G184

829

large for rectangular

boss cycle, but it cannot be greater

G188

pocket and boss

than the half of the wide side,

otherwise this alarm will be generated.

For round boss G189 or rectangular

Blank

size

defined

G188

boss G188, the blank size must be

830

smaller than machining

G189

larger than the contour size, otherwise

size

this alarm will be generated.

G181

G182

V represents the compensation

G183

number in the tool compensation

Tool radius cannot be

G184

table. The value filled in the

873

zero

G185

compensation number is the tool

G186

radius. This value cannot be zero,

G188

otherwise this alarm will be generated.

G189

G182

During finishing machining, the

G183

finishing allowance of groove wall

No finishing allowance

874

G184

and the finishing allowance of groove

defined

G185

bottom cannot be unspecified or

G186

specified as

0 at the same time,

304

G188

otherwise this alarm will be generated.

G189

G182

G183

C sets a value other than 0, 1, 2, and 3.

G184

Milling

direction

If a milling direction not supported by

817

G185

definition error

the system is defined, this alarm will

G186

be issued.

G188

G189

G182

G183

D sets a value other than 1 and 2. If a

G184

Machining

type

milling direction not supported by the

818

G185

definition error

system is defined, this alarm will be

G186

issued.

G188

G189

305

Function and Purpose



This cycle includes the inner (outer) diameter roughing multiple repetitive cycle with pocket and

without pocket.

This command executes rough machining as shown in the figure below, and the tool returns to

the starting point of the cycle. The finishing path A→A'→B'→B is executed sequentially based

on the following commands.

1. Path of inner/outer diameter roughing multiple repetitive cycle without pocket

2. Path of inner/outer diameter roughing multiple repetitive cycle with pocket

Command Format

1. Inner/outer diameter roughing multiple repetitive cycle without pocket

G71 U(d) R(r) P(ns) Q(nf) X(x) Z(z) F(f) S(s) T(t)

307

Parameter

Meaning

U

Cutting depth, without sign. The direction is determined by vector

AA′

R

Retraction amount

P

Sequence number of the first program block (AA' in the below

figure) for finishing path

Q

Sequence number of the last program block (BB' in the below

figure) for finishing path

X

Finishing allowance in X direction

Z

Finishing allowance in Z direction

FS T

F, S, T in G71 are valid in roughing, and F, S, T between block ns

and nf are valid in finishing

2. Inner/outer diameter roughing multiple repetitive cycle with pocket

G71 U(d) R(r) P(ns) Q(nf) E(e) F(f) S(s) T(t)

Parameter

Meaning

U

Cutting depth, without sign. The direction is determined by vector AA′

R

Retraction amount

P

Sequence number of the first program block (AA' in the below figure) for

finishing path

Q

Sequence number of the last program block (BB' in the below figure) for

finishing path

E

Finishing allowancewhich is the equal height distance in the X direction;

positive for outer diameter cutting, and negative for inner diameter

cutting

F S T

F, S, T in G71 are valid in roughing, and F, S, T between block ns and nf

are valid in finishing

Description



In the G71 cutting cycle, the cutting feed direction is parallel to the Z axis, so it is suitable for the

inner and outer diameter cutting along the axial direction.

This cycle is a rough machining cycle. It is necessary to reserve an appropriate allowance for

subsequent finishing. The finishing allowance in the X\Z axis direction is X(x) and Z(z), x

is the allowance on X, z is the allowance on Z.

Since the direction of the allowance is determined by the programmer based on the processing

technology, the system determines the direction of the feed according to the direction of the

finishing allowance set by the program. The direction of the finishing allowance (positive and

negative settings) must be correct, otherwise it will cause an error in the feed direction of the tool.

308

The relationship between the sign of the finishing allowance and the feed direction is shown in

the figure below. (+) means that the contour allowance is kept in the positive direction of the axis,

and (-) means that the contour allowance is kept in the negative direction of the axis.

Machine tool with rear tool post

Machine tool with front tool post

Example

Example 1: Use the outer diameter roughing multiple repetitive cycle to compile the machining

program of the part shown in the figure below: the starting point of the cycle is required to be A

(46, 3), and the cutting depth is 1.5mm (radius), the retraction amount is 1mm, the finishing

allowance in the X direction is 0.4mm, and the finishing allowance in the Z direction is 0.1mm.

The dotted line is the workpiece blank.

%3325

T0101; Set coordinate system, select No.1 tool

N1 G00 X80 Z80; Move to starting point of program

N2 M03 S400; Spindle rotates CW at 400r/min

309

N3 G01 X46 Z3 F100; Move to starting point of cycle

N4 G71U1.5R1P5Q14X0.4 Z0.1; Rough cut：1.5mm Finish cut：X0.4mm Z0.1mm

N5 G00 X0; Finishing contour starts, move to extension line of chamfer

N6 G01 X10 Z-2 ; Finishing 2×45°chamfer

N7 Z-20; Finishing Φ10 outer circle

N8 G02 U10 W-5 R5; Finishing R5 arc

N9 G01 W-10; Finishing Φ20 outer circle

N10 G03 U14 W-7 R7; Finishing R7 arc

N11 G01 Z-52; Finishing Φ34 outer circle

N12 U10 W-10; Finishing outer cone

N13 W-20; Finishing Φ44 outer circle

N14 U1; Finishing contour end

N15 X50; Exit the machined surface

N16G00 X80 Z80; Return to tool setting point

N17 M05; Spindle stop

N18 M30; Main program end and reset

Example 2: Use the inner diameter roughing multiple repetitive cycle to compile the processing

program of the part shown in the figure below: the starting point of the cycle is required to be A

(6, 5), and the cutting depth is 1.5mm (radius). The retraction amount is 1mm, the finishing

allowance in the X direction is 0.4mm, and the finishing allowance in the Z direction is 0.1mm.

The dotted line is the workpiece blank.

%3326

N1 T0101; Select No. 1 tool, and determine the coordinate system

N2 G00 X80 Z80; Move to starting point of program or the tool change position

N3 M03 S400; Spindle rotates CW at 400r/min

N4 X6 Z5; Move to starting point of cycle

310

G71U1R1P8Q16X-0.4Z0.1 F100; Machining in inner diameter roughing cycle

N5 G00 X80 Z80; After rough cutting, move to tool change position

N6 T0202; Change to No.2 tool, and determine the coordinate system

N7 G00 G41X6 Z5; Tool nose radius compensation is added to No. 2 tool

N8 G00 X44; Finishing contour starts, move to Φ44 outer circle

N9 G01 Z-20 F80; Finishing Φ44 outer circle

N10 U-10 W-10; Finishing outer cone

N11 W-10; Finishing Φ34 outer circle

N12 G03 U-14 W-7 R7; Finishing R7 arc

N13 G01 W-10; Finishing Φ20 outer circle

N14 G02 U-10 W-5 R5; Finishing R5 arc

N15 G01 Z-80; Finishing Φ10 outer circle

N16 U-4 W-2; Finishing chamfer 2×45°, finishing contour end

N17 G40 X4; Exit machined surface, cancel tool radius compensation

N18 G00 Z80; Exit inner hole of workpiece

N19 X80; Return to starting point of program or tool change position

N20 M30; Spindle stop, main program end and reset

Example 3: Use the outer diameter roughing multiple repetitive cycle with pocket to compile the

processing program of the part shown in the figure below, where the dashed line is the workpiece

blank.

%3327

N1 T0101; Change to No.1 tool, and determine the coordinate system

N2 G00 X80 Z100 ; Move to starting point of program or tool change position

M03 S400; Spindle rotates CW at 400r/min

N3 G00 X42 Z3; Move to the starting point of cycle

311

by "XZ"; if there is a groove on the processed contour path in the X direction, the machining

allowance at this time is represented by "E".

(8) In principle when machining the outer circle, the cycle starting point must be established

higher than the highest point of the contour; when machining the inner hole, it must be lower than

the lowest point of the contour. (The starting point of the cycle can be controlled to be 0 to 1mm

lower than or higher than the highest point of the contour through the machine user parameter

010161)

(9) 10 pockets are supported at maximum for the machining of contour with pocket.

(10) G71 cannot be in the same line as M code

(11) In the any line with scanning mode, the block between ns and nf cannot be specified.

17.2

End Face Roughing Multiple Repetitive Cycle (G72)

Function and Purpose



This cycle is similar as G71.

The G72 turning is shown in the figure below, where the finishing path is A→A'→B'→B

Command Format

G72W(△d) R(r) P(ns) Q(nf) X(△x) Z(△z) F(f) S(s) T(t)；

Parameter

Meaning

W

Cutting depth, without sign. The direction is determined by vector

AA′

R

Retraction amount

P

Sequence number of the first program block (AA' in the below

figure) for finishing path

313

Q

Sequence number of the last program block (BB' in the below

figure) for finishing path

X

Finishing allowance in X direction

Z

Finishing allowance in Z direction

F ST

F, S, T in G72 are valid in roughing, and F, S, T between blocks ns

and nf are valid in finishing

Description



In the G72 cutting cycle, the cutting feed direction is parallel to the X axis, so it is suitable for

face cutting along the X axis.

This cycle is a rough machining cycle. It is necessary to reserve an appropriate allowance for

subsequent finishing. The finishing allowance in the X\Z axis direction is X(x) and Z(z), x

is the allowance on X, z is the allowance on Z.

Since the direction of the allowance is determined by the programmer based on the processing

technology, the system determines the direction of the feed according to the direction of the

finishing allowance set by the program. Therefore, the direction of the finishing allowance

(positive and negative settings) must be correct, otherwise it will cause an error in the feed

direction of the tool.

The relationship between the sign of the finishing allowance and the feed direction is shown in

the figure below. (+) means that the contour allowance is kept in the positive direction of the axis,

and (-) means that the contour allowance is kept in the negative direction of the axis.

Machine tool with rear tool post

Machine tool with front tool post

314

华中 8 型数控系统编程说明书

Example

Example 1: Compile the machining program of the part as shown in the figure below: The starting

point of the cycle is required to be A (80, 1), and the cutting depth is 1.2mm. The retraction amount

is 1mm, the finishing allowance in the X direction is 0.2mm, and the finishing allowance in the Z

direction is 0.5mm. The dotted line is the workpiece blank.

%3328

N1 T0101; Change to No. 1 tool, and determine the coordinate system

N2 G00 X80 Z80; Move to starting position of program

N3 M03 S400; Spindle rotates CW at 400r/min

N4 X80 Z1; Move to starting point of cycle

N5 G72W1.2R1P8Q17X0.2Z0.5F100 ; Machining in face roughing cycle

N6 G00 X100 Z80; Move to tool change position after roughing

N7 G42 X80 Z1; Tool nose radius compensation is added

N8 G00 Z-53; The finishing contour starts, and move to extension line of chamfer

N9 G01 X54 Z-40 F80; Cone finishing

N10 Z-30; Φ54 outer circle finishing

N11 G02 U-8 W4 R4; R4 arc finishing

N12 G01 X30; Z26 face finishing

N13 Z-15; Φ30 outer circle finishing

N14 U-16; Z15 face finishing

N15 G03 U-4 W2 R2; R2 arc finishing

N16 G01 Z-2; Φ10 outer circle finishing

N17 U-6 W3;

2×45°chamfer finishing, contour finishing end

N18 G00 X50; Exit machined surface

N19 G40 X100 Z80; Cancel radius compensation, return to starting position of

program

N20 M30; Spindle stop, main program end and reset

315

华中 8 型数控系统编程说明书

Example 2: Compile the machining program of the part as shown in the figure below: The starting

point of the cycle is required to be A (6, 3) and the cutting depth is 1.2mm. The retraction amount

is 1mm, the finishing allowance in the X direction is 0.2mm, and the finishing allowance in the Z

direction is 0.5mm. The dotted line is the workpiece blank

%3329

N1 T0101; Set coordinate system

N2 G00 X100 Z80; Move to starting point

N3 M03 S400; Spindle rotates CW at 400r/min

N4 G00 X6 Z3; Move to starting point of cycle

N5 G72W1.2R1P6Q16X-0.2Z0.5F100; Machining in face roughing cycle

N6 G00 Z-61; Contour finishing starts, move to extension line of chamfer

N7 G01 U6 W3 F80;

2×45°chamfer finishing

N8 W10; Φ10 outer circle finishing

N9 G03 U4 W2 R2; R2 arc finishing

N10 G01 X30 ; Z45 face finishing

N11 Z-34; Φ30 outer circle finishing

N12 X46 ; Z34 face finishing

N13 G02 U8 W4 R4; R4 arc finishing

N14 G01 Z-20; Φ54 outer circle finishing

N15 U20 W10; Cone finishing

N16 Z3; Φ74 outer circle finishing, contour finishing end

N17 G00 X100 Z80; Return to tool setting position

N18 M30; Spindle stop, main program end and reset

316

Function and Purpose



This cycle function is suitable for the machining of blanks with rough outlines, such as forging

and casting parts. When processing this kind of blank parts, this function can effectively achieve

a relatively balanced margin.

Command Format

G73 U(I) W(K) R(r) P(ns) Q(nf) X(△x) Z(△z) F(f) S(s) T(t)；

Parameter

Meaning

W

Cutting depth, without sign. The direction is determined by vector

AA′

R

Retraction amount

P

Sequence number of the first program block (AA' in the below

figure) for finishing path

Q

Sequence number of the last program block (BB' in the below

figure) for finishing path

X

Finishing allowance in X direction

Z

Finishing allowance in Z direction

F ST

F, S, T in G72 are valid in roughing, and F, S, T between block ns

and nf are valid in finishing

Description



When this function is cutting the workpiece, the tool path is shown in the figure below. The tool

gradually feeds to make the path gradually close to the final shape of the part, and finally cut into

the shape of the workpiece. The finishing path is A→A'→ B'→B.

318

_{I： Roughing allowance in X axis direction}

_{k： Roughing allowance in Z axis direction}

r： Number of rough cuts

ns： Sequence number of the first program block (AA' in the below figure) for finishing path

nf： Sequence number of the last program block (BB' in the below figure) for finishing path

Δx： Finishing allowance in X axis direction

Δz： Finishing allowance in Z axis direction

f，s，t：F, S, T in G73 are valid in roughing, and F, S, T between block ns and nf are valid in

finishing

Note

ΔI and ΔK represent the total cutting amount during roughing, the number of roughing is r, the

cutting amount in X and Z direction is ΔI/r and ΔK/r;

The cycle machining is realized based on the P and Q values in G73 block. Note the signs of △

x and △z, △I and △K.

Example

Example 1: Set the starting point of cutting at A (60, 5); the rough machining allowances in the X

and Z directions are 3mm and 0.9mm respectively; the number of rough machining is 3; the

finishing allowances in the X and Z directions are 0.6mm and 0.1mm respectively. The dotted

line part is the workpiece blank.

319

Content      ..     6      7      8      9     ..