Content      ..     6      7      8      9     ..

HNC-818. User Manual - page 8

12. Fixed Cycle

Parameter graph

Y

X

A

I

G

k

w

Y

G3

X

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 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

G02

3: in G03 direction

G03

G03

Left blank

G03

G03

1.

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

groove without any collision.

Operation Procedure

2.

Rough machining (D=1):

Go to the center of the long side of the groove with G00(reserve the

finishing allowance for the groove margin). The tool feeds

downward with the depth specified by Q, and then conducts milling

from the margin to the center for the upper part of the groove in the

milling direction specified by C. Then backing to the same start

position, the tool conducts milling from the groove surface to the

groove bottom (reserve the finishing allowance).

Finish machining (D=2):

Go to the center of the long side of the groove with G00

214

12. Fixed Cycle

Y

Y

A

A - B

R8

B

60

X

Z

17.5

%0526

N10 G54 G90 G17

N20 T20

N30 M06

N40 M04 S600

N50 G00 X60 Y40 Z5

N60 G98G184R5Z-17.5K60W40X60Y40I8F120Q4E0.75O0.2D1V5

N70 M30

216

12. Fixed Cycle

12.1.22 Circular Groove Cycle (G185)

Description

This cycle is used for rough or finish machining for circular grooves.

Format

(G98/G99)G185R_Z_X_Y_I_ 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

R

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

Z

groove bottom to the reference point R for incremental

programming.

The center of the groove. The first axis coordinate of

the current plane for absolute programming, and the

X

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

Y

incremental value to the start point for incremental

programming.

I

The radius of the circular groove.

F

Milling speed during rough machining.

The maximum feed depth for each time during rough

Q

machining

(It is optional when Q= groove depth-

finishing allowance of the groove bottom).

217

12. Fixed Cycle

The finishing allowance of the groove margin (It is optional

E

when E=0).

The finishing allowance of the groove bottom

(It is

O

optional when O=0 ).

The maximum feed rate for finish machining (It is optional

H

when H=Q).

The feed rate for finish machining (It is optional when

U

U=F ).

The spindle speed for finish machining (It is optional when

P

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；

C

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 ).

D

1: rough machining; 2: finish machining

V

Tool radius.

Parameter graph

Y

X

G3

G2

I

Y

X

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 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

M03 spindle CW

0: same direction

G03

G02

1: reversed direction

G02

G03

218

12. Fixed Cycle

12.1.23 Face Milling Cycle (G186)

Description

This cycle can be used to conduct milling for any rectangular end face.

The cycle for rough machining (perform multi-step reaming from surface

to finishing allowance) and finish machining (finish the end face) is

different.

Foramt

(G98/G99)G186R_Z_N_W_X_Y_ I_ A_F_Q_J_O_H_K_U_P_C_D_V_

Parameter

Description

The coordinate value of the reference point R for

absolute programming, or the distance from reference

R

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

Z

groove bottom to the reference point R for incremental

programming.

N

The first axis length of the workpiece.

W

The second axis length of the workpiece.

The start position.

The first axis coordinate of the current plane for

X, Y

absolute programming, or the incremental value to the

current point during incremental programming.

The safety margin in the milling direction (It is

I

optional when I= tool radius).

The angle formed by the long side of the end face and

A

the first positive axis (It is optional when A=0 ).

F

Milling speed during rough machining.

The maximum feed depth for each time during rough

Q

machining (It is optional when Q= groove depth-

finishing allowance of the groove bottom).

The milling width during rough machining (It is

J

optional when J= tool radius x 80%).

The finishing allowance of the workpiece bottom (It is

O

optional when O=0).

The maximum feed depth during finish machining (It

H

is optional when H=Q).

The cutting width during rough machining (It is

K

optional when K= tool radius x 80%).

221

12. Fixed Cycle

The milling speed for finish machining (It is optional when

U

U=F).

The spindle speed for finish machining (It is optional when

P

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；

C

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 and D=1 by default)

D

y

1: rough machining

y

2: finish machining

V

The tool radius.

• C=0, D=1, bidirectional machining along the X axis

Basic description

N

J

W

Q

+Y

+Z

Z-O Q

J

Q

+X

+Y

I

(X,

I

222

12. Fixed Cycle

•

•

• C=1, D=1, bidirectional machining along the Y axis

N

J

J

I

J

W

Q

+Y

+Z Z-O Q

Q

+X

I

+X

(X, Y)

J

• C=2, D=1, unidirectional machining along the X axis

N

J

W

Q

+Y

+Z

Z-O Q

J

Q

+Y

+X

I

(X, Y)

I

• C=3, D=1, unidirectional machining along the Y axis

N

I

J

W

+Y

Q

+Z

Z-O Q

Q

+X

I

(X, Y)

J

+Y

Note: The figures above show the milling cycle (rough machining) only

for the end face of the G17 plane. The cycle for G18/G19 is similar, and

223

12. Fixed Cycle

12.1.24 Rectangular Boss Cycle (G188)

Description

This cycle is used to conduct machining for rectangular boss of arbitrary

size on a plane. The rectangular boss may have rounded corners. You

may select roughing, finishing or comprehensive machining as required.

Format

(G98/G99)G188R_Z_N_W_X_Y_J_K_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

R

point R to the initial plane for incremental

programming.

The coordinate value of the boss bottom for absolute

programming, or the incremental value from the boss

Z

bottom to the reference point R for incremental

programming.

N

The length of the rectangular boss.

W

The width of the rectangular boss.

The center of the rectangular boss. The first axis

coordinate of the current plane for absolute

X

programming, and the incremental value to the start

point for incremental programming.

The center of the rectangular boss. The second axis

coordinate of the current plane for absolute

Y

programming, and the incremental value to the start

point for incremental programming.

J

The length of the rough rectangular boss.

225

12. Fixed Cycle

K

The width of the rough rectangular boss.

The radius of the rounded corner in the rectangular boss (It

I

is optional when I=W/2 ).

The angle formed by the long side of the rectangular boss

A

and the first positive axis (It is optional when A=0).

F

The milling speed for rough machining.

The maximum feed depth for each rough machining (It is

Q

optional when Q = groove depth - finishing allowance at

the groove bottom).

The finishing allowance at the boss margin (It is optional

E

when E=0).

The finishing allowance at the boss bottom (It is optional

O

when O=0).

The maximum feed depth for finish machining (It is

H

optional when H=Q).

The feed speed for finish machining (It is optional when

U

U=F).

The spindle speed for finish machining (It is optional when

P

P= the spindle speed before cycle or the default spindle

speed).

The milling direction for the boss (It is optional when

C=3 ).

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

C

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 and D=1 by default).

D

1: rough machining; 2: finish machining

V

Tool radius.

Parameter graph

Y

X

A

I

N

W

Y

X

226

12. Fixed Cycle

Y

Path for entering

Semicircle path for entering and

existing

X

Path for existing

To ensure the tool smoothly moves into the workpiece, the cycle

automatically adds a semicircle path when entering and exiting the

workpiece. The semicircle radius is determined by the cycle parameters,

and the semicircle direction is opposite to the milling direction. For

example, if the milling direction is specified by G2, then the added

semicircle is in the direction of G3.

Dimension of rough boss

Y

K

J

X

For the machining of workpiece with prior casting, the rough size of

rectangular boss, which is symmetrical to the size of the boss with the

center(X,Y), may be taken into account.

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

commands. See the table below:

Milling Direction

Execute M03/M04 before the cycle

227

12. Fixed Cycle

(Parameter C)

M03 spindle CW

M03 spindle CW

0: same direction

G03

G02

1: reversed direction

G02

G03

2: in G02 direction

G02

G02

3: in G03 direction

G03

G03

Left blank

G03

G03

Operation procedure

1.

Selecting a start point, which must be to the right of the boss in the

first postive axis direction of the plane. You need to consider the

automatically added semicircle during the cycle.

2.

Rough machining (D=1):

Go to the reference plane over the long side of the boss with G00, feed

downward with the specified depth, and then in the milling direction,

enter the workpiece contour through a semicircle path to conduct milling

from the surface to the finishing allowance of the margin, and exit the

workpiece contour through a semicircle path in the opposite direction.

Use G00 to rapidly move to the start point, and then conduct milling

from the groove surface to the finishing allowance of the bottom.

Finish machining (D=2):

Go to the reference plane over the long side of the boss with G00, feed

downward with the specified depth, and then in the milling direction,

enter the workpiece contour through a semicircle path to machine the

finishing allowance of margin. After that, exit the workpiece contour

through a semicircle path in the opposite direction. Use G00 to rapidly

move to the start point, feed downward again to machine the finishing

allowance of the bottom.

3.

After completing the machining, exit the tool to the initial point or

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

then the cycle ends.

Attention

1.

For the information about alarms, see section 12.1.26.

2.

The values of W, J, K, I, O, Q and H should be non-negatives. If the

specified value is a negative value, the system will ignore the

negative symbol.

228

12. Fixed Cycle

3.

For the maximum feed depth

for rough and finish machining

(specified by Q and H

respectively), if the feed rate is

not divisible , the final cut will

4.

Before executing the cycle, use the command to enable the spindle

be less than Q or H.

rotation.

5.

If the specified width is greater than the length, the system will

automatically exchange them and rotate to the expected position.

Example

Conduct milling for the boss as shown in the figure below:

Dimension: 60 mm x 40 mm; rough dimension: 80 mm x 50 mm; tool

radius: 3 mm

Y

Y

A

A - B

R1

10°

B

80

X

Z

17.5

%1019

G17 G54 G90

T10

M06

M03 S650

G98 G188 R2Z-17.5N60W40X80Y60J80K50I15A10F200Q11E2O1V3

M30

229

12. Fixed Cycle

12.1.25 Circular Boss Cycle (G189)

Description

The cycle is used to conduct machining for circular boss with arbitrary

size.

Format

(G98/G99)G189R_Z_X_Y_ I_ J_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

R

point R to the initial plane for incremental

programming.

The coordinate value of the boss bottom for absolute

programming, or the incremental value from the boss

Z

bottom to the reference point R for incremental

programming.

The center of the rectangular boss. The first axis

coordinate of the current plane for absolute

X

programming, and the incremental value to the start

point for incremental programming.

The center of the rectangular boss. The second axis

coordinate of the current plane for absolute

Y

programming, and the incremental value to the start

point for incremental programming.

I

The radius of the circular boss.

J

The radius of the rough circular boss.

F

The milling speed for rough machining.

230

12. Fixed Cycle

The maximum feed depth for each rough machining (It is

Q

optional when Q = groove depth - finishing allowance at

the groove bottom).

The finishing allowance at the boss margin (It is optional

E

when E=0).

The finishing allowance of the boss bottom (It is optional

O

when O=0 ).

The maximum feed depth for finish machining

(It is

H

optional when H=Q).

The feed speed for finish machining (It is optional when

U

U=F ).

The spindle speed for finish machining (It is optional when

P

P= the spindle speed before cycle or the default spindle

speed).

The milling direction for the grooves (It is optional when

C=3 ).

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

C

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)

D

1: rough machining; 2: finish machining

V

Tool radius.

Semicircle path for entering and

Y

existing

Return to the running contour

X

Exit the running contour

Similar as G188, to ensure the tool smoothly moves into the workpiece,

the cycle automatically adds a semicircle path when entering and exiting

the workpiece. The semicircle radius is automatically determined by the

cycle. The direction of the semicircle is opposite to that of milling.

231

12. Fixed Cycle

Dimension of rough boss

Similar as G188, you may set the dimension of the rough boss, with the

center (X, Y).

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

commands. 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

G02

3: in G03 direction

G03

G03

Left blank

G03

G03

1.

Select a start point, which must be to the right of the boss in the first

Operation procedure

postive axis direction of the plane. You need to consider the

automatically added semicircle during the cycle.

2.

Rough machining (D=1):

Go to the reference plane over the long side of the boss with G00, feed

downward with the specified depth, and then in the milling direction,

enter the workpiece contour through a semicircle path to conduct milling

from the surface to the finishing allowance of the margin, and exit the

workpiece contour through a semicircle path in the opposite direction.

Use G00 to rapidly move to the start point, and then conduct milling

from the groove surface to the finishing allowance of the bottom.

Finish machining (D=2):

Go to the reference plane over the long side of the boss with G00, feed

downward with the specified depth, and then in the milling direction,

enter the workpiece contour through a semicircle path to machine the

finishing allowance of margin. After that, exit the workpiece contour

through a semicircle path in the opposite direction. Use G00 to rapidly

move to the start point, feed downward again to machine the finishing

allowance of the bottom.

232

12. Fixed Cycle

3.

After completing the machining, exits the tool to the initial point or

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

then the cycle ends.

1.

For the information about alarms, see section 12.1.26.

Attention

2.

The values of J, K, I, E, O, Q and H should be non-negatives. If the

specified value is a negative value, the system will ignore the

negative symbol.

3.

For the maximum feed depth for rough and finish machining

(specified by Q and H respectively), if the feed rate is not divisible

by them, the final cut will be less than Q or H.

4.

Before executing the cycle, use the command to enable the spindle

rotation.

5.

If the specified width is greater than the length, the system will

automatically exchange them and rotate to the expected position.

Example

Conduct milling for the boss as shown in the figure below:

Rough boss radius: 55 mm; each feed depth: 10 mm; tool radius: 5 mm

Y

Y

A

A - B

60

B

X

Z

20

%1020

G17 G54 G90

T10

M06

M03 S650

G98G189 R2Z-20X60Y70I25J27.5F200Q10E1O1V5

M30

233

12. Fixed Cycle

12.1.26 Alarm Information for Milling Cycle

During fixed cycle, if the system detects an error, an alarm will be

reported, and the current cycle execution will be stopped. After you

modify the program, the system will proceed to run the ongoing cycle.

This section describes the alarms that may be reported during the milling

cycle, and provides alarm analysis and suggestions, based on which you

may modify the program.

Alarm

Alarm Text

Source

Reasons and Suggestions

No.

G181

G182

"MILLING

G183

CYCLE: TOOL

G184

The tool radius V is not specified

800

OFFSET

G185

before executing the cycle.

NUMBER NOT

G186

DEFINED."

G188

G189

G181

This alarm is reported if R is not

G182

specified in the program and the cycle

"MILLING

G183

cannot detect the modal R value. This

CYCLE:

G184

parameter should be specified as it is

801

REFERENCE

G185

required when the groove depth is

PLANE NOT

G186

defined in the incremental value or the

DEFINED."

G188

tool exits to the R plane after the cycle

G189

is completed.

G181

"MILLING

G182

CYCLE:

G183

The groove bottom position must be

POSITION OF

G184

802

specified; otherwise, the groove depth

BOTTOM OF

G185

cannot be defined.

GROOVE NOT

G186

DEFINED."

G188

G189

"MILLING

This alarm is reported when the

CYCLE:

G181

groove number is set to 0. The number

803

NUMBER OF

G182

of grooves should be an integer

GROOVE IS

G183

greater than 0.

SET TO ZERO."

234

12. Fixed Cycle

"MILLING

CYCLE: GROOVE

For the groove with user-defined width,

804

LENGTH

G182

the length should be greater than the

DEFINED

TOO

width; otherwise, this alarm is reported.

SMALL."

G181

G182

G183

This alarm is reported when the tool

"M-CYC: TOOL

G184

radius is greater than the defined groove

805

RADIUS

TOO

G185

length. You may select a milling tool with

MUCH."

G186

relative smaller radius for the milling.

G188

G189

"MILLING

This alarm is reported if the arc center is

CYCLE: CENTER

G181

not specified in the program and no

806

POSITION

OF

G182

related modal position is detected by the

ARC MADE OF

G183

cycle.

GROOVES."

"M-CYC:

AR

G181

If there is no modal arc radius value, the

807

MADE OF GV

G182

radius should be specified in this line;

NOT DEFINED."

G183

otherwise, this alarm is reported.

Because of the angle formed by the tool

radius and the groove, there may be

"M-CYC:

G181

interference

among the machined

INTERFER

808

G182

grooves, which may affect the groove

BTWN

G183

contour shape. The system conducts the

GROOVE"

interference detection before the cycle

and provides prompts for you.

This alarm is reported when the groove

"M-CYC:

GV

G181

number or the angle between grooves is

809

NO.&DEF OF AI

G182

defined improperly, e.g. groove number x

CONFLICTS"

G183

the angle between grooves > 360 degrees.

G181

G182

G183

This alarm is reported when the

"The maximum feed

G184

maximum feed depth for each time (Q) is

810

depth for each time

G185

greater than the groove depth. You may

is over large."

G186

decrease the value of Q.

G188

G189

235

12. Fixed Cycle

G181

G182

G183

This alarm is reported when the spindle

"M-CYC:

G184

does not rotate before the cycle. The

811

ROTATE SPDL

G185

spindle status is detected before the

BEF CYC RUN."

G186

cycle is executed.

G188

G189

G184

"CG OR BOSS

This alarm is reported when the center

G185

812

CP

NOT

of the circular groove or boss is not

G188

DEFINED."

specified.

G189

"M-CYC: CG OR

This alarm is reported when the radius

G185

813

BOSS R NOT

of the circular groove or boss is not

G189

DEFINED."

specified.

G182

"M-CYC:

G183

The reserved finishing allowance for

F.ALOW

OF

G184

814

the margin is too large to complete. You

MARGIN

G185

may decrease the finishing allowance.

MUCH."

G188

G189

G182

G183

"M-CYC:

G184

The reserved finishing allowance for

F.ALOW

OF

815

G185

the bottom is too large to complete. You

BOTTOM

G186

may decrease the finishing allowance.

MUCH."

G188

G189

G182

G183

For finish machining, this alarm is

"M-CYC: MAX

G184

reported if the maximum feed depth for

816

F.DEP

OF

G185

each time (H) is greater than the groove

FINISH MUCH."

G186

depth. You may decrease the value of

G188

H.

G189

236

12. Fixed Cycle

G182

G183

This alarm is reported if the defined

"M-CYC: DIR

G184

milling direction is not supported by

817

MILLING

G185

the system, that is the value specified

ERROR."

G186

for C is not within the allowed range

G188

(0, 1, 2, 3).

G189

G182

G183

This alarm is reported if a milling

"M-CYC: DEF

G184

type not supported by the system is

818

OF MACHING

G185

defined, that is the value specified for

TYPE ERROR."

G186

D is not within the allowed range (1,

G188

2).

G189

For G186, the dimension of the end

face should be specified for the

"M-CYC: W.SIZE

819

G186

workpiece to be machined, e.g.

NOT DEFINED."

length and width; otherwise, this

alarm is reported.

For G186, the start point for the

"M-CYC: ST PT

milling should be specified, generally

820

OF MIL NOT

G186

the lower left corner of the workpiece

DEFINED."

on the machining plane; otherwise,

this alarm is reported.

For G186, the safety margin should

"M-CYC:

be specified for a good milling effect.

821

SAFETY LMT

G186

Its value cannot be lower than the

TOO SMALL."

radius of the milling tool.

"M-CYC: WID

For G186, the milling width for

822

OF RM TOO

G186

rough machining cannot be greater

MUCH."

than the tool diameter.

"M-CYC: WID

For G186, the milling width for finish

823

OF RM TOO

G186

machining cannot be greater than the

MUCH."

tool diameter.

"M-CYC:

WP

For G189 and G188, the workpiece

G188

824

SIZE ON BOSS

dimension should be defined;

G189

NOT DEF."

otherwise, this alarm is reported.

237

12. Fixed Cycle

G181

This alarm is reported if the

"M-CYC:

G182

groove length or width is not

GV/BOSS

826

G183

specified in this line or the related

LEN/WID

G184

modal value of the groove length

NOT DEF."

G188

cannot be detected.

"M-CYC:

For

184 or

188, the rounded

CR

OF

corner can be defined, but the arc

G184

829

REC.GV/B

radius cannot be greater than long

G188

OSS

side / 2; otherwise, this alarm is

MUCH."

reported.

"M-CYC:

For G189 and G188, the rough

WP SIZE

G188

boss dimension should be greater

830

ON

G189

than the contour dimension;

BOSS<MA

otherwise, this alarm is reported.

C SIZE."

G181

The parameter V indicates the

G182

compensation number in the tool

"M-CYC:

G183

compensation table. The value

TOOL RAD

G184

873

entered in the compensation

CANNOT

G185

number is the tool radius. This

BE 0."

G186

value cannot be zero; otherwise,

G188

this alarm is reported.

G189

"The

G182

This alarm is reported when the

finishing

G183

finishing allowances of groove

allowances

G184

wall and groove bottom are not

874

is

not

G185

defined simultaneously or both

defined for

G186

are specified as

0 during finish

the

G188

machining.

finishing."

G189

238

12. Fixed Cycle

12.2 Simple Cycle for Turning Machines (T)

For turning machines, there are five simple cycles. See the table below:

G Code

Functions

G80

Inner (outer) diameter cutting cycle

G81

End-face cutting cycle

G82

Thread cutting cycle

G74

End-face deep-hole drilling cycle

G75

Outer diameter grooving cycle

The cycle is to use a G code program block to complete the machining of

multiple blocks, to simplify the programs.

Attention

1.

The cycle described in this section can only be used for turning

machines.

2.

The commands G83, G87, G84and G88 have no positioning

function. To conduct positioning, you need to execute G01 or G00

outside the fixed cycle.

239

12. Fixed Cycle

12.2.1 Inner (Outer) Diameter Cutting Cycle (G80)

This cycle can be used for inner (outer) diameter cutting of cylindrical

and conical surfaces.

Cylindrical surface cutting

G80 X_/U_ Z_/W_ F_

Parameter

Description

X/U Z/W

The cutting end point C at the workpiece coordinate

system for absolute value programming;

The relative distance from the cutting end point C to

the cycle start point A for the incremental value

programming.

Use U and W to express them in the blueprint and the

direction of path 1 and 2 determine whether it is a

positive or a negative value.

F

Feed speed (indicates to move at the speed specified

by F) (mm/min)

The tool moves along the path AĺBĺCĺDĺA. See the figure below:

+X

z

w

Tool exit point

Cycle start point

D

4R

A

3F

1R

u/2

2F

C

Cutting end point

B

Cutting start

x/2

point

+Z

240

12. Fixed Cycle

G80 X_/U_ Z_/W_ I_ F_

Parameter

Description

X/U Z/W

The cutting end point C at the workpiece coordinate

Conical surface cutting

system for absolute value programming;

The relative distance from the cutting end point C to

the cycle start point A for the incremental value

programming.

Use U and W to express them in the blueprint and

the direction of path 1 and 2 determine whether it is

a positive or a negative value.

I

The radius difference between the cutting start point

B and the end point C. Either in the absolute value

programming or in the incremental value

programming, the sign (+ or -) of the difference

value determines whether the value of I is positive

or negative.

F

Feed speed (indicates to move at the speed specified

by F) (mm/min)

The tool moves along the path AĺBĺCĺDĺA. See the figure below:

+X

z

w

D

4R

A

3F

1R

u/2

C

i

2F

x/2

B

+Z

241

12. Fixed Cycle

Conduct machining for the workpiece as shown in the figure below: use

G80 to conduct rough and finish machining for simple cylindrical parts.

Example 1

ĭ30

ĭ35

50

%3320

N1 T0101

N2 M03 S460

N3 G00 X90Z20

N4 X40 Z3

N5 G80 X31 Z-50 F100

N6 G80 X30 Z-50 F80

N7 G00X90 Z20

N8 M30

Example 2:

Conduct machining for the workpiece as shown in the figure below: use

G80 to conduct rough or finish machining for simple conical parts.

242

12. Fixed Cycle

ĭ30

ĭ26

ĭ35

50

%3321

N1 T0101

N2 G00 X100Z40 M03 S460

N3 G00 X40 Z5

N4 G80 X31 Z-50 I-2.2 F100

N5 G00 X100 Z40

N6 T0202

N7 G00 X40 Z5

N8 G80 X30 Z-50 I-2.2 F80

N9 G00 X100 Z40

N10 M05

N11 M30

243

12. Fixed Cycle

12.2.2 End-face cutting cycle (G81)

This cycle can be used for end face cutting and conical face cutting.

End face cutting

G81 X_/U_ Z_/W_ F_

Parameter

Description

X/U Z/W

The cutting end point C at the workpiece coordinate

system for the absolute value programming; The

relative distance from the cutting end point C to the

cycle start point A for the incremental value

programming. Use U and W to express them in the

blueprint and the direction of path 1 and 2

determines whether it is a positive or a negative

value.

F

Feed speed (inidicates to move at the speed

specified by F) (mm/min)

The tool moves along the path AĺBĺCĺDĺA. See the figure below:

w

+X

Cutting

B

start point

1R

A

Cycle start point

2F

4R

u/2

Cutting

3F

C

end point

D

Tool exit

x/2

+Z

z

point

Conical face cutting

G81 X_/U_ Z_/W_ K_ F_

Parameter

Description

X /U Z/W

The cutting end point C at the workpiece coordinate

system for absolute value programming; The

relative distance from the cutting end point C to the

cycle start point A for the incremental value

programming. Use U and W to express them in the

blueprint and the direction of path

1 and

2

determines whether it is a positive or a negative

244

Content      ..     6      7      8      9     ..