HNC-818. User Manual

10. Tool Compensation Functions

Tool movement around the outer

Linear ĺ Linear

corner

(Į<90 degrees)

Workpiece

Programming path

Tool center path

Linear ĺ Circular

Workpiec

Tool center path

Programming path

Circular ĺ Linear

Workpiec

Programming path

Tool center path

122

10. Tool Compensation Functions

Circular ĺ Circular

Program

Workpiece

L C

Tool center path

10.4.3 Tool Movement during Offset Cancelation

In the program block including

Linear ĺ Linear

offset cancelation, tool movement

around the inner corner

(Į180 degrees)

Workpiece

G40

Programming path

Tool center path

Linear ĺ Circular

Workpiece

G40

G42

Programming path

Tool center path

123

10. Tool Compensation Functions

In the program block including

Linear ĺ Linear

offset cancelation, tool movement

around the outer obtuse angle

G40

(90 degrees Į<180 degrees)

Workpiec

G42

Programming path

Tool center path

Intersection point

Circular ĺ Linear

G40

Workpiece

C Intersection point

Programming path

Tool center path

124

10. Tool Compensation Functions

10.5 Tool Length Compensation (M) (G43, G44, G49)

between the tool length specified in programming and the actual tool

length. You may save this difference in the CNC's tool offset register,

and then use the tool length compensation codes to conduct the

compensation for the difference, in order to simplify the operation and

programming. This way, even tools with different length are used for

machining, you may conduct normal machining without modifying the

program if you know the difference between the programmed tool length

and the actual length.

Programmed tool length

Actual tool length

Tool length compensation

Generally, there may be a difference

Attention

The length compensation does not support interruption codes such as

G31.

Abstract

There are three kinds of tool length compensation based on the type of

the axis allowed tool length compensation.

Tool length compensation A

Tool length compensation along Z axis direction

Tool length compensation B

Tool length compensation vertical to the selected plane

Tool length compensation C

Tool length compensation along specified axis direction

126

10. Tool Compensation Functions

Format

Type

Format

Tool length compensation A

G43/G44 Z_H_

Tool length compensation B

G17 G43/G44 Z_H_

G18 G43/G44 Y_H_

G19 G43/G44 X_H_

Tool length compensation C

G43/G44 X_H_

G43/G44 Y_H_

G43/G44 Z_H_

……

Cancel tool length compensation

G49 IP_

Description

Tool length compensation is defined by G43 and G44.

G43: Tool length compensation in the positive direction (plus the tool

length compensation value to the theoretical position in the tool axis

direction)

G44: Tool length compensation in the negative direction (minus the tool

length compensation value to the theoretical position in the tool axis

direction)

G17: Select XY plane

G18: Select ZX plane

G19: Select YZ plane

H: The number of tool length compensation amount in the tool

compensation table

Attention

The direction of tool length compensation is always vertical to the

plane defined by G17/G18/G19.

When the offset number is changed, the new offset value will not be

added to the old offset value. Example:

H1: Tool length compensation amount

20.0; H2: Tool length

compensation amount 30.0

G90 G43 Z100 H01; Z reaches 120

G90 G43 Z100 H02; Z reaches 130

G43, G44, G49 are modal codes which can be canceled by each

other.

The axis movement is invalid if no tool length compensation after

G49.

127

10. Tool Compensation Functions

Example 1

Take into account the tool length compensation, and create a program for

the workpiece as shown in the figure below.

Requirements: establish a workpiece coordinate system and conduct

machining in the direction shown by the arrow in the figure below:

120

Offset value = 4mm

Actual position

○

Programming

position

H1 = -4.0 (tool length compensation value)

%3325

G92 X0 Y0 Z0

G91 G00 X120 Y80 M03 S600

G43 Z-32 H01

G01 Z-21 F300

G04 P2000

G00 Z21

X30 Y-50

129

11. Programming Simplification Functions

11.1 Mirroring Function (M) (G24, G25)

When the workpiece is symmetric around an axis, you may use the

mirroring functions and subprograms to create a program only for one

part of the workpiece, and other symmetrical parts can be produced. This

is called mirroring.

Format

G24 IP_; Create mirror

……

G25 IP0; Cancel mirror

Parameter

Description

The position of the mirror axis.

Attention

you may establish the symmetrical mirror of the ȕ axis by

specifying G24 Į_.

After establishing the mirror of the ȕ axis, you may cancel the

mirror of the ȕ axis by specifying G25 Į0. If you establish a

point-symmetrical mirror by specifying G24 X0Y0, the symmetrical

mirror of the Y axis can be canceled by specifying G25 X0, and

then only the X axis mirror is specified.

The character "Į" represents the first axis in the selected plane

while "ȕ" represents the second axis in the selected plane.

G24 and G25 program blocks are specified in separate lines.

G24 is a modal function. You may use G25 to cancel the mirroring

function after it is ended.

When no axis is after G25, all mirroring functions are canceled.

132

11. Programming Simplification Functions

Mirroring

path 1

Programming path

Description

Mirroring

Mirroring path 3

path 2

The mirroring path 1 and the programming path is axisymmetric,

with the symmetry axis Į=50.

The mirroring path 2 and the programming path is point-symmetric,

with the symmetry point (50, 60).

The mirroring path 3 and the programming path is axisymmetric,

with the symmetry axis ȕ=60.

Axisymmetric mirror

(G17/G18/G19) G24 Į_/ȕ_;

…… ;

G25;

G17/G18/G19: Selects the mirror plane which should contain the

programming tool path.

G24 Į_/ȕ_: Specifies the symmetry axis of the mirror. You can only and

must specify either Į_ or ȕ_. The character "Į" represents the first axis in

the selected plane, and "ȕ" represents the second axis in the selected

plane. If an axis that is not in the selected plane is specified, an alarm

will be reported.

……: Programming command of tool path.

G25Į0/ȕ0: Cancels the mirroring function. Only the command G25 or

the command with G25 followed by the random value of "a" and "b" can

cancel the mirroring function.

Point-symmetric mirror

(G17/G18/G19) G24 Į_ ȕ_;

…… ;

G25;

133

11. Programming Simplification Functions

G17/G18/G19: Selects the mirror plane which should contain the

programming tool path.

G24 Į_ ȕ_: Specifies the symmetry point of the mirror. When Į_ or ȕ_ is

blank, the point is the actual tool position by default. If an axis that is not

in the selected plane is specified, an alarm will be reported.

……: Programming command of tool path.

G25Į0ȕ0: Cancels the mirroring function. Only the command G25 or the

command with G25 followed by the random value of "a" and "b" can

cancel the mirroring function.

Example

Use the mirroring function to create a program for the machining of the

contour as shown in the figure below: The distance from the start point

of the tool to the workpiece surface is 100 mm, and the cutting depth is 5

mm.

-30

-10

-30

%3331 Main program

G92 X0 Y0 Z100

G91 G17 M03 S600

G24 X0; Y axis mirroring, with mirroring position X=0

G24 Y0; X&Y axis mirroring, with mirroring position (0, 0)

G25 X0; X axis mirroring remains valid, and cancel the Y axis mirroring

134

11. Programming Simplification Functions

11.2 Scaling Function (M) (G50, G51)

The scaling function can be used to zoom in or zoom out the

programming path by a given scaling factor.

Uniform scaling

G51 IP_ P_; Start scaling

……

G50; Cancel scaling

Parameter

Description

Specify the center point coordinates for the scaling. If

the center point is not specified, the current point will be

specified by default.

The command always specifies the absolute position of

the scaling center in the workpiece coordinate system.

Specifies the scaling factor for each axis.

All axes are scaled according to the scaling factor.

Tool Compensation

In the case of tool compensation, scaling is conducted before the tool

radius compensation or tool length compensation. The scaling will not

change the tool radius compensation value or tool length compensation

value.

Attention

1. Specify G51 block in a separate line.

2. Use G50 to cancel the scaling after the scaling is completed.

3. In the G51 block, either in the incremental (G91) or absolute mode

(G90), the center coordinates of the scaling IP_ refers to the absolute

position in the workpiece coordinate system.

136

11. Programming Simplification Functions

Example

Use the scaling function to create a program for the machining of the

contour as shown in the figure below: The apexes of the triangle ABC

are A (10, 30), B (90, 30), C (50, 110); the triangle A'B'C 'is the shape

after scaling, with the scaling center D (50, 50)and the scaling factor 0.5;

the distance from the start

point of the tool to the surface

the

workpiece is 50 mm.

C (50, 110)

C’

A’

B (90, 30)

O A (10, 30)

%3332; Main program

G92 X0 Y0 Z60

G17 M03 S600 F300

G43 G00 Z14 H01

X110 Y0

#51=0

M98 P100; Machining for the triangle ABC

#51=6

G51 X50 Y50 P0.5; Scaling center (50, 50), scaling factor 0.5

M98 P100; Machining for the triangle A'B'C'

G50; Cancel the scaling

G49 Z60

G00 X0 Y0

M05 M30

137

11. Programming Simplification Functions

11.3 Rotation Function (M) (G68, G69)

The rotation function can be used to rotate the programming path around

the rotation center with the specified angle. If the workpiece consists of

multiple parts with the same shape, you may create sub programs and

then use the rotation command to call the subprograms.

It can simplify the programming and save storage space.

Format

G17/G18/G19; Select a rotation plane

G68 IP_ P_; Establish rotation

……

G69; Cancel rotation

Parameter

Description

Specifies the rotation center coordinate. If nothing is

specified as the rotation center, the current point of the

tool will be specified by default.

Either in the incremental or absolute mode, the specified

value refers to the absolute position in the workpiece

coordinate system.

Rotation angle (unit: degree)

Rotation angle

The rotation angle P ranges from -360 to 360 degrees, positive in the

counterclockwise direction and negative in the clockwise direction.

Either specified by G90 or G91, P is always the absolute value of the

angle which is based on the positive direction of the first axis in the

specified plane.

Tool compensation

Conduct tool radius compensation, tool length compensation, tool offset,

and other compensation after the coordinate system rotation. If rotation

and scaling are both required, rotation should be programmed prior to the

scaling function; otherwise a message prompting you "SWITCHING

NESTING ORDER ERROR." will be displayed.

Attention

The G code (G28, G29, G30, etc.) related to reference or the

command used for changing the coordinate system (G52, G54-G59,

G54.X, G92, etc.) cannot be specified in the rotation mode. To

specify such commands, please firstly cancel the coordinate rotation

command.

139

11. Programming Simplification Functions

If you Specify G68 and G69 in the tool radius compensation mode,

the rotation plane must be consistent with the tool radius

compensation plane.

Use G69 to cancel the rotation function after it is completed.

Specify the G68 program block in a separate line.

Example

Use the rotation function to create a program for the machining of the

contour as shown in the figure below: the distance from the tool start

point to the workpiece surface is 50 mm, and the cutting depth is 5 mm.

X’

错误

Y’

45°

错误

%3333; Main program

N10 G92 X0 Y0 Z50

N15 G90 G17 M03 S600

N20 G43 Z-5 H02

N30 G68 X0 Y0 P45; Rotate 45 degrees

N60 G68 X0 Y0 P90; Rotate 90 degrees

N20 G49 Z50

N80 G69 M05 M30 ; Cancel rotation

G41 G01 X20 Y-5 D02 F300

N105 Y0

140

11. Programming Simplification Functions

11.4 Direct Programming based on Blueprint Dimensions (T)

Straight angles, chamfering values, corner arc transition values and other

dimensional values on machining blueprint can be directly entered for

programming. In addition, chamfer or transition arc can be inserted

between the straight lines of any dip angle. This program mode is called

direct programming based on blueprint dimensions.

This programming mode is used only for G01 command of turning

series G01.

Command format

The programming mode consists of eight command modes. The meaning

of each character is as below:

X_/Z_: Linear destination address word

A_: The angle between the direction of linear movement and the positive

direction of Z-axis, negative in the clockwise direction and positive in

the counterclockwise direction. Unit: degree.

C_: Chamfer side length.

R_: Rounding radius.

Specify a straight line

(X2, Z2)

X1_Z1_

X2_(Z2_)A_;

(X1, Z1)

Note: You can only specify the amount of displacement in one direction

for the target position. For example: Z50a45 or X100a45.

142

11. Programming Simplification Functions

Specify straight lines continuously

(X3, Z3)

X1_Z1_

A1_;

X3_Z3_A2_;

(X2, Z2)

(X1, Z1)

Rounding

(X3, Z3)

X2_Z2_R1_;

A2 R1

X3_Z3_

A1_R1_;

(X2, Z2)

(X1, Z1)

X3 Z3 A2 ;

Chamfer

X2_Z2_C1_;

(X3, Z3)

X3_Z3

A1_C1_;

X3_Z3_A2_;

(X2, Z2)

(X1, Z1)

143

11. Programming Simplification Functions

Continuous rounding

X2_Z2_R1_;

(X4, Z4)

(X3, Z3)

X3_Z3_R2_;

X4_Z4_

A1_R1_;

(X2, Z2)

X3_Z3_A2_R2;

X4_Z4_;

Continuous chamfer

X2_Z2_C1_;

(X3, Z3)

X3_Z3_C2_;

X4_Z4_

(X4, Z4)

A1_C1_;

(X2, Z2)

X3_Z3_A2_C2;

X4_Z4_;

Rounding and then chamfer

144

11. Programming Simplification Functions

X2_Z2_R1_;

X3_Z3_C2_;

(X3, Z3)

X4_Z4_

(X4, Z4)

A1_R1_;

Chamfer and then rounding

X3_Z3_A2_C2;

(X2, Z2)

X4_Z4_;

X2_Z2_C1_;

X3_Z3_R2_;

(X4, Z4)

(X3, Z3)

X4_Z4_

A1_C1_;

X3_Z3_A2_R2;

(X2, Z2)

X4_Z4_;

Attention

To avoid the conflicts between the address word in this function and the

axis name, make sure to set the channel parameter Parm040035

[ANGLE PROGRAMMING ENABLED] (channel 0) when using this

function.

145

12. Fixed Cycle

12 Fixed Cycle

During CNC machining, some machining cycle has been stylized. Some

typical machining operations such as drilling, boring, milling, turning,

etc., are pre-created via the macro program and are saved in the system.

Call the programs through G codes to simplify the programming. This

chapter includes the following sections:

12.1 Drilling Fixed Cycle for Milling Machines

12.2 Simple Cycle for Turning Machines

12.3 Drilling Fixed Cycle for Turning Machines

12.4 Combined Cycle for Turning Machines

12.5 Exceptions in Fixed Cycle

146

12. Fixed Cycle

12.1 Drilling Fixed Cycle for Milling Machines (M)

Commands of drilling fixed cycle

Drilling (-Z

Action at the

Tool Exist (+Z

for milling machines

Code

Direction)

Hole Bottom

Direction)

G70

Cutting feed

Pause

Rapid tool exit

G71

Cutting feed

Pause

Rapid tool exit

G73

Intermittent

Pause

Rapid tool exit

cutting feed

G74

Cutting feed

Pause—Spinlde

Cutting back

clockwise

roation

G76

Cutting feed

Spindle

Rapid tool exit

orientation

G78

Cutting feed

Pause

Rapid tool exit

G79

Cutting feed

Pause

Rapid tool exit

G81

Cutting feed

—

Rapid tool exit

G82

Cutting feed

Pause

Rapid tool exit

G83

Cutting feed

Pause

Rapid tool exit

G84

Cutting feed

Pause—Spindle

Cutting back

counter

clockwise

roation

G85

Cutting feed

—

Cutting back

G86

Cutting feed

Pause—Spindle

Rapid tool exit

stop

G87

Cutting feed

Spinlde

Rapid tool exit

clockwise

roation

G88

Cutting feed

Pause—Spindle

Manually

stop

G89

Cutting feed

Pause

Cutting back

G80

—

Drilling actions

Generally there are six actions for the drilling cycle in order:

Action 1: X&Y axis positioning

Action 2: Rapidly move to the R plane

Action 3: Execute drilling

147

12. Fixed Cycle

Action 4: Operations at the hole bottom

Action 5: Exit the tool to the R plane

Action 6: Rapidly exit the tool to the initial Z plane

Operation 1

Intital level

Operation 2

Operation 6

R Level

Operation 5

Operation 3

Rapid traverse

Operation 4

Feed

Locate plane

G17 plane (X, Y axis)

Drilling axis

Z axis

Drilling data

G73, G74, G76 and the codes from G81 to G89 are modal G codes,

which are valid before they are canceled. The parameters defined in

these drilling cycle commands are modal data, which indicates that the

parameters are valid before they are canceled.

Return to the reference plane G99

The G99 command can be used to return to the reference point plane

specified by the R parameter after the fixed cycle is ended.

Initial plane

R level

148

12. Fixed Cycle

Return to the start plane G98

The G98 command can be used to return to the start plane where the

fixed cycle is commanded after the fixed cycle is ended. G98 is the

initial modal G code of Group 15.

Initial plane

R level

Cancle the fixed cycle

G80 or the G codes of Group 01 can be used to cancle the fixed cycel.

Symbol description

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

Manual feed

Dwell

Attention

When the fixed cycle program lines without X, Y, Z axis movement

command are executed, the tool will not move, but the cycle

parameter modal value of the current lines will be saved.

Specifying the G code of Group 1 or G80 will cancel the current

fixed cycle G code modal, and also clear the cycle parameter modal

value.

If you need to execute the fixed cycle repeatedly by specifying L,

an alarm will be reported when L is set to 0.

149

12. Fixed Cycle

When the G53 command is specified in a fixed cycle block, its

positioning data (X, Y) is still the original workpiece coordinate

system data, but not the coordinate system data specified by G53.

Example:

Use ĭ10 drilling bit to drill the holes shown in the figure below:

Y—

—750

—550

—250

X+

Z—

1000

300

—150

X+

Program example

%5647

G54

G90 X0 Y0 Z80

M3 S1000;

G90 G99 G81 X300 Y-250 Z-150 R-120 F120; Position, drill hole 1,

return to the point of R

Y-550; Position, drill hole 2, return to the point of R

Y-750; Position, drill hole 3, return to the point of R

X1000; Position, drill hole 4, return to the point of R

Y-550; Position, drill hole 5, return to the point of R

G98 Y-750; Position, drill hole 6, return the initial plane

G80 G28 G91 X0 Y0 Z0; Cancel the fixed cycle and return to the

reference point

M5;

M30

150

12. Fixed Cycle

12.1.1 Circumference Drilling Cycle (G70)

Description

In the circumference with the radius I and the center being the coordinate

(X, Y). Divide the circle into N equal parts based on the angle J and the

X axis. Conduct drilling for N holes. Execute fixed cycle of G81 and

G83 based on the value of Q, K for each hole. The movement between

holes is performed through G00. G70 is a modal code, and the command

word following it is non-modal.

Initial point B

Reference

G98

point R

Reference

point R

G99

Hole bottom

Hole

bottom

Delay at the hole

point Z

bottom for P seconds

Format

(G98 / G99) G70 X_ Y_ Z_ R_ I_ J_ N_[Q_K_P]_ F_ L_

151

HNC-818. User Manual - page 5