HNC-818. User Manual

5. Interpolation Functions

5.8 GOTO Function (G31)

G31 is followed by axes, the motion path of which is similar to the G01

linear interpolation. When G31 command is executed, if an external

GOTO signal is input, the execution will be interrupted and the system

proceeds to execute the next block instead.

You may use the GOTO function if the processing end point is not

specified in the program, but specified with the signal from the machine,

e.g. grinding. The GOTO function can also be used to measure the

dimension of the workpiece.

Format

G31 L_IP_; The number behind L indicates the trigger point number,

which must be the same as that in PLC.

G31: non-modal G-code

Description

The coordinate values when the GOTO signal is connected can be used

in user macro-program because they are stored in the axis macro

variables of user macro programs. The axis macro variables start from

60000, and each axis uses 100 macro variables. For example, if the X

axis number is 0, the X-axis variables start from 60000 to 60099; if the Y

axis number is 1, the Y-axis macro variables starts from 60100 to 60199;

similarly, the Z axis macro variables start from 60200 to 60299. Macro

variables related to measurement are defined as follows:

#60010-60011: The command position of the axis 0 on the machine

when receiving measurement signals

#60012-60013: The real position of the axis 0 on the machine when

receiving measurement signals

#60014-60015: The position of the No.2 encoder on the axis 0 when

receiving measurement signals

#60016: The speed on the axis 0 when receiving measurement signals

#60017: The current of the axis 0 when receiving measurement signals

Example

If there is a X7.6 signal, then go to the next block.

5. Interpolation Functions

X7.6

ESC

BLK

The program block after G31 is incremental command.

G31L1G91X100.0F100;

Y50.0;

Input GOTO signal here

50.0

100.0

Actual motion

Without GOTO signal

The program block after G31 is absolute command to one axis.

G31L1G90X200.0F100;

Y100.0;

Y100.0

Input GOTO signal here

X200.0

Actual motion

Without GOTO signal

The program block after G31 is absolute command to two axes,

6. Feed Functions

6.1 Rapid Feed (G00)

In the G00 mode, the tool moves at the rapid feed speed to the specified

position.

Format

G00 IP_

Parameter

Description

In the absolute value mode (G90): the coordinate value

of the end point in the workpiece coordinate system.

In the incremental value mode

(G91): the relative

movement amount of the end point away from the start

point.

Description

The rapid motion speed of each axis in the G00 command is defined by

the axis parameter Rapid Traverse Feed Rate (100034 axis 0). You

cannot specify it with the F command.

G00 is generally used for quick positioning before processing or fast tool

retreat after machining. In the positioning mode initiated by G00, the

tool speeds up to the specified speed from the start point of the block and

slows down when close to the target position. After reaching the end

point, the CNC system will execute the next block.

The rapid traverse speed can be adjusted with the override ratio

button on the control plane.

G00 is modal code, of which functions can be canceled by G01, G02, or

G03.

6. Feed Functions

6.2 Unidirectional Positioning (G60)

Positioning direction

Offset

Start point

End point

Format

G60 IP_

Parameter

Description

In the absolute value mode (G90): the end point position

in unidirectional positioning.

In the incremental value mode (G90): the distance from

the current position to the end point.

Description

In order to eliminate the influence of backlash, you may control the axis

to conduct positioning in one direction.

As shown in the figure, conduct positioning in a common mode when the

motion direction is the same as the positioning direction; when the

motion direction is different from the positioning direction, move the

tool in the motion direction, then move one offset in the positioning

direction. Then the tool reaches the end point.

Offset Value

When running G60, you also need to specify the offset value and the

offset direction. The positive and negative values of the following

parameters indicate the offset directions of G60.

Axis

Parameter Index

Description

1^st axis

Parm100030

G60 offset vector of the first axis.

G60 offset vector of the second

2^nd axis

Parm101030

axis.

3^rd axis

Parm102030

G60 offset vector of the third axis.

6. Feed Functions

Attention

Conduct unidirectional positioning even if the tool movement is

zero.

The specified overshoot in unidirectional orientation must be

greater than the backlash of the corresponding shaft; otherwise you

cannot completely eliminate the backlash during unidirectional

orientation.

Example

(Set 100030 to 10, G60 end point - parameter value of 10X030 = G60

center point)

%0008

G54

G00X20

G60X0; move to X-10, and then move to 0

M30

6. Feed Functions

6.3

Define Feed Speed Unit (G93, G94, G95)

During workpiece machining, the feed speed of linear interpolation (G01)

and circular interpolation (G02, G03) are defined by the value after F.

The feed speed unit is defined by G93, G94, and G95.

M: three commands

y Feed per minute (G94)

After F, specify the tool feed per minute.

y Feed per revolution (G95)

After F, specify the tool feed per revolution around the spindle.

y Inverse-time feed (G93)

After F, specify FRN

T: two commands

y Feed per minute (G94)

After F, specify the tool feed per minute.

y Feed per revolution (G95)

After F, specify the tool feed per revolution around the spindle.

Format

G93; Specify FRN feed

G94; Specify feed per minute

G95; Specify feed per revolution

G94

Feed per minute

In the G94 mode (feed per minute), F specifies the tool movement

amount per minute. Unit: mm/min (G21) or in/min (G20)

G95

6. Feed Functions

Feed per revolution

G95 specifies the tool movement amount per revolution around the

spindle as the feed rate F. Unit: mm/r (G21) or in/r (G20)

Only when the spindle is configured with an encoder, can G95 be

specified.

G93

FRN feed

FRN feed is achieved by specifying the time which is taken to execute

the current program block.

Attention

G93, G94, and G95 are modal functions, which can be canceled by

each other. G94 is the default modal.

In the FRN feed mode, if the calculated speed exceeds the

maximum cutting speed, the actual speed is limited to the maximum

cutting feed speed.

G93 must be programmed in a separate line.

Example

%0008

G54X0Y0Z0; the F value in each mode below is 1000.

G94

G01X50F1000

M3S500

G95

G01Y50F2

G93

G01Z50F20; movement distance x F = final feed speed

M30

6. Feed Functions

6.4 Exact Stop Verification (G09)

Control the tool stop exactly at the end point of the program block.

Format

G09; specified in a separate line

Description

Stop exactly at the end point of the program block including G09 before

proceeding to execute another program block. The function is used for

machining sharp corners.

G09 is non-modal command, which is valid only in the defined program

block.

The difference between G09 and G61 is that G09 is valid in program

blocks but G61 is valid in the modal mode.

6. Feed Functions

6.5 Cutting Mode (G61/G64)

The cutting mode is used to control feed speed.

Position verification

Tool path in the exact stop mode

Tool path in the cutting or tapping

mode

Description

G61: exact stop mode

In each block after G61, the programmed axis must exactly stop at

the end point of the block, and then proceed to the next block.

G64: continuous cutting mode

In each block after G64, the programmed axis executes the next

block right after it begins to slow down

(not reaching the

programmed end point). However, in the block including position

commands (G00, G60) or exact stop verification command (G09),

or in the block excluding motion command, the position verification

will be executed only when the feed speed slows down to zero.

Attention

1. The programming contour of G61 is consistent with the actual

contour.

2. The difference between G61 and G09 is that G61 is modal

command.

3. The programming contour of G64 is inconsistent with the actual

contour. Its difference depends on the value of F and the angle

between the two paths. The greater the value of F is, the greater the

difference is.

4. G61 and G64 are modal commands, which can be canceled by each

6. Feed Functions

other.

5. After running small line programs and changing from the automatic

mode to the single block mode, the G64 command will execute the

splines in the look-ahead buffer, and then execute program blocks in

single block mode; therefore, a number of program blocks may be

continuously executed in a single block. Small lines program

includes programs generated by CAM and programs generated by

macro operation.

Example

1: Create a program for the machining as shown in the figure below: The

programming contour must be consistent with the actual contour.

%0061

100

G92 X0 Y0 Z0

G91 G00 G43 Z-10 H01

G41 X50 Y20 D01

G01 G61 Y80 F300

X100

…

150

2: Create a program for the machining as shown in the figure below: no

stops between program blocks.

%0061

100

G92 X0 Y0 Z0

G91 G00 G43 Z-10 H01

Actual path

G41 X50 Y20 D01

G01 G64 Y80 F300

X100

…

150

6. Feed Functions

6.6 Feed Hold (G04)

During automatic running, you may use G04 to pause the tool feed. The

system will automatically execute the ongoing program blocks after the

specified time is expired.

Format

G04 P_; Feed hold

G04 X_;

X: Unit: second

P: Unit: millisecond

Attention

The minimum feed hold time is specified as an interpolation cycle

(Parm000001). If the specified time is less than an interpolation

cycle, it will be executed as an interpolation cycle.

The value after X cannot be greater than 2000; otherwise, the

system will not execute the program.

6. Feed Functions

6.7 High-Speed High-Precision Mode Selection (M) (G05.1)

The command is used to switch among different machining modes to

meet different requirements.

Format

G05.1 Q_; Specify machining mode

……

G05.1 Q0; Default mode

Parameter

Description

Select a machining mode 0, 1, 2 and 3, which can be

switched by G05.1Q_.

Description

Command

Description

G05.1Q0

Default mode; focuses on the balance between efficiency

and precision

G05.1Q1

High-precision mode; focuses on the machined surface

and dimensional accuracy.

G05.1Q2

High-speed and high-precision mode; focuses on

processing smoothness and the balance between the

efficiency and precision.

G05.1Q3

High-speed mode; focuses on the processing efficiency,

improves the processing speed for free curve.

Attention

G05.1Q_ must be specified in a separate line.

7. Reference Point

7.1 Return to Reference (G28, G29, G30)

Reference point is a fixed point on the machine. There are a total of five

reference points: the first, the second, the third, the fourth and the fifth

reference points. You may use the reference command to easily move the

tool to the reference points. The referent points can be used as the tool

change position.

Take the axis 0 as an example. You may set five reference points in the

machine coordinate system by setting the reference point position

parameters (100017, 100021, 100022, 100023, and 100024).

Execution procedure

When you execute the command of returning to the reference point, the

tool automatically passes through the intermediate point to reach the

reference point rapidly. At the same time, the specified intermediate

point is saved in the CNC system, and the tool automatically passes

through the intermediate point and moves along the specified axis to the

end point.

The figure below shows the process that a tool returns to the reference

point:

Start point

Intermediate point

end point

Reference point

Automatically home to reference

point

G28 IP_; Return to the first reference point

G30 P2 IP_; Return to the second reference point (P2 can be omitted )

G30 P3 IP_; Return to the third reference point

G30 P4 IP_; Return to the fourth reference point

G30 P5 IP_; Return to the fifth reference point

7. Reference Point

Parameter

Description

In the absolute value mode (G90), specify the absolute

position of the intermediate point; in the relative value

mode (G91), specify the distance from the intermediate

point to the start point. You do not need to calculate the

The coordinate value specified by IP is

specific movement amount from the intermediate point

the value in the workpiece coordinate

to the reference point.

system. Only the axis specified with the

intermediate point can move when the command of automatic returning

to reference is executed.

G29 IP_;

The coordinate value specified by IP is the value in the workpiece

coordinate system.

The intermediate point is that of G28, G30 specified previously.

Return from reference point

The table below describes the running mode for the relative value (G91):

Execute program

Workpiece coordinate system x, y, z

G54X0Y0Z0

0,0,0

G91G28X10Y10Z10

10,10,10--------->0,0,0

X100

100,0,0

Y100

100,100,0

Z100

100,100,100

G29X10Y10Z10

10,10,10--------->20,20,20

Move to the intermediate point of

G28, and then execute G91

Parameter

Description

In the absolute value mode (G90), specify the end point;

in the relative value mode (G91), the intermediate point

of G29 must be that of G28 specified previously. To

execute G29, you may execute G91 based on the

intermediate point of G28.

7. Reference Point

G29 can be executed only after G28 or G30 has been executed;

otherwise, the execution may be abnormal as there is no intermediate

Attention

point.

(Reference

Return to reference point (G28)

AĺBĺR

point)

Return from reference point

RĺBĺC

(G29)

B (Intermediate point)

Example

500

300

200

A (start point)

C (End point)

200

1000

1300

%1234

G54

G00 X200Y300

G28 G90 X1000.0 Y500.0; program from point A to B. Move through the

intermediate point B, and to the reference point R.

T6;

M06; change tool at the reference point

G29 X1300.0 Y200.0; program from point B to C. Move from the

reference point R, through the intermediate point B, and to the end point

specified by C

M30

8. Coordinate System

8 Coordinate System

reach a predefined position, which is defined based on the coordinate

values within a coordinate system. The coordinate value is specified by

program axis value, so as to process workpiece according to the specific

program.

• Milling machine

(use X40.0 Y50.0 Z25.0 to define the tool

position)

25.0

50.0

40.0

• Turning machine (use X50.0 Z40.0 to define the tool position)

40.0

50.0

Origin

This CNC system provides the following coordinate systems:

• Machine coordinate system

• Workpiece coordinate system

• Local coordinate system

During the machining, the tool may

•

8. Coordinate System

8.1 Machine Coordinate System Programming (G53)

There is a fixed mechanical point on the machine, which can be used as a

datum point of the machine. It is called as the machine origin, of which

position is defined by Zero Block or Grating Zero point. This point is

used as the origin to establish the coordinate system which is called the

machine system.

After power on, you may establish the machine coordinate system by

manually returning to the reference point. Once the machine coordinate

system is established, it remains unchanged before cutting off the power

supply.

Format

G53 IP_;

Parameter

Description

Target position in the machine coordinate system

Define Machine Coordinate

Before calling G53, the machine coordinate system must be established

System

by returning to the reference point.

The reference point does not coincide with the origin of the machine

coordinate system. The figure below shows the relationship between

them:

Machine coordinate system

Machine origin

Reference point

Attention

G53 is a non-modal command, which must be specified at the

current line when conducting the machine coordinate programming.

8. Coordinate System

The target position specified by

G53 cannot be relative

programming. You must use

absolute command for

programming.

The compensation functions such as tool radius compensation, tool

length compensation, and cutter radius compensation are cleared

when the G53 command is specified.

Before specifying the G53 command, you must set the machine

coordinate system; therefore it is necessary to manually return to the

reference point or return to the reference point with the G28

command after power on. You may skip this operation when using

the absolute position encoder.

8. Coordinate System

8.2 Workpiece Coordinate System

The coordinate system used for workpiece machining is called as a

workpiece coordinate system.

The workpiece coordinate system is predefined in the CNC system

(Define workpiece coordinate system).

You may create programs in the defined workpiece coordinate system

and machine the workpiece (Select workpiece coordinate system).

You may move the origin of the defined workpiece coordinate system to

change the workpiece coordinate system (Change workpiece coordinate

system).

8.2.1 Define Workpiece Coordinate System (G92)

workpiece coordinate system:

1. Use G92 to define the workpiece coordinate system.

2. Define the workpiece coordinate system through the selecton of

G code.

Use the workpiece coordinate system on the HMI interface to

define six standard workpiece coordinate systems (G54-59) and

60 extended workpiece coordinate systems (G54.X) (for milling

machining center), and then use the corresponding program

commands to define the workpiece coordinate.

3. For turning machines, in the absolute tool offset compensation

mode, you may define the origin of the workpiece coordinate

system via T commands (see section 10.1)

Under the absolute commands, the workpiece coordinate system must be

established by using any of the methods above.

There are three methods to define a

Format

G92 IP_;

Parameter

Description

The orientation distance from the origin of the

coordinate system to the tool start point.

8. Coordinate System

Set Workpiece Coordinate System

The G92 command can be used to set the relative position of the tool

start point to the coordinate origin. Thereby defining the workpiece

coordinate system. Once the workpiece coordinate system is defined, the

command value in absolute programming is the coordinate value in the

workpiece coordinate system.

1. The execution of this program block is only to set the workpiece

Attention

coordinate system, but the tool will not move.

2. G92 is a non-modal command.

3. In the tool length compensation mode of milling machines, the

coordinate system set G92 command is the specified coordinate

system before conducting the compensation. However, the G code

cannot be executed in the program blocks where the tool length

compensation vector changes. For example, it is cannot be executed

in the following blocks:

• Program blocks where the G43/G44 is specified.

• Program blocks where H code is specified in G43/G44 modes

• Program blocks where G49 is specified in G43/G44 modes

• Program blocks where the compensation vector is canceled by

G28/G53 in G43/G44 modes and the vector is restored

In addition, when setting the workpiece coordinate system with G92, the

programs before it will be stopped and the tool length compensation

defined by MDI cannot be changed.

Use G92 to set the workpiece coordinate system as shown below:

Example

G92 X30.0 Y30.0 Z20.0

8. Coordinate System

8.2.2 Select Workpiece Coordinate System (G54-G59)

You may select the following workpiece coordinate systems that have

been defined:

In the workpiece coordinate system defined by G92, the absolute

command defined is a position in this coordinate system.

Select among 6 standard workpiece coordinate systems of G54 to

G59.

For milling machines and machining centers, select among

extended workpiece coordinate systems of G54.X.

For turning machines, in the absolute tool offset mode, select a

workpiece coordinate system with T commands. For details, see

section 10.1.

Example

%1234

G54

G90 G00 X100 Y100 Z50; Locate X=100 Y=100 Z=50 in the G54

coordinate system

M30

8.2.3 Change Workpiece Coordinate System (G10)

You may change the workpiece coordinate system defined in the

following modes by changing an external workpiece origin offset or

workpiece origin offset:

Workpiece coordinate systems defined by G54-G59

• Set the Coordinate system on the HMI interface.(see relevant

section of Operation manual)

• Select the G code to define the workpiece coordinate systems

• Change the coordinate system origin with G10 command(for

details, see section 15)

Workpiece coordinate systems defined by G54.X for milling

machines

8. Coordinate System

•

• Set the Coordinate system on the HMI interface.(see relevant

section of Operation manual)

• Select the G code to define the workpiece coordinate systems

• Change the coordinate system origin with G10 command(for

details, see section 15)

•

Workpiece coordinate systems defined with absolute tool offset for

turning machines

• Set the Coordinate system on the HMI interface.(see relevant

section of Operation manual)

• Select the G code to define the workpiece coordinate systems

8.2.4 Select Extended Workpiece Coordinate System (G54.x)

In addition to the six standard workpiece coordinate systems, you may

select extended workpiece coordinate systems for milling machines as

required.

A total of

60 extended workpiece coordinate systems for milling

machines are available.

Format

G54.n, G54.1Pn, G54Pn: Select No. n workpiece coordinate system

Parameter

Description

Number of Extended workpiece coordinate system,

ranging from 1 to 60.

Example

%1234

G54.18; or G54.1P18, G54P18

G90 G00 X100 Y100 Z50; locate the position where X=100 Y=100 Z=50

in the 18^th coordinate system

M30

8. Coordinate System

8.3 Define Local Coordinate System (G52)

During workpiece coordinate system programming, you may create a sub

workpiece coordinate system, which is called local coordinate system.

Format

G52 IP_; Define the local coordinate system

G52 IP 0; Cancel the local coordinate system

Parameter

Description

Define the origin of the local coordinate system

Description

The G52 IP_; command can be used to create the local coordinate

systems in all workpiece coordinate systems. The origin of the local

coordinate system becomes the position defined by IP_ in the

corresponding workpiece coordinate system.

Once the local coordinate system is defined, the axial movement

command to be specified will be the coordinate value in the local

coordinate system.

If you want to cancel the local coordinate system or specify coordinate

value in the workpiece coordinate system, you may make the origin of

the local coordinate system coincide with the origin of the workpiece

coordinate system.

Example

%1234

G55; select G55, assuming that the value of G55 in the machine

coordinate system is (10, 20)

G1 X10Y10F1000; move to the point (20, 30) in the machine coordinate

system

G52 X30Y30; set local coordinate system based on G55 in the workpiece

coordinate system, with the origin of (30, 30)

G1 X0Y0; move to the origin of the local coordinate system (the current

position in the machine coordinate system is (40, 50))

G52 X0Y0; cancel the local coordinate system, and restore the G55

8. Coordinate System

workpiece coordinate system

G1 X10Y10; move to the machine coordinate system (20, 30)

M30

Attention

If the local coordinate system is not canceled and the workpiece

coordinate system changes, the local coordinate system is still valid.

Example

%1234

G54; select G54, assuming that the value of G54 in the machine

coordinate system is (10, 10, 10)

G0X0Y0Z0; move to the point (10, 10, 10) in the machine coordinate

system

G52X20Y20Z20; set local coordinate system based on G54 in the

workpiece coordinate system, with the origin of (20, 20, 20)

G0X0Y0Z0; move to the point (30, 30, 30) in the machine coordinate

system

G55; select G55, assuming that the value of G55 in the machine

coordinate system is (12, 12, 12)

G0X0Y0Z0; move to the point (32, 32, 32) in the machine coordinate

system; the local coordinate system is still valid.

G52X0Y0Z0; cancel the local coordinate system and restore the G55

coordinate system

G0X0Y0Z0; move to the point (12, 12, 12) in the machine coordinate

system; the local coordinate system is still valid.

M30

8. Coordinate System

8.4 Select Coordinate Planes (G17, G18, G19)

The coordinate plane selection command G17/G18/G19 is used to select

machining planes during circular interpolation, cutter radius

compensation (M), rotation transformation (M), etc.

Description

G code

Plane

G17

XY plane

G18

ZX plane

G19

YZ plane

Attention

G17, G18, and G19 are modal functions, which can be canceled by each

other.

The motion command has nothing to do with the plane selection. For

example, the Z axis moves even the command G17 G01 Z10 is executed.

HNC-818. User Manual - page 3