HNC8 Series CNC Controller. Programming Manual (V2.4)

G13

G0Z10

G109

G0X120

M105

M30

Example 2: Face contour milling

Programmed

contour

Programmed

path

Tool

%1234

G54

T0101；The workpiece coordinate system is built at the center of rotation on the right end

of the blank, with end milling cutter φ6

G108；Spindle is switched from speed mode to position mode

M103 S1=2000；Tool rotation CW

G37； Radius programming

G0X52Z50C0

G0 Z-5

G12X0CO

G1X50C10F500

N1 G42D1G01X30C10（D1=3）

N2 G1C25

N3 G03X25C30R5

N4 G1X15

N5 G03X10C25R5

N6C10

N7 X30

N8 G40X50

G13

G0Z10

G109；Spindle is switched from speed mode to position mode

G0X52

M105；Tool stops

M30

Note

Before entering the polar coordinate interpolation mode, cancel the tool radius compensation and

tool length compensation, and specify the tool compensation in the polar coordinate interpolation

mode.

11.10

Cylindrical interpolation（G07.1）

Function and Purpose



With this function, the shape of the side surface of the cylinder (the shape on the cylindrical coordinate

system) is expanded into a plane, and the expanded shape is used as the plane coordinate for the program

command, then the system converts it to the movement on linear axis and rotary axis of the cylindrical

coordinate when performing machining to execute the contour control.

Rotary axis

Linear axis

Linear

axis

Expand the cylinder

Rotary

axis

Command Format

G07.1 RC= r

； Start of cylindrical interpolation (r: radius of cylinder)

……

G07.1 RC=0

； End of cylindrical interpolation

Description



Circular interpolation

The circular interpolation (G02, G03) in the cylindrical interpolation plane is performed, and the

coordinate system plane is determined based on the parallel axis in the cylindrical interpolation.

Set X axis as the horizontal axis in

G02, G03 are specified in X-C plane

Parm040092 = 0

the cylindrical interpolation plane

(G17) with IJR programming

Set Y axis as the horizontal axis in

G02, G03 are specified in Y-C plane

Parm040092 = 1

the cylindrical interpolation plane

(G19) with JKR programming

Set Z axis as the horizontal axis in

G02, G03 are specified in Z-C plane

Parm040092= 2

the cylindrical interpolation plane

(G18) with IKR programming

Compensation

The tool radius compensation and tool length compensation should be cancelled before entering

the cylindrical interpolation mode, and the tool compensation should be specified in the

cylindrical interpolation mode.

Related parameters

Parameter name

Parameter

Default

Description

Channel parameter

Parm040090

5（C axis）

Rotary axis No. in cylindrical interpolation

(CH0)

Parm040091

2（Z axis）

Linear axis No. in cylindrical interpolation

Parm040092

1（Y axis）

Parallel axis No. in cylindrical interpolation

Example

Example 1: Contour milling

G54

T0101；Radial face milling cutter ø2, workpiece ø30

G108

G19；Select a plane

M103 S1=1000；The second spindle rotates CW, the direction of tool rotation is related

to the tool post

G0X50C0

G0X50C0

G40G1 Z5

G0 Z50

M99

G07.1 RC=18.5

G0Z5

M98P1L4

G90

G07.1 RC=0;

G109

G18

G0X100 Z100

M105

M30

11.11

Polar Coordinate Command（G15/G16）

Function and Purpose



When the angle and radius are marked on the drawings of the parts, the "polar diameter" and

"polar angle" of polar coordinate are used to define the end positions of the program, which can

greatly simplify the programming calculation.

In the specified plane of the polar coordinate system, the counterclockwise direction of the polar

axis movement is the positive direction of the polar angle, and the clockwise direction of the polar

axis movement is the negative direction of the polar angle.

Both "polar diameter" and "polar angle" can be specified under absolute

programming/incremental programming (G90, G91).

Command Format

G17(or G18/G19)；

G16 ；

G90 X- Y-

(or G91 X- Y-)；

G15；

XY plane: polar radius is specified with X axis, and polar angle is

G17

specified with Y axis.

To specify the plane of

ZX plane: polar radius is specified with Z axis, and polar angle is specified

G18

polar coordinate system

with X axis.

YZ plane: polar radius is specified with Y axis, and polar angle is specified

G19

with Z axis.

To specify the origin of

Workpiece coordinate system zero (or local coordinate system zero) is

G90

polar coordinate system

specified as the origin of polar coordinate system (polar origin)

G91

The current position is specified as the origin of polar coordinate system

(polar origin)

G16

Polar coordinate programming starts

G15

Polar coordinate programming ends

In absolute programming: Polar diameter measured from the workpiece

To specify polar diameter

coordinate system zero (or local coordinate system zero)

In incremental programming: Polar diameter measured from the current

point

In absolute programming: Polar angle measured with workpiece zero as

To specify polar angle

the polar origin

In incremental programming: Polar angle measured with the current point

as the polar origin

Description



Polar coordinate system origin setting

There are two ways to set the polar coordinate system origin:

(1) At the time of programming with polar coordinate, if the polar origin is defined in absolute

mode (G90), the polar coordinate system origin will be the workpiece origin or the local

coordinate system origin.

(2) At the time of programming with polar coordinate, if the polar origin is defined in incremental

mode (G91), the polar coordinate system origin will be the current point.

Polar coordinate command position

(1) When workpiece coordinate system origin is the center of polar coordinate,

The workpiece coordinate system origin is the polar coordinate center when the radius is specified

in absolute mode.

Only when the local coordinate system (G52) is used, the origin of the local coordinate system is

the center of the polar coordinate.

Command position

Radius

Current position

Angle

When the angle is in absolute mode

When the angle is in incremental mode

(2) When the current position is the center of polar coordinate,

The current position is the polar coordinate center when the radius is specified in incremental

mode.

Command position

Angle

Radius

Angle

Current position

When the angle is in absolute mode

When the angle is in incremental mode

(3) When radius command is ignored,

When the radius is ignored, the origin of the workpiece coordinate system is the polar coordinate

center, and the distance from the polar coordinate center to the current position is the radius. Only

when the local coordinate system (G52) is used, the local coordinate origin is the polar coordinate

center.

Command position

Current position

Angle

Current position

Angle

Radius

When the angle is in absolute mode

When the angle is in incremental mode

(4) When angle command is ignored,

When the angle command is ignored, the angle of the current position in the workpiece coordinate

system is the angle command.

When the radius is commanded in the absolute mode, the origin of the workpiece coordinate

system is the polar coordinate center. Only when the local coordinate system (G52) is used, the

origin of the local coordinate system is the polar coordinate center.

In addition, when the radius is specified in the incremental mode, the current position is the polar

coordinate center.

Command position

Radius

Current position

Angle

When the angle is in absolute mode

Example

Example 1: Mill a hexagon with the polar coordinate programming, the workpiece origin is set at

the center of the hexagon (as shown below), and the processing path is a→b→c→d→e→f.

Processing path

Absolute

Incremental

Commanded

programming

position

Position to a point

G54G0X50Y0

(X50、Y0)

Polar coordinate command

G17G90G16

(X50、Y0)

starts

a→b

G1X50Y60F120

G1X50Y60F600

(X25、Y43.3)

b→c

Y120

G91Y60

(X-25、Y43.3)

c→d

Y180

Y60

(X-50、Y0)

d→e

Y240

Y60

(X-25、Y-43.3)

e→f

Y300

Y60

(X25、Y-43.3)

f→a

Y360

Y60

(X50、Y0)

Polar coordinate command is

G15

(X50、Y0)

disabled

Program ends

M30

Example 2: As shown in the figure below, use polar coordinate programming to drill 3 holes with

a diameter of 10mm on the workpiece.

(The workpiece coordinate system zero is O, and the rotation polar origin A of polar coordinate

is outside the worktable the machine tool)

Absolute

Incremental

Processing path

Commanded position (X, Y, Z)

programming

Position above the zero

G54G0X50Y0Z30

(50、0、30)

Establish G52 local coordinate system

G52X-50Y-270

(50、270、Z30)

Polar coordinate command starts

G17G90G16

(50、270、Z30)

Drill hole at c point in the plane

G82X300Y85Z-

(26.147，298.858，-10)

10R5F100

Drill hole at b point in the plane

Y90

G91Y5

(0、300、-10)

Drill hole at a point in the plane

Y95

(-26.147，298.858，-10)

Polar coordinate command is disabled

G15

(-26.147，298.858，30)

Local coordinate system is cancelled

G52X0Y0

(-76.147，28.858、30)

Program ends

M30

Note

(1) The axis commands accompanied by the following commands will not be regarded as polar

coordinate commands;

 Dwell G04

 Programmable data input G10

 Local coordinate system G52

 Workpiece coordinate system change G92

 Machine coordinate system selection G53

 Coordinate rotation G68

 Scaling G51

(2) In polar coordinate mode, the angle and radius R cannot be specified;

(3) For polar coordinate programming, when radius is specified in absolute mode, the workpiece

origin is set as the polar coordinate center; when radius is specified in incremental mode, the

current position is set as the polar coordinate center. However, when only the angle is specified

in the command, regardless of whether it is in absolute or incremental mode, the workpiece origin

is set as the polar coordinate center.

11.12

NURBS Spline Interpolation

Function and Purpose



This function only needs to specify the NURBS

(non-uniform rational B-spline) curve

(degree/weight/node/control point) used in curve/curved surface processing to realize NURBS

curve processing without replacing tiny line segments.

In NUBRS interpolation, interpolation is performed at the commanded speed, but at positions

with large curvature, the speed is limited to a speed that does not exceed the allowable acceleration

of the machine tool.

Command Format

NURBS P_ K_ X_ Y_ Z_ W_ F_ E_ ;

Parameter

Meaning

Order of NURBS curve, only cubic spline is supported. P is 4

Node

X, Y, Z

Coordinate value of control point

Weighting

Feedrate

2nd feedrate

Description



Cancel interpolation

NURBS belongs to the 01 group of modal, and the NURBS interpolation modal can be released

by specifying G01 or G00.

Order of curve

P is to specify the order of NURBS curve;

When P=4, it indicates the cubic NURBS curve;

P is a modal address word, and P will remain valid until it is changed or other modal commands

of group 01 are specified.

Node

In NURBS interpolation, user must specify the first control point as the starting point and the final

control point as the end point.

In addition, when specifying the node of the first block, please use the following format:

Single spline

NURBS P4 K{0,0,0,0,1} X1 Y0 Z0

Double-spline

NURBSB P4 K{0,0,0,0,0.5}Q{10,0,0,38.28,0,28.28} W1F60

Weighting

The weight is the weight of the designated control point in the same block. When it is omitted,

the default value is 1.0

Compensation

Tool radius compensation cannot be used in NURBS curve interpolation.

Description

Single spline NURBS is generally used for three-axis small line segment interpolation.

Double-spline NURBS is generally used for five-axis small line segment interpolation.

Example

R=50mm Please use the single spline NURBS interpolation for the full circle shown as below,

R=50mm.

%0001

G54

G90G17F500G64

G01X0Y0Z0

NURBS P4 K{0.0,0.0,0.0,0.0,0.5} X0.0Y0.0Z0.0 W1.0

K0.5

X0.0000 Y100.0 W0.3333

K0.5

X100.0 Y100.0 W0.3333

K1.0

X100.0 Y0.0

W1.0

K1.0

X100 Y-100.0 W0.3333

K1.0

X0.0

Y-100 W0.3333

K1.0

X0.0

Y0.0

W1.0

M30

11.13

HSPLINE Spline Interpolation

Function and Purpose



HSPLINE is the abbreviation of Hermite SPLINE. Hermite interpolation function can also

improve the processing effect of small line segments and make the processed surface smooth.

Unlike the NURBS curve, the Hermite curve passes through the control points, while the Nurbs

curve does not pass through the control points. The system performs spline interpolation by

specifying the control points and vectors of the Hermite curve

Command Format

HSPLINE P_X_Y_Z_I_J_K_W_F_ ；

Parameter

Meaning

Degree of HSPLINE spline curve

X,Y,Z

Coordinates of control point

I,J,K

Vector of control point

Weighting

Order of Hermite curve

Description



Cancel interpolation

HSPLINE belongs to the 01 group modal, and the HSPLINE interpolation modal can be cancelled

by specifying G01 or G00.

Degree of curve

The degree of HSPLINE spline curve is specified with P, and this value is 3 currently.

Compensation

The tool radius compensation cannot be used in the HSPLINE curve interpolation mode.

Example

Example 1: Use cubic Hermite spline to interpolate the following spatial curve

%0001

G54G0X0Y0Z0

G90G17 F1000G64

X0.005Y-0.987Z0.04

HSPLINE P3 X0.005 Y-0.987 Z0.040 I1.000 J-0.026 K-0.002；Q1

X0.748 Y-0.727 Z0.027 I0.756 J0.655 K-0.016

；Q2

X1.049 Y-1.097 Z0.023 I0.967 J0.256 K-0.011

；Q3

X1.249 Y-0.727 Z0.053 I0.497 J0.866 K0.050

；Q4

M30

Example 2: Use Hermite spline interpolation to program R50 full circle (starting point X0Y0) in

G17 plane

%1234

G54G01 X0 Y0 Z0 F2000

HSPLINE P3 X0 Y0 Z0 I0 J1 K0 （0°）

X6.698729 Y25 Z0 J0.866025 I0.5 K0；(30°)

X14.644661 Y35.355339 Z0 I0.707107 J0.707107 K0(45°)

X25 Y43.301270 Z0 J0.5 I0.866025 K0 ；(60°)

X50 Y50 Z0 I1 J0 K0；(90°)

X75 Y43.301270 Z0 J-0.5 I0.866025 K0 ；(120°)

X85.355339 Y35.355339 Z0 I0.707107 J-0.707107 K0 ；(135°)

X93.301270 Y25 Z0 J-0.866025 I0.5 K0； (150°)

12 Tool Compensation Function

12.1

Turning Tool offset Compensation（T）

Function and Purpose



When editing the program, it is generally assumed that the positions of the tool noses are the same,

but due to the difference in tool shape and installation, the actual positions of the tool noses cannot

be consistent. The position deviation between the programmed assumption and actual positions

is handled with the tool offset compensation for lathes.

Command Format

The first two digits of the T command (turning system) are the tool number, and the last two digits

are the tool offset number, that is, the number of the register where the tool offset value is stored.

The call of lathe tool offset compensation is implemented by the last two digits of the command

The format of T command is : T and the following 4 digits. See the figure below.

 The first two digits is the tool number (the currently selected tool number)

 The last 2 digits is the tool offset number (the number of the register where the offset is stored

and the number of the register where the radius compensation is stored)

Tool offset number

Tool No. selection

Description



1. Tool offset compensation setting

One tool needs to use one tool number, and one tool nose position needs to use one tool offset

number. When the tool has only one tool nose position, the tool number and tool offset number

are generally the same number for easy memory, such as T0101. When a tool has multiple tool

nose positions to be used, a tool number needs to correspond to multiple offset numbers. To

facilitate memory, the unit digit value of the tool number generally keep the same with that of the

tool offset number, such as T0202, T0212, T0222.

2. Cancel tool offset compensation

When the offset number is set to 00, it means that the tool offset function is cancelled and the

offset is 0.

3. Relative offset compensation and absolute offset compensation

There are two modes of the tool offset value: incremental offset and absolute offset

 Incremental offset

The position deviation of each tool nose relative to the standard tool nose. In this mode, the

program also needs a command to call the positional relationship between the standard tool

and the workpiece zero (such as the G92 command).

 Absolute offset

When each tool is at the machine zero (the machine returns to zero and the tool is at the

machining position), the position deviation of the workpiece zero relative to the nose of each

tool is shown as below:

Machine zero

No.1 tool offset on Z

No.2 tool

offset on Z

Workpiece zero

No.2 tool

No.1 tool

offset on X

The HNC8 system adopts the absolute offset compensation mode. In the above figure, the absolute

offset value of No. 1 tool is: X axis X1 (diameter value), Z axis Z1; the absolute offset value of

No. 2 tool is: X axis X2 (diameter value), Z axis Z2.

During programming, the tool number and offset number of each tool are generally set to be the

same for user to remember. As shown in the figure above, T0101 and T0202 are used to execute

tool change and offset compensation. At this time, the offset values X1 Z1 of No. 1 tool must be

stored in the No. 1 offset compensation register, and the offset values X2 Z2 of No. 2 tool must

be stored in the No. 2 offset compensation register.

When the system executes the tool offset compensation, the machining coordinate system of No.1

and No.2 tools are set as (X1, Z1) and (X2, Z2) respectively. Therefore, though the geometric

dimensions of tools 1 and 2 are different, and the distances of both tools relative to workpiece

zero are different when tool post is at the machine zero, the coordinate system established for

each is coincident with the workpiece coordinate system.

4. Tool wear compensation

The error caused by tool wear is handled with wear compensation. The system stores the wear

compensation amount and the offset compensation amount in the same register address number.

Therefore, when the T command is used for offset compensation in the program, the position

offset and wear stored in the register will be called for compensation.

5. Tool path for tool offset and wear compensation

The figure below shows the tool position point trajectory for the situation: first establishing the

tool offset and the wear compensation, and then canceling the tool offset and the wear

compensation.

Tool compensation path

Programmed path

Example

N1 G00X100Z140

N2T0313 (No. 3 tool and No. 13 tool offset is selected)

N3X200Z150

As shown in the figure below, if the tool path has compensation values in the X and Z directions

relative to the programmed path (the vector composed of the compensation components in the X

and Z directions is called the compensation vector), then the end position in the block is added or

subtracted by the compensation amount (compensation vector) specified by the T code is the end

position of the tool path section.

Compensation path

Compensation vector (composed

of components on X and Z

Programmed path

Block including T code

Note

1) The tool offset compensation value can be automatically generated through the tool setting

operation, or it can be manually input into the offset compensation register after tool setting and

calculation. Please refer to the operation manual for specific operations.

2) Both the wear value and the offset value will be included in the program. If they are not needed,

be sure to set to 0.

12.2

Turning Tool Nose Radius Compensation（G40/G41/G42）（T）

Function and Purpose



The CNC program is generally aimed at a certain point on the tool which is the tool position to

compile the path of the tool. The tool position of the turning tool is an imaginary tool nose point

in an ideal state. This point is small enough and strong enough, and the workpiece contour is

finally machined by this point. However, due to process or other factors, the actual lathe tool nose

is often not an ideal point but a circular arc, so the actual cutting point of the tool (the final contact

point between the tool and the workpiece) will be changed on the circular arc of tool nose. This

position deviation between the actual cutting point and the tool position will inevitably cause

overcutting or undercutting of the workpiece, as shown in the figure below.

Actual contour

Programmed path

The machining error caused by the tool nose being not an ideal point but a circular arc can be

eliminated by the tool nose radius compensation function.

Command Format

G code

Workpiece position

Tool path

G40

Tool nose radius

Move along tool path

compensation is cancelled

G41

Tool nose radius

The left of the programmed path is compensated.

compensation left

G42

Tool nose radius

The right of the programmed path is compensated.

compensation right

Note: Radius compensation does not support the programs in interrupt format, such as G31.

Description



1. Imaginary tool nose point

 The imaginary tool nose point during programming;

 The point is assumed to be small enough and strong enough during programming, without

interference and cutting point position change;

 The contour of the workpiece is formed by the final processing trajectory of this point;

 This point is the description point of the programmed path;

2. Tool position

 Standard imaginary tool nose point;

 This point is the description point of programmed path;

 This point is the tool setting point;



9 positions can be used as the tool position for each tool nose. There are a total of 10 numbers

of tool position;

 No. 0 and No. 9 tool positions are the circular center of the tool, and the other No. 1 to 8 tool

positions respectively correspond to a point position;

 The main principle of tool position selection is ease of operation;

 According to the numbering rules of tool position, there is a certain difference in the visual

expression of tool positions between machine tools with front tool post and with rear tool

post

3. Tool position of machine tool with front tool post

represents the tool position point A, + represents the tool nose

center O

4. Tool position of machine tool with rear tool post

represents the tool position point A, + represents the tool nose

center O

5. Tool nose radius compensation left/right（G41\G42）

 How to determine the right or the left,

 G41（compensation left

：On the positive side of the third axis, user views

along the direction of tool movement, when the tool is on the left side of the

tool path, tool nose radius compensation left is determined.

 G42（compensation right）：On the positive side of the third axis, user views

along the direction of tool movement, when the tool is on the right side of the

tool path, tool nose radius compensation right is determined.

 Tool nose radius compensation left/right for machine tool with front tool post and rear tool

post

 Because the direction of the third axis for machine tools with the front and rear tool post, the

directions of the tool nose radius compensation are different. The third axis of the machine

tool with rear tool post points to the same direction as the customary direction; the third axis

direction of the machine tool with front tool post is opposite to the customary direction. See

the figure below for details

 Figure of tool nose radius compensation for tool machine with front tool post

Workpiece side

Left compensation G41

Tool movement

direction

Right compensation G42

Workpiece side

 Figure of tool nose radius compensation for tool machine with rear tool post

Workpiece side

Left compensation G42

Tool movement

direction

Right compensation G41

Workpiece side

6. Add or cancel tool nose radius compensation

 The tool radius compensation can only be added or cancelled in the G00 or G01 block. When

it is added or cancelled in the G02 or G03 block, the system will alarm;

 When adding or canceling tool radius compensation, it must be in the traverse command

block and there is enough moving distance, otherwise overcutting will occur;

 When adding tool radius compensation, user needs to specify the corresponding tool nose

radius compensation value. The register for storing the radius compensation value has the

same number as the offset compensation register, so the tool offset number must be specified

with the T command;

 After the execution of the tool radius compensation (G41/G42) block is completed, the center

of the tool stops directly above the normal direction of the starting point of the lower path.

N3 G00 X40 Z5

(Move to the starting position of program)

N4 G00 X0

(Tool moves to the workpiece center)

N5 G01 G42 Z0 F60

(Tool radius compensation is added, and move close to workpiece)

N6 G03 U24 W-24 R15

(Process R15 arc)

N7 G02 X26 Z-31 R5

(Process R5 arc)

N8 G01 Z-40

(Process Φ26 outer circle)

N9 G00 X30

(Exit the processed surface)

N10 G40 X40 Z5

(Cancel radius compensation, return to the starting position of program)

N11 M30

(Spindle stops, main program ends and resets)

Note

(1) G40, G41, and G42 are all modal codes, which can be mutually cancelled.

(2) Only G00 or G01 instead or G02 or G03 can be used for the creation and cancellation of tool

nose radius compensation.

(3) When using G41 or G42 to enable radius compensation, the corresponding radius

compensation register with radius compensation value must be designated. The radius

compensation register number is the same as the tool offset compensation register number.

(4) There must be a traverse command and a traverse distance in the block where the tool radius

compensation Enable (G41/G42) or the tool radius compensation Disable (G40) is added.

12.3

Milling Tool Length Compensation（M）

Function and Purpose



It is to set the difference between the tool length during programming and the actual tool length

in the tool length compensation register. Calling this function can move the tool to the

programmed end position without modifying the program, thus making the program universal.

Tool used in programming

Actually used tool

Tool length compensation

Command Format

G43/G44 H_ Z_

…...

G49

Tool length compensation is specified with G43 and G44.

Parameter

Meaning

Tool length compensation plus (The tool length compensation value is added to

G43

the theoretical position in the tool axis direction)

Tool length compensation minus (The tool length compensation value is

G44

subtracted from the theoretical position in the tool axis direction)

The number of tool length compensation amount in the tool compensation table

G49

Cancel tool length compensation

Description



Tool length compensation type

(1) According to the tool length compensation axis, the following two tool length compensation

types can be used,

Type

Description

Format

Tool length compensation along basic Z axis

G43/G44 Z_H_

Tool length compensation along the vertical direction of the

G17 G43/G44 Z_H_

selected plane

G18 G43/G44 Y_H_

G17：XY plane；G18：ZX plane；

G19 G43/G44 X_H_

G19：YZ plane；

(2) The tool length compensation types A and B are set by the parameters, and the related

parameter are as below,

Parameter

Description

000012

Tool axis selection mode

000012：This parameter is used to determine which axis the G43/G44 tool length compensation

function should be performed on.

0: The tool length compensation is always performed on Z axis;

1: Tool length compensation axis is switched based on the coordinate plane selection

(G17/G18/G19) corresponding to Z/Y/X-axis respectively.

Movement amount of tool length compensation

(1) Movement amount of tool length compensation: when G43 or G44 tool length compensation

is executed, the movement amount is calculated according to the below formula:

G43 Z_ H_；Z_ + H_（tool length compensation）Compensaiton in + direction

G44 Z_ H_；Z_- H_（tool length compensation） Compensation in - direction

As shown in the above calculations, regardless of whether the absolute command or the

incremental value is used, the actual end point is of the coordinates which is compensated with

the specified compensation amount based on the end point coordinates of programmed traverse

command

(2) When there is length wear in the tool compensation table: for the execution of tool length

compensation command G43 or G44, the movement amount is calculated according to the

following formula

G43 Z_ H_；Z_ + H_（tool length compensation）+ H_（tool length wear）

G44 Z_ H_；Z_- H_（tool length compensation）- H_（tool length wear）

(3) When there is coordinate value in the workpiece coordinate system: for the execution of tool

length compensation command G43 or G44, the movement amount is calculated according to the

following formula

G43 Z_ H_；Z（workpiece coordinate system）+ Z_ + H_（tool length compensation）

G44 Z_ H_；Z（workpiece coordinate system）+ Z_- H_（tool length compensation）

(4) When there is coordinate value in the workpiece coordinate system and length wear in the tool

compensation table: for the execution of tool length compensation command G43 or G44, the

movement amount is calculated according to the following formula

G43 Z_ H_；Z（workpiece coordinate system）+ Z_ + H_（tool length compensation）+ H_

（tool length wear）

G44 Z_ H_；Z（workpiece coordinate system）+ Z_- H_（tool length compensation）- H_（tool

length wear）

(5) When there is coordinate value in the workpiece coordinate system, and there is a coordinate

value of external zero offset: for the execution of tool length compensation command G43 or G44,

the movement amount is calculated according to the following formula

G43 Z_ H_；Z（workpiece coordinate system）+ Z（external zero offset）+ Z_ + H_（tool length

compensation）

G44 Z_ H_；Z（workpiece coordinate system）+ Z（external zero offset）+ Z_- H_（tool length

compensation）

(6) When there is coordinate values in workpiece coordinate system and external zero offset, and

there is length wear in the tool compensation table: for the execution of tool length compensation

command G43 or G44, the movement amount is calculated according to the following formula

G43 Z_ H_；Z（workpiece coordinate system）+ Z（external zero offset）+Z_ + H_（tool length

compensation）+ H_（tool length wear）

G44 Z_ H_；Z（workpiece coordinate system）+ Z（external zero offset）+Z_- H_（tool length

compensation）- H_（tool length wear）

Tool length compensation number

(1) The working range of the compensation number depends on the parameter setting. The

relevant parameters are as follows:

Parameter

Description

000060

Number of tools stored in system

NC000060: This parameter is to set the number of tool of which the data (tool offset, wear, radius,

tool nose direction, etc.) is saved in the tool compensation table. The value must be greater than

or equal to the sum of the tools in each channel.

Max. value：1000 Default：100 Min. value：0

(2) When the commanded compensation number exceeds the range, the system will give an alarm

of "illegal tool compensation number".

(3) After the compensation number specified in G43 or G44 block, it cannot become the modal

called later to be effective.

For example, H1 modal in N1 line cannot take effect in N4 line in the following program.

N1 G43 Z0 H1； Perform tool length compensation via H1

N2 G0 X0 Y0；

N3 G49 Z0； Tool length compensation is cancelled

N4 G43 Z0； Tool length compensation will not be performed through H1 again, and the

compensation number must be specified again.

(4) In the G43/G44 modal, when G43/G44 is commanded again, the compensation will be

performed according to the new compensation number, that is, the new offset value will not be

added to the old offset value when the offset number is changed.

For example, the N2 line of the following program is compensated according to the new

compensation number H2.

N1 G43 Z0 H1； Tool length compensation is performed via H1

N2 G43 Z0 H2； Tool length compensation is performed with the new compensation number

Cancel the tool length compensation

(1) After the system restarts and M02, M30, G49 are executed, tool length compensation is

cancelled.

(2) H0 is specified, tool length compensation is cancelled.

(3) When Reset or Emergency Stop is pressed during tool length compensation modal, tool length

compensation is cancelled.

(4) When tool length compensation type B is used, the following items must be noted for

canceling tool length compensation with G49.

(a) When the length compensation is cancelled with G49, only the length compensation in

the last selected plane before G49 command is cancelled;

For example, in the below program, G49 in N6 line only cancels the length compensation in

G19 plane.

N1 G28 X0 Y0 Z0；

N2 G92 X0 Y0 Z0；

N3 G17 G43 Z0 H1； Tool length compensation in XY plane is performed via H1

N4 G18 G43 Y0 H2； Tool length compensation in ZX plane is performed via H2

N5 G19 G43 X0 H3； Tool length compensation in YZ plane is performed via H3

N6 G49；

The length compensation only in G19 plane is cancelled

N7 G0 X0 Y0 Z0；

(b) When using G49 to cancel the length compensation in all planes, the plane selection

command (G17/G18/G19) must be specified after the G49 command, and it must be specified

in a separate line;

For example, the correct programming based on the above is as following

N6 G49 G17；

N7 G49 G18；

N7 G18；

N8 G49 G19；

N8 G19；

Wrong way: G49 G17 G18 G19, only the length compensation in the last plane selected

before the G49 command.

Actions when other commands are executed in the tool length compensation modal

(1) Whether the tool length compensation will be restored after G53 or G28 is executed in the tool

length compensation modal depends on the parameter setting. The relevant parameters are as

follows:

Parameter

Description

000014

Whether tool length compensation is restored after

G53/G28

000014：This parameter is to set whether to automatically restore the tool length compensation

function after executing G53/G28 commands.

0: After executing G53/G28 command, the tool length compensation function will not be

restored automatically.

1: After executing G53/G28 command, the tool length compensation function will be

restored automatically.

(2) Whether the tool length compensation will be restored after the G30 command is executed in

the tool length compensation modal depends on the setting of parameter 000014

(3) When G29 is executed in tool length compensation modal, the tool length compensation will

not be cancelled, and cannot be controlled by 000014 parameter.

For example,the machine coordinate is Z55.0 after N4 line is executed when H1=50 in the

following program

N1 G28 Z10；

N2 G90 G92 Z0；

N3 G43 Z0 H1； Tool length compensation is performed via H1.

N4 G29 Z5； Machine coordinate is Z55.0. Machine coordinate is Z-45.0 when G44 is used.

N5 G49； Tool length compensation is cancelled.

(4) When G54 to G59 commands are executed in the tool length compensation modal to change

the workpiece coordinate system, the tool length compensation will not be cancelled, and the end

point coordinates of the compensation axis will be recalculated based on the given coordinate

system.

Example

Create the machining program for the parts shown in the figure below with tool length

compensation. Requirements are as follows:

(1) Set the workpiece coordinate system in the G54 coordinate system based on the workpiece

zero as shown in the figure

(2) Process according to the path 1 to 13 indicated by the arrow

(3) Write out the coordinate value in the workpiece coordinate system and the compensation value

in the tool compensation table before programming

(4) Write the comment and machine coordinate of each line of program

(5) The program must be safe and reliable

Tool length=120mm

Tool nose=4mm

Machine origin

Tool length

Workpiece origin

Workpiece coordinate system：G54（X200，Y100，Z-280） Compensation value：H01=-

120

%1234

G54 G90 M03 S600

； Select workpiece coordinate system G54, use absolute command G90

to program, spindle rotates CW

G00 Z50

；Rapid traverse to Z50, （Z-230）

X0 Y0

；X0 Y0, Rapid traverse to X0 Y0, （X200，Y100）

X30 Y80

；①, Rapid traverse to X30 Y80（X230，Y180）

G43 Z5 H01 ；②, Establish tool length compensation, and rapid traverse to Z25，（Z-395）

G01 Z-18 F300

；③, Z-18Process #1 hole to Z-18，（Z-418）

G04 P2000

；④, Pause for two seconds at the bottom of the hole

G00 Z5

；⑤, Rapid traverse to Z5，（Z-395）

X60 Y30

；⑥, Rapid traverse to X60 Y30，（X260，Y130）

G01 Z-40

；⑦, Process #2 hole to Z-40，（Z-440）

G00 Z5

；⑧, Rapid traverse to Z5，（Z-395）

X110 Y60

；⑨, Y60Rapid traverse to X110 Y60，（X310，Y160）

G01 Z-22

；⑩, Process #3 hole to Z-22，（Z-422）

G04 P2000

；⑪, Pause for two seconds at the bottom of the hole

G49 G0 Z50 ；⑫, Cancel the tool length compensation, and rapid traverse to Z50，（Z-230）

X0Y0

；⑬, Rapid traverse to X0 Y0，（X200，Y100）

M05

； Spindle stops

M30

； Program ends

Note

(1) The direction of tool length compensation is always perpendicular to the plane selected by

G17/G18/G19.

(2) The compensation number H_ must be given after G43/G44 command, otherwise the system

will issue an alarm of "No compensation number specified".

(3) The compensation axis (X/Y/Z) must be specified after G43/G44 command, or the traverse

command of compensation axis must be specified before the next G43/G44 command, otherwise

the length compensation will be invalid.

(4) G43/G44/G49 are all modal codes and can be mutually cancelled, but they can be mutually

cancelled only when they are not specified in the same line. When G43 and G44 are specified in

the same line, the system will alarm; when G49 is specified in the same line as G43/G44, G49

will not take effect.

(5) G43/G44/G49 For G43/G44/G49, after startup, emergency stop and reset, G49 state is the

default.

(6) When using G43/G44 to specify H0, the tool length compensation will be cancelled, but the

modal display area is still G43/G44, and will not be changed to G49, so when H_ is given

separately at this time, the tool length compensation will take effect again.

(7) When G49 is not used, use H0 to cancel the tool length compensation, and then add the tool

length compensation with H_; When H0 is used to cancel the tool length compensation, there is

no tool length compensation until H_ is used again.

For example,

N1 G43 Z0 H1

； Tool length compensation is performed with H1

N2 G43 Z0 H0

； Tool length compensation is cancelled with H0

N3 G0 Z5

； There is no tool length compensation

N4 H2

； Tool length compensation is performed with H2

N5 G0 Z0

； There is tool length compensation

N6 G49

； Tool length compensation is cancelled

(8) After the tool length compensation is set in MDI, it will always be valid for the subsequent

MDI program. The tool length compensation will only be cancelled after HO is specified with

reset, emergency stop and MDI, as well as G49 command being executed on MDI interface.

(9) After the tool length compensation is set in MDI, it will not be effective for the program in the

program file. After switching from the MDI interface to the program interface, the modal becomes

the G49 modal, so it will not be effective.

(10) When the G43/G44 tool length compensation program is stopped with reset or emergency

stop, the tool length compensation will be cancelled. When the program is stopped with the dwell

or switching mode, the tool length compensation will not be cancelled.

(11) After the tool length compensation is set with G43/G44, the tool length compensation will

be performed based on the corresponding H number.

(12) In the auto mode, when using the breakpoint save and restore functions after the tool length

compensation command, the system can correctly establish the tool length compensation after the

program resumes execution. If there are multiple G43/G44 tool length compensation commands

in the program, the system can also correctly establish tool length compensation through the

corresponding G43/G44 commands after the breakpoint is restored.

(13) After the tool length compensation command is used to specify the line operation with any

line function, the system can correctly establish the tool length compensation; If there are multiple

G43/G44 tool length compensation commands in the program, the system can also correctly

establish tool length compensation through the corresponding G43/G44 commands.

For example, when the following program runs from line N3 with any line function, the system

can correctly establish tool length compensation

N1 G43 Z0 H1

N2 G0 Z5

N3 G0 Z10； Use any line function to run from this line

N4 G0 Z15

N5 G0 Z20

N6 G49；

12.4

Milling Tool Radius Compensation（G40/G41/G42）（M）

Function and Purpose



When the CNC machine tool mills the contour of the workpiece, the tool center is usually used

as the path for easy programming. The tool radius is not considered when programming, and the

tool path is programmed based on the contour size of the workpiece. But there will be an offset

(tool radius) between the actual tool path and the workpiece contour. Therefore, the offset of the

tool center path is needed during programming to make the tool path consistent with the

workpiece contour, which is called tool radius compensation function.

In addition, the tool radius is changed due to tool change or tool wear. With this function, user

can directly modify the corresponding radius compensation value or wear value in the tool

compensation table without modifying programming.

After the tool radius compensation is performed, the tool path is shown as the dotted line in the

figure below:

Command Format

G00 X_ Y_ D_

G17 G41/G42

{

G01 X_ Y_ D_

G00 X_ Z_ D_

G18 G41/G42

{

G01 X_ Z_ D_

G00 Y_ Z_ D_

G19 G41/G42

{

G01 Y_ Z_ D_

Parameter

Meaning

G17/G18/G19

To specify compensation plane, XY, XZ, ZY-plane respectively.

Tool radius compensation is valid. G41: Tool radius compensation

G41/G42

Left; G42: Tool radius compensation Right

To specify the compensation number

Description



1) Tool radius compensation direction

Tool compensation path

Description:

G41 Tool radius compensation Left

Viewed from the positive direction to the negative

direction of the third axis that is not in the machining

Programmed path

plane, the tool is on the left side of the workpiece

relative to the direction of tool movement

Left compensation

G41：Offset is performed to the left side of the tool path (as shown in the figure a below).

G42：Offset is performed to the right side of the tool path (as shown in the figure b below).

Tool compensation path

Description:

G42 Tool radius compensation Right

Viewed from the positive direction to the negative

direction of the third axis that is not in the machining

Programmed path

plane, the tool is on the right side of the workpiece

relative to the direction of tool movement

Right compensation

2) Tool radius compensation number

The effective range of tool compensation numbers in this system defaults to 99 groups, and the

effective range of compensation numbers can be set by NC parameter 000060 (number of tool

data saved by the system).

3) Tool radius compensation plane selection

Offset plane

Plane selection

G17

X_Y_

G18

X_Z_

G19

Y_Z_

The radius compensation calculation is performed on the plane determined by the G17/G18/G19

commands. The plane on which the compensation calculation is performed is called the

compensation plane. The axis coordinate values that are not in the compensation plane will not

be compensated. The projection of the tool path in each plane is compensated at the time of

simultaneous 3-axis control.

The compensation plane must be switched when radius compensation is cancelled. If the plane is

switched during compensation, the alarm "Coordinate plane cannot be switched during tool radius

compensation" will appear and the machine tool will stop.

4) Tool radius compensation amount setting

Use the D code to call the compensation amount set in the tool compensation table by specifying

the number of the tool radius compensation amount.

The D code remains valid until another D code is designated.

The change of the tool radius compensation amount is usually carried out in the G40, reset or tool

change mode.

In general, the compensation amount is positive (+). If the compensation amount is negative (-),

G41 and G42 are interchanged. If the compensation amount is positive, the tool center moves

around the outer contour of the workpiece, then if the compensation is negative, it will move

around the inner side, as shown in the figure below.

When the compensation amount is positive, the tool path is shown in Figure (1). If the

compensation amount is changed to a negative value (-), the tool path is shown in Figure (2).

Therefore, for the same program, both male and female shapes can be processed by the positive

and negative values of the compensation, and the gap between them can also be adjusted with the

compensation.

Tool center path

Example

Starting position

G92 X0 Y0 Z0； The absolute value is specified, and the tool is at the starting point

N1 G90 G17 G00 G41 D01 X25 Y25； Tool radius compensation (tool starts) starts

N2 G01 Y50 F150； Process from N2

N3 X30； Process from N3

N4 G03 X40 Y60 R10.0； Process from N3 to N4

N5 G01 X50 Y90； Process from N4

N6 G02 X90 Y90 R20； Process from N5

N7 G01 X100 Y60； Process from N6

N8 G03 X110 Y50 R10； Process from N6 to N7

N9 G1 X120； Process from N7

N10 X120 Y25； Process from N8

N11 X25 Y25； Process from N9

N12 G00 G40 X0 Y0； Cancel tool radius compensation, and tool returns to the starting

position (X0,Y0,Z0)

Note

1) The length compensation H command is ignored in the tool radius compensation, and only the

D command is valid.

2) The plane selection for tool radius compensation is specified by G command (G17/G18/G19),

and only the axes in the specified plane are compensated, the axes not in the plane are not

compensated.

12.5

Detailed Explanation of Tool Radius Compensation

12.5.1 Tool Radius Compensation Action

Function and Purpose



The process of tool radius compensation is divided into three steps: tool compensation

establishment, tool compensation in progress and tool compensation cancelation. As shown below:

Description



Tool radius compensation establishment and start

When the compensation is canceled, and the radius compensation command is used to establish

tool radius compensation, if the following compensation establishment conditions are not met,

there may occur compensation overcutting, undercutting or alarms.

(1) The establishment of tool radius compensation mode is valid only in G00/G01 traverse

command mode;

(2) The tool radius must be established on the axis where movement distance is not 0 in the

compensation plane. The compensation cannot be established when only the third axis movement

is performed; however, in special cases, the system also supports the establishment of tool

compensation with a movement amount of 0, and in order to prevent errors, it is recommended to

give a movement greater than the tool radius value when creating tool compensation.

(3) The establishment is usually performed with G01 to ensure the safety of the tool and workpiece

(4) When the sign of the compensation value changes, the compensation direction of G41/G42

will also change.When the compensation value of G41 is positive, the compensation direction is

on the left, and when the compensation value is negative, the compensation direction is on the

right. G42 is also like this.

(5) When using tangential cutting or normal cutting to establish tool compensation, if the

establishment conditions are not met, auxiliary line segments can be added to establish tool

compensation when cutting into the workpiece.

(6) The number of tool radius compensation is: 0＜D＜maximum compensation number.

(7) The establishment of tool radius compensation in circular interpolation (G02/G03) is invalid,

the system will alarm, and the machine stops moving

(8) In the process of radius compensation, G00

(rapid traverse positioning), G01

(linear

interpolation) or G02/G03 (circular interpolation) is used to realize compensation. If two or more

blocks where the tool does not move (such as auxiliary functions, pause, etc.) are executed during

radius compensation, there will occur overcutting or undercutting.

In the process of tool radius compensation

(1) When starting the radius compensation, whether it is in auto mode or single-block mode, three

traverse commands must be read in. If there is no three traverse commands, the execution will be

performed after reading up to 5 consecutive blocks.

(2) When the radius compensation is valid, the compensation plane must not be switched,

otherwise it will alarm and stop the movement.

(3) In the state of radius compensation, the linear movement of the milling cutter and the radius

for the inner circular cutting must be greater than or equal to the radius of the milling cutter,

otherwise it may cause interference and overcutting.

When tool radius compensation is cancelled

The cancellation of tool radius compensation needs to be executed in the G00 or G01 block. When

any of the following conditions is met, the system enters the radius compensation cancellation

state.

(1) When the machine is turned on, the system will initialize and restore the default tool

compensation cancellation state.

(2) After machine is reset.

(3) The tool compensation cancellation command G40 is executed.

(4) M02 and M30 commands with the reset function are executed.

(5) When the block where the tool radius compensation offset number is 0 is executed.

Example

%0001

G54G90G17G0Z50

X0Y0

M3S10000

G41G01X30Y20D01 ； Tool radius compensation is established, and register value of

No.1 tool compensation is called

Y70

X70

Y20

X30

G40G01X0Y0 ； Tool radius compensation is cancelled.

M30

Note

It is invalid when the radius compensation is cancelled by the circular command (G02/G03). If

the circular command is designated for the cancellation, an alarm will be issued and the machine

tool will stop moving.

12.5.2 Tool Radius Compensation Action Diagram

Function and Purpose



Inside and outside: When the included angle of the tool path established by two programs exceeds

180°, the path is referred to as "inside". When the included angle is between 0° and 180°, it is

referred to as "outside".

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