HNC-818. User Manual

9. Coordinate Values and Dimension Unit

9.1 Absolute Commands and Incremental Commands (G90, G91)

There are two methods to specify tool movement: absolute commands

and incremental commands:

y Absolute commands are used to create programs for the tool

movement end point coordinates.

y Incremental command is used to create programs for the amount of

tool movement.

Format

y Milling Machines

Absolute command G90 IP_;

Incremental command G91 IP_;

y Turning Machines (two formats):

First: Absolute command G90 IP_;

Incremental command G91 IP_;

Second: UVW incremental programming

When UVW is not defined as a coordinate axis and the channel

parameter Enable Programming with UVW (040033) is set

to 1, you may use UVW to present the incremental value of

XYZ.

Description

It can simplify programming by selecting a proper programming mode.

When the blueprint dimension is based on a fixed point, it is

recommended to use the absolute programming. When the blueprint

dimension is based on the distance between contour vertexes, it is

recommended to use the incremental programming.

9. Coordinate Values and Dimension Unit

Milling machines

G90 X40.0 Y70.0;

Absolute command

G91 X-60.0 Y40.0;

Incremental command

End point

70.0

Example

30.0

Start point

40.0

100.0

Turning machines

The tool moves from P to Q (X axis indicates the diameter value

commands).

Absolute command: G90X400Z50

Incremental command: G91X200Z-400 or U200W-400

X Q (400, 50)

P (200, 450)

ĭ400

ĭ200

ĭ450

9. Coordinate Values and Dimension Unit

9.2 Dimension Unit Selection (G20, G21)

You may select dimension unit with G20/G21.

Format

G20

Inch input mode

G21

Metric input mode

Description

G Code

Linear Axis

Rotation Axis

Inch input (G20)

inch

Degree (deg)

Metric input (G21)

Millimeter (mm)

Degree (deg)

Attention

G20 and G21 are modal functions, which can be canceled by each

other. G21 is the default value after power on.

The unit of the data input for G codes has nothing to do with the

unit of the data displayed on the HMI interface. G20/21 is used to

select the unit of the data input for G codes, but cannot change the

data unit displayed on the HMI interface. The NC parameter SIZE

METRIC/INCH (000025) is used to set the coordinate data unit

displayed on the interface.

Example

%0007

G54

G01 x10y10z10

G20

x2y2z2

M30

9. Coordinate Values and Dimension Unit

9.3 Polar Coordinate Programming (M) (G16, G15)

For G code programming, it is more convenient and faster to create

programs by entering the coordinate values of the end point at the polar

coordinate system of the radius and angle.

From the positive direction of the first axis in the specified polar

coordinate plane, the angle in the CCW direction is positive, and the

angle in the CW direction is negative.

The absolute command and incremental command (G90, G91) can be

used to specify radius and angle.

Format

XY plane: The X axis specifies the polar radius

Define the

G17

while the Y axis specifies the polar angle.

plane of the

ZX plane: The Z axis specifies the polar radius

polar

G18

while the X axis specifies the polar angle.

coordinate

YZ plane: The Y axis specifies the polar radius

system

G19

while the Z axis specifies the polar angle

Define the

Specify the workpiece coordinate system origin

origin of the

G90

as the origin of the polar coordinate system,

polar

and measure radius from this point.

coordinate

Specify the current point as the origin of the

system

G91

polar coordinate system, and measure radius

from this point.

G16

Start of the polar coordinate programming

command

G15

End of the polar coordinate programming

command

Set origin of polar coordinate

system

There are two methods to set the origin of the polar coordinate system:

Specify the workpiece coordinate system zero point as the origin of

the polar coordinate system

Specify the radius with absolute value.

Specify the workpiece coordinate system origin as the origin of

the polar coordinate system.

When using the local coordinate system (G52), the origin of the

9. Coordinate Values and Dimension Unit

local coordinate system is the

origin of the polar coordinate

system.

Command position

Radius

Actual position

Angle

Origin of workpiece coordinate system

a) When the angle is specified with an

b) When the angle is specified

absolute command

with an incremental command

Specify the actual position as the origin of the polar coordinate

system

Specify the radius with incremental value.

Specify the actual position as the origin of the polar coordinate

system.

Command position

Angle

Actual position

Origin of workpiece coordinate system

a) When the angle is specified with an

b) When the angle is specified

absolute command

with an incremental command

Attention

The axis command with the following commands will not be

regarded as polar coordinate command:

y Pause G04

y Programmable data input G10

y Local coordinate system G52

y Change workpiece coordinate system G92

y Machine coordinate system selection G53

9. Coordinate Values and Dimension Unit

y Coordinate rotation G68

y Scaling G51

In the polar coordinate system, any degrees of angle/convex corner

R cannot be specified.

In the polar coordinate system, you cannot use fixed cycle G

commands.

For polar coordinate programming, when specifying the radius with

absolute values, set the workpiece coordinate system origin as the

polar coordinate system origin; when specifying the radius with

incremental values, set the actual position as the polar coordinate

system origin. However, if only angle is specified in the command,

set the workpiece coordinate system origin as the polar coordinate

system origin both in absolute mode and incremental mode.

Examples

Use absolute commands to specify the radius and angle

%1000;

G54

G00 X0Y0Z0

G17 G90 G16;

G01 X100.0 Y30.0F1500

Y150.0;

Y270.0;

G15

M30

Use absolute command to specify

the

radius

and

incremental

command to specify the angle

%1000

G54

G00 X0Y0Z0

G17 G90 G16;

G01 X100.0 Y30.0F1500

G91Y120.0;

Y120.0;

9. Coordinate Values and Dimension Unit

9.4 Diameter and Radius Programming (T) (G36, G37)

Format

G36; Diameter programming

G37; Radius programming

Description

The shape of the workpiece to be processed in a turning machine is

usually a rotating piece, and its X axis dimension can be specified in two

ways: diameter and radius modes. G36, the default value, indicates the

diameter programming.

Attention

The Z-axis command input has nothing to do with the diameter or

radius programming.

When G02 or G03 is specified, the parameter values of R, I, K are

radius values.

In single fixed rotation, the parameter R used as the tool feed along

the X axis indicates the radius value.

For turning machines or machining center, the default mode is the

diameter programming (G36).

Specify the axial feed rate based on the change of radius.

Example

254

160

10. Tool Compensation Functions

10.1 Tool Offset (T)

The programming path is the motion path of the tool nose. However, in

real machining, the geometry dimensions and installation positions of

different tools are different; therefore, the relative position of the tool

nose to the center of the turret is different. You need to measure and set

the tool nose position, so that the system may conduct tool offset

compensation during the machining. When programming, you do not

need to take into account the tool nose position difference caused by tool

shape and installation position.

Tool dimension error may be caused by tool wear after a period of usage;

therefore the compensation is required. The compensation and tool offset

compensation are stored in the same register address number. The tool

wear compensation of a tool is only valid for the tool (including the

standard tool).

10.1.1 T Command for Tool Offset

The tool compensation is specified by T commands, and the four digits

after T express selected tool number and tool offset compensation (for

details, see section 4.3).

The description of T command is as follows:

Tool geometry offset

number

Tool number

The tool offset number is the address number of the tool offset

compensation register which stores the tool offset compensation values

and tool wear compensation value of X axis and Z axis.

T plus compensation number starts the offset compensation feature. The

offset number 00 expresses the offset is 0. In this case, the offset feature

101

10. Tool Compensation Functions

is canceled.

The tool geometry offset number and tool number may be the same or

different. In other words, multiple tool offset numbers

(value) may

correspond to one tool.

Example

N1 G00X100Z140

N2 T0313 (select No. 3 tool and the tool offset of No. 13 tool)

N3 X200Z150

As shown in the figure below, if there is compensation value for the tool

path (relative to the programming path) in the X, Z axis (the vector of the

compensation in the X, Z direction is referred to as compensation vector),

the position of the end point in the program segment plus or minus

compensation amount

(compensation vector) is the end position

specified by the T command.

Compensation path

Compensation vector

(components in X and Z

axis directions）

Programming path

Program block containing T

commands

10.1.2 Tool Offset Compensation and Tool Wear Compensation

The programming path of the turning machine is actually the movement

path of the tool nose. But in the actual situation, the geometry dimension

and installation position of different tools are different, and the relative

position of the tool nose to the center of the turret is different. Hence,

you need to measure and define the tool nose position of each tool, so

that the system may conduct tool offset compensation during the

processing. This way, you do not need to take account of the tool nose

position difference caused by the difference of tool shape and installation

position in programming.

102

10. Tool Compensation Functions

Machine origin

No. 1 tool Z

Absolute Compensation Mode

axis offset

Z₁

No. 2 tool Z

axis offset

Z₂

2/2

X₁/2

No. 2 tool X

Workpiece origin

axis offset

The absolute tool offset indicates the orientation distance from the tool

nose of each tool on the turret to the workpiece zero when the machine

returns to the machine zero. When executing tool offset compensation,

the processing coordinate system of each tool is defined based on the

distance. This way, when the turret is at the machine zero, even the tool

dimension and the distance from the tool position to the workpiece zero

are different, the defined coordinate system of each tool is coincide with

the workpiece coordinate system (programmed).

Example

As shown in the figure below, set tool offset wear compensation, and

then cancel the tool offset wear compensation:

100

T0202

Tool compensation path

G01 X50 Z100

Z200

X100 Z250 T0200

Programming path

M30

100

200

250

103

10. Tool Compensation Functions

10.2

Tool Nose Radius Compensation (T) (G40, G41, G42)

The CNC program is generally created based on the dimension of the

workpiece for a point that is on the cutting tools (cutter location point),

which is generally the imaginary tool nose

(point A) under ideal

conditions or the center point of the tool nose circle (O). But in the actual

processing, the tool nose may not be a point but an arc because of the

processing craft or other requirements. During cutting, the cutting point

changes on the arc. This way, there may be deviation between the actual

cutting position and the cutter location point, and thereby causing

excessive or less cutting. The processing error, caused because that the

tool nose is not an ideal point but one arc, can be eliminated by the nose

radius compensation function.

Tool nose

Tool path without compensation

Tool path with compensation

Workpiece

Cutting depth without tool nose radius compensation

Attention

Radius compensation does not support interruption command such as

G31.

10.2.1 Imaginary Tool Nose

As shown in the figure below, the imaginary tool nose point (A) does not

exist. It is more difficult to set the radius center of actual tool nose at the

start point than to set the imaginary tool nose at the start point. Hence,

the imaginary is necessary.

When using the imaginary tool nose, you do not need to consider the

radius of tool nose during programming.

When the tool is set at the start point, the position is as below:

104

10. Tool Compensation Functions

Start point

Programming based on the

tool nose center

imaginary tool nose

Description

The tool nose arc radius compensation function can be used to add or

cancel radius compensation, which is specified with the G41/G42/G40

and too nose radius compensation number specified by T.

Format

G Code

Workpiece Position

Tool Path

G40

Canceling tool nose

Move along the tool path

radius compensation

G41

Left tool compensation

Compensation at the left side of

the tool movement direction

G42

Right tool

Compensation at the right side

compensation

of the tool movement direction

See the figure below:

G42: tool on the right of its

movement direction

G41:too on the left of its

movement direction

105

10. Tool Compensation Functions

10.2.2 Define Tool Nose Direction

The direction number of cutting tool nose defines the relationship

between the cutter location point and tool nose center. There are ten

directions ranging from 0 to 9. See the figure below:

Back tool turret

"Ɣ": Cutter location point A, "+": Tool nose circle center O

Front tool turret

"Ɣ": Cutter location point A, "+": Tool nose circle center O

106

10. Tool Compensation Functions

Attention

G40, G41, and G42 are modal codes, which can be canceled by

each other.

G41/G42 is not followed by any parameters, and its compensation

number

(indicating the tool nose radius compensation

corresponding to the tool) is specified by T commands. The tool

nose arc compensation number corresponds to the tool offset

compensation number.

The command used to establish or cancel the tool radius

compensation can be only G00 or G01, but cannot be G02 or G03.

Tool Offset Transition

The program block changing from G40 to G41 or G42 is called the

program of tool offset transition.

G40_;

G41_; (starting cutting)

The tool offset transition movement is performed in this program block.

In the start point of the next program block after it, the tool nose center is

located in the vertical line of the programming path.

G40

G42

Workpiece

G42 (Start)

The program block changing from G41 or G42 to G40 is called the offset

Cancel Offset

cancelation program.

G41_;

G40_; (offset cancelation program)

In the program block prior to the offset cancelation program, the tool

nose center moves to the position vertical to the programming path. The

tool is located at the end point of the offset cancelation program. See the

figure below:

107

10. Tool Compensation Functions

End point

G40

G42

Workpiece

Example

Create a program for the workpiece machining as shown in the figure

below (considering the tool radius compensation):

R15

%3323

N1 T0101 (change to the No. 1 tool and set the coordinate system)

N2 M03 S400 (CW rotate spindle at 400r/min)

N3 G00 X40 Z5 (move to the program start point)

N4 G00 X0 (the tool moves to the workpiece center)

N5 G01 G42 Z0 F60 (add tool radius compensation, and move to the

workpiece position)

N6 G03 U24 W-24 R15 (process the R15 arc segment)

N7 G02 X26 Z-31 R5 (process the R5 arc segment)

N8 G01 Z-40 (process the ĭ26 external circle)

N9 G00 X30 (exit the processed surface)

N10 G40 X40 Z5 (cancel the radius compensation, and return to

108

10. Tool Compensation Functions

10.2.3 Usage of Tool Radius Compensation

Tool nose radius compensation of

Movement path in the direction of the imaginary tool

inner/outer diameter cutting cycle

The tool movement path direction is generally parallel to the

(G80) or end-face cutting cycle

programming path. The figure below shows the paths with tool nose

(G81)

radius compensation in nine tool nose directions:

G80 tool path center

Start point

Programming path

G81 tool path center

Start point

Programming path

Offset direction

G80

110

10. Tool Compensation Functions

G81

Tool nose radius compensation of

When you specify the following cutting cycle, the tool offset will be a

cutting cycle

tool nose radius compensation vector, without intersection calculation

during the cycle.

Note: The establishment and cancelation of radius compensation must be

between the P/Q segments of the combined cycle.

y G71 Inner (outer) diameter rough-turning compound cycle

y G72 End-face rough-turning compound cycle

y G73 Closed turning compound cycle

Tool nose radius compensation of

The figure below shows the compensation motion:

chamfer

(G42)

Programming path

(G41)

111

10. Tool Compensation Functions

10.3 Introduction to Tool Radius Compensation (M) (G40, G41, G42)

Attention

Radius compensation does not support interruption command such as

G31.

In the program block between G41/G42 and G40, G0 automatically

changes to G01.

10.3.1 Tool Radius Compensation for Milling Machines

During programming, only the tool center path is generally programmed

(the tool radius is assumed as 0). However, in the actual machining, you

need to conduct offset for the tool center path because the tool radius is

not zero (The offset distance equals to the tool radius and the offset

direction may be left or right based on the actual programming). In this

case, tool radius compensation function is required.

Format

G17 (or G18/G19) G41 (or G42) G00 (or G01) IP_ D_;

Attention

Tool radius compensation does not support radius change.

Tool radius compensation does not support the status change of

G41/G42.

Establish Tool Compensation

G17/G18/G19: Define the compensation plane, XY, YZ, ZX plane

respectively

G41/G42: Tool radius compensation is valid. G41: left compensation.

G42: Right compensation.

D: Define the tool radius compensation number.

Cancel Tool Radius Compensation

G40 IP_;

G40: Cancel tool radius compensation (G40, G41, G42 are modal codes,

which can be canceled by each other.)

IP_: The command value of axis movement

113

10. Tool Compensation Functions

The tool radius compensation function is defined by G41or G42.

G41: Conduct left offset along the tool movement (see a)

Offset Direction

G42: Conduct right offset along the tool movement (see b)

Tool compensation path

Programming

path

a: left tool

b: right tool

compensation

10.3.2 Establish or Cancel Tool Compensation

Establish or cancel radius compensation through G00 or G01.

If the arc interpolation commands (G02, G03) are used to establish or

cancel the tool compensation, an alarm will be reported.

10.3.3 Define Tool Radius Compensation Amount

You may use the D codes to set the tool radius compensation amount by

defining the number of tool radius compensation amount.

The D code is valid until another D code is defined.

Attention

The change of tool radius compensation amount is generally conducted

during tool change when the tool compensation is canceled.

10.3.4 Plane Selection and Vector

114

10. Tool Compensation Functions

The offset calculation is based on the

plane defined by G17, G18, and G19.

The plane for offset calculation is

called the offset plane.

The coordinate value on the axis

outside the offset plane is not

Change the offset plane in the offset cancelation mode. An alarm will be

affected by the offset, and can be

reported and the tool stops if the offset plane is changed in the offset

used as originally.

the

mode.

simultaneous 3-axis control, the tool

moves in the offset mode based on

the shape

projected

the

offset

P₃’

plane.

P₃

P₅

P₄

P₄’

P₂

P₂’

Example

P₀

P₀’

P₁’’

P₁’

%0504

N01 G92 X0 Y0

N02 G0 X-40 Y-26.66

N03 G90 G41 G0 X0 Y0 D3

N04 G1 X-20 Y30 F2000

N05 G1 X43.135529 Y156.271057

N06 G2 X175.554 Y73.70 R80

N07 G1 X20 Y-30

N08 G1 X0 Y0

N09 G40 G0 X-40 Y-26.66

N10 M30

115

10. Tool Compensation Functions

10.4 Description of Tool Radius Compensation (M) (G40, G41, G42)

10.4.1 Tool Movement during Tool Start

The figure below shows the tool movement when the mode is changed

from the offset cancelation into the offset mode:

Tool movement around the inner

corner

Linearĺ Linear

(Į180 degrees)

Workpiece

Programming path

G42

Start point

Tool center path

Linear ĺ Circular

Workpiece

G42

Start point

Tool center path

Programming path

117

10. Tool Compensation Functions

Tool movement around the outer

Linear ĺ Linear

corner

Start point

(90 degrees Į<180 degrees)

G42

Workpiece

Programming path

Intersection point

Tool center path

Linear ĺ Circular

Start point

G42

Workpiece

Intersection point

Tool center path

Programming path

Tool movement around the outer

Linear ĺ Linear

corner

Start point

(Į<90 degrees)

G42

Workpiece

Programming path

Tool center path

118

10. Tool Compensation Functions

Linear ĺ Circular

Start point

G42

Workpiece

Tool center path

Programming path

10.4.2 Tool Movement in Offset

Tool movement around the inner

Linear ĺ Linear

corner

Workpiece

(Į180 degrees)

Programming path

Tool center path

Intersection point

Linear ĺ Circular

Start point

Workpiece

Intersection

point

Tool center path

Programming path

119

10. Tool Compensation Functions

Circular ĺ Linear

Workpiece

Programming path

Intersection

Tool center path

point

Circular ĺ Circular

Workpiece

Intersection

point

Programming path

Tool center path

Tool movement around the outer

Linear ĺ Linear

corner

(90 degrees Į<180 degrees)

Workpiece

Programming path

Intersection point

Tool center path

120

HNC-818. User Manual - page 4