Content      ..     6      7      8      9     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL - page 8

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.6.6

Interference Check

Tool overcutting is called interference. The interference check

function checks for tool overcutting in advance. However, all

interference cannot be checked by this function. The interference

check is performed even if overcutting does not occur.

Explanation

- Condition under which an interference check is possible

To perform an interference check, it is necessary to read at least three

blocks with tool movement. If, therefore, three or more blocks with

tool movement cannot be read in offset mode because blocks without

tool movement, such as independent auxiliary function and dwell, are

specified in succession, excessive or insufficient cutting may occur

because an interference check fails. Assuming the number of blocks

to read in offset mode, which is determined by parameter (No. 19625),

to be N and the number of commands in those N blocks without tool

movement that have been read to be M, the condition under which an

interference check is possible is

(N - 3) ≥ M.

For example, if the maximum number of blocks to read in offset mode

is 8, an interference check is possible even if up to five blocks without

tool movement are specified. In this case, three adjacent blocks can

be checked for interference, but any subsequent interference that may

occur cannot be detected.

- Interference check method

Two interference check methods are available, direction check and

circular angle check. Parameter CNC (No. 5008#1) and parameter

CNV (No. 5008#3) are used to specify whether to enable these

methods.

Parameter

Parameter

Operation

CNV

CNC

An interference check is enabled, and a

0

0

direction check and a circular angle check can

be performed.

An interference check is enabled, and only a

0

1

circular angle check is performed.

1

-

An interference check is disabled.

NOTE

There are no settings for performing a direction

check only.

- 196 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Interference reference <1> (direction check)

Assuming the number of blocks to read during cutter compensation to

be N, a check is first performed on the compensation vector group

calculated in

(block

1 - block 2) to be output this time and the

compensation vector group calculated in (block N-1 - block N); if they

intersect, they are judged to interfere. If no interference is found, a

check is performed sequentially in the direction toward the

compensation vector group to be output this time, as follows:

(Block 1 - block 2) and (block N-2 - block N-1)

(Block 1 - block 2) and (block N-3 - block N-2)

:

:

(Block 1 - block 2) and (block 2 - block 3)

Even if multiple number of compensation vector groups are generated,

a check is performed on all pairs.

The judgment method is as follows:

For a check on the

compensation vector group in (block 1 - block 2) and those in (block

N-1 - block N), the direction vector from the specified (end point of

block 1) to the (end point of block N-1) is compared with the direction

vector from the (point resulting from adding the compensation vector

to be checked to the end of block 1) to the (point resulting from

adding the compensation vector to be checked to the end of block

N-1), and if the direction is 90^o or greater or 270^o or less, they are

judged to intersect and interfere. This is called a direction check.

Example of interference standard <1>

(If the block 1 end-point vector intersects with the block 7 end-point

vector)

The direction differs by

180°.

Tool center path

Programmed path

Block 2

Block 7

Block 1

Block 8

Block 3

Block 6

Block 4

Block 5

- 197 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

Example of interference standard <1>

(If the block 1 end-point vector intersects with the block 2 end-point

vector)

Programmed path

Tool center path

Block 1

The directions of

these two paths are

different (180°).

Block 2

- Interference reference <2> (circular angle check)

In a check on three adjacent blocks, that is, a check on the

compensation vector group calculated on (block 1 - block 2) and the

compensation vector group calculated on (block 2 - block 3), if block

2 is circular, a check is performed on the circular angle between the

start and end points of the programmed path and the circular angle of

the start and end point of the post-compensation path, in addition to

direction check <1>. If the difference is 180^o or greater, the blocks

are judged to interfere. This is called a circular angle check.

Example of <2> (if block 2 is circular and the start point of the

post-compensation arc coincide with the end point)

Tool center path

Programmed path

Block 3

Block 1

Programmed path

Block 2

- 198 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- When interference is assumed although actual interference does not occur

<1> Depression which is smaller than the cutter compensation value

Programmed

path

Tool center path

Stopped

A

C

B

There is no actual interference, but since the direction

programmed in block B is opposite to that of the path after the

cutter compensation, the tool stops and an alarm is displayed.

<2> Groove which is smaller than the cutter compensation value

Programmed

path

Tool center path

Stopped

A

B

C

Like <1>, an alarm is displayed because of the interference as the

direction is reverse in block B.

- 199 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.6.6.1 Operation to be performed if an interference is judged to

occur

The operation to be performed if an interference check judges that an

interference (due to overcutting) occurs can be either of the following

two, depending on the setting of parameter CAV (No. 19607#5).

Parameter

Function

Operation

CAV

An alarm stop occurs before the

Interference check

0

execution of the block in which

alarm function

overcutting (interference) occurs.

The tool path is changed so that

Interference check

1

overcutting (interference) does not

avoidance function

occur, and processing continues.

6.6.6.2 Interference check alarm function

- Interference other than those between adjacent three blocks

If the end-point vector of block 1 and the end-point vector of block 7

are judged to interfere as shown in the figure, an alarm will occur

before the execution of block 1 so that the tool stops. In this case,

the vectors will not be erased.

Stopped

Tool center path

Block 1

Block 8

Programmed path

Block 2

Block 7

Block 3

Block 6

Block 4

Block 5

- 200 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Interference between adjacent three blocks

If an interference is judged to occur between adjacent three blocks, the

interfering vector, as well as any vectors existing inside of it, is erased,

and a path is created to connect the remaining vectors. In the

Example shown in the figure below, V₂ and V₅ interfere, so that V₂

and V₅ are erased, so are V₃ and V₄, which are inside of them, and V₁

is connected to V₆. The operation during this time is linear

interpolation.

V₆

V₁

V₂

V₅

V₄

V₃

Tool center path

Programmed path

If, after vector erasure, the last single vector still interferes, or if there

is only one vector at the beginning and it interferes, an alarm will

occur immediately after the start of the previous block (end point for a

single block) and the tool stops. In the Example shown in the figure

below, V₂ and V₃ interfere, but, even after erasure, an alarm will occur

because the final vectors V₁ and V₄ interfere.

Stopped

Tool center path

Programmed path

V4

V1

V3

V2

- 201 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.6.6.3 Interference check avoidance function

Overview

If a command is specified which satisfies the condition under which

the interference check alarm function generates an interference alarm,

this function suppresses the generation of the interference alarm, but

causes a new compensation vector to be calculated as a path for

avoiding interference, thereby continuing machining. For the path

for avoiding interference, insufficient cutting occurs in comparison

with the programmed path. In addition, depending on the specified

figure, no path for avoiding interference can be determined or the path

for avoiding interference may be judged dangerous. In such a case,

an alarm stop will occur. For this reason, it is not always possible to

avoid interference for all commands.

- Interference avoidance method

Let us consider a case in which an interference occurs between the

compensation vector between

(block

1

- block

2) and the

compensation vector between (block N-1 - block N). The direction

vector from the end point of block 1 to the end point of block N-1 is

called a gap vector. At this time, a post-compensation intersection

vector between

(block

1 - gap vector) and a post-compensation

intersection vector between (gap vector - block N) is determined, and

a path connecting them is created.

Post-compensation intersection vector

Post-compensation intersection vector

between gap vector and block 8

between block 1 and gap vector

Movement o f block 7

Post-compensation

path

Gap vector

Block 1

Block 8

Block 2

Block 7

Programmed path

Block 3

Block 6

Block 4

Block 5

In this case, the post-compensation end points of blocks 2 to 6 coincide with the end

point of block 1. Thus, after compensation, blocks 2 to 6 will be blocks without tool

movement.

- 202 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

If the post-compensation intersection vector of (block 1 - gap vector)

and the post-compensation intersection vector of (gap vector - block

N) further intersect, vector erasure is first performed in the same way

as in "Interference between adjacent three blocks". If the last vectors

that remains still intersects, the post-compensation intersection vector

of (block 1 - block N) is re-calculated.

Post-compensation path

Re-calculation

Programmed path

Block 1

Block 8

Block 1

Block 8

Post-

Post-compensation

compensation

Post-compensation

intersection

intersection vector

intersection between

between block 1 and

vector between

gap vector and block 8

block 1 and

gap vector

block 8

Block 2

Gap vector

Block 7

Block 2

Block 7

Block 3

Block 3

Block 6

Block 6

Block 4

Block 4

Block 5

Block 5

In this case, the post-compensation end points of blocks 2 to 7

coincide with the end point of block 1. Thus, after compensation,

blocks 2 to 7 will be blocks without tool movement.

- 203 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

If the cutter compensation value is greater than the radius of the

specified arc as shown in the figure below, and a command is

specified which results in compensation with respect to the inside of

the arc, interference is avoided by performing intersection calculation

with an arc command being assumed a linear one. In this case,

avoided vectors are connected with linear interpolation.

Post-compensation path

Programmed path

- 204 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- If no interference avoidance vector exists

If the parallel pocket shown in the figure is to be machined, the

end-point vector of block 1 and the end-point vector of block 2 are

judged to interfere, and an attempt is made to calculate, as an

interference avoidance vector, the intersection vector of the

post-compensation path of block 1 and the post-compensation path of

block 3. In this case, because blocks 1 and 3 are parallel to each

other, no intersection exists. In this case, an alarm will occur

immediately before block 1 and the tool will stop.

Stopped

Tool center path

Programmed path

Block 1

Block 3

Block 2

If the circular pocket shown in the figure is to be machined, the

end-point vector of block 1 and the end-point vector of block 2 are

judged to interfere, and an attempt is made to calculate, as an

interference avoidance vector, the intersection vector of the

post-compensation path of block 1 and the post-compensation path of

block

3.

In this case, because blocks

1 and 3 are circular, no

post-compensation intersection exists. In this case, an alarm will

occur immediately before block 1 and the tool will stop, as in the

previous example.

Programmed path

Tool center path

Stopped

Block 1

Block 3

Block 2

- 205 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- If it is judged dangerous to avoid interference

If the acute-angle pocket shown in the figure is to be machined, the

end-point vector of block 1 and the end-point vector of block 2 are

judged to interfere, and an attempt is made to calculate, as an

interference avoidance vector, the intersection vector of the

post-compensation path of block 1 and the post-compensation path of

block 3. In this case, the movement direction of the post-avoidance

path extremely differs from the previously specified direction. If the

post-avoidance path extremely differs from that of the original

command (90° or greater or 270° or less), interference avoidance

operation is judged dangerous; an alarm will occur immediately before

block 1 and the tool will stop.

Post-compensation intersection of

blocks 1 and 3

Tool center path

Stopped

Programmed path

Block 1

Block 3

Block 2

If a pocket in which the bottom is wider than the top, such as that

shown in the figure, is to be machined, the end-point vector of block 1

and the end-point vector of block 2 are judged to interfere, and an

attempt is made to calculate, as an interference avoidance vector, the

intersection vector of the post-compensation path of block 1 and the

post-compensation path of block 3. In this case, the relation between

blocks 1 and 3 is judged an outer one, the post-avoidance path results

in overcutting as compared with the original command. In such a

case, interference avoidance operation is judge dangerous; an alarm

will occur immediately before block 1 and the tool will stop.

Stopped

Tool center path

Programmed path

Block 1

Block 3

Block 2

Post-compensation intersection

of blocks 1 and 3

- 206 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- If further interference with an interference avoidance vector occurs

If the pocket shown in the figure is to be machined, if the number of

blocks to read is 3, the end-point vector of block 1 and the end-point

vector of block 2 are judged to interfere, and an attempt is made to

calculate, as an interference avoidance vector, the intersection vector

of the post-compensation path of block 1 and the post-compensation

path of block 3. In this case, however, the end-point vector of block

3 that is to be calculated next further interferes with the previous

interference avoidance vector. If a further interference occurs to the

interference avoidance vector once created and output, the movement

in the block will not be performed; an alarm will occur immediately

before the block and the tool will stop.

The intersection vectors of

blocks 3 and 4 further

Tool center path

interfere.

Programmed path

Sropped

Block 5

Block 4

Block 1

Block 3

Block 2

NOTE

1 For "If it is judged dangerous to avoid interference"

and "If further interference with an interference

avoidance vector occurs", by setting parameter

NAA (No. 19607#6) appropriately, it is possible to

suppress an alarm to continue machining. For "If

no interference avoidance vector exists", however,

it is not possible to avoid an alarm regardless of the

setting of this parameter.

2 If a single block stop occurs during interference

avoidance operation, and an operation is performed

which differs from the original movement, such as

manual intervention, MDI intervention, cutter

compensation value change, intersection

calculation is performed with a new path. If such

an operation is performed, therefore, an

interference may occur again although interference

avoidance has been performed once.

- 207 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.6.7

Cutter Compensation for Input from MDI

Explanation

- MDI operation

During MDI operation, that is, if a program command is specified in

MDI mode in the reset state to make a cycle start, intersection

calculation is performed for compensation in the same way as in

memory operation/DNC operation. Compensation is performed in

the same way if a subprogram is called from program memory due to

MDI operation.

Subprogram in program memory

MDI command

G90 G00 X0 Y0 ;

O9000 ;

M98 P9000 ;

N1 G41 G17 G91 G01 X10. Y10.

M02 ;

D1 ;

N2 Y15. ;

N3 X15. ;

N4 Y-15. ;

N5 X-15. ;

N6 G40 X-10. Y-10. ;

M99 ;

N3

N2

N4

N1

N5

N6

- 208 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- MDI intervention

If MDI intervention is performed, that is, if a single block stop is

performed to enter the automatic operation stop state in the middle of

memory operation, DNC operation, and the like, and a program

command is specified in MDI mode to make a cycle start, cutter

compensation does not perform intersection calculation, retaining the

last compensation vector before the intervention.

MEM mode

MDI intervention

(G41)

G91 X30. ;

N2 G91 X10. Y30. ;

X20. Y20. ;

N3 X10. Y-30. ;

X20. Y-20. ;

N4 X40. ;

Last compensation vector

MDI intervention

Retained compensation vector

N2 N3

N4

Program command

- 209 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.7

CORNER CIRCULAR INTERPOLATION (G39)

By specifying G39 in offset mode during cutter compensation, corner

circular interpolation can be performed. The radius of the corner

circular interpolation equals the compensation value.

Format

In offset mode

G39 ;

or

I_ J_

G39

I_ K_

;

J_ K_

Explanation

- Corner circular interpolation

When the command indicated above is specified, corner circular

interpolation in which the radius equals compensation value can be

performed. G41 or G42 preceding the command determines whether

the arc is clockwise or counterclockwise. G39 is a one-shot G code.

- G39 without I, J, or K

When G39 is programmed, the arc at the corner is formed so that the

vector at the end point of the arc is perpendicular to the start point of

the next block.

- G39 with I, J, and K

When G39 is specified with I, J, and K, the arc at the corner is formed

so that the vector at the end point of the arc is perpendicular to the

vector defined by the I, J, and K values.

Limitation

- Move command

In a block containing G39, no move command can be specified.

Otherwise, an alarm will occur.

- Inner corner

In an inner corner block, G39 cannot be specified. Otherwise,

overcutting will occur.

- Corner arc velocity

If a corner arc is specified with G39 in G00 mode, the corner arc block

velocity will be that of the F command previously specified. If G39

is specified in a state in which no F command has never been specified,

the velocity of the corner arc block will be that specified with

parameter (No. 1411).

- 210 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

Example

- G39 without I, J, or K

:

:

(In offset mode)

(G90)

Y axis

N1 X10.0

;

N2 G39 ;

N3 Y-10.0 ;

:

:

X axis

Block N1

Offset vector

Block N2 (Corner arc)

(10.0, 0.0)

Block N3

Programmed path

Tool center path

(10.0, -10.0)

- G39 with I, J, and K

:

:

(In offset mode)

(G90)

Y axis

N1 X10.0 ;

N2 G39 I1.0 J-3.0 ;

N3 X0.0 Y-10.0 ;

:

X axis

:

Block N1

Tool center path

Offset vector

Block N2 (Corner

arc)

(10.0, 0.0)

Programmed

path

Block N3

(I=-1.0, J=3.0)

(0.0, -10.0)

- 211 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.8

TOOL COMPENSATION VALUES, NUMBER OF

COMPENSATION VALUES, AND ENTERING VALUES

FROM THE PROGRAM (G10)

Tool compensation values include tool geometry compensation values

and tool wear compensation (Fig. 6.8 (a)).

Reference

position

OFS_G

OFS_W

OFS_G

: Geometry compensation value

OFS_W

: Wear compensation value

Fig. 6.8 (a) Geometric compensation and wear compensation

Tool compensation values can be entered into CNC memory from the

MDI panel (see section III-1.1.1) or from a program.

A tool compensation value is selected from the CNC memory when

the corresponding code is specified after address H or D in a program.

The value is used for tool length compensation, cutter compensation,

or the tool offset.

Two types of tool compensation memories are available according to

the compensation value configuration: tool compensation memory A

and C. One of the types can be selected (bit 6 (NGW) of parameter

No.8136).

Explanation

- Tool compensation memory A (bit 6 (NGW) of parameter No.8136 = 1)

In tool compensation memory A, memory for geometry compensation

and memory for wear compensation are not distinguished from each

other. So, the sum of geometry compensation and wear compensation

values is to be set in the compensation memory. Moreover, no

distinction is made between memory for cutter compensation (for D

code) and memory for tool length compensation (for H code).

Setting example

Compensation

Compensation value

Common to D code/H code

number

(geometry+wear)

001

10.000

For D code

002

20.000

For D code

003

100.000

For H code

:

:

:

- 212 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Tool compensation memory C (bit 6 (NGW) of parameter No.8136 = 0)

In tool compensation memory C, memory for geometry compensation

and memory for wear compensation are prepared separately. So,

geometry compensation values and wear compensation values can be

set separately. Moreover, memory for cutter compensation (for D

code) and memory for tool length compensation (for H code) are

prepared separately.

Setting example

D code

H code

Compensation

For geometry

For wear

For geometry

For wear

number

compensation

compensation

compensation

compensation

001

10.000

0.100

100.000

0.100

002

20.000

0.200

200.000

0.300

:

:

:

:

:

- Unit and valid range of tool compensation values

The unit and valid range of values that can be set as a compensation

value is either of the following, depending on the bits 1 (OFC) and 0

(OFA) parameter No. 5042.

Unit and valid range of tool compensation values (metric input)

OFC

OFA

Unit

Valid range

0

1

0.01mm

±9999.99mm

0

0

0.001mm

±9999.999mm

1

0

0.0001mm

±9999.9999mm

Unit and valid range of tool compensation values (inch input)

OFC

OFA

Unit

Valid range

0

1

0.001inch

±999.999inch

0

0

0.0001inch

±999.9999inch

1

0

0.00001inch

±999.99999inch

- Number of tool compensation data items

Using the bit 5 (NDO) of parameter No. 8136 enables the total number

of items of tool compensation data to be specified as either 400 (bit 5

(NDO) of parameter No. 8136 = "0") or 32 (bit 5 (NDO) of parameter

No. 8136 = "1").

- 213 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

Format

The format for programming depends on the type of tool

compensation memory.

For tool compensation memory A

G10 L11 P_ R_ Q_ ;

P_

: Tool compensation number

R_

: Tool compensation value

Q_

: Imaginary tool nose number

For tool compensation memory C

G10 L_ P_ R_ Q_ ;

L_

: Type of compensation memory

L10 : Geometry compensation value

corresponding to an H code

L11 : Wear compensation value

corresponding to an H code

L12 : Geometry compensation value

corresponding to a D code

L13 : Wear compensation corresponding

to a D code

P_

: Tool compensation number

R_

: Tool compensation value

Q_

: Imaginary tool nose number

By specifying G10, a tool compensation value can be set or modified.

When G10 is specified by absolute input (G90), the specified value is

used as the new tool compensation value.

When incremental input (G91) is used, a specified value added to the

tool compensation value currently set is used as the new tool

compensation value.

NOTE

1 Address R follows the increment system for tool

offset values.

2 If L is omitted for compatibility with the conventional

CNC format, or L1 is specified, the same operation

as when L11 is specified is performed.

- 214 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

6.9

SCALING (G50, G51)

Overview

A programmed figure can be magnified or reduced (scaling).

Two types of scaling are available, one in which the same

magnification rate is applied to each axis and the other in which

different magnification rates are applied to different axes.

The magnification rate can be specified in the program.

Unless specified in the program, the magnification rate specified in the

parameter is applied.

Y

P₄

P

3

P₄’

P₃’

P₀

P₂’

P₁’

P₂

P₁

0

X

P₀

: Scaling center

P₁ to P₄

: Programmed figure

P₁’ to P₄’

: Scaled figure

Fig. 6.9 (a) Scaling

NOTE

To enable scaling, set bit 5 (SCL) of parameter No.

8132 to "1".

Format

Scaling up or down along all axes at the same rate of magnification

(When parameter XSC (No. 5400#6) = 0)

Format

Meaning of command

G51 IP_P_ ;

Scaling start

IP_

: Absolute command for center coordinate

Scaling is effective.

value of scaling

(Scaling mode)

P_

: Scaling magnification

G50 ;

Scaling cancel

Scaling up or down along each axes at a different rate of magnification (mirror image)

(When parameter XSC (No. 5400#6) = 1)

Format

Meaning of command

G51 IP_I_J_K_; Scaling start

IP_

: Absolute command for center coordinate

Scaling is effective.

value of scaling

(Scaling mode)

I_J_K_

: Scaling magnification for basic 3 axes (X, Y,

and Z axes) respectively

G50 ;

Scaling cancel

- 215 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

CAUTION

1 Specify G51 in a separate block.

2 After the figure is enlarged or reduced, specify G50

to cancel the scaling mode.

NOTE

1 Entering electronic calculator decimal point input

mode (bit 0 (DPI) of parameter No. 3401 = 1) does

not cause the units of the magnification rates P, I, J,

and K to change.

2 Setting the least input increment equal to 10 times

the least command increment (bit 7 (IPR) of

parameter No. 1004 = 1) does not cause the units

of the magnification rates P, I, J, and K to change.

3 An attempt to specify 0 as a magnification rate

causes alarm PS0142 to occur in a G51 block.

Explanation

- Axis for which scaling is to be enabled

For the axis for which scaling is to be enabled, set bit 0 (SCL) of

parameter No. 5401 to 1.

- Minimum unit of scaling magnification

Least input increment of scaling magnification is: 0.001 or 0.00001.

It is 0.00001 (one hundred thousandth) if bit 7 (SCR) of parameter No.

5400 is 0 and 0.001 if it is 1.

- Scaling center

Even in incremental command

(G91) mode, the scaling center

coordinates IP_ specified in the G51 block are assumed those of an

absolute position.

If the scaling center coordinates are omitted, the position assumed

when G51 is specified is assumed the scaling center.

CAUTION

With the move command subsequent to the G51

block, execute an absolute (G90 mode) position

command.

If no absolute position command is executed after

the G51 block, the position assumed when G51 is

specified is assumed the scaling center; once an

absolute position command is executed, the scaling

center assumes the coordinates specified in the

G51 block, after that block.

- 216 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Scaling along each axis at the same rate of magnification

Set bit 6 (XSC) of parameter No. 5400 to 0.

If the scaling magnification P is not specified, the magnification set in

parameter No. 5411 is used.

Decimal point input is not accepted as the magnification P. If decimal

point input is made, alarm PS0007 will occur.

A negative value cannot be specified as the magnification P. If a

negative value is specified, alarm PS0006 will occur.

The allowable magnification range is from 0.00001 to 9999.99999.

- Scaling of each axis, programmable mirror image (negative magnification)

Each axis can be scaled by different magnifications. Also when a

negative magnification is specified, a mirror image is applied. The

axis subject to the mirror image is the one that contains the scaling

center.

Set bit

6 (XSC) of parameter No. 5400to 1 to validate each axis

scaling (mirror image).

Using I, J, and K, specify the scaling magnifications for the basic 3

axes (X to Z axes). Use parameter No. 1022 to specify which axes to

use as the basic 3 axes. For those of the X to Z axes for which I, J,

and K are not specified and for axes other than the basic 3 axes, the

magnification set with parameter No. 5421 is used.

A value other than 0 must be set to parameter No. 5421.

Decimal point programming can not be used to specify the rate of

magnification (I, J, K).

Magnification can be set within the range of

±0.00001 to

±9999.99999.

a/b

: Scaling magnification of X axis

c/d

: Scaling magnification of Y axis

o

: Scaling center

Y axis

Programmed figure

d

Scaled figure

c

o

X axis

a

b

Fig. 6.9 (b) Scaling of each axis

- 217 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Scaling of circular interpolation

Even if different magnifications are applied to each axis in circular

interpolation, the tool will not trace an ellipse.

G90 G00 X0.0 Y100.0 Z0.0;

G51 X0.0 Y0.0 Z0.0 I2000 J1000;

(A magnification of 2 is applied to the X-component and a

magnification of 1 is applied to the Y-component.)

G02 X100.0 Y0.0 I0 J-100.0 F500;

Above commands are equivalent to the following command:

G90 G00 X0.0 Y100.0 Z0.0;

G02 X200.0 Y0.0 I0 J-100.0 F500;

(Because the end point is not on an arc, spiral interpolation is

assumed.)

Y

Scaled shape

X

(0,0)

(100.0)

(200.0)

Fig. 6.9 (c) Scaling for circular interpolation1

Even for an R-specified arc, scaling is applied to each of I, J, and K

after the radius value (R) is converted into a vector in the center

direction of each axis.

If, therefore, the above G02 block contains the following R-specified

arc, the operation will be same as that in which I and J are specified.

G02 X100.0 Y0.0 R100.0 F500 ;

- 219 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

- Scaling and coordinate system rotation

If both scaling and coordinate system rotation are specified at the

same time, scaling is performed first, followed by coordinate system

rotation. In this case, scaling is effective to the rotation center as

well.

To specify both of them, specify scaling first and then coordinate

system rotation. To cancel them, specify them in the reverse order.

Example

Main program

O1

G90 G00 X20.0 Y10.0 ;

M98 P1000 ;

G51 X20.0 Y10.0 I3000 J2000 ; (x 3 in the X direction and x 2

in the Y direction)

M98 P1000 ;

G17 G68 X35.0 Y20.0 R30. ;

M98 P1000 ;

G69 ;

G50 ;

M30 ;

Subprogram

O1000 ;

G01 X20.0 Y10.0 F500 ;

G01 X50.0 ;

G01 Y30.0 ;

G01 X20.0 ;

G01 Y10.0 ;

M99 ;

Y

Rotation center

of coordinate

system before

scaling

Rotation center of

coordinate system

after scaling

Original program

X

Shape after

coordinate system

Scaling center

rotation

Scaled shape

Fig. 6.9 (d) Scaling and coordinate system rotation

- 220 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

- Scaling and optional chamfering/corner R

Chamfering

Scaling

x 2 in the X direction

x 1 in the Y direction

Corner R

Scaling

x 2 in the X direction

x 1 in the Y direction

If different magnifications are applied to the individual axes, corner R results in

a spiral, not an arc, because scaling is applied to the end point and radius of

the arc.

Fig. 6.9 (e) Scaling and optional chamfering/corner R

Limitation

- Tool compensation

This scaling is not applicable to cutter compensation values, tool

length compensation values, and tool offset values (Fig. 6.9 (f) ).

Programmed figure

Scaled figure

Cutter compensation values are not scaled.

Fig. 6.9 (f) Scaling during cutter compensation

- 221 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

Example

Sample program of a scaling in each axis

O1;

G51 X20.0 Y10.0 I750 J250; (× 0.75 in the X direction, × 0.25 in

the Y direction)

G00 G90 X60.0 Y50.0;

G01 X120.0 F100;

G01 Y90;

G01 X60;

G01 Y50;

G50;

M30;

Y axis

90

Programmed figure

80

(60,50)

Scaled figure

30

20

10

Scaling center

X axis

75

100

20

95

120

Fig. 6.9 (g) Program example of scaling in each axis

- 223 -

6.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-2/01

6.10 COORDINATE SYSTEM ROTATION (G68, G69)

A programmed shape can be rotated. By using this function it

becomes possible, for example, to modify a program using a rotation

command when a workpiece has been placed with some angle rotated

from the programmed position on the machine. Further, when there is

a pattern comprising some identical shapes in the positions rotated

from a shape, the time required for programming and the length of the

program can be reduced by preparing a subprogram of the shape and

calling it after rotation.

Y

Angle of rotation

Center of rotation

X

0

Fig. 6.10 (a) Coordinate system rotation

Format

Format

G17







Start rotation of a coordinate system.



G18



G68 α_β_ R_ ;





G19





:

Coordinate system rotation mode

(The coordinate system is rotated.)

G69 ;

Coordinate system rotation cancel command

Meaning of command

G17 (G18 or G19) :

Select the plane in which contains the figure

to be rotated.

α_β_ Absolute programming for two of the X_, Y_, and Z_ axes that

correspond to the current plane selected by a command (G17,

G18, or G19). The command specifies the coordinates of the

center of rotation for the values specified subsequent to G68

R_

Angular displacement with a positive value indicates counter

clockwise rotation. Parameter RIN (No. 5400#0) selects

whether the specified angular displacement is always

considered an absolute value or is considered an absolute or

incremental value depending on the specified G code (G90 or

G91).

Least input increment :

0.001 deg

Valid data range :

-360,000 to 360,000

- 224 -

B-64304EN-2/01

PROGRAMMING

6.COMPENSATION FUNCTION

Y

Angle of rotation R (incremental value)

Center of

Angle of rotation (absolute value)

rotation

(α, β)

X

Fig. 6.10 (b) Coordinate system rotation

NOTE

When a decimal fraction is used to specify angular

displacement (R_), the 1's digit corresponds to

degree units.

Explanation

- G code for selecting a plane: G17,G18 or G19

The G code for selecting a plane (G17,G18,or G19) can be specified

before the block containing the G code for coordinate system rotation

(G68). G17, G18 or G19 must not be designated in the mode of

coordinate system rotation.

- Incremental programming in coordinate system rotation mode

The center of rotation for an incremental programming programmed

after G68 but before an absolute programming is the tool position

when G68 was programmed (Fig. 6.11 (c)).

- Center of rotation

When α_β_ is not programmed, the tool position when G68 was

programmed is assumed as the center of rotation.

- Angular displacement

When R_ is not specified, the value specified in parameter No. 5410 is

assumed as the angular displacement.

To specify angular displacement

(R_) in

0.00001 degrees

(one

hundred-thousandth), set parameter FRD (No. 11630#0) to 1. In this

case, angular displacement R is specified within the range of

-36000000 to 36000000.

- Coordinate system rotation cancel command

The G code used to cancel coordinate system rotation (G69) may be

specified in a block in which another command is specified.

- Tool compensation

Cutter compensation, tool length compensation, tool offset, and other

compensation operations are executed after the coordinate system is

rotated.

- 225 -

Content      ..     6      7      8      9     ..