Content      ..     7      8      9      10     ..

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL - page 9

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

5.3.5

Prevention of Overcutting Due to Tool Nose Radius

Compensation

Explanation

- Machining a groove smaller than the diameter of the tool nose

Since the tool nose radius compensation forces the path of the center

of the tool nose radius to move in the reverse of the programmed

direction, overcutting will result. In this case an alarm is displayed and

the CNC stops at the start of the block.

Tool nose radius

An alarm is displayed and

center path

the operation stops

Programmed path

Workpiece

Overcutting if the operation would not stop

Fig. 5.3.5 (a) Machining a groove smaller than the diameter of the tool

nose

- 224 -

B-64304EN-1/01

PROGRAMMING

5.COMPENSATION FUNCTION

- Machining a step smaller than the tool nose radius

For a figure in which a workpiece step is specified with an arc, the

tool nose radius center path will be as shown in Fig. 5.3.5 (b). If the

step is smaller than the tool nose radius, the tool nose radius center

path usually compensated as shown in Fig. 5.3.5 (c) may be in the

direction opposite to the programmed path. In this case, the first

vector is ignored, and the tool moves linearly to the second vector

position. The single block operation is stopped at this point. If the

machining is not in the single block mode, the cycle operation is

continued.

If the step is of linear, no alarm will be generated and cut correctly.

However uncut part will remain.

Single block stop point

S

Tool nose radius

center path

Programmed path

S

Arc center

Workpiece

Fig. 5.3.5 (b) Machining a step larger than the tool nose radius

Single block stop point

Linear movement

S

Tool nose radius center path

Path to be taken if

the

Programmed path

vector is not ignored

The first vector is ignored

Arc center

Arc

Workpiece

An overcutting will result if the first vector is not ignored.

However, tool moves linearly.

Fig. 5.3.5 (c) Machining a step smaller than the tool nose radius

- 225 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

- Starting compensation and cutting along the Z-axis

It is usually used such a method that the tool is moved along the Z

axis after the tool nose radius compensation (normally XY plane) is

effected at some distance from the workpiece at the start of the

machining. In the case above, if it is desired to divide the motion

along the Z axis into rapid traverse and cutting feed, follow the

procedure below.

Let us consider the following program, assuming the number of blocks

to read in tool nose radius compensation mode

(parameter

(No.

19625)) to be 3.

N1 G00 G41 U500.0 V500.0 T0101 ;

N3 G01 W-300.0 F100 ;

N6 V1000.0 F200 ;

After compensation

N6

N3:Move command in Z axis (one block)

N1

In the program example above, when executing block N1, blocks N3

and N6 are also entered into the buffer storage, and by the relationship

among them the correct compensation is performed as in the figure

above.

Then, suppose that the block N3 (move command in Z axis) is divided

into N3 and N5.

N1 G00 G41 U500.0 V500.0 T0101 ;

N3 G01 W-250.0 ;

N5 G01 W-50.0 F100 ;

N6 V1000.0 F200 ;

After compensation

Workpiece

N6

N3, N5:Move command for the Z axis (two blocks)

N1

At this time, because the number of blocks to read is 3, blocks up to

N5 can be read at the start of N1 compensation, but block N6 cannot

be read. As a result, compensation is performed only on the basis of

the information in block N1, and a vertical vector is created at the end

of the compensation start block. Usually, therefore, overcutting will

result as shown in the figure above.

- 226 -

B-64304EN-1/01

PROGRAMMING

5.COMPENSATION FUNCTION

In such a case, it is possible to prevent overcutting by specifying a

command with the exactly the same direction as the advance direction

immediately before movement along the Z axis beforehand, after the

tool is moved along the Z axis using the above rule.

N1 G00 G41 U500.0 V400.0 T0101 ;

N2 V100.0 ;

N3 W-250.0 ;

N5 G01 W-50.0 F100 ;

N6 V1000.0 F200 ;

After compensation

N6

Workpiece

N3, N5 : Move command for the Z axis (2 blocks)

N2

N1

As the block N2 has the move command in the same direction as that

of the block N6, the correct compensation is performed.

Alternatively, it is possible to prevent overcutting in the same way by

specifying an IJ type vector with the same direction as the advance

direction in the start-up block, as in N1 G00 G41 U500.0 V500.0 I0 J1

T0101;, after the tool has moved along the Z axis.

- 227 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

5.3.6

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.

CNV

CNC

Operation

0

0

An interference check is enabled, and a direction check

and a circular angle check can be performed.

0

1

An interference check is enabled, and only a circular

angle check is performed.

1

-

An interference check is disabled.

NOTE

There are no settings for performing a direction

check only.

- 228 -

B-64304EN-1/01

PROGRAMMING

5.COMPENSATION FUNCTION

- Interference reference <1> (direction check)

Assuming the number of blocks to read during tool nose radius

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

- 229 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

Example of interference standard <1>

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

vector)

Tool nose radius

Programmed path

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 nose radius

Programmed path

center path

Block 3

Block 1

Programmed path

Block 2

- 230 -

B-64304EN-1/01

PROGRAMMING

5.COMPENSATION FUNCTION

- When interference is assumed although actual interference does not occur

<1> Depression which is smaller than the tool nose radius

compensation value

Programmed

path

Tool nose radius 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

tool nose radius compensation, the tool stops and an alarm is

displayed.

<2> Groove which is smaller than the tool nose radius compensation

value

Programmed

path

Tool nose radius center path

Stopped

A

B

C

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

direction is reverse in block B.

- 231 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

5.3.6.1 Operation to be performed if an interference is judged to

occur

Explanation

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).

CAV

Function

Operation

An alarm stop occurs before the execution

Interference check

0

of the block in which overcutting

alarm function

(interference) occurs.

The tool path is changed so that

Interference check

1

overcutting (interference) does not occur,

avoidance function

and processing continues.

5.3.6.2 Interference check alarm function

Explanation

- 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 nose radius

center path

Block 1

Block 8

Programmed path

Block 2

Block 7

Block 3

Block 6

Block 4

Block 5

- 232 -

B-64304EN-1/01

PROGRAMMING

5.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

- 233 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

5.3.6.3 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.

Explanation

- 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.

- 234 -

B-64304EN-1/01

PROGRAMMING

5.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 vector

intersection

intersection between

vector between

between block 1

gap vector and block 8

and gap vector

block 1 and

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.

- 235 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

If the tool nose radius 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

- 236 -

B-64304EN-1/01

PROGRAMMING

5.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

- 237 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

- 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

- 238 -

B-64304EN-1/01

PROGRAMMING

5.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, tool nose

radius 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.

- 239 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

5.3.7

Tool Nose Radius 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.

MDI command

Subprogram in program memory

G00 X0 Y0 ;

O9000 ;

M98 P9000 ;

N1 G41 G17 G01 U10.0 V10.0

M02 ;

T0101 ;

N2 V15.0 ;

N3 U15.0 ;

N4 V-15.0 ;

N5 U-15.0 ;

N6 G40 U-10.0 V-10.0 ;

M99 ;

N3

N2

N4

N1

N5

N6

- 240 -

B-64304EN-1/01

PROGRAMMING

5.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, tool nose

radius compensation does not perform intersection calculation,

retaining the last compensation vector before the intervention.

MEM mode

MDI intervention

(G41)

W30.0 ;

N2 U30.0 W10.0 ;

U20.0 W20.0 ;

N3 U-30.0 W10.0 ;

U-20.0 W20.0 ;

N4 W40.0 ;

Last compensation vector

MDI intervention

Retained compensation vector

N2 N3

N4

Program command

- 241 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

5.4

CORNER CIRCULAR INTERPOLATION (G39)

By specifying G39 in offset mode during tool nose radius

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.

- 242 -

B-64304EN-1/01

PROGRAMMING

5.COMPENSATION FUNCTION

Example

- G39 without I, J, or K

:

:

(In offset mode)

N1 Z10.0

;

X axis

N2 G39 ;

N3 X-10.0 ;

:

:

Z axis

Block N1

Offset vector

Block N2 (Corner arc)

(10.0, 0.0)

Block N3

Programmed path

Tool nose radius

center path

(10.0, -10.0)

- G39 with I, J, and K

:

:

(In offset mode)

N1 Z10.0

;

X axis

N2 G39 I-1.0 K2.0 ;

N3 X-10.0 Z20.0 ;

:

:

Z axis

Block N2 (Corner arc)

Block N1

Offset vector

Block N3

Programmed

path

(10.0, 0.0)

(I=-1.0, K=2.0)

Tool nose radius

center path

(20.0, -10.0)

- 243 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

5.5

AUTOMATIC TOOL OFFSET (G36, G37)

When a tool is moved to the measurement position by execution of a

command given to the CNC, the CNC automatically measures the

difference between the current coordinate value and the coordinate

value of the command measurement position and uses it as the offset

value for the tool. When the tool has been already offset, it is moved

to the measurement position with that offset value. If the CNC judges

that further offset is needed after calculating the difference between

the coordinate values of the measurement position and the

commanded coordinate values, the current offset value is further

offset.

Refer to the instruction manuals of the machine tool builder for

details.

NOTE

To use automatic tool offset, set bit 7 (IGA) of

parameter No. 6240 to 0.

Explanation

- Coordinate system

When moving the tool to a position for measurement, the coordinate

system must be set in advance. (The workpiece coordinate system for

programming is used in common.)

- Movement to measurement position

A movement to a measurement position is performed by specifying as

follows in the MDI, or MEM mode :

G36 Xxa ; or G37 Zza ;

In this case, the measurement position should be xa or za (absolute

programming).

Execution of this command moves the tool at the rapid traverse rate

toward the measurement position, lowers the feedrate halfway, then

continues to move it until the approach end signal from the measuring

instrument is issued.

When the tool tip reaches the measurement position, the measuring

instrument outputs the measurement position reach signal to the CNC

which stops the tool.

- Offset

The current tool offset value is further offset by the difference

between the coordinate value (α or β) when the tool has reached the

measurement position and the value of xa or za specified in G36Xxa

or G37Zza.

Offset value x = Current offset value x+(α-xa)

Offset value z = Current offset value z+(β-za)

xa : Programmed X-axis measurement point

za : Programmed Z-axis measurement point

These offset values can also be altered from the MDI keyboard.

- 244 -

B-64304EN-1/01

PROGRAMMING

5.COMPENSATION FUNCTION

- Feedrate and alarm

The tool, when moving from the stating position toward the

measurement position predicted by xa or za in G36 or G37, is feed at

the rapid traverse rate across area A. Then the tool stops at point T

(xa-γ or za-γ) and moves at the measurement feedrate set by parameter

(No. 6241) across areas B, C, and D. If the approach end signal turns

on during movement across area B, alarm is generated. If the approach

end signal does not turn on before point V, and tool stops at point V

and alarm PS0080 is generated.

Predicted measurement position

F_R

F_P

U

V

X, Z

A

B

C

D

S (xs, zs)

T

ε

ε

Starting

position

γ

|xa-xs|. |za-zs|

U (xa, za)

FR : Rapid traverse rate

FP : Measurement feedrate (set by parameter(No.6241))

γ

: Parameters No.6251, No.6252

ε

: Parameters No.6254, No.6255

Fig. 5.5 (a) Feedrate and alarm

- 245 -

5.COMPENSATION FUNCTION

PROGRAMMING

B-64304EN-1/01

Example

Tool number T01

50

300

X-axis

Programmed zero point

measurement

position

380

Z-axis measurement position

100

800

Offset value

Offset value

(Before measurement)

(After measurement)

X

100.0

98.0

Z

0

4.0

G50 X760.0 Z1100.0 ;

Programming of absolute zero point

(Coordinate system setting)

S01 M03 T0101 ;

Specifies tool T1, offset number

1, and

spindle revolution

G36 X200.0 ;

Moves to the measurement position

If the tool has reached the measurement

position at X198.0

; since the correct

measurement position is 200 mm, the offset

value is altered by 198.0-200.0=-2.0mm.

G00 X204.0 ;

Refracts a little along the X axis.

G37 Z800.0 ;

Moves to the Z-axis measurement position.

If the tool has reached the measurement

position at X804.0, the offset value is altered

by 804.0-800.0=4.0mm.

T0101 ;

Further offsets by the difference.

The new offset value becomes valid when the

T code is specified again.

- 246 -

B-64304EN-1/01

PROGRAMMING

5.COMPENSATION FUNCTION

WARNING

1

Measurement speed(Fp), γ, and ε are set as parameters (Fp : No.6241, γ :

No.6251, ε : No.6254) by machine tool builder. ε must be positive numbers so that

γ>ε.

2

Cancel the tool nose radius compensation before G36, G37.

3

A delay or variation in detection of the measurement position arrival signal is 0 to 2

msec on the CNC side excluding the PMC side. Therefore, the measurement

error is the sum of 2 msec and a delay or variation (including a delay or variation on

the receiver side) in propagation of the measurement position arrival signal on the

PMC side, multiplied by the feedrate set in parameter No. 6241.

4

A delay or variation in time after detection of the measurement position arrival

signal until a feed stops is 0 to 8 msec. To calculate the amount of overrun,

further consider a delay in acceleration/deceleration, servo delay, and delay on the

PMC side.

5

When a manual movement is inserted into a movement at a measurement

feedrate, return the tool to the position before the inserted manual movement for

restart.

6

When tool nose radius compensation is enabled (bit 7 (NCR) of parameter No.

8136 is set to 0), the tool offset amount is calculated with considering the tool nose

radius value. Make sure that tool nose radius value is set correctly.

(Condition under which the tool-nose radius compensation is considered)

For the X-axis (first axis of the basic three axes) : TIP=0/5/7

For the Z-axis (third axis of the basic three axes) : TIP=0/6/8

For the Y-axis (second axis of the basic three axes) : TIP=0

A

B

Tool nose

radius

value

C

Measurement

position

The tool actually moves from point A to point B, but the tool offset value is

determined assuming that the tool moves to point C considering the tool nose

radius value.

NOTE

1 When there is no T code command before G36 or G37, alarm PS0081 is

generated.

2 When a T code is specified in the same block as G36 or G37, alarm PS0082 is

generated.

- 247 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.1

ADDRESSES AND SPECIFIABLE VALUE RANGE FOR

Series 10/11 PROGRAM FORMAT

Some addresses which cannot be used for the this CNC can be used in

the Series 10/11 program format. The specifiable value range for the

Series 10/11 program format is basically the same as that for the this

CNC. Sections II-6.2 to II-6.5 describe the addresses with a different

specifiable value range. If a value out of the specifiable value range is

specified, an alarm is issued.

6.2

SUBPROGRAM CALLING

Format

M98 Pxxxx Lyyyy ;

P : Subprogram number

L : Repetition count

Explanation

- Address

Address L cannot be used in this CNC tape format but can be used in

the Series 10/11 format.

- Subprogram number

The specifiable value range is the same as that for this CNC (1 to

9999).

If a value of more than four digits is specified, the last four digits are

assumed as the subprogram number.

- Repetition count

The repetition count L can be specified in the range from 1 to 9999. If

no repetition count is specified, 1 is assumed.

- 249 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.3.1

Outer Diameter/Internal Diameter Cutting Cycle (G90)

This cycle performs straight or taper cutting in the direction of the

length.

6.3.1.1

Straight cutting cycle

Format

G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length

F_

: Cutting feedrate

X axis

(R)

Rapid traverse

(F)

Cutting feed

Z

W

4(R)

A

3(F)

2(F)

1(R)

U/2

A’

X/2

Z axis

Fig. 6.3.1 (a) Straight cutting cycle

Explanation

- Operations

A straight cutting cycle performs four operations:

(1) Operation

1 moves the tool from the start point

(A) to the

specified coordinate of the second axis on the plane (specified

X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first

axis on the plane (specified Z-coordinate for the ZX plane) in

cutting feed.

(The tool is moved to the cutting end point (A') in

the direction of the length.)

(3) Operation 3 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in cutting

feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis

on the plane

(start Z-coordinate for the ZX plane) in rapid

traverse.

(The tool returns to the start point (A).)

- 251 -

6.MEMORY OPERATION

B-64304EN-1/01

PROGRAMMING

USING Series 10/11 FORMAT

6.3.1.2

Taper cutting cycle

Format

ZpXp-plane

G90 X(U)_ Z(W)_ I_ F_ ;

YpZp-plane

G90 Y(V)_ Z(W)_ K_ F_ ;

XpYp-plane

G90 X(U)_ Y(V)_ J_ F_ ;

X_,Y_,Z_

: Coordinates of the cutting end point (point A' in

the figure below) in the direction of the length

U_,V_,W_ : Travel distance to the cutting end point (point A'

in the figure below) in the direction of the length

I_,J_,K_

: Taper amount (I in the figure below)

F_

: Cutting feedrate

X axis

(R)

Rapid traverse

(F)

Cutting feed

4

(R)

A

3

(F)

U/2

1

(R)

A’

2

(F)

I

X/2

W

Z

Z axis

Fig. 6.3.1 (b) Taper cutting cycle

Explanation

Address I, J, or K for specifying a taper varies with the plane selected.

The figure of a taper is determined by the coordinates of the cutting

end point (A') in the direction of the length and the sign of the taper

amount (address I, J, or K). For the cycle in the figure above, a

minus sign is added to the taper amount.

NOTE

The increment system of address I, J, or K for

specifying a taper depends on the increment

system for the reference axis. Specify a radius

value at I, J, or K.

- 253 -

Content      ..     7      8      9      10     ..