Content      ..     22      23      24      25     ..

FANUC Series 16i/160i/160is-MB, Series 18i/180i/180is-MB5, Series 18i/180i/180is-MB. Operator's Manual - page 24

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Operation in circular interpolation

:Tool center path

:Programmed tool path

G40

G42.2

Tool

Fig. 22.5.1 (c) Operation at compensation start-up and cancellation

(Type B)

(3) Type C

As shown in the following figures, when G41.2, G42.2, or G40 is

specified, a block is inserted which moves the tool perpendicularly

to the movement direction specified in the next block by the distance

of the tool radius.

Operation in linear interpolation

:Tool center path

:Programmed tool path

Tool

G41.2

G40

Operation in circular interpolation

:Tool center path

:Programmed tool path

G40

Tool

G42.2

Fig. 22.5.1 (d) Operation at compensation start-up and cancellation

(Type C)

670

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

NOTE

For type C operation, the following conditions must be satisfied

when tool side compensation is started up or canceled :

1

The block containing G40, G41.2, or G42.2 must be

executed in the G00 or G01 mode.

2

The block containing G40, G41.2, or G42.2 must have no

move command.

3

The block after the block containing G41.2 or G42.2 must

contain a G00, G01, G02, or G03 move command.

D Operation in the

Changing of offset directions and offset values, holding of vectors,

compensation mode

interference checks, and so on are performed in the same way as for cutter

compensation. G39 (corner rounding) cannot be specified. So, note the

following :

(1) When the tool center path goes outside the programmed tool path at

a corner, a linear movement block, instead of an arc movement block,

is inserted to move the tool around the corner. When the tool center

path goes inside the programmed tool path, no block is inserted.

A linear movement block is inserted

No block is inserted

:Tool center path

:Programmed tool path

:Tool offset value

Workpiece

Tool

Workpiece

Tool

Example (1)-1 When going around the out-

Example (1)-2 When going around the in-

side of a corner with an

side of a corner with an

acute angle

acute angle

Fig. 22.5.1 (e) Operation in the compensation mode (1)-1, 2

In the above examples, the term “inside” means that the tool center

path is positioned inside the programmed tool path at a corner, and

“outside” means that the tool center path is positioned outside the

programmed tool path. In Example (1)-3, the relationship between

the tool center path and the programmed tool path is the same as in

Example (1)-1; the tool center path is positioned outside the

programmed tool path. Example (1)-4 has the same relationship as

Example (1)-2, where the tool center path is positioned inside the

programmed tool path.

671

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

:Tool center path

Workpiece

:Programmed tool path

:Tool offset value

Actual tool

Actual tool

Reference tool

Workpiece

Reference tool

Example(1)-3

Example(1)-4

Fig. 22.5.1 (f) Operation in the compensation mode (1)-3, 4

(2) When the tool moves at a corner, the feedrate of the previous block

is used if the corner is positioned before a single-block stop point; if

the corner is after a single-block stop point, the feedrate of the next

block is used.

F100

Q1’

Q2’(Single block stop point)

:Tool center path

Q

:Programmed tool path

Tool

Program(2)-1

N2

N3

:

N1 G90G41.2 Xp Yp Zp Bp Cp D1 ;

N2 G01Xq Yq Zq F100 ;

N3 Xr Yr Zr F200 ;

:

P’

R’

P

R

Example(2)-1

Fig. 22.5.1 (g) Operation in the compensation mode (2)

In the above example, the single block stop point of N2 is Q2’, so that

the feedrates along paths P’-Q1’ and Q1’-Q2’ are the same, namely,

F100.

(3) When a command is specified to make the tool retrace the path

specified in the previous block, the tool path can match the locus of

the previous block by changing the G code to change the offset

direction. If the G code is left unchanged, the operation shown in

Example (3)-2 results :

672

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

:Tool center path

:Programmed tool path

Example(3)-1

Tool movement when

Example(3)-2

Tool movement when the

changing G41.2 to G42.2

G code is left unchanged

(G41.2 mode)

(G41.2 mode)

G91 G01 X100.0

G91 G01 X100.0

G42.2 X-100.0

X-100.0

Fig. 22.5.1 (h) Operation in the compensation mode (3)

(4) Even when the tool movement changes linear to circular (helical),

circular (helical) to linear, or circular (helical) to circular (helical), the

start, end, and center points of a circular (helical) movement are

projected on the compensation plane that is perpendicular to the tool

axis, a compensation vector is calculated for the plane, then the vector

is added to the originally specified position to obtain the command

position. Then the tool is moved linearly or circularly (helically) to

the obtained command position. In this case, the tool moves

circularly (helically) in the currently selected plane. The tool does not

move circularly (helically) in the compensation plane. Therefore,

when the tool compensation is for circular movement, the

compensation plane must be the XY, YZ, or ZX plane.

Z

Tool axis

Tool

Y

Actual offset vector

End point

Start point

X

Move command

Actual tool center path

Projected

Offset vector created in

the compensation plane

Tool center path created in the

compensation plane

(Compensation plane = XY plane)

Fig. 22.5.1 (i) Operation in the compensation mode (4)

673

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

D Compensation vector

calculation

Q

e1=V_T

VD

Z

P

e2

e3

Y

X

R

Fig. 22.5.1 (j) Compensation vector calculation

In above figure, cutter compensation vector VD at point Q is calculated

as follows :

(1) Calculating the tool vector (VT)

(2) Calculating the coordinate conversion matrix (M)

Coordinate systems are defined as follows :

- Coordinate system C1 :

{O; X, Y, Z}

Cartesian coordinate system whose fundamental vectors are the

following unit vectors along the X-, Y-, and Z-axes :

(1, 0, 0)

(0, 1, 0)

(0, 0, 1)

- Coordinate system C2 :

{O; e2, e3, e1}

Cartesian coordinate system whose fundamental vectors are the

following unit vectors :

e2

e3

e1

where, e2, e3, and e1 are defined as follows :

e1 = V_T

e2 = b2 / |b2| , b2 = a2 - (a2,e1)- e1

e3 = b3 / |b3| , b3 = a3 - (a3,e1)- e1 - (a3,e2)- e2

a2 is an arbitrary vector linearly independent of e1, and

a3 is an arbitrary vector linearly indepen dent of e2 and e1.

The coordinate conversion matrix M from coordinate system C1 to

C2, and the coordinate conversion matrix M^-1 from coordinate system

C2 to C1 are expressed as :

e2

M+ƪe3ƫ

,

M-1 + (^te2

^t e3

^t e1)

e1

674

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

(3) Converting coordinates from coordinate system C1 to coordinate

system C2

The coordinates of the start and end points P and Q of a block and

coordinates of the end point R of the next block in coordinate system

C1 are converted to coordinates P’, Q’, and R’ in coordinate system

C2, respectively, by using the following expressions :

PȀ + MP

QȀ + QP

RȀ + MR

(4) Calculating the intersection vector (V_D’) in the compensation plane

{O; e2, e3}

In the coordinates in coordinate system C2 obtained in (3), two

components (the e1 component, the component of the tool direction,

is excluded) are used to calculate intersection vector V_D’ in the

compensation plane.

e3

R’

VD’

P’

Q’

e2

Fig. 22.5.1 (k) Compensation vector calculation

The e1 component of V_D’ is assumed to be always 0. The calculation

is similar to the calculation of cutter compensation C. Although one

vector is obtained in this example, up to four vectors may be

calculated.

If the difference between the e2 and e3 components

(in the

compensation plane) between two points is smaller than the value set

in parameter No. 6114 in intersection vector calculation, the block is

assumed to specify no movement. In this case, intersection calculation

is performed using the coordinates of one block ahead.

(5) Converting the intersection vector from coordinate system C2 to

coordinate system C1

From the following expression, vector V_D’ in coordinate system C2

is converted to vector V_D in coordinate system C1 :

V_D + M-1VDȀ

Vector VD is the compensation vector in the original XYZ coordinate

system.

675

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

D Calculation used when

the compensation plane

(1) When a rotation axis and linear axis are specified at the same time

is changed

When a rotation axis and linear axis are specified in the same block

in the G41.2 or G42.2 mode (the compensation plane changes

frequently), the cutter compensation vector is calculated using the

coordinates of the rotation axis at each point at which the vector is

obtained.

<Example>

G90 G00 X0 Y0 Z0 B0 C0 ;

G01 F1000 ;

N1 G42.2 Xp Yp Zp Bp Cp D1 ;

N2 Xq Yq Zq Bq Cq ;

N3 Xr Yr Zr Br Cr ;

N4 Xs Ys Zs Bs Cs ;

:

Vector calculation at the end point (Q) of block N2

- The tool vector (VT) and coordinate conversion matrix (M) are

calculated using the coordi nates (Bq, Cq) of the rotation axis at point

Q.

- The cutter compensation vector is calculated using the resultant

coordinates into which three points, P, Q, and R, are converted by

matrix M.

Q

N3

R

N2

Q’

R’

N4

P

N1

P’

O

S’

S

Fig. 22.5.1 (l) When a Rotation Axis and Linear Axis Are Specified at the

Same Time

(2) When a rotation axis is specified alone

When a rotation axis is specified alone in the G41.2 or G42.2 mode

(the compensation plane changes), the cutter compensation vector is

calculated as follows :

<Example>

G90 G00 X0 Y0 Z0 B0 C0 ;

G01 F1000 ;

N1 G42.2 Xp Yp Zp D1 ;

N2 Xq Yq Zq ;

N3 Br Cr ;

N4 Xs Ys Zs ;

:

676

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Vector calculation at the end point (Q) of block N2

- The tool vector (V_T) and coordinate conversion matrix (M_N2) are

calculated using the coordinates (B = 0, C = 0) of the rotation axis at

point Q.

- The cutter compensation vector (V_N2) is calculated using the resultant

coordinates into which three points, P, Q, and S, are converted by

matrix M_N2.

Vector calculation at the end point of block N3

- The coordinate conversion matrix (M_N3) is calculated using the

coordinates (Br, Cr) of the rotation axis at point R.

- The cutter compensation vector (V_N3) is calculated from the following

expression :

V_N3 = M_N3-1(M_N2-V_N2)

Q=R(N3)

N4

S

VN2=V3

N2

Q’=R’

S’

P

N1

P’

O

Fig. 22.5.1 (m) When a rotation axis is specified alone

D Interference check made

An interference check is made when the compensation plane (plane

when the compensation

perpendicular to a tool direction vector) is changed.

plane is changed

<Example>

If the program below is executed, a PS0272 alarm (overcutting due to

offsetting) is issued from N4.

O100 F3000

N1 G90 G00 X0 Y0 Z0 A-46 C180

N2 G41.2 D1

N3 G01 X100

N4 Y-200 Z-200

N5 A45

N6 Y-400 Z0

N7 X0

N8 Y-200 Z-200

N9 A-46

N10 Y0 Z0

N11 G40

M30

677

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Z

Y

N3

X

N10

N7

N4

N6

N8

N9

N5

Fig. 22.5.1 (n) Conceptual Diagram

Z

C

A

Vb

Va

45°

46°

B

Y

Va: Tool direction vector when A = -46

Vb: Tool direction vector when A=45

A : End point of N3

B : End point of N4

C : End point of N6

Fig. 22.5.1 (o) Tool Direction Vector

e3

e2

V2

B’

C’

A’

V1

A’ : Point A projected onto the compensation plane

B’ : Point B projected onto the compensation plane

C’ : Point C projected onto the compensation plane

Fig. 22.5.1 (p) Compensation Vector at the End Point (Point B) of N4

(on Compensation Plane)

678

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

The move direction of A’B’ is opposite to that of B’C’, so that two

compensation vectors, V1 and V2, are produced at point B’ (end point of

N4). There is a possibility of overcutting in this case, so an alarm

(PS0272) is issued from N4.

(1) Conditions for issuing the interference alarm

Suppose that the tool direction vector changes considerably from one

block to another due to a move command for a rotation axis. In this

case, an interference alarm is assumed because compensation vectors

are regarded as being generated in the wrong directions when the path

angle difference on the compensation plane is large, even though the

angle difference of the directions of compensation vectors to be

generated by those blocks is small.

Here, the compensation plane is perpendicular to the tool direction

(Va in Fig. 14.14.1(q)) of the first of the two blocks.

Specifically, the conditions below are used for issuing the alarm.

Z

C

A

Vb

Va

Ua

Ub

Wb

Wa

B

Y

X

Ua : Vector AB

Ub : Vector BC

Va : Tool direction vector between A and B

Vb : Tool direction vector between B and C

Wa : Va Ua

Wb : Vb Ub

(Here, represents an outer product operator.)

Fig. 22.5.1 (q) Conceptual Diagram

679

22.

RISC PROCESSOR

PROGRAMMING

B-63534EN/02

e3

e2

B’

C’

A’

Ra

Rb

A’

: Point A projected onto the compensation plane

B’ : Point B projected onto the compensation plane

C’ : Point C projected onto the compensation plane

Ra : Vector A’B’

Rb : Vector B’C’

Fig. 22.5.1 (r) Programmed Path (on the Compensation Plane) before and

after the End Point (Point B) of N4

When all the following conditions are satisfied, an alarm (PS0272)

Issued.

(a) The tool direction vector changes remarkably.

a : Angle for determination set in parameter No. 6261 (The default

is 45°.)

(Va,Vb) v cos(a)(Here, (Va,Vb) means an inner product.)

(b) The difference between the directions of the compensation vectors

to be generated is small.

Wa : Direction of a compensation vector to be generated by the AB

block.

Wb : Direction of a compensation vector to be generated by the BC

block.

Wa = Va Ua

Wb = Vb Ub

(Wa,Wb) w 0

(c) The path angle difference on the compensation plane is large.

(Ra,Rb) < 0

(2) Suppressing the issue of the alarm with a Q command

By inserting a Q command into a block that issued the alarm, the issue

of the alarm can be suppressed.

(a) Q1 command

By inserting a Q1 command, a vertical vector is generated.

Example) N4 Y-200 Z-200 Q1

680

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

e3

e2

B’

C’

A’

V

At point B’, a vector (V) perpendicular to A’B’ is generated.

Fig. 22.5.1 (s) Q1 Command

A vertical vector can also be generated by specifying G41.2 or

G42.1 in the next block as indicated in the example below.

Example) N6 G41.2 Y-400 Z0

(b) Q2 command

With a program specifying a linear-to-linear connection, up to two

compensation vectors are generated. In this case, the second vector

is deleted by inserting a Q2 command. The Q2 command has no

effect on circular interpolation.

Example) N4 Y-200 Z-200 Q2

e3

e2

B’

C’

A’

V1

The second vector (V2) is deleted, and only V1 is used as a compensation vector.

Fig. 22.5.1 (t) Q2 Command

(c) Q3 command

By inserting a Q3 command, the issue of the alarm can be suppressed.

Example) N4 Y-200 Z-200 Q3

e3

e2

V2

B’

C’

A’

V1

The two vectors (V1 and V2) are not deleted.

Fig. 22.5.1 (u) Q3 Command

681

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

22.5.2

Leading edge offset is a type of cutter compensation that is used when a

workpiece is machined with the edge of a tool. A tool is automatically

Leading Edge Offset

shifted by a specified cutter compensation value on the line where a plane

formed by a tool direction vector and tool movement direction intersects

a plane perpendicular to the tool axis direction.

Tool vector

Tool used

Reference

tool

Tool center path

(after

compensation)

Programmed

Cutter compensation

tool path

vector

Cutter compensation

amount

Fig. 22.5.2 (a) Reading edge offset

Format

D Leading edge offset

G41.3 D_ ;

D Leading edge offset

cancel

G40 ;

NOTE

1

G41.3 can be specified only in the G00 or G01 mode. In a

block containing G41.3 or G40, only the addresses D, O,

and N can be specified.

2

The block after a block containing a G41.3 command must

contain a move command. In that block, however, tool

movement in the same direction as the tool axis direction or

the opposite direction cannot be specified.

3

No continuous-state G code that belongs to the same

group as G00 and G01 can be specified in the G41.3 mode.

Explanations

D Operation at

Unlike tool side compensation the operation performed at leading edge

compensation start-up

compensation start-up and cancellation does not vary. When G41.3 is

and cancellation

specified, the tool is moved by the amount of compensation (V_C) in the

plane formed by the movement vector (V_M) of the block after a G41.3

block and the tool vector (V_T) obtained at the time of G41.3 specification.

The tool movement is perpendicular to the tool vector. When G40 is

specified, the tool is moved to cancel V_C. The following illustrates how

the compensation is performed.

682

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

(1) When the tool vector is inclined in the direction the tool moves

: Tool center path

: Programmed tool path

Tool vector(V_T)

Tool

G41.3(V_C)

VM

G40

Fig. 22.5.2 (b) When the tool vector is inclined in the direction the tool

moves

(2) When the tool vector is inclined in the direction opposite to the

direction the tool moves

: Tool center path

: Programmed tool path

Tool vector(V_T)

Tool

G41.3(V_C)

VM

G40

Fig. 22.5.2 (c) When the tool vector is inclined in the direction opposite to

the direction the tool moves

D Operation in the

The tool center moves so that a compensation vector (V_C) perpendicular

compensation mode

to the tool vector (V_T) is created in the plane formed by the tool vector

(V_T) at the end point of each block and the movement vector (V_M) of the

next block.

Tool center path (after compensation)

VT2

VT1

VC1

VC2

Programmed tool path

V

M1

VM3

VM2

VMn: Movement vector of block n

VTn : Tool vector at the end of block n

VCn : Compensation vector of block n (that lies in the VTn- VMn+1 plane, and is

perpendicular to VTn)

Fig. 22.5.2 (d) Operation in the compensation mode

If a G code or M code that suppresses buffering is specified in the

compensation mode, however, the compensation vector created

immediately before the specification is maintained.

When a block involving no movement (including a block containing a

move command for a rotation axis only) is specified, the movement vector

of the block after the block involving no movement is used to create a

compensation vector as shown below.

683

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Tool center path(after compensation)

VT2

VT1

VC1

Programmed path

V

M4

VM1

VM2

VC2 = VC3

There is one block that

specifies no movement.

Fig. 22.5.2 (e) There is one block that specifies no movement.

If block 3 involves no movement, the compensation vector of block 2

(V_C2) is created so that it is perpendicular to V_T2 and lies in the plane

formed by the movement vector (V_M4) of block 4 and the tool vector

(V_T2) at the end point of block 2.

NOTE

If two or more successive blocks involve no movement, the

previously created compensation vector is maintained.

However, such specification should be avoided.

D Block immediately

In the block immediately before the compensation cancel command

before the offset cancel

(G40), a compensation vector is created from the movement vector of that

command (G40)

block and the tool vector at the end point of the block as shown below :

Tool center path (after compensation)

VT2

VT1

G40

VC1

VC2

Programmed path

VM1

VM2

Fig. 22.5.2 (f) Block Immediately before G40

The compensation vector (V_C2) of block 2 is created so that it is

perpendicular to VT2 and lies in the plane formed by the tool vector (V_T2)

at the end point of block 2 and the movement vector (V_M2) of block 2.

D Method of compensation

In leading edge compensation, the compensation vector is calculated as

vector calculation

follows :

(1) Tool vector

(2) Movement vector

The movement vector (V_Mn+1) of block n+1 is obtained from the

following expression :

Xn)1 * X_n

Xn : Absolute coordinate value of X axis at

ȱ

ȳ

end point of block n

VMn)1 +ȧ

Yn : Absolute coordinate value of Y axis at

ȲZn)1 *^Znȴ

end point of block n

Zn : Absolute coordinate value of Z axis at

end point of block n

(3) Compensation vector

The direction of the compensation vector (V_Cn) of block n is defined

as follows :

(a) (V_Mn+1, V_Tn) > 0 (0deg < q < 90deg.)

684

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

VTn

Direction of V_Cn

VCn

q

(V_Mn+1

VTn) VTn

VMn+1

VMn+1

q represents the included angle

VCn

q

between V_Mn+1 and V_Tn.

(0° v q v 180°)

VTn

Fig. 22.5.2 (g) Direction of the compensation vector (1)

(b) (V_Mn+1,V_Tn) < 0 (90deg < q < 180deg.)

VCn

q

Direction of V_C1

VTn

- (V_Mn+1

VTn) VTn

VMn+1

VMn+1

V

Tn

q

VCn

Fig. 22.5.2 (h) Direction of the compensation vector (2)

The compensation vector (V_Cn) of block n is calculated from V_Tn and

V_Mn+1 as described below.

R=Offset value

ȱV^TX

ȳ

V +ȧ

ȲV^TZȴ

ȱV^MX

ȳ

VMn)1 +ȧ

ȲV^MZȴ

ȱV^X

ȳ

+ (VMn)1 V_Tn) V_Tn

V +ȧ

ȲV^Zȴ

ȱV^TZ (^VMZV^TX *^VMXV^TZ)*VTY (^VMXV^TY *^VMYV^TX)

ȳ

+ȧ

ȲV^TY (^VMYV^TZ *^VMZV^TY)*VTX (^VMZV^TX *^VMXV^TZ)ȴ

Then,

(a) When(V_Mn+1, V_Tn) > 0 (0deg. < q < 90deg.)

V_X

ȱ

ȳ

R

V_Cn +

Y

ȧ

ȧ

Ǹ

Vx2 ) Vr2 ) Vz2

ȲV

Z

ȴ

(b) When(V_Mn+1, V_Tn) < 0 (90deg. < q < 180deg.)

V_X

ȱ

ȳ

*R

V_Cn +

Y

ȧ

ȧ

Ǹ

Vx2 ) Vr2 ) Vz2

ȲV

Z

ȴ

685

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

D Compensation

When the included angle q between V_Mn+1 and V_Tn is regarded as 0deg.,

performed when q is

180deg., or 90deg., the compensation vector is created in a different way.

approximately 0deg.,

So, when creating an NC program, note the following points :

90deg., or 180deg.

(1) Setting a variation range for regarding q as 0deg., 180deg., or 90deg.

When the included angle (q) between the tool vector (V_T) and the

movement vector (V_M) becomes approximately 0deg., 180deg., or

90deg., the system regards q as 0deg., 180deg., or 90deg., then

creates a compensation vector which is different from the normal

compensation vector. The variation range used for regarding q as

0deg., 180deg., and 90deg. is or in parameter 6115.

For example, suppose that the angle set in parameter 6115 is Dq.

(a) If 0v q v Dq, q is regarded as 0deg.

∆q

VTn

q

VMn+1

Fig. 22.5.2 (i) Determination of q=0deg.

(b) If (180-Dq)v qv180, q is regarded as 180deg.

q

∆q

VTn

VMn+1

Fig. 22.5.2 (j) Determination of q=180deg.

(c) If (90-Dq)v q v(90+Dq) , q is regarded as 90deg.

∆q

∆q

VTn

VTn

q

q

VMn+1

VMn+1

Fig. 22.5.2 (k) Determination of q=90deg.

(2) Compensation vector when q is regarded as 0deg.or 180deg.

If q is regarded as 0deg.or 180deg.when G41.3 is specified to start

leading edge compensation, alarm PS998 is issued. This means that

the tool vector of the current block and the movement vector of the

686

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

next block must not point in the same direction or in opposite

directions at start-up.

The previously created compensation vector is maintained other than

at start-up at all times.

If the included angles between V_T2 and V_M3, V_T3 andV_M4, and V_T4

and V_M4, and V_T4 and V_M5 are regarded as 05, the compensation

vector V_C1 of block 1 is maintained as the compensation vectors V_C2,

V_C3, and V_C4, of blocks 2, 3, and 4, respectively.

Tool center path

(after compensation)

V_T1

V_T5

V_C1

V_C2

V_C5

V_M1

V_T2VC3

V_C4

V_T3

V_T4

V_M2

V_M6

V_M3

Programmed

V_M4

V_M5

Path

Fig. 22.5.2 (l) When q=0deg.Is Determined

If the included angles between V_T2 and V_M3, VT3 andV_M4, and V_T4

and V_M5 are regarded as 180deg., the compensation vector V_C1 of

block 1 is maintained as the compensation vectors V_C2, V_C3, and V_C4

of blocks 2, 3, and 4, respectively.

Tool center path

(after compensation)

V_T5

V_T1

V_C1

V_M2

V_C2

V_C3

V_C5

V_M1

V_M3

V_T4

V_C4

V_T2

V_M6

Programmed

V_T3

V_M4

V_M5

Path

Fig. 22.5.2 (m) When q=180deg. Is Determined

(3) Compensation vector when q is regarded as 90deg.

If the previous compensation vector (V_Cn-1) points in the opposite

direction ((V_Mn V_Tn-1) V_Tn-1 direction) to V_Mn with respect to

V_Tn-1, the current compensation vector (V_Cn) is created so it points

in the (V_Mn+1 V_Tn) V_Tn direction.

Tool center path

(after compensation)

V_T2

V_T3

V_T4

V_T1

V_T5

V_C1

V_C2

V

C5

V_M1

V_C3

V_C4

V_M2

V_M6

V_M3

Programmed

V_M4

V_M5

Path

Fig. 22.5.2 (n) When q=90deg. Is Determined (1)

If the previous compensation vector

(V_Cn-1) points in the same

direction ( -(V_Mn

V_Tn-1) V_Tn-1 direction) as V_Mn with respect to

V_Tn-1 , the current compensation vector (V_Cn) is created so it points in the

-(V_Mn+1 ( V_Tn) V_Tn direction.

687

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Tool center path

(after compensation)

V_T2

V_T3

V_T4

V_T5

V_T1

V_C5

V_C1

V_C2

V_M1

V_C3

V_C4

V_M2

V_M6

V_M3

Programmed

V_M4

V_M5

Path

Fig. 22.5.2 (o) When q=90deg. Is Determined (2)

22.5.3

Restrictions

D G41.2, G42.2, and G41.3

G41.2, G42.2, G41.3, and G40 are continuous-state G codes that belong

modes

to the same group. Therefore, the G41.2, G42.2, and G41.3 modes cannot

exist at the same time.

D Canned cycle command

Specify a canned cycle command in the compensation cancel mode

(G40).

D Command that must not

In the compensation mode, never successively specify two or more blocks

be specified in two or

that involve no movement. Blocks involving no movement include :

more successive blocks

- M05;

M code output

– S21;

S code output

– G04X1000;

Dwell

– G22X100000;

Machining area setting

– G10P01R100;

Offset value setting

–

(G17)Z2000;

Movement not in the offset plane (movement in

the tool axis direction)

- G90;,O10;,N20; Block containing no move command

- Blocks regarded as involving no movement according to parameter

6114 (for tool side compensation only)

D Reset

Resetting the system in a compensation mode (G41.2, G42.2, or G41.3)

always results in the cancellation mode (G40).

D Limitation of Functions

In the mode for this function, the following functions can be used, but the

condition of each function cannot be changed

- Inch/metric conversion

The alarm is issued when the condition is changed by G20 or G21

command.

- Mirror image

The condition of DI signal cannot be changed.

- Tool life management function

The tool length compensation use the amount of the tool specified by

tool life management function. The command for the tool life

management function have to command before the 3 dimensional

cutter compensation mode.

688

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Alarms

Number

Message

Contents

0037

CRC:PLANE CHANGE

An attempt was made to change the

plane in the cutter compensation mode.

To change the plane, cancel the cutter

compensation mode.

0041

CRC:INTERFERENCE

The depth of the cut is too great during

cutter compensation. Check the pro-

gram.

The criteria for judging interference are

as follows:

(1) The direction of movement of the

programmed block differs from the

direction of movement of the corre-

sponding tool center path block by

90° or more or 270° or less.The

check in this case can be disabled

by setting CNC parameter No.

6001#1 to “1”.

(2) In the case of an arc, the difference

in angle between the start and end

points of the programmed block dif-

fers by 180° or more with the differ-

ence in angle between the start and

end points of the corresponding tool

center path block.

0033

CRC:NO INTERSEC-

There is not point of intersection of the

TION

compensated tool center path during

cutter compensation.

5196

ILLEGAL AXIS OPERA-

A function which cannot be used during

TION

HPCC function ¡¡or 5-axis control func-

tion is being executed was commanded.

5405

ILLEGAL PARAMETER

The parameter settings (parameter Nos.

IN G41.2/G42.2

19610 to 19619) for determining the

relationship between the axis of rotation

and the rotation plane are incorrect.

5406

G41.3/G40 FORMAT

(1) A move instruction was specified in

ERROR

a block in which the G41.3 or G40

code is specified.

(2) A G or M code which suppresses

buffering was specified in the block

in which the G41.3 code was speci-

fied.

5407

ILLEGAL COMMAND

(1) A G code other than G00 or G01 in

IN G41.3

group 01 was specified in the G41.3

mode.

(2) An offset (G code in group 07) was

specified in the G41.3 mode.

(3) The block following the block in

which G41.3 (startup) was specified

did not contain a move command.

691

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Number

Message

Contents

5408

G41.3 ILLEGAL

(1) The G41.3 G code (startup) was

START_UP

specified in a group 01 mode for oth-

er than G00 and G01.

(2) The angle formed by the tool direc-

tion vector and the movement direc-

tion vector was 0° or 180° degrees

at startup.

5409

ILLEGAL PARAMETER

The parameter settings (parameter Nos.

IN G41.3

19610 to 19619) for determining the

relationship between the axis of rotation

and the rotation plane are incorrect.

692

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

Mid-point

X

(X1,Y1,Z1)

Y

Z

Start point

End point

(X2,Y2,Z2)

Fig.22.6 Start, Mid, and End Points

If the modal code is changed by specifying a code such as G01 with the

end point not specified, the arc cannot be obtained, and alarm PS5432 is

issued. During MDI operation, alarm PS5432 is also issued if a cycle start

is applied with only the mid-point specified.

D Movement along axes

In addition to the 3-dimensional circular interpolation axis (X/Y/Z), up

other than the

to two arbitrary axes (α/β) can be specified at a time. If α/β are omitted

3-dimensional circular

from the first block (mid-point specification) and are specified only in the

interpolation axis

second block (end point specification), the tool moves to the specified

point along the α/β axes during movement from the mid-point of the arc

to the end point. If α/β are omitted from the second block (end point

specification) and are specified only in the first block

(mid-point

specification), the tool moves to the specified point along the α/β axes

during movement from the start point of the arc to the mid-point.

With an incremental command, the position of the mid-point relative to

D Incremental commands

the start point must be specified in the first block, and the position of the

end point relative to the mid-point must be specified in the second block.

D Direction of rotation

The direction of rotation cannot be specified. The movement is the same

regardless of whether G02.4 or G03.4 is specified.

D Single block

When operation is performed using a single block, one cycle start causes

movement from the start point to the end point. A single-block stop is

not performed between the first block (mid-point specification) and the

second block (end point specification).

D Start point assumed if

If 3-dimensional circular interpolations are specified consecutively, the

3-dimensional circular

end point in one interpolation is assumed to be the start point in the next

interpolations are

interpolation.

specified consecutively

D Velocity command

Specify a tangential velocity along an arc in the three-dimensional space.

D Deceleration

In a mode other than AI high-precision contour control mode or AI

nano-based high-precision contour control mode, deceleration is applied

at the end point of the block immediately before the block that commands

three-dimensional circular interpolation or the end point of that block.

Then in-position check is performed.

694

B-63534EN/02

PROGRAMMING

22. RISC PROCESSOR

Limitation

D Cases in which linear

interpolation is

D If the start point, mid-point, and end-point are on the same line, linear

performed

interpolation is performed.

D If the start point coincides with the mid-point, the mid-point

coincides with the end point, or the end point coincides with the start

point, linear interpolation is performed up to the end point.

D If the start point, mid-point, and end-point are on the same line and

the end point lies between the start point and the mid-point, the tool

first moves with linear interpolation from the start point to the

mid-point, then returns from the mid-point to the end point with linear

interpolation. Thus, the tool always passes through the specified

point.

Start point

End point

Mid-point

D Whole circles

A whole circle (360 arc) cannot be specified. (This corresponds to the

case in which linear interpolation is performed, as described earlier.)

D Compensation functions

Before using this function, cancel the compensation functions of group

07, such as cutter radius compensation.

D Manual absolute

While this function is in use, manual intervention is not possible with the

manual absolute switch set to the ON position. If intervention is

performed, alarm PS0713 is issued when operation restarts.

D Background graphic

This function cannot be used with background graphic drawing.

D Limitation of Functions

In the mode for this function, the following functions can be used, but the

condition of each function cannot be changed

- Inch/metric conversion

The alarm is issued when the condition is changed by G20 or G21

command.

- Mirror image

The condition of DI signal cannot be changed.

- Tool life management function

The tool length compensation use the amount of the tool specified by

tool life management function. The command for the tool life

management function have to command before the 3 dimensional

cutter compensation mode.

- One-digit F code feed

The feedrate cannot be changed by using manual pulse generator.

695

22. RISC PROCESSOR

PROGRAMMING

B-63534EN/02

– Macro executor ( Execution macro )

- Manual handle interruption operation

- External deceleration

External decelaration is not available in this mode.

- Arbitrary chanfering/Corner rounding

D Others

3 dimensional cutter compensation function cannot be used with the

following function.

- Angular axis control

- Arbitrary angular axis contol

The limitation attaches about the combination of other NC instructions

occasionally.

Please refer to the manual of the each function.

Alarm

Number

Message

Contents

0710

ILLEGAL COMMAND

In a model state in which a 3-dimen-

IN 3-D CIR

sional circular interpolation (G02.4 or

G03.4) cannot be commanded, an at-

tempt for such interpolation was made.

An invalid code was commanded while

in three-dimensional circular interpola-

tion mode. This happens when:

S An M, S, T, or B code was comman-

ded while a command that cancels

three-dimensional circular interpola-

tion was being executed (such a can-

cel command is another G code in

group 01).

S The specified command was not one

that cancels three-dimensional circu-

lar interpolation and includes

G05P10000 or G05P0.

0712

G02.4/G03.4 FORMAT

Three-dimensional circular interpolation

ERROR

(G02.4 or G03.4) was commanded in-

correctly.

0713

MANUAL INTERVEN-

While 3-dimensional circular interpola-

TION IN G02.4/G03.4

tion mode (G02.4 or G03.4) is in prog-

(ABS ON)

ress, manual operation was performed

with the manual absolute switch turned

on.

698

Content      ..     22      23      24      25     ..