Content      ..     15      16      17      18     ..

FANUC MANUAL GUIDE i. OPERATOR’S MANUAL - page 17

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

1.7.4

Arbitrary Figure Blocks for Grooving (XY Plane)

When an arbitrary figure for grooving is input, data such as a figure type

and machining reference position is specified in the start point block.

Other data items to be input such as a straight line and arc are exactly the

same as for arbitrary figures of other machining types.

So, this subsection describes only the start point block of an arbitrary

figure for pocketing.

For other arbitrary figures, see Chapter

5, "DETAILED

DESCRIPTIONS ABOUT ENTERING ARBITRARY FIGURES", in

Part II.

When an arbitrary figure is specified for grooving, a groove with a

specified width is cut along the arbitrary figure line.

Start point: G1200 (XY plane)

ELEMENT

Data item

Meaning

X

START POINT X

X coordinate of the start point of an arbitrary figure

Y

START POINT Y

Y coordinate of the start point of an arbitrary figure

T

FIGURE TYPE

[FACE]

: Used as a figure for facing

[CONVEX]

: Used as an outer figure for contouring

[CONCAVE] : Used as an inner figure for contouring or as a

figure for pocketing

[GROOVE] : Used as a figure for grooving

Remark) When grooving is selected as machining type, be

sure to select [GROOVE].

B

BASE POSITION

Z coordinate of the bottom of a groove or the top surface of

a workpiece subject to grooving (in the tool axis direction)

L

HEIGHT/DEPTH

When the top surface of a workpiece is selected as the

BASE POSITION, specify the distance to the bottom of the

groove by using a negative value (radius value). → Depth

When the bottom of a groove is selected as the BASE

POSITION, specify the distance to the top surface of the

groove by using a positive value (radius value). → Height

D

GROOVE WIDTH

Groove width (radius value, positive value)

- 463 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

1.8

C-AXIS GROOVING

1.8.1

Machining Type Blocks for C-axis Grooving

Roughing: G1056

TOOL COND.

Data item

Meaning

D

TOOL DIAMETER

End mill diameter

NOTE

1 Tab ‘TOOL COND.’ is enabled when bit 0 (TLG) of

parameter No. 27002 = 1.

2 The operator ordinarily sets the above data on the

tab of ‘TOOL DATA’ in Tool Offset window.

Therefore, it is not necessary to display the tab

‘TOOL COND.’

CUT COND.

Data item

Meaning

J*

CUT DEPTH OF AXIS

Depth of cut in the tool axis direction per cutting

operation. By default, one cutting operation is

used. (radius value, positive value)

F

FEED RATE- RADIUS

Feedrate applicable when cutting is performed in

the side face direction of the end mill

E

FEEDRATE - AXIS

Feedrate applicable when cutting is performed in

the tool axis direction toward the bottom of a side

face being machined

C

CLEARANCE OF AXIS

Distance between the surface of a blank being

machined and a cutting start point (point R) in the

tool axis direction (radius value, positive value)

Remark) By referring to the parameter No.27009

(minimum clamp value), the system sets

the data as Initial value.

- 465 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

CUT COND.

Data item

Meaning

Z

APROCH MOTION

[2 AXES]

: When moving from the current

position to the machining start point,

the tool first moves in the machining

plane in two-axis synchronous

operation and then moves along the

tool axis. (initial value)

[3 AXES]

: The tool moves from the current

position to the machining start point in

three-axis synchronous operation.

- 466 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

1.8.2

Figure Blocks for C-axis Grooving and A-axis Grooving

As C-axis grooving figures, a "C-axis groove on the polar coordinate

plane (XC plane)", "X-axis groove on the polar coordinate plane (XC

plane)", "C-axis groove on the cylindrical surface (ZC plane)", "A-axis

groove on the cylindrical surface (XA plane)", "Z-axis groove on the

cylindrical surface (ZC plane)" and "X-axis groove on the cylindrical

surface (XA plane)" are available. When any of these figures is specified,

a groove with the diameter as large as the end mill diameter is cut.

In C-axis grooving, in-feed cutting in the tool axis direction is performed,

but in-feed cutting in the width direction is not performed.

NOTE

C-axis grooving uses neither polar coordinate

interpolation nor cylinder interpolation. So, it is

unnecessary to switch to the polar coordinate

interpolation or cylinder interpolation mode.

- 467 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

C-axis groove: G1570 (XC plane, end face)

On the end face of a workpiece, circular grooves are cut by rotating the

C-axis with the X-axis position of the tool fixed. Multiple grooves of the

same figure can be cut.

POS./SIZE

Data item

Meaning

B

BASE POSITION

Z coordinate of the bottom of a groove or the top

surface of a workpiece subject to grooving (in the tool

axis direction)

L

HEIGHT/DEPTH

When the top surface of a workpiece is selected as the

BASE POSITION, specify the distance to the bottom of

the groove by using a negative value (radius value).

→ Depth

When the bottom of a groove is selected as the BASE

POSITION, specify the distance to the top surface of the

groove by using a positive value (radius value).

→ Height

X

X AXIS POS.(RAD.)

X coordinate of the center line of a groove (radius value)

Q

GROOVE ANGLE

Center angle formed by the start point (tool center) and

end point (tool center) of a groove (positive or negative

value)

A

START ANGLE

C coordinate of the start point (tool center) of the first

groove

REPEAT

Data item

Meaning

C*

PITCH ANGLE

Center angle formed by the start points (tool centers) of

two adjacent grooves (positive or negative value)

M

GROOVE NUMBER

Number of grooves to be cut (positive value)

*

- 468 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

X-axis groove: G1571 (XC plane, end face)

On the end face of a workpiece, radial grooves are cut by moving the tool

in the X-axis direction with the C-axis position fixed. Multiple grooves of

the same figure can be cut.

POS./SIZE

Data item

Meaning

B

BASE POSITION

Z coordinate of the bottom of a groove or the top surface

of a workpiece subject to grooving (in the tool axis

direction)

L

HEIGHT/DEPTH

When the top surface of a workpiece is selected as the

BASE POSITION, specify the distance to the bottom of the

groove by using a negative value (radius value). → Depth

When the bottom of a groove is selected as the BASE

POSITION, specify the distance to the top surface of the

groove by using a positive value (radius value). → Height

X

X AXIS POS.(RAD.)

X coordinate of the start point of a groove (radius value)

P

GROOVE LENGTH

Distance between the start point (tool center) and end

point (tool center) of a groove (radius value,

positive/negative value)

A

START ANGLE

C coordinate of the start point (tool center) of the first

groove

REPEAT

Data item

Meaning

C*

PITCH ANGLE

Center angle formed by the start points (tool centers) of

two adjacent grooves (positive or negative value)

M

GROOVE NUMBER

Number of grooves to be cut (positive value)

*

- 469 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

C-axis groove: G1670 (cylindrical surface)

On the peripheral surface of a workpiece, grooves are cut by rotating the

C-axis with the Z-axis position of the tool fixed. Multiple grooves of the

same figure can be cut.

POS./SIZE

Data item

Meaning

B

BASE POSITION

X coordinate of the bottom of a groove or the top

surface of a workpiece subject to grooving (in the tool

axis direction)

L

HEIGHT/DEPTH

When the top surface of a workpiece is selected as the

BASE POSITION, specify the distance to the bottom of

the groove by using a negative value (radius value).

→ Depth

When the bottom of a groove is selected as the BASE

POSITION, specify the distance to the top surface of the

groove by using a positive value (radius value).

→ Height

Z

Z AXIS POS.

Z coordinate of the center line of a groove

Q

GROOVE ANGLE

Center angle formed by the start point (tool center) and

end point (tool center) of a groove (positive or negative

value)

A

START ANGLE

C coordinate of the start point (tool center) of the first

groove

REPEAT

Data item

Meaning

C*

PITCH ANGLE

Center angle formed by the start points (tool centers) of

two adjacent grooves (positive or negative value)

M

GROOVE NUMBER

Number of grooves to be cut (positive value)

*

- 470 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

Z-axis groove: G1671 (cylindrical surface)

On the peripheral surface of a workpiece, straight grooves are cut by

moving the tool in the Z-axis direction with the C-axis position fixed.

Multiple grooves of the same figure can be cut.

POS./SIZE

Data item

Meaning

B

BASE POSITION

X coordinate of the bottom of a groove or the top

surface of a workpiece subject to grooving (in the

tool axis direction)

L

HEIGHT/DEPTH

When the top surface of a workpiece is selected as

the BASE POSITION, specify the distance to the

bottom of the groove by using a negative value

(radius value). → Depth

When the bottom of a groove is selected as the

BASE POSITION, specify the distance to the top

surface of the groove by using a positive value

(radius value). → Height

Z

Z AXIS POS.

Z coordinate of the start point of a groove

P

GROOVE LENGTH

Distance between the start point (tool center) and

end point (tool center) of a groove (radius value,

positive/negative value)

A

START ANGLE

C coordinate of the start point (tool center) of the first

groove

REPEAT

Data item

Meaning

C*

PITCH ANGLE

Center angle formed by the start points (tool centers)

of two adjacent grooves (positive or negative value)

M*

GROOVE NUMBER

Number of grooves to be cut (positive value)

- 471 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

1.9

REAR END FACING BY MILLING

1.9.1

Rear End Facing

By setting bit 4 of parameter No. 27000 to 1, the input item "FACE

POSITION" is displayed on the figure menu for milling below. By

entering this data, rear end facing is enabled.

1.

Arbitrary-figure (XY plane) - Start point : G1200

2.

Hole position (XY plane) - Random points : G1210

3.

Hole position (XY plane) - Linear points (same interval) : G1211

4.

Hole position (XY plane) - Linear points (different interval) :

G1212

5.

Hole position (XY plane) - Grid points : G1213

6.

Hole position (XY plane) - Rectangle points : G1214

7.

Hole position (XY plane) - Circle points : G1215

8.

Hole position (XY plane) - Arc points (same interval): G1216

9.

Hole position

(XY plane) - Arc points (different interval)

:

G1217

10.

Fixed-figure (XY plane) - Rectangle : G1220

11.

Fixed-figure (XY plane) - Circle : G1221

12.

Fixed-figure (XY plane) - Track : G1222

13.

Fixed-figure (XY plane) - Radial groove : G1223

14.

Arbitrary-figure (XC plane) - Start point : G1500

15.

Fixed-figure (XC plane) - Rectangle : G1520

16.

Fixed-figure (XC plane) - Circle : G1521

17.

Fixed-figure (XC plane) - Track : G1522

18.

Fixed-figure (XC plane) - Radial groove : G1523

19.

C-axis groove on the polar coordinate plane: G1570

20.

X-axis groove on the polar coordinate plane : G1571

21.

C-axis hole on the polar coordinate plane (circle points) : G1572

22.

C-axis hole on the polar coordinate plane

(random points) :

G1573

- 472 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

Example) C-axis groove on the polar coordinate plane: G1570

FACE POSIT

Data item

Meaning

Z

FACE POSITION

[+FACE ]: References the figure below (+ end face).

[-FACE ]: References the figure below (- end face).

Reference position

Reference position

(-)

Depth

Depth

(-)

+Z

+Z

(+)

Height

Height

(+)

+ end face

- end face

Reference position

Reference position

(-)

Depth

Depth

(-)

+Z

+Z

(+)

Height

Height

(+)

- end face

+ end face

- 473 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

1.10

ADDRESS SETTING OF ROTATION AXIS

1.10.1

Support for C-Axis Machining with Rotation Axis

By setting bit

0 of parameter No.

27001 to

1, the input item

"ROTATION AXIS NAME" is displayed on the figure menu for

milling below. By entering this data, C-axis machining using a

rotation axis is enabled.

1.

Rectangle on the polar coordinate plane: G1520

2.

Circle on the polar coordinate plane : G1521

3.

Track on the polar coordinate plane : G1522

4.

Radial groove on the polar coordinate plane : G1523

5.

C-axis groove on the polar coordinate plane: G1570

6.

X-axis groove on the polar coordinate plane: G1571

7.

C-axis hole on the polar coordinate plane (circle points) : G1572

8.

C-axis hole on the polar coordinate plane

(random points) :

G1573

9.

C-axis groove on the cylindrical surface : G1670

10. X-axis groove on the cylindrical surface : G1671

11. C-axis hole on the cylindrical surface (circle points) : G1672

12. C-axis hole on the cylindrical surface (random points) : G1673

13. Arbitrary-figure on the end face : G1500

13. Arbitrary-figure on the cylindrical surface : G1600

- 474 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

Example) C-axis groove on the polar coordinate plane: G1570

ROT. AXIS

Data item

Meaning

Y

ROTATION AXIS NAME

When bit 1 of parameter No. 27001 #1 = 1

[C]: The rotation axis is the C-axis.

[A]: The rotation axis is the A-axis.

When bit 2 of parameter No. 27001 #2 = 1

[C]: The rotation axis is the C-axis.

[B]: The rotation axis is the B-axis.

When bit 3 of parameter No. 27001 #3 = 1

[C]: The rotation axis is the C-axis.

[E]: The rotation axis is the E-axis.

NOTE

This data item is enabled when the parameter

No.27001#0 = 1.

- 475 -

2.TURNING

CYCLE MACHINING TYPES

B-63874EN/05

2

TURNING

With MANUAL GUIDE i, the cycles motions listed below are available

for turning.

Hole machining (workpiece rotation)

G1100

Center drilling

G1101

Drilling

Machining type block

G1102

Tapping

G1103

Reaming

G1104

Boring

Turning

G1120

Outer surface roughing

G1121

Inner surface roughing

G1122

End face roughing

G1123

Outer surface semifinishing

Machining type block

G1124

Inner surface semifinishing

G1125

End face semifinishing

G1126

Outer surface finishing

G1127

Inner surface finishing

G1128

End face finishing

G1450

Start point

G1451

Straight line

G1452

Arc (CW)

Turning figure block

G1453

Arc (CCW)

(ZX plane)

G1454

Chamfer

G1455

Corner rounding

G1456

End

Turning groove

G1130

Outer surface roughing

G1131

Inner surface roughing

G1132

End face roughing

G1133

Outer surface roughing and finishing

Machining type block

G1134

Inner surface roughing and finishing

G1135

End face roughing and finishing

G1136

Outer surface finishing

G1137

Inner surface finishing

G1138

End face finishing

G1470

Outer normal groove

G1471

Outer trapezoidal groove

Groove figure block

G1472

Inner normal groove

(ZX plane)

G1473

Inner trapezoidal groove

G1474

End face normal groove

G1475

End face trapezoidal groove

- 480 -

B-63874EN/05

CYCLE MACHINING TYPES

2.TURNING

Threading

G1140

Outer surface

Machining type block

G1141

Inner surface

G1460

General-purpose thread

G1461

Metric thread

Thread figure block

G1462

Unified thread

(ZX plane)

G1463

PT thread

G1464

PF thread

NOTE

1

When cycle motions are input with MANUAL

GUIDE i, sets of a machining type block and figure

blocks must be input in succession for all cycle

motions except turning hole machining.

For one machining type block, multiple figure

blocks can be input.

However, multiple sets of arbitrary figures can be

input, with one set including up to 50 figures

enclosed between a start point and end block.

2

For each item marked with [*] in the tables below, a

standard value is automatically set if no value is

input.

The screen displays [*] to the right of a data item.

3

In some of the input data items, the system sets

the last inputed data as an initial data. As to these

input data items, the mark of “(COPY)” was

described.

4

The motions go back to the start point where the

machining cycle started after completing the all

cycle motions.

(It is possible not to go back the satrt point when

the parameter No.27102#7 is set to 1.)

5

Cycle machining cannot be performed in any of

control modes of the high-speed and high-precision

functions (commands for advanced preview

control, AI advanced preview control, AI contour

control, AI nano contour control, high-precision

contour control, AI high-precision contour control,

and AI nano high-precision contour control). To

perform cycle machining, control mode must be

canceled.

6

On the CNC for lathe turning with G-code system B

or C, when cycle machining is specified, G90 must

be specified in advance to make a switchover to

the absolute coordinate system. For hole

machining by turning (with the tool rotated), G98

(initial level return) or G99 (R position level return)

must be specified in advance.

- 481 -

2.TURNING

CYCLE MACHINING TYPES

B-63874EN/05

Remarks) Cycle retract motions

In case of No.27102#7=0, Retracting motions indicated as bloken

lines in the following drawing will be outputted. The order of

motion axis will be opposite to the approched motions

Retracting motion of a

machining cycle

Position where the

machining cycle

started

Approaching motions

of a machining cycle

In case of carrying out plural figures machining by one G4 digit

cycle, such like grooving, this retracting motions will be

available at the last figure machining.

- 482 -

B-63874EN/05

CYCLE MACHINING TYPES

2.TURNING

2.1

HOLE MACHINING (WORKPIECE ROTATION)

2.1.1

Machining Type Blocks for Hole Machining (Workpiece

Rotation)

NOTE

Hole machining (workpiece rotation) is performed

only at the center of a workpiece. So, unlike other

cycle motions, figure blocks cannot be specified.

Center drilling: G1100

CUT COND.

Data item

Meaning

C

CLEARANCE

Distance between the surface of a workpiece and

point R (radius value, positive value)

(COPY)

F

FEED RATE

Cutting feedrate (positive value)

(COPY)

P*

DWELL TIME

Dwell time at the bottom of a hole (in seconds,

positive value)

(COPY)

Z

APROCH MOTION

[Z→X]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction.

[X→Z]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction. (initial value)

[2 AXES] : From the current position to the

machining start point, the tool moves

simultaneously in the X- and Z-axis

directions.

POS./SIZE

Data item

Meaning

B

BASE POSITION

Z coordinate of the surface of a workpiece

L

CUT DEPTH

Hole depth (radius value, negative value)

- 483 -

2.TURNING

CYCLE MACHINING TYPES

B-63874EN/05

Drilling: G1101

CUT COND.

Data item

Meaning

Q*

PECKING CUT DEPT

Depth of cut per drilling operation (radius value,

positive value)

(COPY)

(Note)

K*

GO PAST AMOUNT

Length of the incomplete hole at the tip of the tool

(radius value, positive value)

(COPY)

C

CLEARANCE

Distance between the surface of a workpiece and

point R (radius value, positive value)

(COPY)

F

FEED RATE

Cutting feedrate (positive value)

(COPY)

P*

DWELL TIME

Dwell time at the bottom of a hole (in seconds)

(COPY)

Z

APROCH MOTION

[Z→X]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction.

[X→Z]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction. (initial value)

[2 AXES] : From the current position to the

machining start point, the tool moves

simultaneously in the X- and Z-axis

directions.

POS./SIZE

Data item

Meaning

B

BASE POSITION

Z coordinate of the surface of a workpiece

L

CUT DEPTH

Hole depth (radius value, negative value)

NOTE

The system refers to the parameter No.5114 as the

return amount. Therefore, please set No.5114 to

the suitable value before machining.

- 484 -

B-63874EN/05

CYCLE MACHINING TYPES

2.TURNING

Tapping: G1102

CUT COND.

Data item

Meaning

D

THREAD LEAD

Lead of a tapping tool (radius value, positive value)

(COPY)

C

CLEARANCE

Distance between the surface of a workpiece and

point R (radius value, positive value)

(COPY)

P*

DWELL TIME

Dwell time at the bottom of a hole (in seconds,

positive value)

(COPY)

Z

APROCH MOTION

[Z→X]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction.

[X→Z]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction. (initial value)

[2 AXES] : From the current position to the

machining start point, the tool moves

simultaneously in the X- and Z-axis

directions.

POS./SIZE

Data item

Meaning

B

BASE POSITION

Z coordinate of the surface of a workpiece

L

CUT DEPTH

Hole depth (radius value, negative value)

RIGID TAP

Data item

Meaning

R

TAP TYPE

[FLOAT]

: Specifies the float tap. (initial value)

[RIGID]

: Specifies the rigid tap. (Note)

S

SPINDLE SPEED

Spindle speed (min^-1)

NOTE

When you use the rigid tap M code command

(No.5200#0=0), the system refers to the parameter

No.5210 or No.5212 as M code. Therefore, please

set No.5210 or No.5212 to the suitable value

before machining.

- 485 -

2.TURNING

CYCLE MACHINING TYPES

B-63874EN/05

Reaming: G1103

CUT COND.

Data item

Meaning

C

CLEARANCE

Distance between the surface of a workpiece and

point R (radius value, positive value)

(COPY)

F

FEED RATE

Cutting feedrate (positive value)

(COPY)

P*

DWELL TIME

Dwell time at the bottom of a hole (in seconds,

positive value)

(COPY)

Z

APROCH MOTION

[Z→X]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction.

[X→Z]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction. (initial value)

[2 AXES]: From the current position to the

machining start point, the tool moves

simultaneously in the X- and Z-axis

directions.

POS./SIZE

Data item

Meaning

B

BASE POSITION

Z coordinate of the surface of a workpiece

L

CUT DEPTH

Hole depth (radius value, negative value)

- 486 -

B-63874EN/05

CYCLE MACHINING TYPES

2.TURNING

Boring: G1104

CUT COND.

Data item

Meaning

C

CLEARANCE

Distance between the surface of a workpiece and

point R (radius value, positive value)

(COPY)

F

FEED RATE

Cutting feedrate (positive value)

(COPY)

P*

DWELL TIME

Dwell time at the bottom of a hole (in seconds,

positive value)

(COPY)

Z

APROCH MOTION

[Z→X]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction.

[X→Z]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction. (initial value)

[2 AXES] : From the current position to the

machining start point, the tool moves

simultaneously in the X- and Z-axis

directions.

POS./SIZE

Data item

Meaning

B

BASE POSITION

Z coordinate of the surface of a workpiece

L

CUT DEPTH

Hole depth (radius value, negative value)

- 487 -

2.TURNING

CYCLE MACHINING TYPES

B-63874EN/05

2.2

TURNING

2.2.1

Machining Type Blocks for Turning

Outer surface roughing: G1120

TOOL COND.

Data item

Meaning

R

NOSE RADIUS

Tool nose radius of a roughing tool (positive value)

A

CUT EDGE ANGLE

Cutting edge angle of a roughing tool (positive

value)

B

NOSE ANGLE

Tool angle of a roughing tool (positive value)

J

IMAGINARY TOOL NOSE

Imaginary tool nose position of a roughing tool

NOTE

1 Tab ‘TOOL COND.’ is enabled when bit 0 (TLG) of

parameter No. 27102 = 1.

2 The operator ordinarily sets the above data on the

tab of ‘TOOL DATA’ in Tool Offset window.

Therefore, it is not necessary to display the tab

‘TOOL COND.’

CUT COND.

Data item

Meaning

P

CUTTING DIRECTION

[-Z]

: Cuts in the -Z direction.

[+Z]

: Cuts in the +Z direction.

Remark) [+Z] is used for cutting in the reverse

direction or for machining with a

subspindle.

(COPY)

Q

CUT DEPTH

Depth of each cut (radius value, positive value)

H

RATE OF CUT DEPTH

Change rate for the depth of cut. Specify a change

rate in steps of 1%. A second depth of cut and

subsequent ones are sequentially multiplied by a

specified change rate. The default is 100%, meaning

that the depth of cut remains unchanged. (1 to 200,

positive value)

C*

X-AXIS FINISH AMT.

Finishing allowance in the X-axis direction. The

blank is regarded as 0. (radius value, positive value)

- 488 -

B-63874EN/05

CYCLE MACHINING TYPES

2.TURNING

CUT COND.

Data item

Meaning

D*

Z-AXIS FINISH AMT.

Finishing allowance in the Z-axis direction. The

blank is regarded as 0. (radius value, positive value)

F

CUT DIRC.FEEDRATE

Feedrate applicable when the tool cuts in the

workpiece radius direction (positive value)

E

CUT DEPTH FEEDRATE

Feedrate applicable when the tool cuts in the Z-axis

direction (positive value)

V

CUT RISE FEEDRATE

Feedrate applicable when the tool cuts up in the

direction of retraction from the workpiece (positive

value)

DETAIL

Data item

Meaning

K

1ST OVERRIDE

Feedrate override value for the first cut. Specify an

override value in steps of 1%. The default is 100%.

(1 - 200, positive value)

Remark) This data item is used, for example, to cut

the black coating of a cast workpiece.

W

CUT RISE METHOD

[SPEED]: The tool retracts by a distance specified

with ESCAPE AMOUNT in the XZ

direction immediately after cutting.

[CUT]

: The tool retracts by a "retract" distance"

after cutting along the figure.

(COPY)

U

ESCAPE AMOUNT

Distance by which the tool retracts from a cutting

surface after each cut (radius value, positive value)

Remark) By referring to the parameter No. 27128

(minimum clamp value), the system sets

the data as an initial value.

L

X-AXIS CLEARANCE

Distance between a blank and machining start point

(approach point) in the X-axis direction (radius

value, positive value)

Remark) By referring to the parameter No. 27129

(minimum clamp value), the system sets

the data as an initial value.

M

Z-AXIS CLEARANCE

Distance between a blank and machining start point

(approach point) in the Z-axis direction (radius value,

positive value)

Remark) By referring to the parameter No. 27130

(minimum clamp value), the system sets

the data as an initial value.

Z

APROCH MOTION

[Z→X]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction. (initial value)

[X→Z]

: From the current position to the

machining start point, the tool moves in

the Z-axis direction and then in the

X-axis direction.

[2 AXES]

: From the current position to the

machining start point, the tool moves

simultaneously in the X- and Z-axis

directions.

- 489 -

2.TURNING

CYCLE MACHINING TYPES

B-63874EN/05

DETAIL

Data item

Meaning

S

CUT DEPTH DIRECTION

As to X axis Cut direction,

[-X]

: Cuts in the -X direction.

[+X]

: Cuts in the +X direction.

Remark) This data item is enable when the

parameter No.27100#0 = 1.

(COPY)

X

POCKET CUTTING

[CUT]

: Cuts a pocket. (initial value)

[NOTHIN] : Does not cut a pocket.

Remark) This data item is enable when the

parameter No.27100#1 = 1.

Y

OVERHANG CUTTING

[CUT]

: Cuts an overhang. (initial value)

[NOTHIN] : Does not cut an overhang.

Remark) This data item is enable when the

parameter No.27100#1 = 1.

- 490 -

B-63874EN/05

CYCLE MACHINING TYPES

2.TURNING

• Tool path

<1> The tool moves to the position "cut-in start point + clearance (L,

M)" by rapid traverse.

<2> After cutting in in the X-axis direction at the feedrate

(F)

specified for the cutting direction, the tool cuts in to the

entered-figure position where there is still a finishing allowance

in the Z-axis direction at the feedrate (E) specified for the cut-in

direction.

<3> If [SPEED] is selected, the tool immediately retracts by a return

clearance (U) in the X- and Z-axis direction. If [CUT] is selected,

the tool first cuts along the figure and then retracts by a return

clearance (U) in the X- and Z-axis direction.

<4> The tool moves to the cut-in start position in the Z-axis direction

by rapid traverse.

<5> Steps <2> to <4> are repeated until the lowest portion in the

X-axis direction is reached.

<6> If there is another pocket, the tool is positioned on the pocket,

and steps <2> to <4> are repeated.

<7> Once all portions are cut, the tool retracts to the position "cut-in

start position + clearance (L)" in the X-axis direction at the rapid

traverse rate.

NOTE

It is possible to specify "PART" and "BLANK" as

"ELEMENT TYPE" for an individual arbitrary figure.

This "BLANK" can be used to enter an arbitrary

figure resembling a blank figure to be actually

machined, so any portion other than the blank

portion will not be cut. This way, optimum rough

turning can be realized.

- 491 -

Content      ..     15      16      17      18     ..