Content      ..     13      14      15      16     ..

FANUC MANUAL GUIDE i. OPERATOR’S MANUAL - page 15

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

DETAIL

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.

• Tool path

<1> The tool moves to the position "cutting start position + clearance

(Cr)" by rapid traverse.

<2> The tool moves to the position "amount to be chamfered (C) +

ejection stroke (P)" at the feedrate (F) specified for cutting.

<3> The tool cuts in to the portion to be chamfered by the cut depth

(Dr) in the tool radius direction at the feedrate (Fd) specified for

both-edge thread cutting.

<4> The tool cuts along the contour of the hole machining profile at

the feedrate (Fr) specified for single-edge thread cutting.

<5> Steps

<3> and

<4> are repeated until only the finishing

allowance (Tr) in the tool radius direction is left uncut.

<6> The tool turns around the finishing allowance (Tr) in the tool

radius direction to perform finishing at the feedrate (Ff) specified

for finishing.

<7> The tool moves to the position "cut-in start position + clearance

(Cr)" by rapid traverse.

- 402 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

1.4.2

Fixed Form Figure Blocks for Contouring (XY Plane)

Square: G1220 (XY plane)

POS./SIZE

Data item

Meaning

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 contouring is selected as machining

type, select [CONVEX] if an outer figure is

to be machined; if an inner figure is to be

machined, select [CONCAVE].

B

BASE POSITION

Z coordinate of the top surface or the bottom of the

side face of a part to be subject to contouring (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 side face by using a negative value

(radius value). → Depth

When the bottom of a side face is selected as the

BASE POSITION, specify the distance to the top

surface of the workpiece by using a positive value

(radius value). → Height

H

CENTER POINT (X)

X coordinate of the center position of a rectangular

figure

V

CENTER POINT (Y)

Y coordinate of the center position of a rectangular

figure

U

LENGTH FOR X AXIS

Length of the side in the X-axis direction (radius

value, positive value)

W

LENGTH FOR Y AXIS

Length of the side in the Y-axis direction (radius

value, positive value)

R*

CORNER RADIUS

Radius for corner rounding (positive value)

A*

ANGLE

Inclination angle of a rectangular figure relative to

the X-axis (positive or negative value)

- 403 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

Circle: G1221 (XY plane)

POS./SIZE

Data item

Meaning

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 contouring is selected as machining

type, select [CONVEX] if an outer figure is

to be machined; if an inner figure is to be

machined, select [CONCAVE].

B

BASE POSITION

Z coordinate of the top surface or the bottom of the

side face of a part to be subject to contouring (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 side face by using a negative value

(radius value). → Depth

When the bottom of a side face is selected as the

BASE POSITION, specify the distance to the top

surface of the workpiece by using a positive value

(radius value). → Height

H

CENTER POINT (X)

X coordinate of the center position of a circular

figure

V

CENTER POINT (Y)

Y coordinate of the center position of a circular

figure

R

RADIUS

Radius of a circular figure (radius value, positive

value)

- 404 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

Track: G1222 (XY plane)

POS./SIZE

Data item

Meaning

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 contouring is selected as machining

type, select [CONVEX] if an outer figure is

to be machined; if an inner figure is to be

machined, select [CONCAVE].

B

BASE POSITION

Z coordinate of the top surface or the bottom of the

side face of a part to be subject to contouring(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 side face by using a negative value

(radius value). → Depth

When the bottom of a side face is selected as the

BASE POSITION, specify the distance to the top

surface of the workpiece by using a positive value

(radius value). → Height

H

CENTER POINT (X)

X coordinate of the center position of the left

semicircle

V

CENTER POINT (Y)

Y coordinate of the center position of the left

semicircle

U

BETWEEN DISTANCE

Distance between the centers of the right and left

semicircles (radius value, positive value)

R

RADIUS

Radius of the left and right semicircles (radius value,

positive value)

A*

ANGLE

Inclination angle of a track figure relative to the

X-axis (positive or negative value)

- 405 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

1.4.4

Arbitrary Figure Blocks for Contouring (XY Plane)

When an arbitrary figure for contouring 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 contouring.

For other arbitrary figures, see Chapter

5, "DETAILED

DESCRIPTIONS ABOUT ENTERING ARBITRARY FIGURES," in

Part II.

Start point: G1200 (XY plane)

ELEMENT

Data item

Meaning

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 and

emboss machining or as a figure for pocketing

[GROOVE] : Used as a figure for grooving

[OPEN]

: Used when only one side is cut during

contouring

Remark) When contouring is specified as a machining type,

one of [CONVEX], [CONCAVE], and [OPEN] must

be selected.

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

Z

BASE POSITION

Z coordinate of the top surface or the bottom of the side face

of a part to be subject to contouring (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 side

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

When the bottom of a side face is selected as the BASE

POSITION, specify the distance to the top surface of the

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

- 407 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

ELEMENT

Data item

Meaning

P

FIGURE

[RIGHT] : The right side of an entered figure as viewed with

ATTRIBUTE

respect to the direction of movement is cut. (initial

value)

[LEFT]

: The left side of an entered figure as viewed with

respect to the direction of movement is cut. (initial

value)

Remark) These items are displayed only when [OPEN] is

selected as a figure type.

- 408 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

1.5

EMBOSS MACHINING

In the case of the contouring, the tool cuts along the side-face contour

of the machining profile and performs in-feed machining in the tool

radius direction. These tool passes sometimes generate many air-cut

movement as the following left figure.

So, the machining called “EMBOSS MACHINING CYCLE” that can

reduce the air-cut passes as the following right figure is prepared.

NOTE

1 This function is available when parameter

No.27000#7=1.

2 The parameters for the machining conditions for

embossing cycles are same with the parameters for

pocketing cycles. (Ex. No. 27066)

1.5.1

Machining Type Blocks for Emboss machining

Rough: G1080

TOOL COND.

Data item

Meaning

D

TOOL DIAMETER

End mill diameter

- 410 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

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

T*

BOTTOM THICKNESS

Cutting allowance of the bottom in side face

machining. The blank is regarded as 0. (radius

value, positive value)

S*

SIDE THICKNESS

Cutting allowance of the side face. The blank is

regarded as 0. (radius value, positive value)

Remark) When both the side surplus thickness and

bottom surplus thickness are omitted, an

entire pocket area is cut.

L

CUT DEPTH OF RADIUS

Depth of cut on the side face (tool radius direction)

per cutting operation (radius value, positive value)

J

CUT DEPTH OF AXIS

Depth of cut in the tool axis direction per cutting

operation (radius value, positive value)

K*

SIDE FINISH AMOUNT

Finishing allowance on the side face. The blank is

regarded as 0. (radius value, positive value)

H*

BOTTOM FINISHI AMT.

Finishing allowance at the bottom in side face

machining. The blank is regarded as 0. (radius

value, positive value)

F

FEED RATE- SING.CUT

Feedrate applicable when only the one-side cutter

portion of an end mill is used for cutting. This

feedrate is used for cutting in retract operation and

on the side face other than initial cutting.

V

FEED RATE- BOTH.CUT

Feedrate applicable when the entire front side of an

end mill is used for cutting. This feedrate is used for

initial cutting.

E

FEED RATE- AXIS

Feedrate applicable when cutting is performed in the

tool axis direction toward the bottom of a side face

being machined

DETAIL

Data item

Meaning

W

UP CUT/DOWN CUT

[UP CUT]

: Performs machining in up-cut mode,

assuming that the tool is rotating

clockwise.

[DWNCUT] : Performs machining in down-cut

mode, assuming that the tool is

rotating clockwise.

(COPY)

- 411 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

DETAIL

Data item

Meaning

B

CLEARANCE OF RADIUS

Distance between the side face and a tool retract

position in the tool radius direction (radius value,

positive value)

Remark1) When one pocket cutting operation is

completed, the tool performs a retract

operation in the tool axis direction from

the side face of the pocket by this

clearance amount.

Remark2) By referring to the parameter No.27009

(minimum clamp value), the system sets

the data as Initial value.

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.

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.

- 412 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

Bottom Finish: G1081

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

T*

BOTTOM THICKNESS

Cutting allowance at the bottom in side face

machining. The blank is regarded as 0. (radius

value, positive value)

K*

SIDE FINISH AMOUNT

Finishing allowance of the side face. The blank is

regarded as 0. (radius value, positive value)

H*

BOTTOM FINISHI AMT.

Finishing allowance at the bottom in side face

machining. The blank is regarded as 0. (radius

value, positive value)

L

CUT DEPTH OF RADIUS

Depth of cut on the side face (tool radius direction)

per cutting operation (radius value, positive value)

F

FEED RATE- SING.CUT

Feedrate applicable when only the one-side cutter

portion of an end mill is used for cutting. This

feedrate is used for cutting in retract operation and

on the side face other than initial cutting.

V

FEED RATE- BOTH.CUT

Feedrate applicable when the entire front side of an

end mill is used for cutting. This feedrate is used for

initial cutting.

E

FEED RATE- AXIS

Feedrate applicable when cutting is performed in the

tool axis direction toward the bottom of a side face

being machined

- 413 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

DETAIL

Data item

Meaning

W

UP CUT/DOWN CUT

[UP CUT]

: Performs machining in up-cut mode,

assuming that the tool is rotating

clockwise.

[DWNCUT] : Performs machining in down-cut

mode, assuming that the tool is

rotating clockwise.

(COPY)

B

CLEARANCE OF RADIUS

Distance between the side face and a tool retract

position in the tool radius direction (radius value,

positive value)

Remark1) When one pocket cutting operation is

completed, the tool performs a retract

operation in the tool axis direction from

the side face of the pocket by this

clearance amount.

Remark2) By referring to the parameter No.27009

(minimum clamp value), the system sets

the data as Initial value.

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.

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.

- 414 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

Side face finish: G1082

TOOL COND.

Data item

Meaning

I

INPUT

[INPUT] : Inputs a cutter compensation value directly.

[REF.]

: Inputs a cutter compensation number to

read a cutter compensation value by that

number.

D

TOOL DIAMETER

End mill diameter (positive value)

Remark) This item is indicated only when [INPUT] is

selected for INPUT.

M

CUTTER COMP.NO.

Cutter compensation number of an end mill (positive

value)

Remark) This item is indicated only when [REF.] is

selected for INPUT.

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.’

3 Tab ‘TOOL COND.’ is not enabled when bit 3 (PF3)

of parameter No. 27061 = 1.

CUT COND.

Data item

Meaning

K*

SIDE FINISH AMOUNT

Finishing allowance of the side face. The blank is

regarded as 0. (radius value, positive value)

H*

BOTTOM FINISHI AMT.

Finishing allowance at the bottom in side face

machining. The blank is regarded as 0. (radius

value, positive value)

F

FEED RATE- SING.CUT

Feedrate applicable when only the one-side cutter

portion of an end mill is used for cutting. This feedrate

is used for cutting in retract operation and on the side

face other than initial cutting.

V

FEED RATE- BOTH.CUT

Feedrate applicable when the entire front side of an

end mill is used for cutting. This feedrate is used for

initial cutting.

- 415 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

CUT COND.

Data item

Meaning

E

FEED RATE- AXIS

Feedrate applicable when cutting is performed in the

tool axis direction toward the bottom of a side face

being machined

DETAIL

Data item

Meaning

W

UP CUT/DOWN CUT

[UP CUT]

: Performs machining in up-cut mode,

assuming that the tool is rotating

clockwise.

[DWNCUT] : Performs machining in down-cut mode,

assuming that the tool is rotating

clockwise.

(COPY)

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.

P

APPROACH TYPE

[ARC]

: Approaches a side face along an arc.

[TANGEN]: Approaches a side face along the straight

line tangent to the first figure in side face

cutting.

[VERTIC] : Approaches a side face along the straight

line normal to the first figure in side face

cutting.

(COPY)

R

APPROACH RAD./DIST.

Radius when [ARC] is specified.

Straight line length when [TANGEN] or [VERTIC] is

specified. (radius value, positive value)

Remark) By referring to the parameter No.27010

(minimum clamp value), the system sets the

data as Initial value.

A*

APPROACH ANGLE

Center angle of the arc when [ARC] is specified. The

default is 90 degrees. (positive value)

Remark) This data item is indicated only when [ARC]

is selected for APPROACH TYPE.

(COPY)

Q

ESCAPE TYPE

[ARC]

: Retracts from a side face along an arc.

[TANGEN]: Retracts from a side face along the

straight line tangent to the last figure in

side face cutting.

[VERTIC] : Retracts from a side face along the

straight line normal to the last figure in

side face cutting.

(COPY)

- 416 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

DETAIL

Data item

Meaning

X

ESCAPE RAD./DIST.

Radius when [ARC] is specified.

Straight line length when [TANGEN] or [VERTIC] is

specified. (radius value, positive value)

Remark) By referring to the parameter No.27010

(minimum clamp value), the system sets the

data as Initial value.

Y*

ESCAPE ANGLE

Center angle of the arc when [ARC] is specified. The

default is 90 degrees. (positive value)

Remark) This data item is indicated only when [ARC]

is selected for ESCAPE TYPE.

(COPY)

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.

- 417 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

Chamfer: G1083

TOOL COND.

Data item

Meaning

K

TOOL SMALL DIAMETER

Diameter of the tip of a chamfering tool (positive

value)

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

S

CHAMFER AMOUNT

Chamfer length (radius value, positive value)

H

EJECTION STROKE

Distance between the tip of a chamfering tool and an

actually cut position in the tool axis direction (radius

value, positive value)

F

FEED RATE - RADIUS

Feedrate applicable when cutting is performed in the

tool radius direction

E

FEED RATE - AXIS

Feedrate applicable when cutting is performed in the

tool axis direction

DETAIL

Data item

Meaning

W

UP CUT/DOWN CUT

[UP CUT]

: Performs machining in up-cut mode,

assuming that the tool is rotating

clockwise.

[DWNCUT] : Performs machining in down-cut mode,

assuming that the tool is rotating

clockwise. (initial value)

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.

- 418 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

DETAIL

Data item

Meaning

P

APPROACH TYPE

[ARC]

: Approaches a side face along an arc.

[TANGEN]: Approaches a side face along the straight

line tangent to the first figure in side face

cutting.

[VERTIC] : Approaches a side face along the straight

line normal to the first figure in side face

cutting.

(COPY)

R

APPROACH RAD./DIST.

Radius when [ARC] is specified.

Straight line length when [TANGEN] or [VERTIC] is

specified. (radius value, positive value)

Remark) By referring to the parameter No.27010

(minimum clamp value), the system sets the

data as Initial value.

A*

APPROACH ANGLE

Center angle of the arc when [ARC] is specified. The

default is 90 degrees. (positive value)

Remark) This data item is indicated only when [ARC]

is selected for APPROACH TYPE.

(COPY)

Q

ESCAPE TYPE

[ARC]

: Retracts from a side face along an arc.

[TANGEN]: Retracts from a side face along the

straight line tangent to the last figure in

side face cutting.

[VERTIC] : Retracts from a side face along the

straight line normal to the last figure in

side face cutting.

(COPY)

X

ESCAPE RAD./DIST.

Radius when [ARC] is specified.

Straight line length when [TANGEN] or [VERTIC] is

specified. (radius value, positive value)

Remark) By referring to the parameter No.27010

(minimum clamp value), the system sets the

data as Initial value.

Y*

ESCAPE ANGLE

Center angle of the arc when [ARC] is specified. The

default is 90 degrees. (positive value)

Remark) This data item is indicated only when [ARC]

is selected for ESCAPE TYPE.

(COPY)

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.

- 419 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

1.5.2

Arbitrary Figure Blocks for Emboss machining (XY Plane)

When an arbitrary figure for emboss machining 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.

In creating the arbitrary figure for the emboss machining, create the

arbitrary figures which are the outside boundary of the cutting area at

fast. After finishing the outside boundary figures, press [ISLAND]

soft key and create the arbitrary figures which are the contour product

figure.

Start point: G1200 (XY plane)

ELEMENT

Data item

Meaning

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 and

emboss machining or as a figure for pocketing

[GROOVE] : Used as a figure for grooving

Remark) When emboss machining is selected as machining

type, be sure to select [CONCAVE].

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

B

BASE POSITION

Z coordinate of the top surface of a workpiece subject to

pocketing or the bottom of a pocket (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 side

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

When the bottom of the side face is selected as the BASE

POSITION, specify the distance to the top surface of the

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

- 420 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

1.6

POCKETING

1.6.1

Machining Type Blocks for Pocketing

Rough: G1040

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

T*

BOTTOM THICKNESS

Cutting allowance of the bottom in side face

machining. The blank is regarded as 0. (radius

value, positive value)

S*

SIDE THICKNESS

Cutting allowance of the side face. The blank is

regarded as 0. (radius value, positive value)

Remark) When both the side surplus thickness and

bottom surplus thickness are omitted, an

entire pocket area is cut.

L

CUT DEPTH OF RADIUS

Depth of cut on the side face (tool radius direction)

per cutting operation (radius value, positive value)

J

CUT DEPTH OF AXIS

Depth of cut in the tool axis direction per cutting

operation (radius value, positive value)

K*

SIDE FINISH AMOUNT

Finishing allowance on the side face. The blank is

regarded as 0. (radius value, positive value)

H*

BOTTOM FINISHI AMT.

Finishing allowance at the bottom in side face

machining. The blank is regarded as 0. (radius

value, positive value)

- 422 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

CUT COND.

Data item

Meaning

F

FEED RATE- SING.CUT

Feedrate applicable when only the one-side cutter

portion of an end mill is used for cutting. This

feedrate is used for cutting in retract operation and

on the side face other than initial cutting.

V

FEED RATE- BOTH.CUT

Feedrate applicable when the entire front side of an

end mill is used for cutting. This feedrate is used for

initial cutting.

E

FEED RATE- AXIS

Feedrate applicable when cutting is performed in the

tool axis direction toward the bottom of a side face

being machined

NOTE

When a non-zero value is input for just one of the

data items, side surplus thickness and bottom

surplus thickness, cutting is performed for the input

surplus thickness, and for the omitted surplus

thickness, cutting operation is not performed on the

assumption that the omitted surplus thickness is 0.

When non-zero values are input for both the side

surplus thickness and bottom surplus thickness,

cutting is performed for each surplus thickness.

DETAIL

Data item

Meaning

W

UP CUT/DOWN CUT

[UP CUT]

: Performs machining in up-cut mode,

assuming that the tool is rotating

clockwise.

[DWNCUT] : Performs machining in down-cut

mode, assuming that the tool is

rotating clockwise.

(COPY)

B

CLEARANCE OF RADIUS

Distance between the wall of a pocket and a tool

retract position in the tool radius direction (radius

value, positive value)

Remark1) When one pocket cutting operation is

completed, the tool performs a retract

operation in the tool axis direction from

the side face of the pocket by this

clearance amount.

Remark2) By referring to the parameter No.27009

(minimum clamp value), the system sets

the data as Initial value.

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.

- 423 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

DETAIL

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.

A*

CUT ANGLE

Angle at which the tool cuts into the pocket

obliquely. The blank is regarded as 0 degrees. (in

one-degree increments, positive value)

Remark) By performing cutting also using the side

face of an end mill, the load on the tool can

be reduced.

(COPY)

P*

START PT.(1ST AXIS)

1st-axis coordinate of the cutting start point of

pocketing. When omitting this item, also omit the

2nd-axis coordinate. In this case, the coordinates of

the start point are determined automatically.

Remark1) The 1st axis is the X-axis on the XY

plane, the Y-axis on the YZ plane, the

X-axis on the XC plane, the Z-axis on the

ZC plane, or the X-axis on the XA plane.

Remark2) This item is enable when the parameter

No. 27060#7(PR7) = 1.

Q*

START PT.(2ND AXIS)

2nd-axis coordinate of the cutting start point of

pocketing. When this item is omitted, the coordinate

is determined automatically.

Remark1) The 2nd axis is the Y-axis on the XY

plane, the Z-axis on the YZ plane, the

C-axis on the XC plane, the C-axis on the

ZC plane, or the A-axis on the XA plane.

Remark2) This item is enable when the parameter

No. 27060#7(PR7) = 1.

- 424 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

• Tool path

The inside of a pocket machining profile is cut off in a spiral manner.

The following tool path is created.

More than one island machining profile and more than one cavity

machining profile can be defined for a pocket machining profile. The

island machining profiles are left uncut.

The cavity machining profiles are detoured so that they will not be

cut.

The tool path is created in such a way that an anticipated interference

with pocket machining profiles or island machining profiles can be

avoided.

The created tool path is effective because retraction in the tool axis

direction is avoided as much as possible.

For this tool path, in-feed machining in the tool axis direction is

possible.

Only specified cutting allowances can be cut off.

The direction of cutting can be either up-cut or down-cut. The

direction of cutting is controlled automatically around islands.

It is possible to cut in from the inside and outside of the machining

profile.

If there is a portion left uncut at a corner, it is possible to

automatically discriminate the uncut portion and cut it off.

It is possible to cut in at an arbitrary angle in the tool axis direction.

It is possible to specify an arbitrary position as a cutting start point.

It is possible to determine a cutting start point automatically.

It is possible to select a movement method for tool movement.

It is possible to control automatically a cut-in depth on the island

machining profile top surface automatically.

It is possible to set up cutting conditions, such as finishing allowance

for island machining profiles, for each island machining profile.

- 425 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

In the following pocket machining profile, which has a pocket through

which the tool can pass, the tool is lifted automatically to cut only a

range that can be cut.

If there is more than one cut in the tool axis direction, each range is

cut completely before another.

A contour specified as an open element of a pocket machining profile

is cut off as shown below.

- 426 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

Bottom Finish: G1041

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

T*

BOTTOM THICKNESS

Cutting allowance at the bottom of a pocket. The

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

K*

SIDE FINISH AMOUNT

Finishing allowance on the side face of a pocket.

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

value)

H*

BOTTOM FINISHI AMT.

Finishing allowance at the bottom of a pocket. The

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

L

CUT DEPTH OF RADIUS

Depth of cut on the side face (tool radius direction)

per cutting operation (radius value, positive value)

F

FEED RATE- SING.CUT

Feedrate applicable when only the one-side cutter

portion of an end mill is used for cutting. This

feedrate is used for cutting in retract operation and

on the side face other than initial cutting.

V

FEED RATE- BOTH.CUT

Feedrate applicable when the entire front side of an

end mill is used for cutting. This feedrate is used for

initial cutting.

E

FEED RATE- AXIS

Feedrate applicable when cutting is performed in the

tool axis direction toward the bottom of a side face

being machined

- 427 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

DETAIL

Data item

Meaning

W

UP CUT/DOWN CUT

[UP CUT]

: Performs machining in up-cut mode,

assuming that the tool is rotating

clockwise.

[DWNCUT] : Performs machining in down-cut

mode, assuming that the tool is

rotating clockwise.

(COPY)

B

CLEARANCE OF RADIUS

Distance between the wall of a pocket and a tool

retract position in the tool radius direction (radius

value, positive value)

Remark1) When one pocket cutting operation is

completed, the tool performs a retract

operation in the tool axis direction from

the side face of the pocket by this

clearance amount.

Remark2) By referring to the parameter No.27009

(minimum clamp value), the system sets

the data as Initial value.

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.

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.

A*

CUT ANGLE

Angle at which the tool cuts into the pocket

obliquely. The blank is regarded as 0 degrees. (in

one-degree increments, positive value)

Remark) By performing cutting also using the side

face of an end mill, the load on the tool can

be reduced.

(COPY)

- 428 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

DETAIL

Data item

Meaning

P*

START PT.(1ST AXIS)

1st-axis coordinate of the cutting start point of

pocketing. When omitting this item, also omit the

2nd-axis coordinate. In this case, the coordinates of

the start point are determined automatically.

Remark1) The 1st axis is the X-axis on the XY

plane, the Y-axis on the YZ plane, the

X-axis on the XC plane, the Z-axis on the

ZC plane, or the X-axis on the XA plane.

Remark2) This item is enable when the parameter

No. 27060#7(PR7) = 1.

Q*

START PT.(2ND AXIS)

2nd-axis coordinate of the cutting start point of

pocketing. When this item is omitted, the coordinate

is determined automatically.

Remark1) The 2nd axis is the Y-axis on the XY

plane, the Z-axis on the YZ plane, the

C-axis on the XC plane, the C-axis on the

ZC plane, or the A-axis on the XA plane.

Remark2) This item is enable when the parameter

No. 27060#7(PR7) = 1.

• Tool path

The bottom surface of a pocket machining profile is finished in a

spiral manner.

The tool path for it is the same as for pocketing (roughing).

See descriptions about pocketing (roughing) for details.

No in-feed machining in the tool axis direction is performed, though.

The top surface of island machining profiles is not cut off either.

- 429 -

1.MILLING

CYCLE MACHINING TYPES

B-63874EN/05

Side face finish: G1042

TOOL COND.

Data item

Meaning

I

INPUT

[INPUT] : Inputs a cutter compensation value directly.

[REF.]

: Inputs a cutter compensation number to

read a cutter compensation value by that

number.

D

TOOL DIAMETER

End mill diameter (positive value)

Remark) This item is indicated only when [INPUT] is

selected for INPUT.

M

CUTTER COMP.NO.

Cutter compensation number of an end mill (positive

value)

Remark) This item is indicated only when [REF.] is

selected for INPUT.

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.’

3 Tab ‘TOOL COND.’ is not enabled when bit 3 (PF3)

of parameter No. 27061 = 1.

CUT COND.

Data item

Meaning

K*

SIDE FINISH AMOUNT

Finishing allowance on the side face of a pocket.

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

value)

H*

BOTTOM FINISHI AMT.

Finishing allowance at the bottom of a pocket. The

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

F

FEED RATE- SING.CUT

Feedrate applicable when only the one-side cutter

portion of an end mill is used for cutting. This feedrate

is used for cutting in retract operation and on the side

face other than initial cutting.

V

FEED RATE- BOTH.CUT

Feedrate applicable when the entire front side of an

end mill is used for cutting. This feedrate is used for

initial cutting.

- 430 -

B-63874EN/05

CYCLE MACHINING TYPES

1.MILLING

CUT COND.

Data item

Meaning

E

FEED RATE- AXIS

Feedrate applicable when cutting is performed in the

tool axis direction toward the bottom of a side face

being machined

DETAIL

Data item

Meaning

W

UP CUT/DOWN CUT

[UP CUT]

: Performs machining in up-cut mode,

assuming that the tool is rotating

clockwise.

[DWNCUT] : Performs machining in down-cut mode,

assuming that the tool is rotating

clockwise.

(COPY)

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.

P

APPROACH TYPE

[ARC]

: Approaches a side face along an arc.

[TANGEN]: Approaches a side face along the straight

line tangent to the first figure in side face

cutting.

[VERTIC] : Approaches a side face along the straight

line normal to the first figure in side face

cutting.

(COPY)

R

APPROACH RAD./DIST.

Radius when [ARC] is specified.

Straight line length when [TANGEN] or [VERTIC] is

specified. (radius value, positive value)

Remark) By referring to the parameter No.27010

(minimum clamp value), the system sets the

data as Initial value.

A*

APPROACH ANGLE

Center angle of the arc when [ARC] is specified. The

default is 90 degrees. (positive value)

Remark) This data item is indicated only when [ARC]

is selected for APPROACH TYPE.

(COPY)

Q

ESCAPE TYPE

[ARC]

: Retracts from a side face along an arc.

[TANGEN]: Retracts from a side face along the

straight line tangent to the last figure in

side face cutting.

[VERTIC] : Retracts from a side face along the

straight line normal to the last figure in

side face cutting.

(COPY)

- 431 -

Content      ..     13      14      15      16     ..