Content      ..     5      6      7      8     ..

FANUC Series Series 16i-TB, Series 18i-TB, Series 160i-TB, Series 180i-TB. OPERATOR’S MANUAL - page 7

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

WARNING

Notes on this thread cutting are the same as in thread

cutting in G32. However, a stop by feed hold is as follows;

Stop after completion of path 3 of thread cutting cycle.

CAUTION

The tool retreats while chamfering and returns to the start

point on the X axis then the Z axis, as soon as the feed hold

status is entered during thread cutting (motion 2) when the

“Thread Cutting Cycle retract” option is used.

Ordinary cycle

Motion at feed hold

Stop point

Rapid traverse

Feed hold is effected here.

Another feed hold cannot be made during retreat. The

chamfered amount is the same as that at the end point.

159

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

D Taper thread cutting

cycle

G92X(U)__ Z(W)__ R__ F__ ; Lead (L) is specified.

X axis

Z

W

4(R)

(R) 0Rapid traverse

U/2

(F) 0Specified by

3(R)

1(R)

F code

2(F)

R

X/2

Z axis

L

(The chamfered angle in the left figure

is 45 degrees or less because of the

delay in the servo system.

Approx. 45°

r

Detailed chamfered thread

Fig. 13.1.2 (b) Taper thread cutting cycle

160

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

13.1.3

End Face Turning

Cycle (G94)

D Face cutting cycle

G94X(U)__ Z(W)__ F__ ;

X axis

(R)……Rapid traverse

(F)……Specified by F code

1(R)

2(F)

4(R)

U/2

3(F)

X/2

X/2

0

W

Z axis

Z

Fig. 13.1.3 (a) Face Cutting Cycle

In incremental programming, the sign of numbers following addresses U

and W depends on the direction of paths 1 and 2. That is, if the direction

of the path is in the negative direction of the Z axis, the value of W is

negative.

In single block mode, operations 1, 2, 3, and 4 are performed by pressing

the cycle start button once.

161

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

D Taper face cutting cycle

X axis

1(R)

(R) Rapid traverse

(F) Specified by F code

2(F)

4(R)

U/2

3(F)

X/2

R

W

Z axis

Z

Fig. 13.1.3 (b)

D Signs of numbers

In incremental programming, the relationship between the signs of the

specified in the taper

numbers following address U, W, and R, and the tool paths are as follows:

cutting cycle

1. U < 0, W < 0, R < 0

2. U > 0, W < 0, R < 0

X

X

1(R)

R

W

Z

Z

3(F)

U/2

2(F)

4(R)

U/2

2(F)

4(R)

3(F)

1(R)

R

W

3. U < 0, W < 0, R > 0

4. U > 0, W < 0, R<0

at  R  x

 W 

at  R  x  W 

X

X

R

W

Z

Z

3(F)

1(R)

U/2

2(F)

4(R)

U/2

2(F)

4(R)

3(F)

1(R)

W

R

162

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

NOTE

1

Since data values of X (U), Z (W) and R during canned cycle are

modal, if X (U), Z (W), or R is not newly commanded, the previously

specified data is effective. Thus, when the Z axis movement

amount does not vary as in the example below, a canned cycle can

be repeated only by specifying the movement commands for the

X-axis.

However, these data are cleared, if a one-shot G code expect for

G04 (dwell) or a G code in the group 01 except for G90, G92, G94

is commanded.

(Example)

X axis

66

4

8

12

16

Workpiece

0

Z axis

The cycle in the above figure is executed by the following program.

N030

G90 U-8.0 W-66.0 F0.4 ;

N031

U-16.0 ;

N032

U-24.0 ;

N033

U-32.0 ;

2

The following two applications can be performed.

(1) If an EOB or zero movement commands are specified for the

block following that specified with a canned cycle, the same

canned cycle is repeated.

(2) If the M, S, T function is commanded during the canned cycle

mode, both the canned cycle and M, S, or T function can be

performed simultaneously. If this is inconvenient, cancel the

canned cycle once as in the program examples below (specify

G00 or G01) and execute the M, S, or T command. After the

execution of M, S, or T terminates, command the canned cycle

again.

(Example)

N003 T0101 ;

:

:

N010

G90 X20.0 Z10.0 F0.2 ;

N011

G00 T0202 ;

N012

G90 X20.5 Z10.0 ;

163

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

13.1.4

An appropriate canned cycle is selected according to the shape of the

material and the shape of the product.

How to Use Canned

Cycles (G90, G92, G94)

D Straight cutting cycle

(G90)

Shape of material

Shape of product

D Taper cutting cycle (G90)

Shape of material

Shape of product

164

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

D Face cutting cycle (G94)

Shape of material

Shape of product

D Face taper cutting cycle

(G94)

Shape of material

Shape of product

165

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

This option canned cycles to make CNC programming easy. For instance,

13.2

the data of the finish work shape describes the tool path for rough

MULTIPLE

machining. And also, a canned cycles for the thread cutting is available.

REPETITIVE CYCLE

(G70-G76)

13.2.1

There are two types of stock removals in turning : Type I and II.

Stock Removal in

Turning (G71)

D Type I

If a finished shape of A to A′ to B is given by a program as in the figure

below, the specified area is removed by ∆d (depth of cut), with finishing

allowance ∆u/2 and ∆w left.

C

B

(R)

A

∆d

(R)

(F)

45,

e

(F)

Program command

(F) : Cutting feed

∆u/2

(R) : Rapid traverse

∆w

A′

G71 U (∆d) R (e) ;

G71 P (ns) Q (nf) U (∆u) W (∆w) F (f ) S (s ) T (t)

N (ns)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

F____

The move command between A and B is

S____

specified in the blocks from sequence

T____

number ns to nf.

N (nf)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅;

∆d

: Depth of cut (radius designation)

Designate without sign. The cutting direction depends on the direction AA′. This

designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter (No. 5132), and the parameter is

changed by the program command.

e

: Escaping amount

This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter (No. 5133), and the parameter

is changed by the program command.

ns

: Sequence number of the first block for the program of finishing shape.

nf

: Sequence number of the last block for the program of finishing shape.

∆u

: Distance and direction of finishing allowance in X direction (diameter / radius

designation).

∆w : Distance and direction of finishing allowance in Z direction.

f,s,t

: Any F , S, or T function contained in blocks ns to nf in the cycle is ignored, and the

F, S, or T function in this G71 block is effective.

Fig. 13.2.1 (a) Cutting Path in Stock Removal in Turning (Type I)

166

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

NOTE

1

While both ∆d and ∆u, are specified by address U, the

meanings of them are determined by the presence of

addresses P and Q.

2

The cycle machining is performed by G71 command with P

and Q specification.

F, S, and T functions which are specified in the move

command between points A and B are ineffective and those

specified in G71 block or the previous block are effective.

When an option of constant surface speed control is

selected, G96 or G97 command specified in the move

command between points A and B are ineffective, and that

specified in G71 block or the previous block is effective.

The following four cutting patterns are considered. All of

these cutting cycles are made paralleled to Z axis and the

sign of ∆u and ∆w are as follows:

+X

+Z

B

A

A

U(+)…W(+)

U(+)…W(-)

A′

A′

Both linear and cir-

A′ A′

cular interpolation

are possible

U(-)…W(+)

U(-)…W(-)

A

A

The tool path between A and A′ is specified in the block with

sequence number “ns” including G00 or G01, and in this

block, a move command in the Z axis cannot be specified.

The tool path between A′ and B must be steadily increasing

or decreasing pattern in both X and Z axis. When the tool

path between A and A′ is programmed by G00/G01, cutting

along AA′ is performed in G00/G01 mode respectively.

3

The subprogram cannot be called from the block between

sequence number “ns” and “nf”.

167

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

D Type II

Type II differs from type I in the following : The profile need not show

monotone increase or monotone decrease along the X axis, and it may

have up to 10 concaves (pockets).

10

3

2

1

Fig. 13.2.1 (b) Number of Pockets in Stock Removal in Turning (Type II)

Note that, however, the profile must have monotone decrease or increase

along the Z axis. The following profile cannot be machined:

Monotone change is not

observed along the Z axis

Fig. 13.2.1 (c) Figure Which Cannot Be Machined in Stock Removal in

Turning (Type II)

The first cut portion need not be vertical ; any profile is permitted if

monotone change is shown along the Z axis.

Fig. 13.2.1 (d) Figure Which Can Be Machined (Monotonic change) in

Stock Removal in Turning (Type II)

After turning, a clearance is provided by cutting along the workpiece

profile.

168

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

e (set by a parameter)

Fig. 13.2.1 (e) Chamfering in Stock Removal in Turning (Type II)

The clearance e (specified in R) to be provided after cutting can also be

set in parameter No. 5133.

A sample cutting path is given below:

30

4

3

13

5

1

29

2

12

18

14

9

24

10

6

23

8

25

11

19

15

7

16

17

22

20

26

21

28

27

Fig. 13.2.1 (f) Cutting Path in Stock Removal in Facing

The offset of the tool tip radius is not added to finishing allowances

∆u and ∆w. In turning, the offset of the tool tip radius is assumed to be

zero.

W=0 must be specified ; otherwise, the tool tip may cut into one wall side.

For the first block of a repetitive portion, two axes X (U) and Z (W) must

be specified. When Z motion is not performed, W0 is also specified.

D Distinction between type

When only one axis is specified in the first block of a repetitive portion

I and type II

Type I

When two axes are specified in the first block of a repetitive portion

Type II

When the first block does not include Z motion and type IIis to be used,

W0 must be specified.

(Example)

TYPE I

TYPE II

G71 V10.0 R5.0 ;

G71 V10.0 R5.0 ;

G71 P100 Q200

; G71 P100 Q200

;

N100X (U)___;

N100X (U)___ Z(W)___;

:

:

:

:

N200

;

N200

;

169

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

13.2.2

As shown in the figure below, this cycle is the same as G71 except that

cutting is made by a operation parallel to X axis.

Stock Removal in

Facing (G72)

∆d

C

A′

A

Tool path

(F)

(R)

e

(R)

45°

(F)

Program command

∆u/2

B

∆w

G72 W(∆d) R(e) ;

G72 P(ns) Q(nf) U(∆u) W(∆w) F(f) S(s) T(t) ;

The meanings of ∆d, e, ns, nf, ∆u,∆w, f, s, and t are the same as

those in G71.

Fig. 13.2.2 (a) Cutting Path in Stock Removal in Facing

D Signs of specified

The following four cutting patterns are considered. All of these cutting

numbers

cycles are made parallel to X axis and the sign of ∆u and ∆w are as follows:

+X

B

B

+Z

U(-)…W(+)…

U(-)…W(-)…

Both linear and circular

A′

A

A

A′

interpolation are possible

A

A

A′

A′

U(+)…W(+)…

U(+)…W(-)…

B B

Fig. 13.2.2 (b)

Signs of Numbers Specified with U and W in Stock Removal in Facing

The tool path between A and A′ is specified in the block with sequence

number “ns” including G00 or G01, and in this block, a move command

in the X axis cannot be specified. The tool path between A′ and B must

be steadily increasing and decreasing pattern in both X and Z axes.

Whether the cutting along AA′ is G00 or G01 mode is determined by the

command between A and A′, as described in item 13.2.1.

170

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

13.2.3

This function permits cutting a fixed pattern repeatedly, with a pattern

being displaced bit by bit. By this cutting cycle, it is possible to efficiently

Pattern Repeating

cut work whose rough shape has already been made by a rough

(G73)

machining, forging or casting method, etc.

∆k+∆w

D

∆w

∆i+∆u/2

C

∆u/2

A

(R)

B

∆u/2

A′

∆w

The pattern commanded in the program should be as follows.

A→A′→B

G73 U (ni) W (nk) R (d) ;

G73 P (ns) Q (nf) U (nu) W (nw) F (f ) S (s ) T (t) ;

N (ns)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅

The move command between A and B is

F____

specified in the blocks from sequence

S____

number ns to nf.

T____

N (nf)⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅⋅;

∆i

: Distance and direction of relief in the X axis direction (Radius designation).

This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5135, and the parameter

is changed by the program command.

∆k

: Distance and direction of relief in the Z axis direction.

This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5136, and the parameter

is changed by the program command.

d

: The number of division

This value is the same as the repetitive count for rough cutting. This designation

is modal and is not changed until the other value is designated. Also, this value

can be specified by the parameter No. 5137, and the parameter is changed by

the program command.

ns

: Sequence number of the first block for the program of finishing shape.

nf

: Sequence number of the last block for the program of finishing shape.

nu : Distance and direction of finishing allowance in X direction (diameter/radius

designation)

nw : Distance and direction of finishing allowance in Z direction

f,s,t

: Any F, S, and T function contained in the blocks between sequence number “ns”

and “nf” are ignored, and the F, S, and T functions in this G73 block are effective.

Fig. 13.2.3 Cutting path in Pattern Repeating

171

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

NOTE

1

While the values ∆i and ∆k, or ∆u and ∆w are specified by

address U and W respectively, the meanings of them are

determined by the presence of addresses P and Q in G73

block. When P and Q are not specified in a same block,

addresses U and W indicates ∆i and ∆k respectively. When

P and Q are specified in a same block, addreses U and W

indicates ∆u and ∆w respectively.

2

The cycle machining is performed by G73 command with P

and Q specification.

The four cutting patterns are considered. Take care of the

sign of ∆u, ∆w, ∆k, and ∆i.

When the machining cycle is terminated, the tool returns to

point A.

13.2.4

After rough cutting by G71, G72 or G73, the following command permits

finishing.

Finishing Cycle (G70)

Format

G70P (ns) Q (nf) ;

(ns) : Sequence number of the first block for the program of

finishing shape.

(nf) : Sequence number of the last block for the program of

finishing shape.

NOTE

1

F, S, and T functions specified in the block G71, G72, G73

are not effective but those specified between sequence

numbers “ns” and “nf” are effective in G70.

2

When the cycle machining by G70 is terminated, the tool is

returned to the start point and the next block is read.

3

In blocks between “ns” and “nf” referred in G70 through

G73, the subprogram cannot be called.

172

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

Examples

Stock Removal In Facing (G72)

X axis

7

Start point

88

110

Z axis

φ160

φ120

φ80

φ40

Å

ÅÅÅ

ÅÅÅ

ÅÅÅ

ÅÅ

Å

40

10

10 10

20

20

2

190

(Diameter designation, metric input)

N010 G50 X220.0 Z190.0 ;

N011 G00 X176.0 Z132.0 ;

N012 G72 W7.0 R1.0 ;

N013 G72 P014 Q019 U4.0 W2.0 F0.3 S550 ;

N014 G00 Z58.0 S700 ;

N015 G01 X120.0 W12.0 F0.15 ;

N016

W10.0 ;

N017

X80.0 W10.0 ;

N018

W20.0 ;

N019

X36.0 W22.0 ;

N020 G70 P014 Q019 ;

173

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

Pattern Repeating (G73)

16

B

X axis

16

110

130

14

2

Z axis

0

φ180

φ160

φ120

φ80

ÅÅ

ÅÅ

ÅÅ

2

14

ÅÅ

ÅÅ

20

ÅÅ

220

(Diameter designation, metric input)

N010 G50 X260.0 Z220.0 ;

N011 G00 X220.0 Z160.0 ;

N012 G73 U14.0 W14.0 R3 ;

N013 G73 P014 Q019 U4.0 W2.0 F0.3 S0180 ;

N014 G00 X80.0 W-40.0 ;

N015 G01 W-20.0 F0.15 S0600 ;

N017 W-20.0 S0400 ;

N018 G02 X160.0 W-20.0 R20.0 ;

N019 G01 X180.0 W-10.0 S0280 ;

N020 G70 P014 Q019 ;

174

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

13.2.5

The following program generates the cutting path shown in Fig. 13.2.5.

Chip breaking is possible in this cycle as shown below. If X (U) and Pare

End Face Peck Drilling

omitted, operation only in the Z axis results, to be used for drilling.

Cycle (G74)

Dk′

Dk

Dk

Dk

Dk

Dd

A

[0<Dk′xDk]

Di

C

(R)

(R)

(R)

(R)

(R)

(R)

(F)

U/2

(F)

(F)

(F)

(F)

Di

Di′

X

B

[0<Di′xDi]

W

Z

e

G74R (e) ;

G74X(U)_ Z(W)_ P(ni) Q(nk) R(nd) F (f ) ;

e

: Return amount

This designation is modal and is not changed until the other value is

designated. Also this value can be specified by the parameter No. 5139, and

the parameter is changed by the program command.

X

: X component of point B

U

: Incremental amount from A to B

Z

: Z component of point C

W

: Increment amount from A to C

∆i

: Movement amount in X direction (without sign)

∆k

: Depth of cut in Z direction (without sign)

∆d

: Relief amount of the tool at the cutting bottom. The sign of ∆d is always plus

(+). However, if address X (U) and ∆i are omitted, the relief direction can be

specified by the desired sign.

f

: Feed rate

Fig. 13.2.5 Cutting Path in End Face Peek Drilling Cycle

NOTE

1

While both e and nd are specified by address R, the

meanings of them are determined by the present of address

X (U). When X(U) is specified, nd is used.

2

The cycle machining is performed by G74 command with X

(U) specification.

175

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

13.2.6

The following program generates the cutting path shown in Fig. 13.2.6.

This is equivalent to G74 except that X is replaced by Z. Chip breaking

Outer Diameter /

is possible in this cycle, and grooving in X axis and peck drilling in X axis

Internal Diameter

(in this case, Z, W, and Q are omitted) are possible.

Drilling Cycle (G75)

(R)

A

Di

(F)

(R)

e

(F)

(R)

U/2

(F)

(R)

(F)

(R)

(F)

Dd

Dk

X

Z

W

G75R (e) ;

G75X(U)_ Z(W)_ P(∆i) Q(∆k) R(∆d) F(f) ;

Fig. 13.2.6

Cutting Path in Outer Diameter / Internal Diameter Drilling Cycle

Both G74 and G75 are used for grooving and drilling, and permit the tool

to relief automatically. Four symmetrical patterns are considered,

respectively.

176

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

13.2.7

The thread cutting cycle as shown in Fig.13.2.7 is programmed by the

G76 command.

Multiple Thread Cutting

Cycle (G76)

E

(R)

A

U/2

(R)

(F)

B

Dd

i

D

k

r

C

X

Z

W

Fig. 13.2.7 Cutting Path in Multiple thread cutting cycle

177

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

Tool tip

ÅÅ

ÅÅ

B

ÅÅ

ÅÅ

∆ d

ÅÅÅ aÅÅ

∆pn

1st

k

2nd

ÅÅÅÅÅ

3rd

th

ÅÅÅn

d

ÅÅ

Å

G76P (m) (r) (a) Q (∆d min) R(d);

G76X (u) _ Z(W) _ R(i) P(k) Q(∆d) F(L) ;

m

; Repetitive count in finishing (1 to 99)

This designation is modal and is not changed until the other value is

designated. Also this value can be specified by the parameter No.

5142, and the parameter is changed by the program command.

r

: Chamfering amount

When the thread lead is expressed by L, the value of L can be set from

0.0L to 9.9L in 0.1L increment (2-digit number from 00 to 90).

This designation is modal and is not changed until the other value is

designated. Also this value can be specified by the parameter No.

5130, and the parameter is changed by the program command.

a

: Angle of tool tip

One of six kinds of angle, 805, 605, 555, 305, 295, and 05, can be

selected, and specified by 2-digit number.

This designation is modal and is not changed until the other value is

designated. Also this value can be specified by the parameter No.

5143, and the parameter is changed by the program command.

m, r, and a are specified by address P at the same time.

(Example)

When m=2, r=1.2L, a=60°, specify as shown below (L is lead of thread).

02

12

60

P

m

r

a

∆dmin : Minimum cutting depth (specified by the radius value)

When the cutting depth of one cycle operation (∆d - ∆d -1) becomes

smaller than this limit, the cutting depth is clamped at this value. This

designation is modal and is not changed until the other value is

designated. Also this value can be specified by parameter No.

5140, and the parameter is changed by the program command.

d

: Finishing allowance

This designation is modal and is not changed until the other value

is designated. Also this value can be specified by parameter No.

5141, and the parameter is changed by the program command.

i

: Difference of thread radius If i = 0, ordinary straight thread cutting

can be made.

k

: Height of thread

This value is specified by the radius value.

nd

: Depth of cut in 1st cut (radius value)

L

: Lead of thread (same as G32).

Fig. 13.2.7 (b) Detail of cutting

178

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

Examples

Multiple repetitive cycle (G76)

X axis

0

1.8

1.8

ÔÔÔ

3.68

ϕ68

ϕ60.64

ÔÔ

Z axis

ÅÅ

G80 X80.0 Z130.0 ;

6

G76 P011060 Q100 R200 ;

G76 X60640 Z25000 P3680 Q1800 F6.0 ;

25

105

D Staggered thread cutting

Specifying P2 can perform staggered thread cutting with a constant depth

of cut.

Example: G76 X60640 Z25000 K3680 D1800 F6.0 A60 P2;

For staggered thread cutting, always use the FS15 tape format (see

Section 18.5).

If the depth of cut in one cycle is less than dmin (specified in parameter

No. 5140), the depth of cut is clamped at ∆dmin.

NOTE

Multiple repetitive cycle II is required.

Tool nose

(Ǹ2⋅Ǹ4) D/2

(Ǹ 4⋅ Ǹ6) D/2

Hn

a

Ǹ2⋅D

2

H1

Ǹ2⋅D

K

Ǹ4⋅D

H2

H3

H4

H5

H6

H7

H8

α (Finishing allowance)

H9

Staggered thread cutting with a constant depth of cut

180

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

The canned cycle for drilling simplifies the program normally by

13.3

directing the machining operation commanded with a few blocks, using

CANNED CYCLE FOR

one block including G code.

DRILLING (G80-G89)

This canned cycle conforms to JIS B 6314.

Following is the canned cycle table.

Table 13.3 (a) Canned Cycles

G code

Drilling

Hole machining

Operation in the

Retraction operation

Applications

axis

operation (- direction)

bottom hole position

(+ direction)

G80

____

_____

_____

___

Cancel

G83

Z axis

Cutting feed / intermittent

Dwell

Rapid traverse

Front drilling cycle

G84

Z axis

Cutting feed

Dwell→spindle CCW

Cutting feed

Front tapping cycle

G85

Z axis

Cutting feed

_____

Cutting feed

Front boring cycle

G87

X axis

Cutting feed / intermittent

Dwell

Rapid traverse

Side drilling cycle

G88

X axis

Cutting feed

Dwell→Spindle CCW

Cutting feed

Side tapping cycle

G89

X axis

Cutting feed

Dwell

Cutting feed

Side boring cycle

In general, the drilling cycle consists of the following six operation

sequences.

Operation 1 Positioning of X (Z) and C axis

Operation 2 Rapid traverse up to point R level

Operation 3 Hole machining

Operation 4 Operation at the bottom of a hole

Operation 5

Retraction to point R level

Operation 6

Rapid traverse up to the initial point

Operation 1

Initial level

Operation 2

Operation 6

Point R level

Operation 5

Operation 3

Rapid traverse

Operation 4

Feed

Fig. 13.3 Drilling Cycle Operation Sequence

182

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

Explanations

D Positioning axis and

A drilling G code specifies positioning axes and a drilling axis as shown

drilling axis

below. The C-axis and X- or Z-axis are used as positioning axes. The

X- or Z-axis, which is not used as a positioning axis, is used as a drilling

axis.

Although canned cycles include tapping and boring cycles as well as

drilling cycles, in this chapter, only the term drilling will be used to refer

to operations implemented with canned cycles.

Table13.3 (b) Positioning axis and drilling axis

G code

Positioning plane

Drilling axis

G83, G84, G85

X axis, C axis

Z axis

G87, G88, G89

Z axis, C axis

X axis

G83 and G87, G84 and G88, and G85 and G89 have the same function

respectively except for axes specified as positioning axes and a drilling

axis.

D Drilling mode

G83AG85 / G87A89 are modal G codes and remain in effect until

canceled. When in effect, the current state is the drilling mode.

Once drilling data is specified in the drilling mode, the data is retained

until modified or canceled.

Specify all necessary drilling data at the beginning of canned cycles; when

canned cycles are being performed, specify data modifications only.

D Return point level

In G code system A, the tool returns to the initial level from the bottom

G98/G99

of a hole. In G code system B or C, specifying G98 returns the tool to the

initial level from the bottom of a hole and specifying G99 returns the tool

to the point-R level from the bottom of a hole.

The following illustrates how the tool moves when G98 or G99 is

specified. Generally, G99 is used for the first drilling operation and G98

is used for the last drilling operation.

The initial level does not change even when drilling is performed in the

G99 mode.

G98 (Return to initial level)

G99 (Return to point R level)

Initial level

Point R level

183

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

D Number of repeats

To repeat drilling for equally-spaced holes, specify the number of repeats

in K_.

K is effective only within the block where it is specified.

Specify the first hole position in incremental mode.

If it is specified in absolute mode, drilling is repeated at the same position.

Number of repeats K The maximum command value = 9999

When K0 is specified with parameter K0E (parameter No. 5102 #4) set

to 0, drilling is performed once.

When K0 is specified with parameter K0E (parameter No. 5102 #4) set

to 1, drilling data is just stored without drilling being performed.

D M code used for C-axis

When an M code specified in parameter No. 5110 for C-axis clamp /

clamp/unclamp

unclamp is coded in a program, the CNC issues the M code for C-axis

clamp after the tool is positioned and before the tool is fed in rapid traverse

to the point-R level. The CNC also issues the M code for C-axis unclamp

(the M code for C-axis clamp +1) after the tool retracts to the point-R

level. The tool dwells for the time specified in parameter No. 5111.

D Cancel

To cancel a canned cycle, use G80 or a group 01 G code.

Group 01 G codes

G00 : Positioning (rapid traverse)

G01 : Linear interpolation

G02 : Circular interpolation (CW)

G03 : Circular interpolation (CCW)

D Symbols in figures

Subsequent sections explain the individual canned cycles. Figures in

these explanations use the following symbols:

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01)

Manual feed

P1

Dwell specified in the program

P1

Dwell specified in parameter No.5111

Mα

Issuing the M code for C-axis clamp

(The value of a is specified with parameter No. 5110.)

M (α+1) Issuing the M code for C-axis unclamp

184

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

13.3.1

The peck drilling cycle or high-speed peck drilling cycle is used

depending on the setting in RTR, bit 2 of parameter No. 5101. If depth

Front Drilling Cycle

of cut for each drilling is not specified, the normal drilling cycle is used.

(G83) / Side Drilling

Cycle (G87)

D High-speed peck

This cycle performs high-speed peck drilling. The drill repeats the cycle

drilling cycle (G83, G87)

of drilling at the cutting feedrate and retracting the specified retraction

(parameter RTR

distance intermittently to the bottom of a hole. The drill draws cutting

(No. 5101#2) =0)

chips out of the hole when it retracts.

Format

G83 X(U)_ C(H)_ Z(W)_ R_ Q_ P_ F_ K_ M_ ;

or

G87 Z(W)_ C(H)_ X(U)_ R_ Q_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data

Z_ or X_

: The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

Q_ : Depth of cut for each cutting feed

P_ : Dwell time at the bottom of a hole

F_ : Cutting feedrate

K_ : Number of repeats (When it is needed)

M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Mα

Mα

Initial level

M (a+1), P2

Point R

M (α+1)

Point R

Point R

P2

q

q

d

d

q

q

d

d

q

q

P1

Point Z

P1

Point Z

Mα

: M code for C-axis clamp

M(α+1)

: M code for C-axis unclamp

P1

: Dwell specified in the program

P2

: Dwell specified in parameter No. 5111

d

: Retraction distance specified in parameter No. 5114

186

13. FUNCTIONS TO SIMPLIFY

B-63524EN/01

PROGRAMMING

PROGRAMMING

D Peck drilling cycle

(G83, G87) (parameter

No. 5101#2 =1)

Format

G83 X(U)_ C(H)_ Z(W)_ R_ Q_ P_ F_ K_ M_ ;

or

G87 Z(W)_ C(H)_ X(U)_ R_ Q_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data

Z_ or X_

: The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

Q_ : Depth of cut for each cutting feed

P_ : Dwell time at the bottom of a hole

F_ : Cutting feedrate

K_ : Number of repeats (When it is needed.)

M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Mα

Initial level

Mα

M (a+1), P2

Point R

M (a+1),

Point R

Point R

P2

q

q

d

d

q

q

d

d

q

q

Point Z

Point Z

P1

P1

Mα

: M code for C-axis clamp

M(α+1)

: M code for C-axis unclamp

P1

: Dwell specified in the program

P2

: Dwell specified in parameter No. 5111

d

: Retraction distance specified in parameter No. 5114

Examples

M51 ;

Setting C-axis index mode ON

M3 S2000 ;

Rotating the drill

G00 X50.0 C0.0 ;

Positioning the drill along the X- and

C-axes

G83 Z-40.0 R-5.0 Q5000 F5.0 M31 ; Drilling hole 1

C90.0 Q5000 M31 ;

Drilling hole 2

C180.0 Q5000 M31 ;

Drilling hole 3

C270.0 Q5000 M31 ;

Drilling hole 4

G80 M05 ;

Canceling the drilling cycle and

stopping drill rotation

M50 ;

Setting C-axis index mode off

187

13. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING

B-63524EN/01

NOTE

If the depth of cut for each cutting feed

(Q) is not

commanded, normal drilling is performed.

(See the

description of the drilling cycle.)

D Drilling cycle

If depth of cut is not specified for each drilling, the normal drilling cycle

(G83 or G87)

is used. The tool is then retracted from the bottom of the hole in rapid

traverse.

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

or

G87 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data

Z_ or X_

: The distance from point R to the bottom of the hole

R_ : The distance from the initial level to point R level

P_ : Dwell time at the bottom of a hole

F_ : Cutting feedrate

K_ : Number of repeats (When it is needed.)

M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode)

G83 or G87 (G99 mode)

Mα

Mα

Initial level

Point R level

Point R level

M (a+1), P2

M (a+1), P2

Point Z

Point Z

P1

P1

Mα

: M code for C-axis clamp

M(a+1)

: M code for C-axis unclamp

P1

: Dwell specified in the program

P2

: Dwell specified in parameter No. 5111

188

Content      ..     5      6      7      8     ..