Content .. 8 9 10 11 ..

FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 10

2.CONTROLLED AXES

PROGRAMMING

B-63944EN/03

- 36 -

2.2

NAMES OF AXES

Explanation

The move axes of machine tools are assigned names. These names are
referred to as addresses or axis names. Axis names are determined
according to the machine tool. The naming rules comply with
standards such as the ISO standards.
With complex machines, one character would become insufficient for
representing axis names. So, up to three characters can be used for
axis names. A move axis may be named "X", "X1", or "XA1". The
first character of the three characters is called the first axis name
character, the second character is called the second axis name
character, and third character is called the third axis name character.
Example)

X A 1

3rd axis name character

2nd axis name character

1st axis name character

NOTE

1 Axis names are predetermined according to the

machine used. Refer to the manual supplied by the
machine tool builder.

2 Since many ordinary machines use one character

to represent each address, one-character
addresses are used in the description in this
manual.

B-63944EN/03

PROGRAMMING

2.CONTROLLED AXES

- 37 -

2.3

INCREMENT SYSTEM

Explanation

The increment system consists of the least input increment (for input)
and least command increment (for output). The least input increment
is the least increment for programming the travel distance. The least
command increment is the least increment for moving the tool on the
machine. Both increments are represented in mm, inches, or deg.
Five types of increment systems are available as indicated in Table 2.3
(a). For each axis, an increment system can be set using a bit from bit
0 to bit 3 (ISA, ISC, ISD, or ISE) of parameter No. 1013.
IS-C, IS-D, and IS-E are optional functions.

Table 2.3 (a) Increment system

Name of increment

system

Least input increment

Least command

increment

0.01 mm 0.01 mm
0.001 inch

0.001 inch

IS-A

0.01 deg 0.01 deg
0.001 mm

0.001 mm

0.0001 inch

IS-B

0.001 deg

0.0001 mm

0.00001 inch

IS-C

0.0001 deg

0.00001 mm

0.000001 inch

IS-D

0.00001 deg

0.000001 mm

0.0000001 inch

IS-E

0.000001 deg

The least command increment is either metric or inch depending on
the machine tool. Set metric or inch to the parameter INM
(No.0100#0).
For selection between metric and inch for the least input increment, G
code (G20 or G21) or a setting parameter selects it.
Combined use of the inch system and the metric system is not allowed.
There are functions that cannot be used between axes with different
unit systems (circular interpolation, cutter compensation, etc.). For the
increment system, see the machine tool builder's manual.

NOTE

1 The unit (mm or inch) in the table is used for

indicating a diameter value for diameter programming
(when bit 3 (DIA) of parameter No. 1006 is set to 1)
or a radius value for radius programming.

2 Some increment systems are unavailable depending

on the model. For details, refer to “Descriptions” (B-
63942EN).

2.CONTROLLED AXES

PROGRAMMING

B-63944EN/03

- 38 -

2.4

MAXIMUM STROKE

Explanation

The maximum stroke controlled by this CNC is shown in the table
below:
Maximum stroke = Least command increment

999999999

(99999999 for IS-A)
Commands that exceed the maximum stroke are not permitted.

Table 2.4 (a) Maximum strokes

Name of increment

system

Least input increment Maximum

stroke

0.01 mm

999999.99 mm

0.001 inch

99999.999 inch

IS-A

0.01 deg

999999.99 deg

0.001 mm

999999.999 mm

0.0001 inch

99999.9999 inch

IS-B

0.001 deg

999999.999 deg

0.0001 mm

99999.9999 mm

0.00001 inch

9999.99999 inch

IS-C

0.0001 deg

99999.9999 deg

0.00001 mm

9999.99999 mm

0.000001 inch

999.999999 inch

IS-D

0.00001 deg

9999.99999 deg

0.000001 mm

999.999999 mm

0.0000001 inch

99.9999999 inch

IS-E

0.000001 deg

999.999999 deg

NOTE

1 The actual stroke depends on the machine tool.
2 The unit (mm or inch) in the table is used for

indicating a diameter value for diameter
programming (when bit 3 (DIA) of parameter No.
1006 is set to 1) or a radius value for radius
programming.

3 Some increment systems are unavailable

depending on the model. For details, refer to
"Descriptions" (B-63942EN).

B-63944EN/03

PROGRAMMING

- 39 -

3.PREPARATORY FUNCTION

(G FUNCTION)

PREPARATORY FUNCTION
(G FUNCTION)

A number following address G determines the meaning of the
command for the concerned block.
G codes are divided into the following two types.

Type Meaning

One-shot G code

The G code is effective only in the block in which it
is specified.

Modal G code

The G code is effective until another G code of the
same group is specified.

(Example)

G01 and G00 are modal G codes in group 01.
G01 X_ ;

Z_ ; G01 is effective in this range.

;

G00 Z_ ; G00 is effective in this range.
X_

;

G01 X_ ;
:

There are three G code systems in the lathe system: A, B, and C
(Table 3.1(a)). Select a G code system using bits 6 (GSB) and 7
(GSC) of parameter No. 3401. To use G code system B or C, the
corresponding option is needed. Generally, User’s Manual describes
the use of G code system A, except when the described item can use
only G code system B or C. In such cases, the use of G code system B
or C is described.

PROGRAMMING

B-63944EN/03

- 40 -

3. PREPARATORY FUNCTION

(G FUNCTION)

Explanation

1. When the clear state (bit 6 (CLR) of parameter No. 3402) is set at

power-up or reset, the modal G codes are placed in the states
described below.
(1) The modal G codes are placed in the states marked with

as indicated in Table.

(2) G20 and G21 remain unchanged when the clear state is set

at power-up or reset.

(3) Which status G22 or G23 at power on is set by bit 7 (G23)

of parameter No. 3402. However, G22 and G23 remain
unchanged when the clear state is set at reset.

(4) The user can select G00 or G01 by setting parameter G01

(No. 3402#0).

(5) The user can select G90 or G91 by setting parameter G91

(No. 3402#3).

When G code system B or C is used in the lathe system,
setting bit 3 (G91) of parameter No. 3402 determines which
code, either G90 or G91, is effective.

(6) In the machining center system, the user can select G17,

G18, or G19 by setting bits 1 (G18) and 2 (G19) of
parameter No. 3401.

2. G codes other than G10 and G11 are one-shot G codes.
3. When a G code not listed in the G code list is specified, or a G

code that has no corresponding option is specified, alarm PS0010
occurs.

4. Multiple G codes can be specified in the same block if each G

code belongs to a different group. If multiple G codes that belong
to the same group are specified in the same block, only the last G
code specified is valid.

5. If a G code belonging to group 01 is specified in a canned cycle

for drilling, the canned cycle for drilling is cancelled. This means
that the same state set by specifying G80 is set. Note that the G
codes in group 01 are not affected by a G code specifying a
canned cycle for drilling.

6. G codes are indicated by group.
7. The group of G60 is switched according to the setting of bit 0

(MDL) of parameter No. 5431. (When the MDL bit is set to 0,
the 00 group is selected. When the MDL bit is set to 1, the 01
group is selected.)

8. When G code system A is used, absolute or incremental

programming is specified not by a G code (G90/G91) but by an
address word (X/U, Z/W, C/H, Y/V). Only the initial level is
provided at the return point of the canned cycle for drilling..

B-63944EN/03

PROGRAMMING

- 41 -

3.PREPARATORY FUNCTION

(G FUNCTION)

3.1

G CODE LIST IN THE MACHINING CENTER SYSTEM

Table 3.1 (a) G code list

G code

Group

Function

G00

Positioning (rapid traverse)

G01

Linear interpolation (cutting feed)

G02

Circular interpolation CW or helical interpolation CW

G03

Circular interpolation CCW or helical interpolation CCW

G02.2, G03.2

Involute interpolation CW/CCW

G02.3, G03.3

Exponential interpolation CW/CCW

G02.4, G03.4

Three-dimensional coordinate system conversion CW/CCW

G04

Dwell

G05

AI contour control (high-precision contour control compatible command),
High-speed cycle machining

G05.1

AI contour control / Nano smoothing / Smooth interpolation

G05.4

HRV3, 4 on/off

G06.2 01

NURBS

interpolation

G07

Hypothetical axis interpolation

G07.1 (G107)

Cylindrical interpolation

G08

AI contour control (advanced preview control compatible command)

G09 Exact

stop

G10

Programmable data input

G10.6

Tool retract and recover

G10.9 Programmable

switching

diameter/radius specification

G11

Programmable data input mode cancel

G12.1

Polar coordinate interpolation mode

G13.1

Polar coordinate interpolation cancel mode

G15

Polar coordinates command cancel

G16

Polar coordinates command

G17

XpYp plane selection

G18 ZpXp

plane

selection

G19

YpZp plane selection

Xp: X axis or its parallel axis
Yp: Y axis or its parallel axis
Zp: Z axis or its parallel axis

G20 (G70)

Input in inch

G21 (G71)

Input in mm

G22

Stored stroke check function on

G23

Stored stroke check function off

G25

Spindle speed fluctuation detection off

G26

Spindle speed fluctuation detection on

G27

Reference position return check

G28 Automatic

return

to reference position

G29

Movement from reference position

G30

2nd, 3rd and 4th reference position return

G30.1

Floating reference position return

G31 Skip

function

G31.8

EGB-axis skip

G33 Threading
G34

Variable lead threading

G35

Circular threading CW

G36

Circular threading CCW

PROGRAMMING

B-63944EN/03

- 42 -

3. PREPARATORY FUNCTION

(G FUNCTION)

Table 3.1 (a) G code list

G code

Group

Function

G37

Automatic tool length measurement

G38

Tool radius/tool nose radius compensation : preserve vector

G39

Tool radius/tool nose radius compensation : corner circular interpolation

G40

Tool radius/tool nose radius compensation : cancel
3-dimensional cutter compensation : cancel

G41

Tool radius/tool nose radius compensation : left
3-dimensional cutter compensation : left

G42

Tool radius/tool nose radius compensation : right
3-dimensional cutter compensation : right

G41.2

3-dimensional cutter compensation : left (type 1)

G41.3

3-dimensional cutter compensation : leading edge offset

G41.4

3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)

G41.5

3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)

G41.6

3-dimensional cutter compensation : left (type 2)

G42.2

3-dimensional cutter compensation : right (type 1)

G42.4

3-dimensional cutter compensation : right (type 1) (FS16i-compatible command)

G42.5

3-dimensional cutter compensation : right (type 1) (FS16i-compatible command)

G42.6

3-dimensional cutter compensation : right (type 2)

G40.1

Normal direction control cancel mode

G41.1

Normal direction control on : left

G42.1

Normal direction control on : right

G43

Tool length compensation +

G44

Tool length compensation -

G43.1

Tool length compensation in tool axis direction

G43.4

Tool center point control (type 1)

G43.5

Tool center point control (type 2)

G45

Tool offset : increase

G46

Tool offset : decrease

G47

Tool offset : double increase

G48

Tool offset : double decrease

G49 (G49.1)

Tool length compensation cancel

G50 Scaling

cancel

G51

Scaling

G50.1

Programmable mirror image cancel

G51.1

Programmable mirror image

G50.2

Polygon turning cancel

G51.2

Polygon turning

G50.4

Cancel synchronous control

G50.5

Cancel composite control

G50.6

Cancel superimposed control

G51.4

Start synchronous control

G51.5

Start composite control

G51.6

Start superimposed control

G52

Local coordinate system setting

G53

Machine coordinate system setting

G53.1

Tool axis direction control

B-63944EN/03

PROGRAMMING

- 43 -

3.PREPARATORY FUNCTION

(G FUNCTION)

Table 3.1 (a) G code list

G code

Group

Function

G54 (G54.1)

Workpiece coordinate system 1 selection

G55

Workpiece coordinate system 2 selection

G56

Workpiece coordinate system 3 selection

G57

Workpiece coordinate system 4 selection

G58

Workpiece coordinate system 5 selection

G59

Workpiece coordinate system 6 selection

G54.2

Rotary table dynamic fixture offset

G54.4

Workpiece setting error compensation

G60

Single direction positioning

G61

Exact stop mode

G62

Automatic corner override

G63 Tapping

mode

G64

Cutting mode

G65 00

Macro

call

G66

Macro modal call A

G66.1

Macro modal call B

G67

Macro modal call A/B cancel

G68

Coordinate system rotation start or three-dimensional coordinate conversion mode on

G69

Coordinate system rotation cancel or three-dimensional coordinate conversion mode off

G68.2

Tilted working plane command

G68.3

Tilted working plane command by tool axis direction

G68.4

Tilted working plane command (incremental multi-command)

G70.7 Finishing

cycle

G71.7

Outer surface rough machining cycle

G72.7

End rough machining cycle

G73.7

Closed loop cutting cycle

G74.7

End cutting off cycle

G75.7

Outer or inner cutting off cycle

G76.7

Multiple threading cycle

G72.1

Figure copying (rotary copy)

G72.2

Figure copying (linear copy)

G73

Peck drilling cycle

G74

Left-handed tapping cycle

G75

Plunge grinding cycle

G76

Fine boring cycle

G77

Plunge direct sizing/grinding cycle

G78 Continuous-feed

surface grinding cycle

G79

Intermittent-feed surface grinding cycle

G80 09

Canned cycle cancel
Electronic gear box : synchronization cancellation

G80.4

Electronic gear box: synchronization cancellation

G81.4

Electronic gear box: synchronization start

G80.5

Electronic gear box 2 pair: synchronization cancellation

G81.5

Electronic gear box 2 pair: synchronization start

G81 09

Drilling cycle or spot boring cycle
Electronic gear box : synchronization start

G81.1

Chopping

Content .. 8 9 10 11 ..