FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 32

8.COORDINATE VALUE AND DIMENSION

 PROGRAMMING 

B-63944EN/03

 

 

- 212 - 

8.2 

INCH/METRIC CONVERSION (G20, G21) 

 
Either inch or metric input (least input increment) can be selected by 
G code. 
 

Format 

G20 ;

 Inch 

input 

G21 ;

 Metric 

input 

 
This G code must be specified in an independent block before setting 
the coordinate system at the beginning of the program. After the G 
code for inch/metric conversion is specified, the unit of input data is 
switched to the least inch or metric input increment of increment 
system (II-2.3). The unit of data input for degrees remains unchanged.   
The unit systems for the following values are changed after 
inch/metric conversion: 

•

 Feedrate commanded by F code 

•

 Positional command   

•

 Workpiece origin offset value   

•

 Tool compensation value 

•

 Unit of scale for manual pulse generator 

•

 Movement distance in incremental feed 

•

 Some parameters 

When the power is turned on, the G code is the same as that held 
before the power was turned off. 
 

 WARNING 

 

G20 and G21 must not be switched during a 
program. 

 

NOTE 

1  When the least input increment and the least 

command increment systems are different, the 
maximum error is half of the least command 
increment. This error is not accumulated. 

2  The inch and metric input can also be switched 

using settings (see III-12.3.1). 

3  If a function selected using bit 2 (IRF) of parameter 

No. 14000 or bit 0 (NIM) of parameter No. 11222 is 
not used, be sure to perform inch/metric conversion 
at the reference position (machine coordinate 
system origin). 

 

B-63944EN/03

 PROGRAMMING 

8.COORDINATE VALUE AND DIMENSION

 

 

- 213 - 

Performing inch/metric conversion in the reference position (parameter No. 1240 is 
not 0) 

 
Conventionally, inch/metric conversion must be performed at the 
machine coordinate system origin.  However, setting bit 2 (IRF) of 
parameter No. 14000 to 1 enables inch/metric conversion to be 
performed in the reference position (parameter No. 1240). 
 
If an attempt is made to perform inch/metric conversion when an axis 
with this function enabled is not in the reference position, alarm 
PS5362 is issued to cancel the attempt. 
Before trying to perform inch/metric conversion, be sure to set the 
axis of interest to the reference position, using the G28 command, for 
example. 
 
In addition, if the workpiece coordinate system has been shifted from 
the machine coordinate system, using the following commands or 
operations, bit 1 (CIM) of parameter No. 11222 can be used to select 
whether to issue alarm PS1298 or to clear the offset. 

•

 

Manual intervention performed with the manual absolute signal 
being off 

•

 

Move command issued with the machine locked 

•

 

Move command issued using a handle interrupt 

•

 

Mirror image-based operation 

•

 

Workpiece coordinate system shift caused by local coordinate 
system setting (G52) or workpiece coordinate system setting 
(G92) 

 

Switching conditions 

Performing inch/metric conversion in any position other than the 
reference position requires satisfying all of the following conditions.   
Failing to satisfy any of the conditions results in alarm PS1298 being 
issued.    For electronic gear box 2 pair synchronization or electronic 
gear box synchronization, alarm PS1595 is issued. 

•

 

Positioning or linear interpolation 

•

 

Polar coordinate interpolation cancel mode 

•

 

Polar coordinate command cancel 

•

 

Spindle Speed fluctuation detection off 

•

 Tool 

radius 

⋅

 tool nose radius compensation cancel / 

3-dimensional tool compensation cancel 

•

 

Normal direction control cancel 

•

 

Tool length offset cancel 

•

 Scaling 

cancel 

•

 

Programmable mirror image cancel 

•

 

Polygon turning cancel 

•

 

Macro modal call A/B cancel 

•

 

Coordinate system rotation or 3-dimensional coordinate system 
conversion mode off 

•

 

Mirror image for double turret or balanced cutting mode cancel 
(T series only) 

•

 

Canned cycle cancel 

8.COORDINATE VALUE AND DIMENSION

 PROGRAMMING 

B-63944EN/03

 

 

- 214 - 

•

 

Electronic gear box 2 pair synchronization cancel 

•

 

Electronic gear box synchronization cancel 

•

 

Constant surface speed control cancel 

 
In addition, performing inch/metric conversion in any position other 
than the reference position requires the following options.

 

•

 Inch/metric 

conversion 

•

 

Workpiece coordinate system 

 

Restrictions 

When performing the following operations, make sure that the axis of 
interest is in the reference position (machine coordinate system 
origin). 

•

 

Inch/metric conversion based on bit 2 (INI) of setting parameter 
No. 0 

•

 

Inch/metric conversion based on programmable parameter input 
(G10) 

•

  Inch/metric conversion based on custom macro variable No. 

3005 

 

Performing inch/metric conversion in positions other than the reference position 

Setting bit 0 (NIM) of parameter No. 11222 enables inch/metric 
conversion to be performed even in positions other than the reference 
position. 
 
In addition, if the workpiece coordinate system has been shifted from 
the machine coordinate system, using the following commands or 
operations, bit 1 (CIM) of parameter No. 11222 can be used to select 
whether to issue alarm PS1298 or to clear the offset. 

•

 

Manual intervention performed with the manual absolute signal 
being off 

•

 

Move command issued with the machine locked 

•

 

Move command issued using a handle interrupt 

•

 

Mirror image-based operation 

•

 

Workpiece coordinate system shift caused by local coordinate 
system setting (G52) or workpiece coordinate system setting 
(G92) 

 
If an axis is under any of the following controls, however, no 
automatic coordinate system conversion based on this function can be 
carried out for the axis. 

•

 

Axis control by PMC 

•

 

Axis synchronous control (for slave axes when the master axis is 
a PMC axis) 

•

 

Flexible synchronous control (for slave axes when the master 
axis is a PMC axis) 

•

 Chopping 

•

 

Spindle control with servo motor 

•

 

Spindle control with Cs contour control 

•

 

Servo/spindle synchronous control 

 

B-63944EN/03

 PROGRAMMING 

8.COORDINATE VALUE AND DIMENSION

 

 

- 215 - 

Switching conditions 

Performing inch/metric conversion in any position other than the 
reference position requires satisfying all of the following conditions.   
Failing to satisfy any of the conditions results in alarm PS1298 being 
issued.    For electronic gear box 2 pair synchronization or electronic 
gear box synchronization, alarm PS1595 is issued. 

•

 

Positioning or linear interpolation 

•

 

Polar coordinate interpolation cancel mode 

•

 

Polar coordinate command cancel 

•

 

Spindle Speed fluctuation detection off 

•

 Tool 

radius 

⋅

 tool nose radius compensation cancel / 

3-dimensional tool compensation cancel 

•

 

Normal direction control cancel 

•

 

Tool length offset cancel 

•

 Scaling 

cancel 

•

 

Programmable mirror image cancel 

•

 

Polygon turning cancel 

•

 

Macro modal call A/B cancel 

•

 

Coordinate system rotation or 3-dimensional coordinate system 
conversion mode off 

•

 

Mirror image for double turret or balanced cutting mode cancel 
(T series only) 

•

 

Canned cycle cancel 

•

 

Electronic gear box 2 pair synchronization cancel 

•

 

Electronic gear box synchronization cancel 

•

 

Constant surface speed control cancel 

 
In addition, performing inch/metric conversion in any position other 
than the reference position requires the following options.

 

•

 Inch/metric 

conversion 

•

 

Workpiece coordinate system 

•

 

Workpiece coordinate system preset 

 

Restrictions 

When performing the following operations, make sure that the axis of 
interest is in the reference position (machine coordinate system 
origin). 

•

 

Inch/metric conversion based on bit 2 (INI) of setting parameter 
No. 0 

•

 

Inch/metric conversion based on programmable parameter input 
(G10) 

•

  Inch/metric conversion based on custom macro variable No. 

3005 

 

8.COORDINATE VALUE AND DIMENSION

 PROGRAMMING 

B-63944EN/03

 

 

- 216 - 

8.3 

DECIMAL POINT PROGRAMMING 

 
Numerical values can be entered with a decimal point. A decimal 
point can be used when entering a distance, time, or speed. Decimal 
points can be specified with the following addresses: 
 

M

 

X, Y, Z, U, V, W, A, B, C, I, J, K, Q, R, F 

 

T

 

X, Y, Z, U, V, W, A, B, C, I, J, K, R, F 

 

Explanation 

There are two types of decimal point notation: calculator-type notation 
and standard notation. 
When calculator-type decimal notation is used, a value without 
decimal point is considered to be specified in millimeters inch, or deg.   
When standard decimal notation is used, such a value is considered to 
be specified in least input increments.  Select either calculator-type 
or standard decimal notation by using the bit 0 (DPI) of parameter 
No.3401.Values can be specified both with and without decimal point 
in a single program. 
 

Example 

Program command

Pocket calculator 

type decimal point 

programming 

Standard type decimal point 

programming 

X1000 
Command value 
without decimal point

1000mm 
Unit :mm 

1mm 
Unit : Least input increment 
(0.001mm) 

X1000.0 
Command value with 
decimal point 

1000mm 
Unit :mm 

1000mm 
Unit :mm 

 

 CAUTION 

 

When specifying a dimension word for a command 
G code in a block, be sure to place the dimension 
word after the command G code. 

 

B-63944EN/03

 PROGRAMMING 

8.COORDINATE VALUE AND DIMENSION

 

 

- 217 - 

NOTE 

1  A specified value less than the minimum unit is 

treated as described below. 

Example 1) 
  When a value is specified directly at an address 

(in the case of IS-B) 
 X1.2345 ;    Treated as X1.235 
 X-1.2345 ;   Treated as X-1.234 

Example 2) 
  When a value is assigned to a macro variable (in 

the case of IS-B) 
 #100=1.2345;  
 X#100 ;     Treated as X1.235 
 #100=-1.2345;  
 X#100 ;     Treated as X-1.234 

2  When more than eight digits are specified, an 

alarm occurs. If a value is entered with a decimal 
point, the number of digits is also checked after the 
value is converted to an integer according to the 
least input increment. 

Examples: 
 X1.23456789; 

Alarm PS0003 occurs because more than 
eight digits are specified. 

 X123456.7; 

If the least input increment is 0.001 mm, the 
value is converted to integer 123456700. 
Because the integer has more than eight 
digits, an alarm occurs. 

 

8.COORDINATE VALUE AND DIMENSION

 PROGRAMMING 

B-63944EN/03

 

 

- 218 - 

8.4 

DIAMETER AND RADIUS PROGRAMMING 

 
Since the workpiece cross section is usually circular in CNC lathe 
control programming, its dimensions can be specified in two ways : 
Diameter and Radius 
 

Z axis

A

B

D

1

X axis

D

2

R

1

R

2

D1, D2 : Diameter programming

R1, R2 : Radius programming

When the diameter is specified, it is called diameter programming and 
when the radius is specified, it is called radius programming. 
 

Explanation 
  - Notes on diameter programming/radius programming for each command 

Radius programming or diameter programming can be specified by bit 
3 (DIA) of parameter No.1006. When using diameter programming, 
note the conditions listed in the Table 8.4 (a). 
 

Table 8.4 (a)    Notes on specifying diameter value 

Item Notes 

X axis command 

Specified with a diameter value 

Incremental command 

Specified with a diameter value 
In the above figure, specifies D2 
minus D1 for tool path B to A. 

Coordinate system setting (G50) 

Specifies a coordinate value with a 
diameter value 

Component of tool offset value 

Bit 1 of parameter No.5004 
determines either diameter or radius 
value 

Parameters in canned cycle, such 
as cutting depth along X axis. (R) 

Specifies a radius value 

Radius designation in circular 
interpolation (R, I, K, and etc.) 

Specifies a radius value 

Feedrate along axis 

Specifies change of radius/rev. or 
change of radius/min. 

Display of axis position 

Displayed as diameter value 

 

B-63944EN/03

 PROGRAMMING 

8.COORDINATE VALUE AND DIMENSION

 

 

- 219 - 

8.5 

DIAMETER AND RADIUS SETTING SWITCHING 
FUNCTION 

 

Overview 

Usually, whether to use diameter specification or radius specification 
to specify a travel distance on each axis is uniquely determined by the 
setting of bit 3 (DIAx) of parameter No. 1006.  However, this 
function enables switching between diameter specification and radius 
specification by using a signal or G code. 
Thus, a coordinate, program, and so forth can be specified by 
switching between diameter specification and radius specification for 
each controlled axis. 
 

Explanation 
  - Selection of a diameter/radius specification switching method 

Two methods are available for switching between diameter 
specification and radius specification: 
1)  Signal 
2)  G code 
Use bit 5 (PGD) of parameter No. 3400 to determine which method to 
use. 
 

  - Switching method using a signal 

For switching between diameter specification and radius specification, 
set the diameter/radius specification switch signal from DI1 to DI8 
(input signals) corresponding to a desired axis, from 0 to 1.

 

If an input signal is set from 0 to 1, and radius specification is selected 
(with bit 3 (DIAx) of parameter No. 1006 = 0) for the axis 
corresponding to the input signal, the specification method switches to 
diameter specification; the specification method switches to radius 
specification if diameter specification is selected (with bit 3 (DIAx) of 
parameter No. 1006 = 1).

 

During switching, the diameter/radius specification switching 
in-progress signal from DM1 to DM8 (output signals) corresponding 
to a switched axis is output.

 

To return the diameter/radius specification of an axis to the original 
state, set the setting of the corresponding diameter/radius specification 
switch signal from DI1 to DI8, from 1 to 0.