Selection Of G Code System A, B, Or C; Decimal Point Programming - Siemens Sinumerik 802D sl Programming Manual

04.07
1.1.6

Selection of G code system A, B, or C

ISO Dialect T distinguishes between G code system A, B, and C. G code system B
is default setting. The G code system in use is selected by MD $MN_MM_EX--
TERN_GCODE_SYSTEM as follows:
$MN_MM_EXTERN_GCODE_SYSTEM = 0: G code system B
$MN_MM_EXTERN_GCODE_SYSTEM = 1: G code system A
$MN_MM_EXTERN_GCODE_SYSTEM = 2: G code system C
G Code system A
If G code system A is active, G91 is not available. In this case, incremental axes
movement for axis X,Y, and Z is programmed by address U, V, and W. U, V, and W
are not available as axis designation in this case resulting in a maximum axes
number of 6.
Address H is used for programming incremental movement of the C axis in G code
system A.
Notice
If not otherwise noted, the manual in hand describes G code system B.
S
For the differences between G code system A, B, and C refer to the G code list
S
in the appendix.
1.1.7

Decimal point programming

There are two notations for the interpretation of programming values without a
decimal point in ISO Dialect mode:
S pocket calculator type notation
Values without decimal points are interpreted as mm, inch or degrees.
S standard notation
Values without decimal points are multiplied by a conversion factor.
The setting is defined by MD 10884, see Chapter 4 "Startup".
There are two different conversion factors, IS-B and IS-C. This evaluation refers to
addresses X Y Z U V W A B C I J K Q R and F.
Example of linear axis in mm:
X 100.5
X 1000
© SIEMENS AG 2007 All rights reserved
SINUMERIK 802D sl/840D sl840D/840Di sl/840Di/810D ISO Turning - - 04.07 Edition
corresponds to value with decimal point: 100.5mm
pocket calculator type notation: 1000mm
standard notation: IS-B: 1000* 0.001= 1mm
IS-C: 1000* 0.0001 = 0.1mm
Programming Basics
1.1 Introductory explanations
1-13