Switchover; G Code Display; Maximum Number Of Axes/Axis Designation - Siemens SINUMERIK 802D sl Programming Manual

Programming Basics
1.1 Introductory explanations
1.1.3

Switchover

The following two G commands are used to switch between Siemens mode and
ISO Dialect mode:
-- G290 -- Siemens NC programming language active
-- G291 -- ISO Dialect NC programming language active
The active tool, the tool offsets and the zero offsets are not changed by this action.
G290 and G291 must be programmed in a separate program block.
1.1.4

G code display

The G code display must always be implemented in the same language type
(Siemens/ISO Dialect) as the current block display. If the block display is suppres-
sed with DISPLOF, the current G codes continue to be displayed in the language
type of the active block.
Example
The Siemens standard cycles are called up using the G functions of the ISO Dia-
lect mode. DISPLOF is programmed at the start of the cycle, with the result that
the ISO Dialect G commands remain active for the display.
PROC CYCLE328 SAVE DISPLOF
N10 ...
...
N99 RET
Procedure
External main program calls Siemens shell cycle. Siemens mode is selected impli-
citly on the shell cycle call.
DISPLOF freezes the block display at the call block; the G code display remains in
external mode. This display is refreshed while the Siemens cycle is running.
The SAVE attribute resets the G codes modified in the shell cycle to their original
state when the shell cycle was called on the return jump to the main program.
1.1.5

Maximum number of axes/axis designation

In ISO Dialect--M the maximum number of axis is 9. Axis designation for the first
three axes is fixed to X, Y and Z. Further axes can be designated A, B, C, U, V, W.
1-12
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) - - 04.07 Edition
© Siemens AG 2007 All rights reserved
04.07