Programming manual
CNC 8070
STATEMENTS AND INSTRUCTIONS
Programming statements
15.
(SOFT V02.0X)
419
15.1.3 Programming referred to machine reference zero (home)
With this CNC, the movements may be referred to home, temporarily
canceling the active zero offsets and tool radius and length
compensation.
When moving with respect to machine reference zero, function G70
or G71 programmed by the user is ignored. The movements are
carried out in the units (millimeters or inches) set by the OEM (units
assumed by the CNC on power-up).
The programmed movements do not admit polar coordinates, nor
other kinds of transformations such as mirror image, coordinate
(pattern) rotation or scaling factor. While the #MCS function is active,
functions for setting a new origin such as G92, G54-G59, G158, G30,
etc. are not admitted either.
#MCS Movement referred to machine zero.
This instruction may be added to any block containing a movement so
it is executed in the machine reference system.
#MCS ON It activates the machine coordinate system
#MCS OFF It cancels the machine coordinate system
The #MCS ON and #MCS OFF instructions activate and deactivates
the machine coordinate system so the movements programmed
between both instructions are executed according to the machine
reference system.
Both instructions must be programmed alone in the block.
G92 X0 Y0
G01 X30 Y30 F850
(Origin : Part zero)
#MCS X30 Y30
(Origin : Machine zero (home))
G01 X40 Y40
(Origin : Part zero)
M30
G92 X0 Y0
G01 X50 Y50
#MCS ON
(Origin : Machine zero (home))
G01 ···
G02 ···
G00 ···
#MCS OFF
(Origin : Part zero)
G01 X70 Y70
M30
To Next Page
Loading...
