Siemens SINUMERIK 802D sl Programming And Operating Manual page 204

Programming
10.1 Fundamental principles of NC programming
Address Meaning
T Tool number
X Axis
Z Axis
AC Absolute coordinate
axis
ACC[ ] Percentage
acceleration override
ACP Absolute coordinate;
approach position in
the positive direction
(for rotary axis,
spindle)
ACN Absolute coordinate;
approach position in
the negative direction
(for rotary axis,
spindle)
ANG Angle for the
specification of a
straight line for the
contour definition
AR Aperture angle for
circular interpolation
CALL Indirect cycle call
CHF Chamfer;
general use
204
Value assignments Information
1 ... 32 000 The tool change can be
only integer, no performed either directly using
sign the T command or only with M6.
This can be set in the machine
data.
±0.001 ... 99 Positional data
999.999
±0.001 ... 99 Positional data
999.999
- The dimension can be specified
for the end or center point of a
certain axis, irrespective of
G91.
1 ... 200, integer Acceleration override for an
axis or spindle; specified as a
percentage
- It is also possible to specify the
dimensions for the end point of
a rotary axis with ACP(...)
irrespective of G90/G91; also
applies to spindle positioning
- It is also possible to specify the
dimensions for the end point of
a rotary axis with ACN(...)
irrespective of G90/G91; also
applies to spindle positioning
±0.00001 ... Specified in degrees;
359.99999 one possibility of specifying a
straight line when using G0 or
G1 if only one end-point
coordinate of the plane is
known
or
if the complete end point is
known with contour ranging
over several blocks
0.00001 ... Specified in degrees; one
359.99999 possibility of defining the circle
when using G2/G3
- Special form of the cycle call;
no parameter transfer; the
name of the cycle is stored in a
variable;
only intended for cycle-internal
use
0.001 ... 99 Inserts a chamfer of the
999.999 specified chamfer length
between two contour blocks
Programming and Operating Manual, 11/2012, 6FC5398-5CP10-3BA0
Programming
T...
X...
Z...
N10 G91 X10 Z=AC(20) ;X -
incremental dimension,
Z - absolute dimension
N10 ACC[X]=80 ;for the X
axis 80%
N20 ACC[S]=50;for the
spindle: 50%
N10 A=ACP(45.3) ;
Approach absolute position
of the A axis in
the positive direction
N20 SPOS=ACP(33.1);
Position spindle
N10 A=ACN(45.3) ;
Approach absolute position
of the A axis in
the negative direction
N20 SPOS=ACN(33.1);
Position spindle
N10 G1 X... Z....
N11 X... ANG=...
or contour over several
blocks:
N10 G1 X... Z...
N11 ANG=...
N12 X... Z... ANG=...
See G2, G3
N10 CALL VARNAME ;
variable name
N10 X... Z.... CHF=...
N11 X... Z...
Surface grinding