Siemens SINUMERIK 840C - Manual (Page 326)

12.93 6 NC Machine Data (NC MD), NC Setting Data (NC SD)
6.6.3 Channel-specific MD bits 1 (channel bits)
With SINUMERIK 840C, the initial plane is defined in NC MD 110*. In NC MDs 548*, 550* and
552* you define to which axes the radius compensation and/or length compensation is to apply
when the NC is switched on. In NC MD 548* and 550* you define the axes to which the radius
compensation is to apply in the default setting, i.e. when the NC is switched on. In NC MD
552* you define the axis to which the length compensation 1 (tool parameter P2) is to apply
(for cutters only). The axis to which the second length compensation (tool parameter P3) is to
apply depends on the order of the programmed axes and the tool type.
Example:
NC MD 548* = 0000 0000 X axis
NC MD 550* = 0000 0001 Y axis
NC MD 552* = 0000 0010 Z axis
• Program
N10 G0 G41 D1 X0 Y0 Z0 (D1 = tool type 20 cutter)
Radius is calculated in X-Y
L1 is calculated in Z
L2 is not calculated
• Program
N10 G16 X Y Y Z (plane selection)
N20 G0 G41 D1 X ... Y ... Z ... (D1 = tool type 30 angle-headed cutter)
Radius is calculated in X-Y
L1 is calculated in Y
L2 is calculated in Z
• Program
N10 G16 Z X Z (plane selection)
N20 G0 D1 Z ..... (D1 = tool type 10 drill)
No radius is calculated
L1 is calculated in Z
Z-X (G18) is to be selected as the initial plane on a lathe with an X and Z axis. The NC MD
must be set as follows:
NC MD 548* = 0000 0000
NC MD 550* = 0000 0010
NC MD 552* = 0000 0010
Plane Z-X is defined with NC MD 548* and 552*. The axis to which the L1 geometry is to apply
is set in NC MD 550* if a drill or a cutter is used.
Applies up to tool type 9: Length 1 (tool parameter P2) always refers to the second
axis name behind G16<
Length 2 (tool parameter P3) always refers to first axis
name behind G16
Length 1 (tool parameter P2) always refers to the
transverse axis.
© Siemens AG 1992 All Rights Reserved 6FC5197- AA50 6–141
SINUMERIK 840C (IA)