Siemens SINUMERIK 840D sl Function Manual page 1932

Detailed Description
2.8 Special handling of tool compensations
NC program
Temperature compensation values in the NC program
The compensation values assigned to axes X and Z are not zero and are applied for
temperature compensation with respect to tool length. The machine axis positions reached in
each case are specified as comments in the program lines.
SD42960 TOOL_TEMP_COMP[0] = -0.3
SD42960 TOOL_TEMP_COMP[1] = 0.0
SD42960 TOOL_TEMP_COMP[2] = -1.0
N10 g74 x0 y0 z0 a0 b0
N20 x20 y20 z20 f10000
N30 traori()
N40 x10 y10 z10 b90
N50 trafoof
N60 x0 y0 z0 b0 c0
N70 m30
With the exception of block N40, temperature compensation always acts in the original
directions, as the tool is pointing in the basic orientation direction. This applies particularly in
block N50. The tool is actually still pointing in the direction of the X axis because the B axis is
still at 90 degrees. However, because the transformation is already deactivated, the applied
orientation is parallel to the Z axis again.
MD20390 TOOL_TEMP_COMP_ON = TRUE
Option
MD32750 TEMP_COMP_TYPE[ AX1 ] = 4
MD32750 TEMP_COMP_TYPE[ AX2 ] = 4
MD32750 TEMP_COMP_TYPE[ AX3 ] = 4
For more details on "Temperature compensation" see:
References:
/FB2/ Function Manual Extended Functions; Compensations (K3)
For information on "Generic 5-axis transformations" see:
References:
/FB3/ Function Manual Special Functions; 3- to 5Axis Transformation (F2)
144
; First compensation value
;
; Second compensation value
; Position setpoints of the machine axes
; X Y Z
; 20.30 20.00 21.00
; 20.30 20.00 21.00
; 11.00 10.00 9.70
; 10.30 10.00 11.00
; 0.30 0.00 1.00
; Temperature compensation active
; Activate option
; Compensation in tool direction
; Compensation in tool direction
; Compensation in tool direction
Basic logic functions: Tool Offset (W1)
Function Manual, 11/2006, 6FC5397-0BP10-2BA0