Tolerance Parameters (R33, R34, R36, R37, R40/R41) - Siemens SINUMERIK 840 User Manual

08.96 1 Introduction

1.7 Tolerance parameters (R33, R34, R36, R37, R40/R41)

1.7 Tolerance parameters (R33, R34, R36, R37, R40/R41)
Averaging by itself is not sufficient to ensure a permanent high standard of machining
accuracy. For constant deviations (no trend), the dimensional deviation measured can be
corrected by an empirical value. In addition, further corrections can be derived for deviations
following a trend. For this purpose, tolerance bands must be allocated to the associated set
dimension via parameters (R parameters) in the machining program prior to measuring cycle
call.
The set workpiece dimension is placed in the middle of the permissible ± tolerance band for
reasons of symmetry.
The tolerance bands and the reactions derived from them have been specified as follows:
Safe area (R36):
This limit has no influence on averaging. It is used for diagnostics. When this limit is reached,
this means that there is a probe fault or that an incorrect setpoint position has been specified.
AUTOMATIC operation is interrupted and the program cannot be continued. An alarm text
appears on the display to warn the operator.
Caution:
In the case of tool measurement, the "safe area" tolerance is derived from the difference
between the old correction value (TOA memory) and the new tool length.
Dimensional difference check (R37):
Tool wear from workpiece n to workpiece n+1.
This limit has no influence on correction value generation either. When this limit is reached,
the tool is probably worn down and must be replaced.
An alarm is displayed to warn the operator. The program can be continued by NC Start.
This tolerance limit is generally used by the PLC for tool management (twin tools, wear
monitoring).
Caution:
For tool measurement, the tolerance is determined as in the case of the safe area.
Workpiece tolerance (R40/R41):
When measuring a dimensional deviation ranging between "2/3 tolerance of the workpiece"
and "dimensional difference check" (this might be the case when using a new tool, for
instance), this dimensional deviation is regarded 100% as tool offset.
As a further step, the previous average value is erased.
This allows fast counteraction when major dimensional deviations occur. AUTOMATIC
operation is interrupted when the tolerance limit of the workpiece is exceeded. "Oversize" or
"undersize" is indicated to the operator on the control display monitor, depending on the
tolerance zone position. Machining can be continued by NC Start.
© 1–23
Siemens AG 1990 All Rights Reserved 6FC5197- AB70
SINUMERIK 840/850/880 (BN)