Tolerance And Accuracy - Siemens SINUMERIK 828D Manual

2.2
Tolerance
Accuracy
28
General information on workpiece production
Calculation and simulation
When simulating the calculated tool paths / machine movements, different levels of quality
can be used. From straightforward simulation of the tool paths through to complete simulation
of the G and M codes that takes account of all machine-specific and control-specific data.
Here, potential collisions can be detected and avoided, for example, and the machine's maxi-
mum axis traversing ranges can be taken into account.
Output of the NC code with the postprocessor
The postprocessor converts the sequences into NC programs taking into account the control-
specific syntax and the control's special functions. For this purpose, CAM systems make use
of universal postprocessors or special postprocessors that have been optimized for the
SINUMERIK system. Manufacturer-specific functions such as separate coolant strategies
must be implemented in the postprocessor in consultation with the machine manufacturer.

2.2.1 Tolerance and accuracy

When working with CAD/CAM systems, certain tolerances and levels of accuracy that will have
an impact on subsequent machining must be observed.
The CAM system uses the CAD surface (spline) to generate a contour consisting of linear
traversing blocks (straight line elements). The extent to which the linear contour deviates from
the real contour from the CAD system is known as the chord error or chord tolerance. This
tolerance depends on the strategy and on the workpiece. The tolerance for roughing strategies is
greater than for finishing strategies. When the NC programs are executed on the machine, the
tolerance is specified by the CAM system in CYCLE832 so that optimum results can be achieved
in terms of surface quality and contour accuracy.
Tolerance guide values
Technology Recommended values
Roughing Tolerance 0.05 - 0.1 mm - with 5-axes OTOL = 0.3
Semi-finishing Tolerance 0.01 - 0.05 mm - with 5 axes OTOL = 0.15
Finishing Tolerance 0.002 mm - max. point separation 0.3 - 0.5 mm
with 5-axes OTOL = 0.01 - 0.1
When outputting the NC blocks from the CAM system, you can specify the number of decimal
places. The required level of accuracy is dependent on the type of interpolation.
Accuracy guide values
Axes interpolation Recommended values
Linear axes for 3-axis programs, at least 4 decimal places
(X Y Z)
Rotary axis positions for 5-axis programs, at least 6 decimal places in linear and rotary axes
(A B C) for optimum surface quality
Direction vector 4 decimal places in linear axes and at least 7 decimal places for
(A3 B3 C3) direction vectors
© Siemens AG All rights reserved SINUMERIK, Manual, Mold-Making with 3- to 5-Axis Simultaneous Milling