Siemens SINUMERIK 840D Manual page 20

2.2
Tolerance
Accuracy
20
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 maximum
axis traversing ranges can be taken into account.
Output of the NC code with the post processor
The post processor converts the sequences into NC programs taking into account the con-
trol-specific syntax and the control's special functions. For this purpose, CAM systems make
use of universal post processors or special post processors that have been optimized for the
SINUMERIK system. Manufacturer-specific functions such as separate coolant strategies
must be implemented in the post processor in consultation with the machine manufacturer.
Key parameters
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 tra-
versing 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 used and is greater in the case of roughing strategies than with 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 qual-
ity and contour accuracy.
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. In the case of
linear axes (X, Y, Z), at least 3 decimal places should be used for 3-axis programs.
If the blocks are to be output as rotary axis positions, with 5-axis programs 5 decimal commas
should be used in the linear and rotary axes for optimum surface quality. If they are to be output
in the form of a direction vector, we recommend 5 decimal places in the linear axes and 6 for the
direction vectors.
© Siemens AG All rights reserved. SINUMERIK, Manual, 5-axis machining