If you are postprocessing Mechanical harmonic-analyzed files and all of the variable values are incorrectly displaying as zeroes, you can set the environment variable CFDPOST_RST_SKIP_LAST_DATASET=1 to plot the variables with nonzero values from the second-last dataset of the results file (which does not contain frequency values of zero).

CFD-Post does not fully support undefined and user-defined as values for RST units. In those cases, CFD-Post assumes SI units.

If you want to use CFD-Post to postprocess a Mechanical RST file outside of Ansys Workbench and you do not want to have CFD-Post assume SI units, you can set an environment variable (CFDPOST_RST_SHOW_UNITS_DIALOG=1) to cause the Solution Units dialog box (described in Solution Units Dialog Box) to appear. Note that this will cause the Solution Units dialog box to appear even when CFD-Post can read the units in the results file.

The Ansys Mechanical solver does not output minimum/maximum ranges for each of the calculated variables; these ranges are calculated when the results file is loaded by CFD-Post. Calculating the range for a very large problem would, however, require prohibitively large amounts of CPU time. As a result, range values are calculated for the loaded time step only. This means that values that appear as global range, are in fact ranges that exist for that time step only, at first. As more time steps are added, the global range is extended accordingly. If you want to enable the calculation of true global ranges (and incur the potentially large CPU time each time you load a non-Ansys CFX file), you can do this by selecting Edit > Options and selecting Pre-calculate global variable ranges, under Files. For details, see Files.

CFD-Post plots only Mechanical variables that exist in RST files; unlike Mechanical, it will not calculate other variables automatically. Therefore, some variables that you would expect to be able to plot (as in Mechanical) either will be missing or will have all zero values in CFD-Post.

RST files do not store data for principal stresses. There is a slight difference for principal stress calculated in CFD-Post and Mechanical. CFD-Post calculates principal stresses on a node by averaging the stresses on each element touching the node. However, Mechanical calculates principal stresses based on node-averaged stresses. This difference can be minimized by the use of a finer mesh.

You can also configure Mechanical to calculate principal stresses the same way as CFD-Post by issuing the command avprin, 1, and replotting the values.

By default, a Mechanical results file does not contain the definitions of any components that you may have created in the simulation set up and so these will not be available as regions for plotting in CFD-Post. However, it is possible to produce an additional "components" file that does contain these definitions. If CFD-Post finds a file with the name <filename>.cm in the same directory and with the same filename (excluding the file extension) as the Mechanical results file, then it will read component definitions from this file. For instance, if you are postprocessing the Mechanical results file OscillatingPlate.rst, CFD-Post will look for the file OscillatingPlate.cm in the same directory to find component definitions. You can make Mechanical write the components file by including a command CMWRITE,<jobname>,cm in your Mechanical input file, before the SOLVE command. If .cm files are to be loaded into CFD-Post, job names need to be consistent across restarts, input file processing, and regular runs.

Components files (CM files) must have been output in blocked format (which is the default output format). Refer to the Ansys Mechanical documentation to learn how to control the Mechanical output format.

All regions from components files are read as surfaces. If a region is volumetric, CFD-Post will read the outer surface only.

CFD-Post will read only nodal components. Components that consist of elements will be ignored.

CFD-Post can read a limited number of Mechanical results files that contain shell elements only. It depends on the problem setup details as to whether a file can be successfully read or not. CFD-Post cannot read any Mechanical results files that contain no 3D or shell elements.

When reading RST files, CFD-Post ignores mid-side nodes and duplicate nodes. The latter situation occurs when a case has multiple bodies with matching meshes on the interfaces. The simulation picks up duplicate nodes and plots accordingly, giving a discontinuous plot. However CFD-Post picks up only one of the nodes, causing one domain to appear to spill into the next.

In Mechanical, simulation characteristics such as maximum values are derived from actual local node values. In CFD-Post values need to be presented on global nodes, therefore CFD-Post takes a simple average from all shared elements' local values. When compared the two calculations will be similar, but not exactly the same.

Mechanical results files that contain mid-edge nodes will cause mesh reports to be inaccurate (the Connectivity range may be reported as zero).

When Mechanical electrical data is read in CFD-Post, units are not displayed for quantities such as Electric Potential or for Electric Flux^[2].

Mechanical results files contain shell elements with data on both the top and bottom sides. CFD-Post currently does not support separate data on the two sides. Only data from the top side will be read. If you want to load results from the bottom side, you can set the environment variable CFDPOST_RST_READ_BOTTOM_SHELL_DATA.

When exporting Heat Flux to Mechanical, you should always select the fluid side of the interface.