When the Options dialog box appears, CFD-Post options can be configured under CFD-Post.
- Interpolation Tolerance
The Interpolation Tolerance sets the amount of the area outside the domain that will be treated as a part of the domain when interpolating variables. For example, a point that is within this tolerance distance will be given a value that is interpolated from the nearest domain boundary face.
By default the tolerance "layer" is 0.2% of the domain. You can set the value to 0 to turn the Interpolation Tolerance off.
Note that this value should be set to a value less than half the size of the smallest openings or features of the domain geometry. This prevents a point from being detected in two overlapping Interpolation Tolerance regions.
If the Interpolation Tolerance setting is too high, there could be undefined nodes and malformed elements in the virtual layer, especially around sharply-contoured regions of the domain surface.
Changes to the interpolation tolerance can affect how data is interpolated onto objects such as Sample Planes, Polylines, User surfaces, Surfaces of Rotation, and so on. Each of these objects, depending on how close the defined points are to the domain, may have slightly changed behavior, depending on how close to the domain the points are defined.
- Angular Shift for Rotating Locations
This option takes effect when a new case is loaded, and affects rotating domains and Monitor Surfaces defined with a rotating coordinate frame. The option can be set to:
AutomaticThis is the default option. CFD-Post displays the rotated position of the rotating locations considering the currently-loaded timestep. CFD-Post uses the rotated position for a domain (and associated locations such as domain boundaries) only if the domain is connected with a transient rotor-stator interface, either directly or through one or more connected domains. The rotated position for a Monitor Surface is always used.
Always rotateCFD-Post displays the rotated position of the rotating locations applicable to the currently-loaded timestep. Domains and Monitor Surfaces are always displayed in their rotated position regardless of any interfaces in the setup.
Never rotateCFD-Post always uses the initial position of the rotating domains and Monitor Surfaces.
Because the rotating domains may be in a rotated position when they are loaded into CFD-Post for postprocessing, force calculations made on the rotating domains can have different results depending on the setting of the option above.
Enable Beta Features
Some Beta features are hidden in the user interface. You can select this option to "unhide" those features. When selected, such features are identified by "(Beta)" in the user interface. Note that Beta features are unofficial and not well tested.
Changes made in this section will take effect the next time you load a file.
Warn prior to loading the same results file more than once controls whether you are warned when you attempt to load a file that is already loaded. The warning appears when both the filename and the file contents are the same as a currently loaded file.
Select Multi-Domain > Show domain selector before load to enable you to choose which domains to load when more than one domain exists in the results file. If this option is turned off, then all domains will be loaded next time you load a results file.
Under Keyframe Animation > Command Timeout, specify the minimum number of milliseconds that must pass after clicking to change the number of keyframes in the Animation dialog box (in the # of Frames field with the Keyframe Animation option selected) before a subsequent mouse click can be registered. This time enables CFD-Post to finish generating the currently specified number of keyframes without the specified number changing during the generation process. The allowed range for Command Timeout is 400 to 1000.
If Enable GPU Shader Rendering is selected (default), then:
The graphics card GPU (if eligible, and with sufficiently recent drivers) is used to compute objects (for example, Turbo Surfaces) that display Transient Blade Row (TBR) results.
GPU Accelerated Animation becomes available for objects except those that are based on a domain for which more than one data instance is set in the domain details view, on the Data Instancing tab. In other words, data instancing as set in the domain details view is incompatible with GPU Accelerated Animation.
For objects that display Transient Blade Row (TBR) results, graphical instancing, as set in the domain details view on the Instancing tab, acts like data instancing would without GPU acceleration, in the sense that variables are not simply copied to new instances but are instead calculated for each instance using a Fourier series.
In the details view for boundaries and other surfaces, on the Color tab, the Contour setting "
Banded" is functional, enabling you to color a surface with contour bands without having to create a contour object. For details, see Contour.
Note: Due to limitations of the graphics card and/or graphics driver, the graphics card might not be able to render an image using all of the sine-cosine pairs of Fourier coefficients (per vertex) available to be included in the graphics data. For multi-disturbance (see Multiple Disturbances in the CFX-Solver Modeling Guide) and mesh deformation (see Mesh Deformation in the CFX-Solver Modeling Guide) cases in particular, you might see the following error message:
CreateShader ERROR: The number of vertex attributes used may have exceeded the hardware limit.
Please consult the documentation for ways to resolve the issue.If this error occurs, try setting the following environment variable to a value less than
7, for example3:CFDPOST_GPU_ANIMATION_TBR_MAXIMUM_FOURIER_COEFFICIENT_PAIRSThis reduces the maximum number of Fourier coefficient pairs in the Fourier series sent to the GPU. For example, a setting of 3 would use the first 6 Fourier coefficients.
By restricting the number of Fourier coefficient pairs, the graphical fidelity of plotted variables may be diminished. Consequently, you should set the environment variable temporarily, only for cases that require it. For most cases not involving multi-disturbance or mesh deformation, you can leave the environment variable undefined; doing so enables graphical rendering using the full set of Fourier coefficient pairs.
Changes made in this section will take effect the next time you load a file.
Under Mass Flow Expression Method Used for Physical Surfaces, select an option to control how mass flow data is calculated, for example by the
massFlow,massFlowAve, andmassFlowAveAbsfunctions:Use surface shape approximated by the nearest control volume faces (not recommended for cases with GGI interfaces)
This method can provide more accurate massFlow rates. However, it may provide inaccurate results if the surface over which the mass flow is evaluated crosses a GGI interface.
Use surface mass flows computed from interpolated nodal values (recommended for general cases)
This method is recommended because the results do not suffer if the surface over which the mass flow is evaluated crosses a GGI interface.
When Transient > Load missing variables from nearest FULL time step is cleared, it makes all variables that are not written to the partial results file undefined for the current timestep. When selected, CFD-Post loads the missing variables from the nearest full results file. This option is used when partial transient results files do not contain all of the variables calculated by the CFX-Solver. By default, these variables will be undefined (but still visible in the variables list) for the current timestep.
Important: Take care when using this option because values that are plotted may not apply to the current timestep.
Select Regions > Don't load mesh regions if you do not want to have region definitions loaded when you load a file that contains them.
Select Turbo > Don't prompt to auto-load reports to prevent CFD-Post from automatically asking you if you want to load a report upon loading results files.
Load interior face zones controls whether or not interior face zones are displayed.
Fluent cases contain cell zones and face zones. (Cell zones are similar to element sets in CFD-Post, and face zones are similar to face sets.) All cell zones are read into CFD-Post and are listed as domains. Of the face zones, by default only those that bound a cell-zone/domain are shown in CFD-Post[3]. However, Fluent meshes can also contain 'interior' face zones that are useful for postprocessing. Interior face zones are inside a domain and do not form a boundary of the domain. To see interior face zones, enable Load interior face zones.
Note: The names of 'interior' zones in CFD-Post are kept same as that in Fluent, except that characters that are not allowed in CFD-Post (such as '-', ':' and so on) are replaced by space characters.
Show warning for incompatible variables in old files controls whether a message box will appear if the Fluent .dat file you are loading contains incompatible variables. These variables, when written by versions of Fluent earlier than 18.0 may show differences when displayed in CFD-Post when compared to Fluent. For details, see Exporting to Ansys CFD-Post.
Define vector variables controls whether or not vector variables are created if Cartesian vector components are present in a CGNS file. It should not be necessary to turn this option off unless this is required to allow compatibility with state or session files from previous releases.
Non CFX Files > Translate variable names to CFX-Solver style names converts variable names into CFX variable names for results files that are both:
Not from the CFX-Solver, and
Not written using the Common Fluids Format (CFF).
For example, the variable
Pin a CFX-TASCflow file will be converted toPressure.Note: Variables from CFF files are not affected by the Non CFX Files > Translate variable names to CFX-Solver style names setting. Instead, they are affected by the Common Fluids Format > Name Convention setting (described below).
Important:By default, CFD-Post will not modify the variable names in the .rso file. If you want to use all of the embedded CFD-Post macros and calculation options, you will need to convert variable names to CFX types.
In order to use the Turbo Charts feature with Fluent files, you must have Translate variable names to CFX-Solver style names selected.
The complete list of translated variables is given in Variable Translation.
Clear Non CFX Files > Pre-calculate global variable ranges to turn off the calculation of all variable ranges.
Set Common Fluids Format > Name Convention to one of the following options:
CFD-PostVariables read from a CFF file are, where applicable, renamed with standard CFX variable names, which are used by various features in CFD-Post, such as functions, reports, and macros. If this option is not used, such features might not work.
NativeVariables read from a CFF file are not renamed.
Common Fluids FormatVariables read from a CFF file are, where applicable, renamed with standard Ansys Fluids variable names, which are used by various Ansys Fluids products. Not all variables supplied in the CFF file are renamed; some variables retain their supplied name.
CFD-Post has a Solution Units option that is available from the Options tab.
The solution units assumed, which are read when the file was loaded, are displayed on the right. When files that do not store solution units (such as CFX-4 dump files, CFX-TASC files, Fluent files, or Ansys results files) are loaded, you will be prompted to specify the solution units. You can enable the Don't prompt for Solution Units before loading results toggle to suppress this prompt, in which case the default units of kilograms, meters, seconds, Kelvin, and radians will be used.
The units shown on this dialog box are not necessarily those used by CFD-Post, but are the solution units used in the currently loaded file. The units used by CFD-Post are set elsewhere; for details, see Setting the Display Units. CFD-Post needs to know the solution units used in the file so that it can convert them to the units specified. When CFX files are loaded into CFD-Post, the solution units that were used by the CFX-Solver are automatically read from the file. For this reason, Don't prompt for Solution Units before loading results is ignored when loading CFX files and selected by default for other file types.
When postprocessing a results file in CFD-Post, the units used are not necessarily those used in the results file. CFD-Post will convert to your preferred units.
Note: In CFD-Post, the temperature solution units must be an absolute scale (for example, Kelvin [K] or Rankine [R]); you cannot use Celsius and Fahrenheit. Temperature quantities elsewhere in Ansys CFX can be set in Celsius and Fahrenheit.
To configure the viewer, right-click the viewer and select Viewer Options.
Controls how an object that is generated after a change to the setting of this option is highlighted in the viewer. Such highlighting occurs when in picking mode, when selecting a region in a list, or when selecting items in the tree view.
Under Type, select one of the following:
Surface Mesh: Displays the surface mesh for selected regions using lines.Wireframe: Traces objects that contain surfaces with green lines.Bounding Box: Highlights the selected objects with a green box.
Note: When you load a state file, the highlighting is dictated by the setting that is stored in the case, rather than by the current preferences setting.
Set Mode to Color or Image.
Use Color Type to set either a solid color or a gradient of colors; use Color to set the color (and Color 2 for gradients).
Select one of a list of predefined images or a custom image.
If selecting a custom image, choose an image file and a type
of mapping. Image types that are supported include
*.jpg, *.png, and *.ppm. Mapping options are Flat and Spherical. Flat maps are
stationary while spherical maps surround the virtual environment and
rotate with the objects in the viewer.
Custom images have some restrictions: all background images and textures sent to the viewer must be square and must have dimensions that are powers of 2 (for example, 512 x 512 or 1024 x 1024).
If the dimensions of your background image is not a power of 2, the viewer sizes the image to be a power of 2 by doing bicubic resampling.
To make the background image square, transparent pixels are added to the smaller dimension to make it the same as the larger dimension. The transparent pixels enable you to see the regular viewer background, which gives you control over what fill color your background has.
Select or clear Axis Visibility or Ruler Visibility to show or hide the axis indicator or ruler in the viewer.
See Stereo Viewer.
[3] CFD-Post will never list:
Default interior zones.
Walls created during creation of non-conformal interfaces.
Sliding interface zones.
Any other zones that cannot be displayed from the Mesh Display panel in Fluent.