Limitations in Previous Versions

• Grid interfaces from Fluent versions 6.3 and older are not supported by CFD-Post. If your .cas file has old grid interfaces, read the .cas and .dat file into the Fluent Release 12.0 (or later), run at least one iteration, and save the file to change to the new grid interfaces. This will convert grid interfaces to use the virtual polygon method and make the file readable in CFD-Post. Attempting to read old grid interfaces may cause CFD-Post to exit.

• To postprocess forces or fluxes using the DBNS solver of Fluent for cases from versions prior to Release 12.0, you must read the case into Fluent Release 12.0 (or later), iterate at least once, and then write out the .cas and .dat files.

• Holes may appear in Planes/iso-surfaces created using old Fluent mesh/case files (from earlier than Release 14.5) for hex-core/cut-cell mesh cases.

Limitations Involving Elements and Nodes

• Node Values for Wall Adjacent Temperature are only available on faces if they are supplied by Fluent. This may result in undefined plots on non-wall locations when using Wall Adjacent Temperature. Exporting Wall Adjacent Temperature on non-wall locations may also show null values where data does not exist.

• In Ansys Fluent, any element can have any number of faces. The maximum number of nodes in a polyhedron element is 256 and in a polygon face is 128 (however the contour-creation algorithm has a limit of 64 nodes per face).

• Plots created in CFD-Post that are based on node values (not cell/face values) can have undesired results where nodes are shared by multiple objects.

• CFD-Post does not smooth out values across non-conformal interface boundaries; that is, there must be a 1-1 mapping of nodes across the interface. As a result, contour and color plots as well as iso-surfaces are discontinuous across these interfaces. Therefore, the node values displayed by CFD-Post at non-conformal interfaces may differ from those shown by Fluent.

• Case comparison is not available for cell based contours of Fluent results.

File-based Limitations

• The restrictions on loading CFF files also apply to Fluent CFF Case and Mesh (.h5) files. For details, see Limitations with Ansys CFF Files.

• CFD-Post does not support UDNM (User-Defined Node Memory) variables from Fluent.

• Unsteady statistic variables (such as Mean X Velocity and RMS Static Pressure) are not to be read from the standard .dat file. If needed, you can export these variables explicitly in a .cdat file or append the variables to the .dat file.

• For Fluent files, the gradients computed by CFD-Post are discontinuous across domains.

• CFD-Post can read zone-motion variables (origin, axis, omega, grid-velocity) on profile boundaries from Fluent files only if the variables are constants. For cases where any of these values are specified as non-constants, CFD-Post ignores the variable. In such conditions, CFD-Post cannot transform the velocity from absolute to the relative frame or the reverse. Other dependent variables (such as Mach Number and Vorticity) will not be available unless explicitly exported from Fluent using either a .cdat file or data file options. There will be a warning message issued when these files are read.

• For Fluent files using the energy model, Heat Flux is available for all boundaries and Wall Heat Flux is available only for walls. The values of these two variables will be same on walls.

• You need to be careful when choosing geometry names in Fluent when the file will be read in CFD-Post. The geometry names must not contain special characters such as '-', '|', and ':'. All such characters will be replaced by a space (which is allowed in names in CFD-Post).

• CFD-Post can read files written from Fluent, but the reading of mesh files written from TGrid or GAMBIT is not supported and may cause CFD-Post to terminate abnormally.

• CFD-Post reads User-Defined Memory (UDM) and User-Defined Scalars (UDS) as follows:

  • When .cas/.dat files are read into CFD-Post, UDM/UDS variables will appear with names as "User Defined Memory 0"/"Scalar 0".

  • When .cas/.dat files are read into CFD-Post, CFD-Post will show all UDM/UDS variables that were exported to the CDAT file.

• Fluent .cas, .dat, and .cdat files do not contain the units for user-defined scalars, user-defined memory, or custom field functions, so these will be dimensionless in CFD-Post.

• CFD-Post cannot import Boundary Mesh files, even though Boundary Mesh files have the .msh file extension.

• CFD-Post can read Fluent case files that have imprinted surfaces defined in them. However, the imprinted surfaces are ignored in CFD-Post.

General Limitations

• When reading a Fluent results file, CFD-Post may report an incorrect sign for mass flow through a conformal internal boundary (known as an "interior" type in Fluent) that is located at the boundary between two domains. To determine the direction of mass flow, use a CEL expression based on the normalized dot product of the local velocity and the face normal. The equations for computing the corrected mass flow through a conformal internal boundary, based on the local mass flow summed over the boundary, are:

  Corrected Mass Flow = sum(abs(Mass Flow)*massFlowCorrectionNorm)@<region>
  massFlowCorrection = Normal X*u + Normal Y*v + Normal Z*w
  massFlowCorrectionNorm = -massFlowCorrection/abs(massFlowCorrection)

• For axisymmetric cases, the point values in CFD-Post may differ from values reported in Fluent due to the extrusion of the 2D domain in the theta direction.

• When selecting to output additional variables in a .dat file in Fluent (via the Data File Quantities panel), a variable is written to the user-specified section of a .dat file. CFD-Post will check to see if the same variable is available in the basic section of the .dat file. If so, the variable from the basic section will not be read in CFD-Post; only the variables from the user-specified section of the .dat file will be read.

• The value ranges shown in a contour plot may differ from the value ranges reported by the function calculator. Contour plots show either cell/face values or node values, as described in Variable Location: Vertex and Face Options. Function calculator results are based on either cell/face values or node values, in accordance with how the variables are stored. Note that, for Fluent results loaded into CFD-Post, all variables, including X, Y, and Z, are stored at either cell centers (for 3D regions) or face centers (for boundary regions) — not at nodes. As a result, the minVal() and maxVal() functions return minimum and maximum cell-centered values of X,Y, or Z on 3D locations, and minimum and maximum face-centered values of X, Y, or Z on boundary regions.

• CFD-Post does not account for surface tension forces.

• Certain real gas properties are not available in CFD-Post for use: gas constant, molecular viscosity, specific heat, and sound speed.

• The variable Boundary Heat Flux Sensible is available only for boundary types velocity-inlet, mass-flow-inlet, pressure-inlet, pressure-outlet, pressure-far-field, and outflow.

• For transient Fluent cases, there is no support for adding or removing time steps in the timestep selector.

• There may be problems postprocessing transient Fluent cases that involve boundary name or type changes at intermediate time steps.

• There is no support for loading of a subset of domains. All domains are always loaded.

• A DBNS solver with laminar flow will have zero shear stress on all walls. Force calculations will not include viscous component in such cases.

• CFD-Post will not display any shear stress values on coupled non-conformal interfaces as shear stresses are undefined on such interfaces.

• CFD-Post cannot read Fluent cases that have CAS and DAT files output in different directories.

• You cannot use X, Y, or Z variables in expressions or plots in moving mesh transient cases. For example, instead of an Isosurface of X, use a YZ Plane.

• Surface streamlines cannot be created on wall boundaries as wall velocities are zero. The recommendation is to create the streamline based on the Wall Shear vector. Ensure that Wall Shear is in the file; if it is not, return to Fluent and export that variable.

  Alternatively, you can use the near wall velocity for streamlines (and other plots) by setting CFDPOST_BOUNDARY_DATA_FROM_ELEMENTS before running CFD-Post.

  In the regions where the mesh is coarse and vector variable gradients are steep, streamlines in CFD-Post may hit walls earlier than similar streamlines in Fluent. This is due to a difference in computation methods, and can be avoided by refining the mesh.

• Molar Weight will always have units of kg/mol in CFD-Post, but units of kg/kmol in Fluent. This will be true for all quantities involving 'mol' or 'kmol' in units.

  To learn how to control the units displayed by CFD-Post, see Setting the Display Units.

• When creating Streamlines for Dual Cell heat exchanged Fluent cases, exclude Auxiliary Fluid domains from the Domains list as these domains can cause the streamlines to terminate too early.

Differences Between CFD-Post and Fluent

• A line in CFD-Post of type Sample gives results that match with Fluent's 'line' if the environment variable CFDPOST_BOUNDARY_DATA_FROM_ELEMENTS is set to 1. However, a line in CFD-Post of type Cut gives results that do not match with Fluent's 'rake' as the former in infinite and the latter is clipped.

• Plots of velocity vectors on wall boundaries do not match between CFD-Post and Fluent. Fluent always uses adjacent cell velocity for plotting vectors whereas CFD-Post uses node velocity (interpolated from cell/face values).

• The results of calculations by CFD-Post for Fluent 2D cases are for a reference-depth from the Fluent case file. For axisymmetric cases, the reference-depth is ; that is, the results calculations are for the complete cylindrical region, and not what is shown in the viewer (which is a sector from the complete cylinder). This matches the behavior of Fluent.

  Results will be consistent for all quantitative calculations on all locations. For example, a slice plane will be assumed to be cutting the full cylinder.

• CFD-Post reads Total Pressure data from the Fluent results file if this quantity exists. If the data is not supplied in the file, this quantity is not calculated by CFD-Post.

• Averaging of vector quantities to nodes differs between CFD-Post and Fluent. In Fluent, vector magnitudes are averaged to nodes explicitly; in CFD-Post, only vector components are averaged to nodes, while the magnitude is calculated from the components at the nodes. The two magnitudes will differ in cases with sharp vector gradients or high face angles (usually due to a coarse mesh).

  For example, if a node has four faces attached that have shear stresses in directions radially away from the node, in CFD-Post the shear stress values at the node will be much smaller in magnitude compared with the face stresses because the stresses in opposite directions cancel out. In Fluent, the direction is ignored and only magnitude is taken into account while calculating the stress magnitude at the node.

  Plots cannot display cell or face data directly, only nodal averages. However, cell and face data will be used in quantitative reports on volumes, boundaries, planes, iso clips, and isosurfaces (averages, mass flows, integrals). Lines, polyline, and points will use only nodal averages for quantitative calculations.

• Velocity magnitude values for Fluent in CFD-Post are not in good agreement with Fluent results for cases with multiple-frame-of-reference or sliding-mesh models.

  For cases solved with relative velocity:

  • The "Velocity in Stn Frame" plotted in CFD-Post is equivalent to "Velocity Magnitude" in Fluent. Similarly, other quantities dependent on Velocity such as Total Pressure or Total Temperature will have the suffix "in Stn Frame" (e.g. Total Temperature in Stn Frame corresponding to Total Temperature) for stationary frame variables in Fluent. Variables in the relative frame of motion will be without this suffix.

  • There is no Fluent equivalent for the CFD-Post variable "Velocity" as this represents a relative velocity in the local reference frame of the domain (which is not available for postprocessing in Fluent).

  • There is no CFD-Post equivalent for Fluent's "Relative Velocity". In Fluent, "Relative Velocity" is always relative to a global frame of reference (which you can select in Fluent Reference Values panel; if no reference frame is selected, an "Absolute Velocity" is used, not a "Reference Velocity").

  • When loading Fluent results, CFD-Post does not calculate global ranges by default as this would be too time-consuming (there is a warning to this effect when you load a Fluent case). However, when the variable is used for the first time (for example, when it is plotted), and as timesteps are loaded, the global range should be continually updated.

• For cases with 1:1 interfaces, due to a difference in the handling on nodes at these interfaces, the number of nodes reported by CFD-Post will be different than the number reported by Fluent. However, the number of cells should match.

• In the cavitation model in Fluent, the minimum value for Pressure is limited by the cavitation pressure; (this is not done in CFD-Post).

• For the cavitation model, there are differences in the volume fraction values between Fluent and CFD-Post.

• For some cases (for example, shell conduction model), the number of cells/elements reported by Fluent is more than that of CFD-Post. This difference is due to the additional cells Fluent creates internally for solving some physics; these are never written into the case file. Fluent reports include these cells as well.

• CFD-Post and Fluent may use different sources of data when generating contour plots. For details, see Variable Location: Vertex and Face Options.

• CFD-Post and Fluent display contours differently in the vicinity of a hanging node. Fluent takes values from cells only on one side, causing a discontinuity of contours. In CFD-Post, the hanging node is made to be a conformal node and takes values from cells on both sides, making a smoother contour.

• A periodic surface in Fluent is actually a pair of surfaces. In CFD-Post this pair appears as a Periodic object and a corresponding Periodic Shadow. When looking at quantitative results in CFD-Post, you need to look at a surface group that contains the "periodic/periodic-shadow" to see output that is in agreement with Fluent's results.

• Field variables may be discontinuous across an interface that joins domains of differing porosity. Variable values on the interface boundaries are not averaged across the interface. You can inspect variable values on each side of the interface separately.

• There may be substantial differences between gradients calculated in the Fluent solver and gradients calculated in CFD-Post. The Fluent solver uses options such as boundary treatments and limiters to calculate gradients; CFD-Post calculates gradients independently of the Fluent solver, and does not have access to all of the same data.

  The gradients computed by the Fluent solver can be transferred into CFD-Post by exporting them as variables and then loading them into CFD-Post.

• When plotting velocity components on periodic boundaries, there may be differences in CFD-Post compared to Fluent when using .cas and .dat files. You should use .cdat files, as outlined in CDAT for CFD-Post and EnSight, to get the correct values.

• For Eulerian multiphase cases, the velocity of secondary phases is incorrect in CFD-Post compared to Fluent when using .cas and .dat files. You should use .cdat files, as outlined in CDAT for CFD-Post and EnSight, to get the correct values.

• Also see Quantitative Differences Between CFD-Post and Fluent.

Turbo Limitations

• CFD-Post can initialize turbo space only for domains that are enclosed with inlet, outlet, hub, and shroud regions. For more complex geometries you must set up the problem such that the region of interest is isolated into a separate domain that can be initialized in CFD-Post.

• When choosing a report template for a Fluent turbo report, choose Release 12 templates (which do not have the word "Rotor" in the template name).

  Report template that have "Rotor" in the template name are from Release 11 and require variables that are not available from Fluent turbo files.

• For rotating machinery applications, identification of components and ordering, regions, rotation axis, number of passages, and interfaces cannot be done automatically; you must supply this information on the Turbo initialization panel. When generating turbo reports, select variables, instance transforms, and expressions will require manual updates; for details see Procedures for Using Turbo Reports when Turbomachinery Data is Missing.

Limitations of Load Transfer to Mechanical

• In cases where forces on surfaces are transferred between Fluent and Mechanical, the forces displayed on the surface are read directly from the Fluent results file, while the forces on the corresponding mechanical surface are averaged to the nodes. When viewed in CFD-Post, the values of the surface and mechanical forces will not match.

Polyflow and FIDAP Limitations

• Some Polyflow and FIDAP cases may have interior surfaces that are read into CFD-Post as boundaries. Unlike other boundaries, these "interior boundaries" cannot be used to create Polyline objects by intersecting them with a slice plane.

• CFX Results files generated by Polyflow do not contain all the necessary information required for some automatic calculations in CFD-Post, including force and torque functions.

Limitations in the Export and Display of Fluent Particle Tracks

• If particle track files from Fluent were written with rpvar dpm/io/cfd-post/export-int64? set to #t (default is #f), then, in order for CFD-Post to read the particle track files, you must have environment variable CFXPOST_READ_64BIT_FLUENT_PARTICLE_IDS set to 1.

• It is not possible to group or color transient particles by stream.

• The size of exported files and the intermediate history file is limited to 2 GB on architectures that have sizeof(long)==4 (for example: win64, ntx86, and lnx86).

• When Fluent particle tracks cross periodic boundaries, there will be a gap between the point on one side of the periodic boundary and the point on the other side. This is most visible if instancing is enabled, but appears only in transient cases.

• CFD-Post displays particle tracks as segments, whereas Ansys Fluent displays particle tracks as points. This is particularly shown by transient cases when viewing tracks for a particular timestep: CFD-Post displays tracks as segments of the track from the previous timestep to the current timestep, while Ansys Fluent shows points at the current timestep. Because of this, the range of the color variable will include data that is not included by Ansys Fluent when displaying particle tracks.

• Computing the sum of any variable on any surface returns a value in CFD-Post that is the Fluent value divided by .

• In a case with two domains, the nodes on the boundary in Fluent will get their values from the domain that has the higher priority; CFD-Post uses the average of the boundary values from both domains.

• If Volume Fraction is not available in the list of variables for multiphase Fluent cases, the phase forces reported by CFD-Post will be same as the total force.

• Wall Heat Flux values reported by CFD-Post for moving and deforming meshes cases will not match those for Fluent. This is because Fluent adds pressure work to get the energy balance.

• For some cases, the fluxes (Mass Flow()@<surface> or AreaInt(Boundary Heat Flux)@<surface>) from CFD-Post are different from the values reported by Flux Reports panel from Fluent. This is due to some additional physics model-based calculations done by Fluent that are not available in CFD-Post. However, you can use the Fluent Surface Integral or Volume Integral panel results for comparison with CFD-Post.

• The Function Calculator may give variable averages on slice planes, isosurfaces, and interiors that are different from those given by Fluent. These differences may occur when the surface is cutting through a mesh face that joins two mesh elements. In this situation, CFD-Post may use the element-center data from a different element than Fluent uses. Note that as both elements are equally valid choices, both calculations are correct.

• Due to differences between Fluent and CFD-Post in the handling of vector quantities, velocity values can be different on 'interior' zones (conformal domain interfaces).

• In CFD-Post, on boundaries that have zero velocity, Total Temperature and Total Pressure will have same values as Temperature and Pressure, respectively (as expected). In Fluent, Total Temperature is different from Temperature for boundaries that have zero velocity; similar differences apply between Total Pressure and Pressure. This is a limitation in Fluent.

  If you export 'Total Pressure' from Fluent, the CFD-Post results will be closer to what Fluent shows.

• On boundaries, CFD-Post produces more accurate quantitative results involving geometric variables (such as X, Y, Z) than Fluent reports. This is because Fluent uses geometric variable data from adjacent cell centers instead of the boundary face centers. However, you can get CFD-Post results to match Fluent results exactly by setting the environment variable CFDPOST_MATCH_FLUENT_RESULTS to 1 before running CFD-Post.

• There are very small differences between Fluent and CFD-Post in the way that area is calculated for axisymmetric cases; this area is used in quantitative functions. Fluent calculates the area for any axisymmetric case as , where is centroid-y of the facet. CFD-Post extrudes the 2D geometry to create a 3D wedge (of wedge angle 7.5°) then calculates the area by repeating the wedge to create a 360° cylinder. This is similar to approximating the perimeter of a circle by measuring the perimeter of an inscribed uniform polygon.

• CFD-Post results match with Fluent "Vertex" values instead of "Facet" values for Species Reaction and VOF cases. To have results from CFD-Post match results from Fluent, set the environment variable CFDPOST_BOUNDARY_DATA_FROM_ELEMENTS to 1.

• Global variable ranges shown in plots are nodal (averaged) ranges.

• The Global variable range for a Wall Heat Transfer Coefficient is incorrectly reported as zero; use the Local variable range instead.

• For the cavitation model, there are differences in values for volume fraction and pressure between Fluent and CFD-Post. In CFD-Post, pressure values are not clipped to the cavitation pressure. The values for pressure and volume fraction displayed in Fluent are correct.

• Face/cell data is not available on any surface that was exported from Fluent and then subsequently used as a location in CFD-Post. Only nodal values are used for all qualitative (contours/vector) as well as quantitative purposes. It is expected that there may be differences in quantitative results when compared to Fluent.