• CFD, Fluid Flow, FEA, Heat/Mass Transfer

Post-processing of CFD Results (- Last updated on 03-Mar-2024 -)

Extracting Engineering Information from CFD Results

Post-processing activity includes generation of detailed report with the help of quantitative data, qualitative data, contour plots, vector plots, streamlines, area-average values, mass-average values, pressure coefficient, lift coefficient, centre of pressure.

One of the commonly used term in post-processing and visualization technique is 'rendering'. This refers to the process of converting underlying mathematical representation of solid geometry into visual forms.

The screen is represented by a 2D array of locations called pixels. One of 2N intensities or colors are associated with each pixel, where N is the number of bits per pixel. Greyscale typically has one byte per pixel, for 28 = 256 intensities. Color often requires 1 byte per channel, with 3 color channels per pixel: red, green, and blue. An "image map" or 'bitmap' or "frame buffer" is a array or variable to store color data. Z-buffer is the element of the computer hardware/software that is expected to manage the depth of the image (in the z-direction - into the plane of the screen).The important of visual data is summarized in image below. Look at the comparative statistics of information retained by people: 80% in case of visual information, 20% of reading and just 10% of information reaching through ears.

Impact of Visuals

Excerpts from ParaView tutorial manual: "the process of visualization is taking raw data and converting it to a form that is viewable and understandable to humans. This allows us to get a better cognitive understanding of our data. Scientific visualization is specifically concerned with the type of data that has a well defined representation in 2D or 3D space. Data that comes from simulation meshes and scanner data is well suited for this type of analysis. There are 3 basic steps to visualizing your data: reading, filtering and rendering. First, your data must be read into ParaView. Next, you may apply any number of filters that process the data to generate, extract or derive features from the data. Finally, a viewable image is rendered from the data."

Before you proceed to generate a report

Check mass balance as sum of mass flow rates at inlet(s) and outlet(s), energy balance at all walls (excluding inlets and outlets), reverse flow at outlets, Y+ at all walls (minimum, maxium and area-averaged), minimum and maximum values of velocity, pressure and temperature in the domain... One may try to develop a script or journal to make these checks and report a summary.

Common Issues in Post-Processing

The maximum value of a domain (eg: maxVal(Temperature)@wallX) gives a cell-centred value (Fluent is coded with this method). The maximum value from a (probe) point corresponds to the temperature value of the nearest node (CFX and CFD-Post operate on this principle). The cell centred value must be used to obtain a more accurate maximum or minimum value as this bases the value on the centroid of the cell.

STAR: The output shows maximum temperature limited to 5000 in 3468 no. of cells... These messages very often indicate a problem with mesh or unreasonably high heat flux. Check the quality of it before running: Right click on your Region -> Remove Invalid Cells -> Preview -> The boxes should indicate 0 problem cells found for a good mesh. Additionally, visualize where this (unrealistic) minimum or maximum temperature is taking place by making a threshold: Representations -> Expand Volume Mesh -> Right click on Cell Sets -> Threshold). Create a lower threshold for unreasonable low temperature and higher threshold for unreasonably high temperatures. Note that temperature thresholds are ALWAYS in Kelvin no matter how solution units are set. In FLUENT one can try turning secondary gradient OFF.

Checklist for Simulation Result

01Has the overall mass imbalance of ≤ 0.01% achieved?
02Have the velocity and pressure profiles at inlets and outlets been checked for uniformity?
03 Has the pressure drop reported for porous domains been checked with expected value as per P-Q curve?
04 Has the contour plot been set as banded instead of continuously coloured?
05Has the precision of labels (number of decimal places) set as per the range of data on legend?
06 Has the format of number labels on legend set as per magnitude of values: float, decimal or exponential?
07 Has the material properties at inlets and outlets checked to be closed to expected and/or specified values?

These are some basic sanity checks which one should make before starting to prepare detailed report. One should always think how easy the plots are to read, interpret and draw conclusions.

Vector Plot

A vector plot is qualitative representation of spatial magnitude. The only limitation is that it can be drawn plane or a 3D twisted surface. For any vector or contour plot, one of the important consideration is to selection the number of colour bands (also called the legend).
  • This should be small enough to have a distinct interval and high enough to keep it legible and easy to read and distinguish.
  • A value between 8 and 16 normally is a good choice.
  • Note the example below has 20 bands (with 21 values) and how cluttered it looks. There are 2 colours very close in intensity and cannot be easily distinguished looking at the plots.

Vector Plot


Streamlines are very good representation of velocity field, at least to beginners in CFD. It is closely related to velocity vector and any inconsistency may arise only because of post-processing interpolation on coarse mesh. As theoretically explained, tangent to streamlines gives direction of velocity field at that point.

Streamline Plot

Contour Plot

Contour plots are "coloured-band" plots of any variable where range of value is represented by a single colour band. This is good presentation of information in both the qualitative and quantitative format.

Contour Plot


Iso-surfaces are surface or planes with constant value of a particular variable. CFX-post has feature to create interactively, same feature is available in FLUENT through Iso-surface option. Hence, to create a plane parallel to X-Y plane, Z value will remain constant. Iso-surfaces are also useful to visualize the effect of one variable on any other variable over the entire domain.


As on version 2021R1, there is no iso-volume function in Fluent pre-post. Adaption registers can be used to generate the data equivalent to isovolume operation and then exported into other formats. Cell Registers -> Field Variable and then change the Type to Cells in Range. Some post-processors (such as CFD Post) has capability to generate the volume of domain based on range of specified variables such as temperature or pressure.


An Iso Clip takes a copy of any existing location (plane, boundary...) and then clips (trims) it using one or more criteria. E.g. a outlet boundary plot which is then clipped by Velocity ≥ 1 [m/s] and Velocity ≤ 2 [m/s]. Clip operation can be performed using any variable, including geometric variables and user created variables.

Surface of Revolution

in CFD-Post, predefined options to create Cylinder, Cone, Disc, Sphere and "From Line" are available. The last one is a more general way to use any line (existing Line, Polyline, Streamline, Particle Track) and rotate about an axis.

Other features are: Point Cloud - To Create multiple points which is usually used as seeds to streamlines and vectors, Instance Transform - Usually used to re-create full plots from symmetric/periodic solution data, Clip Plane - Define a plane which when active all viewer objects in front / behind this plane are hidden

Hybrid vs Conservative Value in CFX

CFX Hybrid-Conservative

For visualization purposes, ANSYS CFD-Post uses hybrid values by default, because non-zero wall velocities may look incorrect for otherwise stationary walls with no-slip boundary condition. For calculation purposes conservative values are used by default This is physically correct. For example mass flow is calculated correctly — a velocity of zero would produce zero mass flow through the wall adjacent control volume which is clearly wrong.

Mass-weighted or Area-weighted?

The features explained above are more qualitative in nature and may not be used directly in design calculations which usually require a discrete value. This can be obtained by "area-weighted average" or "mass-weighted average" feature available in the post-processing tools. But, the choice of area-weighting or mass-weighting should be based on the gradients of the chosen field variable. For example, to estimate average temperature at a given section for internal flow, mass-weighted option is the correct method as explained below.

area-weighted averaging recommendation

In the pipe flow example above, for calculation of temperature at the planes shown by dashed lines, area-weighted option may not give the correct result as it is a function of mesh size near wall. In the example below, area-weighted average velocity at inlet and the two outlets will not be in the ratio of flow areas even though flow is assumed incompressible. This is because of the error in integration or summation due to sharp gradient of velocity in the boundary layer and mesh may not be fine enough to capture it. Also note that the narrower sections have 4 boundary layers as compared to 2 boundary laters in inlet section.

area-weighted averaging error

Area-weighted average pressure in a fully-developed turbulent flow exit:

area-weighted average dynamic pressure

Mass-weighted average pressure in a fully-developed turbulent flow exit:

mass-weighted average dynamic pressure

Example calculations: let's assume a 5x5 grid with total area of 70 [cm2]. The assumed distribution of velocity, temperature and density for each cell is also described.

mass-Weighted vs. areaWeighted Example

For this sample grid, the average velocity is 1.550 [m/s], the area-weighted average velocity = 2.171 [m/s], mass-weighted average velocity = 3.251 [m/s], average temperature = 37.7 [°C], area-averaged temperature = 32.9 [°c] and mass-weighted average temperature = 27.8 [°C]

Separation and Re-attachment

There are few post-processing operations which require not only a good insight into the flow physics but experience as well. For example, the estimation of separation length (the reattachment point) needs careful evaluation. There are many methods, one recommended method can be generation of y+ plot. By virtue of re-attachment, the velocity necessarily has to go close to zero and hence y+ or shear stress will follow the same variation. The following image represents y+ plot for flow over back-facing step.

Re-attachment point

Special variables such as Line Integral Convolution Visualization (reference ANSA Training and Brochure Documents):

Line Integral Convolution

General Recommendations for Report Preparation

  • One picture or sketch (preferably an isometric or sectional view) representing the extent, origin and axes of computation domain, boundaries and moving walls (if any).
  • Sectional view of mesh in area of interest highlighting the boundary layer, growth and orthogonality.
  • Mesh quality matrix, worst values of mesh Equi-angle skewness and aspect ratios.
  • The description of material properties and its thermodynamic behaviour.
  • Tabulated summary of boundary conditions and turbulence parameters.
  • Tabulated summary of solver setting: discretization scheme, wall function, relaxation factors
  • Contour plots
    1. Limit the number of colour bands to 10
    2. Set the decimal notation to FLOAT, INTEGER or SCIENTIFIC (exponential) based on mangnitude. E.g. for values ≤ 1000, it is better to use decimal notation istead of exponential format
    3. Chose the unit easy to read and interpret: e.g. [K] for temperature is difficult to quicky visualize in mind. For most of us, 37 [°C] which is out body temperature or 25 [°C] which is standard ambient temperature serves as reference
    4. Similarly, a value of 0.075 [m] takes more time to interpret than 75 [mm]. It is quicker to deal with integers than fractions

Postprocessing Simulation Results on Irregular Surfaces: Import surfaces as STL geometry and then imprint them in existing volume mesh within FLUENT Pre-Post. This feature is available in almost all modern post-processors including CFD-Post and ParaView.

post-Processing on Imported Surfaces

Note that an STL file is a surface file and cannot represent a volumetric region even if the surface is a closed one. This means that if you cut through it say to generate Iso Clip, you shall get the appearance of edges rather than a solid object. Steps to generate STL surfaces are: Slice or create post-processing surfaces using edges/boundaries of original geometry in SpaceClaim -> Save as .STL using Options and switch STL output to ASCII format -> Import the surface in FLUENT Pre-Post as explained earlier.

Surface Groups and Clipped Surfaces

Some programs (e.g. CFD-Post) have option to combine boundary surfaces to a named surface group for ease of post-processing. In FLUENT Pre-Post you cannot create a surface group but you can create a single surface for all the walls defining a fluid or solid zone. Then after you can clip the newly created surface based on X-, Y- or Z-coordinates to use say a symmetrical half of the domain.

Paragraph, Fonts...
  1. Chose font size ≥ 11 px, font-type should be easy to read. Calibri, Arial are few good fonts.
  2. Use line spacing of 1.50 or higher. For bullet points, it can be reduced to 1.25
  3. If paragraphs are not indented, quadruple-space the paragraphs i.e. add extra space before the pargraphs
  4. Keep margin of 20 ~ 25 [mm] on each side
  5. Add page number centred under footer
  6. Maintain uniformity of font sizes such as for Paragraphs, Headers, Captions...
  7. Use unique symbols for variables
  8. Do not use mix of small letters and capital letters for same variables such as u or U, p or P
  9. Use over-dot for mass flow rates such as
  10. List standard (Roman) alphabets and Greek alphabets separately
  11. Arrange the variable names in alphabetical order
  12. Keep a separate list for subscripts and superscripts
  13. Add page number in references, typically any documents (books, journals, theses, research papers...) having number of pages ≥ 5
  14. Do not use superscript of 'o' or '0' as degree symbol. All of the MS-Office programs Excel, Word and PowerPoint provide degree symbol (°).
  15. Do not use underline for words containing g, j, p, q, y
  16. Write all units within square brackets [...]
  17. No space should be left in front of (before) a punctuation mark
  18. It is better to write inline reference with page number (e.g. Sukhatme, 1998, p. 21)
  19. For all title of in-text citations, the first letter of every word except articles (a, an, the), prepositions (such as in, on, under...), and conjunctions (such as and, because, but, however ...) should be capitalized, unless they occur at the beginning of the title or subtitle
  20. In-text citations must provide the name of the author or authors and the year the source was published
  21. The references page should be double-spaced and lists entries in alphabetical order by the author’s last name

Spelling Errors:

  1. Note that there is no space before any of the punctuations such as . (full stop) , (comma) : (colon) ; (semi-colon) closing ' (apostophe) and closing " (double quote)
  2. There are some words which spell check cannot identify as error. There are words generated due to nearby key on the kewords: e.g. [any:nay], [out:our], [neat:near], [near:hear], [below:bellow], [field:filed], [from:form], [for:fro], [its:it's], [though:through], [it is:it it]
  3. Check all the occurrences of 'it' and ensure 'it' and 'is' are used appropriately. Note that its and it's are not same
  4. Do not use &
  5. Full stop is used only at the end of last entry of a bulletted list.

In ANSYS FLUENT pre-post (V19 or earlier), walls and section planes are diplayed along with partition boundaries. To remove the partition boundaries - try (cxg-stitch-shells). This SCHEME command needs to be used after every new plot operation. Alternatiely, you can try TUI: "define beta yes" followed by "display set duplicate yes".

  • Use same lower and upper limits of legends for contour as well as vector plots
  • Use decimal notation if variables are > 0.01. Even though scientific notations can be used, it is easier for human mind to read numbers as compared to exponential notations.
  • Use number of significant digits judiciously. For example, for most of the industrial applications, it is not important to specify velocity to the 1/10 of mm/s. The number of significant digit is also dependent on the units chosen. For example, 3 decimal places for [Pa] such as 1045.368 [Pa] is irrelevant where as it is a need if unit chosen is [bar] or [kPa] such as 1.034 [kPa]. Followings are more information about "number of significant figures or digits".

Number Significant Digits

Recommendations for Rotating Reference frame
  • Clearly specify the rotating and stationary domain, direction of rotation, location of the interfaces.
  • Show the overlapping view of meshes at the interfaces, if not 1:1.
  • Mention the location of the place used to estimate pressure heads developed by the machine. It is further recommended to use 3 or more close locations on the upstream as well as downstream sides to estimate the grand average values of the pressure.
  • The physics governing performance of turbo-machines uses many non-dimensional coefficients. Include the plots of important performance parameters such as pressure coefficients on the blades
  • On all the plots dealing with flow passage and blades, explicitly mention the suction and pressure sides.
Cell by cell data: A histogram can be generated in ANSYS FLUENT to check cell data. For example, CFL number is important in transient simulations. CFL number can be checked by post-processing operations: Results → Plots → Histogram → Set Up... → Select Velocity... under Histogram of → Select Cell Courant Number from the Velocity... category → Set the value for Divisions to desired value say 50, 100 or 200 → Click Plot.

Flux Values

Flux values are important to check the conservation of mass, momentum and energy. Note that in case there are reverse flows at the outlet, the area-weighted average values of temperature and pressure may signficantly deviate from expected value. In other words, the gain in internal energy of fluid as calculated from [mass flow rate] x [specific heat capacity] x [TEX - TIN] may not be equal to the heat gained by the air through the walls and the heat soures. However, this is more of a data interpolation error on finite cells at the outlet and has less implication on the global energy balance. In case of flows with heat transfer, it is important to set the temperature of fluid entering into the computational domain at the outlets (the reverse flows) close to the expected values to reduce the deviation with respect to thermodynamics energy balance described above.

The discrepancies increases with reduction in mass flow rates such as buoyancy-driven flows. Hence, it is important to move the outlet plane to a location where such reverse flows are not expected.

  • The mass flow rate through a boundary is computed by summing the [dot product of the density × the velocity vector] and the area projections over the faces of the zone.
  • The total moment vector about a specified center of action is computed by summing the [cross products of the pressure and viscous force vectors] for each face with the moment vector.

Probe Function: Some programs such as ANSYS FLUENT use mouse button click to probe values at an arbitrary point. STAR-CCM+ has a probe function separately defined. In ANSYS FLUENT, when you probe (typically right mouse button) in a contour plot, the output printed in console is the band of the contour plot where the probed location falls. It does not print the coordinates of the location and estimated value at the probe position. In order to print the location and value at the probe position, plot the contour along with the mesh (you can use Scene to combine a mesh and contour plot).

Plot HTC (Heat Transfer Coefficient) in ANSYS FLUENT

Heat Transfer Coefficient FLUENT

Custom Volume: sometimes it is needed to create a custom volume such as cylindrical or conical section and generate volume average for the nodes falling inside or outside it. The equation X2 + Y2 = R2 defines an infinite cylinder along Z-axis. How does one define a finite cylinder between points [0, 0, Z1] and [0, 0, Z2]?

  • Let A and B are the two ends of the cylinder with coordinates [x1, y1, z1] and [x2, y2, z2] denoted by vectors rA and rB respectively.
  • Unit vector along the axis of cylinder is defined by e = rA - rB
  • Let P be an arbitrary point along the cylindre axis is given by t.A + (1−t).B where t varies between 0 and 1
  • The squared distance between a point on the line with parameter t and a point r0 = (x0, y0, z0) is R2 = [(x1 - x0) + (x2 - x1).t]^2 + [(y1 - y0) + (y2 - y1).t]^2 + [(z1 - z0) + (z2 - z1).t]^2
  • The minimum distance between point r0 and axis of the cylinder is: R^2 = [ (x1 - x0)^2 + (y1 - y0)^2 + (z1 - z0)^2 ] + 2.t. [(x2 - x1)(x1 - x0) + (y2 - y1)(y1 - y0) + (z2 - z1)(z1 - z0)] + t^2. [(x2 - x1)^2 + (y2 - y1)^2 + (z2 - z1)^2]
  • The points falling inside a finite cylindrical volume of radius R and axis points x1 and x2 CANNOT be specified by inequality: cylindrical Volume
  • Above inequality only tells that point may lie within radius of the cylinder and does not check if the point lies between the points x1 and x2 on its axis.
  • Boolean operator can be used to truncate a cylinder. For example, a cylinder with left face at (0, 0, z1) and right face at (0, 0, z2) having radius can be specified as (x^2 + y^2 ≤ r^2 AND (z ≥z1 AND z ≤ z2)

volume CFD-Post

The picture above describes 3 methods to create volume in CFD-Post. The inside() function returns 1 when inside the specified location and 0 when outside - this is useful to limit the scope of a function to a subdomain or boundary. The step() function return 1 when the argument is positive and 0 when the argument is negative. This is useful as an on-off switch and alternatively if() function can also be used as a switch. sqrt(X^2 + Z^2) defines distance from the Y-axis and sqrt(X^2 + Y^2 + Z^2) defines a sphere. sqrt(X^2 + Y^2 + (Z - 0.5[m])^2) moves the sphere by a distance of 0.5 [m] in the positive Z direction. Nested conditional statement can be used to create more 3D shapes: if (0.005[m] <= x && x <= 0.025[m], 2.50, 7.50)

Booleans in CEL: Let's write an expression as dx = (x ≥ 0.05 [m] && x ≤ 0.25 [m]). The value of dx for 3 different values of x are as follows:

  • x = 0.0, dx = 0
  • x = 0.15, dx = 1
  • x = 0.50, dx = 0

Note that this expression can be used to define a finite cylinder of radius 0.1 [m] on x-axis between x = 0.05 [m] and x = 0.25 [m]. fincyl = (y*y + z*z ≤ 0.1*0.1 && x ≥ 0.05 [m] && x ≤ 0.25 [m]). CFD-Post offers 4 modes to define clip range: At Value, Below Value, Above Value and Between Values.

In STAR, stepFun = ($$Centroid[2] <= 50) ? 0 : 1 - this creates a step function at the global z-coordinate of centroids of cell ≤ 50. Multiple if conditions - Split a region (Split Regions by Function dialog) into 3 parts: ($$)Position[1] <= 2.5) ? 1 : (($$Position[1] >= 0.5) ? 2 : 0). In this case, after the split: The cells where 0.5 < y < 2.5 belong to Region 1, as the field function does not affect them. The cells where y ≤ 0.5 belong to Region 1 2, as it is the created region with the least cells. The cells where y ≥ 2.5 belong to Region 1 3, as it is the created region with the most cells.

Data Exchange

There is no direct option in any of the commercial software to read results from other commercial software in their native formats. However, most of the software provide options to export data into some common post-processor such as FieldView or Tecplot. The option to export and import data from CGNS format also exist.

Export option in FLUENT
The option File > FSI Mapping provides a method to transfer CFD data to FEA for 1-way FSI (Fluid-Structure Interaction) simulations.

FLUENT data export - CSV ASCII Format

Import option in FLUENT

FLUENT data import

FLUENT FSI Data Mapping

FLUENT FSI Volume Data Mapping

Import option in STAR-CCM+

STAR-CCM+ data import

Centre of Pressure

Centre of pressure - CofP (which depends on the location of each cell and pressure force acting on it) is not same as coefficient of pressure - Cp (which depends on the total pressure force and a arbitrarily chosen reference area). The center of pressure is the point on a body where the total sum of a pressure field acts, causing a force and no moment about that point.

CofP = ∫(x * P.dA)/∫(P.dA) or discretely as ∑(xi * π *Ai)/∑(π * Ai), Cp = ∫(P dA) / AREF

Force-Momentum equation about origin:
  • Let {F} = (Fx, Fy, Fz) and {M} = (Mx, My, Mz)
  • Mx = 0*x + Fz*y - Fy*z
  • My = -Fz*x + 0 *y + Fx*z
  • Mz = Fy*x - Fx*y + 0*z
  • As diagonal of the [F] matrix in {M} = [F] {x} is zero, they are singular (i.e. one or more equations are not independent). inv(F) does not exist and det[F] = 0.
  • Unit vector in force direction {f} = {F}/|F| = (Fx, Fy, Fz)/|F| where |F| = sqrt(Fx*Fx + Fy*Fy + Fz*Fz)
  • Moment parallel to F (pure couple) can be calculated by taking component of {M} along {f}. Thus: {MF} = [{M}.{F}] {f} = (Fx, Fy, Fz) * (Mx*Fx + My*Fy + Mz*Fz) / |F| / |F|
  • We need to find a location about which Mz = 0 then using the equations Mz = Fy*x - Fx*y + 0*z we get 0 = Fx*x - Fy*y. Thus, y = (Fx*x)/Fy
  • Mz = -Fx *y + Fy * x and y = (Fx*x)/Fy. Thus: Mz = -Fx*(Fx*x)/Fy) + Fy*x = (-Fx2/Fy)*x + Fy*x
  • Hence, x = Mz/(-Fx2/Fy + Fy)
  • Note: The equations used to calculate the CofP location cannot be used to calculate the moment at the CofP. The moments in those equations are the moments about the origin.

Rules of Thumb: Interpolation of Results

Pressure Loss Ratios


One of the expectations from a simulation engineer is to provide design recommendations that may help those who are not familiar with fluid mechanics and heat transfer or those who may not be able to interprete the contour plots. For example, if pressure drop criteria is not reached, one recommendation would be to increase the width of the flow channels. But this is only an opinion and cannot be classified as design recommendations. "Increase the diameter by 20% and increase the ratio of bend radii to tube diameter to value ≥ 2.0" is a design recommendation easier to follow and implement. In order to arrive at these numbers, one has to be familiar with the empirical correlations and thumb-rules. For example, the dependence of pressure drop on diameter of circular channels and gap of narrow channels are described below.

For circular, squre or nearly circular channels

Pressure drop in circular channels

For rectangular channels

Pressure drop in rectangular channels

Post-processing for DPM

When tracking particles in parallel, the DPM model cannot be used with any of the multiphase flow models (VOF, mixture, or Eulerian) if the Shared Memory option is enabled.

Post-Processing for DPM

ANSYS FLUENT reports the magnitudes of the interphase exchange of momentum, heat, and mass in each control volume as well as the total concentration of the discrete phase. These variables can be displayed graphically, by drawing contours or profiles and are available under the Discrete Phase Model... category of the variable selection drop-down list in postprocessing dialog boxes.

Particle states (position, velocity, diameter, temperature, and mass flow rate) can be written to files at various boundaries and planes (lines in 2D) using the Sample Trajectories Dialog Box accessed by Reports -> Sample -> Set Up... Histograms can be plotted from sample files created in previous step by Reports -> Histogram -> Set Up...

Trajectory Fates: Shed trajectories are newly generated particles during the breakup of a larger droplet and appear only if a breakup model is enabled. Coalesced trajectories are removed particles which have coalesced after particle-particle collisions and appear only if the coalescence model is enabled. Splashed trajectories are particles which are newly generated when a particle touches a wall-film. Those trajectories appear only if the wall-film model is enabled.

Overall Checklist

No. CheckpointRecord [Y/N]
01 Have the fluid and solid zones named as per material type say by adding air, ss, al, pl, cr (ceramics)... as suffix?
02 Have appropriate prefixes been added to the boundary names as per boundary type: e.g. mf for mass-flow, vi for velocity inlets, po for pressure outlets...
03Has the mesh quality been checked for skewness and aspect ratios (for boundary layers and for freestream elements)?
04 Have sliver elements been collapsed? With minimum size ~ 0.05 [mm], elements having area < 0.002 [mm2] or volume 0.0001 [mm3] are unreasonable.
05Have the areas of the boundaries been checked and matched with the values used to estimate boundary condition parameters?
06 Have the walls been grouped into logical surface-groups easy to maintain during solution and post-processing?
07 Have the inlet and outlet planes of a porous domain been assigned to separate internal patches?
08Has the basic checks been made: scale of mesh, quality, default interfaces settings (CFX may create unwanted interfaces)?
09Has the density, viscosity and thermal conductivity of fluid been correctly assigned as per operating temperature and pressure?
10Has the auto-save frequency and file name correctly defined? For runs on clusters, specify only file name without full path.
11For transient simulations, have the specific heat capacity and density of solids been correctly assigned?
12Has the relaxation factors for k, ε and turbulent viscosity been reduced to value lower than 1.0 say 0.25 or 0.50?
13Has the convergence criteria been set to low value such as 1e-05 or lesser? Run may stop early if set to higher number such as 1e-3.
14Has the discretization schemes set to first order for initial 500~1000 iterations? Gradually move to second order.
15Has the monitor points been created for global mass imbalance?
16In FLUENT, have contour plots been created? This helps avoid repeating the process on repeated set-up of different cases.
17Has a monitor for heat transfer through all walls been created? Do not include inlets and outlets.
18Have the interfaces of porous and fluid domains changed to type 'internal'?

Overall Steps of Simulations

The following table summarizes all the steps which one needs to follow to make CFD simulations. They have already been described in detail on various pages of this website. Yet, the following table shall act as a ready-reckoner for the information to look for.

StepDescription of the Step Activities Performed Tool Name
01Prepare the geometry Rename the parts as per identifier such as applicable boundary condition, material or interface type ANSYS SpaceClaim, HyperMesh, ANSA
02Inspect geometryCheck for interferences, gaps, proximities and leakages to ensure volumes do not mix and mergeSpaceClaim, HyperMesh, ANSA
03Create named selection or names zones / patchesTo apply required mesh setting and boundary conditions - easy to filter and select in subsequent operationsSpaceClaim, HyperMesh, ANSA
04Prepare geometry for pre-processorMerge volumes, imprint surfaces, share topology (merge overlapping surfaces)SpaceClaim, ANSA, Hypermesh
05Import the CAD geometry in pre-processor (meshing)Get boundary mesh and required refinement at curvaturesFLUENT Mesher, ANSA, Hypermesh
06Correct surface mesh for topological and quality issuesIntersections, proximities, leakages, skewed cells, high aspect ratio (sliver elements)FLUENT Mesher, ANSA, Hypermesh
07Define meshing parametersGlobal mesh controls, local mesh controls, boundary layer controls FLUENT Mesher, ANSA, Hypermesh
08Compute volumeRegenerate volumes for fluid and solid zones, ensure each volume is correctly identified FLUENT Mesher, ANSA, Hypermesh
09Generate volume meshCheck quality of volume mesh: skewness (≤ 0.90), orthogonality (≥ 0.10) and aspect ratio (≤ 50)FLUENT Mesher
10Improve mesh qualityUse mesh improvement tools (move and merge nodes, refine mesh) to meet required targetFLUENT Mesher
11Export mesh into solver format and read into pre-processorCheck the mesh, scale into metric unitsFLUENT Pre-Post
12Apply solver settingsDefine materials, boundary conditions, turbulence models, relaxation factors FLUENT Pre-Post
13Identify run-time variablesDefine monitor points and planes, section planes for contours, result back-up frequencyFLUENT Pre-Post
14Make runsMonitor convergence residualsFLUENT Solver and Cluster
15Post-process resultCreate contour plots, vector plots, streamlines, animationsFLUENT Pre-Post, CFD-Post, ParaView
16Create special plotsOverlap of contour and vectors, Iso-volumes, Import special planes for post-processing, uniformly spaced vectorsFLUENT Pre-Post, CFD-Post, ParaView
Contact us
Disclaimers and Policies

The content on CFDyna.com is being constantly refined and improvised with on-the-job experience, testing, and training. Examples might be simplified to improve insight into the physics and basic understanding. Linked pages, articles, references, and examples are constantly reviewed to reduce errors, but we cannot warrant full correctness of all the contents.