Fluent FAQ
From CFD-Wiki
This section is empty. This is just a suggestion on how to structure it. Please feel free to add questions and answers here!
FLUENT
Solver Related
What does "floating point error" mean? How can I avoid it?
The floating point error has been reported many times and discussed a lot. Here are some of the answers found in the Fluent Forum:
From numerical computation view point , the basic operations performed by computer are represented inside computer in what is called floating point numbers. The errors that are either because of invalid numeric computation initiated by user or limitation of machine that is used are floating point errors.
1)Invalid Operations:- Simplest example is if one uses Newton Raphson root finding method to solve f(x)=0 and for some Nth iteration if we get x = x(N) such that derivative of function f(x), f'(x(N))=0 then formula for calculating next iterate x(N+1) = x(N) - f(x(N))/f'(x(N)) requires division by f'(x(N)) which is zero. Here you get divide by zero type of floating point error.
2) Over or Underflow:- Another type is having data with either too large or too small magnitude called 'overflow' or 'underflow' respectively.Such data cannot be physically represented on computer for direct processing by arithmetic processing part of Processor.
3) Rounding off errors :- While rounding off a decimal number , some significant digits are lost which cannot be recovered . e.g. if we round off 0.1 to integer (not greater than it called 'floor' of the given no.) then it is zero. If this value if further used for computation then it may lead to several errors.
SOLVER AND ITERATION -----I think if you set shorter time step, it may be good. Or changing little Under-Relaxiation-Factors, it may be good. In my experience, I set 1/3 Under-Relaxiation-Factors as default.� -----�also lower the values of under relaxation factor and use the coupled implicit solver� -----�Try to change under-relaxation factors and if it is unsteady problem maybe time step is to large.� -----�you can improve the ratio in the solve--control--limits, maybe that can help.� -----�you will need to decrease the Courant number� -----�If you still get the error, initialize the domain with nothing to 'Compute from...' Then click 'init'. Again select the surface from which you want to compute the initial values & iterate. This should work.� -----�Another reason could be a to high courant number - that means, that the steps between two iterations are too large and the change in the results is too large as well (high residuals)�
GRID PROBLEMS -----�this error comes when I start scaling grid. in gambit, all my dimension is in mm, when in fluent i convert it in meter using buttone SCALE. after it, when i iterate, about hundred iteration, this error appeared. but when i not scale my drawing to m...and let it be as in gambit..then the iteration is success. -----�hi I think you should check your mesh grid mesh is very high. your problem solve by selection a low mesh.� -----�Your mesh is so heavy that your computers resources are not enough. try to use coarser mesh.�
BOUNDARY CONDITIONS -----�In my case I had set a wall boundary condition instead of an axis boundary condition and then FLuent refuses to calculate telling me 'floating point error'.� -----�Your Boudary Conditions do not represent real physis.� -----�wrong boundary condition definition might cause the floating point error. For example setting an internal boundary as interior� -----�Once I had the problem, simulating a 2D chamber with a symmetry BC. I set the symmetry somewhere as �axe symmetric� and the floating point error occur� -----�check the turbulence parameter you set. reduce the turbulence intensity to less that one for first, say 50 iterations.
MULTI PROCESSOR ISSUES -----"I've had similar problems recently with floating point errors on a multi processor simulation. The solution for my problem seems to be to run on a single processor, where it runs fine....?�
WRONG INITIATION ----- Initiating the case with wrong conditions may lead to floating point error when the iterations start.
Model Related
What is the turbulent viscosity ratio warning and how can I handle it?
The problem can be caused by improper values for the boundary condition turbulence parameters. Check the fluent manual (which is kind of more like a textbook), about modeling turbulence.
For the case of internal flow, you basically have to consider the physical state of the fluid upon entrance to your control volume. If the fluid is coming into your volume from a fully developed turbulent pipe flow, it will have more turbulent energy than from a stagnant fluid. Think of lots of little vortices, which mostly mix things up, and those all have kinetic energy associated). This energy can be expressed as a nondimensional Intensity (a percentage is used). In addition, a Length parameter is specified.
How can I determine the inputs for a porous media or porous jump from flow versus pressure drop data?
How do I model heat conduction in a composite wall?
What pressures should be specified at inlets and outlets for buoyancy flow problems?
Are there any general guidelines on selecting a turbulence model?
How can both turbulent and laminar flow be included in one model?
Depends. Fluent cannot presently compute boundary layer instability and subsequent transition to turbulence using a RANS approach (ke, SST, RSM etc). CFX has a new feature to do this, so perhaps it will be incorporated into Fluent soon as they are both owned by ANSYS.
You therefore have two options :
1. If you know the point of transition (like on an aircraft wing) from experimental data or DNS simulations, you can impose laminar flow in some regions by meshing a separate fluid region, and enabling "laminar zone" for this region in boundary settings. That is also useful in heat transfer cases, if for example you have turbulent flow one side of a thermal wall, and natural convection on the other side.
2. A "near-wall" turbulence approach : Either k-omega, SST, or Low Reynolds k-E (which you have to select from the "Turbulence modelling/expert" menu), will damp turbulence near to the wall, either by empirical damping of turbulent "k" (Low Reynolds k-E) or by full solution of the omega equation on a fine enough mesh (k-omega/SST). If you have flows in small gaps in a larger, turbulent domain, in which large lengthscales of turbulence of course could not be supported, the flow will re-laminarise in a physically sensible (although perhaps not mathematically exact) manner. These models will also MAINTAIN laminar flow in external boundary layers, PROVIDED that you have a fine enough mesh (use the laminar mesh distribution guidelines in Fluent manual, too coarse a mesh will lead to non-physical turbulence generation in the BL). BUT they will maintain this laminar flow and evolution of the laminar profile (in the absence of significant disturbance by separation or impingement at the wall) forever, no spontaneous instability or transition to turbulence will occur. So check the length-based Reynolds numbers of walls where you think there will be undisturbed laminar boundaries, that there is not expected to be spontaneous transition of these BLs.
How to start a 3D simulation with an compressible medium and temperature changes? What is important to consider
What is the difference between the coupled and the seggregated solver
The coupled solver will solve all equations (conservation equations for mass, momentum and energy) simultaneously instead of sequentially (=segregated from one another). You should use the coupled solver when the velocity and pressure are strongly coupled (high pressures and high velocities). Very long calculation times can occur when you use the coupled solver.
In the coupled solvers, the Species Diffusion Term is always included in the energy equation.
When you use the segregated solver, FLUENT allows you to specify anisotropic conductivity for solid materials
look at http://www.cfd-online.com/Forum/fluent.cgi?read=40127
Choice of solvers depends heavily on the model being solved. The segregated solver solves based on the pressure, while the coupled solver solves based on density. This makes the segregated solver better at low speed flows and the coupled solver better at solving transonic / supersonic cases. I wouldn't recommend the coupled solver at any flows below Mach .4 (until the pressure based coupled solver comes out in the next release of Fluent). I've used the Segregated solver up to Mach 1.5 with great results, but the higher speed, the more mesh dependent you become (because the segregated solver tends to "smooth out" shocks), so you have to pay a lot of attention to your meshing.
The coupled solver tends to be more stable with the defaults settings. The segregated solver tends to be very sensitive to the allowable limits. When trying to get a solution with the segregated solver, DO NOT increase the turbulent viscosity ratio limit (unless you have a great reason to based on past experience or the physics of your current model truly exceeding that limit, but I've never even heard of that being realistic). Instead limit the pressure and temperature limits to reasonable limits (i.e. Plimits = Pstatic +/- (2 * dynamic pressure), and calculate the appropriate temps). You need to give the solution "room to move" while it reaches a solution, but you don't want to give it enough room where it goes out to some totally impossible numbers, and the limits help prevent this.
Solution Methodology
How do I carry out rotating body analysis, eg a rotating sphere or cylinder in flow?
Rotating cylinder problem ( assume circular ), can be done easily by specifying angular velocity on the cylinder wall. As i observed no need of moving mesh for this case. you need to specify the rotation axis with respect to which your cylinder is rotating.
How do I get better and faster convergence?
What is the role of under-relaxation parameters? What should be the optimum choice of these parameters?
They limit the influence of the previous iteration over the present one. If you choose small values it may prevent oscillations in residuum developing. At the same time the solution may need more time to converge. Keep the default values as they are given in FLUENT. You can decrease them gradually if necessary. Momentum 0.6, pressure 0.1, k 0.4, eps 0.4, mass source 1, viscosity 1.
User-Defined Function (UDF) Related
How do I create/build/load a UDF?
The simplest way to add a UDF into Fluent is to write your UDF in the C programming language and then use Define -> User-Defined -> Functions to either interpret or compile your UDF. It can then be loaded. Fluent provides good documentation of the UDF interface with numerous examples, so read that before trying too much.
Do I have to use C?
Yes and no. To hook your UDF into Fluent, you'll probably have to use on if the DEFINE_* macros that Fluent provides, and this is most easily done using C. However, you can write routines that are used in the routines that are defined with the DEFINE_* macros in other languages and then link them together. This requires some knowledge of mixed language programming, Makefiles, the text user interface (TUI) and is not necessarily very portable.
My UDF won't interpret or compile - what is wrong?
The answer depends upon what exactly has happened.
- If Fluent complains about not being able to find a compiler, then check to make sure that the compiler is properly installed. On Windows machines, it is possible to install the Visual C++ compiler without fully setting up the command line compiler (which Fluent needs to be able to find). In this case, you are likely to see complaints about things being "not recognized as an internal or external command, operable program or batch file" or missing DLL's.
- If you are interpreting, keep in mind that not everything that is supported for compiled UDF's is supported for interpreted UDF's. This is true both for the UDF interface and the C language. If you are doing something pretty involved and it fails inexplicably, try compiling to see if that makes a difference.
- There is also the possibility of coding errors. Keep in mind that your source code gets run through the C preprocessor (to change the Fluent macros into C code), so unintended interactions are very possible.
My UDF interprets/compiles but fails to execute - what is wrong?
This commonly occurs due to a faulty operation of some kind. For example, user-defined memory (UDM) is not allocated until initialization, so attempting to access a UDM variable before initialization can lead to a segmentation fault. Try to isolate wht cause, and then look for places where your expectation of what is available may not match reality. Finally, keep in mind that if you do something really bad, you may need to restart Fluent before even a fixed UDF will work.
Tips
How do I merge two mesh files into one mesh file?
To merge two mesh files the suggested utility is tmerge. The syntax of tmerge is simple.
utility tmerge -3d file1 file2 finalfile
To join the two interior faces use:
Grid->Fuse
from the menu with Fluent.
How do I write a journal file?
How do I add a comment in a journal file?
Any line beginning with a ; (semicolon) is treated as a comment.
How to set boundary condition?
How to write a XY-plot?
look at http://www.cfd-online.com/Forum/fluent.cgi?read=40200
How to set material properties?
look at http://www.cfd-online.com/Forum/fluent.cgi?read=38768
one example:
//define/materials/delete air_50c //define/materials/delete air_1bar //define/materials/change-create air air_1bar y incompressible-ideal-gas y piecewise-linear 2 298.15 1007 323.15 1008 y piecewise-linear 2 298.15 0.02606 323.15 0.02788 y piecewise-linear 2 273.15 1.72E-05 433.15 2.45E-05 n n n n n n y
How do I generate a hardcopy of a window?
display set-window 1 ; if window nr. 1 is the window you want to be hardcopied //display/set/windows/scale/form ; setting the options for the graph (colourmap) "%0.2f" //display/set/color-ramp bgr //display/set/hardcopy/color ; setting the options for the window< color //display/set/hardcopy/driver tiff //display/set/hardcopy/y-res 2400 //display/set/hardcopy/x-res 3106 //display/set/hardcopy/inv no //display/hard filename.tiff //display/set/hardcopy/inv yes //display/hard filename_inv.tiff
How to run multiple cases in batch mode
This could be achieved by running it from journal file. The example journal file that runs two cases is given as:
file read-case-data xxx1.cas solve dual-time-iterate yyy1 file write-case-data zzz1.cas file read-case-data xxx2.cas yes ; for discard cas dialog solve dual-time-iterate yyy2 file write-case-data zzz2.cas
Another example:
rcd filemname.cas yes it 10000 wcd filemname.cas yes
Have a look at this discussion: http://www.cfd-online.com/Forum/fluent_archive_2005.cgi/read/32615
How do I export Fieldview data for postprocssing during iterations?
This could be done with the help of menu solve->Execute Commands . Here are two examples:
Steady Case
file/export/fug/File_grid-%n file/export/fud/File_data-%n pressure velocity-magnitude x-velocity y-velocity z-velocity ()
Unsteady Case
file/export/fug/File_grid-%t file/export/fud/File_data-%t pressure velocity-magnitude x-velocity y-velocity z-velocity ()
You can chose the frequency of export from the Execute Command panel.
What does abbreviation X mean?
| BC | Boundary Conditions |
| B-L | Boundary Layer |
| CFD | Computational Fluid Dynamics |
| DES | Detached Eddy Simulation |
| DPM | Discrete Phase Model |
| FDM | Finite Difference Method |
| FEM | Finite Element Method |
| FVM | Finite Volume Method |
| GUI | Graphical User Interface |
| LES | Large Eddy Simulation |
| MUSCL | Monotone Upstream-centered Scheme for Conservation Laws |
| Probability Density Function | |
| PBM | ? |
| QUICK | Quadratic Upstream Interpolation for Convective Kinematics |
| RANS | Reynolds Averaged Navier-Stokes |
| RSM | Reynolds Stress Model |
| SIMPLE | Semi-Implicit Method for the Pressure-Linked Equation |
| SST | Shear Stress Transport |
| TUI | Text User Interface |
| UDF | User defined function |
| URF | Under Relaxation Factor |
| VOF | Volume Of Fluid |
What is the difference between FE and FV?
See the answer in the General CFD FAQ.
FloWizard
FIDAP
POLYFLOW
Gambit
Why does Gambit refuse to open my .dbs file and say that my file is already open? I get an error message - ERROR: IDENTIFIER "X" CURRENTLY OPEN.
Before opening your file "X.dbs", Gambit looks for a file named "X.lok" to determine the status of your file. If it finds the .lok file, you'll get the above error message (or something like it). If you are in a multi-user environment, you should check that it is not actually already open elsewhere, but in other situations the most likely reason that there is still a X.lok file is that Gambit encountered a problem the last time X.dbs was open. Deleting the .lok file should solve your problem.
Q: Why does Gambit complain about the number of nodes on edges being odd and then refuse to mesh a face?
A: It is mathematically impossible to create an all-quad mesh with an odd number of intervals on the outer edge loop. If this is inconvenient for you, you may consider a quad-dominant mesh (mostly quads, with a few triangles), or even an all-triangle mesh. Many users achieved good solutions with triangle surface meshes and prism (wedge) boundary layers.
Q: What are these boundary layers things defined in Gambit? Do they represent the real situation?
A: Gambit's boundary layers allow you to generate specific semi-structured grids topologies on faces that grow out from an edge or edges. You can specify the initial cell height, the growth rate, and a transition pattern that changes the edge-parallel interval count. There are several default settings, which can affect the quality of boundary layers. For cases with sharp corners, normal and offset smoothing can greatly improve quality. Such smoothing is off by default because it requires significantly more computation time.
Q: If my quad face mesh has cells with high skewness or large aspect ratios, the pyramiding procedure used by the tet mesher will frequently lead to failure, why?
A: This is because the triangles on the tops of the pyramids have very high skewnesses which can prevent tet meshing. Consider a quad face with a 10-to-1 aspect ratio. Connect opposite corners to create diagonals. This is the "top view" of the pyramid that would be created on this face. The triangles are very highly skewed. It is recommended that your quad faces bounding a region to be tet-meshed have aspect ratios of 5-to-1 or lower.
Q: I'm trying to mesh a geometry but I'm getting this message: “check the skewnesses of you face meshes and make sure the face mesh sizes are not too large in areas of small gaps.” I checked the skewness and it's low enough.
A: Your problem is most likely that you have small gaps where the local surface mesh sizes are much larger than the gap sizes. Refining the surface meshes in those areas is likely to solve the problem.
Q: I would like to generate grids for different zones using Gambit. How do I merge them together using Gambit or Tgrid later?
A: For a valid conformal mesh, mesh nodes on the faces at the interface of the two parts have to be matching within a tolerance. Then, you can either merge the nodes (using Tgrid) or fuse the zones (using Fluent). If you use Tgrid to merge the duplicate nodes, the resulting surface at the interface will have the boundary type as "wall" which should be changed to "interior" if both sides of the interface have same cell (fluid) zone. Fluent automatically converts the resulting surface after fuse to be of "interior" type if both sides of it has the same cell (fluid) zone.
Also, if you are not using Tgrid, you need to use tfilter tmerge3d to merge the meshes together before reading them into Fluent. Tgrid does the same when you load multiple mesh files at a time.
Q: How do I determine what kind of grid to generate? (I would like to known selection criteria between structured and unstructured mesh.)
A: Try this approach - consider the meshing options in this order: Single-Block Structured, Multi-Block Structured, Multi-Block Hybrid/Mixed, Fully Unstructured. Gambit can generate most of the cells types and topologies that Fluent can use (with the notable exception of nonconformal meshes). Here are some guidelines/suggestions:
- If you can generate a single-block structured mesh for your problem, then stop there. There is no need to go further.
- If your solution is having problem around a corner (or the like), try multi-block structured mesh. If you are getting improved solution, then stop there.
- If you still have problems around different part of the corner, try the unstructured mesh, with high density mesh around the corner. Before going to a fully unstructured mesh, try making only the problem region unstructured. If the solution is good, then stop there.
- If one part of the mesh still requires special attention, then you can use Fluent's adaptive unstructured facility to refine the mesh until the solution is acceptable. Ideally, you should still get a mesh independent solution.
- It is very important to be able to control every part of your mesh so that you can get good solution everywhere. This is more difficult with unstructured meshes.
- For many geometries, if you can use a structured mesh you will end up with fewer cells (this is particularly true in three dimensions). It is a good idea to use structured-type meshes in regions that will allow it, and use unstructured meshes everywhere else.
- Don't forget that Fluent can handle prismatic cells. If you have an unstructured surface mesh, Gambit can generate a layer of prismatic cells that will resolve boundary layers without requiring a (fully) structured mesh.
Q: How do I run GAMBIT as a batch process?
A: To run Gambit in "batch" mode, prepare a journal file (e.g., "test.jou"), then use the command : gambit test -in test.jou
I am having trouble uniting two volumes, what should I do?
"misclassified graph coedge - probably geometrical problem"
-> you can try healing the volumes
-> deleting the volume (without lower geometry), healing and uniting the faces, then build the volume again
Other Preprocessing Codes
Gambit Turbo
TGrid
Application specific codes
Icepak
Airpak
MixSim
Educational codes
FlowLab
