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.
USING A UDF -----�What I mean is really often when people creates UDF they generally forget that for the first iteration some variable can be zero. Therefore if you are divided a number by zero your solver will blow up telling you 'non floating error'. 'non' means 'not a number'. Depending on your UDF this kind of error does not effectively happens at the first iteration. An example, if you are simulated a domain with a stagnant water as initial condition and you are calculated for the first iteration something like 1/Re therefore lets call it BOOM !!! because Re=0 . To find this kind of think there a simple way : reread your UDF.�
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). 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.
Tips
How to merge two mesh files and make one?
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 to write a journal file?
How to commend a journal file?
look at http://www.cfd-online.com/Forum/fluent_archive.cgi?read=34815
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
Want to 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
Pre-processoring
Gambit
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.
possible errors and how to avoid them
meshing
WARN: Exact projection failed for node on edge xx near vertex xx. mesh size may need to be enlarged for this virtual edge if mesh is not acceptable
meshing failed for volume xx. This is usually caused by problems in the face meshes. Check the skewness of your face meshes and make shure the face mesh sizes are not to large in the area of small gaps
uniting two volumes
"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
Gambit Turbo
TGrid
Application specific codes
Icepak
Airpak
MixSim
Educational codes
FlowLab
