Evaluation of length scale ratio for LES, DES, SAS etc.
 

Hi,

This post is based on the guidance in Best Practice: Scale-Resolving Simulations in ANSYS CFD by F. Menter which is now in the CFX Help.

Before running a SRS (i.e. LES, DES, SAS etc.) a precursor RANS simulation is run from which it is possible to post-process and determine if the mesh in the scale-resolving regions is fine enough to capture to eddy scales that you require. The BPG (version 2.00) page 34 gives the equations:



but how is possible to get which is the maximum edge length of each mesh element (hexa, tetra, penta, pyra) from CFD-Post in a RANS simulation?

In CFX-Pre, when SAS, DES etc., is selected the Output Control / Results / Extra Output Variable List now includes Mesh Length Scale. Does anyone know what this is exactly because it is not mentioned in the CFX Help Guides? Maybe it is possible to run a SRS for one timestep just to get access to Mesh Length Scale in CFD-Post to evaluated . If anyone has conducted any SRS in CFX can they explain how they evaluated that their mesh is resolved enough for their purposes before running the time consuming SRS (or a few iterations of).

Thanks

You do not need exact numbers for this check. Approximate is close enough. So if you are considering this sort of model you should be closely controlling your mesh and you should have a good idea what the element edge length in the important regions are.

I think there is also the length variable accessible in CFD-Post. You would have to check it is correct before proceeding, however.

Glenn, you said that one should have a good idea of the element edge length, but what do you use to judge that? Do you approach a scale-resolving simulation with a minimum eddy size that you want to resolve (i.e. from well known energy spectrum) and then use the precursor RANS and equations above to refine the mesh based on some preliminary runs on a baseline mesh?

Just for the purposes of running a test case I am modelling the flow around a wall-mounted bluff body. So having made a preliminary mesh with a refined scale in the body wake, but the element size is not based on any prior knowledge/calcs (what would they even be?), have run a precursor RANS to I was intending to determine the length scale ratio, hence the original CFD-Post question.

Then the next question in mind for the SRS (SAS, DDES or whatever) is what eddy scales do I want to resolve: e.g. 50% down from the integral length scale. There is a plot in Turbulent Flows by Pope (attached here) which I think can be used to relate, generally, the required element size to the desired resolved eddy scales.

By doing this then there would be no need to run SRS for awhile and find the mesh has insufficient resolution to capture the desire eddy scale.

I think that as guideline as element size (Volume)^(1/3) can be used, and L_RANS/element size needs to be at least 4,5 mesh elements per turbulent length scale in the LES region. To be honest I have never run a LES from scratch, but I was trying to learn how to do it time ago and guidelines like these were given in some text I did read.

One of the documents I read is "Quick Guide to Setting Up LES-type Simulations" Prepared and compiled by Dr Aleksey Gerasimov
European Technology Group ANSYS UK Ltd

I have not done LES type models for a long time, but the approach I use for industrial LES models are:

* Do a RANS model to get an estimate of the turbulence field in the flow
* Work out the turbulence length and time scales in the flow
* Note you can skip the previous two steps if you already have a turbulence spectrum or good turbulence information for the flow.
* Use turbulence spectrums or estimates of Taylor length scales to establish the length scales you need to resolve.
* Generate a new mesh with mesh element edge lengths based on what is required. As highorder says you need a few elements inside the desired length scale so you can actually resolve a vortex of that size.

Glenn, what do you use to work out the timescale, I had a quick look through Wilcox's Turbulence Modeling in CFD but did not notice a simply relationship? Do you rather use adaptive time stepping and specify in CFX-Pre the CFL number to be about 0.5 and let the solver find its own time step?

I use adaptive time stepping and let CFX sort the time step out. But home in on 3-5 coeff loops per iteration, not a CFL number.

Hi Glen

1)For how many time steps do you run your simulation before starting the time averaging? ( I read at least 10 000 to start the turbulent structures)
2) For how many time steps the time averaging is usually conducted? (I did read at least other 10 000, thus 20 000 in total)

Thanks in advance

I run it until I am happy the turbulence has reached equilibrium, and then run it long enough that I have convinced myself I have enough that I am covering all important time scales. General guides like you time step count are dangerous as you can think of plenty of scenarios when they do not apply.

Glenn, you said above about aiming for 3 to 5 coefficient loops per iteration and not a CFL number, but as the attached images show you need to set conditions in the Analysis Type (e.g. CFL number) as well as in the Solver Controls (i.e. Coefficient Loops). What do you do in this regard?

Those controls are managing very different things. The time step control tab only controls the adaptive time step settings. The convergence tab only controls how convergence is handled. You want to make sure that you do not artificially limit the convergence by putting the minimum coeff loops to 1 or 2 and the maximum to a large number, maybe 10. Then you can adapt to 3-5 coeff loops knowing that the solver can use more or less loops if it requires it.

hi
 

hi, if anyone has this document "Best Practice: Scale-Resolving Simulations in ANSYS CFD" please share this for knowledge . advance thanks

1 second on google
http://resource.ansys.com/Resource%2...ef+Version+2.0