It was noticed in the CFD calculation of metal flow and soildification process, the viscosity of the liquid appears to be much greater than the actual physical viscosity of the material. Apparently the numerical calculation has caused the extra viscosity. Does anyone have ideas about this kind of viscosity, and any iedas on how to compensate it ? I'll appreciate any answers.

How did you come up with this conclusion or (observation)? How did you measure the actual physical viscosity of metal ? How did you compute the viscosity of the liquid (metal)?What was the method you used in the CFD code ? Was the solution grid independent? What is " numerical viscosity" ? Can you define it in mathematical terms?

I have recently been involved in predicting filling flows in moulds using FLUENT/UNS for several commercial organizations who have expessed concerns that CFD programs over predict viscosity and hence lose the definition of jets etc. This higher viscosity can be generated for a number reasons.

Firstly, for turbulent flows, most cfd programs employ an eddy-viscosity model. In which the behaviour of small eddies that are present in the flow, too small to be resolved by the grid, are represented by calculating a local turbulent viscosity and adding it onto the molecular viscosity to give an effective viscosity at each cell. This methodology is widely accepted in industry and is being used successfully. The higher values for viscosity due to this technique alone are nothing to worry about and we should instead, look to address the numerical errors to overcome any over-prediction of viscosity.

Secondly, the numerical schemes that are used within the cfd programs are open to error that manifests itself as numerical or artificial diffusion. This is due to the resolution of the cfd grid and can be reduced by either refining the grid or using higher order discretization schemes both spatially and temporally.

FLUENT/UNS can address all the points mentioned above.

Turbulence models in FLUENT/UNS (K-E, RSM RNG and LES) all use the eddy-viscosity concept in one form or another. However, any of the turbulence models should yeild accurate results for appropriate usage and we should look at numerical error to expalian any higher values for viscosity.

FLUENT/UNS has embedded solution based mesh addaption which can automatically refine the mesh where the shear layers are present, based on the local gradients. This minimizes the size of the mesh whilst maximizing accuracy and is a very powerful technique to combat numerical diffusion.

FLUENT/UNS uses higher order discretization schemes for both the spatial grid and the time step (if the flow is transient, as it is in mould filling). This means that the solution accuracy is high and that the important features of the flow are captured correctly, such as liquid metal jetting through the gates of the mould. This technique can often yield higher accuracy on a relatively coarse mesh.

These are the common reasons why you may experience higher viscosity and are by no means the only ones. There are more subtle things that can affect the solution but we would need to look at specific problems in order to persue them.

Turbulent viscosity was probably not the topic of the original post, but anyway, I would like to comment on Russell's answer regarding this.

Overprediction of turbulent energy is a major problem with many turbulence models that are commonly used today. This is true for all linear k-epsilon and k-omega models. These models greatly overpredict turbulent production in regions with large normal strain - that is stagnation regions, strongly accelerated regions etc. You also see a similar problem in swirling flows. The RNG "fix" that Fluent uses helps somewhat in certain kinds of flows but is in no way a general solution, in fact most of the time it doesn't work very well. Non-linear (or EARSM) models are better, but still are not mature enough to be a general solution.

I agree with Russell in that this is a "widely accepted methodology", but it sure isn't "used successfully" everywhere. An example from my field - if you try to predict turbine blade heat transfer with a linear EVM (k-epsilon or k-omega) you will greatly overpredict the heat transfer in the leading edge region (several 100% too high) and the too high turbulent viscosity/energy will also trigger too early transition and all kinds of problems. Using a coarse grid, which doesn't resolve all gradients sometimes "fixes" this problem a bit (that is why you see so many "good" results with linear models published even today).

Does fluent offer any non-linear EVM models yet?

Just my $0.02

>FLUENT/UNS has embedded solution based mesh addaption which
>can automatically refine the mesh where the shear layers
>are present, based on the local gradients. This minimizes
>the size of the mesh whilst maximizing accuracy and is a
>very powerful technique to combat numerical diffusion.

Is there a problem in choosing which variable to use to calculate how the grid should be adapted in which region? For heat transfer (especially natural convection) T, u, v and w can all be coupled so which variable should be chosen? Do you have a user set parameter that caps the total number of grid cells created? What is Fluent's experience in this area?

Thanks for all the responses. Being more specific about the problem, the following is the observation. We use ProCast (FEM) to simulate the mold filling process. Liquid metal flow, considering Re number, is in turbulent. If we use gravity as the the only driving force of the flow (use a large pour cup on the inlet and assume the pour cup is full of metal with atmospheric pressure and minimal velocity on top surface)to counter the viscosity, the flow moves much slower than what it should be. Grid size is not a fact. We used a finer mesh but it did not help. The major problem seems to be at the free surface of the metal (inside the mold). The numerical formulation caused the lack of moving force on the free surface.

To me that sounds like a contradiction. A finer mesh didn't reduce the problems but yet you claim that the problems are caused by numerical diffusion (numerical viscosity). A finer mesh should reduce your numerical diffusion! How do you know that your problems are related to the numerics and not to the models you use?

There are several areas you can look into to identify the problem and to find a solution. The mesh refinement is the first step. You have to do this several times in order to reach the conclusion. For example, just to run a case from 11x11 to 21x21 is not going to give you the answer. In turbulent flow with a wall boundary, you need 60 points to cover the whole boundary in order to get good result. This does not include regions outside the boundary layer. Plotting the skin friction vs the total grid number will give you some indication about the grid effect. Since the numerical errors are proportional to the grid size or the grid size squared, the numerical errors should gradually diminish as you reduce the grid size systematically. Having done this, the second step is to fool around with the turbulence model. At this point, you must have direct access to the code. If you don't have the access to the code, you can still change the parameters used in the turbulence model( some codes allow you to do this ). For example, you can adjust the Cmu parameter from 0.09 to 0.07 to lower the turbulent eddy viscosity. You should be able to see the effect easily in your computed results. There is no limit to this because "modeling is just modeling". With this approach, you should be able to fix your problem. There are always problem associated with code implementation, I mean how the code was actually coded. Without the access to the code, it's a black box. No one can help you except the code developer. ( whether a numerical scheme or a turbulence model is correctly implemented in the code could also be an important factor. What was printed in the user's does not always reflected in the version of the code you are running. Only the person who have access to the code listing can tell you what is in the code.) The turbulence model can always be adjusted for a particular application because it is very difficult to find a turbulence model with a set of universal parameters which will work for all applications.

As variables within the solution are closely coupled, the choice of variable on which to adapt is not so critical.

Obvious choices for adaption are pressure, velocity magnitude, turbulent energy, temperature, mach number, species concentration or actual error; depending on the application. There will probably be one that yeilds more cells but this can be found by previewing the cells chosen for adaption before they are actually adapted.

The number of grid cells to be added is controlled by the within the adaption process by the user. The overall number of cells after adaption can be reduced by simultaneously coarsenning the mesh where the gradiants are low.

There are other ways of adapting the mesh besides flow gradiants that can be combined in a bolean sense to give absolute control of the adaption process.

If you would like any more detailed information please contact me by e-mail and I would be happy to help.

I agree with your opinion. I met the same problem that I don't know how to define the force near the interface between the two different fluids. Some methods will cause different results which are not valid for the real problem. It'll be helpful if someone will provide the information about this problem, Thanks in advance, Davy