# Numerical Viscosity?

 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 12, 1998, 17:49 Numerical Viscosity? #1 P. Diao Guest   Posts: n/a 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.

 July 12, 1998, 19:05 Re: Numerical Viscosity? #2 John C. Chien Guest   Posts: n/a 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?

 July 13, 1998, 07:18 Combat Numerical Viscosity with FLUENT/UNS #3 Russell King Guest   Posts: n/a 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.

 July 13, 1998, 07:43 Re: Combat Numerical Viscosity with FLUENT/UNS #4 Jonas Larsson Guest   Posts: n/a 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

 July 13, 1998, 09:30 Re: Combat Numerical Viscosity with FLUENT/UNS #5 Robin Guest   Posts: n/a >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?

 July 13, 1998, 12:02 Re: Combat Numerical Viscosity with FLUENT/UNS #6 Pat Diao Guest   Posts: n/a 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.

 July 13, 1998, 12:44 Re: Combat Numerical Viscosity with FLUENT/UNS #7 Steve Guest   Posts: n/a 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?

 August 21, 1998, 07:46 Re: #10 Davy Guest   Posts: n/a 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

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post maximsch2 Main CFD Forum 12 October 11, 2011 18:04 sonsiest Main CFD Forum 0 May 23, 2011 15:37 Ertan Karaismail Main CFD Forum 0 November 20, 2008 18:02 Dave Main CFD Forum 20 August 12, 2008 13:17 diaw Main CFD Forum 2 October 2, 2005 10:56

All times are GMT -4. The time now is 11:01.