Hi all, There is a parameter in ANSYS Flotran called Artificial Viscosity, which can be used to make convergence easier. I can not get converged results without it. Does this parameter alter the final result? I mean, is my result trustfull, even if I use values well above the recommended ones (which is 10 times the effective viscosity) Best Regards, Luiz

(1). There are two key issues here; one is the mesh independent solution, and the other is the solution validation. (2). The first one will make sure that your solution is repeatable, that is converged and unique. (3). The second one will tell you whether your code and solution is useful or not. (4). Getting a solution by running a code, is definitely "NOT CFD". Just like the GE and Honeywell merger case, the European said it's "NO GOOD". (5). So, looks like that there are people day dreaming all the time.

Dear Mr. Chien, I did not understand what you meant by people day dreaming all the time. I got pretty repeatable results. The problem is that I just have an evaluation version running on few nodes, and I would like to know from the expertise, how close do I get from the real solution by using artificial viscosity parameter set to 10 in a Re = 10^7. Obviously I will have later a consulting services (running full version of CFD, with expertise) to validate this device I am working on, which is an object of patent. I am sure that I can count on your expertise about these "magic CFD parameters" and I am aware I am not good at CFD. (That is why I am writing to cfd-online...) Best Regards, Luiz

(1). First of all, I don't know what is in a commercial code. (2). And even if they allow me to see their source code, I don't think I will be able to answer your question in six months. That how long it is usually take to decode the source code. (3). In other words, your question was based on the assumption that someone out there knows the answer. (4). The best place is the vendor's support engineer. Anyway, if I were you, I would check out other commercial CFD codes first. (5).The question "I would like to know from the expertise, how close do I get from the real solution by using artificial viscosity parameter set to 10 in a Re = 10^7. " is truely a day dream. Because no one would be able to understand your question at all. (6). Mesh independent solution must be done first, and then validate your solution against well-known data or solution. The test case does not have to be exactly the same as your patent device, but it should be as close as possible. (even at this point, I don't even know what problem you are trying to solve. )

One of the first things I tried as a young graduate student was to ramp up the artificial viscosity on a test problem. I was fascinated by how it affected the solution, decreasing the time to converge to steady state, while smoothing out all the details. You may want to try the same experiment. At best, increasing artificial viscosity trades accuracy for stability, and the final solution is a smeared-out version of the true solution. At worst, increasing artificial viscosity completely destroys the accuracy, or even destablizes the calculation.

Artificial viscosity is often viewed as a minor enhancement, a simple add-on to reduce unsightly oscillations. However, in reality, unless its extremely small, the exact form and size of the artificial viscosity fundamentally changes the numerical method. Thus, when you increase the coefficient of artificial viscosity by an order-of-magnitude, you essentially substitute a completely different and unknown numerical method for the one intended. The choice of the coefficient of artificial viscosity is part of the basic design of the method. For a properly designed method, the coefficient should be "set and forget" -- the user should NEVER change it. Of course, experts will always fiddle around with any parameters they have access to, and slight variations in the artificial viscosity are often justifiable. But such twiddling gets experts into trouble all the time, so you can imagine what happens to amateurs.

There is most likely some mistake with your problem setup -- your boundary conditions are wrong, your grid is too coarse, the grid cells are too oddly-shaped, your time step is too high, or any one of thousand different things. By increasing the artificial viscosity, you're trying to overcome a mistake in the problem setup by changing the numerical method. Bascially, you're asking a stupid question, and the method is giving you a stupid answer -- change your question and not your solution method. Yes, a large artificial viscosity helps damp out the oscillations that are symptomatic of instability, but instability is probably symptomatic of a mistake in your setup, so if you want a legitimate solution, you need to elminate the cause of the instability. (If your problem is exotic, its also possible you've exceeded the capabilities of the solution method, but you're never going to fix this problem just by increasing artificial viscosity.)

While otherwise generic and unresponsive, John Chien is correct in saying that anyone unfamiliar with a concept as basic as artificial viscosity probably should not attempt to run a CFD code. However user-friendly they may appear to be, they're still not "black boxes" that can be used without any specific training. Just because you have the scalpels doesn't make you a surgeon. Why not take a few days and skim through a basic book on CFD?

(1). It seems to me that people are treating codes like Bible. (2). They first think that it has the true solution. (3). Then, they realize that they are not sure. (4). The reality is the source of the conflict comes from the Bible. That is: people think that it has the true solution. (5). The forum can not solve this problem, because it used to be a crime to think that the world is round. (6). The right approach is: I need the true solution only, why is it necessary to use this Artifical Viscosity anyway? You can't first commit the crime then read the Bible. You can't accept the artificial viscosity, then look for the true solution. A code with an artificial viscosity is like a Bible with nice stories. All are trying to get more readers and followers. Whether they will be able to get the true solution or not? It is like the struggle between the Capitalism and the Communism. (7). So, it is a good idea to think, and ask why. You will have the true solution, only when you have the answer to WHY.

Yes I am willing to read a very good CFD book. Could you suggest me a few? Best Regards, and thank you very much for your helpfull advices. Luiz

Just read his: "Computational Gas Dynamics". It's focused on inviscid compressible CFD. My only complaint about Laney's book is that the origin (the "why they work?" or "where they are coming from?") of the advanced numerical methods he is outlining (i.e. Van Leer FVS, Roe, AUSM, etc) is not always clear.

Another CFD book I recommend is the one by Patankar, "Numerical Heat Transfer and Fluid Flow". It's focused on incompressible flows and the SIMPLE method. His method is very widely used in commercial softwares (for incompressible and semi-compressible applications).

For CFD beginners I'd suggest the one by Anderson et al: "Computational Fluid Mechanics and Heat Transfer" by Tannehill, Anderson and Pletcher.

(1). The minimum requirement to do CFD is: the ability to do technical journal search, read CFD technical papers, and books. (2). CFD depends strongly on analysis. You can't do it by trial-and-error, or just get some comments from others. (unless you are repeating the standard problems which have been solved previously)

For an absolute beginner who just wants to spend a few days, which seems to be the case with this poster, I recommend the following:

J. D. Anderson, Jr., Computational Fluid Dynamics: The Basics with Applications, McGraw-Hill. 1995.

C. T. Shaw, Using Computational Fluid Dynamics. Available (for free) on-line at the following link: http://www.eng.warwick.ac.uk/staff/cts/cfdbook/

My only caveat is that neither book is more than a basic start. Since I don't have them at hand, I can't say how well they treat the concept of artificial viscosity in particular.

Of course, I certainly don't discourage spot reading of my own text, say, the chapter on artificial viscosity. But I would imagine that, as a whole, its more than a casual applications-oriented reader would want to know.

Regarding Mr. Parent's complaint, the part of the book which treats advanced solution-adaptive methods certainly requires especially careful study. I still like to hope that this is the most readily comprehensible treatment of this advanced material currently available. But for those who disagree, my web site list a full range of other books that cover some of the same material:

http://capella.colorado.edu/~laney/

dear bert,

very interesting information, that on uttilization of artificial viscosity.

Experience with this, other tools seems to confirm that solution get's stabilized but altered in a fuzzy manner, consequently attempts to demonstrate uniquiness of solution obtained wouldn't gain certainty eihter.

Question arises why CFD codes advocate the use of such stabilization techniques, if they basically alter the correctly tuned algorithm. Does what you said apply, have validity for a particular formulation only, e.g. FVM, FDM or FEM based CFD?

Please let me know some, Thank you, Frank

In my dissertation, I studied the effect of numerical (or artificial) viscosity of different numerical methods for the inviscid (Euler) equations, the core of any compressible NS solver. I tested each method by applying it to the shock tube problem, for which an (exact) analytic solution exists. This chapter includes many graphical results, so you will get a pretty good idea of artificial viscosity just by looking at the 'pretty' graphs.

My dissertation can be downloaded from my web site at,

www.cfd4pc.com/papers.htm

My personal opinion/answer to your question: If you are trying to get a solution to a Re = 10^7 flow, you better have the numerical viscosity COMPLETELY TURNED OFF, otherwise, your boundary layer has nothing to do with physical viscosity, and it could be an order of magnitude overpredicted. To make things stable, you need a very refined mesh (BL resolution req's for given Re is also discussed in my dissertation) and an appropriate time step (for explicit solver).

I hope this helps!

Axel

[budaksenak]

axel...how can i close the artificial viscosity for the ausm scheme....i develop the ausm scheme..where i dont need an artificial viscosity..