Hello,

I am fighting up against the high Reynolds number flow now (more than 10**8). It is known to me that the high Reynolds number flow is ¡§very difficult¡¨ to solve. But very less I can hear about the difficulties, especially some experiences. I have few experiences and some felling. They may be poor, but are felt and have been seen myself.

1) It is hard to do such an experiment for it because of high cost for equipment and difficulties in measurements. Hence a fine and reliable turbulence model can not be available.

2) To solve for it, it is needed to establish a fine enough grid system. Then, up to the present, the computer resources can¡¦t support such an enormous calculation.

3) When cells of the used grid are very small, they will cause numerical unstabilities or it will be necessary to use a meaningless time step for an unsteady problem.

Problems for 3): I have tried to calculate the 2-D incompressible N-S equations without any turbulence models for a NACA4412 airfoil in uniform inflow. I use the control volume method, the pressure correction method and an implicit SIMPLE/SIMPLEC scheme. A C-type, non-staggered, multi-block grid system is adopted. Some non-dimensional geometric characteristics of the inner fine block, which surrounds the airfoil, are provided.

Maximum cell area is about 9.1*10**-7.

Minimum cell area is about 1.5*10**-8.

Maximum cell slender ratio is about 240. It seems to me that for such small cells a very small time step, for example 10**-4 (Using a reference time T=U/C), is required. But I still failed. Does anybody know any way that may be used to improve it? Thanks!

wowakai

Did u try using limiters. There was a discussion about convergence problems just a few dicussions before this one. The last message in that ref gives a ref for this. It is always possible that ur scheme is unstable for high reynolds numbers.

It seems that the scheme you use may cause numerical boundary layes if the time step is not VERY small. Your mesh resolves it. This might provide poor results, especially if the solution near a boundary is important. The cure can be in using schemes of more coupled "p-u" nature.

Hi, I have no experience on such high Reynolds number flow, 10^8. But I found a algorithm for incompressible flow, which is based on the project method and the Godunov procedure is applied. According to the author, this algorithm can remove the cell Reynolds number constrain, which may be your problem.

The problem is not related to the absolute values of the Reynolds number, the absolute values of the cell size, or the absolute values of the time steps. It lies in the finite difference or finite volume cells. The question really is : With this numerical formulation, can I get a solution for this FD cell or FV cell ? ( with some arbitrary initial conditions for the un-steady flow case.) So the answer to the secret is in your formulation. Look closely at your formulation, check it out on several simpler configurations, including the Reynolds number values ( for a range of Re ), then hopefully, you will be able to find the answer. In 2-D, I would try the simplest method of using the stream function-vorticity formulation and the first-order up-wind scheme first to develop some feeling about the formulation. The high Reynolds number flow is not difficult to compute, the problem is we simply don't know how.

What do you mean by difficult? convergency or accuracy? If you have problems with convergence, you may need to look hard into your scheme and your coding because Hi-Re should not bring any problem to the convergence. It is simple because if the Re increase to infinity, the flow becomes inviscid and there should be no problem at all. However, if you have problems with accuracy, you are absolutely right. For Hi-Re flows, the viscous terms are extreamly small except for in the boundary layers or wakes. In all schemes, there is a truncation error associated with the discritezation. If the viscous terms are small enough so that they are comparible to the truncation errors, I am afraid that you may never get reasonable solutions. There are few suggestions you may consider: (1) Try high-order scheme, the higher the order of numerical scheme, the smaller the truncation errors. (2) Use small grid size as you did. Small grids also reduce truncation error but will increase relative round-off error which is associated with numerical precision. When use small grids, try to use higher precision (at least use double precision). (3) Use smooth and orthogonal grids to reduce numerical dissipation (sometime called numerical viscousity). (4) Pay close attention to the treatment of boundary conditions, particularly if you have wall boundary. Numerical errors at the boundary conditions may completely kill the accuracy of viscous flows.

Good Luck!

Hongjun Li

Excuse me! But I am still thinking about this "high Reynolds number flow" problem these days. I wondered and have to thank you, those who have given me some useful hints or helpful suggestions.

It seems there should be no problems to solve the high Reynolds number flow just with correct high-order scheme, with smooth, orthogonal and small grids, with suitable problem setting, with good precision maintaining, with the algorithm/procedure developed by Godunov(I didn't get his article yet!) to remove the cell Reynolds number constrain. And then what is the left? Maybe the left problem is to seek a man, who has known all of the skills mentioned above and is free enough, and to support him with good computer equipments. It seems not difficult at all for the people. But what is the reason we have been staying constantly and saying --"The high Reynolds number flow is not difficult to compute, the problem is we simply don't know how," till now?

I have only PII computers for use. With constant and finite computer resources, I'd rather 1) use a fine grid with 2-order accuracy scheme than a coarse one with higher order scheme, in order to solve more vortex structures, 2) use small time steps, for small cells, to describe the vortex motion, 3) use the large eddy simulation with a dynamic model to avoid the choice of some turbulence parameters. I wonder if you will have any suggestions to me?

wowakai

All those thchniques you proposed to use or you are using are correct. The problem you are facing, not only you but everyone in this area, is how ACCURATE and RELIABLE the solutions are? The answer to this question depends on what you do you want to calculate. If you want to calculate the pressure distribution or flow angles, there is no problem at all. Even inviscid flow gives you very close solution less than 2% error. But if you want to know the EXACT drag force or the stress, you may have reached the limit of the current technology. 2% total pressure loss due to Hi-Re viscous, abslute or relative? For example, if an airfoil flying at Hi-Re has a drag coefficient around 0.03. 2% absolute error will make it ranges from 0.01-0.05, the solution seems close enough but in reality has no use in airfoil optimization; 2% relative is in the order 0.0006, which is beyond the accuracy of any CFD code on earth (commercial or home-made).

There are two issues in this argument: (1) The numerical issue. No matter what schemes you try to use, there are always unavoided errors associated with it. To understand this, you can make a simple test: run inviscid flow over a single airfoil using a N-S code by turning off the viscous terms, then look at the total pressure. You may never get zero total pressure loss. (2) Physics model, turbulence is still a mystery to human being. In most case, we use Reynolds-averaged N-S equation with turbulent models, which may not be physically correctly in reality. All turbulent models work but no one is perfect. In order to solve the REAL turbulent flow, one needs to use DNS (direct numerical simulation) to the FULL N-S equations. But this can't be done with your PII, neither with the most powerful supercomputer for Hi-Re.

You may do your own research in this area. But CFD has not come to the stage to make ACCURATE loss calculations even with mid-Re flows, although many people clam they can. The prediction of loss with CFD is down on relative bases. This is, to compare the difference between two or more designs of silimar geometry.

The above statements only apply to the accuracy to the solutions. If you have difficulte to make it converges, this is another story. In that case, you need to pay attention to your solution approach and the problem you are trying to solve. At Hi-Re, the N-S eq. is close to Euler eq., if you use incompressible and steady-state eq., you may have difficulties because, you know, there is no solution for incompressible Euler equations in rotational flows. You may try to use compressible unsteady-state equations. This will help you to resolve the convergence problem, but not the accuracy problem.

Good Luck

Dear Hongjun Li,

Thanks! You are so right! I am interested in the computation of DRAG force because of its importance and its playing key role in the Lift/Drag calculation. I am a CFD starter and have less numerical knowledge and experiences, except a few incomplete physical images or feeling that everyone may has. But it seems to me worth to consider such a problem to win my PhD degree. I don¡¦t know in what percent the drag error I can approach will be. 50%? 20%? 10%? Or even less, what is the level today¡¦s techniques can reach? Do you have a number in your mind? It is encouraging for me to know it!

I haven¡¦t learned any turbulence models till now, but can propose such an alternative problem to you. If there are two codes for choice, then which one will you have more confidence in the computation of DRAG force? 1)The first code is to solve N-S equations with a well-developed turbulence model; 2)the second one is to solve the FULL N-S equations without any turbulence consideration, but is capable of computing with 100(=10*10 for a 2-D problem) or 125(=5*5*5 for a 3-D problem) times cells than the former.

What is your choice? And why? I just feel not interesting in using turbulence models. Because there are even more complicated equations to solve for the turbulent stress, and follow with so many model parameters/constants. Then people still have to develop more skills or put more carefulness to maintain the numerical stability, and finally get hundred solutions for comparison/reference.

Best Regards,

wowakai

Dear Mr. Wu: There is a good CFD artical by Hirsch. In that paper, most of your questions may be got answered. This paper is "CFD Methodology and Validation for Turbomachinery Flows" AGARD-LS-195, 1994.

In terms of the codes, it depends on your purpose: If you want to develop a code or a method for practical applications, you may not use the full N-S with DNS, which is far beyond the capability of current computer speed and storage. But if you just want to do research to get your Ph.D., the DNS method is a very good topic.

Today's applied CFD technology still relies on turbulent models. Each turbulent model has certain application range, the choise of a model largely depends on your application. People may tell you that a more complicate model would give you more accurate results. But it is not always right. For example, if you want to calculate the viscous effects due to attached boundary layer (no massive separation, no large swirl and mixing), you may not use the k-e model which was not developed for this purpose. You may rather use the simple Baldwin-Lomax model with fine meshes at the near wall zone (first y+ near unity), or you may use more complicate Reynold stress model.

The accuracy of drag prediction is very hard to say. I have done some work in the past few years but I still have no idea how accurate we can reach. The most important part of using CFD in drag or loss prediction is the consistency. That is, when you change flow conditions (M, Re, etc.), the predicted drag or loss follow the right trend regardless the absolute level. Also, the solutions should be grid insensitive (you may never get grid independed drag, but it should not be very sensitive to the grid density). If you can get these two points, your code is great CFD code. To get there, you need to be very careful in selecting schemes, turbulent models, grid quality, and programming. Keep in mind that the only errors that are allowed in the code are due to the order of accuracy, and the imprefection of turbulent model. These errore are called system errors which are almost constant for the same grid density. Then, you can calibrate your drag prediction with test data (run as many tests as possible) to get an idea how much the system errors are. When you know the system error, you can closely get the actual drag from your prediction with similar grid density. The worst error is flow and grid dependend error due to improper treatment of boundary conditions and poor programming. This error is called 'random error'. If this error is large, the code may not be adequate for drag or loss prediction.

Hongjun

I would suggest testing the code against Blasius' boundary layer solution (flow past a flat plate at zero dp/dx). This should be done for Re numbers ranging from a few thousand up to, say, ten millions (eventually using three increasingly finer meshes at each Re). As suggested in a recent AIAA paper by Jameson et. al. (don't have the exact reference right here, e-mail me if you need it) the meshes should be constructed to have the same resolution at least through (=normal to the plate) the boundary layer. This can be done by placing the same number of meshpoints in the boundary layer coordinate (call it \eta); since this depends on x,y and Re, the vertical resolution will remain essentially unchangend for the different Reynolds numbers. Of course, one gets different meshes for different Reynolds numbers. By keeping the same number of meshpoints along the flat plate is unpractical, you will observe a growth of the cell's aspect ratio with increasing Re (roughly with the sqrt(Re)). Better refer to the journal article if the explanation about mesh generation is unclear. At Re=10 millions you will probably get an aspcect ratio of 1000 or 10.000. If at this extreme (laminar) Re number you still get a converged and accurate solution (especially compare the normalized Cf/Cd, which is independent of Re, for the different computations at the different Reynolds number as well as the normalized u and v profiles) you have fullfilled at least a necessary conditions in the code verification phase.