I am looking at a simple cuboid configuration of dims 2*1*1 (X*Y*Z) and have an inlet 0.1m high located on the X=0 boundary supplying air to the space at 1.0m/s. The location of the supply is half way up the X=0 wall. Opposite to this is an extract i.e. located on the X=L wall. Same dims as supply.

The configuration is such that the flow is essentially left to right.

The mesh configuration and the boundary condition specification suggests that the flow is 2d.

The mesh is set at 40*1*20 and is uniformly distributed throughout the domain.

For now I am ignoring temperature influences and the flow is assumed laminar. Hybrid differencing is applied and gravity is switched off.

The results are puzzling and although the configuration is symmetric the results are not. i.e. the inlet 'jet' is predicted to be drawn towards the floor of the domain!

I have also re-set up the case, with the same details except the inlet and outlet suggest the flow is now 'top to bottom'. I have changed the dimensions of the enclosure so that essentially I am asking the code to re-solve the original problem but with the configuration 'rotated' 90 degrees clockwise. The flow is again predicted asymmetric and the flow moves towards the west wall. i.e. if the soloution plot is rotated back to its original position (90 deg anticlockwise ) the flow is again predicted to move towards the floor.

After a long intro' my question is simple. Why would I get an asymmetric flow prediction to a symmetric problem definition.

Whilst I initially posted this to the PHOENICS forum, as that's the code I'm using, I have now posted it here because the problem I'm observing may be cfd/user oriented and not necessarily PHOENICS oriented.

Any suggestions/comments are gratefully recieved.

You can have asymmetric flows in otherwise symmetric problems. This is even quite common in some applications. The coanda effect you notice (that the jet is drawn to one wall) is a typical symmetry-breaking phenomenon. You often see this kind of symmetry-breaks in ventilation flows where bouancy is important.

The symmetric solution with the jet in the center is probably an unstable solution and any small numerical pertubation will cause the solution to instead go towards a stable asymmetric solution. Which asymetric solution you get depends on inital conditions and details in your numerics (how you solve your equations).

Jonas, Thanks for your response. As a follow up, if I may, how can I GET such a symmetric prediction. i.e. if the prediction is more due to numerical instabilities and not the physics, then what chance cfd?

I suppose this is at the heart of the beast and will continue our drive to develop better codes and better non-obtrusive methods.

For now, how can I be sure that the predictions I get are based on capturing the physics of the problems and not the result of the numerical method? If, for instance, I wanted to look for jet attachment, and the length of the jet before it attaches to a neigbouring surface as say a function of inlet RE or problem geometry then I need to be sure that unwnated intrusions are not hindering my predictions/trends.

Mark

I think you missunderstood my previous message a bit - The asymmetric solution is most likely the physical solution (assuming that you haven't done any trivial error in your simulation).

In reality a small disturbance will cause the jet to go be drawn to one of the walls. In your simulation a small asymmetry in your numerical method will have the same effect. This is perfectly okay. What causes the symmetry break is not important.

The only way to be sure of your simulations is to validate your code for similar cases with experimental data. You should also test grid-independence.

(1). I can only say that based on my experience and my own code, it is "very difficult" to obtain asymmetric solution with your problem. (2). You can try to build a cardboard shipping box model, attach an office fan to the inlet duct, a couple of windows covered with kitchen plastic wrapping sheet from the inside. Test it with smokes. You can easily verify the flow field. (3). Your question is an excellent one. I have said many times that companies or persons using CFD codes without experience and validation are likely to die more than once. If you are interested in solving your problem, we need to know more about your problem setup, such as the code, the mesh size and arrangement, the boundary conditions, the turbulence model,etc. Also take a look at the "Boundary Layer Theory" book by Schlicting, there is a chapter on jet and wake. You need to study the jet flow field in great detail first.

(1). Your question is a very good question. (2). From my observation, I think, there is a general trend in using CFD in simulation. Americans tends to use it with eyes closed, British tends to use it and ask questions, German knows how to run the test first but does not know why the CFD results are different from the test data. (3). I think, the only thing I can say is Americans are hard working people.

Jonas is correct. In reality, the jet will be asymmetric and the direction in which the jet sways from the computation will depend on the numerics. A very popular example is the flow exiting a geometrically symmetric sudden expansion. Here, even changing the mesh distribution can effect the direction in which the jet sways. You will get a very good converged (stable) asymmetric solution. Experimentally, small perturbations or imperfections in the flow apparatus are enough to trigger the direction of the jet to one side. Quite a fascinating problem.

hello all,

sure this is the coanda effect.this is also not physical .one can check this out with simple experiment.i suggest u to refer some papers on jets,where this concept will be dealt with.sure this is not physical.Even a small assymetry in the domain may cause this.

Hi all,

although some good points have been made. I cannot accept that just because some numerical perturbations exist in the simulation that we may automatically assume the REAL physical purturbations will lead to the same solution.

1. The asymmetric aspects of the code can be due to the order of node sweeps, round-off, asymmetric discretization, linearization, etc.

2. The pysical asymmetries are due to imperfections in the geometry and boundary conditions and are usually functions of time. For example, a stalled diffuser usually has one separation zone larger than the other. Maybe because the wall has a scratch (and it can be very tiny due to expreme sensitivities to imperfections). Or it could be the start-up procedure since valves are opened slowly and are seldom symmetric not symmetric impulsive starts as we usually specify in the numerical diffuser.

To demonstrate that the numerical flow produced by 1 is the same physical flow in 2 is not easy and should not be assumed.

Although it has not been done much (atleast not in fluids) I think we should start talking about a PERTURBATION MODEL such that we start to control the purturbations deliberatly and in some sense in agreement with the known range of perturbations of the physical geometry and boundary conditions. This would require writing a code that introduces negligilble numerical perturbations relative to the modeled physical perturbations. Not easy indeed.

A couple of other points to consider is how a turbulence model on the RANS equations affects the instabilities. ie. this guy has reported a jet drawing to the wall...which may look much like the Coanda effect but does a coarse grid with a hi-Re 2 equation turbulence model and a wall function (my assumptions on what the model may be) capture the physics of the Coanda effect. I doubt it! The physics is certainly is an anisotropic and if all the assumptions that go into a standard wall function are satisfied well that would be amazing! Another point worth a look is what we expect from the grid and discretization ie. 40*1*20 with hybrid!! Is that going to capture much physics for a 3-D asymmetry?

Anyhow, I think we need to be very careful with these issues and hopefully the active research in the area will start to provide us with some practical tools. Currently there are some very lively discussions between people who belive in VLES (Very large eddy sim) and those who dont...we will see how it all turns out!

Regards................Duane

I tried to simulate this. Interestingly with time-dependent choice you always get a sumetric solution. but for time independent solution it starts off as symetric one but as you do more iterations solutions begins to become asymetric.

Bala et al, Thanks for your replies, they are most interesting. This problem will indeed capture the next few weeks? of my spare time. Interestingly, I too have observed the same effect as that noted by Bala. i.e. that a transient solution to this problem is seemingly symmteric as is the start of a steady solution, prior to convergence, i.e. (inlet/outlet inbalance) etc,. I will now explore when the steady converged solution starts to demonstrate deviations from symmetry.

Although I haven't exhausted my efforts studying what Im' observing, but for now, it does make me wary about the notion of applying a line of symmetry as a boundary condition.

I was puzzled by John Chien's second note. John are you saying that you find it difficult to obtain asymetric solution or that you find it difficult to obtain a symmetric solution with my setup?

Thanks for your help.

Mark.

(1). The nice thing about the commercial codes is that you can always get anything you want. I think, what you are discussing is the behavior of a code (when it is played by the user), not the real test data of the problem. (2). Like the Internet .com business, you can't survive with the code(s) only. The code has nothing to do with the physics, the real world, or the true result one is looking for. (3). This is the most fundamental mistake a non-CFD expert do in using CFD technology. (4). The simplest answer is to design a good experiment and obtain the test data fisrt. Then try to model the results with CFD approach. Whether the particular CFD approach taken is capable of producing a realistic result or not, is still up in the air. (5). But I guess, the right answer to your physical problem is steady-state symmetric, even though the unsteady-state solution can have oscillating behavior. The asymmetric steady-state solution is only the numerical solution from a code.(including the modeling of the geometry and mesh, turbulence model, and solution procedure) (6). In other words, you are trying to model a physical problem, and you can't get the right solution by running a code. And to model a physical problem, you need to understand the physics of the problem first,by studying the test data. (7). CFD forum is not a place to discuss the result of a code, because we know that a code can not produce a true solution, right from the begining. (8). If a CFD code can produce a real solution, then every country and every company would have stock piled all the available CFD codes in their computers. (9). So, let me state it clearly again, "A CFD code (or codes) simply can not produce a true result (by running the code)." But if, the person has extensive knowledge of the problem he is trying to solve, (that is he has study the problem and gathered test data), then if he models the problem properly, there is a likelyhood that he will be able to obtain the true solution he has been looking for. (that is, the true solution is not stored in the computer codes). (10). CFD deals with approximation and simulation. It is the modeling processes which produce a solution. The modeling process is not equal to running a code. When you have a code, the process is already fixed. By running a code with a fixed process(or model), it will not produce another solution. (that is, you can't fool around with the code to produce the desirable solutions.) That is why people are trying out various different codes to find out whether they can win the big lottery prize. (11). I am not against the desire to search for the true solution, by trying out various codes. But one also must be smart enough to know that it is not enough. More research must be done before the true solution can be found.

John I totally agree with you. A numerical solution(s) is only to a given set of I.C. and B.C for a p.d.e. It is trouble with many engineers who know v.little about maths modelling and numerical methods etc. that they always expect a real physical answer from a cfd code, without understanding the effect of limits imposed through their chosen b.c. 2. Full N-S =ns are time-dependent. Removing d/dt terms is adding one extra assumption. and there are many more assumptions one makes to simplify the modelling process just to be able to get an answer. In reality there is gravity, buoyancy turbulence and many more.

3. One can get more than one solutions for p.d.e's and o.d.e's (true for N-S also )there can be symetric but unstable solutions or asymetric but stable solutions to a symetric problem (all numerically correct). It is the job of engineer to decide what solution is physiclly possible and choose that solution as a true one.

This is where mathematicians & engineers differ. Engineer has to give meaning to numbers. For a mathematicians these numbers only mean varables or constants. For a modeller/engineer these are physical quantities be it a velocity, temperature or material properties etc. Same p.d.e can represent flow of water in a pipe or flow of cars on a highway. same p.d.e. can be used for heat transfer in solids or contaminate diffusion in lakes or in share price predictions in stock market

Unless people who are using the codes understand the physics behind the problem they are seeking solution for, you 'll have these questions.

hello all a mistake in my previous message.It is physical.

(1). Very good point here. (2). I'd like to expand it a little by an example in the aerospace industries. ( I mean, back in 80's) (3). In the aircraft design, analysis, testing and validation processes, the codes used are: (a).fast panel code integrated with CAD to do performance analysis and trade study. These codes normally will include empirical equations. (b). Linear Potential flow equation code to do inviscid analysis of 3-D model. These codes can not handle shock waves correctly, and they do not include viscous effect at all. But these codes can handle the full configuration, not just a wing. (c). The 3-D inviscid Euler equation codes to capture more accurately the shock waves in transonic and supersonic flows. This is the reason why you have seen a lot of inviscid Euler solver development in 80's. This is because shock wave is an important issue in transonic and supersonic flows. (d). The 3-D compressible, Navier-Stokes codes for turbulent flows to address the viscous effects, such as the drag, the boundary layer separation, the shock wave/boundary layer interaction, etc.. (4). So, as you can see that in the CFD approach, people simply do not just use one code to model the flow and design the product. This is a very important point to understand, because the whole aerospace industries will be laughing at our readers, if our readers are still thinking that a CFD code can solve the problem. And in addition to the various CFD codes used in the analysis, the wind tunnel testings are also done on the routine basis using various kind and size of wind tunnels. (5). So, even if our reader is an expert in using a commercial CFD code, there is very little chance of designing a product which will fly. You have to understand that a working product is not equal to some CAD drawings with colorful CFD pictures obtained from a simulation using a code. (6). On the other hand, the cut back in CFD research and development in aerospace and engine industries will sure attract some ill-prepared engineers equipped with quick turn around commercial codes to reduce the cost of operation. Serious problems will start to appear, just like the poor decision in the electrical power business in California. As a matter of fact, based on my experience in the last several years, engine business is already having the impact of the problem I've just mentioned. (7). If one creates a lot of underground holes and shock waves, don't you think that sooner or later it will trigger large earth quake in that area? Well, that's a different story. It is just timing.