Hi all!

I have run simulations of a 3D shape of a real car. I first start with k-e Realizable 1st order and after 200 iterations I switch to 2nd order QUICK discretization scheme. After 1000 more iterations periodic oscillation appears in all parameters of the solution: masss-weighted average, Cd, Cl, residuals. Specification in Cd and Cl can be resumed thus:

Cd=0.3 +/-0.0017 Cl=0.02 +/-0.005

I'm wondering if I can assume this as a good solution because my grid is in the limit of the capacity of my computer (I mean that I cannot make more refines because RAM gets saturated and time computation becomes prohibiting). And can also anybody give me any results of any wind tunnel test made with a vehicle in order to see if the Cd and Cl results are given with a certain "tolerance"? It is to compare with my results and see if they are similar.

Another question is according to residuals and how fluent makes the computation. I thought that when I make a steady state computation this means that a "mean picture" of the flow is calculated, but this oscillations makes me think now that Fluent has captured a sort of vortex shedding somewhere in my model and that is making to oscillate the solution. But this makes me to think that the steady state computation and the way the solution oscilates is like a unsteady computation! I mean that solution behaves as if every iteration was as a kind of "time step", so I can see this periodical oscillation as time was running, but at the end, I am solving my model with a steady state solver, so I don't understant very well what is happening. Can anybody enlighten me in this?

Thank you very much!

I met the same question in the simulation of cyclone separator with a steady state solver. I feel this is related to density of meshes. Who can give the authoritative reponse to this question?

thanks!

Yes, I think so too. When my solution starts to oscillate, all residuals are below 1e-4 (also the continuity residual, that is between 1e-4 and 2e-4) , so I think I get an acceptable solution.

I hope someone else explain this a little. Thanks!

If your boundary conditions are constant in time, the solution should be steady. A steady state must be found(it doesn't mean that the flow is really steady in the physical sytem).

Oscillations in residuals occur usually when a zone with high gradients are not correctly meshed(boundary layers...)

Oscillations during a steady simulation can also occur if your geometry has some symmetry but your grid is not symmetric (strongly or weakly). Do not forget that a steady state can be only symmetric. The solver trys to find the steady state solution (the symmetric solution), but due to the unsymetric grid it cannot. The numerical solution oscillates arround the steady state solution just like it was unsteady...but the solution is false. The distribution of the flow rate between the right and the left can not be exactly equal...this leads to oscillations between the left and right.

So if there is a symmetry in your system, try to build a symmetric grid...for this reason avoid tetraedars...This is also true for transient simulations....

Many thanks for your reply Kharicha: it has been to the point. Due to the complexity of my geometry, it is nearly impossible to mesh with with a structured grid.

There's something that I am afraid of, after reading your answer. You said that "the numerical solution oscillates arround the steady state solution just as it was unsteady, but the solution is false". Do you mean that only the oscillation is false but it would be correct to calculate the mean (RMS?) of that oscillation as the solution of the problem, or otherwise the whole oscillating solution is wrong? I have allways an oscillation in my solution, but due to my residuals are 2e-4 or so, I thing that the mean of that oscillations, let's say in Cd or Cl, could be the solution of the steady state. Is this statement correct?

Thanks a lot! Regards, Freeman.

By false I mean "do not fullfill the steady and symmetric condition". If you are looking for a steady state solution, and you can not get it...it means that there is a problem somewhere.

I have some experience with using unstructured mesh (so not symmetrical), the solution was oscillating with high amplitude(residuals arround 10-4 amplitude 10%). But once I have used a totally symmetric and structured grid, the solution converged to 10-10 with less than 0.5% of fluctuation.

The solution was totally steady and of course symmetric. Then I used this solution as initial condition for a transient simulation. With this procedure I can be sure that the transient behaviour of my solution is not created by nummerics, but by physics.

The question is how much time you have for your investigation? If it is for a short time, then you can use a time or iteration averaged results...but you should have a limited trust on your results.

Many thanks, Kharicha: your replies are being very helpful to me!

When you say that your amplitude was 10%, are you referring to the solution of the Cd, Cl and so, or to the residuals? And are you referring to a steady or unsteady case? My Cd solution always fluctuates (I only run steady state simulations) less than 1% (and also some mass-weighted average of velocity and pressure of some "observation points" that I've created), but Cl has a 10% of fluctuation (by the way, I understand this percentage as the difference of the maximum "distance" in absolute value from the mean divided by the mean). Could I considerate it an acceptable steady state?

And yes, you're right: I don't have much more time nor computational resources to make an unsteady case and then use the solution as the initial solution of the steady state. When you say a time or iteration results, do you mean that you would calculate the RMS mean of the Cd plot for example (calculated with the values since the periodic oscillations begins of course)?

Thanks a lot! Regards, Freeman.

The percentage here is on the magnitude of the residuals, but I do not have the exact amplitude of oscillation of the solution (velocity, pressure...) but it was very high, the solution changes with iteration just like in a transient procedure.

So I repeat in my case I could not find a steady solution until I modified my grid.

The amplitude of residuals is not everything, verify that your solution does not oscillate with a big amplitude. An oscillation of the residuals with a constant solution is better than low magnitude residuals with fluctuating solution (velocity...).

How much is it for your Cd or Cl? 10% or more ? (amplitude =variation/mean value)

An example could be the simulation of a 2D laminar cylinder wake. If you perform your Steady state simulation and find von karman vortices, with oscillations in the residuals, the solution is not acceptable (amplitude of oscillation >~100%). But if you observe a small waves occuring arround the symmetry plane...this is ok. Then when you will switch on the transient simulation those waves will be amplified and give rise to von karman eddies.

So do you see big flow structures in your results?

If you have no time, perform the iteration average (RMS mean of the Cd plot)....

I have also the same question. I do the simulation of flow field in a cyclone separator, When I perform Steady state simulation, the amplitude of oscillation of the velocity is very high, the solution changes with iteration just like in a transient procedure. However, when I perform Unsteady state simulation, the amplitude of oscillation of the velocity with time step is very low. What is the reasion of this?

Thanks!

Thanks for your help and time kharicha! Here you can see a screenshot of one of the simulations (the worst I've found):

http://img380.imageshack.us/my.php?image=sim7qf.jpg

As you see, residuals are kept quite low (under 3e-4), Cd oscillation is 6% and Cl is 30%. Before the refine, Cd oscillation was 10% (with practically the same mean value of oscillation) and Cl was also 30%. The problem is that I am in the limit of my computational resources (with more than 750.000 elem. RAM gets saturated)

Flow structure seems to be "stable", I mean that wakes are steady and vortex shedding or other instabilities are not present at large scales. Perhaps, I see a little perturbation in the wake of the tire: the wake is not as straight as it should be, but I don't think it could be considered as an instability (perhaps it is like the small waves you said in your example of the cylinder). I wish I could refine as much as I wanted: it seems to reduced oscillations (but not residuals!?)

What's your opinion about these results?

And one other question I missed: if you had to choose between a YPlus refine or a refine by pressure gradient (or other preference if you have other), what would it be?

I can only make one refine ... and because of this I think it could be better a YPlus, but I not sure about it.

Thanks a lot!

To ICW

This could simply due to a bad initial condition used for the steady solution. This is important specially for turbulence modelling, I advice to start first with transient simulation with small then large time step, then switch to the steady solver.

second possibility:

It can be shown that a steady simulation with under-relaxation factors is equivalent to a transient procedure with a time step depending on the value of your underelaxation factors.

When you switch to a transient simulation with a specific time step dt you filter phenomenon that have a period smaller than dt.

And it is possible that ,in your system, dt is larger than the time scale corresponding to your underrelaxation factor.

In your system there exists a larger period (smaller frequency) Tmax, if you perform a transient simulation with dt>Tmax...you are likely to get the steady state solution (correspond to periode T =infinity)...

My guess is that your dt is too large for a real transient simulation, if you decrease dt to a certain level I am sure you will get again the oscillations observed with the steady solver...

So you have no vortices periodically released...your residuals and results look very accepteble for me... the oscillations in the results are very limited..this is not what I call transient behavior...

It looks ok!!

I do not know how important are your pressure gradient, but the effect (on mean flow and turbulence variables) of too high y+ is known to be very important...do not neglect this point...

To kharicha, Many thanks for your big help, I have a try.

LCW

Thanks a lot for your advice!

Regarding to the gradient adaption, I've got one more queston to solve. Without any gradient refine, max. gradient in static pressure is 1500 and if I compute it for turbulence kinetic energy, it is about 120, and for velocity magnitude is 25. I don't have any experience in gradient adaptions, so I don't know if they are acceptable or not. Have you any "rule of a thumb" to see if a gradient of static pressure, k, etc. is ok? I don't have still the "feeling" in gradient adaptions to make a decition.

Many thanks for all your help!

Those values are meaningless....

what is important is to a get a smooth solution. If you have the same gradient all along a line (example: between a rotation disk and a stationary disk) the solution is ok, even if the gradient is high.

But if two area of different velocity are separated by a region of high gradient, you have to be refine your grid until you get a smooth transition between the two velocities.

This is the case when you want to simulate kelvin-helmoltz instability occuring at the interface between two fluid layers with a relative velocity. At steady state you have an area of strong gradient between the two layers, the instability are created whithin the area of strong gradient, to get a correct solution it is necessary to resolve it correctly...

If you fulfill this rule, you will quickly get the grid independant results...

Thank you very much for your explanations Kharicha: they have been all the key to make me being sure about what I am doing. Now I understand that it's better to take an eye on my y+ values more than in the gradients, because the former are more meaningfull in a first look than the gradients... and I don't have much computational resources to go more than one refine beyond with the original mesh I made.

Thanks a lot again! Regards, Freeman

I have been away for some time now (I did not access this forum for maybe 3 months), and coming back I found that some people started spreading really wrong teachings around here !!! I'm talking about deep misunderstandings, dear Mr. kharicha.

Mr. Freeman, first of all, the results you obtained are not necesarily wrong. Might be wrong when compared to experimental results and what I want to say is that the mean values you obtained are not close to the real ones, mainly due to the turbulence model you're using. For really good results you should use RSM instead! But this of course will be out of the reach, considering your hardware. Realizable k-e is a good model anyway, it can give you 4-5% precision, but only when using a very good mesh. And for everybody out there trying this kind of simulation:

GOOD AUTOMOTIVE MESH = a (at least) y+=40-50 (area averaged value) mesh, especially in sensitive areas (car end), with B-L of minimum 6-7 layers and a good clustering behind the car (this is the region with most influence on final results)

The real reson for the oscillating results is the use of Realizable k-e with QUICK discretisation scheme. Let me explain this a little:

- Realizable k-e is a MUCH better model than standard k-e, meaning that it can give you more physics, more accurately. The immediate result is greater "risk" of capturing flow unsteadiness;

- If you didn't enabled QUICK scheme, trust me, you would have never seen oscillations in the results! 1st order discretisation scheme is very effective in damping them. So, QUICK comes also in this category of "more physics capturing" schemes.

If somebody doesn't belive me, I invite him to try calculating a flow with known unsteady behaviour, like flow past circular cylinder, using good turbulence model (let's say sst k-w or RSM) and high order discretisation scheme (QUICK or MUSCL) in steady-state mode. At a certain moment in the simulation, the unsteadiness will come out, for sure.

Mr. kharicha's idea of separating the flow domain in two, using the symmetry plane, has indeed the potential to "calm down" the solution through the elimination of one mechanism of unsteadiness: lateral vortex shedding. But this might not be quite enough if you are going to use RSM (there will still exist vertical vortex shedding)!!

But anyway, you are of course free to choose your own way for dealing with this problem or trust whoever you like. I only wanted to clarify some problems for the benefit of everybody on this forum.

Best whishes, Razvan

Any (constructive) critics is allways wellcome, so thanks for your post.

Well, you are right. I allways started with a 1st order discretization scheme in order to get faster convergence: when I got it, I switched to 2nd order scheme QUICK. I had never any oscillation in my results when in 1st order, but they were very imprecise.

After your post I'm afraid that if I had chose RSM model, my results would have been "worst" than the actual ones due to if I have already little oscillations with Rzble model, I would have captured more pysics in my model with the RSM and results have oscillated even more, haven't them?

Another interesting thing that I have read in many posts and yours is the fact that 1st order schemes damp flow instabilities by numerical diffusion: could you explain in a few plain words (if it is possible) how this "numerical mechanism" is able to do such thing?

And the last thing: can you enumerate the different kind of vortex sheddings that exist? Or is as simpler as it is one for each coordinate axis (the vertical, the longitudinal and the lateral)?

Thanks a lot for your time.

Regards, Freeman