CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > FLUENT

I dare you all...

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 2, 2006, 05:12
Default I dare you all...
  #1
razvan
Guest
 
Posts: n/a
I've been on this forum, actively or passively, 2 years by now. I have never posted any new messages because I never had to: everytime I needed to find an answer to a certain problem, I knew how to find it on the forum. And everytime I could help someone in need, I did so. I never pretended to be a smart guy, and tried as much as possible not to hurt anyone in any way possible. If unfortunately this had happened in the past, I appologise to the ones involved.

Due to some recent posts, I've decided to brake the silence and dare you all beautiful minds out there, over two interesting problems I came across in the past. These problems involve the use of steady laminar solver vs. turbulence models.

FIRST CASE: NACA 0012 2D airfoil

I made a 70,000 nodes fully structured grid with y+=0.8-1.2 over the airfoil (at Re=500,000, although this grid could be easily used up to Re=2 milion w/o noticeable error). At Re=500,000, the flow is almost entirely laminar, only at the last third of the airfoil transition starts . First, I have considered the case turbulent, so I used, starting with S-A, ALL turbulence models in FLUENT up to LES, including low-re-ke models. From RANS models, SST-kw was the one closest to the experimental values of Cd and Cl (with about 16 percent error), and of course DES&LES were much better. But at a certain point, I decided to make a laminar simulation, to have some reference point, or to see if the problem for such overprediction of Cd and Cl comes from the too early transition all RANS models predicted (SST-kw predicted transition to about 45 percent chord). My great surprise was the impossibility to converge the simulation using the steady laminar solver! The residuals first decended, but after a while, started to rise and at a certain point, stabilised around a high value, slightly oscillating. Interestingly, restarting and stopping the simulation and displaying velocity contours once in a while, I noticed that the velocity field was continuously evolving, but only in the region of experimentally turbulent flow (last third of the airfoil), like the LAMINAR solver was beeing able to calculate an unsteady TURBULENT flow. Continuing to iterate never led me to a converged solution (at least from the steady solver's point of view). One of my proffesors suggested that I should switch to unsteady laminar solver. I did so, and to my total surprise, the residuals slowly flattened and velocity field stopped oscillating. This way I reached a fully converged, truly, unquestionably, steady solution! With the unsteady laminar solver!!

You will be tempted to tell me that my boundary conditions were not appropriate, or the grid was not correctly constructed. First, I'm going to warn you that I've been using FLUENT almost 4 years now, and not empirically, but in the most accurate and responsible way, I have dealt with all sorts of problems, ranging from aerospace to steel industry, and solved them all succesfully. So, what I am trying to tell you is that I know what I'm doing, quite well. Second, for all ones out there not trusting my experience, I will gladly send you the .cas&.dat files, to examine and find the mistake (if any...).

SECOND CASE: Backstep 2D flow

The geometry consisted of a classic backstep configuration (H=step height, H=channel height before step, 2H=channel height after step). Inlet conditions: turbulence intensity 0.2 percent (practically laminar), distance from inlet to step long enough to achieve fully developed flow, distance from step to outlet 1.5 times recirculation lenght (about (10+15)H). Fully structured 85,000 nodes grid, y+= 0.8-2 for Re~17,000 (based on step height, H). To put it short, ALL turbulence models were able to reach steady state solution, from ske (most easily), to RSM (most hardly). Not ONE of them was able to predict ANY unsteadyness using steady solver. To say even more, switching to unsteady solver could not get me a real unsteady solution! Turbulence models were simply wiping any trace of unsteadyness in the flow, slowly but surely. The only model that could give me the right answer was of course LES (and DES too). It never crossed my mind to try the laminar solver. The flow was too strongly turbulent for that.

But, one day someone told me about High Resolution Methods. I don't know if you're familiar with the concept, but briefly, it means that laminar solvers coupled with certain high discretisation methods (at least 2nd order accurate) and a sufficiently dense grid, will behave much like LES does (because numerical viscosity induced by these methods acts like a SGS (sub-grid-scale) model from LES). I was very curious about that of course, and tried it on my backstep grid, which was dense enough for LES, so it must have been appropriate for HRM too. Not small was my surprise when I noticed that steady laminar solver could not reach steady state converged solution again (not even with first order discretisation!), and unsteady laminar solver with second order discretisation results were so very close to LES results!!!

Of course that in this case too, I am opened to send the .cas&.dat files to anyone curious or interested or even looking to hunt me down.

In the end (because I already wrote to much), I would like to thank you all that read this message. I can only hope that you find it at least interesting, and I can't wait for your answers.

With all due respect, Razvan
  Reply With Quote

Old   October 2, 2006, 06:18
Default Re: I dare you all...
  #2
Eilon Shimshi
Guest
 
Posts: n/a
Hi Razvan, I have no answer for you, but I can tell you of other cases that behave similarly.

I am running steady invicid 2D simulations of overexpanded jets. With first order discretization and a course grid, I get good convergence and a smooth jet boundary. When I try to increase the accuracy by using a finer mesh and a second order discritization I start getting ripples on the jet boundary (like KH instability) that increase as I continue iterating, somewhat like unsteady simulation. It sound's something like what you describe. I have found no way to avid this problem. But I'll start looking for literature on HRM.

Eilon

  Reply With Quote

Old   October 2, 2006, 21:04
Default Re: I dare you all...
  #3
zxaar
Guest
 
Posts: n/a
"One of my proffesors suggested that I should switch to unsteady laminar solver. I did so, and to my total surprise, the residuals slowly flattened and velocity field stopped oscillating. This way I reached a fully converged, truly, unquestionably, steady solution! With the unsteady laminar solver!! "

I only have few comments. One when you see that it converges with unsteady laminar calculations, did you ever wonder to as yourself about what has changed between these two approaches. From your description, my conclusion is the convergence is due to the fact that the central coefficient Ap is not strong, which favours convergence. So now if strong Ap gives you convergence, why not the Ap with steady solver gives you convergence, that means it is not strong enough. One another way to make it more strong is to apply more under relaxation, (may be urf around 0.075 etc, but in fluent case I doubt this approach as they mention they do not do this Ap = Ap /urf) Anyway, this Ap is the root of your problems and the solution to your problems. un-convergence in steady solver is nothing new. It can happen. If Ap is the issue, you shall be able to get the converged solution with first order upwind, since in this case Ap is always positive and mostly stronger than other elements). If you are using other schemes fluent use recontruction gradients to assist in them, so in case, the solution tries to blow up, they are limited, and this thing hampers the convergence, (this is also a known issue, by the way, fluent uses venkatakrishnan's limiter, you can find details about it).

"But, one day someone told me about High Resolution Methods. I don't know if you're familiar with the concept, but briefly, it means that laminar solvers coupled with certain high discretisation methods (at least 2nd order accurate) and a sufficiently dense grid, will behave much like LES does (because numerical viscosity induced by these methods acts like a SGS (sub-grid-scale) model from LES). I was very curious about that of course, and tried it on my backstep grid, which was dense enough for LES, so it must have been appropriate for HRM too. Not small was my surprise when I noticed that steady laminar solver could not reach steady state converged solution again (not even with first order discretisation!), and unsteady laminar solver with second order discretisation results were so very close to LES results!!! "

About the method you are talking about, they are used for doing MiLES, which uses the property you described. But they are for LES calculations (unsterady), why you want to compare them to steady calculations and make some judgement. Anyway if you do want to use laminar calculations with higher order scheme, the issue is still the limiter and gradient calculations. I guess by calculating gradient more appropiately the problems in convergence might be handled. But you can change the way fluent calculates the gradients (by Green-Gauss). So the situation might not change. I would suggest you to try it with another solver with more freedom. Take openFOAM for example, you can use least square based gradients, and play with Gamma scheme to see if it converges.

We do not doubt your knowledge, but thinking that after using fluent for 4 years you can not make mistake, is little arrogant remark in my judgement. There is always scope for learning.
  Reply With Quote

Old   October 3, 2006, 01:20
Default Re: I dare you all...
  #4
razvan
Guest
 
Posts: n/a
Dear Zxaar,

I can see from your response that somehow my post offended you. As I already stated, it never was, or will be my intention. I am glad that you joined the discution, I'm prepared to give you all the credit you deserve.

All I wanted was to show that the possibility of divergence in subsonic regime is real even in Fluent. And that using the appropriate case setup. Why am I so confident in the setup of these cases? I've been doing this type of problems from the beginning, under the supervision of some very good proffesors (I graduated from Aerospace Engineering 2 years ago and now completing my Master degree in Gas Dynamics). They've been my playground for almost 6 years. I admit that I am young, and there is so much more to learn for me. Maybe sometimes I'm too confident in my abilities, which may appear as arrogance to some people. I'm more a FLUENT user than a CFD theoretician. I'm more an engineer than a mathematician. I could have doubdts for the setup of a coupled heat and mass transfer, multiphase Eulerian case, or a MHD or PEM fuel-cell cases, but not aerodynamics! Let's face it: from users point of view, aerodynamics is the EASYEST set of problems in FLUENT. Of course that I'm aware of the tremendous effort that has been and will be done in the field of turbulence modeling, but strictly from users POV, the aerdynamics has the most straightforward setup of all engineering problems! A combustion case is much more difficult, and to sustain that I only have to say this: how often do we see a post on this forum involving combustion modeling with FLUENT? I will leave the answer to you all.

Concerning your comments:

- You may be right about central coefficient Ap's importance, but running a steady model with 0.075 under-relaxation will probably be prohibitive from engineering POV, and unsteady solver might be a faster answer.

- I really cannot see a clear answer in your second comment, you are just guessing and you didn't convince me. And I never wanted to compare steady laminar solver with LES. I just wanted to underline the fact that steady laminar solver detects instability where steady RANS solver returns a wonderful steady solution.

Maybe I did not make myself clear. It is true that I did not pose a specific question in my original post. I will do that now: to me, analysing these two cases, it seems that laminar solver is much more sensitive to the physics in the turbulent flow then the RANS solver (even when using steady state aproach); is this statement correct, and if so, what is the explanation? Laminar N-S equations do not contain turbulence generating terms. Where does this instability come from? Is there much more to this laminar solver then we are prepared to admit?

If anyone thinks that I should leave CFD and start writing Science-Fiction or poetry, don't be shy, say it to me! But I want arguments. Remember my words: in any scientific field, there must be some art besides mathematics for true beauty to be achieved!

All the best, Razvan
  Reply With Quote

Old   October 3, 2006, 20:19
Default Re: I dare you all...
  #5
zxaar
Guest
 
Posts: n/a
I can see from your response that somehow my post offended you. As I already stated, it never was, or will be my intention. I am glad that you joined the discution, I'm prepared to give you all the credit you deserve.

It has not offended me. My response was just to point out that there is always a possiblity of making mistake. I said so probably because of lot of programming I do. Many times if the code not working properly, if I think that I have been programming for last 4 years so I can not be wrong, most of my code would not work. And problems are sometimes so small to figure out that we go through that portion of code thinking that, its obviously correct (but it is not).

All I wanted was to show that the possibility of divergence in subsonic regime is real even in Fluent.

fluent is a robust solver, but still is a solver. Further to make the solution stable, sometimes sacrifies have to be made in accuracy. It works sometimes, it may fail also.

You may be right about central coefficient Ap's importance, but running a steady model with 0.075 under-relaxation will probably be prohibitive from engineering POV, and unsteady solver might be a faster answer.

You are correct here, i suggested to experiment and see what happens if you do. I further doubted that it owuld work because , fluent say they do not do Ap = Ap/urf.

Another thing that i wanted to point out that the behaviour of fluent for not converging and oscillating around one place is due to the fact that, it uses limiters on gradients (this is the origin of this behaviour). And since gradient play important role in higher order schemes they play big role is what you get as a result.

If anyone thinks that I should leave CFD and start writing Science-Fiction or poetry, don't be shy, say it to me! But I want arguments. Remember my words: in any scientific field, there must be some art besides mathematics for true beauty to be achieved!

Why do you think that its all an arguement, it could very well be a discussion, as i wanted to point you to some points you might not be considering (this is why i wrote, there is always scope for learning). I am sure there are many people here who can add their thoughts and you might not have considered them.

  Reply With Quote

Old   October 20, 2006, 12:44
Default Re: I dare you all...
  #6
Robin
Guest
 
Posts: n/a
Hi Razvan,

I think you have misunderstood what a turbulence model does. The turbulence model does not introduce instability, but rather it stabilizes the solution.

By switching to a Reynolds Averaged Numerical Simulation (RANS) method, the code is no longer solving for the true velocity, but rather it solves for the mean values of velocity and calculates an "effective" viscosity which accounts for the transport effects of turbulence. The effective viscosity is the sum of the Eddy Viscosity and Dynamic Viscosity. The Eddy Viscosity represents the turbulent transport of a quantity due to the motion eddies and in a turbulent flow it is typically several orders of magnitude greater than the dynamic viscosity. A major difference from the dynamic viscosity is that the tubulent viscosity arises from the flow field, as opposed to being a property of the fluid.

In any flow, instabilities arise when the advective transport of momentum is much larger than the diffusive transport of momentum. In other words, when the Reynolds number is large (Reynolds number can be viewed as the ratio of advective to diffusive transport), instabilities can arrise. The increase in effective viscosity due to the Eddy Viscosity therefore increases the "effective" Reynolds number and stabilizes the flow, thus allowing you to acheive a steady-state solution of an inherently transient flow (because turbulence is transient by it's very nature).

If you think this sounds artificial, well, you're right. And the main problem with any turbulence model is how it relates the flow field to this Eddy Viscosity. There are many assumptions involved and terms that are dropped, so a turbulence model is really only appropriate for certain classes of flow.

By the way, your observations on the problems with the steady state solver vs. transient are not new. This is a known problem with segregated solution methods. Many other codes do away with the relaxation factors and actually use the transient term to stabilize the solution. A timestep can then be used to control the amount of relaxation. CFX uses this method, for instance.

Good luck with your studies.

Regards, Robin
  Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On



All times are GMT -4. The time now is 16:46.