Dear CFD users,

I am dealing with simulating a bouyancy-driven flow in a room with Fluent.

When I set up the case and lauch the simulations, the residuals drop down of two orders of magnitude in the space of one-two hundreds of iterations, depending on the boundary conditions I impose. After that, residuals stop to drop down and begin to fluctuate slightly, without increasing or decreasing any more.

Changing the under-relaxation factors for pressure, energy and/or turbulence variables makes the residuals drop down some few iterations, but after that they begin again to fluctuate around another value.

At the same time, I monitor the value of some variables I am interested to, and they oscillate very slightly too. To give an idea, a volume flow rate at a surface of interest have fluctuations of 0.1% around its absolute value.

My question is: can I consider converged the solution, even though residuals have drop down only of two orders? If yes, is it normal that residuals and solutions fluctuates slightly when reached convergence? Could this mean that a steady-state solution does not exist?

Thank you in advance.

Best regards,

Marcello Caciolo phD student CEP - Center for Energy and Processes of Ecole de Mines de Paris

Hi,

I think you have 2 options here. It seems you will not get steady state but I think that if you average over enough iterations you will have a decent solution given that your residuals have dropped sufficiently and that your oscillations are very small. If you run for long enough you will see the solution oscillating with a certain period and average over that. You can also run it a transient simulation but you must be careful selecting time-steps and I would not say you need a time accurate solution.

I maybe wrong so see what others say. Tom

I have had similar experience with these flows at larger Rayleigh numbers using my own code. This leveling off of the residual can be reduced by going to even more under-relaxation. If the relaxation parameter is small enough, there is no leveling of the residual down to the level of numerical roundoff, but who is to say that it still would not level off with higher numerical precision.

Probably your solution is not changing much (to engineering accuracy) as you increase under-relaxation, and you can accept the remaining residual.

Though it is a stretch to accept this analogy, there is the case of evaluation of asymptotic series. As you add terms to the partial sums, the error gets smaller, up to a point where the error increases and the series diverges. The accepted procedure is to sum until the error stops decreasing and stop summation there. That is the best you can get out of this series.

try increasing the mesh density

Nah, try decreasing mesh density. It's likely that you're resolving transient flow features (big wobbly plumes). A good old bit of numerical diffusion will help to settle things down

My experience with my code: this behavior is largely independent of mesh density.

not mine

Jonas Holdman wrote "this behavior is largely independent of mesh density." (I guess you refer to the stationary oscillations of the residuals).

The left hand side of the Navier's Stokes equation is hyperbolic in nature, that means the advection of scalar and vectorial quantities is carried out by wave like phenomenun. Translate that to the computational grid, and a discrete perturbation analysis will show you the effect of the so called "cell Peclet Number". Good Luck

Jonas, sorry I did not have this reference at hand, when I wrote my previous comment, Computational Fluid Dynamics For Engineers by Klaus A Hoffmann has some nice figures showing the nature of error.

if you stick a radiator in a middle of a room and pour some smoke to visualize air movement from buoyancy, you are not going to see some sort of a nice steady-state hot air rising, you will see a blob of warm stuff accumulating over the thing and then puff, it goes up, and then the deal repeats itself, in other words, there is no steady-state and most of the time buoyancy stuff is transient. Now, all commercial codes are full of diffusion and won't just blow up, they will converge a bit and then keep oscillating and that's what you are seeing in the residuals. So, take them and be happy, just like Jonas suggested. And, btw why would you add more diffusion with coarser mesh, to get as far as possible from an already remotely correct solution and dispersion has nothing to do with buoyancy driven stuff either....

how many grid sytem did you use and laminar flow or tubulent flow

"you will see a blob of warm stuff accumulating over the thing and then puff"

Are u sure about this? I know the buoyant plume is transient, i.e. it will meander/wobble like people say, but what you are suggesting is different to that. You seem to be saying that the plume stops and starts, which I don't think could be physical. Unless you have seen the plume to loop right around before rising?

Maybe if you could point me to the appropriate literature that proves this.

[wc34071209]

I am sorry to dig this thread out, but I am wondering if there is any progress for commercial codes such as ANSYS Fluent to solve buoyancy flows. I could not even converge a simple validation case.

[arjun]

Originally Posted by wc34071209

I am sorry to dig this thread out, but I am wondering if there is any progress for commercial codes such as ANSYS Fluent to solve buoyancy flows. I could not even converge a simple validation case.

If you are in fluent you can try body force weighted scheme. These problems remain tough. You can solve them by increasing coupling between velocity and pressure.

In my solver Wildkatze you can use a scaling factor for pressure velocity dissipation more than 1 and hence can increase stability and convergence of body force based calculations.

[wc34071209]

Hi Arjun,

Thank you for your kind reply. The body-force-weighted and PRESTO! are the recommended scheme by Fluent to solve buoyancy driven flow.

I tried both and they do show slightly better performance but convergence is still a problem.

Do you have experience in other codes such as OpenFOAM. I have a feeling (maybe I am wrong) that OpenFOAM is easier to solve buoyancy driven flows than Fluent.

Originally Posted by arjun

If you are in fluent you can try body force weighted scheme. These problems remain tough. You can solve them by increasing coupling between velocity and pressure.

In my solver Wildkatze you can use a scaling factor for pressure velocity dissipation more than 1 and hence can increase stability and convergence of body force based calculations.

[arjun]

Originally Posted by wc34071209

Hi Arjun,

Thank you for your kind reply. The body-force-weighted and PRESTO! are the recommended scheme by Fluent to solve buoyancy driven flow.

I tried both and they do show slightly better performance but convergence is still a problem.

Do you have experience in other codes such as OpenFOAM. I have a feeling (maybe I am wrong) that OpenFOAM is easier to solve buoyancy driven flows than Fluent.

I do not think that it will be easier to solve with openFOAM, if these forums to be believed openfoam is not as stable as fluent.

I am not sure what will help you here, but once a bouyoncy driven case that was not converging for a month, converged well when we refined mesh. (It was with fluent with version 6.3). So you might try grid refinement, it may or it may not help.

I believe (not verified) that instead of using implicit under relaxation for momentum one might need to use explicit under relaxation and that might help.
But that is my guess and not been verified even once.

[wc34071209]

It is an excellent idea to try an explicit under-relaxation for momentum. I will give a try and let you know. But could you please explain a little why it would help?

Have you even used the coupled solver with pseudo transient in Fluent? Some people say that it might help converge buoyancy flows.

Many thanks!

Originally Posted by arjun

I do not think that it will be easier to solve with openFOAM, if these forums to be believed openfoam is not as stable as fluent.

I am not sure what will help you here, but once a bouyoncy driven case that was not converging for a month, converged well when we refined mesh. (It was with fluent with version 6.3). So you might try grid refinement, it may or it may not help.

I believe (not verified) that instead of using implicit under relaxation for momentum one might need to use explicit under relaxation and that might help.
But that is my guess and not been verified even once.

[arjun]

Originally Posted by wc34071209

It is an excellent idea to try an explicit under-relaxation for momentum. I will give a try and let you know. But could you please explain a little why it would help?

Have you even used the coupled solver with pseudo transient in Fluent? Some people say that it might help converge buoyancy flows.

Many thanks!

The reason behind this thinking is that even though the implicit urf is derived from formula of explicit urf (Patankar, derived in Prof. Peric's book) , the end result is not the same correction.

To explain this, because Patankar derived implicit urf formula using explicit form people think that in the end they provide same correction but it is not true because the derivation assumes that the system (Ax=b) is solved to machine precision.
Which does not happen as the solvers (fluent for example) reduces the error by only say 10 times.

So every iteration the correction that you add to solution is far off from the correction you would be adding if you used explicit urf. This is why I believe that explicit urf method though more unstable shall be fast converging here.