[cardioCFD]

Hi

I am simulating a advection-diffusion-reaction system where the permeabilty of a sub-domain in my flow domian reduces with concentration of some species.
BCs are not varying with time.

I have run the model in steady state mode with 4 monitor points inside the reactive sub-domain. The concentration of species increased to a constant level after ~500 iterations and will continue to be constant for 3000 iterations, then there is a slight depletion to the soichiometric concentrations after 10000 iterations. This happens because some species will trap in the sub-domain as permeabilty is decreasing and then the problem becomes a diffusion dominant one with a very slow convergence rate where species diffuse out of the porous subdomain to reach final steady state of stoichiometric level.

So when running the model as steady state, the problem is a two part one. In the first 500 iteration I have acceptable convergence rate up to the point that the subdomain becomes fully porous (filled) and then problems becomes a diffusion dominant and will take for ever to reach the convergence criteria.

I have discussed this with a senior member of our team and he suggested to use Peclet number to interupt the simulation at the point when the subdomain is filled and problems become diffusion dominant.

Note that, I do not want to use aggresively large timescales to reach steady state, because I am not really interested in the final steady state. I would like to see how much species are traped inside the subdomain (under the effect of advection) when the subdomain is filled, and if I continue the simulation to the end then all of these species will be slowly washed out with diffusion and every thing reaches the stoichiometric concentration.

Actually, there is a missing component in my model, which is solidification that is not available in CFX. In reallity, everything is finished when the subdomain is filled because it turns to solid. However I have modelled this with decreasing permeability! Thats why I want to interupt simulation after the subdomain is filled and fully porous, and thats why my colleague suggested using peclet number to interrupt simulation.

I used Peclet number and that seems to be fine as it interrupts the simulation perfectly.

Then I did a new test for myself, I ran the system in the transient mode with Peclet number again as interruption condition with the hope to get same results. But I did not get the same results. Because at every timestep, CFX iterates to reach convergence. It means that at every time step a tiny part of the subdomain will be filled with the porous material and it will iterate to the point of stoichiometric concentrations (diffusive wash out of a gradually filling subdmain).

So it seems that transient simulation does not work for this system and RMS is also not a good candidate to judge convergence in the steady state in my problem. I need to run it as steady with the subdomain peclect number as interruption criteria and montoring concentration to reach constant level.

That was the story I just was wondering if any of you also have any comments to add.
Thanks a lot

[ghorrocks]

So it seems that transient simulation does not work for this system

That means you are missing some important physics in the transient simulation. But you appear to be saying that if you use a steady state simulation then the time history (as modelled with steady state pseudo time presumably) is a better match for the expected results. Is this correct? If so this is concerning as steady state simulations do not guarantee time accurate simulations, several simplifications have been made to make convergence easier at the cost of inaccurate time history. The only thing which matters in a steady state simulation is the final converged result.

RMS is also not a good candidate to judge convergence in the steady state in my problem

Yes, that can happen. You might be sensitive to the small regions of high residual which RMS tends to average out. That is why the MAX option is there, to handle these cases.

[cardioCFD]

In a nutshell, I have tried a SS solution to my problem and achieved convergence (max RMS < 5e-4) after ~14K iterations, increasing timescale by a factor of 1000 after iteration number 10K.

Monitoring concentrations at some points, I realised that they monotonically increase and reach a SS after ~500 iterations, then they start to slightly decrease after iteration 5-6K to reach a new SS at iteration 14 K. The convergence criteria of max RMS < 0.0005 just reached after 14 K although my monitor points were flat at the first SS.

I am actually interested in the first SS (the one after 500 iterations), so I used a stop criteria (Peclet<some threshold) and stopped it. Note that flow is already reached convergence at the iteration 500.

I tried to solve the problem in the transient mode, to see if I can replicate this behaviour, again I used Peclet as the stop criteria, but this time I got completely different results, more similar to the final SS (the one after 14K iterations) of the SS solution!

I am a bit confused about this difference. Does it mean that my SS solution (the one at iteration 500) is wrong?

I would appreciate any comment on this. Thank you.

[cardioCFD]

Originally Posted by ghorrocks

That means you are missing some important physics in the transient simulation. But you appear to be saying that if you use a steady state simulation then the time history (as modelled with steady state pseudo time presumably) is a better match for the expected results. Is this correct? If so this is concerning as steady state simulations do not guarantee time accurate simulations, several simplifications have been made to make convergence easier at the cost of inaccurate time history. The only thing which matters in a steady state simulation is the final converged result.



Yes, that can happen. You might be sensitive to the small regions of high residual which RMS tends to average out. That is why the MAX option is there, to handle these cases.

Hi Glenn,

Thanks a lot. My system seems to have 2 steady states. I monitored the concentrations at some monitor points, and I reach a flat curve after 500 iterations and they stay at the same level for almost 5-6K more iterations, then they start slight depletion to a new SS, where the max RMS criteria will be met (after 14K iterations)

I am actually interested in the first SS, but I am a bit concerned about the max RMS not being reached although the monitor points concentration curves are flat.

I tried to switch to transient and to ensure that I get a converged solution at every timestep, but I got completely different results more similar to the final SS after 14 K after simulating my system for 70 sec and non of the transient solutions at smaller times are similar to the first SS.

[ghorrocks]

My system seems to have 2 steady states.

What you have described does not sound like 2 steady states. Rather, it sounds like you have a simulation with two time scales and the first time scale converges in about 500 iterations and the second time scale converges in about 14k iterations. Many complex simulations have multiple time scales so this is not unusual.

Often when convergence initial proceeds well, then levels off then starts converging again and goes to convergence; this is the sign of something from the inlet making its way to the outlet. It could be when the flow from the inlet finally reaches the outlet, or it could be that the heat from one side of a block finally reaches the other side.

Do not be fooled into thinking that the leveling off of the convergence at 500 iterations is the sign of anything meaningful. It is still just an unconverged simulation and should not be used for anything until your convergence criteria is achieved for ALL variables.

The normal way of dealing with large differences in time scales like this in a steady state simulation is to advance the different equations at different rates. For instance in fluid flow + solid heat transfer simulations usually the fluid domain converges quickly but the heat in the solid transfer is much slower. To help in these cases we use "Solid Timescale Factor" which is an acceleration factor for the heat equation. It can greatly accelerate convergence in the solid domain.

You need to work out which equation is converging fast and which is slow, and accelerate the slow one.

A final point: if you are interested in the transient response, then you need to run a transient simulation. You cannot use any acceleration then, you just have to run it until all the transients you wish to resolve (both the fast and slow ones) are completed.

[cardioCFD]

Thanks a lot Glenn, I will work on that and update this post.