[supermanks]

Hello all,

I have been simulating a room air-conditioning system. Its basically a room with a few surfaces of heat generation, and inlets and outlet for air entry and exit, respectively. I made a mesh in ICEM, consisting of almost 4,00,000 cells. Its basically a tetra(mixed) mesh with a hexacore (for almost 95% of the volume), and I went for this method because the hexa blocking procedure proved to be really tedious, and even though I managed to block the geometry, I ended up with a few negative volumes.

But now, after making the tetra/mixed mesh(with hexacore), I have around 200 cells that are highly skewed, and the mesh has a min. orthogonal quality of about 0.06, again with very few cells. I tried all kinds of smoothing, but couldn't get to improve the quality by much. I still went ahead with the simulation, giving 2000 iterations, with std. k-epsilon model, low relaxation factors- pressure= 0.2, (k, epsilon, momentum)= 0.4 and this is what I got:

(1) Even though I set my residuals' criteria to 1e-04, my continuity remained almost forever around 1e-02. I did some reading here, and found that this might be because of the bad mesh, or because the initial guess was very good, and that the continuity equation arrived at the solution. All my other residuals fell to 1e-03, and 1e-04, and it looked pretty neat, with all gradually sloping downwards, never oscillating or diverging. I know this doesn't mean much, but even my velocity vectors looked fine. So does this mean my solution was reasonable and the bad cells never affected my solution, or did they mess up the whole solution, which is why the continuity never converged?

(2) I set area-averaged temperature over two different surfaces, as monitors. One of them became constant after 500 iterations, and the other, after 1500. So does it make sense that I took these monitors to guide me with deciding about convergence, or are there any other better monitors that I should look towards to know if convergence is reached? And what really should I take to be the convergence point, 500 or 1500?

I'd be really happy if you could take the time to please analyze this situation and help me out with it. Thanks people !

[CFD-fellow]

Hi
Monitoring temperature or velovity points in different parts of your domain will be helpful.
In my opinion you cant trust in your results. Residuals and monitors simultaneously can be good convergency criteria.
Do you have natural convection?
Have you tried double precision solver or SIMPLEC pressure-velocity coupling?
Regards

[supermanks]

Hi Cfd-Fellow,

Yes, I have given two monitors for area-weighted average( on two different surfaces), and one for volume-average of velocity, to see if the temperature and velocity fields are converged. But does this make sense, taking area/volume-averaged value? And are these three monitors sufficient, or should I put different more/different monitors?

And yes, there is natural convection, but that is taken care of automatically in the solver isn't it?

And are you referrring to the double precision that we select before open fluent window? If you are referring to the same, then yes it is enabled in my case. And I haven't tried SIMPLEC, because I never really was that clever on when to use coupled solvers and so on. More of your ideas would be helpful. Thank you.

Regards

[supermanks]

Any more opinions people?

[LuckyTran]

Highly skewed elements can definitely cause a lot of damage. I've been royally screwed over by a single skewed cell. What could be happening is that the cell quality is not poor enough to not cause the solution to immediately diverge. The solution is converging somewhat but to an inaccurate solution.

1) A very good initial guess will cause the continuity residual to not decrease, but not the momentum and other transport properties: energy, turbulence, etc. These other residuals will continue to drop. What you can do to check is reset the residual counter and keep iterating. If the initial guess is perfect, the continuity residual will be stuck at 1 while the others drop to insanely small values.

2) What you're doing with monitors is making sense but try point monitors instead of area/volume monitors. If point monitors are okay I'd say it's fine. For large problems, a few instabilities are hard to detect using global averages. As for 500 vs 1500, more iterations is usually better, but the choice is up to you and your definition of convergence. Ultimately, I think that monitors are hard to argue against as long as you have enough monitors and are monitoring appropriate variables. It's not an excuse though for a mesh dependence study.

[supermanks]

Hi Luckytran,

Thanks for the reply.

(1)I didn't actually get what you meant by "resetting the counters" in your first point. My continuity residual is actually at 1e-02, whereas the others are dropping steadily. I have lowered the Under-relaxation factors considerably. As for the accuracy of the solution, I'm again unsure of it, because I just performed a Steady-state steady flow energy analysis on the control volume, and I calculated an exit air temperature. When I took the average exit temperature from fluent, it almost matched exactly the analytical value. So now, the question is: can the temperature field be solved properly (how it happened here), while the flow field was inaccurate, or is it necessary that the temperature field cannot be accurate without the flow field being solved accurately? Does the correct exit temperature value indicate that my solution is right, or is there something more to be considered here?

(2) I'll try s few point monitors as you suggested. But, here I have a doubt pertaining to meshing in ICEM. Fluent says I have elements that have skewness greater than 0.98, and I do not know which "skewness" factor to check in ICEM mesh quality option. I am using a tet/mixed mesh with a hexacore, and I do not have any idea as to how I can get to decrease the skewness. Any help with regards to this would be greatly appreciated too. Thanks a lot !!

Regards

[LuckyTran]

You can clear the residual history. On the GUI it's under Solution Initialization and click the Reset button. Don't worry the reset clears only the residual and calculation history, it doesn't make your current solution disappear. If you only have text command the text is:
/solve/monitors/residual reset y

Originally Posted by supermanks

So now, the question is: can the temperature field be solved properly (how it happened here), while the flow field was inaccurate, or is it necessary that the temperature field cannot be accurate without the flow field being solved accurately? Does the correct exit temperature value indicate that my solution is right, or is there something more to be considered here?

It is the latter case, the temperature field cannot be accurate without the velocity field being accurate first. That is because the temperature is one of the transported quantities (gets advected around by velocity). The converse is also true, if the velocity field is not accurately solved, then definitely the temperature field is also inaccurate. Extra emphasis on fields and local solutions.

The correct exit temperature does indeed indicate that your solution is correct. It's still possible that the exit average temperature matches the analytical solution while the local temperature distribution does not, in the sense that you can average many different things and get the same result. But you're on the right track.

[supermanks]

Hello LuckyTran,

Thanks a lot for your reply, which is quite comforting because of what you said about the solution being correct as my exit temperature matches the analytical solution.

To summarize what you said, there is a very good chance that my solution is correct now, in spite of highly skewed elements at few places. But there is a chance the local distribution might not be correct, as the quality is bad for some elements.

So probably if I have to eliminate that possibility also, I'm going to have to make a better mesh isn't it?

How can I know for sure if the local temperature distribution is correct or not?

And also, how can I figure out whether the velocity field has been resolved correctly? The same applies to the velocity field too, doesn't it? Thanks a lot for your time !!

(I'm trying to produce a better-quality mesh as we speak, to eliminate all doubt! )

[CFD-fellow]

You can also decrease your mesh skewness with mesh adaption (adapt> gradient) it has options for skewness.

[supermanks]

Thanks CFD-Fellow, I'll try that and get back to you !