[chrisf90]

Hi everybody,

I know there are several posts on convergence problems in this forum and I checked a great number of them but nothing helped me solving my problems.

My issue is that the residuals (especially those of continuity and x velocity) have a short diverging trend and then "stuck" on a level. I have attached a figure of it. In the image it might look like that they would come down again, but they won't. I have ran a lot of simulations for much more iterations and they stay at this level.
However heat transfer and mass balance is achieved after certain iterations. Also monitored quantities of interest (surface temp., mass flow rates, velocity) seem to be flat after some iterations.

brief overview of my setup:
I try to predict air flow and heat transfer through a Double Scin Facade (DSF). Air flow occurs through the increase of temperature inside the cavity because incident solar radiation.
1) Geometry and B.C. (overview) see attachment
2) k-e RNG turbulence modell
3) boussinesq approximation for the solar chimney effect
4) DO modell with 2 bands (solar and thermal radiation)
5) pressure based solver in double presicion
6) SIMPLE algorithm
7) Discretization: PRESTO for pressure; 2nd order for all others
8) Tolerances of Residuals: E-6 for energy, DO; E-4 for all others

What I have tried so far for solving the issue:
1) changed the Settings of the DO model
2) applied the gravity in steps (9.81e-3, 9.81e-2 ...)
3) modeled the density of air with "incompressible ideal gas"
4) played with URF
5) switched to k-epsilon Realizable
6) changed settings of turbulence model
7) and last but not least changed the mesh literally 100 times
(2 images of my last Mesh version are attached)

I think the problem occurs from my mesh, because in an earlier stage I have modeled the solar shading in a simplified way (just vertical lines with thikness). And therefor I didn't have any troubles with running to convergence with this solver setup.

As I am still quite new to Fluent and CFD I am not really sure if the mesh is appropriate for my problem and also if the quality of it is good enough.
max skewness 0.71 (average 5.5e-2)
min orth. quality 0.41 (average 0.97)
max aspect ratio 36.7 (average 2.2)

I would really appreciate some advices on my issue.
Am I right with my thoughts that the mesh is due for convergence issue?
Or may there also be another problem with my setup?

Thanks in advance!
Chris

[mrswordf1sh]

Did you check your y+ value?

And why do you think that it's not converged? X velocity and continuity seem to reach 10^-3, and other's seem to have something smaller than 10^-5. That's already good enough.

About meshing, your quality results are awsome. I have simulated a wind turbine blade having 0.9 skewness value and still results were close to experimental ones.

Is there some similar experimental case from which you can obtain experimental results? You can use it for validation.

[chrisf90]

Thank you for your reply.

For this particular case I did not check y+ so far. But I worked with same first cell heights (0.5mm) as in earlier models and the velocities are comparable. So I think y+ will be in the region of 1.

I am worried about the diverging trend. I know that in natural convection problems residuals won't drop that much because of the low velocities and it may be that they stuck at a certain level. But as I said I am worried about the diverging trend? Because many users say that diverging trends are caused by bad meshing or inappropriate B.C. setup.
Also in similar studies they reach lower values of residuals which makes me doubt on my solution.
But of course I know residuals are not the only thing for judging convergence.

Yes, there are some similar studies as I mentioned above also ones which includes experimental studies. I will adapt my B.C. to those of the similar studies and see if the solutions will fit together.

Regards
Chris

[flotus1]

From the residuals in your figures I do not see a diverging trend. I would run the simulation for 2 or 3 times more iterations and see what happens.
What usually helps with natural convection setups that refuse to converge is switching to a transient simulation.

[chrisf90]

Thank you for your advice Alex.

I will keep the simulation run for another few thousand iterations. I would be thankful if you could take another look on it then.

I also will try it with the transient solver.

[chrisf90]

Hi guys,

Sorry that it tooks me a while for calculating but I simple haven't got the computing power at home

I kept the simulation running for about 13k iterations and after that it looked like the attached figure:
-The "oscillating" behaviour might be another indicator for switching to transient solver, right?
-Mass flow balance is achieved. Heat transfer balance is not achieved yet, but the Error is at about 7% and I think it would further decrease by calculating for another few iterations
-Monitored quantities: surface temperatures are flat but mass flow rate and velocities are also not perfect stable. They are oscillating with an error of about 1%.
-What do you think about it? I'm pretty worried about it to announce it as converged solution.

I also tried to setup a transient solution. But I think what I have done was a complete mess (see attachment).
I think the problem was in the choice of timestep. In the figure I have chosen 1 sec and I think it was too big, as I think all residuals have to drop about 3 orders of magnitude, right?
But when I have chosen smaller time steps (e.g. 0.01) the Residual patterns had looked better but the flow has not developed?

I found a formula for optimal time step size for natural convection problems in an old tutorial, but I have got problems with a variable:
t = L / (g*beta*detaT*L)^(1/2)
t... time step size
g ... gravity
detaT ... temperature difference
L... characteristic length
beta ... I'm not sure if this is the thermal expansion coefficient or what else? Can you help me with that or do you have another advice for the choise of timestep?

Sorry for my questions but this is the first time I'm working with transient solver.

Thank you in advance.

Regards
Chris