Hi, all

I have some problems with the convergence in CFX5.

The problem is about ventialtion of a large atrium with many small inlets and outlets. Ratio between size of inlets heigth compared to Atrium heigth is 1:250. At the inlet the velocity are giving and at the outlets opening is applied. The total number of elements is about 600.000. Upwind in used for advection schemes. RNG-k-eps is used. Buoyancy is applied. In the beginning I use small physical timestep in order to get the solution process going (0.1s). The advection time scale is 5.1. But after 30-50 iteration the solution process suddenly divergence (FINMEM).

I have no idea what could be the problem. Lower the physical time the solution process takes forever.

Could anyone give me an idea of what could be the solution to this problem.

Regards

Soren

Have you tried using local timestep factors? Try 5, as a starter.

Hi,

This has no effect.

The iteration process diverges af 5 steps.

Any new hints.

Regards

Soren

Hi,

Standard k-e or SST turbulence model are more robust in that kind of cases, RNG k-e can be quite unstable. Other thing might be still lower your physical timestep and run 100 iterations with it and then change to bigger physical timestep (depending on inlet velocity and mesh size at inlets), however if it crashed also with local timestep factor, reason is probably turbulence model (I suppose you did not get any meshing warnings, because bad quality mesh can also have an effect to that).

Regards Panu

Hi,

Thanks for the tip.

I will try that tomorrow.

Actually I think that the RNG k-eps should be a quite stable turbulence model.

By I might be wrong.

I did not get any mesh warnings. I once tried to lower the large elements size by 2, but still I had convergence problems.

Regards

Soren

Does the solution always diverge at around iteration 5. If so then try turning "smart start" off (if you haven't already). Smart start often causes divergence at iteration 5 when the turbulence model is added to the iteration loop.

Also how have you calculated the physical timescale. I think CFX uses an average length scale. However you have length scales that vary by 1:250. In such a case I would use the smallest length scale as there may be processes operating at this scale.

Steve

Hi,

No the solution process does not always diverge after 5 iterations.

Most of the time between 30 - 50 iteration is performed before it suddenly diverge.

I have try to lower the physical time step starting from 1, 0.5 0.1, then 0.05.

Length scale: I have a number of inlet which is narrow. 2m in lenght, but only 0.05m in height.

The inlets goes into a large space with the height of 14 m, width: 30 m, depth: 13 m.

There are around 15 surface elements on each inlet.

Regards

Soren

Hi Soren,

For a buoyant flow, try using a timestep roughly equal to the following:

dt = sqrt(L/(Beta*g*delta T)

Where L is a characteristic lenght for your problem, Beta is the thermal expansivity of the fluid, g is the acceleration due to gravity and delta T is the expected temperature range.

Also, if you are running with an ideal gas, consider switching to a general fluid (such as Air at STP) with an appropriate thermal expansivity. This will use the Boussinesque approximation for buoyant forces rather than solving the equation of state (which is much more expensive). For this sort of problem, the difference in the solution will be unnoticable.

Lastly, run it with k-e or zero equation model to start, these will be much more robust.

Regards, Robin

- What is your maximum aspect ratio? Keep it below 200 for the best performance.

- How does your inflation look like?

- Do you observe any unwanted inflow through outlets? If the temperature that you have defined at the outlet differs a lot from the flow temperature that leaves the domain, you might be in trouble.

- Do you observe any unwanted artificial walls on the inlet and or outlet?

Astrid

Hi

I have run some tests today.

I switch to use k-e only. I refined the mesh. But did not use inflation. Aspect ratio is between 8-10. There has been one outlet which could give problems. But it is define as an opening with a specified velocity.

The temperatur range is 290- 303 K. The outlet temperatur is set to 295 K. I already use buoyancy and use general Fluid Air at STP , and modified with the termal coefficient beta.

I have monitor the convergence rate. And it seems to start okay for the for the first 30-35 iterations. It lies in the range 0.95-0.65. But after that the konvergence rate lies close to 1 or between 0.98 and 1.

Regards

Soren

- You definitely need inflation. How does your Yplus values look like. They will be way up in the thousands. Keep them below 300, preferably below 100.

- With these temperature differences, your driving forces are very small, leading to very unsteady behaviour. I think you will never obtain a steady solution. Therefore, consider swithing to transient calculations.

Astrid

Hi Soren,

Firstly, check that your energy balance has been achieved by looking at the values in the outfile when you stop your run. If you are taking small timesteps and have a large domain, it may take a while to get all the energy transferred. Your residuals may flatten out for a while, then eventually resume their descent. If this is not the case, and you are really having problems with convergence, the following may help.

You should find out where the model is having difficulties. You can set the expert parameter "Output EQ Residuals" to true and the solver will write the residual fields to the .res file to post process. These will not be the normalized residuals, so be aware that values can be positive or negative.

The other option is to set your backup interval to 1, and set the expert parameter "Delete Backup Files" to false. Run for ~10 iterations and stop. You will then be able to view these backup files in Post as transients. This will not be a true transient, as you are not converging fully at each timestep, but you will be able to see where changes are occuring.

With this information, you may want to consider increasing the mesh density or improving the mesh in the problem area (if it looks like a mesh problem). As Astrid points out, the problem may be inherently transient, making a transient run more appropriate. Since you said you had good convergence with the fine mesh, I suspect it is not the latter.

Lastly, although I don't encourage this, if the high residuals are restricted to a particular area, and the regions you are interested in are not changing, you can stop your run and use the results as they are.

Regards, Robin

What do the global balances look like? i.e., global mass balance and global energy balance. Maybe a small region of your domain is causing the problem. If so, then you might simply have bad grid in that region, or the problem may be transient (which would suck).

Neale

Hi,

The

Global U-Mom -8.9987E-02 Global Imbalance, in%: -0.0133 %

Global V-Mom Balance: 2.1589E-01 Global Imbalance, in % 0.0320 %

Global W-Mom Balance: -5.7215E-01 Global Imbalance, in : -0.0848 %

Global P-Mass Balance: -6.9828E-02 Global Imbalance, in %: -2.8986 %

Global H-Energy Balance: 1.1524E+04 Global Imbalance, in %: 1.6104 %

What Robin saids about the energy transfer seems okay. Small time step will mean that it takes longer time for the flow to propogate into the domain.

Would it be good idea to have a subdomain around the small inlet with a very fine mesh ???

I will carry out some test today and get back.

Regards

Soren

Hi Soren,

Your global mass imbalance is very large. Typically, this should drop to .001 % fairly easily. Try running with as large a timestep as you can get away with at least until your P-Mass residual drops off. The mass balance may be off because the air coming in has a different density than the air coming out, therefore you are still in a transient phase of the solution.

The mesh resolution around your small inlet should not affect the conserved quantities, but will obviously affect the detailed effect it has.

You mentioned you have a boundary set as an opening. Do you expect air to go both ways through this? If not, set it back to an outlet or outlet and let the code put up walls for a while.

Hi,

Well the opening bc was choosen because CFX suggest this instead of uisng an outlet. I will give this a try with outlet instead.

But I have tried to refine the mesh, by using inflation on a part of the problem. This seems to help on the convergence.

And I am now in the process to applied inflation to the full problem. BUT I now got the following error message, that I have not seen before:

$# Starting surface meshing ... $# Failed to open file $# file = "House_large_mesh_fluid_init.fro" $# IOSTAT = 29 $# unit = 24 $# status = old $# form = formatted $# Error opening file : l:\House_sim_cfx_new\#cfx.355\codan_large_mesh_flu id.fro fo $# r display purposes $# $# An error has occurred during surface meshing. $# ------------------------------------- $# Please refer to the Meshing Messages for possible causes, alternatively, $# verify the surface mesh on individual surfaces to isolate the problem surfaces. $# UNDO: Topology file

Any hints.

Thanks very much in advance. This is really a big help.

Kind regards

Soren

Your mass imbalance is quite high. With proper choice of timestep CFX-5 should have this converged within 10 iterations. The fact that it isn't suggests to me that 1) your timestep may be too small, 2) the solution is in a transient, 3) Inlet turbulence levels not right

As far as a timestep goes, usually 1/5th to 1/3rd typical length over velocity scale is good. With buoyancy however you might also need to limit using a gravity based scale (as suggested by Robin).

Transient solutions can occur for several reasons. You can check your solutions as Robin suggested, by setting backup frequency = 1, and delete backup files = f. Then load the files into CFX-Post. I've seen cases which just don't get a steady state answer because large vortices are being shed from certian parts of the geometry. This could be happening in your case.

As far as the inlet turbulence levels go take a look at turbulent kinetic energy in CFX-Post. Does it die off within a few cells from the inlets? If so, then your inlet turbulence levels may not be high enough. Also look at what the turbulence viscosity is doing as well, or more importantly the viscosity ratio. You may have regions of your domain which are behaving essentially laminar which would result in convergence problems.

Neale

Some additional hints:

- To monitor the totals after every iteration, set the keyword:

MONITOR TOTALS = TRUE

in the expert parameter section.

- If you have imbalances in mass and in energy, that are not the same (as you showed in your list of numbers) but you want them to be the same, consider to run a case with only the energy equation solved. This can also be set in the expert parameter section by the keywords:

SOLVE FLUIDS = FALSE SOLVE k EPS = FALSE

I may have misspeld these keywords.

- I have seen comparable errors when I set SURFACE PROXIMITY on. For some reason this does not work properly. If you have switch it on, switch it off and define some mesh controls in order to obtain a fine mesh where surfaces come close.

Astrid

Astrid

Just to add a tiny correction here: I think the monitor totals parameter is available in the definition file editor, but is now obsolete in CFX-5.5. You can use the solver manager to monitor all flow balances instead.

Neale