# bubbleFoam - behavior on finer mesh

 Register Blogs Members List Search Today's Posts Mark Forums Read

 November 15, 2011, 03:56 bubbleFoam - behavior on finer mesh #1 New Member   Martin Holecek Join Date: Nov 2011 Location: Prague Posts: 21 Rep Power: 5 Hello foamers, I am investigating a case of completely closed domain where a large bubble is rising and spreading across the ceiling. The domain is a cylinder "on side" and the calculation works quite correctly for cruder hexahedral mesh. 3DModel.jpg SmallTank_800.jpg But the target is to use a polyhedral mesh, but the calculation doesn't converge on it... so I tested a finer hexahedral mesh and finer polyhedral mesh and I have got those strange results... Crude Hexahedral mesh Normal-Mesh-400.png Fine Hexahedral mesh Finer-Mesh-400.png Fine Polyhedral mesh PH-T0.04-400.jpg I am quite new to the CFD solving... and I understand that this is not correct. But why? Thanks in advance for all hints you can offer Martin

 November 15, 2011, 06:05 Convergence #2 New Member   Martin Holecek Join Date: Nov 2011 Location: Prague Posts: 21 Rep Power: 5 So, in the first step I examined the convergence and it is as those attached graphs shows. The most correct calculation, with the crude hexahedral mesh looks like this: (convergence of p in individual time steps) Screenshot-HexCrude.png The finer hexahedral mesh then looks like this Screenshot-HexFiner.png And the finer polyhedral mesh like this Screenshot-PH.png So the convergence is poor in the beginning in all the calculations... And it is similar in Hex Crude and Hex Finer mesh... I assume that the bad convergence in the polyhedral model is in the moment the model touches the wall...

 November 15, 2011, 06:30 fvSolution #3 New Member   Martin Holecek Join Date: Nov 2011 Location: Prague Posts: 21 Rep Power: 5 Hello all, In the next step, I am going to try to change the fvScheme file... but I have no clue which is good to modify first... I do know what the lines in fvScheme stand's for and I do know how each scheme looks, but I am not sure how to guess the influence on the result. Is there any hint? What to start with, which literature read, some similar cases etc? Thanks again for any help or hint... Martin.

 November 15, 2011, 08:28 #4 Senior Member     Anton Kidess Join Date: May 2009 Location: Delft, Netherlands Posts: 921 Rep Power: 17 First of all, did you reduce the maximum time step after refining the mesh?

 November 15, 2011, 09:43 Time step #5 New Member   Martin Holecek Join Date: Nov 2011 Location: Prague Posts: 21 Rep Power: 5 Hello Anton, Thanks for the hint... No, I did not... I know this: The original model (crude) was: dx = 0.01 m max dt = 0.001 s The ux is 0 in the beginning of the calculation and maximally 10 m/s (because the bubble toutches the top after cca 0.5s) so let's take 10 m/s the C is max 1. When I am using the finer model (both are 2x finer in each direction) the cell size is decreased to: dx = 0.005 m all other parameters weren't changed: max dt = 0.001 s max ux =~ 10 m/s so let's say C is max 2. Ok, so I suppose that the time step should be halved... For this I introduced the calculated time step... the same which is in twophaseEulerFoam... or in interFoam. Is it necesarry to set the maxDeltaT always to some calculated value by the equation above? What if I can't limit the velocity? I am suppose to calculate quite large models and too small dT will increase the calculation time... I thought that the calculated dT (calculated in the run in each time step accordingly to actual Courant number) will solve this problem but not if I will force it manually to use some small value. I will test smaller dT ... for example 1/10 dT should be sufficient and post the results. Thanks again, Martin.

 November 15, 2011, 09:58 #6 Senior Member     Anton Kidess Join Date: May 2009 Location: Delft, Netherlands Posts: 921 Rep Power: 17 I think a Courant number of 1 is already pretty large for multiphase flows; 2 is just asking for trouble. Definitely check if your results change with smaller time steps. MaxDeltaT is not always necessary, but more strictly enforced than maxCo, so if you notice the solver jumping over the maxCo number it helps to limit maxDeltaT as well.

 November 15, 2011, 10:27 #7 Senior Member   Aurelien Thinat Join Date: Jul 2010 Posts: 154 Rep Power: 7 I agree with Anton. An Euler/Euler multiphase flow calculation needs a small courant number. In my different tests, I used to bound the Courant number (based on Ur) by 0,4.

 November 16, 2011, 10:05 #8 New Member   Naveed Iqbal Join Date: Oct 2009 Location: Germany Posts: 19 Rep Power: 7 Courant could be set upto 0.5 maximum in Euler-Euler multiphase flows, beyond this value is not recommended

 November 22, 2011, 06:15 Final Results #9 New Member   Martin Holecek Join Date: Nov 2011 Location: Prague Posts: 21 Rep Power: 5 Hello All, Thanks again for the recommendations. You were right... the Time step has quite influence on the convergence / divergence of the whole model. I tried the "adjustTimeStep" switch (added to bubbleFoam) to correct this problem, but the calculation turned out to be still dependent on the time step. To save the calculation time, I examined following rhetorical question: Why do we have the calculated Courant Number for each time step when we need to limit the deltaT anyway? If I force the calculation to push the Courant number (with maxCo constant) down do I still need the maxDeltaT? What if the problems with divergence are only in the beginning of the calculation cycle before the timeStep is pushed down by the MaxCo criteria? In this case, it would be enough to set maxCo (0.4) and Calculate sufficient deltaT for T=0... and let the maxDeltaT to be higher... because the limitation by maxCo should be enough. For now I have some results on finer mesh (T = 0.5 s ) (120 000 polyhedral cells)... fixed dT = 0.1 ms, maxCo = 0.4 PH-F-Fixed_dT-Graph.png PH-F-Fixed_dT-Pic.jpg variable dT = 0.5 ms,dT(T=0) = 0.1 ms, maxCo = 0.4 PH-F-Variable_dT-Graph.png PH-F-Variable_dT-Pic.jpg As it looks, the results are similar, so the convergence problem was in the first part of the calculation... BUT the results does differ quite a bit, and the residua (thick green results in graph) are quite worse for the variable dT. The scary thing is the yellow value of the Courant number... even the parameter maxCo is 0.4 the calculated maxCo is in one moment little bit over 4. So, the problem isn't fully solved. When the calculation reaches a problematic place it fails (if the time step is fixed) or it creates unrealistic results, if the time step is variable. But the first question, the divergence at the beginning is now solved. I will create necessary graphs and submit the other problematic place in the calculation. Thanks again Anton, Aurelien and Naveed a lot for the hints... fluid dynamics are now again a little bit clearer for me. Martin.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42 tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24 aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52 SSL FLUENT 2 January 26, 2008 12:55 arya CFX 4 June 19, 2007 12:21

All times are GMT -4. The time now is 14:11.