CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

bubbleFoam - behavior on finer mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 15, 2011, 03:56
Default bubbleFoam - behavior on finer mesh
  #1
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
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
darai is offline   Reply With Quote

Old   November 15, 2011, 06:05
Default Convergence
  #2
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
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...
darai is offline   Reply With Quote

Old   November 15, 2011, 06:30
Default fvSolution
  #3
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
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.
darai is offline   Reply With Quote

Old   November 15, 2011, 08:28
Default
  #4
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
First of all, did you reduce the maximum time step after refining the mesh?
akidess is offline   Reply With Quote

Old   November 15, 2011, 09:43
Default Time step
  #5
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
Hello Anton,

Thanks for the hint... No, I did not...
I know this:
\Delta t \cdot \sum_{i=1}^{n} \frac{u_{x_{i}}}{\Delta x_{i}}\leq C

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.
darai is offline   Reply With Quote

Old   November 15, 2011, 09:58
Default
  #6
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Delft, Netherlands
Posts: 919
Rep Power: 17
akidess will become famous soon enough
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.
akidess is offline   Reply With Quote

Old   November 15, 2011, 10:27
Default
  #7
Senior Member
 
Aurelien Thinat
Join Date: Jul 2010
Posts: 154
Rep Power: 7
Aurelien Thinat is on a distinguished road
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.
Aurelien Thinat is offline   Reply With Quote

Old   November 16, 2011, 10:05
Default
  #8
New Member
 
Naveed Iqbal
Join Date: Oct 2009
Location: Germany
Posts: 19
Rep Power: 7
niqbal is on a distinguished road
Courant could be set upto 0.5 maximum in Euler-Euler multiphase flows, beyond this value is not recommended
niqbal is offline   Reply With Quote

Old   November 22, 2011, 06:15
Default Final Results
  #9
New Member
 
Martin Holecek
Join Date: Nov 2011
Location: Prague
Posts: 21
Rep Power: 5
darai is on a distinguished road
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.
darai is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
3D Hybrid Mesh Errors DarrenC ANSYS Meshing & Geometry 11 August 5, 2013 06:42
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55
basic of mesh refinement arya CFX 4 June 19, 2007 12:21


All times are GMT -4. The time now is 13:51.