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

VOF interface

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 26, 2005, 09:38
Default I'm just starting to use the O
  #1
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
I'm just starting to use the OpenFOAM. I'm interested in VOF methods for ship hydrodynamics simulations. I had previously used other CFD tools when I worked at University.
The first test I'm making is a very simple undisturbed free surface 2D case. An uniform velocity field enters from the left and, after having crossed the domain, leaves the domain through an outlet boundary condition. I'm using the rasInterFoam, as I'm interested in getting a model more and more sophisticated (the complete simulation will require a 3D full rigid body dynamics for a boat... I would like to make roll damping calculations and performance analyses).

But I must confess I hadn't obtained good results even for this simple problem. The problem is well initialised and starts well. But after about 2.6 seconds the free surface is distorted (I was expecting a trivial solution of steady undisturbed free surface). The link to a picture of gamma is the following:
http://www.lem3.it/tests/gamma_2.57102.png

The process becomes unstable some time after, as can be seen in the following picture:
http://www.lem3.it/tests/gamma_3.15095.png

The time step is limited by a Courant number of 0.2, the fields are initialised accordingly with the boundary conditions...

I was considering what I was missing... Thanks in advance.
Michele.
michele is offline   Reply With Quote

Old   May 26, 2005, 13:36
Default The second picture looks like
  #2
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
The second picture looks like a problem of a wave trying to reflect back from an inlet boundary...

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 26, 2005, 16:05
Default What are your left and right b
  #3
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
What are your left and right boundary conditions on gamma? They should be fixed value on the left and zeroGradient on the outlet.

I assume in terms of numerics you used all the default settings from the rasInterFoam test case? Try running it with both
div(phi,U) Gauss upwind;
div(rho*phi,U) Gauss upwind;
in your fvSchemes dictionary. If this doesn't solve your problem (and even if it does), it is more than likely an issue with the step change between the air and liquid at the inlet.

Could you please pack up the case and post it to this forum? I would like to take a look at it some time.
eugene is offline   Reply With Quote

Old   May 27, 2005, 03:33
Default Thanks for your kind replies.
  #4
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
Thanks for your kind replies. I think I imposed correctly the boundary conditions. The numerical scheme used for the momentum equation is upwind (at the first trials I realised that the gamma schemes where more unstable).
Herebelow, as Eugene requested to me, I attach the whole case.

By he way, its name, "waves", is misleading... it is a simple steady case (when the current issues will be solved, I will implement a time/space varying inlet boundary condition accordingly with potential wave theory).
I'm however still having problems with the case attached... any suggestions?

Thanks,
Michele.
michele is offline   Reply With Quote

Old   May 27, 2005, 03:39
Default Thanks for your kind replies.
  #5
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
Thanks for your kind replies. I think I imposed correctly the boundary conditions. The numerical scheme used for the momentum equation is upwind (at the first trials I realised that the gamma schemes where more unstable).
Herebelow, as Eugene requested to me, is a link to the case (it's too big to be posted to this forum):
www.lem3.it/tests/waves.tar.gz

By he way, its name, "waves", is misleading... it is a simple steady case (when the current issues will be solved, I will implement a time/space varying inlet boundary condition accordingly with potential wave theory).
I'm however still having problems with the case attached... any suggestions?

Thanks,
Michele.
michele is offline   Reply With Quote

Old   May 27, 2005, 06:33
Default It might be worth running with
  #6
New Member
 
Chris Greenshields
Join Date: Mar 2009
Posts: 28
Rep Power: 8
chris is on a distinguished road
It might be worth running with interFoam (rather than rasInterFoam) with upwind on the momentum equation. See if you hit the same problem.
chris is offline   Reply With Quote

Old   May 27, 2005, 09:44
Default I tried running the case even
  #7
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
I tried running the case even with interFoam (with upwind discretisation for the momentum equations), but I experienced the same issues, i.e.
1. during the first part of the simulation the free surface continues going down (instead of keeping the original height)
2. after this starting phase, instabilities near the inlet boundary are observable

Michele.
michele is offline   Reply With Quote

Old   May 27, 2005, 09:53
Default The conservation problem you h
  #8
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
The conservation problem you have sounds like your mesh is incorrect, have you tried running checkMesh on it? Have you tried simpler meshes?
henry is offline   Reply With Quote

Old   May 27, 2005, 10:01
Default Hello Michele, I've got an
  #9
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
Hello Michele,

I've got an idea for you, but before I can think of a fix, I need you to try something out for me. Could you please repeat the same run but set the gravity vector to zero:

constant/environmentalProperties

g g [0 1 -2 0 0 0 0] (0 0 0);

Now you should get a perfect undisturbed surface, right? If not, something else is badly wrong, but if you do, the problem will be easier to solve.

Please let me know,

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   May 27, 2005, 10:32
Default Check the number of faces of t
  #10
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
Check the number of faces of the front and back "empty" patches, these should be equal to the number of cells otherwise the case is not 2D. Are you sure the mesh is 1-cell thick everywhere and is properly connected? How did you generate the mesh?
henry is offline   Reply With Quote

Old   May 30, 2005, 07:03
Default > The checkMesh tool suggests
  #11
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
> The checkMesh tool suggests using zipUpMesh, but nothing happens

Are you sure nothing happens? Doesn't it write out the corrected mesh? If you run it a second time what does it tell you? If you run checkMesh after running zipUpMesh do you still get errors/warnings?

> Another strange issue: the mesh non-orthogonality should be zero

Does your mesh contain refined regions? If so the mesh will not be perfectly orthogonal.
henry is offline   Reply With Quote

Old   May 30, 2005, 08:46
Default Thank you, Henry. Yes, indeed
  #12
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
Thank you, Henry.
Yes, indeed the mesh contains refined regions.
So I assume that the non-orthogonality and skewness parameters are non zero due to the refined faces. That's OK.

Indeed, if I run the zipUpMesh tool twice, it always outputs the following message:

-------------------------------------------------------------------------------
/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

Exec : zipUpMesh . waves
Date : May 30 2005
Time : 14:34:03
Host : binah
PID : 6479
Root : /home/michele/OpenFOAM/michele-1.1/run/simulations/rasInterFoam
Case : waves
Nprocs : 1
Create time

Reading polyMesh
Cycle 1 changed 3600 faces.
Cycle 2 changed 0 faces.
-------------------------------------------------------------------------------

No one of the files into the polyMesh directory is modified (I verified to have write access to these files). There is the
polyMesh/sets/zipUpCells
file, generated during the checkMesh execution.
I don't understand what is going wrong with this mesh.

Michele
michele is offline   Reply With Quote

Old   May 30, 2005, 08:53
Default I am not sure why zipUpMesh do
  #13
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
I am not sure why zipUpMesh doesn't write a new mesh, we will investigate. However the test checkMesh fails on and requests running zipUpMesh is only important is you want to run finite-elements on the mesh, i.e. mesh-motion, because it relates to edge connectivity which is only used for that purpose.
henry is offline   Reply With Quote

Old   May 31, 2005, 08:48
Default I haven't had a chance to look
  #14
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
I haven't had a chance to look at this case yet. Has anything changed since last week?
eugene is offline   Reply With Quote

Old   June 1, 2005, 04:38
Default Dear Henry, thanks for the sup
  #15
Member
 
Rattin Michele
Join Date: Mar 2009
Posts: 36
Blog Entries: 1
Rep Power: 8
michele is on a distinguished road
Dear Henry, thanks for the support.
I've just uploaded on my webspace the whole test case (www.lem3.it/tests/waves_050601/waves.tar.gz). Note that in the constant/polyMesh/star_mesh directory reside the exported star mesh (the simple mesh is "star" and the mesh containing embedded regions is "star2").

I however assume that for this simulation the mesh "star2" (the one that fails the checkMesh tests) is correct.
Regarding the rasInterfoam simulation made with this mesh, the following observations came out:

1. The visualiser shows skewed elements in the refinement interface region (as it can be seen two refinements were applied)
(see fig: http://www.lem3.it/tests/waves_05060...30s/1_mesh.png)
The mesh instead is made of hexaedra with split faces on refinement. (Is it due to this the fact that checkMesh reveals skewed elements?)
Is it a problem of starToFoam conversion or only of visualisation? I think the latter, as I manually verified the vertex positions (into the imported vertices files) and they seemed to be correct.

2. One small issue: the runFoamX applications, when saving the simulation files, forgets adding the
div((nuEff*dev(grad(U).T()))) divScheme in the fvSchemes dictionary... only a little bug.


Regarting the simulations results, at time 30s, I have to make the following observations:

a. Gamma shows a wavy pattern (see fig: http://www.lem3.it/tests/waves_05060...0s/2_gamma.png).
I think that this type of instability has no hydrodynamic sense. What's happening?

b. Turbulence grows when the wavy instability starts as a coupled effect (see fig: http://www.lem3.it/tests/waves_050601/res_30s/3_k.png and http://www.lem3.it/tests/waves_05060.../4_epsilon.png).

c. pressure shows some spikes (of large magnitude, up to pd= 426Pa/density, i.e. the pressure goes up to 4.26 bar see fig: http://www.lem3.it/tests/waves_050601/res_30s/5_pd.png)

d. The graphs of velocity also show these kind of instabilities. (see Ux in fig: http://www.lem3.it/tests/waves_050601/res_30s/6_Ux.png and Uy in fig: http://www.lem3.it/tests/waves_050601/res_30s/7_Uy.png).

The fvSchemes employed in this simulation are of high order. No numerical instability problems arose.

I will appreciate any comment.
Yours sincerely,
Michele.
michele is offline   Reply With Quote

Old   June 1, 2005, 05:43
Default Hi Michele, we found a bug
  #16
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Hi Michele,

we found a bug in the writing of zipUpMesh. It does do its work but doesn't write the new mesh!

Attached a version of zipUpMesh which does. I have however no files to test it with so let me know if it actually helps.

Compile as usual:
- unpack
- wclean
- wmake

zipUpMesh.tgz
mattijs is offline   Reply With Quote

Old   June 1, 2005, 05:43
Default 1) The split-hex cells are de
  #17
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
1) The split-hex cells are decomposed into pyramids for ParaView because it cannot directly handle cells "higher" than hex.

2) Yes this is an omission in the FoamX configuration files which is easy to fix.

Have you tried:

making the walls slip?
lower-order schemes?
or any other schemes?
compression coefficient of 1?
henry is offline   Reply With Quote

Old   June 1, 2005, 06:28
Default I also notice you have a relat
  #18
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
I also notice you have a relative tolerance set for pd, I think this is unwise although it what is set for the tutorial case. For the next release I will reset and test all the settings for tutorial cases of all the interFoam-based codes. I suggest you try:

Setting relative tolerance on pd to 0

cGamma to 1

the coefficient on the Gamma201 to 1 on both terms

nNonOrthogonalCorrectors to 0
henry is offline   Reply With Quote

Old   June 1, 2005, 06:29
Default I had a quick look at this cas
  #19
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
I had a quick look at this case.

Neither upwind, setting cGamma=0, changing surface tension to zero nor any combination of these factors changes the occurrance of the initial perturbation near the inlet (lower order schemes do of course damp out the larger perturbations further downstream).

However, switching off gravity makes the problem disappear very rapidly.

I'm not quite sure why this happens, but it is noteworthy that a fixedValue outlet as used in this case is not valid. Pressure should increase with depth, not remain constant.

It is not clear whether this erronous BC influences the deccelelation of the interfacial gas phase near the inlet. I think it somewhat unlikely, but I dont have the time to pinpoint the origin at the moment.
eugene is offline   Reply With Quote

Old   June 1, 2005, 06:34
Default > but it is noteworthy that a
  #20
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
> but it is noteworthy that a fixedValue outlet as used in this case is not valid. Pressure should increase with depth, not remain constant.

Why do you think there is a problem with the oulet pressure BC? Remember we are solving for pd which is p - rho*g*h, i.e. is constant with depth at the outlet.
henry 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
2d interface Rogerio Fernandes Brito CFX 2 July 26, 2008 12:25
interface rym FLUENT 2 January 16, 2008 05:55
About Interface BC Philip FLUENT 0 January 3, 2008 02:51
How to set BC at the interface K Tamemy FLUENT 0 June 5, 2006 10:45
interface braket FLUENT 1 November 15, 2005 02:58


All times are GMT -4. The time now is 02:22.