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

BubbleInterTrackFoam Wedge Problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 12, 2017, 11:40
Default BubbleInterTrackFoam Wedge Problem
  #1
New Member
 
Manuel
Join Date: Jan 2013
Location: Darmstadt
Posts: 25
Rep Power: 6
Manuel CFD is on a distinguished road
Sponsored Links
Dear All,

I am trying to use bubbleInterTrackFoam with a wedge geometry in foam-extend 3.1.
After few time steps the solver blows up. Any hints??

Thanks

Manuel
Manuel CFD is offline   Reply With Quote
Sponsored Links

Old   April 18, 2017, 04:30
Default BubbleInterTrackFoam Wedge Problem
  #2
New Member
 
Manuel
Join Date: Jan 2013
Location: Darmstadt
Posts: 25
Rep Power: 6
Manuel CFD is on a distinguished road
Some more details...
I have duplicated the points on the axis and I have created small faces out of them.
These faces belong to a "symmetryPlane" patch called "centerline".
First I tried to create a standard wedge geometry with zero faces along the axis but in this case the mesh motion did not work at all. Having a look at the freeSurface class then I have figured out that a patch "centerline" along the axis is required by the solver for a correct
mesh motion.
Despite this correction, the solver blows up immediately. At the moment I have no idea about what causes the problem.
I have attached the case. Run the script "meshCreation" in order to create the
fvMesh and faMesh.
Has anyone ever performed a wedge simulation with bubbleInterTrackFoam??
I am waiting for your comments and suggestions.
Thanks.

Manuel
Attached Files
File Type: zip bubbleWedge.zip (10.7 KB, 8 views)
Manuel CFD is offline   Reply With Quote

Old   April 20, 2017, 21:53
Default
  #3
p.b
New Member
 
Join Date: Apr 2017
Posts: 9
Rep Power: 2
p.b is on a distinguished road
A few things that could help, but I'm not sure

1.) Have you tried bringing your foam-extend to version 4.0:https://sourceforge.net/p/foam-exten...i/master/tree/
But I just confirmed that in foam-extend-4.0 your case also runs only a few time steps until it crashes...

2.) Try to turn your wedge mesh into an annulus with a tiny whole along the central axis and apply a symmetray plane there

3.) Use a fvMotionSolver instead of the tetFemMotionSolver, as the latter might still have problems with the axis

4.) Try to decrease the time step and adjust all schemes

5.) Something seems to be wrong with the inletOutlet boundary condtion of U at the space patches, as the velocity field gets weird there. You should re-check this. Maybe there is a nasty bug in bubbleInterTrackFoam for wedgeMeshes...

6.) Have you tested the tutorials with bubbleInterTrackFoam? Do they run properly?
p.b is offline   Reply With Quote

Old   April 26, 2017, 06:44
Default BubbleInterTrackFoam Wedge Problem
  #4
New Member
 
Manuel
Join Date: Jan 2013
Location: Darmstadt
Posts: 25
Rep Power: 6
Manuel CFD is on a distinguished road
Hi p.b.,

Sorry for the late answer but due to other tasks I could not try your suggestions immediately. Regarding the geometry I was already using along the central axis a tiny patch with symmetryPlane conditions instead of a line. Maybe I did not explain it well in my previous post. I switched from the tetFemMotionSolver to the fvMotionSolver. It helps slightly and makes the computation faster but it does not solve the problem.
Looking more deeply at the code, I have noticed that the bubble center is not correctly
computed in the solver in the case of wedge geometry because it does not consider that the domain is only a slice of the "real" bubble. For this reason I have changed the file
createBubble.H and updateMovingReferenceFrame.H imposing Cb.x() =0.
In addition to this, I have found out that in the updateVelocity() of the freeSurface class
the term tangentialSurfaceTensionForce causes some troubles at the top of the bubble.
Since in my simulations I have no gradient of the surface tension coefficient I have
commented out this term for the moment.
With these two changes the simulation runs longer but slightly before 1ms it crashes again. Looking at the p and U fields in Paraview they seem fine apart the z component of the velocity which continuously raises during the simulation.
I attach the pictures of the fields at a time instance close to the crash.
Do you have any suggestions about it?

Thanks

Manuel
Attached Images
File Type: jpg p.jpg (26.1 KB, 9 views)
File Type: jpg Ux.jpg (29.0 KB, 8 views)
File Type: jpg Uy.jpg (31.9 KB, 10 views)
File Type: jpg Uz.jpg (27.4 KB, 10 views)
Manuel CFD is offline   Reply With Quote

Old   April 27, 2017, 10:21
Default
  #5
p.b
New Member
 
Join Date: Apr 2017
Posts: 9
Rep Power: 2
p.b is on a distinguished road
Sorry, but I have no more ideas. The tangential surface tension term made also problems in some of my simulations with interTrackFoam. I could also not run any cases with wedge-meshes for too small axis-patches (maybe try a "larger whole" in the centre of the bubble, just to see if this has any influence). To me it looks like there lurks a nasty bug in the freeSurface library (and there are for sure some!) or the moving reference frame calculations. It could also be related to the calculation/scaling of phi.

I'd suggest you to contact Zeljko Tukovic (the author of bubbleInterTrackFoam) from the University of Zagreb (Croatia) with a friendly mail, directly! :-) Another option would be to contact Holger Marschall from the University of Darmstadt (Germany). They both are great experts in the field.

If you have any update on this, please let me know, as I'm very curious how to fix this problem!
p.b is offline   Reply With Quote

Old   April 27, 2017, 10:33
Default
  #6
p.b
New Member
 
Join Date: Apr 2017
Posts: 9
Rep Power: 2
p.b is on a distinguished road
There is one more!

Try to define the axis patch as general patch (not as symmetryPlane) and use slip boundary conditions for all fields! There maybe some boundary cases missing in the freeSurface library or the calculations for bubbleInterTrackFoam.

For the tetPointVectorField, slip seems to be broken, too. So either stick with fvMotionSolver for this test or use the componentMixed boundary condition for motionU at the axis:
Code:
    axis
    {
//         type            slip; // broken in combination with wedge?
        type            componentMixed;
        refValue        uniform (0 0 0);
        valueFraction   uniform (1 0 0); // axis direction should be one!
    }
Also try to play with the pointNormalsCorrectionPatches in freeSurfaceProperties...
p.b is offline   Reply With Quote

Old   April 27, 2017, 10:48
Default
  #7
p.b
New Member
 
Join Date: Apr 2017
Posts: 9
Rep Power: 2
p.b is on a distinguished road
Have you also tried killing the y-component of U in the solver, e.g. by
Code:
U.replace(2, ZERO_VOL_SCALARFIELD);
?
p.b is offline   Reply With Quote

Old   April 28, 2017, 06:04
Default BubbleInterTrackFoam Wedge Problem
  #8
New Member
 
Manuel
Join Date: Jan 2013
Location: Darmstadt
Posts: 25
Rep Power: 6
Manuel CFD is on a distinguished road
Hi p.b.,

I have tried all your suggestions but the simulation still crashes. Also forcing the z component of the velocity to zero doesn't help because the problem is transferred
to the other components. I work in Darmstadt in the Holger Marschall's group. So if he had
a solution it would be easy for me to contact him . I will try to send an email to Zeljko Tukovic.
If I have any update, I will let you know.
Thanks for your help!!

Manuel
Manuel CFD is offline   Reply With Quote

Reply

Tags
bubbleintertrackfoam, interface tracking, wedge

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
Wedge shape meshing problem! aydemirk OpenFOAM Native Meshers: blockMesh 3 August 20, 2014 10:50
Wedge water impact DFBI Overset mesh jcamilleri STAR-CCM+ 1 March 31, 2014 12:58
Wedge Impact Problem Vimal FLUENT 0 September 24, 2007 17:21
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13

Sponsored Links


All times are GMT -4. The time now is 12:11.