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

Inappropriate boundary conditions?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 23, 2012, 07:32
Default Inappropriate boundary conditions?
  #1
New Member
 
Join Date: Sep 2012
Location: Germany
Posts: 25
Rep Power: 6
Studi is on a distinguished road
Hello everyone!
I want to ask, if you might take a look into my following case? The calculations abort after ten or some more iterations due to an excessively raising Courant number. Apparently the fast raising velocity U causes the solver to give up. In my experience most cases aborted in consequence of wrong boundary conditions, but I can't see any mistakes there. (see codes below)
The model is a flow channel (see attachment 'model) which has an inlet 'einlass' on its upper side (green) and an outlet (red) below. The wall 'wand' is yellow.
Postprocessing the few time steps before the calculations stop shows me results I really don't understand.
Time step 1 (1.jpg) seems okay, but time step 11 (11.jpg) already shows an outrageous high velocity U.

The BCs:
U
Code:
dimensions      [0 1 -1 0 0 0 0];
internalField   uniform (0 0 0);
boundaryField
{
    einlass
    {
        type            fixedValue;
        value           uniform (1e-3 0 0);
    }
    auslass
    {
         type            zeroGradient;
    }
    wand
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
}
p
Code:
dimensions      [0 2 -2 0 0 0 0];
internalField   uniform 1;
boundaryField
{
    einlass
    {
        type            zeroGradient;
    }
    auslass
    {
        type            fixedValue;
        value           uniform 1;
    }
    wand
    {
        type            zeroGradient;
    }     
}
transportProperties
Code:
transportModel  CrossPowerLaw;
CrossPowerLawCoeffs
{
    nu0             nu0 [ 0 2 -1 0 0 0 0 ] 300000;
    nuInf           nuInf [ 0 2 -1 0 0 0 0 ] 50;
    m               m [ 0 0 1 0 0 0 0 ] 2.5;
    n               n [ 0 0 0 0 0 0 0 ] 0.8;
}
Does anybody have an idea or sees a mistake?
Salome meshes without errors and checkMesh is happy, too. (see below)
Code:
Mesh stats
    points:           5378
    faces:            46288
    internal faces:   39840
    cells:            21532
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     0
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    21532
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
    Patch               Faces    Points   Surface topology                  
    einlass             908      503      ok (non-closed singly connected)  
    auslass             116      77       ok (non-closed singly connected)  
    wand                5424     2778     ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-0.15 -0.0559199 -0.125) (-0.0297394 0.045 -0.035)
    Mesh (non-empty, non-wedge) directions (1 1 1)
    Mesh (non-empty) directions (1 1 1)
    Boundary openness (3.0834e-16 2.71627e-17 8.63031e-17) OK.
    Max cell openness = 2.25618e-16 OK.
    Max aspect ratio = 30.2779 OK.
    Minumum face area = 1.31017e-09. Maximum face area = 9.67659e-05.  Face area magnitudes OK.
    Min volume = 2.37245e-13. Max volume = 3.29188e-07.  Total volume = 0.000503545.  Cell volumes OK.
    Mesh non-orthogonality Max: 84.4948 average: 19.033
   *Number of severely non-orthogonal faces: 10.
    Non-orthogonality check OK.
  <<Writing 10 non-orthogonal faces to set nonOrthoFaces
    Face pyramids OK.
    Max skewness = 1.41613 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End
I appreciate any idea or any help! Many thanks in advance.


Regards
Sebastian
Attached Images
File Type: jpg model.jpg (10.5 KB, 17 views)
File Type: jpg 1.jpg (77.5 KB, 23 views)
File Type: jpg 11.jpg (94.8 KB, 24 views)
Studi is offline   Reply With Quote

Old   November 23, 2012, 07:44
Default
  #2
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 585
Rep Power: 20
chegdan will become famous soon enoughchegdan will become famous soon enough
Can you use hex or polyhedral cells instead of tetrahedral? Tets are known to behave badly. If there is swirl at the exit, you might want to try inletOulet for velocity. Also, it has been noted in the forum and from my own personal experience, that fixedMeanValue for pressure can be a little more stable. However, I have only used that BC in steady-state problems. Lastly, how does a steady-state solver perform, can you get a SS solution?
__________________
Dan

Find me on twitter @dancombest and LinkedIn
chegdan is offline   Reply With Quote

Old   November 23, 2012, 11:32
Default
  #3
New Member
 
Join Date: Sep 2012
Location: Germany
Posts: 25
Rep Power: 6
Studi is on a distinguished road
Thanks for your response, chegdan!

I use Salome for the meshing... What would you recommend?
The BC inletOutlet unfortunately didn't solve my problem, but I have to admit, that I am not sure, if i used it correctly. I integrated it for the velocity U at the outlet. Would you use it for pressure BCs, too?
Concerning the fixedMeanPressure I didn't try it until now. Did I read correctly, that I have to compile it from other sources?


Sebastian
Studi is offline   Reply With Quote

Old   November 23, 2012, 12:10
Default
  #4
Senior Member
 
Lieven
Join Date: Dec 2011
Location: Leuven, Belgium
Posts: 297
Rep Power: 15
Lieven will become famous soon enough
Have a look at http://www.cfd-online.com/Forums/ope...condition.html for a link (and some explanation) to the sources of the fixedMeanValue boundary condition.

Do you let your time step to be determined dynamically (i.e. based on the courant number)? If not, try to run the case with pimpleFoam (or the equivalent if its not an incompressible flow) and set the maximum courant number < 1.

Greetz,

L
Lieven is offline   Reply With Quote

Old   November 23, 2012, 12:21
Default
  #5
Senior Member
 
chegdan's Avatar
 
Daniel P. Combest
Join Date: Mar 2009
Location: St. Louis, USA
Posts: 585
Rep Power: 20
chegdan will become famous soon enoughchegdan will become famous soon enough
Sebastian,

If you can get an stl out of salome for the surfaces, you might want to give snappyHexMesh a try and generate Hex cells. If you want to go the arbitrary polyhedral mesh route, you can generate a Delaunay triangulate tet mesh and then convert it to arbitrary polyhedral using polyDualMesh. fixedMeanValue is in the extend version of OpenFOAM and you can get the code and compile it with minimal effort. There is a discussion located at http://www.cfd-online.com/Forums/ope...condition.html. Good luck and have a great weekend!


Quote:
Originally Posted by Studi View Post
Thanks for your response, chegdan!

I use Salome for the meshing... What would you recommend?
The BC inletOutlet unfortunately didn't solve my problem, but I have to admit, that I am not sure, if i used it correctly. I integrated it for the velocity U at the outlet. Would you use it for pressure BCs, too?
Concerning the fixedMeanPressure I didn't try it until now. Did I read correctly, that I have to compile it from other sources?


Sebastian
__________________
Dan

Find me on twitter @dancombest and LinkedIn
chegdan is offline   Reply With Quote

Old   January 17, 2013, 09:08
Default
  #6
Senior Member
 
Dongyue Li
Join Date: Jun 2012
Location: Torino, Italy
Posts: 743
Rep Power: 9
sharonyue is on a distinguished road
Quote:
transportModel CrossPowerLaw;
CrossPowerLawCoeffs
{
nu0 nu0 [ 0 2 -1 0 0 0 0 ] 300000;
nuInf nuInf [ 0 2 -1 0 0 0 0 ] 50;
m m [ 0 0 1 0 0 0 0 ] 2.5;
n n [ 0 0 0 0 0 0 0 ] 0.8;
}
Are you sure the nu0 and nuInf is correct? what kind of substance is this so viscous?
sharonyue 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
Impinging Jet Boundary Conditions Anindya Main CFD Forum 25 February 27, 2016 13:58
symmetry boundary conditions in cfx lost.identity CFX 41 May 22, 2013 07:21
OpenFOAM Variable Velocity Boundary Conditions NickolasPl OpenFOAM Programming & Development 2 May 19, 2011 05:37
boundary conditions and mesh exporting vaina74 Open Source Meshers: Gmsh, Netgen, CGNS, ... 2 May 27, 2010 09:38
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 22:10.