CFD Online URL
[Sponsors]
Home > Forums > OpenFOAM Running, Solving & CFD

Case is not 3D or 2D ???

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

Like Tree2Likes
  • 2 Post By herbert

Reply
 
LinkBack Thread Tools Display Modes
Old   December 14, 2010, 09:49
Default Case is not 3D or 2D ???
  #1
Member
 
P.A.
Join Date: Mar 2009
Location: Germany
Posts: 42
Rep Power: 7
blaise is on a distinguished road
Hi Foamers,

I am running into a problem with a pure blockMesh grid case. It is a simple circular cylinder (3 dimensional, finite length) in another cylindrical domain (see attached pictures). The blockMesh is done in a way that the innermost cells are wedge shaped. I do this by collapsing two vertices of the respective blocks. The vertices on which the others are being collapsed are in the center of the domain at (0 0 z).
The pictures attached do not show the real grid as it has many cells and slightly confusing gradings, so to make things clearer I left these details out.
When I start my LES calculation (which runs perfectly well with a cuboid instead of the cylinder, and has of course an O-grid structure) I get this error:

[0]
[0]
[0] --> FOAM FATAL ERROR:
[0] Case is not 3D or 2D, LES is not applicable
[0]
[0] From function cubeRootVolDelta::calcDelta()
[0] in file [1]
[1]
[1] --> FOAM FATAL ERROR:
[1] Case is not 3D or 2D, LES is not applicable
[2]
[2]
[2] --> FOAM FATAL ERROR:
[2] Case is not 3D or 2D, LES is not applicable
[2]
[2] From function cubeRootVolDelta::calcDelta()
[2] in file cubeRootVolDelta/cubeRootVolDelta.C at line 72.
[2]
FOAM parallel run exiting

Huhhh? If this grid is not 3D, the earth is a flat disc. So what am I doing wrong here?

Any hint is warmly appreciated!

Thanks in advance!

Pascal.
Attached Images
File Type: jpg grid_overview.jpg (44.7 KB, 35 views)
File Type: jpg grid_detail.jpg (50.8 KB, 28 views)
blaise is offline   Reply With Quote

Old   December 14, 2010, 10:03
Default
  #2
Senior Member
 
Stefan Herbert
Join Date: Dec 2009
Location: Darmstadt, Germany
Posts: 129
Rep Power: 8
herbert is on a distinguished road
Hi,

what is checkMesh reporting regarding "Mesh (non-empty, non-wedge) dimensions"?

Regards,
Stefan
herbert is offline   Reply With Quote

Old   December 14, 2010, 10:22
Default checkMesh output
  #3
Member
 
P.A.
Join Date: Mar 2009
Location: Germany
Posts: 42
Rep Power: 7
blaise is on a distinguished road
Hi Stefan,

sorry, I should have posted this as well - here we go:


-------- snippet -------------
Checking geometry...
Overall domain bounding box (-2.000011128 -2.000011128 0) (1.997266201 1.997266201 1.2)
Mesh (non-empty, non-wedge) directions (0 0 1)
Mesh (non-empty) directions (0 0 1)
***Number of edges not aligned with or perpendicular to non-empty directions: 24196
<<Writing 12500 points on non-aligned edges to set nonAlignedEdges
Boundary openness (-2.83056898103e-16 -2.13649125299e-16 -2.01622418729e-16) OK.
Max cell openness = 2.51676265652e-16 OK.
Max aspect ratio = 91.4751493518 OK.
Minumum face area = 1.17191508658e-05. Maximum face area = 0.055424148824. Face area magnitudes OK.
Min volume = 9.3753206926e-07. Max volume = 0.00443393190592. Total volume = 15.000079513. Cell volumes OK.
Mesh non-orthogonality Max: 1.50002356678 average: 0.18251629292
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.327643281514 OK.

Failed 1 mesh checks.

----------- snippet end -----------

The 12500 points in set nonAlignedEdges are exactly the total number of points in the case (regarding to paraview information). I do not understand why points appear in a set of non aligned edges, though. When I try to visualize the set in paraview, nothing is displayed.

Regarding the "nonempty, non-wedge" thing, please see above. What does it tell me?

Regards,

Pascal.
blaise is offline   Reply With Quote

Old   December 14, 2010, 12:34
Default
  #4
Senior Member
 
Stefan Herbert
Join Date: Dec 2009
Location: Darmstadt, Germany
Posts: 129
Rep Power: 8
herbert is on a distinguished road
Hi Pascal,

it seems that you have patches of type empty in your mesh (defined in constant/polyMesh/boundary) which is not valid for 3-D cases. It is only useable in 2-D cases. Just change the definition of these patches in the above mentioned file into "patch" and your boundary conditions eventually, too, if not alreay done.

Regards,
Stefan
large_eddy and abtin_c4 like this.
herbert is offline   Reply With Quote

Old   December 15, 2010, 04:51
Default How could I define internal empty patches?
  #5
Member
 
P.A.
Join Date: Mar 2009
Location: Germany
Posts: 42
Rep Power: 7
blaise is on a distinguished road
Hi Stefan,

I attach some pictures showing the internal structure of the grid. It turns out that the empty patches you are referring to are not on boundaries, but inside the grid. The edges resp. vertices of the inner cuboid region are collapsed onto the origin (0 0 z) so that the faces of this cuboid disappear. As far as I understand this, those faces are the ones the "empty" boundary type applies to. How am I supposed to apply a different bc to these faces?

No idea...

What do you recommend? Is a structure like this generally impossible in OF?

Thanks,

Pascal.
Attached Images
File Type: gif simpleView_1.gif (5.2 KB, 25 views)
File Type: gif simpleView_3.gif (10.5 KB, 22 views)
File Type: gif simpleView_internalStructure.gif (5.7 KB, 19 views)
File Type: gif simpleView_internalStructure_iso.gif (11.0 KB, 19 views)
File Type: jpg grid_with_inner_block_visualized.jpg (56.0 KB, 25 views)
blaise is offline   Reply With Quote

Old   December 15, 2010, 05:12
Default
  #6
Senior Member
 
Stefan Herbert
Join Date: Dec 2009
Location: Darmstadt, Germany
Posts: 129
Rep Power: 8
herbert is on a distinguished road
Hi Pascal,

as I said, the only information you have to edit is inside constant/polyMesh/boundary. Change their type or even delete them if they are showing "nFaces 0".

Regards,
Stefan
herbert is offline   Reply With Quote

Old   December 15, 2010, 07:27
Default
  #7
Member
 
P.A.
Join Date: Mar 2009
Location: Germany
Posts: 42
Rep Power: 7
blaise is on a distinguished road
Hi Stefan,

I tried to change the type "empty" to "patch", but I get errors saying that a value is required. When I enter a value line, I only can use "uniform" or "nonuniform", which is not applicable here. I tried to set the defaultFaces type to "calculated", but this gives the following error:

-------------------------------------
[3] --> FOAM FATAL ERROR:
[3]
gradientInternalCoeffs cannot be called for a calculatedFvPatchField
on patch defaultFaces of field U in file "/daten/ShipLES/geom_bodies/zylinder/cyl_blockMesh_LES_10Mz_v0.2/processor3/0/U"
You are probably trying to solve for a field with a default boundary condition.
[3]
[3] From function calculatedFvPatchField<Type>::gradientInternalCoef fs() const
[3] in file fields/fvPatchFields/basic/calculated/calculatedFvPatchField.C at line 186.
[3]
FOAM parallel run exiting

-------------------------------------

(I am not really sure about the meaning of "calculated" here).

I will now try to apply a "wall" bc to the four faces of the cuboid, as the faces get infinitely small and do not form a real wall, but a singularity with a line shape.

Any other idea?

Thanks and best regards,

Pascal.
blaise is offline   Reply With Quote

Old   December 15, 2010, 08:08
Default
  #8
Senior Member
 
Stefan Herbert
Join Date: Dec 2009
Location: Darmstadt, Germany
Posts: 129
Rep Power: 8
herbert is on a distinguished road
Hi Pascal,

please don't mix up patch definition (which should be patch in the file "constant/polyMesh/boundary") and your boundary condition definiton in the respective fields. Which bc in apporiate for you is hard to tell without knowing your case. But it should be something like zeroGradient, fixedValue etc. Calculated can not be used when you want to solve an equation for that field.

Regards,
Stefan
herbert is offline   Reply With Quote

Old   December 15, 2010, 10:01
Default Solved
  #9
Member
 
P.A.
Join Date: Mar 2009
Location: Germany
Posts: 42
Rep Power: 7
blaise is on a distinguished road
Hi Stefan,

I wasn't precise enough as where to set what (boundary type vs. bc). Anyway, things turned out to be a simple blockMeshDict tuning: I now define the four innermost blocks so that they all use the same pair of vertices to collapse on, and this works fine. What I had before was that I used a single collapsing point for each block, thus implicit defining the four interiour faces that went to defaultFaces (at least that is my understanding). Although the positions of these collapsing vertices were all the same, the faces seemed to be there, though infinitely small.

Thanks a lot for your assistance!

Best regards,

Pascal.
blaise is offline   Reply With Quote

Old   December 16, 2010, 03:52
Default
  #10
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,891
Rep Power: 25
alberto will become famous soon enoughalberto will become famous soon enough
Posting blockMeshDict would be helpful ;-)
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 16, 2010, 06:11
Default blockMeshDict for LES cylinder
  #11
Member
 
P.A.
Join Date: Mar 2009
Location: Germany
Posts: 42
Rep Power: 7
blaise is on a distinguished road
Here we go!

This is the final blockMesh with 10 Mio. cells (mind the gradings) and a simplified version for studying purposes. The latter is generally the same, but has different vertex locations and doesn't look very nice. With only 11200 cells it is more laptop compatible. ;-)

In the end I do not know yet if this kind of grid structure runs better than having a real O-grid for the empty cylinder, so I give no guarantee that this blockMesh works, but I will find out soon.

Comments appreciated!

Cheers, Pascal.
Attached Files
File Type: zip blockMeshDict_study.zip (2.1 KB, 11 views)
File Type: zip blockMeshDict_final.zip (2.1 KB, 13 views)
blaise 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
Superlinear speedup in OpenFOAM 13 msrinath80 OpenFOAM Running, Solving & CFD 17 August 22, 2009 04:59
Transient case running with a super computer microfin FLUENT 0 March 31, 2009 12:20
Is Playstation 3 cluster suitable for CFD work hsieh OpenFOAM 8 March 12, 2008 06:58
new mesh, same case file student FLUENT 1 January 29, 2007 11:37
Doubt in unsteady case vijay FLUENT 1 April 24, 2006 12:11


All times are GMT -4. The time now is 15:29.