# Case is not 3D or 2D ???

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

December 14, 2010, 09:49
Case is not 3D or 2D ???
#1
Member

P.A.
Join Date: Mar 2009
Location: Germany
Posts: 48
Rep Power: 8
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!

Pascal.
Attached Images
 grid_overview.jpg (44.7 KB, 43 views) grid_detail.jpg (50.8 KB, 35 views)

 December 14, 2010, 10:03 #2 Senior Member   Stefan Herbert Join Date: Dec 2009 Location: Darmstadt, Germany Posts: 129 Rep Power: 8 Hi, what is checkMesh reporting regarding "Mesh (non-empty, non-wedge) dimensions"? Regards, Stefan

 December 14, 2010, 10:22 checkMesh output #3 Member   P.A. Join Date: Mar 2009 Location: Germany Posts: 48 Rep Power: 8 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 <

 December 14, 2010, 12:34 #4 Senior Member   Stefan Herbert Join Date: Dec 2009 Location: Darmstadt, Germany Posts: 129 Rep Power: 8 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.

December 15, 2010, 04:51
How could I define internal empty patches?
#5
Member

P.A.
Join Date: Mar 2009
Location: Germany
Posts: 48
Rep Power: 8
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
 simpleView_1.gif (5.2 KB, 33 views) simpleView_3.gif (10.5 KB, 29 views) simpleView_internalStructure.gif (5.7 KB, 26 views) simpleView_internalStructure_iso.gif (11.0 KB, 27 views) grid_with_inner_block_visualized.jpg (56.0 KB, 34 views)

 December 15, 2010, 05:12 #6 Senior Member   Stefan Herbert Join Date: Dec 2009 Location: Darmstadt, Germany Posts: 129 Rep Power: 8 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

 December 15, 2010, 07:27 #7 Member   P.A. Join Date: Mar 2009 Location: Germany Posts: 48 Rep Power: 8 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::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.

 December 15, 2010, 08:08 #8 Senior Member   Stefan Herbert Join Date: Dec 2009 Location: Darmstadt, Germany Posts: 129 Rep Power: 8 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

 December 15, 2010, 10:01 Solved #9 Member   P.A. Join Date: Mar 2009 Location: Germany Posts: 48 Rep Power: 8 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.

 December 16, 2010, 03:52 #10 Senior Member   Alberto Passalacqua Join Date: Mar 2009 Location: Ames, Iowa, United States Posts: 1,895 Rep Power: 26 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

December 16, 2010, 06:11
blockMeshDict for LES cylinder
#11
Member

P.A.
Join Date: Mar 2009
Location: Germany
Posts: 48
Rep Power: 8
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.

Cheers, Pascal.
Attached Files
 blockMeshDict_study.zip (2.1 KB, 17 views) blockMeshDict_final.zip (2.1 KB, 15 views)

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post hsieh OpenFOAM 9 August 16, 2015 14:53 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36 microfin FLUENT 0 March 31, 2009 11:20 student FLUENT 1 January 29, 2007 11:37 vijay FLUENT 1 April 24, 2006 11:11

All times are GMT -4. The time now is 04:59.