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

LESdelta cubeRootVol dimension problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 14, 2005, 10:12
Default dear all, i am using oodles
  #1
Member
 
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 7
vvqf is on a distinguished road
dear all,

i am using oodles solver to solve a 2D case.
with delta cubeRootVol
But only ran into error :
 FatalErrorIn("cubeRootVolDelta::calcDelta()")
<< "Case is not 3D or 2D, LES is not applicable"

later i tried to change delta to smooth(just let the case run at first), by changing the entries in turbulenceProperties for delta, then I got another error:
------
Selecting incompressible transport model Newtonian
--> FOAM Warning :
From function dictionary::read(Istream&, const word&)
in file db/dictionary/dictionaryIO.C at line 92
Reading "/auto/people/evebe514/ewenqui/OpenFOAM/ewenqui-1.2/run/project/cases/cavity3/co nstant/turbulenceProperties" at line 175
could not add entry
smoothCoeffs
{
delta smooth;
smoothCoeffs
{
deltaCoeff 1;
}
maxDeltaRatio 1.1;
}
on line 175 of dictionary "/auto/people/evebe514/ewenqui/OpenFOAM/ewenqui-1.2/run/project/cases/cavity3/co nstant/turbulenceProperties"


--> FOAM FATAL IO ERROR : Attempt to return dictionary entry as a primitive

file: /auto/people/evebe514/ewenqui/OpenFOAM/ewenqui-1.2/run/project/cases/cavity3/con stant/turbulenceProperties::smoothCoeffs from line 124 to line 124.

From function ITstream& primitiveEntry::stream() const
in file db/dictionary/dictionaryEntry/dictionaryEntry.C at line 79.

FOAM aborting


Questions:
1. is the problem with geometry mesh?
I read cubeRootVolDelta.C
 const Vector<label>& directions = mesh().directions();
label nD = (directions.nComponents + cmptSum(directions))/2;

if nD is neither 2 nor 3, then the error will popup. And I think it might be the problem of the mesh.

2. how could i set the proper entry for delta smooth,
if i switch delta to smooth can help solve the problem?

Thank you in advance.
vvqf is offline   Reply With Quote

Old   December 16, 2005, 13:45
Default For delta smooth; you wan
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 724
Rep Power: 11
eugene is on a distinguished road
For
delta smooth;

you want

smoothCoeffs
{
delta cubeRootVol;
cubeRootVolCoeffs
{
deltaCoeff 1;
}
maxDeltaRatio 1.1;
}

This is a nested structure.
You cant derive smooth delta from smooth delta. You have to derive it from a more basic type, like cubeRootVol.
eugene is offline   Reply With Quote

Old   December 19, 2005, 03:40
Default Thank you very much for the re
  #3
Member
 
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 7
vvqf is on a distinguished road
Thank you very much for the reply.

I took the turbulenceProperties file from the tutorial case "oodles/pitzDaily". At the very beginning to avoid the "Case is not 3D or 2D" error, I tried to apply delta smooth and I just changed one line at the top of the turbulenceProperties file:
//delta cubeRootVol;
delta smooth;
But I still got the same error "Case is not 3D or 2D".

So later I guessed there might be more to change. Then I just roughly substituted all "cubeRootVol" with "smooth". -- That's the mistake you pointed out above. But after reading your reply, my understanding is you meant I just need to change delta cubeRootVol;
to
delta smooth;
as i did before.
However, the mistake remains.

Do you think it's the geometry problem of my mesh ? Or I did any mistake in using delta ?

Sorry to make the post long, but I want to state my problem clear. And as you can see i do not have this experience.

Expecting responding..
Thanks.
vvqf is offline   Reply With Quote

Old   December 19, 2005, 06:02
Default Yes. Have a look at /users/s
  #4
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 724
Rep Power: 11
eugene is on a distinguished road
Yes. Have a look at
/users/software/OpenFOAM/OpenFOAM-1.2.1/src/LESmodels/LESdeltas/cubeRootVolDelta /cubeRootVolDelta.C
from line 45 to 77
Also
/users/software/OpenFOAM/OpenFOAM-1.2.1/src/OpenFOAM/lnInclude/fvMesh.H
line 87

You probably have to many empty patches, that make the mesh think it is neither 2 or 3D.

Check your boundaries and make sure the only empty patches you have are the front and back of the the 2D geometry. If that still doesnt work, make the existing empty patches symmetry planes. This is bad practice and much more expensive, but it might help you find your problem.
eugene is offline   Reply With Quote

Old   December 19, 2005, 08:00
Default Thank you so much for the time
  #5
Member
 
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 7
vvqf is on a distinguished road
Thank you so much for the timely responding.

I did as you suggested, and also with reference to the tutorial case "oodles/pitzDaily". -- I made a lot changes comparing with the initial case I got.
Now the case runs!

There are now convergent problem: extremely huge Mean and max Courant Numbers. :s
I now have to have a look into it.

Thanks again.
vvqf is offline   Reply With Quote

Old   December 19, 2005, 08:48
Default one more thing: the only empt
  #6
Member
 
VVqf
Join Date: Mar 2009
Location: Braunschweig
Posts: 66
Rep Power: 7
vvqf is on a distinguished road
one more thing:
the only empty patches of my case are indeed the front and back of the 2D geometry.
Now I changed them into symmetryPlane.

Earlier I also made 'meanlingless' change of the boundary file.-- only to combine side1(front) and side2(back) into defaultFaces:
defaultFaces
{
type empty;
physicalType empty;
startFace 39176;
nFaces 39300;
}
still, FOAM FATAL ERROR : Case is not 3D or 2D, LES is not applicable.

PS:
in the polyMesh directory i dont have the <u>blockMeshDict</u> file. Well, it doesn't matter, I can still run the case, although a little difficult for me to understand the whole case.
vvqf 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
Dimension problem faroque OpenFOAM Running, Solving & CFD 5 February 19, 2008 08:56
Dimension problem with dyn LES models fabian_korn OpenFOAM Running, Solving & CFD 0 February 4, 2008 05:35
Is one dimension problem possible for Fluent alpha FLUENT 1 April 7, 2005 05:37
problem with grid dimension nisheet goyal Phoenics 1 June 18, 2001 09:28


All times are GMT -4. The time now is 17:23.