CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   Coodles (http://www.cfd-online.com/Forums/openfoam-pre-processing/62153-coodles.html)

anja January 6, 2006 07:17

Hi, does someone know, wher
 
Hi,

does someone know, where I can get basic information on the coodles solver, as there no links in the UserGuide?

Thanks a lot,
Anja

eugene January 6, 2006 07:22

Your best bet would be inspect
 
Your best bet would be inspecting the source code. What kind of information were you looking for?

anja January 6, 2006 07:53

I don't know how to set the in
 
I don't know how to set the initial variables, e.g. muSgs and muTilda.
Furthermore I get error messages concerning the laplacian schemes.

eugene January 6, 2006 08:01

I take it you are using the co
 
I take it you are using the coodles tutorial case as a template?

muSgs and muTilda are just nuSgs and nuTilda multiplied by the density.

Use the fvSchemes and fvSolution dictionaries from the coodles tutorial case. If you still have problems, please post the error messages here.

anja January 6, 2006 08:13

Yes, I do use the tutorial as
 
Yes, I do use the tutorial as a template.

Error for example:
Non-optional dictionary entry 'laplacian(nu,U)' not found in dictionary .../system/fvSchemes::laplacianSchemes in file .../system/fvSchemes::laplacianSchemes

hjasak January 6, 2006 08:28

Works out of box for me. The
 
Works out of box for me. The laplacian schemes section is as follows:

laplacianSchemes
{
default none;
laplacian(muEff,U) Gauss linear corrected;
laplacian((rho*1|A(U)),p) Gauss linear corrected;
laplacian(alphaEff,h) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DBEff,B) Gauss linear corrected;
laplacian(DmuTildaEff,muTilda) Gauss linear corrected;
}

Incodentally, when you hit messages like this, feel free to edit the offending dictionary to get it to work. In your case, I would add something like:

laplacian(nu,U) Gauss linear corrected;

into the appropriate secton and try again. Hope you can follow my idea.

Hrv

eugene January 6, 2006 08:44

Yeah, but if you are running c
 
Yeah, but if you are running coodles, there should be no need to define laplacian(nu,U).
More info please.

anja January 6, 2006 08:45

I also had to add: laplacian(
 
I also had to add:
laplacian(1|A(U),p)Gauss linear corrected;

But now it's saying:
Invalid boundary type name 'pressureTransmissiveOutlet'

anja January 6, 2006 08:57

Okay, I'm so so sorry. I made
 
Okay, I'm so so sorry. I made a mistake in the ControlDict, which was not a problem with coodles at all.

But here is the next one, I try to postprocess my results with paraFoam and then:
FOAM FATAL IO ERROR:wrong token type - expected scalar found on line 36 the word 'nan'

What does that mean?

anja January 6, 2006 09:25

There might be a problem with
 
There might be a problem with the 'Courant number'.

The tutorial for the lid-driven cavity flow says, that to achieve temporal accuracy and numerical stability when running icoFoam, a Courant number of less than 1 is required.

But which number is required for using coodles?

eugene January 6, 2006 10:32

nan means "not-a-number". This
 
nan means "not-a-number". This means youre calculation has blown up and written some nonsence to file.

Max courant number for standard coodles should also remain below 1. Preferrably below 0.7-8'ish.

anja January 10, 2006 08:06

I tried to set Co=0.75, but al
 
I tried to set Co=0.75, but all I get during the calculation is:
Mean and max Courant Numbers = nan nan
time step continuity errors : sum local = nan, global = nan, cumulative = nan
time step continuity errors : sum local = nan, global = nan, cumulative = nan
bounding k, min: 0 max: 0 average: 0

Does someone have any suggestion why this happens?

Thanks a lot for the help,
Anja

anja January 10, 2006 08:27

Or can someone please explain
 
Or can someone please explain me, what B for the initial variables of the coodles means?

Thanks again,
Anja

fabianpk January 10, 2006 09:05

It is the term form filtering
 
It is the term form filtering the Navier stokes equations, you can take a look at the H file of the LES model you are using to see its exact definition. For example /OpenFOAM/OpenFOAM-1.2/src/LESmodels/compressible/oneEqEddy/oneEqEddy.H

B = 2/3*k*I - 2*nuEff*dev(D)

/Fabian

eugene January 10, 2006 10:57

B is only needed as initial co
 
B is only needed as initial condition when you are using a Reynolds stress SGS model. It represents the SGS stresses.

On the rest, keep making your timestep smaller. If that doesnt eventually work, you have problems with your boundary conditions.

melanie March 9, 2006 14:26

Hi, I want to run a coodle
 
Hi,

I want to run a coodle calculation from a simpleFoam result, as an initial guess of the flow. I copied the case and made the adequate corrections in the system files, but there is still something wrong as I get the error message:

--> FOAM FATAL ERROR : dimensions of phi are not correct

From function CrankNicholsonDdtScheme<type>::fvcDdtPhiCorr
in file finiteVolume/ddtSchemes/CrankNicholsonDdtScheme/CrankNicholson

I suppose that the trouble comes from the compressibility, but I don't find where to set the dimension of phi.
Could someone give me a hint ? Thanks !
mélanie

gschaider March 9, 2006 16:18

If you open the file with the
 
If you open the file with the phi-data, just below the header before the line internalField you'll find a line "dimensions" with 7 numbers (Which number corresponds to which SI-unit is documented in the Programmer's Manual).

BUT: most solvers (don't know about coodle, never worked with that) calculate phi from U and rho if they don't find it in the initial time-step. So you might as well remove phi from the ICs and start the simulation.

grtabor March 9, 2006 16:20

phi will be one of the fields
 
phi will be one of the fields in the timestep directory that you are starting from; the dimensions are contained in the header. Alternatively just delete the file; coodles should recalculate it during startup if it can't find it.

Gavin

melanie March 10, 2006 04:26

Thanks for your answers; I loo
 
Thanks for your answers; I looked in the time directory and did not find the phi file, but I forgot to mention what's in the log-file:

Create mesh for time = 0

Reading thermophysical properties
Selecting thermodynamics package hThermo<pureMixture<constTransport<specieThermo<hC onstThermo<perfect
Gas>>>>>

Reading field U
Reading/calculating face flux field phi

Creating turbulence model
--> FOAM Warning :
From function cubeRootVolDelta::calcDelta()
in file cubeRootVolDelta/cubeRootVolDelta.C at line 54
Case is 2D, LES is not strictly applicable

Creating field DpDt

Starting time loop
Time = 5e-07

Mean and max Courant Numbers = nan nan

As the same case is running well with oodles (exactly the same except the application and thermophysical properties), I think it does not come from LES.
Thanks !
mélanie

grtabor March 10, 2006 05:24

Looks like you must have chang
 
Looks like you must have changed _something_ as the code is now starting up, albiet with a problem with the Courant number. Why are you trying to run an LES case in 2d?

The courant numbers are evaluated in
src/cfdTools/compressible/CourantNo.H - have a look there to figure out why you are generating NaN's. Looking at what is there, my guess is that there is something wrong with your rho field; since

surfaceScalarField SfUfbyDelta =
mesh.surfaceInterpolation::deltaCoeffs()*mag(phi)/fvc::interpolate(rho);

and this is on the bottom it could be screwing things up.

Gavin


All times are GMT -4. The time now is 10:18.