CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Coodles

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 6, 2006, 07:17
Default Hi, does someone know, wher
  #1
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
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
anja is offline   Reply With Quote

Old   January 6, 2006, 07:22
Default Your best bet would be inspect
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Your best bet would be inspecting the source code. What kind of information were you looking for?
eugene is offline   Reply With Quote

Old   January 6, 2006, 07:53
Default I don't know how to set the in
  #3
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
I don't know how to set the initial variables, e.g. muSgs and muTilda.
Furthermore I get error messages concerning the laplacian schemes.
anja is offline   Reply With Quote

Old   January 6, 2006, 08:01
Default I take it you are using the co
  #4
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   January 6, 2006, 08:13
Default Yes, I do use the tutorial as
  #5
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
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
anja is offline   Reply With Quote

Old   January 6, 2006, 08:28
Default Works out of box for me. The
  #6
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,763
Rep Power: 21
hjasak will become famous soon enough
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
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   January 6, 2006, 08:44
Default Yeah, but if you are running c
  #7
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Yeah, but if you are running coodles, there should be no need to define laplacian(nu,U).
More info please.
eugene is offline   Reply With Quote

Old   January 6, 2006, 08:45
Default I also had to add: laplacian(
  #8
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
I also had to add:
laplacian(1|A(U),p)Gauss linear corrected;

But now it's saying:
Invalid boundary type name 'pressureTransmissiveOutlet'
anja is offline   Reply With Quote

Old   January 6, 2006, 08:57
Default Okay, I'm so so sorry. I made
  #9
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
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 is offline   Reply With Quote

Old   January 6, 2006, 09:25
Default There might be a problem with
  #10
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
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?
anja is offline   Reply With Quote

Old   January 6, 2006, 10:32
Default nan means "not-a-number". This
  #11
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   January 10, 2006, 08:06
Default I tried to set Co=0.75, but al
  #12
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
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 is offline   Reply With Quote

Old   January 10, 2006, 08:27
Default Or can someone please explain
  #13
Member
 
Anja Stretz
Join Date: Mar 2009
Posts: 92
Rep Power: 8
anja is on a distinguished road
Or can someone please explain me, what B for the initial variables of the coodles means?

Thanks again,
Anja
anja is offline   Reply With Quote

Old   January 10, 2006, 09:05
Default It is the term form filtering
  #14
Member
 
Fabian Peng Karrholm
Join Date: Mar 2009
Posts: 61
Rep Power: 8
fabianpk is on a distinguished road
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
fabianpk is offline   Reply With Quote

Old   January 10, 2006, 10:57
Default B is only needed as initial co
  #15
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
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.
eugene is offline   Reply With Quote

Old   March 9, 2006, 14:26
Default Hi, I want to run a coodle
  #16
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
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
melanie is offline   Reply With Quote

Old   March 9, 2006, 16:18
Default If you open the file with the
  #17
Assistant Moderator
 
Bernhard Gschaider
Join Date: Mar 2009
Posts: 3,915
Rep Power: 40
gschaider will become famous soon enoughgschaider will become famous soon enough
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.
__________________
Note: I don't use "Friend"-feature on this forum out of principle. Ah. And by the way: I'm not on Facebook either. So don't be offended if I don't accept your invitation/friend request
gschaider is offline   Reply With Quote

Old   March 9, 2006, 16:20
Default phi will be one of the fields
  #18
Senior Member
 
Gavin Tabor
Join Date: Mar 2009
Posts: 181
Rep Power: 8
grtabor is on a distinguished road
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
grtabor is offline   Reply With Quote

Old   March 10, 2006, 04:26
Default Thanks for your answers; I loo
  #19
Member
 
Mélanie Piellard
Join Date: Mar 2009
Posts: 86
Rep Power: 8
melanie is on a distinguished road
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
melanie is offline   Reply With Quote

Old   March 10, 2006, 05:24
Default Looks like you must have chang
  #20
Senior Member
 
Gavin Tabor
Join Date: Mar 2009
Posts: 181
Rep Power: 8
grtabor is on a distinguished road
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
grtabor 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
Coodles vs sonicTurbFoam hsieh OpenFOAM Running, Solving & CFD 10 February 3, 2009 07:17
Pressure waves bouncing around while using coodles ankgupta8um OpenFOAM Running, Solving & CFD 4 March 5, 2008 07:54
Nonphysical flow field while using coodles solver ankgupta8um OpenFOAM Running, Solving & CFD 5 January 26, 2008 17:54
Question about coodles tangd OpenFOAM Running, Solving & CFD 0 June 20, 2006 03:58
Startingsetting coodles on an academic case melanie OpenFOAM Running, Solving & CFD 5 March 30, 2006 04:00


All times are GMT -4. The time now is 02:48.