[Archoncomando]

Hello, i've only started using OpenFOAM a few days back so i'm still fairly new to the whole process.



I'm working on a bachelor's thesis regarding a hydrofoil wing profile. My thesis is based in large part on several other students work over the last 4 years.



I'm currently struggling with getting through a complete InterFoam simulation without fatal errors.



The current one reads like this:


"method" not found in dictionary "mnt/c/.../system/fv.schemes ./mnt/c/.../fv.schemes.wallDist"


I'm not sure what is being referred to as method.



My fv.schemes file looks like this:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      fvSchemes;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

ddtSchemes
{
    default         localEuler rDeltaT;
}

gradSchemes
{
    default         Gauss linear;
}

divSchemes
{
    div(rhoPhi,U)   Gauss linearUpwind grad(U);
    div(phi,alpha)  Gauss vanLeer;
    div(phirb,alpha) Gauss interfaceCompression;
    div(phi,k)      Gauss upwind;
    div(phi,omega)  Gauss upwind;
    div((muEff*dev(T(grad(U))))) Gauss linear;
}

laplacianSchemes
{
    default         Gauss linear corrected;
}

interpolationSchemes
{
    default         linear;
}

snGradSchemes
{
    default         corrected;
}

fluxRequired
{
    default         no;
    p_rgh;
    pcorr;
    alpha.water;
}


// ************************************************************************* //

I'm working with the current OpenFOAM release version. Most of the work done before me is however made on OpenFoam 2.3. I've already adressed a lot of the issues with the changes but i'm really breaking my head on this one.



Or would you recommend just going back to OpenFOAM 2.3 instead of trying to adapt the project to 4+? Also is there a good source for file templates for the current version?



I'd be very grateful about some insights or Ideas on how to adress this.



Thanks in Advance


Florian

[pete20r2]

Add to fvShemes

wallDist
{
method meshWave;
}

[Archoncomando]

Hey there thanks for the quick fix! Did you just do that off the top of your head or is there some source for templates / guidelines what each file needs to include?

Is the fix for this issue similarly easy? OpenFOAM is now complaining about not having a pcorrfinal in the fvSolution.solvers.

Thanks again for the quick help

[pete20r2]

Hello again Florian, welcome, I just noticed you are new here
Free fish is good but catching them yourself is better huh.

Unfortunately, I could answer that off the top of my head lol.
But here is how I figured it out the first time.
There are lots of clues in the errors OF generates, unless something has gone very wrong the errors should guide you to a solution.

"method" not found in dictionary "mnt/c/.../system/fv.schemes ./mnt/c/.../fv.schemes.wallDist"

Notice how the file it's reading is called fvSchemes and it's looking for something called wallDist inside? The other clue is it's trying to read "method" from the fvSchemes.wallDist dictionary.
So we make an entry in fvSchemes for wallDist with an entry "method", but what is an appropriate value to ascribe to "method"?
There is a technique we call the 'banana' and it works for all variables, it's useful for dictionaries where the value needs to be some keyword but you don't know what your options are. Just set it to 'banana' or anything that is unlikely to be a valid input and run the solver.

wallDist
{
method banana;
}

OF will stop running and give you a list of options that are actually valid.
You can try it yourself but I ran it here just to show:

Selecting patchDistMethod banana


--> FOAM FATAL ERROR: 
Unknown patchDistMethod type banana

Valid patchDistMethod types : 

3
(
Poisson
advectionDiffusion
meshWave
)

Try it out on your fvSolutions problem

I find I end up here (direct to the meshWave entry):
Extended Code Guide - meshWave
The User Guide:
http://foam.sourceforge.net/docs/Gui...erGuide-A4.pdf
The wiki:
https://openfoamwiki.net/index.php/Main_Page
And of course these forums (you should probably post in the "OpenFOAM Running, Solving & CFD" subforum next time, more likely to get attention there )

Finally,
I know it's really exciting to get up and running and go straight for solving your problem but I can't recommend the tutorials enough.
They are included in the OF package and sorted by physics and solver.
Run some of them that have similar features to your problem and dig around the setup files ( steal things that work ). Find examples using the same solver, same boundary conditions, same mesh type, similar physics etc. Doesn't have to be all at once, just grab the bits you need from each.