[astri]

Hi all,

I am running a case of natural ventilation of a simple building (box) with open windows. I created it as an outdoor case inside the wind tunnel, write the case in Butterfly then trying to run it in openFoam. Everything is fine when I execute blockMesh and snappyHexMesh. However, when I execute simpleFoam I've got an error message:


--> FOAM FATAL ERROR: (openfoam-2206)
cannot find file "/mnt/c/Users/astri/butterfly/boxexplode_45/2/p"

From virtual Foam::autoPtr<Foam::ISstream> Foam::fileOperations::uncollatedFileOperation::rea dStream(Foam::regIOobject&, const Foam::fileName&, const Foam::word&, bool) const
in file global/fileOperations/uncollatedFileOperation/uncollatedFileOperation.C at line 540.

FOAM exiting

I am trying different setting, but It always goes the same way. Would anyone share a thought why this is happen? Any advice would be very much appreciated

Best regards,

Astri

[Yann]

Hello Astri,

You get this error because the solver does not find the files containing the boundary conditions for each variable (p, U, ...) as stated in the error message:

cannot find file "/mnt/c/Users/astri/butterfly/boxexplode_45/2/p"

Posting the whole log file would help to know exactly what is going on, but my best guess is that you ran snappyHexMesh without the -overwrite option and snappy created new timeStep folders (1, 2) to write the castellated and snapped mesh.

I'm quoting the documentation (https://www.openfoam.com/documentati...yhexmesh-usage)

By default, each of snappyHexMesh's phases, i.e castellation, snapping and layer addition will write a complete mesh in time folders. This behaviour can be suppressed by using the option

snappyHexMesh `-overwrite`

To solve this issue you can use the overwrite option or manually move folders:

• move the polyMesh folder from 2/constant to constant/
• remove folders 1 and 2
• run simpleFoam

Let us know if it solves the issue!

Regards,
Yann

[astri]

Hi Yann,

Thank you very much for your kind response.
I've already done it as per your suggestion (the snappyHexMesh -overwrite), but another error message appears.



--> FOAM FATAL IO ERROR: (openfoam-2206)
Missing or invalid PatchFunction1 entry: d


file: 0/U.boundaryField.inlet at line 81.

From static Foam::autoPtr<Foam::PatchFunction1<Type> > Foam::PatchFunction1<Type>::New(const Foam:olyPatch&, const Foam::word&, const Foam::entry*, const Foam::dictionary&, bool, bool) [with Type = double]
in file /usr/src/packages/BUILD/src/meshTools/lnInclude/PatchFunction1New.C at line 124.

FOAM exiting
------------------------------------------------------

I really want to upload the U file from folder 0 to the attachment, but I always failed. It says invalid file. I don't know If I did it wrong, I am new to this forum.

What is written in line 81 of the script U is
type atmBoundaryLayerInletVelocity;


and this is I copy also the whole script.

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v1706+ |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
/* Butterfly 0.0.4 https://github.com/ladybug-tools/butterfly *\
\*---------------------------------------------------------------------------*/
FoamFile
{
version 4.0;
format ascii;
class volVectorField;
location "0";
object U;
}

dimensions [0 1 -1 0 0 0 0];

#include "initialConditions";

internalField uniform $flowVelocity;

boundaryField
{

right_side
{

type slip;

}

box
{

type fixedValue;

value uniform (0 0 0);

}

outlet
{

type inletOutlet;

inletValue uniform (0 0 0);

value $internalField;

}

left_side
{

type slip;

}

top
{

type slip;

}

ground
{

type fixedValue;

value uniform (0 0 0);

}

inlet
{

type atmBoundaryLayerInletVelocity;

#include "ABLConditions";

}

}





Do you know what happened, and could you advise me on what should I do?

Anyway, I can't open the documentation that you quoted in your reply. Is there any way for me to open it?

Thank you very much for your help.
Best regards,

Astri

[Yann]

Hello,

It complains about your inlet boundary condition, more specifically about the d parameter.

--> FOAM FATAL IO ERROR: (openfoam-2206)
Missing or invalid PatchFunction1 entry: d


file: 0/U.boundaryField.inlet at line 81.

Your current condition:

inlet
{

type atmBoundaryLayerInletVelocity;

#include "ABLConditions";

}

You must have a file named ABLConditions in your 0 directory. Is there a parameter d defined there?

Regards,
Yann

EDIT: I fixed the dead link in my previous post.

[astri]

Hi Yann, thank you so much!

Yes, you're right, there's no parameter d defined in my ABLConditions file.
Here's what's written in the file:


/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: v1706+ |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
/* Butterfly 0.0.4 https://github.com/ladybug-tools/butterfly *\
\*---------------------------------------------------------------------------*/

Uref 2.97;

Zref 10;

z0 uniform 1.0;

flowDir (0.0 1.0 0.0);

zDir (0 0 1);

zGround uniform -0.10000000149;

value $internalField;


-------------------------------------------------------------------

I have no idea how to define the parameter d. I've checked the OpenFOAM user guide, the example of ABLConditions in this link https://www.openfoam.com/documentati...daryLayer.html



inlet
{
// Mandatory and other optional entries
...

// Mandatory (inherited) entries (runtime modifiable)
flowDir (1 0 0);
zDir (0 0 1);
Uref 10.0;
Zref 0.0;
z0 uniform 0.1;
d uniform 0.0;
-----------------------------------------------------------

Should I just copy the definition for parameter d just like the example?
Thank you so very much Yann for your advice.

Best regards,
astri

[Yann]

Hi Astri,

You're welcome. About the d parameter, I have no idea since I never used this boundary condition.
There is a note about it in the documentation:

d is the displacement height, and "is relevant for flows over forests and cities" ([17], p. 28). "The displacement height gives the vertical displacement of the entire flow regime over areas which are densely covered with obstacles such as trees or buildings" ([17], p. 28).

Up to you to decide how to define this parameter. Checking the cited reference might help.

Cheers,
Yann