[FlyBob91]

Hello to all,
I found this explanation to read data from file to set the initial condition

2.2.10 The #include and #inputMode directives
For example, let us say a user wishes to set an initial value of pressure once to be used as the internal field and initial value at a boundary. We could create a file, e.g. named initialConditions, which contains the following entries:

    pressure 1e+05; 
    #inputMode merge
In order to use this pressure for both the internal and initial boundary fields, the user would simply include the following macro substitutions in the pressure field file p:

    #include "initialConditions" 
    internalField uniform $pressure; 
    boundaryField 
    { 
        patch1 
        { 
            type fixedValue; 
            value $internalField; 
        } 
    }
This is a fairly trivial example that simply demonstrates how this functionality works. However, the functionality can be used in many, more powerful ways particularly as a means of generalising case data to suit the user’s needs. For example, if a user has a set of cases that require the same RAS turbulence model settings, a single file can be created with those settings which is simply included in the turbulenceProperties file of each case. Macro substitutions can extend well beyond a single value so that, for example, sets of boundary conditions can be predefined and called by a single macro. The extent to which such functionality can be used is almost endless.

How can i modify these code to read a nonuniform vecotr field at my boundary? I want to set a non uniform field for the velocity boundary condition



Thanks for help

[FlyBob91]

Ok, i found the solution to the problem.

First, create the file where you want to store your velocity field. The file must have this format

velocityProfile         // name of your velocity prfoile
List<vector>
300                         // number of vectors (points)
(
(Ux Uy Uz)
.....
(Ux Uy Uz)
);

Second, put this file in the 0 directory (suppose to name it "inletCondition").
Now open the U file

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

internalField   uniform (0 0 0);

#include "inletCondition"

boundaryField
{
    inlet
    {
        type            fixedValue;
        value          nonuniform $velocityProfile;
    }

// ...... other boundary conditions

}

[deepbandivadekar]

Originally Posted by FlyBob91

Ok, i found the solution to the problem.
First, create the file where you want to store your velocity field. The file must have this format

velocityProfile         // name of your velocity prfoile
List<vector>
....

Footnote to this:

Both the semi-colons are important: 1) in the list file at the end after the ")" and 2) in the inlet conditions file after the keyword. Else OF will give errors.

[ddcampayo]

Originally Posted by FlyBob91

... The file must have this format

velocityProfile         // name of your velocity prfoile
List<vector>
300                         // number of vectors (points)
(
(Ux Uy Uz)
.....
(Ux Uy Uz)
);

[/CODE]

Any ideas on how to do this efficiently. What I mean is: usually the field will depend on the position, and the latter should be read from constant/polyMesh/points. I guess this calls for a python script that reads coordinates from that file and generates the field.

[deepbandivadekar]

Originally Posted by ddcampayo

Any ideas on how to do this efficiently. What I mean is: usually the field will depend on the position, and the latter should be read from constant/polyMesh/points. I guess this calls for a python script that reads coordinates from that file and generates the field.

I did the same. Because I needed the field values off of a particular face. Other way is to dabble with the solver. I wasn't particularly keen to get into that muck.

[Chhardik94]

I want to create the vector file from the outlet patch.how can i extract that in openfoam?

[deepbandivadekar]

Originally Posted by Chhardik94

I want to create the vector file from the outlet patch.how can i extract that in openfoam?

It's hard to figure out what exactly you want to do without many details.
It seems what you're trying to do is unrelated to this thread. I'd suggest to first search the forum for what you seek and see if you find any clues or start your own thread.

[Chhardik94]

Originally Posted by ddcampayo

Any ideas on how to do this efficiently. What I mean is: usually the field will depend on the position, and the latter should be read from constant/polyMesh/points. I guess this calls for a python script that reads coordinates from that file and generates the field.

I want to do this same thing but for only one patch. want to extract the foam file of the result for any boundary patch.

[deepbandivadekar]

Originally Posted by Chhardik94

I want to do this same thing but for only one patch. want to extract the foam file of the result for any boundary patch.

If you mean, you want to get data for variables like U, p, T.. for a single patch you can use the surfaceFieldValue functionobject.

In controlDict add this:

functions
{

    inletData
    {
        type            surfaceFieldValue; //surfaceFieldValue;
        libs            ("libfieldFunctionObjects.so");
        writeControl    writeTime;
        writeFields     true;
        surfaceFormat   foam;
        regionType      patch; //faceZone;
        name            inlet;
        operation       none;
        fields
        (
            p T U
        );
    }
  }

[alexj]

Hi,
I am in the same position, I need to create an initial condition of an internal velocity field. How did you go about doing that.


BTW, the order in the internal field file is according to cells and therefore probably better to use cell center coordinates instead of point coordinates from constant/polyMesh/points


Any help is greatly appreciated.