[Per]

Dear all

I have (most likely) an unusual problem. I want to set a constant velocity field in a part of the solution domain. Let's say (1 0 0) for simplicity; and I want this value to be constant throughout the whole simulation. Please note that this not is an investigation of an actual physical problem. I only want to investigate the effect of this imposed velocity field.

I tried to use setFields, but as expected it only gave the desired velocity field as an initial condition at T=0. I have searched the forum, but have not yet found a solution that does not involve altering the source code. Does anyone know if this is possible without altering the source code?

Thanks in advance for replies.
Regards
Per

[fisch]

Using a boundary condition at this point could solve your problem
but then you have to define a BC for p etc, too...

[Per]

I actually want to impose a velocity field on a control volume; not a surface or a point. So I guess a boundary condition will not be sufficient. Is there no way to set a fixed velocity inside some chosen cells (or control volume)?

Regards
Per

[gschaider]

Originally Posted by Per

I actually want to impose a velocity field on a control volume; not a surface or a point. So I guess a boundary condition will not be sufficient. Is there no way to set a fixed velocity inside some chosen cells (or control volume)?

Regards
Per

There are two ways:
- you modify the solver to fix the values during the solution of the linear equation. All these methods are based on the setValues-method of fvMatrix. One would be the explicitSource-class in OF (havn't used that yet). The other would be forceEquation in swak4Foam (I think there is a discussion on this somewhere here on the board). explicitSource sets a constant value in a fixed cell region. forceEquation can use any expression (for the value and the location)
- the other method would be to use a functionObject to reset the field in a specific region after the solution process. That is more of a hack but works in a lot of instances. One such functionObject would be manipulateField in the swak4Foam-suite. But maybe there are others

[Per]

Thanks for the reply Bernhard

I guess I have to install swak4Foam. Since I have trouble with compiling (due to dependency problems), is it possible to download and install swak4Foam without compiling? I ask because I read something about it at https://openfoam-extend.svn.sourcefo...ies/swak4Foam/. I did not install OF on the system myself. The one who did had problems with compiling, and therefor installed pre-compiled OF libraries and utilities.

Btw, I use OF 2.1.0.

Regards
Per

[gschaider]

Originally Posted by Per

Thanks for the reply Bernhard

I guess I have to install swak4Foam. Since I have trouble with compiling (due to dependency problems), is it possible to download and install swak4Foam without compiling? I ask because I read something about it at https://openfoam-extend.svn.sourcefo...ies/swak4Foam/. I did not install OF on the system myself. The one who did had problems with compiling, and therefor installed pre-compiled OF libraries and utilities.

Btw, I use OF 2.1.0.

Regards
Per

Dependencies for swak4Foam are not too bad: only flex and bison

It is true. In the swak4Foam-sources there is everything needed to roll Debian-packages (this is needed for the yearly Workshop-ISO) But I don't have the time (nor am I very motivated as I don't have Ubuntu/Debian systems nor have the people I work for) to roll binary releases in addition to the source releases. I have said it before: if someone volunteers to do that I will gladly assist her (same goes for anyone who wants to package RPM-releases)

[Eloise]

Originally Posted by Per

I actually want to impose a velocity field on a control volume; not a surface or a point. So I guess a boundary condition will not be sufficient. Is there no way to set a fixed velocity inside some chosen cells (or control volume)?

Hi Per!
I have the intention to do something similar. Could you give me some feedback about the methods you tested? What were pros and cons? What finally worked?
Thanks!
Eloïse

[jiahui_93]

Originally Posted by Per

Dear all

I have (most likely) an unusual problem. I want to set a constant velocity field in a part of the solution domain. Let's say (1 0 0) for simplicity; and I want this value to be constant throughout the whole simulation. Please note that this not is an investigation of an actual physical problem. I only want to investigate the effect of this imposed velocity field.

I tried to use setFields, but as expected it only gave the desired velocity field as an initial condition at T=0. I have searched the forum, but have not yet found a solution that does not involve altering the source code. Does anyone know if this is possible without altering the source code?

Thanks in advance for replies.
Regards
Per

Hi, I am facing the same problem as you. I saw your post when i plan to started a new thread here. haha. May I ask for your advice on this matter if you had solved it? I would be very grateful for your help. Thanks =)

[Antimony]

Hi,

Does not a combination of fvOptions and codedSource boundary condition help?

Cheers,
Antimony

[gschaider]

Originally Posted by jiahui_93

Hi, I am facing the same problem as you. I saw your post when i plan to started a new thread here. haha. May I ask for your advice on this matter if you had solved it? I would be very grateful for your help. Thanks =)

Try the "fixedValue" fvOption

[jiahui_93]

Originally Posted by Antimony

Hi,

Does not a combination of fvOptions and codedSource boundary condition help?

Cheers,
Antimony

Originally Posted by gschaider

Try the "fixedValue" fvOption

Hi, Thanks for the help and suggestions. I learned a new thing FvOptions works, i use scalarFixedValueConstraint and vectorFixedValueConstraint as following:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  plus                                  |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
carIntFixedScalar
{
type scalarFixedValueConstraint;
active yes;
scalarFixedValueConstraintCoeffs
{
selectionMode cellZone;
cellZone carIntCZ;
fieldValues
{
P  0;
k  0;
epsilon  0;
}
}
}

carIntFixedVector
{
type vectorFixedValueConstraint;
active yes;
vectorFixedValueConstraintCoeffs
{
selectionMode cellZone;
cellZone carIntCZ;
fieldValues
{
U  (0 0 0);
}
}
}


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

But the movingWall of my solid(20 m/s U, 0 P) within the domain(0 U, 0 P) seems cannot generate any airflow U. It come out to be whole things has no flow. May I get some opinion on how to get the movingWall to produce airflow. I mean theoretically moving solid should produce air velocity and pressure surrounding it, is it? May I get some suggestion on this matter? Is fvOptions useful in this? Thanks

[gschaider]

Originally Posted by jiahui_93

Hi, Thanks for the help and suggestions. I learned a new thing FvOptions works, i use scalarFixedValueConstraint and vectorFixedValueConstraint as following:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  plus                                  |
|   \\  /    A nd           | Web:      www.OpenFOAM.com                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant";
    object      fvOptions;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
carIntFixedScalar
{
type scalarFixedValueConstraint;
active yes;
scalarFixedValueConstraintCoeffs
{
selectionMode cellZone;
cellZone carIntCZ;
fieldValues
{
P  0;
k  0;
epsilon  0;
}
}
}

carIntFixedVector
{
type vectorFixedValueConstraint;
active yes;
vectorFixedValueConstraintCoeffs
{
selectionMode cellZone;
cellZone carIntCZ;
fieldValues
{
U  (0 0 0);
}
}
}


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

But the movingWall of my solid(20 m/s U, 0 P) within the domain(0 U, 0 P) seems cannot generate any airflow U. It come out to be whole things has no flow. May I get some opinion on how to get the movingWall to produce airflow. I mean theoretically moving solid should produce air velocity and pressure surrounding it, is it? May I get some suggestion on this matter? Is fvOptions useful in this? Thanks

Without more details (for instance: is carIntCZ next to the movingWall?) it is hard to tell

[jiahui_93]

Originally Posted by gschaider

Without more details (for instance: is carIntCZ next to the movingWall?) it is hard to tell

Hi, thanks again for help and i'm sry for lack of info. Here are my posts for more details:

PimpleDyMFoam --Simulate turbulence caused by moving object

Linear motion of a solid inside a fluid

Actually, i am trying to build a 3D hollow box(car) moving in a rectangular tube domain (shaft), and i aim to mesh the space btwn hollow box and rectangular tube to study the external airflow and pressure and turbulence parameters. This is my starting step to learn the simulation of aerodynamic outside vehicle or body within a domain. It seems didnt work if delete the cells within the box to make it hollow. So, i am now trying to set every fields of cellZone in the car (carIntCZ) to be zero value. Is appropriate?
I am sry for my dummy questions. Thanks a lot =)

[Eloise]

Originally Posted by jiahui_93

This is my starting step to learn the simulation of aerodynamic outside vehicle or body within a domain.

Hi,
Have you tried the motorbike tutorial to get started?
Regards,
Eloïse