[Dan1788]

Hello all,

I am using reactingFoam with OF 2.2.0 to simulate turbulent premixed combustion. Attached here is my mesh for the computational domain.

https://www.dropbox.com/s/hcb7tqhylz...itled.jpg?dl=0

I wanted to ignite the flame which is why I have decided to use setFields for flame ignition. Following is the file I picked up online.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM Extend Project: Open Source CFD        |
|  \\    /   O peration     | Version:  1.6-ext                               |
|   \\  /    A nd           | Web:      www.extend-project.de                 |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "system";
    object      setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
    volScalarFieldValue T 300
);

regions
(
    boxToCell
    {
        box (-1 -1 -1) (1 0 1);
        fieldValues
        (
            volScalarFieldValue T 1650
        );
    }
);

1. Can this same file be used for OF 2.2.0??
2. What does the term boxToCell mean and are the points (-1 -1 -1) and (1 0 1) the corner points of the box??
3. If I have a 2D axisymmetric mesh as shown in the link above, how can I specify a region/plane of high temperature??
3. If I want to give the information that the premixed gas, CH4+O2 is fully burnt in this box, how can I do so ??

[Yuri Almeida]

Hi Daniel,

1) You should look at a setFieldsDict file from the OF-2.2.0 to know this. Apparently it is OK.

2) It means that the setFields utility will set in the mesh, inside the box given by the corner points (-1 -1 -1) and (1 0 1), the desired characteristics, like the temperature equal to 1650.

3) Using the setFields, as explained above. Even though it is a 3D utility, the third coordinate will be ignored.

4) I'm not used to premixed flames, but they are controlled by chemistry. If you want to burn all the gases, you should set a high temperature (according to Arrhenius model) in this box, using the setFields utility.

But this does not necessary keep the flame burning all the gases. It will happen if the flame produces enough heat to sustain itself and it have enough space in the domain to burn all reagents.

[Dan1788]

Hi Yuri,

Thanks for your reply, it certainly helps

However, I am still confused about how to create a box for a 2D axisymmetric simulation. In OpenFoam an axisymmetric domain is simply a wedge of 5 degrees. How do I create a box in the wedge ??

[Yuri Almeida]

Hi Daniel,

It is not exactly a box that you create inside the mesh, but you will manipulate the elements that are at the intersection between this box and the mesh.

For instance, try in the cavity tutorial (incompressible/icoFoam/cavity) the setFields, using the setFieldsDict below:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | foam-extend: Open Source CFD |
| \\ / O peration | Version: 3.1 |
| \\ / A nd | Web: http://www.extend-project.de |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
volScalarFieldValue p 0
);

regions
(
boxToCell
{
box ( 0.04 0.04 -1.0 ) ( 0.06 0.06 1.0 );
fieldValues
(
volScalarFieldValue p 100
);
}
);

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

You will see in the centre of the cavity the new values for pressure. As you can see, it does not matter if the box is not bounded inside the geometry, as the z-coordinate clearly surpasses the z values for the mesh ( 0 to 0.1).

So, you only need to be sure that the box contain the mesh elements that you want to manipulate. Try this setFieldsDict in your wedge geometry as well and you will get the idea.

[Dan1788]

Hi Yuri,

Thanks for the info, it worked well.

I was looking at a tutorial and they specify velocity as volVectorFieldValue U (0 0 0) in the defaultFieldValues but do not specify it in the 'box'. Does that have any significance ??

[Yuri Almeida]

Hi Daniel,

No, it is just a default value that will be read during the execution of setFields.

The fieldValues in the boxToCell only defines the values inside the box, the other mesh parts will be set with default value.