[Adamkat]

Hi all,
I am trying to simulate heavy gas flow into my domain. The problem is I don't get any in flow velocity?!
I suspect it is either wrong boundary conditions or wrong mesh/patches.
Please help, I have no idea how to advance.
Thanks,
Adam

I am using rhoReactiveBuoyantFoam

Here are my /0 files:

U

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

internalField   uniform (0 0 0);

boundaryField
{
    gasInlet
    {
        type            fixedValue;
        value           uniform (0 -1 0);
    }


    gasOutlet
    {
        type            pressureInletOutletVelocity;
        value           $internalField;
      //  phi             phi;
    }
    frontAndBack
    {
        type            empty;
    }

p_rgh

dimensions      [1 -1 -2 0 0 0 0];

internalField   uniform 1e5;

boundaryField
{
    gasInlet
    {
        type            zeroGradient;
    }
    gasOutlet
    {
        type            totalPressure;
        p0              $internalField;
        U               U;
        phi             phi;
        rho             rho;
        psi             none;
        gamma           0;
        value           $internalField;
    }
    frontAndBack
    {
        type            empty;
    }

N2

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0.5;

boundaryField
{
    gasInlet
    {
        type            fixedValue;
        value           uniform 0.0;
    }
    gasOutlet
    {
        type            inletOutlet;
        inletValue      uniform 1.0;
        value           uniform 1.0;

    }
    frontAndBack
    {
        type            empty;
    }

SF6 //the heavy gas

dimensions      [0 0 0 0 0 0 0];

internalField   uniform 0.5;

boundaryField
{
    gasInlet
    {
        type            fixedValue;
        value           uniform 1.0;
    }
    gasOutlet
    {
        type            inletOutlet;
        inletValue      uniform 0.0;
        value           uniform 0.0;
    }
    frontAndBack
    {
        type            empty;
    }

Perhaps it has something to do with the geometry so I attached a picture of the domain.
blockMeshDict:

convertToMeters 1;

vertices
(
                      // bottom box
    (0.0  -0.1 -0.01) //0
    (0.2 -0.1 -0.01)  //1
    (0.2  0.1 -0.01)  //2
    (0.0   0.1 -0.01)  //3
    (0.0  -0.1  0.01)  //4
    (0.2 -0.1  0.01)  //5
    (0.2  0.1  0.01)  //6
    (0.0   0.1  0.01)// 7
                     // top part
                     //center
    (0.09 0.1 -0.01) //8
    (0.11 0.1 -0.01) //9
    (0.11 0.16 -0.01) //10
    (0.09 0.16 -0.01) //11
    (0.09 0.1 0.01) //12
    (0.11 0.1 0.01) //13
    (0.11 0.16 0.01) //14
    (0.09 0.16 0.01) //15
                    // corners
    (0 0.16 -0.01) //16
    (0.2 0.16 -0.01) //17
    (0 0.16 0.01) //18
    (0.2 0.16 0.01) //19
);

blocks
(
    hex (0 1 2 3 4 5 6 7) (100 100 1) simpleGrading (1 1 1) //bottom box
    hex (8 9 10 11 12 13 14 15) (10 30 1) simpleGrading (1 1 1) //center top box
    hex (3 8 11 16 7 12 15 18) (45 30 1) simpleGrading (1 1 1) //left top box
    hex (9 2 17 10 13 6 19 14) (45 30 1) simpleGrading (1 1 1) //right top box);
);
edges
(
);

boundary
(
  gasInlet
      {
          type patch;
          faces
          (
            (10 11 14 15)
          );
      }

  gasOutlet
  {
      type patch;
      faces
      (
          (4 7 3 0)
          (7 18 16 3)
          (1 2 6 5)
          (2 17 19 6)
          (0 1 5 4)
          (17 10 14 19)
          (11 16 18 15)
      );
  }
  frontAndBack
  {
      type empty;
      faces
      (
          (4 5 6 7)
          (13 6 19 14)
          (12 13 14 15)
          (7 12 15 18)
          (0 3 2 1)
          (10 17 2 9)
          (11 10 9 8)
          (16 11 8 3)

      );
  }
);

mergePatchPairs
(
);

[floquation]

I'm guessing that having an inlet and an outlet directly adjacent to each other like that is a bad thing numerically.

I know from interFoam that in order to have an inlet next to a wall in the same geometry that you are using, I require to add some sort of tube or nozzle-like geometry on top of the inlet, such that the inlet is not directly adjacent to the wall, e.g.:

  inlet
    __
   |  |
___|  |___

[Adamkat]

Thanks man!
I'll try and update.

[kcjarvis56]

The mesh has some empty faces on the inside specifically (7 3 8 12) (12 8 9 13) (13 9 2 6). Try the below block mesh.

convertToMeters 1;

vertices
(
	(0 -0.1 -0.01) //0
	(0.09 -0.1 -0.01) //1
	(0.09 0.16 -0.01) //2
	(0 0.16 -0.01) //3
	(0 -0.1 0.01) //4
	(0.09 -0.1 0.01) //5
	(0.09 0.16 0.01) //6
	(0 0.16 0.01) //7
	(0.11 -0.1 -0.01) //8
	(0.11 0.16 -0.01) //9
	(0.11 0.16 0.01) //10
	(0.11 -0.1 0.01) //11
	(0.2 -0.1 -0.01) //12
	(0.2 0.16 -0.01) //13
	(0.2 0.16 0.01) //14
	(0.2 -0.1 0.01) //15

);

blocks
(
	 hex (0 1 2 3 4 5 6 7) (45 130 1) simpleGrading (1 1 1)
	 hex (1 8 9 2 5 11 10 6) (10 130 1) simpleGrading (1 1 1)
	 hex (8 12 13 9 11 15 14 10) (45 130 1) simpleGrading (1 1 1)

);

boundary
(
	gasInlet
	{
		type	patch;
		faces	
		(
			(2 6 10 9)
		);
	}
	gasOutlet
	{
		type	patch;
		faces	
		(
			(9 10 14 13)
			(12 13 14 15)
			(8 12 15 11)
			(1 8 11 5)
			(0 1 5 4)
			(0 4 7 3)
			(3 7 6 2)
		);
	}
	frontAndBack
	{
		type	empty;
		faces	
		(
			(4 5 6 7)
			(5 11 10 6)
			(11 15 14 10)
			(8 9 13 12)
			(1 2 9 8)
			(0 3 2 1)
		);
	}
);

edges
(
);

[Adamkat]

Dear Kirk,
The mesh you propose is much more elegant than mine, yet I don't understand why these empty faces pose a problem?
Also, if I take Floquation's advice I will have this kind of "empty face" (8 12 13 9) in the nozzle-chamber interface (see figure).

Could you please explain?
Thanks

BTW I found an awesome way to display the blocks and vertices using

paraFoam -block

PS I also attached your mesh suggestion for the convenience of the readers.

[kcjarvis56]

On the mesh I provided you could add the four point above (2 6 10 9 ) and make a new Hex for the nozzle.

Sent from my SM-N920V using CFD Online Forum mobile app

[kcjarvis56]

See how the hexs share points. There are ways to mesh the faces or extrude the faces however off the top of my head this is easier and doesn't require extra steps and in my opinion is a fundamental you should learn if plan on using openfoam.

Sent from my SM-N920V using CFD Online Forum mobile app

[kcjarvis56]

Look up mergePatchPairs in the user-guide. That might do it also if I remember right. You would define the two faces that you are connecting. In the blockMeshDict.

Sent from my SM-N920V using CFD Online Forum mobile app