CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Strange incorrect inlet behavior for reactingFoam (http://www.cfd-online.com/Forums/openfoam-solving/59472-strange-incorrect-inlet-behavior-reactingfoam.html)

mrangitschdowcom August 24, 2007 15:05

Hi all, I finally got back
 
Hi all,
I finally got back to using openFoam and ran into an old problem again, but I've found out more about it. I have a model with two inlets that doesn't seem to calculate the temperature correctly. The domain is a 'pipe in a pipe' with only a quarter of the system modeled (two symmetry planes). The inlet boundary condition on the inner pipe seems to work fine. All the species & temperature are advected downstream as one would expect. The other inlet (actually an annulus) does not. The species are advected correctly, but the temperature is not. In fact, it is not advected at all. The boundary nodes have the correct temperature values, but the downstream values do not change, even though all the species advect correctly. I haven't a clue as to what is going wrong. The boundary conditions are defined exactly the same for both inlets.

The grid for the model comes from gambit, if that has any impact on the system. It is quite orthogonal at the inlets, and most of the domain is a hex mesh.

Any help would be greatly appreciated!


Mike

msrinath80 August 24, 2007 15:13

Did checkMesh report any incon
 
Did checkMesh report any inconsistencies? Also if you're really confident that the Boundary conditions are in order, you could always run a much simpler test case (say a cube in a cube) with the mesh done using blockMesh to single out any GAMBIT related issues.

mrangitschdowcom August 24, 2007 15:44

checkMesh show OK's across the
 
checkMesh show OK's across the board. I used my chemkin file and modified boundary files for the example case (backward step) that comes with the reactingFoam files from the wiki. It seems to work correctly. What the backwards step doesn't have is the symmetry boundaries, but these seem to work. The problem is just in the temperature equation.

My temperature boundary condition file is below (the one that doesn't work is inlet_cycle):



inferno:0> more T
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.4.1 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format binary;

root "/home/u091108/OpenFOAM/u091108-1.4.1/run/tutorials/reactingFoam";
case "reactingTest";
instance "0";
local "";

class volScalarField;
object T;
}

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

dimensions [0 0 0 1 0 0 0];

internalField uniform 323.15;

boundaryField
{
wall
{
type zeroGradient;
}
cone
{
type zeroGradient;
}
hole
{
type zeroGradient;
}
finger_outer
{
type zeroGradient;
}
finger_end
{
type zeroGradient;
}
finger_inner
{
type zeroGradient;
}
inlet_oxygen
{
type fixedValue;
value uniform 293.15;
}
inlet_cycle
{
type fixedValue;
value uniform 383.15;
}
outlet
{
type zeroGradient;
}
symmetry2
{
type symmetryPlane;
}
symmetry1
{
type symmetryPlane;
}
}

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




Thanks much!

Mike

mrangitschdowcom August 27, 2007 16:03

Hi again all, Just checked
 
Hi again all,
Just checked what's going on using a different grid (the pitz daily grid supplied with the reactingFoam example). With the above temperature boundary condition file, the 383.15K flow (inlet_cycle) doesn't advect into the domain like it should. The temperature at the inlet plane is set correctly, but it is never convected downstream with the flow. The other variables are -- all species, k, epsilon... but not the temperature. Does anyone have an idea why this may be?

Thanks in advance

Mike

mrangitschdowcom August 29, 2007 15:55

Found the problem! It turne
 
Found the problem!

It turned out that there was a boundary condition problem, but one that I wouldn't have thought would have made a difference in the temperature equation. I had left out a species from my chemkin file, and the summation of my mole fractions of the other species didn't come to 1.0. Somehow this caused the temperature equation to go haywire. There is no consistency check in the startup for the mole fractions (I think).

Does openFOAM solve for all the species, or can you specify Nspecies-1 mole fractions and have it compute the other one by 1.0 - sum(Y1+Y2+Y3+...)?

Thanks for the help!


Mike


All times are GMT -4. The time now is 06:38.