[pss47]

Hi all,

I am performing steady state vehicle cabin simulations using buoyantSimpleFoam solver. The geometry is complex but I got pretty good mesh which has 3 nonOrthogonal Faces with Max nonOrthogonality = 73 degrees.


The boundary conditions are simple for now, Velocity and Temperature are specified at inlet. All walls are adiabatic.



The internal field is reaching the inlet temperature but still the 'h' residuals are almost constant throughout the simulation. I have attached the related images with the post. I don't know what is the reason for this issue. Any help is appreciated.

//Temperature 



dimensions      [0 0 0 1 0 0 0];

internalField   uniform 300;

boundaryField
{

    #includeEtc "caseDicts/setConstraintTypes"

    "Wall_.*"
    {
        type            zeroGradient;
    }

    "Inlet_.*"
    {
        type            fixedValue;
        value           uniform 280;
    }

    "Outlet_.*"
    {
        type            inletOutlet;
        inletValue      uniform 280;
        value           uniform 280;
    }

}

//Velocity

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

internalField   uniform (0 0 0);

boundaryField

{
#includeEtc "caseDicts/setConstraintTypes"
    "Wall_.*"
    {
        type         noSlip;
    }

    "Inlet_.*"
    {
        type            surfaceNormalFixedValue;
            refValue        uniform -2;

//        type                flowRateInletVelocity;
//            volumetricFlowRate  0.0035;
//            value               (0 0 0);

    }

    "Outlet_.*"
    {
        type            inletOutlet;
            inletValue      uniform (0 0 0);
            value           uniform (0 0 0);
    }
}

Temperature.png

Residuals.png

CaseFiles.zip

[pete20r2]

None of the other fields, except for maybe epsilon are converged either.
I think you need to keep running for more timesteps.
That being said, I think you need to converge the flow fields (U and p_rgh) (also the turbulent quantities) before you can trust the h field.
Depending on what result you are actually trying to quantify from this study, you can choose what level of convergence is acceptable when it becomes clear that the temperature field (at your sensor locations) looks to be stable.
In your T plot the temperatures are clearly still falling (visually), hence there is still a substantial residual.

[pss47]

Originally Posted by pete20r2

None of the other fields, except for maybe epsilon are converged either.
I think you need to keep running for more timesteps.
That being said, I think you need to converge the flow fields (U and p_rgh) (also the turbulent quantities) before you can trust the h field.
Depending on what result you are actually trying to quantify from this study, you can choose what level of convergence is acceptable when it becomes clear that the temperature field (at your sensor locations) looks to be stable.
In your T plot the temperatures are clearly still falling (visually), hence there is still a substantial residual.

Hello Peter,


I agree that the flow fields has not yet converged. But, what i don't understand is that why residuals of h field is almost constant even though the temperature is coverging to the required solution(It has to reach 280K according to the BC).



Thank you for your interest on the issue
Sudarshan

[pete20r2]

The convergence reported by the solver is for the entire field. Since your flow field is not converged there can be no certainty in where the h field is not converged. Constant residual just mean that there is the same difference between solution steps, the solver may still be working towards a converged solution. The difference may not be in the location you are sensing at so it is not showing up in your plot.
Depending on you problem, it is generally recommended to get flow field convergence below 1e-4 to 1e-6 to have consistent results.

[pss47]

Originally Posted by pete20r2

The convergence reported by the solver is for the entire field. Since your flow field is not converged there can be no certainty in where the h field is not converged. Constant residual just mean that there is the same difference between solution steps, the solver may still be working towards a converged solution. The difference may not be in the location you are sensing at so it is not showing up in your plot.
Depending on you problem, it is generally recommended to get flow field convergence below 1e-4 to 1e-6 to have consistent results.

The value of Temperature in the entire mesh is below 281 ( initial value being 300) when I check it in the paraview.

[pss47]

I have found the reason for the strange behavior. It is the combination of BC and computation of residuals in OpenFOAM.


According to this source, the errors for the residuals are normalized using the average of the computed variable. When the final solution is completely homogeneous throughout the domain, The mean value is approximately equal to the computed variable which keeps the residual constant.


I changed the boundary condition to get non uniform solution, the residuals started decreasing.

internalField   uniform 300;

boundaryField
{

    #includeEtc "caseDicts/setConstraintTypes"

    "Wall_.*"
    {
        type            zeroGradient;
    }

    "Wall_Floor_.*"
    {
        type            fixedValue;
        value           uniform 300;
    }

    "Inlet_.*"
    {
        type            fixedValue;
        value           uniform 280;
    }

    "Outlet_.*"
    {
        type            inletOutlet;
        inletValue      uniform 280;
        value           uniform 280;
    }

}

Residuals_new.png