[Tushar@cfd]

Well now,
Make the "p" BC zeroGradient instead of $calculated. Try to see if the result is coming..

[Ank]

I did the same..I changed calculated to zerogradient.

Tht error was from that only.

[Tushar@cfd]

If you wish then you can upload your complete case files here..

Like complete "/constant" directory with mesh.

[Ank]

Hey Tushar

I am not able to upload the mesh file. Can I send it to you by email or message?

[Tushar@cfd]

Give me your email-id. I will contact you.

[Ank]

ankursingh59@gmail.com

[Ank]

Hey

I modified the simpleFoam solver and added T equation in it. It is also showing me the same problem as it was with buoyantBoussinesqSimpleFoam. The velocity is increasing from inlet to outlet. It is going from 1 m/s to 1.1 m/s. I tried it on pitzDaily tutorial but result was almost same and velocity peaked midway to 10.99 m/s (should be 10 m/s) and then decreased. I am not able to get after adding T what is the problem it is having.

Any suggestions?

[fabian_roesler]

Hi Ank

you have a quite orthogonal mesh. So you could just switch the snGradScheme back to uncorrected and use this for the laplacian schemes as well. Moreover, for the epsilon, omega and R divSchemes you could use a linear interpolation scheme instead the diffusive first order upwind.
Have you tried a momentum predictor step or changed all upwind to linearUpwind schemes?

Best regards

Fabian

  ddtSchemes
  {
      default         Euler;
  }
   
  gradSchemes
  {
      default         leastSquares;
  }
   
  divSchemes
  {
      default         none;
      div(phi,U)      Gauss linearUpwindV grad(U);
      div(phi,T)      Gauss linearUpwind grad(T);
      div(phi,k)      Gauss linear;
      div(phi,epsilon) Gauss linear;
      div(phi,omega) Gauss linear;
      div(phi,R)      Gauss linear;
      div(R)          Gauss linear;
      div((nuEff*dev(T(grad(U))))) Gauss linear;
  }
   
  laplacianSchemes
  {
      default         none;
      laplacian(nuEff,U) Gauss linear uncorrected;
      laplacian(Dp,p_rgh) Gauss linear uncorrected;
      laplacian(kappaEff,T) Gauss linear uncorrected;
      laplacian(DkEff,k) Gauss linear uncorrected;
      laplacian(DepsilonEff,epsilon) Gauss linear uncorrected;
      laplacian(DepsilonEff,omega) Gauss linear uncorrected;
      laplacian(DomegaEff,omega) Gauss linear uncorrected;
      laplacian(DREff,R) Gauss linear uncorrected;
  }
   
  interpolationSchemes
  {
      default         linear;
  }
   
  snGradSchemes
  {
      default         uncorrected;
  }
   
  fluxRequired
  {
      default         yes;
      p_rgh              ;
  }

[fabian_roesler]

Hi Ank

one more question. You say you use a SIMPLE solver, no matter which exactly. But you have a ddtScheme in your fvSchemes dictionary. Do you have a kind of transient SIMPLE solver? Could it just be that your results did not jet converge for steady-state solution? If you want steady-state, try to increase your number of time steps.

Regards

Fabian

[Ank]

Hey Fabian

Thanks for your reply.

These suggestions are really good. But the problem was rather simple and has been solved. The increase in the velocity near the outlet was because velocity decreases near the wall along the length (boundary layer development). So to maintain a mass balance it increases near the centre of the outlet. And I am using steady state only, I don't have any transient SIMPLE solver. I have corrected that ddtScheme also to steady state.

Thanks and I will incorporate your suggestions also.

[Sherlock_1812]

Hi Ankur,

What changes did you finally make to the 0/p and 0/p_rgh directory?

[Ank]

Hey Srivathsan,

I am attaching my p and p_rgh files. It works well, you can have a look at it.


p file:


FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0;

boundaryField
{

inlet
{
type calculated;
value $internalField;


}
tube
{
type calculated;
value $internalField;
}

outlet
{
type calculated;
value $internalField;
}

wall
{
type calculated;
value $internalField;
}
fin
{
type calculated;
value $internalField;
}
symmetry
{
type symmetryPlane;
}

}


p_rgh file :

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 0;

boundaryField
{
inlet
{
type zeroGradient;
}

outlet
{
type fixedValue;
value uniform 0;
}

wall
{
type zeroGradient;
}
tube
{
type zeroGradient;
}
fin
{
type zeroGradient;
}
symmetry
{
type symmetryPlane;

}

}