CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

forced convection of air inside a heated rectangular channel

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 6, 2013, 02:59
Default
  #21
Senior Member
 
Tushar Chourushi
Join Date: Jul 2009
Location: IIT-Indore, India
Posts: 318
Blog Entries: 1
Rep Power: 8
Tushar@cfd is on a distinguished road
Well now,
Make the "p" BC zeroGradient instead of $calculated. Try to see if the result is coming..
Tushar@cfd is offline   Reply With Quote

Old   June 6, 2013, 03:01
Default
  #22
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
I did the same..I changed calculated to zerogradient.

Tht error was from that only.
Ank is offline   Reply With Quote

Old   June 6, 2013, 04:03
Default
  #23
Senior Member
 
Tushar Chourushi
Join Date: Jul 2009
Location: IIT-Indore, India
Posts: 318
Blog Entries: 1
Rep Power: 8
Tushar@cfd is on a distinguished road
If you wish then you can upload your complete case files here..

Like complete "/constant" directory with mesh.
Tushar@cfd is offline   Reply With Quote

Old   June 6, 2013, 04:20
Default
  #24
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
Hey Tushar

I am not able to upload the mesh file. Can I send it to you by email or message?
Attached Files
File Type: zip test.zip (9.0 KB, 5 views)
File Type: zip constant1.zip (1.8 KB, 3 views)
Ank is offline   Reply With Quote

Old   June 6, 2013, 04:30
Default
  #25
Senior Member
 
Tushar Chourushi
Join Date: Jul 2009
Location: IIT-Indore, India
Posts: 318
Blog Entries: 1
Rep Power: 8
Tushar@cfd is on a distinguished road
Give me your email-id. I will contact you.
Tushar@cfd is offline   Reply With Quote

Old   June 6, 2013, 04:34
Default
  #26
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
ankursingh59@gmail.com
Ank is offline   Reply With Quote

Old   June 8, 2013, 06:45
Default
  #27
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
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?
Ank is offline   Reply With Quote

Old   June 11, 2013, 08:36
Default
  #28
Senior Member
 
fabian_roesler's Avatar
 
Fabian Roesler
Join Date: Mar 2009
Location: Bad Friedrichshall, Germany
Posts: 154
Rep Power: 8
fabian_roesler is on a distinguished road
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


Code:
  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 is offline   Reply With Quote

Old   June 11, 2013, 08:43
Default Transient Simple?
  #29
Senior Member
 
fabian_roesler's Avatar
 
Fabian Roesler
Join Date: Mar 2009
Location: Bad Friedrichshall, Germany
Posts: 154
Rep Power: 8
fabian_roesler is on a distinguished road
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
fabian_roesler is offline   Reply With Quote

Old   June 11, 2013, 08:46
Default
  #30
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
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.
Ank is offline   Reply With Quote

Old   September 25, 2013, 01:30
Default
  #31
Senior Member
 
Srivathsan N
Join Date: Jan 2013
Location: India
Posts: 101
Rep Power: 4
Sherlock_1812 is on a distinguished road
Hi Ankur,

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

Srivaths
Sherlock_1812 is offline   Reply With Quote

Old   September 25, 2013, 06:41
Default
  #32
Ank
Member
 
ankur
Join Date: May 2012
Location: India
Posts: 50
Rep Power: 5
Ank is on a distinguished road
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;

}

}
Ank is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
air bubble is disappear increasing time using vof xujjun CFX 9 June 9, 2009 07:59
Creating a grid for a channel inside a brick sanin FLUENT 0 November 6, 2008 09:03
how to estimage air speed with natural convection? Pei-Ying Hsieh Main CFD Forum 2 May 1, 2008 15:29
Modelling the Heat flow inside the curing oven Marios Vlad CFX 1 February 6, 2008 08:11
CFX-5.5 simulating air free convection Dustin Lee CFX 0 April 16, 2003 02:54


All times are GMT -4. The time now is 03:12.