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

Turbulent flow in a rectangular duct foam vs fluent

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 29, 2006, 20:26
Default I am simulating a turbulent fl
  #1
atzaru
Guest
 
Posts: n/a
I am simulating a turbulent flow in a square duct (0.2*0.2*6) in foam and fluent. I am concern about the velocity distribution difference between the two programs.

Reynolds number around 11 000.
in fluent i obtain a max velocity around 1.24 while in Foam the max velocity is 1.14. Does anybody know why and how i can correct this?

in both programs i introduced the same inlet (velocity, V=1m/s), the same initial k and epsilon, and outlet condition.


turb_flow_v2.tar.gz


ddtSchemes
{
default steadyState;
}

gradSchemes
{
default Gauss linear;
grad(p) Gauss linear;
grad(U) Gauss linear;
}

divSchemes
{
default Gauss <>;
div(phi,U) Gauss upwind;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,R) Gauss upwind;
div(R) Gauss linear;
div(phi,nuTilda) Gauss upwind;
div((nuEff*dev(grad(U).T()))) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(nuEff,U) Gauss linear corrected;
laplacian(1|A(U),p) Gauss linear corrected;
laplacian(DkEff,k) Gauss linear corrected;
laplacian(DepsilonEff,epsilon) Gauss linear corrected;
laplacian(DREff,R) Gauss linear corrected;
laplacian(DnuTildaEff,nuTilda) Gauss linear corrected;
}

interpolationSchemes
{
default linear;
interpolate(U) linear;
}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}


The boudary condition are:
(
wall
{
type wall;
physicalType wall;
startFace 97040;
nFaces 6720;
}

outlet
{
type patch;
physicalType pressureOutlet;
startFace 103760;
nFaces 400;
}

inlet
{
type patch;
physicalType inlet;
startFace 104160;
nFaces 400;
}

)
  Reply With Quote

Old   January 30, 2006, 08:25
Default What does the experimental dat
  #2
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
What does the experimental data say?

From what information you provided I would guess the source of inconsistency is either the turbulence model or the wall function. Please post which turbulence models and wall options you used for Fluent and Foam. Also, what is your y+ value.
eugene is offline   Reply With Quote

Old   February 2, 2006, 11:51
Default hello thanks for your reply
  #3
atzaru
Guest
 
Posts: n/a
hello

thanks for your reply

1 - in both programs Foam and Fluent I used the basic k-epsilon equations

2 the standard wall functions based on launder and spalding is used in both cases (the same Constants E =9.0 and kappa=0.4187)

3 The same k-eps coeff have been used cmu=0.009, c1=1.44, c2=1.92. I do not know why in Foam we do not have Tke=1 and TDR=1.3 but a coeff alphaEps = 0.7692. What is this coeff?

4 The y+ is 24

5 For the moment i do not have experimental data to compare with.

It is strange i obtain so different results.
  Reply With Quote

Old   February 2, 2006, 12:08
Default If you are using log the law o
  #4
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
If you are using log the law of the wall it is not valid at y+ = 24. My best guess is that fluent does something clever to improve at these intermediate values.

For Foam y+ needs to be around 100 with the standard k-epsilon model.
eugene is offline   Reply With Quote

Old   February 2, 2006, 14:28
Default FLUENT has different requireme
  #5
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
FLUENT has different requirements for its wall functions, according to its manual (30 < y+ < 60).

Also, in the OpenFOAM case files there is an error: in the 0\k dictionary the condition at the wall should be

wall
{
type zeroGradient;
}

instead of

wall
{
type fixedValue;
value uniform 0;
}

However it's strange that OpenFOAM 1.2 starts the calculation because it should quit and tell you the error.

Best regards,
Alberto
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   February 3, 2006, 06:01
Default Unfortunately/fortunately that
  #6
Senior Member
 
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 12
eugene is on a distinguished road
Unfortunately/fortunately that is one of the features of OpenFOAM. It allows you complete freedom in choosing individual boundary conditions, but at the same time, it wont tell you if you make an unwise choice.
eugene is offline   Reply With Quote

Old   February 3, 2006, 11:04
Default Sorry, I wasn't clear. I disco
  #7
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Sorry, I wasn't clear. I discovered the error because trying to run the case with a grid I did, OpenFOAM 1.2 told me the problem in the BC ;-)

Regards,
Alberto
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   February 13, 2007, 15:42
Default Well... So the problem was jus
  #8
New Member
 
Cesar Belaunde Zarate
Join Date: Mar 2009
Location: Quillota, V region, Chile
Posts: 8
Rep Power: 8
cesarbz is on a distinguished road
Well... So the problem was just de grid ? it's the same mesh for both programs?

Another questions...

What is the BC ?
And what represent de y+ value ?

thanks.
cesarbz 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
Turbulent Flow in a Square Duct using LES Hock Ming FLUENT 0 February 7, 2009 21:25
Turbulence flow in a rectangular duct Watchapon Main CFD Forum 0 April 7, 2007 07:34
Turbulence Model for Rectangular Duct Flow ken FLUENT 4 May 26, 2005 20:39
3D rectangular duct flow UDF - urgnet Yogesh FLUENT 0 March 27, 2005 01:36
laminar viscous flow in a rectangular duct Bastian FLUENT 0 July 2, 2004 08:51


All times are GMT -4. The time now is 13:08.