CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

pisoFoam, fully developed pipe flow using cyclic BC's

Register Blogs Community New Posts Updated Threads Search

Like Tree2Likes
  • 2 Post By thijs1909

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   January 29, 2018, 08:44
Default pisoFoam, fully developed pipe flow using cyclic BC's
  #1
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Dear Foamers,

I would like to study the influence fully developed flow in tubes with a helix structure. I am particulary interested in the influence of the structure on the pressure drop. My Re=5300 and I am using kOmegaSST as a turbulence model.

I started three months ago using simpleFoam, cyclicAMI boundary conditions and fvOptions to specify the mass flow. I did not get good mesh independent solution for my tube with a helix structure so I went back to a simple tube using a structured mesh.

But instead of using simpleFoam I decided to use pisoFoam and solve in time. Again I wanted to using periodic boundary conditions to reduce my spatial domain. I noticed that both cyclic and cyclicAMI boundary conditions gave me severe osciliations for the pressure term. To overcome this problem I tried to using the mappedPatch boundary condition, mapping my outlet at z=0.01 to my inlet at z=0. So far I succesfully modelled hagen poiseuille flow, but now I turned on the turbulence and I do not know how to set the boundary conditions for k, omega and nut:

BC's I use for velocity U and pressure, which I know they are correct while they show the correct Hagen-poiseuille velocity profile:

HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 1);

boundaryField
{
    INLET
    {
        type            mapped;
        value           uniform (0 0 1);
        interpolationScheme cell;
        setAverage true;
        average (0 0 1);
    }

    WALL
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    OUTLET
    {
        type            zeroGradient;
    }
}
Pressure P:
HTML Code:
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;
    }

    WALL
    {
        type            zeroGradient;
    }

    OUTLET
    {
        type            fixedValue;
        value           uniform 0;
    }
}
turbulent kinetic energy:
HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0.0045;

boundaryField
{
    INLET
    {
        type            mapped;
        value uniform 0.0045;
interpolationScheme cell;
setAverage false;
average 0.0045;
       
    }
    OUTLET
    {
        type            zeroGradient;
    }
    WALL
    {
        type            fixedValue;
        value           uniform 0;
          }
    }
For omega:
HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 333.2391;

boundaryField
{
    OUTLET
    {
        type            zeroGradient;
       // inletValue      $internalField;
        //value           $internalField;
    }

    WALL
    {
        type            fixedValue;
        value           uniform 1.3441e+7;
    }

    INLET
    {
        type           mapped;
value uniform 333.2391;
interpolationScheme cell;
setAverage false;
average 333.2391;
     //   value           $internalField;
    }

   }
For nut:

HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    INLET
    {
        type            zeroGradient;
       
    }
    OUTLET
    {
        type            zeroGradient;

    }
    WALL
    {
       type            fixedValue;
       value           uniform 0;  
}
    
}
The geometry I use is a straight tube of Ø5,3mm and a length of 10mm.

I just basically do not know how to correctly set k, omega and nut. I only want to map the outlet conditions to my inlet. For velocity I specify an average bulk velocity of 1m/s.

Kind regards,

Thijs
ashrufsyed and randolph like this.
thijs1909 is offline   Reply With Quote

Old   January 29, 2018, 11:20
Default
  #2
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
or should I use directMappedPatch instead of mapped?
thijs1909 is offline   Reply With Quote

Old   January 29, 2018, 11:37
Default
  #3
gu1
Senior Member
 
Guilherme
Join Date: Apr 2017
Posts: 245
Rep Power: 10
gu1 is on a distinguished road
Quote:
Originally Posted by thijs1909 View Post
or should I use directMappedPatch instead of mapped?
What version of OpenFOAM?
Put your 'boundary' file so we can analyze.
In fact, I did not understand why z = 0.1? Could you explain ?!
gu1 is offline   Reply With Quote

Old   January 29, 2018, 11:41
Default
  #4
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Quote:
Originally Posted by gu1 View Post
What version of OpenFOAM?
Put your 'boundary' file so we can analyze.
In fact, I did not understand why z = 0.1? Could you explain ?!
Hi there,

What I mean with coordinate z is the offset I would like to map to my inlet. I use openFOAM 5.0 on bash ubuntu on windows.

My inlet plane is located at z = 0 and my outlet plane is located at z= 0.01

HTML Code:
/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       polyBoundaryMesh;
    location    "constant/polyMesh";
    object      boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

3
(
    INLET
    {
        type            mappedPatch;
        offset (0 0 0.01);
        sampleRegion region0;
        sampleMode nearestCell;
        samplePatch none;
        nFaces          1805;
        startFace       535895;
//neighbourPatch OUTLET;
//transform translational;
//separationVector (0 0 0.01);

    }
    WALL
    {
        type            wall;
        inGroups        1(wall);
        nFaces          7600;
        startFace       537700;
    }
    OUTLET
    {
        type            patch;
        nFaces          1805;
        startFace       545300;
//neighbourPatch INLET;
//transform translational;
//separationVector (0 0 -0.01);
    }
)
thijs1909 is offline   Reply With Quote

Old   January 29, 2018, 11:49
Default
  #5
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
I also found this old thread: simpleFoam + cyclic pipe = unstable?

But the proposed boundary conditions for 0/k 0/omega and 0/nut do not seem to work.

As I understand I start with an initial length of pipe. Then in the next time iteration the outlet is mapped to the inlet. For laminar the setup with 0/U and 0/p work while I find the hagen poiseuille velocity profile. My understanding is that in the next time iteration the k, omega and nut values should be mapped to my inlet, but how do I specify a value at the outlet I do not know how it will evolve?
thijs1909 is offline   Reply With Quote

Old   January 29, 2018, 13:50
Default
  #6
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Quote:
Originally Posted by gu1 View Post
What version of OpenFOAM?
Put your 'boundary' file so we can analyze.
In fact, I did not understand why z = 0.1? Could you explain ?!
I believe directMapped is not available in openFoam 5.0, so I will stick to mapped
thijs1909 is offline   Reply With Quote

Old   January 30, 2018, 00:51
Default
  #7
New Member
 
Yuncheng Xu (Cloud)
Join Date: May 2011
Location: State College, PA
Posts: 20
Rep Power: 15
luther1990 is on a distinguished road
Here are some problems on your BCs
  1. too big omega at wall 1.3441e+7??????
  2. nut is set as calculated at inlet
  3. Fix above, and go back to cyclic or cyclicAMI.
  4. make sure All the variables except for nut are set as cyclic at inlet and outlet
If cyclic gives problems, so will mapped.

Hope it can help you
luther1990 is offline   Reply With Quote

Old   January 30, 2018, 04:36
Default
  #8
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Quote:
Originally Posted by luther1990 View Post
Here are some problems on your BCs
  1. too big omega at wall 1.3441e+7??????
  2. nut is set as calculated at inlet
  3. Fix above, and go back to cyclic or cyclicAMI.
  4. make sure All the variables except for nut are set as cyclic at inlet and outlet
If cyclic gives problems, so will mapped.

Hope it can help you
I tried cyclic with laminar and I find severe oscillations for my pressure.



For my nut value at the wall, I used this formula by Menter:
"Standard" Menter SST Two-Equation Model (SST)
https://turbmodels.larc.nasa.gov/sst.html

Omega_wall = 10 *( (6 *nu)/(B1 *yplus^2))

my viscosity nu = 1.0034e-06 m^2/s
B1 is a model constant = 0.075
I created a boundary layer with a y+ =~ 1 so my first cell height is 7,36e-06meter
thijs1909 is offline   Reply With Quote

Old   January 30, 2018, 04:43
Default
  #9
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Quote:
Originally Posted by luther1990 View Post
Here are some problems on your BCs
  1. too big omega at wall 1.3441e+7??????
  2. nut is set as calculated at inlet
  3. Fix above, and go back to cyclic or cyclicAMI.
  4. make sure All the variables except for nut are set as cyclic at inlet and outlet
If cyclic gives problems, so will mapped.

Hope it can help you
I tried cyclic with laminar and I find severe oscillations for my pressure.

[IMG]<a href="https://ibb.co/b1hoW6"><img src="https://preview.ibb.co/iTEfdm/piso_no_conv.jpg" alt="piso_no_conv" border="0"></a>[/IMG]

For my nut value at the wall, I used this formula by Menter:

Omega_wall = 10 *( (6 *nu)/(B1 *yplus^2))

my viscosity nu = 1.0034e-06 m^2/s
B1 is a model constant = 0.075
I created a boundary layer with a y+ =~ 1 so my first cell height is 7,36e-06meter
thijs1909 is offline   Reply With Quote

Old   January 30, 2018, 08:15
Default
  #10
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Quote:
Originally Posted by thijs1909 View Post
I tried cyclic with laminar and I find severe oscillations for my pressure.



Apparently the laminar case converge to the right solution even with the fluctuations in the pressure residual. The calculated dp/dx source term slowly converges to the analytic solution. The required analytic value for my case is: 0.2286 and I found 0.231091 after 1.024 seconds, but I suspect it will converge better to the analytic value with a finer mesh or a longer runtime, so that is what I will try now.
thijs1909 is offline   Reply With Quote

Old   February 5, 2018, 09:28
Default
  #11
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
pisoFoam for the laminar case converges to the correct pressure gradient for a pipe of Ø5,3mm using cyclic bc's. However when I turn on RANS kOmegaSST I get a velocity profile which has the correct shape, but maybe the wrong max. velocity, and I do not get a correct pressure gradient. I can calculated the pressure gradient with the moody diagram and the correct is: dp/dx=3.5 If I read the moody-diagram for a Re=5282 the friction coefficient Fd should be approx. 0.037. This is also the friction coefficient is used in my calculation of the first layer height, using the blasius fanning coefficient : f= 0.0791/(Re^0.25) and Fd = 4*f

My dp/dx is 4.37 which differs too much.

So I expect my boundary conditions for the turbulence are not correct. I use a lowRe with a y+ = 1.

k
HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      k;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0.0045;

boundaryField
{
    INLET
    {
        type             cyclicAMI;
       
       
    }
    OUTLET
    {
        type            cyclicAMI;
    }
    WALL
    {
        type            fixedValue;
        value           uniform 0;
          }
    }
omega
HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      omega;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 333.2391;

boundaryField
{
    INLET
    {
       type             cyclicAMI;
    }

    WALL
    {
        type            fixedValue;
        value           uniform 1.3441e+7;
    }

    OUTLET
    {
        type           cyclicAMI;
    
    }

   }
nut

HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    location    "0";
    object      nut;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions      [0 2 -1 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    INLET
    {
        type            cyclicAMI;

       
    }
    OUTLET
    {
        type            cyclicAMI;

    }
    WALL
    {
       type            fixedValue;
       value           uniform 0;  
}
    
}
p
HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volScalarField;
    object      p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform 0;

boundaryField
{
    INLET
    {
        type            cyclicAMI;
    }

    WALL
    {
        type            zeroGradient;
    }

    OUTLET
    {
        type            cyclicAMI;
    }
}
U
HTML Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       volVectorField;
    object      U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField   uniform (0 0 1);

boundaryField
{
    INLET
    {
        type            cyclicAMI;
        
    }

    WALL
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }

    OUTLET
    {
        type            cyclicAMI;
    }

I also tried using a lowRe wallfunction for nut --> nutLowReWallFunction but I did not give a better result. The dp/dx remained 4.37

The pressure gradient according to moody can be calculated as:

delta P = Fd*{(rho*Vavg^2*L)/(2*D)} such that the pressure gradient is calculated as: deltaP/(rho*L) =dp/dx= (Fd *Vavg^2 )/ (2*D)

Does someone has a better suggestion? I found this validation case online: https://www.simscale.com/docs/conten...tPipeFlow.html but could not figure out how they set the boundary condition for nut
thijs1909 is offline   Reply With Quote

Old   February 5, 2018, 10:22
Default
  #12
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Could aspect ratio be the problem. I have a y+ = 1 so my first cell layer height is 7,36e-6meter. My spacing in axial direction (z-direction) is 1e-4. But then again why I do checkMesh, openFoam tells everything is OK!

HTML Code:
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  5.x                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 5.x-197d9d3bf20a
Exec   : checkMesh
Date   : Feb 05 2018
Time   : 15:22:03
Host   : "LAPTOP-38GBMABK"
PID    : 5239
I/O    : uncollated
Case   : /mnt/c/Users/thijs/Documents/openFoam_cases/restart/struct_piso/turb/tsu6_res/piso_struct_lvl_1_cyclicAMI
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster (fileModificationSkew 10)
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create polyMesh for time = 0

Time = 0

Mesh stats
    points:           186244
    faces:            547105
    internal faces:   535895
    cells:            180500
    faces per cell:   6
    boundary patches: 3
    point zones:      0
    face zones:       0
    cell zones:       0

Overall number of cells of each type:
    hexahedra:     180500
    prisms:        0
    wedges:        0
    pyramids:      0
    tet wedges:    0
    tetrahedra:    0
    polyhedra:     0

Checking topology...
    Boundary definition OK.
    Cell to face addressing OK.
    Point usage OK.
    Upper triangular ordering OK.
    Face vertices OK.
    Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces...
    Patch               Faces    Points   Surface topology                  
    INLET               1805     1844     ok (non-closed singly connected)  
    WALL                7600     7676     ok (non-closed singly connected)  
    OUTLET              1805     1844     ok (non-closed singly connected)  

Checking geometry...
    Overall domain bounding box (-0.00265 -0.00265 0.01) (0.00265 0.00265001 0.02)
    Mesh has 3 geometric (non-empty/wedge) directions (1 1 1)
    Mesh has 3 solution (non-empty) directions (1 1 1)
    Boundary openness (1.45266e-17 -4.96472e-17 2.58155e-16) OK.
    Max cell openness = 7.75827e-16 OK.
    Max aspect ratio = 15.3833 OK.
    Minimum face area = 6.50758e-10. Maximum face area = 3.38236e-08.  Face area magnitudes OK.
    Min volume = 1.41389e-13. Max volume = 3.38236e-12.  Total volume = 2.20368e-07.  Cell volumes OK.
    Mesh non-orthogonality Max: 7.36316 average: 2.0249
    Non-orthogonality check OK.
    Face pyramids OK.
    Max skewness = 0.358788 OK.
    Coupled point location match (average 0) OK.

Mesh OK.

End
thijs1909 is offline   Reply With Quote

Old   February 5, 2018, 13:04
Default
  #13
New Member
 
Yuncheng Xu (Cloud)
Join Date: May 2011
Location: State College, PA
Posts: 20
Rep Power: 15
luther1990 is on a distinguished road
Just a few suggestions. You need to use wall functions for k and omega too. They do matter. Don’t need to use lowRe for nut. Try spalding or normal wall function for nut. Y+ should be fine, but it will be better to put it in log law sublayer.
luther1990 is offline   Reply With Quote

Old   February 6, 2018, 09:38
Default
  #14
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
Quote:
Originally Posted by luther1990 View Post
Just a few suggestions. You need to use wall functions for k and omega too. They do matter. Don’t need to use lowRe for nut. Try spalding or normal wall function for nut. Y+ should be fine, but it will be better to put it in log law sublayer.
I replaced my y+ = 1 mesh LowRe with a y+ =35 highRe mesh. And used the following wall functions:

k:
type kqRWallFunction;
value uniform 1e-12;

omega:
type omegaWallFunction;
value uniform 100;

nut:
type nutkWallFunction;
value uniform 0;

and my calculate dp/dx term by openFoam reduced to: 3.62 , which is way more close to the analytic solution of 3.5 from the moody diagram. However I observe the following problem for my velocity profile. I do not see noSlip condition at the wall. It says approx. 0,6m/s

Is this the consequence of using wallfunctions or am I doing something wrong?

Kind regards,

Thijs
thijs1909 is offline   Reply With Quote

Old   February 6, 2018, 11:18
Default
  #15
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
The velocity profile I obtaine :S

thijs1909 is offline   Reply With Quote

Old   February 6, 2018, 14:36
Default
  #16
New Member
 
Yuncheng Xu (Cloud)
Join Date: May 2011
Location: State College, PA
Posts: 20
Rep Power: 15
luther1990 is on a distinguished road
Quote:
Originally Posted by thijs1909 View Post
The velocity profile I obtaine :S


Hi Thijs,

I am not sure what caused the ‘no-slip’, but you may check the U value at wall boundary in the latest time directory. See if it is uniform fixed value of (0 0 0). In my experience and based on the codes, these wall functions won’t change velocity on the boundaries. It may be caused by interpolation issue in visualization. Why not try paraview to visualize?
luther1990 is offline   Reply With Quote

Old   February 13, 2018, 04:13
Default
  #17
New Member
 
Thijs
Join Date: Nov 2017
Posts: 29
Rep Power: 9
thijs1909 is on a distinguished road
I have a question regarding grid refinement and the y+ value. Currently I am using a y+ =~ 1 and during grid refinement of h=sqrt(2) in all direction I am also refining y+ such that I get a smaller y+=~0.707 .

But is this the correct procedure in order to study mesh independence. While I observe that my dp/dx term grows with smaller y+ value. And when I was taking my y+ value constant during refinement (y+ =~1) I observed better mesh independence.

Kind regards,

Thijs
thijs1909 is offline   Reply With Quote

Old   February 21, 2018, 23:07
Default
  #18
New Member
 
Yuncheng Xu (Cloud)
Join Date: May 2011
Location: State College, PA
Posts: 20
Rep Power: 15
luther1990 is on a distinguished road
Quote:
Originally Posted by thijs1909 View Post
I have a question regarding grid refinement and the y+ value. Currently I am using a y+ =~ 1 and during grid refinement of h=sqrt(2) in all direction I am also refining y+ such that I get a smaller y+=~0.707 .



But is this the correct procedure in order to study mesh independence. While I observe that my dp/dx term grows with smaller y+ value. And when I was taking my y+ value constant during refinement (y+ =~1) I observed better mesh independence.



Kind regards,



Thijs


Basically, pressure gradient is due to wall shear stress, which is very sensitive to the first grid height or y+. So your observation makes sense to me.

If you do care about pressure gradient, y+ shall be a very important variable in the grid dependence analysis.
luther1990 is offline   Reply With Quote

Reply


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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
fully developed region in pipe akbar.mech FLUENT 2 August 30, 2016 04:08
3D pipe flow - Using UDF's to define fully developed turbulent flow on the inlet Taz-CFD CFD Freelancers 1 February 21, 2016 12:12
UDF for 3D turbulent fully developed flow howhs Fluent UDF and Scheme Programming 0 August 1, 2013 12:47
Fully Developed Flow at an Inlet Ed Mueller CFX 5 January 13, 2009 12:50
2D representation of pipe for fully developed flow Nathan FLUENT 3 November 22, 2008 11:01


All times are GMT -4. The time now is 17:31.