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

interpolation for pressure

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

Like Tree42Likes

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 7, 2011, 09:27
Default
  #21
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 256
Blog Entries: 1
Rep Power: 19
makaveli_lcf is on a distinguished road
Send a message via ICQ to makaveli_lcf
Thank you Alberto, I also found it and now trying to understand this expression.
Please see attached file Volumefield_reconstruction.pdf. I am looking for the original reference where this formulation is established. Could you please give some tips?
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

http://smmp.unileoben.ac.at
makaveli_lcf is offline   Reply With Quote

Old   September 7, 2011, 22:16
Default
  #22
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,912
Rep Power: 36
alberto will become famous soon enoughalberto will become famous soon enough
I do not have a reference for this, but I think you got it.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats (current status: http://albertopassalacqua.com/?p=1541)
OpenQBMM - An open-source implementation of quadrature-based moment methods.

To obtain more accurate answers, please specify the version of OpenFOAM you are using.
alberto is offline   Reply With Quote

Old   September 8, 2011, 04:37
Default
  #23
Senior Member
 
akidess's Avatar
 
Anton Kidess
Join Date: May 2009
Location: Germany
Posts: 1,377
Rep Power: 30
akidess will become famous soon enough
Alexander, I think it would be nice to have this on the wiki. If you agree, do you have the time to copy it to an article there?
akidess is offline   Reply With Quote

Old   September 8, 2011, 04:39
Default
  #24
Senior Member
 
Dr. Alexander Vakhrushev
Join Date: Mar 2009
Posts: 256
Blog Entries: 1
Rep Power: 19
makaveli_lcf is on a distinguished road
Send a message via ICQ to makaveli_lcf
Hi Anton!

Ok, I will put it there. And if Alberto doesn't mind, it would look better with his description of the body forces and the pressure gradient treatment technique.
__________________
Best regards,

Dr. Alexander VAKHRUSHEV

Christian Doppler Laboratory for "Metallurgical Applications of Magnetohydrodynamics"

Simulation and Modelling of Metallurgical Processes
Department of Metallurgy
University of Leoben

http://smmp.unileoben.ac.at

Last edited by makaveli_lcf; September 8, 2011 at 04:43. Reason: Additions
makaveli_lcf is offline   Reply With Quote

Old   September 13, 2011, 02:20
Default
  #25
Senior Member
 
santiagomarquezd's Avatar
 
Santiago Marquez Damian
Join Date: Aug 2009
Location: Santa Fe, Santa Fe, Argentina
Posts: 452
Rep Power: 24
santiagomarquezd will become famous soon enough
Alexander,

Quote:
Originally Posted by makaveli_lcf View Post
Thank you Alberto, I also found it and now trying to understand this expression.
Please see attached file Attachment 9124. I am looking for the original reference where this formulation is established. Could you please give some tips?
we were chatting about fvc::reconstruct() with Alberto few months ago and I took similar notes of the method, writing out the algorithm in mathematical form. I was looking for a "continuum form" of this operator, I think it's based in a generalized form of Gauss Theorem [like (3.9) to (3.16) in Hrv. thesis] due to a surface defined field is transformed in cell defined one, but I couldn't hack it, maybe these ideas could help you to find the basis.

Regards.
__________________
Santiago MÁRQUEZ DAMIÁN, Ph.D.
Research Scientist
Research Center for Computational Methods (CIMEC) - CONICET/UNL
Tel: 54-342-4511594 Int. 7032
Colectora Ruta Nac. 168 / Paraje El Pozo
(3000) Santa Fe - Argentina.
http://www.cimec.org.ar
santiagomarquezd is offline   Reply With Quote

Old   July 26, 2012, 05:28
Default Could you be so kind to write down the corresponding code for the equation for p?
  #26
New Member
 
Join Date: Nov 2010
Posts: 2
Rep Power: 0
vgalindo is on a distinguished road
Dear Alberto,

thank you very much for this very detailed explanation about the issue how to add correctly a body force to the (incompressible) momentum equation!
I would be grateful if you would still specify the corresponding code for the p equation.

Best regards, Vladimir


Quote:
Originally Posted by alberto View Post
I will try to give you the basic idea in the case of a generic body force term F, so that your momentum equation reads:

(1) ddt(U) + div(UU) = div(tau) - grad(p)/rho + F

This equation can be written in semi-discrete form as:

(2) A*U = H - grad(p)/rho + F

where the pressure gradient and the force term we want to include in the momentum interpolation is left explicitly out at this point. In other words, only the first three terms (time derivative, unsteady, divergence of the stress tensor) of Eq. 1 are used to define A and H. For example, in an incompressible code, this could read (it might be different, depending on the solver):

Code:
     fvm::ddt(U)
  + fvm::div(phi, U)
  + turbulence->divDevReff(U)
Normally the pressure gradient would be treated directly as a source term in an incompressible code (see pisoFoam for example). Here we assume we want to treat it with the "improved approach".

From Eq. 2, interpolating on faces and dotting with the surface area vector S the pressure gradient and the force term, we have:

- snGrad(p)*|S|/rho + F_f . S

where F_f is F interpolated on faces. This in OF corresponds to:

Code:
- fvc::snGrad(p)*mesh.magSf()/rhoa + fvc::interpolate(F) & mesh.Sf()
This term can be used as argument of fvc::reconstruct() to add the contribution of the pressure gradient and of the force term to the momentum predictor:

Code:
solve
(
      UEqn == fvc::reconstruct
      (
          - fvc::snGrad(p)*mesh.magSf()/rhoa 
          + fvc::interpolate(F) & mesh.Sf()
   )
)
Then OpenFOAM re-computes U as

U = H/A

where A is updated with the predicted value of U. However, keep in mind that H does not directly include the effect of grad(p) and F.

From Eq. 2 we can derive the flux to construct the pressure equation:

phi = (H/A)_f . S - (1/A)_f * snGrad(p) |S|/rho + (1/A)_f*F_f . S

and imposing div(phi) = 0, you obtain the pressure equation, which will include for the first time all the effects.

The flux is then corrected based on the solution of the pressure equation, and the velocity correction is reconstructed from the flux. Only at this point U will "see" the effect of p and F.

If you take a look at VOF solvers (i.e. interFoam), you will notice that the code does not solve for p, but for p_rgh = p + rho*gh. This is another way to treat the gravity to address the weakness of the Rhie-Chow interpolation, but the idea is similar.

I hope this helps, but please let us know if you have more questions

Best,
vgalindo is offline   Reply With Quote

Old   July 29, 2012, 16:20
Default
  #27
Member
 
Norbert Weber
Join Date: May 2012
Location: Dresden, Germany
Posts: 37
Rep Power: 14
dl6tud is on a distinguished road
Hallo Vladimir,

I don't understand everything yet, but based on interFoam it should be sth like that:
Quote:
ScalarField rUA = 1.0/UEqn.A();
surfaceScalarField rUAf = fvc::interpolate(rUA);

U = rUA * UEqn.H();

surfaceScalarField phi = fvc::interpolate(U) & mesh.Sf();
surfaceScalarField Ff = fvc::interpolate(F) & mesh.Sf();

[...]

fvScalarMatrix pEqn
(
fvm::div(rUAf*fvm::snGrad(p)*mesh.magSf()/rho) == fvc::div(phi)
+ fvc::div(rUAf*Ff);
);


[...]

U += rUA*fvc::reconstruct(Ff/rUAf);
I am not sure how to transform div.(snGrad), but probably we have to use:

Quote:
fvScalarMatrix pEqn
(
fvm::laplacian(rUAf,p*mesh.magSf()/rho
) == fvc::div(phi) + fvc::div(rUAf*Ff) ;
);
In interFoam the velocity is corrected only for the force. But they put phi and Ff together (and name it phi) -> I am not sure why.
Working on pisoFoam, I think rho has to be removed. I do not know if phi has to contain only the velocity flux, or the 'force flux', too. Any idea?

For my understanding: Can someone give me a hint, what 'reconstruct' does? It 'adds' terms to the equation and changes A and H? But there must be a difference between

Quote:
solve ( UEqn == fvc::reconstruct ( - fvc::snGrad(p)*mesh.magSf()/rhoa + fvc::interpolate(F) & mesh.Sf() ) )
and
Quote:
solve ( UEqn == - fvc::snGrad(p)*mesh.magSf()/rhoa + fvc::interpolate(F) & mesh.Sf() )
dl6tud is offline   Reply With Quote

Old   July 30, 2012, 02:33
Default plz help me
  #28
Member
 
vahid
Join Date: Feb 2012
Location: Mashhad-Iran
Posts: 80
Rep Power: 13
vahid.najafi is an unknown quantity at this point
Hi Dear alberto again:
I want to add surface tension(sigma) in one solver,for this reason I added :
#include ''fvCFD.H''
fvc::interpolate(interface.sigma())

in this code:
Foam::tmp<Foam::volScalarField>
Foam:haseChangeTwoPhaseMixtures::SchnerrSauer: Coeff
(
const volScalarField& p
) const
{
volScalarField limitedAlpha1(min(max(alpha1_, scalar(0)), scalar(1)));
volScalarField rho
(
limitedAlpha1*rho1() + (scalar(1) - limitedAlpha1)*rho2()
);
return

//......I want to change it( <<sigma>> surface tension multiple in it):
(3*rho1()*rho2())*sqrt(2/(3*rho1()))*(fvc::interpolate(interface.sigma()))
*rRb(limitedAlpha1)/(rho*sqrt(mag(p - pSat()) + 0.01*pSat()));
//.................................................. ......
}
dont successful wmake, and seen(was not declared ):
phaseChangeTwoPhaseMixtures/SchnerrSauer/SchnerrSauer.C:113: error: 'interface' was not declared in this scope
make: *** [Make/linux64GccDPOpt/SchnerrSauer.o] Error 1
please help me,and tell me ,How to correct this problem???

vahid.najafi is offline   Reply With Quote

Old   June 4, 2014, 11:51
Default
  #29
Senior Member
 
M. Montero
Join Date: Mar 2009
Location: Madrid
Posts: 155
Rep Power: 17
be_inspired is on a distinguished road
HI all,

How could it be done in case it is not a body force but a vectorField?

All is in relation to the rotorDiskSource and how introducing this source in the momentum equation can create wiggles in the pressure field and velocity field.

Thank you

Last edited by be_inspired; June 6, 2014 at 08:14.
be_inspired is offline   Reply With Quote

Old   February 23, 2015, 10:16
Default
  #30
New Member
 
Peter
Join Date: May 2012
Location: New York
Posts: 18
Rep Power: 14
chinaduck is on a distinguished road
Quote:
Originally Posted by harry View Post
Does Openfoam implement body-force-weighted scheme for pressure interpolation?

Hello Harry,
Did you finally solve your problem? I have met a similar problem regarding the body-force-weighted scheme for pressure interpolation.
Do you have any ideas on this? Thanks a lot for your help and time!

Best,

Peter
chinaduck is offline   Reply With Quote

Old   May 12, 2017, 10:26
Default
  #31
New Member
 
Roman G.
Join Date: Apr 2017
Posts: 16
Rep Power: 9
Novel is on a distinguished road
Hi,
I know this treat is old but I'm struggling with the implementation of the force term by the use of the Rhi-Chow interpolation. I'm using pimpleFoam.

So far I added in the momentum predictor my force term like this:

Code:
surfaceScalarField B_fs = fvc::interpolate(lorentz/rho) & mesh.Sf()

if (pimple.momentumPredictor())
{
   solve
   (
      UEqn   
      ==
      fvc::reconstruct
      (   
         - fvc::snGrad(p)* mesh.magSf()
         + B_fs    
      )
    );
    fvOptions.correct(U);
}
In pEqn.H

I added a flux term in the phiHbyA equation:

Code:
surfaceScalarField rAUf("rAUf", fvc::interpolate(rAU));
surfaceScalarField phil(rAUf*B_fs);

surfaceScalarField phiHbyA
(
    "phiHbyA",
    fvc::flux(HbyA)
  + fvc::interpolate(rAU)*fvc::ddtCorr(U, phi)
  + phil
);
and at the end I correct the momentum source with the pressure gradient flux:

Code:
U = HbyA + rAU*fvc::reconstruct((phil - pEqn.flux())/rAUf);
But when I run the solver I get an continuity error:
Code:
Continuity error cannot be removed by adjusting the outflow.
Please check the velocity boundary conditions and/or run potentialFoam to initialise the outflow.
Total flux              : 8.226416123979263e-05
Specified mass inflow   : 0.0005613679754126387
Specified mass outflow  : 6.154738583391114e-17
Adjustable mass outflow : 0
What do I miss here?

Thanks in advance
Novel is offline   Reply With Quote

Old   May 18, 2017, 06:15
Default
  #32
New Member
 
Roman G.
Join Date: Apr 2017
Posts: 16
Rep Power: 9
Novel is on a distinguished road
The problem is solved. I had to add the flux from the force after adjusting phi.

Code:
surfaceScalarField phil(rAUf*B_fs);
surfaceScalarField phiHbyA
(
    "phiHbyA",
    fvc::flux(HbyA)
  + fvc::interpolate(rAU)*fvc::ddtCorr(U, phi)
);

MRF.makeRelative(phiHbyA);

adjustPhi(phiHbyA, U, p);

phiHbyA += phil;
Novel is offline   Reply With Quote

Old   September 19, 2017, 05:42
Default
  #33
Senior Member
 
Przemek
Join Date: Jun 2011
Posts: 249
Rep Power: 16
gaza is on a distinguished road
Quote:
Originally Posted by Novel View Post
The problem is solved. I had to add the flux from the force after adjusting phi.

Code:
surfaceScalarField phil(rAUf*B_fs);
surfaceScalarField phiHbyA
(
    "phiHbyA",
    fvc::flux(HbyA)
  + fvc::interpolate(rAU)*fvc::ddtCorr(U, phi)
);

MRF.makeRelative(phiHbyA);

adjustPhi(phiHbyA, U, p);

phiHbyA += phil;
Hi Novel,
Have you also modified the line
Code:
            // Calculate the conservative fluxes
            phi = phiHbyA - p_rghEqn.flux();
??
__________________
best regards
pblasiak
gaza is offline   Reply With Quote

Old   September 21, 2017, 05:29
Default high residuals for p_rgh
  #34
Senior Member
 
Przemek
Join Date: Jun 2011
Posts: 249
Rep Power: 16
gaza is on a distinguished road
Quote:
Originally Posted by alberto View Post
I will try to give you the basic idea in the case of a generic body force term F, so that your momentum equation reads:

(1) ddt(U) + div(UU) = div(tau) - grad(p)/rho + F

This equation can be written in semi-discrete form as:

(2) A*U = H - grad(p)/rho + F

where the pressure gradient and the force term we want to include in the momentum interpolation is left explicitly out at this point. In other words, only the first three terms (time derivative, unsteady, divergence of the stress tensor) of Eq. 1 are used to define A and H. For example, in an incompressible code, this could read (it might be different, depending on the solver):

Code:
     fvm::ddt(U)
  + fvm::div(phi, U)
  + turbulence->divDevReff(U)
Normally the pressure gradient would be treated directly as a source term in an incompressible code (see pisoFoam for example). Here we assume we want to treat it with the "improved approach".

From Eq. 2, interpolating on faces and dotting with the surface area vector S the pressure gradient and the force term, we have:

- snGrad(p)*|S|/rho + F_f . S

where F_f is F interpolated on faces. This in OF corresponds to:

Code:
- fvc::snGrad(p)*mesh.magSf()/rhoa + fvc::interpolate(F) & mesh.Sf()
This term can be used as argument of fvc::reconstruct() to add the contribution of the pressure gradient and of the force term to the momentum predictor:

Code:
solve
(
      UEqn == fvc::reconstruct
      (
          - fvc::snGrad(p)*mesh.magSf()/rhoa 
          + fvc::interpolate(F) & mesh.Sf()
   )
)
Then OpenFOAM re-computes U as

U = H/A

where A is updated with the predicted value of U. However, keep in mind that H does not directly include the effect of grad(p) and F.

From Eq. 2 we can derive the flux to construct the pressure equation:

phi = (H/A)_f . S - (1/A)_f * snGrad(p) |S|/rho + (1/A)_f*F_f . S

and imposing div(phi) = 0, you obtain the pressure equation, which will include for the first time all the effects.

The flux is then corrected based on the solution of the pressure equation, and the velocity correction is reconstructed from the flux. Only at this point U will "see" the effect of p and F.

If you take a look at VOF solvers (i.e. interFoam), you will notice that the code does not solve for p, but for p_rgh = p + rho*gh. This is another way to treat the gravity to address the weakness of the Rhie-Chow interpolation, but the idea is similar.

I hope this helps, but please let us know if you have more questions

Best,
Hi Alberto,
I am trying to add body force to momentum equation like this
\frac{\partial \mathbf{U}}{\partial t}+\frac{\nabla\cdot(\mathbf{UU})}{\rho}-\frac{\nabla\cdot\mathbf{\tau}}{\rho} =-\frac{\nabla p}{\rho}+\rho_k \mathbf{g} - \mathbf{M}

where M is a body force. I based on buoyantBoussinesqPimpleFoam solver. I followed according to the instructions you provided and others on the forum and I changed the UEqn.H and pEqn.H as follows
UEqn.H
Code:
    tmp<fvVectorMatrix> tUEqn
    (
        fvm::ddt(U) + fvm::div(phi, U)
      + MRF.DDt(U)
      + turbulence->divDevReff(U)
     ==
        fvOptions(U)
    );
    fvVectorMatrix& UEqn = tUEqn.ref();

    UEqn.relax();

    fvOptions.constrain(UEqn);

    if (pimple.momentumPredictor())
    {
        solve
        (
            UEqn
         ==
            fvc::reconstruct
            (
                (
                  - ghf*fvc::snGrad(rhok)
                  - fvc::snGrad(p_rgh)
                )*mesh.magSf()
              - (fvc::interpolate(M) & mesh.Sf())
            )
        );

        fvOptions.correct(U);
    }
pEqn.H
Code:
{
    volScalarField rAU("rAU", 1.0/UEqn.A());
    surfaceScalarField rAUf("rAUf", fvc::interpolate(rAU));
    volVectorField HbyA(constrainHbyA(rAU*UEqn.H(), U, p_rgh));

    surfaceScalarField phig(-rAUf*ghf*fvc::snGrad(rhok)*mesh.magSf());
    surfaceScalarField phiM(-rAUf*(fvc::interpolate(M) & mesh.Sf()));

    surfaceScalarField phiHbyA
    (
        "phiHbyA",
        fvc::flux(HbyA)
      + rAUf*fvc::ddtCorr(U, phi)
      + phig
      + phiM
    );

    MRF.makeRelative(phiHbyA);

    // Update the pressure BCs to ensure flux consistency
    constrainPressure(p_rgh, U, phiHbyA, rAUf, MRF);

                                                

    while (pimple.correctNonOrthogonal())
    {
        fvScalarMatrix p_rghEqn
        (
            fvm::laplacian(rAUf, p_rgh) == fvc::div(phiHbyA)
        );

        p_rghEqn.setReference(pRefCell, getRefCellValue(p_rgh, pRefCell));

        p_rghEqn.solve(mesh.solver(p_rgh.select(pimple.finalInnerIter())));

        if (pimple.finalNonOrthogonalIter())
        {
            // Calculate the conservative fluxes
            phi = phiHbyA - p_rghEqn.flux();

            // Explicitly relax pressure for momentum corrector
            p_rgh.relax();

            // Correct the momentum source with the pressure gradient flux
            // calculated from the relaxed pressure
            U = HbyA + rAU*fvc::reconstruct((phiM + phig - p_rghEqn.flux())/rAUf); //5   (+)
            U.correctBoundaryConditions();
            fvOptions.correct(U);
        }
    }

    #include "continuityErrs.H"

    p = p_rgh + rhok*gh;

    if (p_rgh.needReference())
    {
        p += dimensionedScalar
        (
            "p",
            p.dimensions(),
            pRefValue - getRefCellValue(p, pRefCell)
        );
        p_rgh = p - rhok*gh;
    }
}
However I got high residuals for p_rgh as in the image attached. Have I missed something or done something wrong?
Attached Images
File Type: jpg highResForP_rgh.jpg (66.8 KB, 37 views)
__________________
best regards
pblasiak
gaza is offline   Reply With Quote

Old   November 3, 2017, 05:34
Default
  #35
New Member
 
Roman G.
Join Date: Apr 2017
Posts: 16
Rep Power: 9
Novel is on a distinguished road
Hi gaza,
I had problems when adding a source term without adjusting the flux to ensure mass conservation. Try to add the source terms after adjusting phi to your flux phiHybA.
Quote:
Originally Posted by gaza View Post
hi alberto,
peqn.h
Code:
{
    volscalarfield rau("rau", 1.0/ueqn.a());
    surfacescalarfield rauf("rauf", fvc::interpolate(rau));
    volvectorfield hbya(constrainhbya(rau*ueqn.h(), u, p_rgh));

    surfacescalarfield phig(-rauf*ghf*fvc::sngrad(rhok)*mesh.magsf());
    surfacescalarfield phim(-rauf*(fvc::interpolate(m) & mesh.sf()));

    surfacescalarfield phihbya
    (
        "phihbya",
        fvc::flux(hbya)
      + rauf*fvc::ddtcorr(u, phi)
    );
    mrf.makerelative(phihbya);
    adjustPhi(phihbya, U, p_rgh);
    phihyba += phig + phim;


    // update the pressure bcs to ensure flux consistency
    constrainpressure(p_rgh, u, phihbya, rauf, mrf);

                                                

    while (pimple.correctnonorthogonal())
    {
        fvscalarmatrix p_rgheqn
        (
            fvm::laplacian(rauf, p_rgh) == fvc::div(phihbya)
        );

        p_rgheqn.setreference(prefcell, getrefcellvalue(p_rgh, prefcell));

        p_rgheqn.solve(mesh.solver(p_rgh.select(pimple.finalinneriter())));

        if (pimple.finalnonorthogonaliter())
        {
            // calculate the conservative fluxes
            phi = phihbya - p_rgheqn.flux();

            // explicitly relax pressure for momentum corrector
            p_rgh.relax();

            // correct the momentum source with the pressure gradient flux
            // calculated from the relaxed pressure
            u = hbya + rau*fvc::reconstruct((phim + phig - p_rgheqn.flux())/rauf); //5   (+)
            u.correctboundaryconditions();
            fvoptions.correct(u);
        }
    }

    #include "continuityerrs.h"

    p = p_rgh + rhok*gh;

    if (p_rgh.needreference())
    {
        p += dimensionedscalar
        (
            "p",
            p.dimensions(),
            prefvalue - getrefcellvalue(p, prefcell)
        );
        p_rgh = p - rhok*gh;
    }
}
Please let me know if this solved your problem.
Novel is offline   Reply With Quote

Old   November 10, 2017, 07:35
Default
  #36
Senior Member
 
Przemek
Join Date: Jun 2011
Posts: 249
Rep Power: 16
gaza is on a distinguished road
Hi Novel,
Thank you for your tip however in my case I do not see the difference after adjustPhi.
__________________
best regards
pblasiak
gaza is offline   Reply With Quote

Reply

Tags
body force, force

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Help on 2D interpolation in StarCCM+ madhuri Siemens 1 May 30, 2017 04:20
urgent help needed (rhie-chow interpolation problem) Ardalan Main CFD Forum 2 March 18, 2011 16:22
Surface interpolation schemes and parallelization jutta OpenFOAM Running, Solving & CFD 0 February 25, 2010 15:32
momentum interpolation for collocated grid Hadian Main CFD Forum 4 December 25, 2009 08:25
spline interpolation bajjal Main CFD Forum 0 May 29, 2006 09:27


All times are GMT -4. The time now is 01:26.