[tdof]

See my post in #414 and the reply from Prof. Jasak. The PISO implementation in viscoealsticFluidFoam uses under-relaxation.

[alimea]

Originally Posted by tdof

See my post in #414 and the reply from Prof. Jasak. The PISO implementation in viscoealsticFluidFoam uses under-relaxation.

thanks for your reply
but I couldn't find it. could you please send me the link?

[tdof]

There you go:

Originally Posted by tdof

Hi, I've got a question about the PISO algorithm used in viscoelasticFluidFoam. The official statement in the OF documentation is that it does not use underrelaxation, but the example cases all implement relaxation factors. I therefore assume that the PISO algorithm has been modified to allow their usage, but is a description available somewhere describing this exactly? Edit: I've found it in the source code, but is there a diagram or other explanation available?

Also, does the solver use the complete Navier Stokes equations or only Stokes?

Originally Posted by hjasak

The solver solves the Navier-Stokes equations

I do not think you need an entire book just for the fact that PISO under-relaxaes the momentum equation to improve stability.

In any case, we are moving to coupled solvers - see recent work from Prof Nobrega.

Hrv

[alimea]

Originally Posted by hjasak

The solver solves the Navier-Stokes equations

I do not think you need an entire book just for the fact that PISO under-relaxaes the momentum equation to improve stability.

In any case, we are moving to coupled solvers - see recent work from Prof Nobrega.

Hrv

Hi
Could you plz explain it more?
I am solving the flow a viscoelastic fluid around a cylinder by a viscoelasticFluidFlow solver that is written based on PISO. In all of the tutorials of this solver of openFoam URF is used, however we now that PISO algorithm has no URF. so why did they use?

I decided to solve a problem with urf=0.3 and urf=1 and compare the results with the results of a paper(Oliviera):



I saw a difference in CL amplitude!! I'm confused! what is the truth?!

the second problem was for a big difference in time period that I think this is because of my div(U) scheme that was central and that was better to use some thing like vanLeer. when I use vanLeer for div(U) this difference will be solved:




Is my conclusion correct?
You can see that all of the d/dt schemes are matches in CD amplitude. Also there is not any time period difference between Oliviera values and mine. But again there is a big difference in CD amplitude.


Thanks

[alimea]

Originally Posted by hjasak

The solver solves the Navier-Stokes equations

I do not think you need an entire book just for the fact that PISO under-relaxaes the momentum equation to improve stability.

In any case, we are moving to coupled solvers - see recent work from Prof Nobrega.

Hrv

Any answer?

[alimea]

Hi

please answer me:

according to what I said in my last posts, can we use URF in viscoelasticFluidFoam solver?

[alimea]

Hi foamers

I'm working on viscoelastic fluid flow around a cylinder(Re=10, Elasticity nu. = 0-100). when I check the tau magnitude in domain (in paraView), I see that tau magnitude (tau: polymeric stress tensor) decreases with increasing Weissenberg number!

I don't know if they are correct or not!
I think it should be increased with Wi.

Also when I plot drag coefficient vs. El number, I see that tau portion of drag decreases with El as far as in El=10 it is almost zero!
I can't give a reason for that.

Could you please tell me your idea?

[alimea]

Hi all,

I saw the second order viscoelastic model in many papers which is used as constitutive eqn.

What's the difference between "second order viscoelastic model" and the other familiar viscoelastic models like Giessesk, Oldroyd-B, PTT, etc?

Thanks

[sita]

Hi Alimea,

The second order fluid is a very simple model to describe non-Newtonian flow effects (see e.g. the books by Bird and/or Macosko). It only holds for flows that are sufficiently slow and slowly varying.

Hope this helps,
Sita

[alimea]

Originally Posted by sita

Hi Alimea,

The second order fluid is a very simple model to describe non-Newtonian flow effects (see e.g. the books by Bird and/or Macosko). It only holds for flows that are sufficiently slow and slowly varying.

Hope this helps,
Sita

Dear Sita,

Thanks for your reply.
I solved a problem with PTT model which had been solved with second-order model before I/m worried about the innovation if I want to write a new paper?

Regards,
Ali

[sita]

Dear Ali,

If you're planning to publish your results, I think it would be a good idea to look into the details of both models, and how these models apply to the problem you solved. Ask yourself questions like: what kinds of deformations and stresses do I expect in this problem? Why was it originally solved using a second order model? When the problem was solved using a second order model, were the results satisfactory, did problems occur? Why would the PTT model be better suited for this than the second order model? Why PTT and not Giesekus, or Oldroyd-B, or FENE-P, or ...? Are the results with the PTT model indeed better/more reliable than those with the second order model? Why (not)? Would an improved solution to this problem be relevant/useful? Etcetera... That should help you judge whether publishing your results would be worthwhile.

Good luck,
Sita

[alimea]

Originally Posted by sita

Dear Ali,

If you're planning to publish your results, I think it would be a good idea to look into the details of both models, and how these models apply to the problem you solved. Ask yourself questions like: what kinds of deformations and stresses do I expect in this problem? Why was it originally solved using a second order model? When the problem was solved using a second order model, were the results satisfactory, did problems occur? Why would the PTT model be better suited for this than the second order model? Why PTT and not Giesekus, or Oldroyd-B, or FENE-P, or ...? Are the results with the PTT model indeed better/more reliable than those with the second order model? Why (not)? Would an improved solution to this problem be relevant/useful? Etcetera... That should help you judge whether publishing your results would be worthwhile.

Good luck,
Sita

Dear Sita,

Really thanks for your complete reply.

Best Regards,
Ali

[leoli]

Originally Posted by ata

Hi Purushotam Kumar
I hope you are doing very well. I have been done you desired code in OpenFOAM but because I am PhD student I can not release it before end of my PhD. However you can use interFoam and viscoelasticFluidFoam solvers and combine them to achieve your purpose. I'll be very glad if I can help you.
Best regards

Ata

Hi Ata,

i am now simulating the two phase fluid, one is viscoelatic fluid with Oldroyd B model, the other is newtonian fluid like air. I think i need to combine the two solvers viscoelasticfluidfoam and interfoam together.

but i do not now how exactly i can combine these two solvers, have you already released your solver?

I will really appreciate that!

thank you!

[idrees khan]

Originally Posted by hjasak

It runs fine here, the last change was

commit 6b50e03f4417291ba2c9184244d37e2630ef2dae
Author: Henrik Rusche <h.rusche@wikki-gmbh.de>
Date: Thu Dec 12 00:41:18 2013 +0100

Below is the fvSolution file:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | foam-extend: Open Source CFD |
| \\ / O peration | Version: 3.0 |
| \\ / A nd | Web: http://www.extend-project.de |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object fvSolution;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

solvers
{

p
{
solver PCG;
preconditioner Cholesky;

tolerance 1e-07;
relTol 0;
minIter 0;
maxIter 800;
}

U
{
solver BiCGStab;
preconditioner ILU0;

tolerance 1e-6;
relTol 0;
minIter 0;
maxIter 1000;
}

tau
{

solver BiCGStab;
preconditioner ILU0;

tolerance 1e-6;
relTol 0;
minIter 0;
maxIter 1000;

};

}

PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}

relaxationFactors
{
p 0.3;
U 0.5;
tau 0.3;
}

// ************************************************** *********************** //

Hi sir, is there any related tutorial about A generalized Oldroyd-
Model implemented in foam-extend.4.0.
kindly your help will be highly appreciated.

[arashfluid]

Hello Dear friends,
I am simulating the viscoelastic fluid flow in the microchannel. My Weissenberg number is very high (Wi=28). But my fluid is a Boger type and I use the Oldroyd-B model. At first, I have run the viscoelasticFluidFoam solver in OF1.6-ext in unsteady mode and the solution diverged after 0.008 seconds. Then I have run the same case with the rheoFoam solver in OF4.1 which did not diverge but the number of pressure iterations showed a lack of convergence at each time step. Due to a long time of simulation, I have adjusted and run the rheoFoam solver in a steady mode. But from iteration 50 to the next, the solution goes to divergence. Is there a way I can run the viscoelasticFluidFoam solver in a steady mode so that it is stable?

The settings of my two fvSchemes and fvSolution files in the two solvers are as follows:
for unsteady viscoelasticFluidFoam:

fvSchemes:

ddtSchemes
{
default Euler;
}

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

}

divSchemes
{
default none;
div(phi,U) Gauss upwind;
div(phi,tau) Gauss upwind;
div(tau) Gauss linear;
}

laplacianSchemes
{
default none;
laplacian(etaPEff,U) Gauss linear corrected;
laplacian(etaPEff+etaS,U) Gauss linear corrected;
laplacian((1|A(U)),p) Gauss linear corrected;
}

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

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

fvSolution:

solvers
{

p
{
solver PCG;
preconditioner
{
// preconditioner Cholesky;
preconditioner AMG;
cycle W-cycle;
policy PAMG;
nPreSweeps 0;
nPostSweeps 2;
groupSize 4;
minCoarseEqns 20;
nMaxLevels 100;
scale off;
smoother ILU;
}

tolerance 1e-07;
relTol 0;
minIter 0;
maxIter 800;
}

U
{

solver BiCGStab;
preconditioner
{
preconditioner Cholesky;
}

tolerance 1e-6;
relTol 0;
minIter 0;
maxIter 1000;
}

tau
{

solver BiCGStab;
preconditioner
{
preconditioner Cholesky;
}

tolerance 1e-6;
relTol 0;
minIter 0;
maxIter 1000;

};

}

PISO
{
nCorrectors 2;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}

relaxationFactors
{
p 0.3;
U 0.5;
tau 0.3;
}

for steady rheoFoam:

fvSchemes:
ddtSchemes
{
default steadyState; //Euler;
}

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

}

divSchemes
{
default none;
div(tau) Gauss linear;
div(grad(U)) Gauss linear;
div(phi,U) GaussDefCmpw none;
div(phi,theta) GaussDefCmpw cubista;
div(phi,tau) GaussDefCmpw cubista;
div(phi,C) GaussDefCmpw cubista;
}

laplacianSchemes
{
default none;
laplacian(eta,U) Gauss linear corrected;
laplacian(p|(ap-H1)) Gauss linear corrected;
laplacian(D,C) Gauss linear corrected;

}

interpolationSchemes
{
default linear;

}

snGradSchemes
{
default corrected;
}

fluxRequired
{
default no;
p;
}

fvSolution:

solvers
{
"(p|U)"
{
solver PCG;
preconditioner DIC;
tolerance 1e-10;
relTol 0.;
minIter 0;
maxIter 800;

}

"(theta|tau|C)"
{

solver PBiCG;
preconditioner
{
preconditioner DILU;
}

tolerance 1e-10;
relTol 0.;
minIter 0;
maxIter 1000;
}

}


SIMPLE
{
nInIter 1;
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;

residualControl
{

p 1e-5;
U 1e-5;
tau 1e-5;
theta 1e-5;
C 1e-5;

}
}

relaxationFactors
{
fields
{
p 0.3; //0.01;
}

equations
{
U 0.5; //0.7; //1;
tau 0.3; //0.5;//1;
theta 0.3; //1;
C 0.3; //1;
}
}



Please suggest me a way to resolve this problem steadily and stably.

[sita]

Hi Arash,

The Oldroyd-B model gives unbounded stress if the elongation rate in your flow exceeds 1/(2 lambda), with lambda your relaxation time. I don't know what your flow looks like, but this might well explain your simulation diverging.

If you're aiming for Boger fluid behaviour, the FENE-CR model might be better suited for your simulations (viscoelastic behaviour, without shear thinning).

Hope this helps,
Sita

[sita]

Hi Arash,

Just curious: did you get your simulation to run in the end?

Cheers,
Sita

[arashfluid]

Originally Posted by sita

Hi Arash,

Just curious: did you get your simulation to run in the end?

Cheers,
Sita

The viscoelasticFluidFoam solver in of16ext has diverged in 0.008sec, but the rheoFoam solver is still running up to 0.3sec and the flow conditions have not yet been stabled. Of course, the pressure full iterations are indicative of non-convergence. But it is still progressing.

[sita]

Hi Arash,

When you say that the viscoelasticFluidFoam solver crashed after 0.008 s, was that using the Oldroyd-B model, or the FENE-CR model?

You may want to try running at a lower Wi first, and experiment with parameter values, mesh settings, etc. Visualising your results can be helpful to find out what made your simulation crash. I ran lots of high Wi simulations some years ago, using viscoelasticFluidFoam (with FENE-P and FENE-CR, mostly), so it should be possible alright. From what I remember, the mesh settings can be tricky to get right, though.

Good luck,
Sita

[arashfluid]

Originally Posted by sita

Hi Arash,

When you say that the viscoelasticFluidFoam solver crashed after 0.008 s, was that using the Oldroyd-B model, or the FENE-CR model?

You may want to try running at a lower Wi first, and experiment with parameter values, mesh settings, etc. Visualising your results can be helpful to find out what made your simulation crash. I ran lots of high Wi simulations some years ago, using viscoelasticFluidFoam (with FENE-P and FENE-CR, mostly), so it should be possible alright. From what I remember, the mesh settings can be tricky to get right, though.

Good luck,
Sita

Dear Sita,
I used the Oldroyd-B model for 1000 ppm PEO in DI-water that is a Boger fluid. I have not seen any articles that use the FENE model for Boger fluid. I also tried many meshes. My Wi numbers are in the range of 10-100. May I ask you what kind of schemes did you use?