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

NonNewtonianIcoFoam for steadystate problem

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

Reply
 
LinkBack Thread Tools Display Modes
Old   July 18, 2005, 15:19
Default Hi, Henry, In one of the ea
  #1
New Member
 
Jing Wang
Join Date: Mar 2009
Location: Toronto, Ontario, Canada
Posts: 7
Rep Power: 8
mpml is on a distinguished road
Hi, Henry,

In one of the earlier responses on this forum you said that transient solvers may not converge for steady-state problems. Right now I am trying to model some polymer extrusion process using OpenFOAM, but it looks like there is no solver for steady-state laminar flow of nonNewtonian fluids. Do you think nonNewtonianIcoFoam can be used for my purpose by setting the runTime long enough? (simpleFoam seems to be for turbulent flow, rather than laminar flow)

If you don't think so, could you explain a little bit what I should do? Thanks a lot.
mpml is offline   Reply With Quote

Old   July 18, 2005, 15:21
Default Use simpleFoam with the "lamin
  #2
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
Use simpleFoam with the "laminar" turbulence model.
henry is offline   Reply With Quote

Old   July 19, 2005, 10:31
Default I want to patch, in the first
  #3
Member
 
olivier Petit
Join Date: Mar 2009
Location: Göteborg, Sweden
Posts: 67
Rep Power: 8
olivier is on a distinguished road
I want to patch, in the first zone where y<1,

a viscosity wich is different than the one in the second zone where y>1.
How can i do that, please
Thanks a lot.
olivier is offline   Reply With Quote

Old   July 19, 2005, 14:56
Default Have a look at the setGammaDam
  #4
Super Moderator
 
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,416
Rep Power: 16
mattijs is on a distinguished road
Have a look at the setGammaDambreak utility in the damBreak tutorial on how to access the cell centres.

Change the createFields.H in your solver and make the nu into a volScalarField. Either use the same syntax as for e.g. p in which case it gets read from disk or use the extra constructor argument:


volScalarField nu
(
IOobject
(
"nu",
runTime.timeName(),
mesh,
IOobject::MUST_READ,
IOobject::AUTO_WRITE
),
mesh,
dimensionedScalar(transportProperties.lookup("nu") )
);
mattijs is offline   Reply With Quote

Old   July 19, 2005, 15:32
Default Hi, Henry, Thanks for your
  #5
New Member
 
Jing Wang
Join Date: Mar 2009
Location: Toronto, Ontario, Canada
Posts: 7
Rep Power: 8
mpml is on a distinguished road
Hi, Henry,

Thanks for your last reply. I tried simpleFoam and it got a converged solution for my problem. But the pressure seems about 2 orders lower than expected.

I am somehow confused about the PDE equation defined in simple foam, which is:

tmp<fvvectormatrix> UEqn
(
fvm::div(phi, U)
+ turbulence->divR(U)
);

UEqn().relax();

solve(UEqn() == -fvc::grad(p));

It seems the diffusion term, fvm::laplacian(fluid->nu(), U), doesn't appear here. I think it it included in the turbulence->divR(U) term, but can not figure it out by looking at the source code.

My question is, if I use laminar model in simpleFoam, are the PDEs in nonNewtonianIcoFoam and SimpleFoam going to be exactly the same (except for the time derivative) ? How does simpleFoam read in the transport properties(I don't see 'transportProperties.lookup("nu")' in simpleFoam's sourcecode) ? Thanks a lot.
mpml is offline   Reply With Quote

Old   July 19, 2005, 15:39
Default simpleFoam should give very si
  #6
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
simpleFoam should give very similar results to nonNewtonianIcoFoam.

The laminar transport model is created by

autoPtr<transportmodel> laminarTransport
(
transportModel::New(U, phi)
);

in simpleFoam and equivalently by

autoPtr<transportmodel> fluid
(
transportModel::New(U, phi)
);

in nonNewtonianIcoFoam,

dimensionedScalar nu
(
transportProperties.lookup("nu")
);

is redundant and should be removed.

The laminar stress term is indeed included in

turbulence->divR(U)
henry is offline   Reply With Quote

Old   July 20, 2005, 18:58
Default Thanks, Henry. I checked the s
  #7
New Member
 
Jing Wang
Join Date: Mar 2009
Location: Toronto, Ontario, Canada
Posts: 7
Rep Power: 8
mpml is on a distinguished road
Thanks, Henry. I checked the source code and is much better informed now.

I have a very simple question (maybe stupid) about the following line of code:

fvc::div(nuEff( )*dev(fvc::grad(U)( ).T( )))

It looks like this is the momentum source, which is ignored in nonNewtonianIcoFoam. But I have never seen expressions like "grad(U)( )" in C++ code (a function call followed immediately by a pair of brackets). Is the return value from grad(U) used as a function name here?

Thanks a lot if you can clarify a little bit.
mpml is offline   Reply With Quote

Old   July 20, 2005, 19:09
Default In incompressible flow that te
  #8
Senior Member
 
Join Date: Mar 2009
Posts: 854
Rep Power: 13
henry is on a distinguished road
In incompressible flow that term will be small but only zero if the viscosity is uniform and hence formally should be included in nonNewtonianIcoFoam.

fvc::grad(U) returns a tmp<voltensorfield> and the transpose member function .T() is called for the const volTensorField& returned by the tmp dereferencing operator ().
henry 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
Couette flow with nonNewtonianicoFoam floooo OpenFOAM Running, Solving & CFD 2 December 7, 2010 06:39
SteadyState tutlhino OpenFOAM Running, Solving & CFD 5 April 30, 2009 09:10
Steadystate settlingFoam darrin OpenFOAM Running, Solving & CFD 0 February 28, 2007 05:51
Steadystate Vs Transient solver amitshah OpenFOAM Running, Solving & CFD 1 August 23, 2006 02:54
Steadystate Euler solver jelmer OpenFOAM Running, Solving & CFD 1 June 19, 2006 08:24


All times are GMT -4. The time now is 08:30.