CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Fourth Order Runge Kutta time integration (http://www.cfd-online.com/Forums/openfoam-solving/60452-fourth-order-runge-kutta-time-integration.html)

 lr103476 October 26, 2005 09:07

Hello, Has someone implemen

Hello,

Has someone implemented 4th order Runge Kutta time integration. I think this method will be more efficient than the 2nd order CrankNickolson.

Maybe someone tried it and could give me some hints in order to develop it myself.

Regards, Frank

 misakagan December 16, 2009 09:19

I'm also wondering if someone has runge-kutta implementation for incompressible turbulent flows (LES or DNS). Apparently the only application dealing such flows is Pisofoam and it uses implicit time stepping, which is very slow.

 theory37 June 14, 2010 12:07

I too am wondering about this. I am attempting to implement a 3rd order (low storage) RK scheme for an RSTM I am working on. Any ideas?

 ville September 19, 2010 16:56

Runge-Kutta 4 to top-level OpenFOAM

Hi! I am currently working on compressible flows and writing a RK4 method to OpenFOAM. I am currently learning many things about top-level programming
(mostly from the codes written by other people) but would like to share a simple example of one way to program
RK4 in the top-level code. The following code (that can be put inside the main for-loop of any existing solver to test it) solves the simple advection equation for a variable rho (that can represent of course anything).
Here, we btw can assume for the moment being that
U is a constant field i.e. the velocity.

rhoOld = rho;
phiv = fvc::interpolate(U)& mesh.Sf();
k1 = -runTime.deltaT()*fvc::div(phiv, rhoOld);
k2 = -runTime.deltaT()*fvc::div(phiv, rhoOld + 0.5*k1);
k3 = -runTime.deltaT()*fvc::div(phiv, rhoOld + 0.5*k2);
k4 = -runTime.deltaT()*fvc::div(phiv, rhoOld + k3);

rho = rhoOld + a1*k1 + a2*k2 + a3*k3 + a4*k4;

// ai are the RK4 coefficients

Of the following I would like to hear some further comments about and hopefully the more experienced people could further comment on
these issues (or point out a proper link to a discussion).

When programming explicit code as above the correctBoundaryConditions() function should be used after each update because otherwise there might be
inconsistencies in BC's and also in the processor
BC's. I guess the reason for this is that field operations
such as the ones above have no influence on what
is happening on the boundary; right ?
One can also explicitly update the BC's for a certain
quantity (say e.g. rhoE that is often solved for in
compressible computations) by typing

rhoE.boundaryField() =
rho.boundaryField()*
(
e.boundaryField() + 0.5*magSqr(U.boundaryField())
);

Of course, it remains as user's responsibility
that everything stays consistent when doing
top-level OF solvers.

Regarding the previous question about an incompressible RK4 solver I do not see any problem
of why the above-presented approach for advection
equation would not work also for the
incompressible NS-equations .

Best regards,
Ville

 alberto September 20, 2010 02:47

Quote:
 Originally Posted by ville (Post 275756) When programming explicit code as above the correctBoundaryConditions() function should be used after each update because otherwise there might be inconsistencies in BC's and also in the processor BC's. I guess the reason for this is that field operations such as the ones above have no influence on what is happening on the boundary; right ?
Yes and no :D
Yes, you have to do something to update the boundaries, if you need that. No, what you have to do is not necessarily an explicit call to correctBoundaryConditions().

If you update the value of a field, and you also want to update the corresponding boundaryField, all you have to do is to replace

=

with

==

in the assignment. For example:

k1 == ...;

This should work in OF 1.6 and following. I am not sure about the previous versions, since I noticed this syntax for the first time in 1.6.

Of course, if you do not have an assignment, but a sum with +=, like in the velocity corrector step, you have to call correctBoundaryConditions().

Best,

 juho September 20, 2010 04:54

Quote:
 Originally Posted by alberto (Post 275776) Yes and no :D This should work in OF 1.6 and following. I am not sure about the previous versions, since I noticed this syntax for the first time in 1.6.
I've used it in 1.4.1, so I would assume it also works in all the following versions.

 alberto September 20, 2010 10:26

OK. Thanks for the info :)

 ville September 20, 2010 10:46

Hi and thanks for the comments!
As said, I am currently considering how to nicely implement the boundary conditions for a fully explicit, density based RK4 solver (say the hardest case of subsonic inflow, outflow for the time being).
Currently, in the prototype version, I define the BC's for p, T and U as they are rather convenient to give. The variables that are solved for are rho, rhoU and rhoE. Now, the BC's for rho, rhoU and rhoE would be needed. In e.g. subsonic inflow the BC for rho would need to be determined by the solution. Thus, p and
T may be used for determining the boundary value of rho.
After this the boundary fields of rhoU and rhoE may be constructed. Any ideas of how to conveniently do this?
How would the more experienced OF-people consider simply
updating the boundary field in the top-level code as is done in
e.g. rhoCentralFoam? Another option would be
defining a new BC type for rho, rhoU and rhoE that is constructed from p, T and U.
Best,
Ville

 ville October 31, 2012 12:00

Runge-Kutta 4 density based LES solver implemented

Hi,
to get a closure: I have now implemented into OpenFOAM a RK4 based
fully explicit compressible solver. Works as smoothly as it only can :)
I've also written RK4 solvers for incompressible flows based on the projection method
which allows us to get rid of the PISO solvers if so desired.
Work based on the incompressible solver was published recently in Computers & Fluids
and can be found currently in the "Articles in Press" section of the journal.

Vuorinen V., Schlatter P., Boersma B., Larmi M., and Fuchs L., A Scale-Selective, Low-
Dissipative Discretization Scheme for the Navier-Stokes Equation, (to appear in Computers and Fluids)

Best,
Ville

 ville February 27, 2014 03:29

Publication: Runge-Kutta 4 method for compressible and incompressible flows

Hi,
probably the first published paper on the topic including practical instructions
on how to implement, theory, numerical validation
On the implementation of low-dissipative Runge–Kutta projection methods for time dependent flows using OpenFOAM

Vuorinen et al.
http://www.sciencedirect.com/science...45793014000334

Best,
Ville

 ville November 11, 2014 09:27

Fluid dynamical part of the code shown herein

Large-eddy simulation in a complex hill terrain enabled by a compact fractional step OpenFOAM® solver

http://www.sciencedirect.com/science...65997814001513

Best wishes,
Ville

 syavash August 19, 2015 15:46

Quote:
 Originally Posted by ville (Post 518534) Large-eddy simulation in a complex hill terrain enabled by a compact fractional step OpenFOAM® solver http://www.sciencedirect.com/science...65997814001513 Best wishes, Ville
Dear Ville,

Is it possible to share your incompressible solver?! I am sure many people like me seek for an explicit low-dissipation solver for LES-like simulation.

Syavash.

 ville August 20, 2015 03:27

Hi,
the functional part of the code is given in the above link entirely inside the article.
You just need to copy that text and modify e.g. pisoFoam to get a working solver.
Note that the projection pressure units are a bit different in the rk4projectionFoam solver version than pisoFoam since we apply the projection method. This is just a matter of convention and the way the pressure is introduced to the system. In the end the units on
LHS and RHS of NS eqs are the same.
Best regards, Ville

 syavash August 20, 2015 08:24

Quote:
 Originally Posted by ville (Post 560298) Hi, the functional part of the code is given in the above link entirely inside the article. You just need to copy that text and modify e.g. pisoFoam to get a working solver. Note that the projection pressure units are a bit different in the rk4projectionFoam solver version than pisoFoam since we apply the projection method. This is just a matter of convention and the way the pressure is introduced to the system. In the end the units on LHS and RHS of NS eqs are the same. Best regards, Ville
Thanks Ville,

I have proceeded as the steps in your paper have suggested, but I have encountered some problems in creating the new solver:
1-The variables Uold, Uc, and dU are not defined, so I constructed them in createFields.H as volVectorField. Is it OK?!
2-I have renamed pRef in CreatePoissonMatrix.H to pRefValue because the latter was defined in pisoFoam
3-I have difficulty in defining dt. How should I define this variable? I tried : scalar dt, but OF throws me an error. I think I should consider a dimensionedScalar but do not know the right syntax.
4-Where should I define a1,a2,a3, and a4? I have currently defined them simply as scalar at the beginning of the while-loop.

At the moment the above issues come to my mind. I greatly appreciate if you help me compile the new solver.

Thanks,
Syavash

 ville August 20, 2015 08:32

Hi,

>1-Uold and Uc variables are not defined, so I constructed them in createFields.H. Is it >OK?!

Of course. They are dummy fields which you can define with something like:

volVectorField Uold
(
IOobject
(
"Uold",
runTime.timeName(),
mesh,
IOobject::NO_WRITE
),
U
);

volVectorField dU
(
IOobject
(
"dU",
runTime.timeName(),
mesh,
IOobject::NO_WRITE
),
U
);

>2-I have renamed pRef in CreatePoissonMatrix.H to pRefValue because the latter >was defined in pisoFoam

Sure

>3-I have difficutly in defining dt. How should I define this variable? I tried : scalar dt, >but OF throws me an error. I think I should consider a dimensionedScalar but do not >know the right syntax.

You could replace it with runTime.deltaT() or define e.g. a dimensioned scalar
dt which you set to runTime.deltaT() at the beginning of each timestep. I just wrote
dt in the paper to make it more straightforward

>4-Where should I define a1,a2,a3, and a4? I have currently defined them simply as >scalar at the beginning of the while-loop.

For example you could define a file called rk4coeff.H which you "include" with
#include rk4coeff.H before main loop starts. There you could write something like

Info << "\nDefine RK4 coeff." <<endl;

const scalar a1 = 0.166666666667;
const scalar a2 = 0.333333333333;
const scalar a3 = 0.333333333333;
const scalar a4 = 0.166666666667;

Info << "\n a1 = " <<a1<< "\n a2 = " <<a2<<"\n a3 = " <<a3<<"\n a4 = " <<a4<< endl;

Got it working ?

 syavash August 20, 2015 08:48

Quote:
 Originally Posted by ville (Post 560341) Hi, >1-Uold and Uc variables are not defined, so I constructed them in createFields.H. Is it >OK?! Of course. They are dummy fields which you can define with something like: volVectorField Uold ( IOobject ( "Uold", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), U ); volVectorField dU ( IOobject ( "dU", runTime.timeName(), mesh, IOobject::NO_READ, IOobject::NO_WRITE ), U ); >2-I have renamed pRef in CreatePoissonMatrix.H to pRefValue because the latter >was defined in pisoFoam Sure >3-I have difficutly in defining dt. How should I define this variable? I tried : scalar dt, >but OF throws me an error. I think I should consider a dimensionedScalar but do not >know the right syntax. You could replace it with runTime.deltaT() or define e.g. a dimensioned scalar dt which you set to runTime.deltaT() at the beginning of each timestep. I just wrote dt in the paper to make it more straightforward >4-Where should I define a1,a2,a3, and a4? I have currently defined them simply as >scalar at the beginning of the while-loop. For example you could define a file called rk4coeff.H which you "include" with #include rk4coeff.H before main loop starts. There you could write something like Info << "\nDefine RK4 coeff." <

Now I am getting an error like this:

Code:

```syavash@syavash-VPCF11DGX:~/OpenFOAM/OpenFOAM-2.3.1/applications/solvers/incompressible/rk4projectionFoam\$ wmake options:2:66: warning: backslash and newline separated by space [enabled by default]     -I\$(LIB_SRC)/turbulenceModels/incompressible/turbulenceModel \     ^ Making dependency list for source file rk4projectionFoam.C SOURCE=rk4projectionFoam.C ;  g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3  -DNoRepository -ftemplate-depth-100 -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/turbulenceModels/incompressible/turbulenceModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/../applications/solvers/incompressible/pisoFoam -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/transportModels/incompressible/singlePhaseTransportModel -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude -IlnInclude -I. -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OpenFOAM/lnInclude -I/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/OSspecific/POSIX/lnInclude  -fPIC -c \$SOURCE -o Make/linux64GccDPOpt/rk4projectionFoam.o In file included from rk4projectionFoam.C:58:0: /home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude/setDeltaT.H: In function ‘int main(int, char**)’: /home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude/setDeltaT.H:36:35: error: ‘CoNum’ was not declared in this scope     scalar maxDeltaTFact = maxCo/(CoNum + SMALL);                                   ^ In file included from rk4projectionFoam.C:46:0: /home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude/initContinuityErrs.H:37:8: warning: unused variable ‘cumulativeContErr’ [-Wunused-variable]  scalar cumulativeContErr = 0;         ^ make: *** [Make/linux64GccDPOpt/rk4projectionFoam.o] Error 1```
Any idea where I migh be wrong??!

Edit: I could compile the code by adding #include "CourantNo.H" just after #include "readTimeControls.H".
But this warning still persists:

In file included from rk4projectionFoam.C:46:0:
/home/syavash/OpenFOAM/OpenFOAM-2.3.1/src/finiteVolume/lnInclude/initContinuityErrs.H:37:8: warning: unused variable ‘cumulativeContErr’ [-Wunused-variable]
scalar cumulativeContErr = 0;

Another question: Can I adjust time step by giving courant number as in pimpleFoam?!

 ville August 20, 2015 09:06

The turbulence model warning would be a matter of some normal include statements
that could be copied from pisoFoam. As you can see, you have now created an OpenFOAM code from scratch and this piece of code does not really assume too many
things: there are fields which are updated in time. Thus, the rk4projectionFoam solver
is simply a field update scheme with explicit time integration and finite volume discretization. About time step control: why could you not do it ? Of course one
needs to understand the algorithm: at which point of the main loop you update
it etc but otherwise you would have quite a freedom to do that.

 syavash August 20, 2015 09:13

Quote:
 Originally Posted by ville (Post 560346) The turbulence model warning would be a matter of some normal include statements that could be copied from pisoFoam. As you can see, you have now created an OpenFOAM code from scratch and this piece of code does not really assume too many things: there are fields which are updated in time. Thus, the rk4projectionFoam solver is simply a field update scheme with explicit time integration and finite volume discretization. About time step control: why could you not do it ? Of course one needs to understand the algorithm: at which point of the main loop you update it etc but otherwise you would have quite a freedom to do that.
Dear Ville,

Now I am really willing to compare runtime of pisoFoam and the new solver together.
Do you mind if I post my observations here?!

Thanks,
Syavash

 ville August 20, 2015 09:25

Sure. Please bare in mind that the conclusions I've made on runtime differences
were mostly for turbulent flows in parallel runs. Full conclusions are probably
depending on the number of processors, the parallel system which you use, the linear solver, the case (e.g. laminar vs turbulent). Good to start with lid driven cavity and check if you can reproduce the Ghia's data.

 syavash August 20, 2015 10:14

Quote:
 Originally Posted by ville (Post 560350) Sure. Please bare in mind that the conclusions I've made on runtime differences were mostly for turbulent flows in parallel runs. Full conclusions are probably depending on the number of processors, the parallel system which you use, the linear solver, the case (e.g. laminar vs turbulent). Good to start with lid driven cavity and check if you can reproduce the Ghia's data.
All right,

As something that migh matter, should any modifications be applied in controlDict, fvScheme, or fvSolution?!

Edit: I have encountered the following error during runtime,

Code:

```--> FOAM FATAL IO ERROR: keyword div(U) is undefined in dictionary "/media/syavash/science/PHD_Thesis/New/system/fvSchemes.divSchemes" file: /media/syavash/science/PHD_Thesis/New/system/fvSchemes.divSchemes from line 30 to line 36.     From function dictionary::lookupEntry(const word&, bool, bool) const     in file db/dictionary/dictionary.C at line 437. FOAM exiting```
I think modifying of fvScheme seems to be necessary. Could you tell me what actions should I make here?!

Thanks

All times are GMT -4. The time now is 00:49.