
[Sponsors] 
October 26, 2005, 09:07 
Hello,
Has someone implemen

#1 
Senior Member
Frank Bos
Join Date: Mar 2009
Location: The Netherlands
Posts: 340
Rep Power: 11 
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
__________________
Frank Bos 

December 16, 2009, 09:19 

#2 
New Member
Join Date: Nov 2009
Posts: 17
Rep Power: 9 
I'm also wondering if someone has rungekutta 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.


June 14, 2010, 12:07 

#3 
New Member
Michael B Martell Jr
Join Date: Feb 2010
Location: Amherst, MA
Posts: 18
Rep Power: 9 
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?


September 19, 2010, 16:56 
RungeKutta 4 to toplevel OpenFOAM

#4 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
Hi! I am currently working on compressible flows and writing a RK4 method to OpenFOAM. I am currently learning many things about toplevel 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 toplevel code. The following code (that can be put inside the main forloop 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 toplevel OF solvers. Regarding the previous question about an incompressible RK4 solver I do not see any problem of why the abovepresented approach for advection equation would not work also for the incompressible NSequations . Best regards, Ville 

September 20, 2010, 02:47 

#5  
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
Quote:
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,
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 20, 2010, 04:54 

#6 
Member
Juho Peltola
Join Date: Mar 2009
Location: Finland
Posts: 87
Rep Power: 10 

September 20, 2010, 10:26 

#7 
Senior Member
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,910
Rep Power: 28 
OK. Thanks for the info
__________________
Alberto Passalacqua GeekoCFD  A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as in both physical and virtual formats. OpenQBMM  An opensource implementation of quadraturebased moment methods. To obtain more accurate answers, please specify the version of OpenFOAM you are using. 

September 20, 2010, 10:46 

#8 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
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 OFpeople consider simply updating the boundary field in the toplevel 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 

October 31, 2012, 12:00 
RungeKutta 4 density based LES solver implemented

#9 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
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 ScaleSelective, Low Dissipative Discretization Scheme for the NavierStokes Equation, (to appear in Computers and Fluids) Best, Ville 

February 27, 2014, 03:29 
Publication: RungeKutta 4 method for compressible and incompressible flows

#10 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
Hi,
probably the first published paper on the topic including practical instructions on how to implement, theory, numerical validation On the implementation of lowdissipative RungeKutta projection methods for time dependent flows using OpenFOAM Vuorinen et al. http://www.sciencedirect.com/science...45793014000334 Best, Ville 

November 11, 2014, 09:27 
Fluid dynamical part of the code shown herein

#11 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
Largeeddy simulation in a complex hill terrain enabled by a compact fractional step OpenFOAMŪ solver
http://www.sciencedirect.com/science...65997814001513 Best wishes, Ville 

August 19, 2015, 15:46 

#12  
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 9 
Quote:
Is it possible to share your incompressible solver?! I am sure many people like me seek for an explicit lowdissipation solver for LESlike simulation. Syavash. 

August 20, 2015, 03:27 

#13 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
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 

August 20, 2015, 08:24 

#14  
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 9 
Quote:
I have proceeded as the steps in your paper have suggested, but I have encountered some problems in creating the new solver: 1The variables Uold, Uc, and dU are not defined, so I constructed them in createFields.H as volVectorField. Is it OK?! 2I have renamed pRef in CreatePoissonMatrix.H to pRefValue because the latter was defined in pisoFoam 3I 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. 4Where should I define a1,a2,a3, and a4? I have currently defined them simply as scalar at the beginning of the whileloop. At the moment the above issues come to my mind. I greatly appreciate if you help me compile the new solver. Thanks, Syavash 

August 20, 2015, 08:32 

#15 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
Hi,
>1Uold 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 ); >2I have renamed pRef in CreatePoissonMatrix.H to pRefValue because the latter >was defined in pisoFoam Sure >3I 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 >4Where should I define a1,a2,a3, and a4? I have currently defined them simply as >scalar at the beginning of the whileloop. 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 ? 

August 20, 2015, 08:48 

#16  
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 9 
Quote:
Now I am getting an error like this: Code:
syavash@syavashVPCF11DGX:~/OpenFOAM/OpenFOAM2.3.1/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 Wnounusedparameter Woldstylecast Wnonvirtualdtor O3 DNoRepository ftemplatedepth100 I/home/syavash/OpenFOAM/OpenFOAM2.3.1/src/turbulenceModels/incompressible/turbulenceModel I/home/syavash/OpenFOAM/OpenFOAM2.3.1/src/../applications/solvers/incompressible/pisoFoam I/home/syavash/OpenFOAM/OpenFOAM2.3.1/src/transportModels I/home/syavash/OpenFOAM/OpenFOAM2.3.1/src/transportModels/incompressible/singlePhaseTransportModel I/home/syavash/OpenFOAM/OpenFOAM2.3.1/src/finiteVolume/lnInclude IlnInclude I. I/home/syavash/OpenFOAM/OpenFOAM2.3.1/src/OpenFOAM/lnInclude I/home/syavash/OpenFOAM/OpenFOAM2.3.1/src/OSspecific/POSIX/lnInclude fPIC c $SOURCE o Make/linux64GccDPOpt/rk4projectionFoam.o In file included from rk4projectionFoam.C:58:0: /home/syavash/OpenFOAM/OpenFOAM2.3.1/src/finiteVolume/lnInclude/setDeltaT.H: In function ‘int main(int, char**)’: /home/syavash/OpenFOAM/OpenFOAM2.3.1/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/OpenFOAM2.3.1/src/finiteVolume/lnInclude/initContinuityErrs.H:37:8: warning: unused variable ‘cumulativeContErr’ [Wunusedvariable] scalar cumulativeContErr = 0; ^ make: *** [Make/linux64GccDPOpt/rk4projectionFoam.o] Error 1 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/OpenFOAM2.3.1/src/finiteVolume/lnInclude/initContinuityErrs.H:37:8: warning: unused variable ‘cumulativeContErr’ [Wunusedvariable] scalar cumulativeContErr = 0; Another question: Can I adjust time step by giving courant number as in pimpleFoam?! 

August 20, 2015, 09:06 

#17 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
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. 

August 20, 2015, 09:13 

#18  
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 9 
Quote:
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 

August 20, 2015, 09:25 

#19 
Member
ville vuorinen
Join Date: Mar 2009
Posts: 67
Rep Power: 10 
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. 

August 20, 2015, 10:14 

#20  
Senior Member
Ehsan Asgari
Join Date: Apr 2010
Posts: 311
Rep Power: 9 
Quote:
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 Thanks 

Thread Tools  
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Runge Kutta 4th Order Source Code  sugu  Main CFD Forum  4  October 26, 2012 03:15 
RungeKutta 4rd Order method help for 6DoF in CFD  siw  Main CFD Forum  0  August 29, 2008 06:08 
runge kutta  Shuo  Main CFD Forum  0  January 7, 2008 20:29 
4th and 5th Order TVD RungeKutta Methods  saygin  Main CFD Forum  2  January 30, 2006 12:45 
Runge Kutta vs adams bashforth time marching  vasanth  Main CFD Forum  5  January 1, 2006 01:17 