Local time step

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

 June 16, 2011, 02:23 Local time step #1 New Member   Join Date: Aug 2010 Location: Chennai Posts: 27 Rep Power: 8 I want to use local time steps to converge to steady state quickly. I have fixed the maxCo and want to calculate deltaT for each cell (local time step). My Openfoam rho (for e.g.) equation reads : rho = rho - runTime.deltaT()*fvc::div(phi); ...... I checked setDelta.H, compressibleCourantNo.H which tells runTime.deltaT() as a scalar. But I want a runtime.deltaT() as volScalarField which has delta time defined for each cell. Can anyone help me in this regard

 June 16, 2011, 11:10 #2 Senior Member   David Gaden Join Date: Apr 2009 Location: Winnipeg, Canada Posts: 436 Rep Power: 14 The runTime scalar is used in the fvc and fvm namespaces in the discretization process. If you want to have any of these functions work with the local time, then you are looking at a complex problem. If, on the other hand, you just want to store a "local time" field that you use independently, that would be much easier. How do you plan to use the local time?

 June 16, 2011, 14:16 #3 New Member   Join Date: Aug 2010 Location: Chennai Posts: 27 Rep Power: 8 " If, on the other hand, you just want to store a "local time" field that you use independently, that would be much easier" Exactly the second one. A false time field just to update rho,rhoU and rhoE For e.g. rho = rho - runTime.deltaT()*fvc::div(phi) rhoU = rhoU - ... rhoE = rhoE - ... runTime.deltaT() is very local (or which only plays around setDelta.H, readTimecontrols.H and compressibleCourantNumber.H) and nothing to do with ddt schemes I specify. (whatever ddtscheme in the fvSchemesDict) & Hopefully, I didn't confuse you Thanks, hari

 June 16, 2011, 14:43 #4 Senior Member   Sandeep Menon Join Date: Mar 2009 Location: Amherst, MA Posts: 387 Rep Power: 16 Take a look at the SLTSDdtScheme in \$(FOAM_SRC)/finiteVolume/ddtSchemes/SLTSDdtScheme __________________ Sandeep Menon University of Massachusetts Amherst https://github.com/smenon

 June 17, 2011, 04:02 #5 Senior Member     Anton Kidess Join Date: May 2009 Location: Delft, Netherlands Posts: 1,152 Rep Power: 20 Also, the just released new version of OpenFoam uses a local time step for their new VOF solver: http://www.openfoam.com/version2.0.0/steady-vof.php You might want to have a look at that. sharonyue and Thamali like this.

 July 6, 2011, 09:37 #6 New Member   Join Date: Aug 2010 Location: Chennai Posts: 27 Rep Power: 8 Dear all, ( Please check the previous posts in this thread to have an idea) I have slightly modified the inviscid solver rhoCentralFoam in order to improve the acceleration to steady state using local time step without touching any other part (e.g. reconstruct(). - flux calculations). And it seems working for my case. If anyone have a word/doubt in my modification please post it. //////////Local time step - false time step forAll (mesh.C(),i) { cell faces = mesh.cells()[i]; denom = 0.0; forAll (faces,j) { denom = denom + ( (U[i] & mesh.Sf()[j]) + c[i]*mesh.magSf()[j] ); } falseTime[i] = maxCo * mesh.V()[i] / denom; } //////// Conservation equations // --- Solve density rho = rho - falseTime*fvc::div(phi); // --- Solve momentum rhoU = rhoU - falseTime*fvc::div(phiUp); // --- Solve energy rhoE = rhoE - falseTime*fvc::div(phiEp); mm.abdollahzadeh likes this.

 January 9, 2012, 14:49 #7 Member   Eric M. Tridas Join Date: May 2011 Location: Tampa, Florida Posts: 48 Rep Power: 7 Has anyone else done this? I'm really interested in speeding up my rhoCentralFoam simulations but am having some trouble implementing it. I'd really appreciate the help anyone else can give! Thanks, -Eric

 March 25, 2012, 11:19 #8 Senior Member   ehsan Join Date: Mar 2009 Posts: 106 Rep Power: 9 Dear all I need a reference which describes by more details the new local-time stepping (LTS) approach applied in VOF in openfoam. Thanks

October 7, 2012, 12:23
#9
Senior Member

Join Date: Mar 2011
Location: Covilha,Portugal
Posts: 150
Rep Power: 7
Quote:
 Originally Posted by ramhari Dear all, ( Please check the previous posts in this thread to have an idea) I have slightly modified the inviscid solver rhoCentralFoam in order to improve the acceleration to steady state using local time step without touching any other part (e.g. reconstruct(). - flux calculations). And it seems working for my case. If anyone have a word/doubt in my modification please post it. //////////Local time step - false time step forAll (mesh.C(),i) { cell faces = mesh.cells()[i]; denom = 0.0; forAll (faces,j) { denom = denom + ( (U[i] & mesh.Sf()[j]) + c[i]*mesh.magSf()[j] ); } falseTime[i] = maxCo * mesh.V()[i] / denom; } //////// Conservation equations // --- Solve density rho = rho - falseTime*fvc::div(phi); // --- Solve momentum rhoU = rhoU - falseTime*fvc::div(phiUp); // --- Solve energy rhoE = rhoE - falseTime*fvc::div(phiEp);

Dear Friend

There is one question:

the falsetime that you are calculating is the local deltaT. so its changing from cell to cell.
so its almost the same as the local euler or coeuler scheme in openfoam?

secondly this scheme is not giving unsteady result. just the final result could be correct?

How can u access the simulationtime? how you will control writting the variables according the controldict writecontrol ( considering that u have local time )

Best
Mahdi

 September 27, 2015, 12:24 #10 New Member   Pravin Kadu Join Date: Jun 2015 Posts: 3 Rep Power: 3 Dear friend, Can you please provide the 'local time stepping' related theory. Because I am not getting that how the cells will have different time steps, since they would be interdependent? Thanks.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post richard OpenFOAM Running, Solving & CFD 167 June 18, 2016 06:04 pUl| FLUENT 31 August 21, 2015 04:46 msrinath80 OpenFOAM Running, Solving & CFD 18 March 3, 2015 06:36 lr103476 OpenFOAM Running, Solving & CFD 30 November 19, 2007 15:09 skabilan OpenFOAM Running, Solving & CFD 12 September 17, 2007 17:48

All times are GMT -4. The time now is 11:55.