# Manual limiter of velocity doesn't work

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

 March 13, 2013, 07:40 Manual limiter of velocity doesn't work #1 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 6 Sponsored Links Hi to everyone guys! I'm experiencing this problem and I really don' t know what to do: I'm running with the solver adjointShapeOptimizationFoam, but now I'm trying to modify it a little, since sometimes the equations diverge. What I want to do is to use a manual limiter, that limits the value of the velocity in each cell if it raises too much, so I've inserted these lines at the bottom of the solver: forAll(Ua,cellI) { Ua[cellI].component(0)=min(Ua[cellI].component(0), 200); Ua[cellI].component(1)=min(Ua[cellI].component(1), 200); Ua[cellI].component(2)=min(Ua[cellI].component(2), 200); } forAll(Ua,cellJ) { Ua[cellJ].component(0)=max(Ua[cellJ].component(0), -200); Ua[cellJ].component(1)=max(Ua[cellJ].component(1), -200); Ua[cellJ].component(2)=max(Ua[cellJ].component(2), -200); } I'm expecting that these lines behave like a threshold value for each component of the velocity at each iteration, but I've run a simulation and I discovered that the values of the velocity were bigger than the range [-200:200]. Maybe the lines I've added are wrong? Any help is really appreciated. Thanks in advance Simone P.s. I'm running in parallel, but I hope this is not a problem for the code I've added.

 March 14, 2013, 03:22 #2 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 6 Please guy, is there someone that can help?

 March 14, 2013, 09:29 #3 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 You will need to limit the values on the patches also (all faces on patches) forAll(U.boundaryField(),patchI) { forAll(U.boundaryField()[patchI],faceI) { U.boundaryField()[patchI][faceI].component(0)=some value; } } Also your solver might adjust U values not only after solving momentum equation. So make sure that your are limiting after each calculation step of U

 March 15, 2013, 07:09 #4 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 6 Thank you Omkar! The problem was exactly on the patches, since I had forgotten to loop on them. By adding your lines now it seems to work perfectly.

 March 15, 2013, 07:46 #5 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 hi Simone I think limiting velocity can also resolve my problem. Could you send me your modified solver? Thanks.

 March 16, 2013, 18:29 #6 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 where should i add them exactly?

 March 17, 2013, 20:24 #7 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 can use velocity limiters only on a patch not entire the domain?

 March 17, 2013, 20:26 #8 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 hi Omkar Could you send me the code with added expressions for rhoPimpleFoam?

 March 17, 2013, 20:37 #9 Senior Member   Join Date: Nov 2009 Location: Michigan Posts: 135 Rep Power: 9 My code consists of combination of above two codes. Like I said, it did not work for me so I erased that code. The codes in this forum clearly explain how to limit velocity in the domain and the patches

March 18, 2013, 04:04
#10
Member

Simone
Join Date: Sep 2012
Posts: 95
Rep Power: 6
Hi immortality!
With respect to the adjointShapeOptimizationFoam solver, you should put the " two" limiter just above the lines

Quote:
 // Explicitly relax pressure for adjoint momentum corrector pa.relax(); // Adjoint momentum corrector Ua -= rAUa*fvc::grad(pa); Ua.correctBoundaryConditions();
into the predictor-corrector loop. At least, I did in this way!

If you want to "limit" only the patches you should insert only the lines that doubtsincfd suggested.

If, instead, you asked to limit only one specific patch you can use something like this:

Quote:
 word patchName = "NAME_OF_THE_PATCH"; label patchID = mesh.boundary().findPatchID(patchName2); forAll(U.boundaryField()[patchID],faceI) { U.boundaryField()[patchID][faceI].component(0)=some value; }
Hope this works

Simone

 March 19, 2013, 13:57 #11 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 thanks.where the codes should be added in rhoPimpleFoam? rhoPimpleFoam.C is this: Code: ```#include "fvCFD.H" #include "basicPsiThermo.H" #include "turbulenceModel.H" #include "bound.H" #include "pimpleControl.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // int main(int argc, char *argv[]) { #include "setRootCase.H" #include "createTime.H" #include "createMesh.H" pimpleControl pimple(mesh); #include "createFields.H" #include "initContinuityErrs.H" // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * // Info<< "\nStarting time loop\n" << endl; while (runTime.run()) { #include "readTimeControls.H" #include "compressibleCourantNo.H" #include "setDeltaT.H" runTime++; Info<< "Time = " << runTime.timeName() << nl << endl; #include "rhoEqn.H" // --- Pressure-velocity PIMPLE corrector loop while (pimple.loop()) { #include "UEqn.H" #include "hEqn.H" // --- Pressure corrector loop while (pimple.correct()) { #include "pEqn.H" } if (pimple.turbCorr()) { turbulence->correct(); } } runTime.write(); Info<< "ExecutionTime = " << runTime.elapsedCpuTime() << " s" << " ClockTime = " << runTime.elapsedClockTime() << " s" << nl << endl; } Info<< "End\n" << endl; return 0; } // ************************************************************************* //``` where UEqn.H is: Code: ```// Solve the Momentum equation tmp UEqn ( fvm::ddt(rho, U) + fvm::div(phi, U) + turbulence->divDevRhoReff(U) ); UEqn().relax(); volScalarField rAU(1.0/UEqn().A()); if (pimple.momentumPredictor()) { solve(UEqn() == -fvc::grad(p)); K = 0.5*magSqr(U); }``` hEqn.H: Code: ```{ fvScalarMatrix hEqn ( fvm::ddt(rho, h) + fvm::div(phi, h) - fvm::laplacian(turbulence->alphaEff(), h) == dpdt - (fvc::ddt(rho, K) + fvc::div(phi, K)) ); hEqn.relax(); hEqn.solve(); thermo.correct(); }``` pEqn.H: Code: ```rho = thermo.rho(); rho = max(rho, rhoMin); rho = min(rho, rhoMax); rho.relax(); U = rAU*UEqn().H(); if (pimple.nCorrPISO() <= 1) { UEqn.clear(); } if (pimple.transonic()) { surfaceScalarField phid ( "phid", fvc::interpolate(psi) *( (fvc::interpolate(U) & mesh.Sf()) + fvc::ddtPhiCorr(rAU, rho, U, phi) ) ); while (pimple.correctNonOrthogonal()) { fvScalarMatrix pEqn ( fvm::ddt(psi, p) + fvm::div(phid, p) - fvm::laplacian(rho*rAU, p) ); pEqn.solve(mesh.solver(p.select(pimple.finalInnerIter()))); if (pimple.finalNonOrthogonalIter()) { phi == pEqn.flux(); } } } else { phi = fvc::interpolate(rho)* ( (fvc::interpolate(U) & mesh.Sf()) + fvc::ddtPhiCorr(rAU, rho, U, phi) ); while (pimple.correctNonOrthogonal()) { // Pressure corrector fvScalarMatrix pEqn ( fvm::ddt(psi, p) + fvc::div(phi) - fvm::laplacian(rho*rAU, p) ); pEqn.solve(mesh.solver(p.select(pimple.finalInnerIter()))); if (pimple.finalNonOrthogonalIter()) { phi += pEqn.flux(); } } } #include "rhoEqn.H" #include "compressibleContinuityErrs.H" // Explicitly relax pressure for momentum corrector p.relax(); // Recalculate density from the relaxed pressure rho = thermo.rho(); rho = max(rho, rhoMin); rho = min(rho, rhoMax); rho.relax(); Info<< "rho max/min : " << max(rho).value() << " " << min(rho).value() << endl; U -= rAU*fvc::grad(p); U.correctBoundaryConditions(); K = 0.5*magSqr(U); dpdt = fvc::ddt(p);```

 March 21, 2013, 07:06 #12 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 6 In my opinion after Code: ```if (pimple.turbCorr()) { turbulence->correct(); }``` should be fine.

 March 26, 2013, 08:57 #13 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 thank you dear Simone for your help so I added it.is it correct?why you have wrote patchName2 in findPatchID? I put U[cellI] instead of Ua[cellI] due to use in rhoPimpleFoam does it have any problem? I want not to let U becomes higher than sound speed(flow should be subsonic) will it be true that I write sqrt(1.4*287.14*T[cellI]) instead of 500 I have put now? I want to be certain to compile the modified solver. thanks again. Code: ```word patchName = "left"; label patchID = mesh.boundary().findPatchID(patchName); forAll(U.boundaryField()[patchID],faceI) { U.boundaryField()[patchID][faceI].component(0)=min(U[cellI].component(0), 500); }```

 March 26, 2013, 11:49 #14 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 I used it for the patch.but velocity in cells near the inflow boundary are supersonic. where I add the expressions to limit velocity on top of domain? and what do you mean from cellI and cellJ in this expressions: forAll(Ua,cellI) { Ua[cellI].component(0)=min(Ua[cellI].component(0), 200); Ua[cellI].component(1)=min(Ua[cellI].component(1), 200); Ua[cellI].component(2)=min(Ua[cellI].component(2), 200); } forAll(Ua,cellJ) { Ua[cellJ].component(0)=max(Ua[cellJ].component(0), -200); Ua[cellJ].component(1)=max(Ua[cellJ].component(1), -200); Ua[cellJ].component(2)=max(Ua[cellJ].component(2), -200); }

 March 27, 2013, 10:59 #15 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 6 You have to put those line before the ones to limit the boundary. cellI and cellJ are two (unuseful) different counters. You can use the same for both cycles. immortality likes this.

 March 27, 2013, 11:20 #16 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 thank you dear Simone again is this correct now?: Code: ```forAll(U,cellI) { U[cellI].component(0)=min(U[cellI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30); } forAll(U,cellJ) { U[cellJ].component(1)=max(U[cellI].component(1),-150); } word patchName = "left"; label patchID = mesh.boundary().findPatchID(patchName); forAll(U.boundaryField()[patchID],faceI) { U.boundaryField()[patchID][faceI].component(0)=min(U.boundaryField()[patchID][faceI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30); U.boundaryField()[patchID][faceI].component(1)=max(U.boundaryField()[patchID][faceI].component(1),-150); }``` another question! could we do both loops into single one by for instance I counter? thanks.

 March 27, 2013, 11:29 #17 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 when compiled it this error occurred: Code: ```ehsan@Ehsan-com:~/Desktop/rhoPimpleFoamLimited\$ wmakeMaking dependency list for source file rhoPimpleFoamLimited.C SOURCE=rhoPimpleFoamLimited.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam211/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam211/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam211/src/finiteVolume/cfdTools -I/opt/openfoam211/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam211/src/OpenFOAM/lnInclude -I/opt/openfoam211/src/OSspecific/POSIX/lnInclude -fPIC -c \$SOURCE -o Make/linux64GccDPOpt/rhoPimpleFoamLimited.o rhoPimpleFoamLimited.C: In function ‘int main(int, char**)’: rhoPimpleFoamLimited.C:90:79: error: ‘Foam::T’ does not have class type rhoPimpleFoamLimited.C:90:96: error: ‘patchID’ was not declared in this scope rhoPimpleFoamLimited.C:90:105: error: ‘faceI’ was not declared in this scope rhoPimpleFoamLimited.C:94:41: error: name lookup of ‘cellI’ changed for ISO ‘for’ scoping [-fpermissive] rhoPimpleFoamLimited.C:94:41: note: (if you use ‘-fpermissive’ G++ will accept your code) rhoPimpleFoamLimited.C:100:132: error: ‘Foam::T’ does not have class type make: *** [Make/linux64GccDPOpt/rhoPimpleFoamLimited.o] Error 1``` whats error in T?

 March 27, 2013, 11:30 #18 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 6 Actually I don't know if OF will allow you such a statement: Code: ```U[cellI].component(0)= min(U[cellI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30);``` since you are looping inside the domain for the component of U you can't assign its value with respect to the value of the temperature on the boundary! I don't know if you can use something like this: Code: ```U[cellI].component(0)= min(U[cellI].component(0), sqrt(1.4*287.14*T.[cellI])-30);``` You could try with the line above if I understand well your intention, i.e. you want to threshold the value of the velocity with respect to the local value of the Mach number. Hope this help. immortality likes this.

 March 27, 2013, 11:37 #19 Senior Member     Ehsan Join Date: Oct 2012 Location: Iran Posts: 2,210 Rep Power: 19 thank you. yes Simone you understood well. I modified it as so: Code: ```forAll(U,cellI) { U[cellI].component(0)=min(U[cellI].component(0), sqrt(1.4*287.14*T.[cellI])-30); } forAll(U,cellJ) { U[cellJ].component(1)=max(U[cellI].component(1),-150); } word patchName = "left"; label patchID = mesh.boundary().findPatchID(patchName); forAll(U.boundaryField()[patchID],faceI) { U.boundaryField()[patchID][faceI].component(0)=min(U.boundaryField()[patchID][faceI].component(0), sqrt(1.4*287.14*T.boundaryField()[patchID][faceI])-30); U.boundaryField()[patchID][faceI].component(1)=max(U.boundaryField()[patchID][faceI].component(1),-150); }``` but this error is shown: Code: ```ehsan@Ehsan-com:~/Desktop/rhoPimpleFoamLimited\$ wmakeMaking dependency list for source file rhoPimpleFoamLimited.C SOURCE=rhoPimpleFoamLimited.C ; g++ -m64 -Dlinux64 -DWM_DP -Wall -Wextra -Wno-unused-parameter -Wold-style-cast -Wnon-virtual-dtor -O3 -DNoRepository -ftemplate-depth-100 -I/opt/openfoam211/src/thermophysicalModels/basic/lnInclude -I/opt/openfoam211/src/turbulenceModels/compressible/turbulenceModel -I/opt/openfoam211/src/finiteVolume/cfdTools -I/opt/openfoam211/src/finiteVolume/lnInclude -IlnInclude -I. -I/opt/openfoam211/src/OpenFOAM/lnInclude -I/opt/openfoam211/src/OSspecific/POSIX/lnInclude -fPIC -c \$SOURCE -o Make/linux64GccDPOpt/rhoPimpleFoamLimited.o rhoPimpleFoamLimited.C: In function ‘int main(int, char**)’: rhoPimpleFoamLimited.C:90:79: error: ‘Foam::T’ does not have class type rhoPimpleFoamLimited.C:90:96: error: ‘patchID’ was not declared in this scope rhoPimpleFoamLimited.C:90:105: error: ‘faceI’ was not declared in this scope rhoPimpleFoamLimited.C:94:41: error: name lookup of ‘cellI’ changed for ISO ‘for’ scoping [-fpermissive] rhoPimpleFoamLimited.C:94:41: note: (if you use ‘-fpermissive’ G++ will accept your code) rhoPimpleFoamLimited.C:100:132: error: ‘Foam::T’ does not have class type make: *** [Make/linux64GccDPOpt/rhoPimpleFoamLimited.o] Error 1```

 March 27, 2013, 11:40 #20 Member   Simone Join Date: Sep 2012 Posts: 95 Rep Power: 6 it's Code: `T[cellI]` not Code: `T.[cellI]`

 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 Zaqie Fluent UDF and Scheme Programming 9 June 25, 2016 19:08 houkensjtu OpenFOAM 4 October 8, 2012 04:41 zumaqiong Fluent UDF and Scheme Programming 12 March 25, 2010 13:00 Antech Main CFD Forum 0 April 25, 2006 02:15 chong chee nan FLUENT 0 December 29, 2001 06:13