
[Sponsors] 
What exactly the Relaxation factor does? 

LinkBack  Thread Tools  Search this Thread  Display Modes 
June 18, 2019, 11:27 
What exactly the Relaxation factor does?

#1 
Senior Member
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 7 
Hello Everyone,
I have few questions related to relaxation factor 1. What is the relaxation factor? 2. How it helps in the simulation of our case? 3. Based on what, we modify the relaxation factor for each parameter? I searched for these doubts, but couldn't find much about it. I shall be thankful, if someone can guide me through this. Thank you 

June 19, 2019, 16:05 

#2 
Senior Member
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,907
Rep Power: 33 
Pick up the old book by Patankar  he explains it well
__________________
Hrvoje Jasak Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk 

June 20, 2019, 04:20 

#3 
Member
Ingo Riess
Join Date: Jun 2019
Location: Switzerland
Posts: 40
Rep Power: 7 
A second subdictionary of fvSolution that is often used in OpenFOAM is relaxationFactors which controls underrelaxation, a technique used for improving stability of a computation, particularly in solving steadystate problems. Underrelaxation works by limiting the amount which a variable changes from one iteration to the next, either by modifying the solution matrix and source prior to solving for a field or by modifying the field directly. An underrelaxation factor α,0 < α ≤ 1 specifies the amount of underrelaxation.


June 21, 2019, 04:23 

#4 
Senior Member
Zander Meiring
Join Date: Jul 2018
Posts: 125
Rep Power: 8 
To follow on from the above the relaxation factor blends the previous iteration's solution and the current iteration's solution. If the factor is 1, then the new solution is entirely used, if the relaxation factor is 0, the old solution is entirely used. A simple example of a single cell could be:
iteration 1: p = 10 iteration 2: p is found to be 30, but relaxation factor is 0.6. So P = 0.6(30)+0.4(10) = 22 It's use is to ensure that the solution does not change too wildly between iterations, which could cause instability else wise. Theoretically, as the solution converges, the difference in the answer between two iterations are minimal, and so the effect the relaxation factor has also becomes minimal. Therefor it shouldn't interfere with the answer of the final solution. It may, however, cause the solution to take more iterations to converge, as you are telling the cfd code to change less between each iteration. It is therefor ideal to find a relaxation factor that is as large as possible, whilst causing a converging and stable solution 

June 21, 2019, 05:18 

#5  
Senior Member
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 7 
Quote:
Hi, Indeed, it is an excellent explanation of relaxation factor. Thank you so much. Regards, Raza 

July 1, 2019, 04:35 

#6  
Senior Member
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 7 
Quote:
Hi, I have one more question: Can we change the relaxation factor while running the simulation? Thank you 

July 1, 2019, 05:32 

#7 
Senior Member
Joachim Herb
Join Date: Sep 2010
Posts: 650
Rep Power: 22 
Yes, you can change it during runtime and it will be applied in the next time step (if you have set runTimeModifiable true; in system/controlDict)


July 1, 2019, 06:09 

#8  
Senior Member
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 7 
Quote:
Hi, Thank you so much for your reply. Actually I am having a problem of "maximum number of iterations exceeded" error in my simulation. When I reduce the relaxation factor from 0.7 to 1e3 or 1e4, then the solver RUNS for longer time but at the end it again gives the same error and stops. I try to explain my case, may be you can help. I am using chtMultiRegionSimpleFoam with OpenFoam 4.1. my geomtetry has multiple regions (a box containing some heaters and one fluid region). There is turbulent flow in the fluid region and its compressible also. I am using kEpsilon model. Now, during the flow from inlet to outlet, the fluid should get heat up due to the heaters and the temperature of fluid at the outlet should be equal to the heat transferred from heaters to fluid. After some iterations, the temperature of fluid becomes unrealistic and the solver stops. The strange thing is that, for the same case, I have one another geometry, the only difference is that the other geometry the fluid region is straight, and in the first geometry, the fluid region has multiple curves in it. And for the straight pipe geometry, everything is working fine. The only different thing in both these cases, is the geometry, everything else is same (boundary conditions, initial conditions, thermophysical properties etc.) Can you please help me, that what could be the possible reasons for this error. The error is also attached below: Code:
> FOAM FATAL ERROR: [3] Maximum number of iterations exceeded [3] [3] From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie> >, Foam::sensibleEnthalpy>] [3] in file /home/ubuntu/OpenFOAM/OpenFOAM4.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66. [3] FOAM parallel run aborting [3] [3] #0 Foam::error::printStack(Foam::Ostream&) at ??:? [3] #1 Foam::error::abort() at ??:? [3] #2 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() at ??:? [3] #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() at ??:? [3] #4 ? at ??:? [3] #5 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" [3] #6 ? at ??:?  MPI_ABORT was invoked on rank 3 in communicator MPI_COMM_WORLD with errorcode 1. NOTE: invoking MPI_ABORT causes Open MPI to kill all MPI processes. You may or may not see output from other processes, depending on exactly when Open MPI kills them.  Thank you 

July 1, 2019, 19:27 

#9 
Senior Member
Joachim Herb
Join Date: Sep 2010
Posts: 650
Rep Power: 22 
Relaxation factors in the order of magnitude of 1e3 sound very wrong. There are probably other problems with your simulation.
Does checkMesh complain about something? Are you sure, your boundary conditions are physically valid? 

July 2, 2019, 04:26 

#10 
Senior Member
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 7 
Thank you so much for your reply.
I am attaching my checkMesh below and it seems OK, but can you please have a look. Code:
Create time Create polyMesh for time = 0 Time = 0 Mesh stats points: 1875576 faces: 21909869 internal faces: 21895815 cells: 10951421 faces per cell: 4 boundary patches: 3 point zones: 0 face zones: 0 cell zones: 10 Overall number of cells of each type: hexahedra: 0 prisms: 0 wedges: 0 pyramids: 0 tet wedges: 0 tetrahedra: 10951421 polyhedra: 0 Checking topology... Boundary definition OK. Cell to face addressing OK. Point usage OK. Upper triangular ordering OK. Face vertices OK. Number of regions: 1 (OK). Checking patch topology for multiply connected surfaces... Patch Faces Points Surface topology inlet 264 164 ok (nonclosed singly connected) outlet 234 149 ok (nonclosed singly connected) defaultFaces 13556 6840 ok (nonclosed singly connected) Checking geometry... Overall domain bounding box (0.140981 0.096774 0) (0.132 0.096774 0.03) Mesh has 3 geometric (nonempty/wedge) directions (1 1 1) Mesh has 3 solution (nonempty) directions (1 1 1) Boundary openness (2.35742e18 3.2066e18 8.15718e17) OK. Max cell openness = 2.85893e16 OK. Max aspect ratio = 10.056 OK. Minimum face area = 5.60659e08. Maximum face area = 3.6484e05. Face area magnitudes OK. Min volume = 7.32683e12. Max volume = 4.43234e08. Total volume = 0.00158505. Cell volumes OK. Mesh nonorthogonality Max: 64.003 average: 15.2411 Nonorthogonality check OK. Face pyramids OK. Max skewness = 0.885953 OK. Coupled point location match (average 0) OK. Mesh OK. End I tried putting boundary conditions according to my requirement, but I am not sure either they are correct or NOT. I want to have the velocity of 1.33 at inlet, and also as an initial value. For outlet, I don't have any specification for velocity, so I put zeroGradient. Temperature: at inlet I defined 300K, and at outlet I need to check the temperature(should be higher compared to inlet due to the heaters outside the fluid region). But for alphat, k, epsilon and nut I have put boundary conditions from tutorials, but I am not sure about them. I am attaching my boundary conditions below: Code:
boundary { inlet { type patch; } outlet { type patch; } } T { internalField uniform 300; boundaryField { inlet { type fixedValue; value $internalField; } outlet { type zeroGradient; } "fluid_to_box" { type compressible::turbulentTemperatureCoupledBaffleMixed; Tnbr T; kappaMethod fluidThermo; value uniform 300; } } } U { internalField uniform (1.33 0 0); boundaryField { inlet { type fixedValue; value uniform (1.33 0 0); } outlet { type zeroGradient; } "fluid_to_box" { type noSlip; } } } epsilon { internalField uniform 0.064; boundaryField { inlet { type fixedValue; value uniform 0.064; } outlet { type zeroGradient; } ".*" { type epsilonWallFunction; value uniform 0.064; } } } k { internalField uniform 2.45e3; boundaryField { inlet { type fixedValue; value uniform 2.45e3; } outlet { type zeroGradient; //value uniform 0; } "fluid_to_box" { type kqRWallFunction; value uniform 2.45e3; } } } p_rgh { internalField uniform 0; boundaryField { inlet { type zeroGradient; value uniform 0; } outlet { type fixedValue; value uniform 0; } ".*" { type fixedFluxPressure; value uniform 0; } } } p { internalField uniform 100000; boundaryField { ".*" { type calculated; value $internalField; } } } alphat { internalField uniform 0; boundaryField { inlet { type calculated; value uniform 0; } outlet { type calculated; value uniform 0; } "fluid_to_box" { type compressible::alphatWallFunction; } } } nut { internalField uniform 0; boundaryField { inlet { type calculated; value uniform 0; } outlet { type calculated; value uniform 0; } "fluid_to_box" { type nutkWallFunction; value uniform 0; } } } // ************************************************************************* // I shall be very thankful, if you can guide me through this. Thank you 

July 2, 2019, 04:31 

#11 
Senior Member
Joachim Herb
Join Date: Sep 2010
Posts: 650
Rep Power: 22 
One thing is probably not correct. You use chtMultiRegionSimpleFoam? Then you need to set a physically correct pressure, because it is a "compressible" solver, calculating the density from some equation of state. So p = 0 at the outlet cannot be correct.
Actually, what is the message of the solver, when it crashes? 

July 2, 2019, 04:42 

#12  
Senior Member
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 7 
Quote:
I am putting pressure (p) equals to calculated on all boundaries, but yes p_rgh, I am putting zero at outlet. Do I need to change the boundary conditions for p_rgh? The log file of the solver is given below: Code:
Time = 0.1 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.00248155, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.00420011, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.00300392, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.999619, Final residual = 0.00174638, No Iterations 1 Min/max T:299.968 300.002 GAMG: Solving for p_rgh, Initial residual = 1, Final residual = 0.0294703, No Iterations 10 time step continuity errors : sum local = 1833.44, global = 63.8567, cumulative = 63.8567 Min/max rho:1000 1000 DILUPBiCG: Solving for epsilon, Initial residual = 0.0127737, Final residual = 1.03336e05, No Iterations 1 bounding epsilon, min: 6.47425 max: 198.948 average: 0.11565 DILUPBiCG: Solving for k, Initial residual = 1, Final residual = 0.00132192, No Iterations 1 bounding k, min: 0.0598646 max: 1.36506 average: 0.00247787 Solving for solid region box DICPCG: Solving for h, Initial residual = 0.999899, Final residual = 0.0537438, No Iterations 2 Min/max T:299.999 300 Solving for solid region p1 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0154276, No Iterations 2 Min/max T:300 300.056 Solving for solid region p2 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0150834, No Iterations 2 Min/max T:300 300.044 Solving for solid region p3 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0139625, No Iterations 2 Min/max T:300 300.056 Solving for solid region p4 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0142509, No Iterations 2 Min/max T:300 300.047 Solving for solid region p5 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0159586, No Iterations 2 Min/max T:300 300.049 Solving for solid region p6 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0153529, No Iterations 2 Min/max T:300 300.056 Solving for solid region p7 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0134462, No Iterations 2 Min/max T:300 300.05 Solving for solid region p8 DICPCG: Solving for h, Initial residual = 1, Final residual = 0.0144757, No Iterations 2 Min/max T:300 300.053 ExecutionTime = 133.06 s ClockTime = 134 s Time = 0.2 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 0.504383, Final residual = 0.00162629, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 0.300932, Final residual = 0.00101981, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 0.270728, Final residual = 0.000718876, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 0.316352, Final residual = 0.000658972, No Iterations 1 Min/max T:299.961 300.002 GAMG: Solving for p_rgh, Initial residual = 0.776721, Final residual = 0.0236817, No Iterations 10 time step continuity errors : sum local = 2063.36, global = 36.928, cumulative = 100.785 Min/max rho:1000 1000 DILUPBiCG: Solving for epsilon, Initial residual = 0.480833, Final residual = 6.92497e05, No Iterations 1 bounding epsilon, min: 102.556 max: 5835.89 average: 0.137401 DILUPBiCG: Solving for k, Initial residual = 0.844893, Final residual = 0.000528436, No Iterations 1 bounding k, min: 0.451503 max: 51.2525 average: 0.00274481 Solving for solid region box DICPCG: Solving for h, Initial residual = 0.9999, Final residual = 0.02301, No Iterations 2 Min/max T:299.993 300.015 Solving for solid region p1 DICPCG: Solving for h, Initial residual = 0.689583, Final residual = 0.00986339, No Iterations 2 Min/max T:300.006 300.096 Solving for solid region p2 DICPCG: Solving for h, Initial residual = 0.698901, Final residual = 0.00942908, No Iterations 2 Min/max T:300.006 300.078 Solving for solid region p3 DICPCG: Solving for h, Initial residual = 0.679693, Final residual = 0.00839357, No Iterations 2 Min/max T:300.005 300.1 Solving for solid region p4 DICPCG: Solving for h, Initial residual = 0.692854, Final residual = 0.00897344, No Iterations 2 Min/max T:300.006 300.085 Solving for solid region p5 DICPCG: Solving for h, Initial residual = 0.686304, Final residual = 0.0101575, No Iterations 2 Min/max T:300.006 300.088 Solving for solid region p6 DICPCG: Solving for h, Initial residual = 0.68812, Final residual = 0.00966565, No Iterations 2 Min/max T:300.006 300.099 Solving for solid region p7 DICPCG: Solving for h, Initial residual = 0.696385, Final residual = 0.00854814, No Iterations 2 Min/max T:300.006 300.09 Solving for solid region p8 DICPCG: Solving for h, Initial residual = 0.693705, Final residual = 0.00922509, No Iterations 2 Min/max T:300.007 300.095 ExecutionTime = 145.92 s ClockTime = 147 s Time = 0.3 Solving for fluid region fluid DILUPBiCG: Solving for Ux, Initial residual = 1, Final residual = 0.00696453, No Iterations 1 DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 0.00537407, No Iterations 1 DILUPBiCG: Solving for Uz, Initial residual = 1, Final residual = 0.00773095, No Iterations 1 DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.00227395, No Iterations 1 [3] [3] [3] > FOAM FATAL ERROR: [3] Maximum number of iterations exceeded [3] [3] From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie> >, Foam::sensibleEnthalpy>] [3] in file /home/ubuntu/OpenFOAM/OpenFOAM4.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66. [3] FOAM parallel run aborting [3] [3] #0 Foam::error::printStack(Foam::Ostream&) at ??:? [3] #1 Foam::error::abort() at ??:? [3] #2 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() at ??:? [3] #3 Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::polynomialTransport<Foam::species::thermo<Foam::hPolynomialThermo<Foam::icoPolynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() at ??:? [3] #4 ? at ??:? [3] #5 __libc_start_main in "/lib/x86_64linuxgnu/libc.so.6" [3] #6 ? at ??:?  please let me know if you need any further information. Thank you 

Tags 
openfoam, relaxation factor 
Thread Tools  Search this Thread 
Display Modes  


Similar Threads  
Thread  Thread Starter  Forum  Replies  Last Post 
Lets talk about relaxation factor optimization  chriss85  OpenFOAM Running, Solving & CFD  35  June 21, 2019 10:54 
Long output in terminal.  ssa_cfd  OpenFOAM Running, Solving & CFD  1  March 18, 2019 06:25 
About equation relaxation  chriss85  OpenFOAM Running, Solving & CFD  1  May 2, 2017 20:52 
Relaxation and convergence  sammi  Phoenics  0  March 20, 2008 04:32 
Question on adjusting relaxation factor  CFD Rookie  Main CFD Forum  3  January 26, 2004 15:37 