|
[Sponsors] |
No Convergence for High Viscosity (simpleFoam, Steady-State) |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
S03r3n
Join Date: Feb 2024
Posts: 15
Rep Power: 2 ![]() |
Hello togehter,
I have the issue that my simulation (simpleFoam, steady-state) converges for the case of low viscosity, but no convergence for high viscosity. What can be the reason? Solver related? For more details, here are the viscosity models: - Low viscosity Code:
transportModel BirdCarreau; nuInf [0 2 -1 0 0 0 0] 0; nu0 [0 2 -1 0 0 0 0] 37.521; k [0 0 1 0 0 0 0] 0.25011; n [0 0 0 0 0 0 0] 0.11815; a [0 0 0 0 0 0 0] 1; Code:
transportModel BirdCarreau; nuInf [0 2 -1 0 0 0 0] 0; nu0 [0 2 -1 0 0 0 0] 433.2756; k [0 0 1 0 0 0 0] 6.017543; n [0 0 0 0 0 0 0] 0.1327432; a [0 0 0 0 0 0 0] 1; Below you can find my chosen solver settings and the mesh quality. controlDict Code:
application simpleFoam; startFrom startTime; startTime 0; stopAt endTime; endTime 3000; deltaT 1; writeControl timeStep; writeInterval 100; purgeWrite 1; writeFormat ascii; writePrecision 6; writeCompression off; timeFormat general; timePrecision 6; runTimeModifiable true; Code:
ddtSchemes { default steadyState; } gradSchemes { default Gauss linear; } divSchemes { default none; div(phi,U) bounded Gauss linearUpwind grad(U); div((nuEff*dev2(T(grad(U))))) Gauss linear; } laplacianSchemes { default Gauss linear corrected; } interpolationSchemes { default linear; } snGradSchemes { default corrected; } Code:
solvers { p { solver GAMG; tolerance 1e-10; relTol 0.1; smoother GaussSeidel; } U { solver smoothSolver; smoother GaussSeidel; tolerance 1e-10; relTol 0.1; } } SIMPLE { nNonOrthogonalCorrectors 0; } relaxationFactors { fields { p 0.3; } equations { U 0.7; } } Code:
Checking geometry... Overall domain bounding box (-0.045 -0.045 -3.28327e-06) (0.045 0.045 0.396003) Mesh has 3 geometric (non-empty/wedge) directions (1 1 1) Mesh has 3 solution (non-empty) directions (1 1 1) Boundary openness (-3.07219e-15 2.25183e-15 -7.41942e-17) OK. Max cell openness = 4.00758e-16 OK. Max aspect ratio = 9.9936 OK. Minimum face area = 1.77711e-09. Maximum face area = 5.09394e-05. Face area magnitudes OK. Min volume = 4.96432e-13. Max volume = 1.40176e-07. Total volume = 0.00177843. Cell volumes OK. Mesh non-orthogonality Max: 65.1136 average: 13.681 Non-orthogonality check OK. Face pyramids OK. ***Max skewness = 8.30373, 25 highly skew faces detected which may impair the quality of the results <<Writing 25 skew faces to set skewFaces Coupled point location match (average 0) OK. Failed 1 mesh checks. |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Senior Member
Join Date: Dec 2021
Posts: 230
Rep Power: 5 ![]() |
Hey,
Your mesh has some flaws that might be affecting your case, like non-orthogonal and skewed cells. You should configure fvSchemes and fvSolutions accordingly. Try to set nNonOrthogonalCorrectors to 1 or even 2, and use limited 0.33 for snGradSchemes and Gauss linear limited 0.33 for the laplacian. Instead of Gauss linear for the gradient scheme, leastSquares can handle skewed cells a bit better from what I have read. Limiters can also help for the gradient schemes, for instance grad(U) cellLimited Gauss linear 1; and use first order for divergence schemes as long as the simulation is not stable. If you can, ramp up your inlet velocity (if an inlet is used) over a few dozens iterations to avoid huge changes in the domain. Hope it can help! |
|
![]() |
![]() |
![]() |
![]() |
#3 | |
New Member
S03r3n
Join Date: Feb 2024
Posts: 15
Rep Power: 2 ![]() |
Thanks for your post!
The ramp-up of the inlet velocity (or in my case flow rate at the inlet) helped! Quote:
|
||
![]() |
![]() |
![]() |
![]() |
#4 |
Member
Join Date: May 2024
Location: France
Posts: 32
Rep Power: 2 ![]() |
Hey,
Just in case you are still not achieving the desired solution - the increase in viscosity could be changing your reynolds enough that you are now in a higher turbulence regime than before. If that's the case, your mesh might need to be finer for the BL (assuming this is the type of case you are running). It's good to address the mesh issues via the solver settings, but might be worth to revisit the mesh itself |
|
![]() |
![]() |
![]() |
Tags |
convergence, solver, viscosity |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
Steady state simpleFOAM crash | Galactus | OpenFOAM Running, Solving & CFD | 12 | August 14, 2019 06:06 |
Problems Simulating Pump using simpleFoam, Steady state | coolcrasher | OpenFOAM Running, Solving & CFD | 4 | April 15, 2016 04:04 |
Solver for transonic flow? | Martin Hegedus | OpenFOAM Running, Solving & CFD | 22 | December 16, 2015 04:59 |
NonNewtonian, steady state, Laminar, Incompressible for simpleFoam. | ngjaeho | OpenFOAM Pre-Processing | 1 | December 19, 2014 06:08 |
Time step dependence of convergence behavior of steady state simulations in CFX | Chander | Main CFD Forum | 5 | December 23, 2013 05:31 |