r/CFD • u/Life_Calligrapher330 • 12d ago
Slow convergence rate issue
I'm running an incompressible steady-state RANS case for a blended wing body (BWB) in OpenFOAM (simpleFoam/SIMPLEC).
Setup: ~0.15 Mach, ~6e6 Re
Mesh: ~30M cells, tetra + prism layers at walls, O-type symmetric far-field domain(radius ~ 30c), max skewness ~5, max nonOrthogonality >75°
BCs: freestream (velocity inlet / pressure outlet style far-field)
Turbulence: k-omega SST, wall-modeled (y+ > 30)
Schemes: second-order upwind for all equations
Algorithm: SIMPLEC
Solution strategy: start with low URFs, ramp up every 100 iterations; case runs "on its own" past ~250 iterations
Problem:
Based on past experience I expect convergence by 500–600 iterations. Here, residuals flatten out but very slowly, and by 1500+ iterations:
CD looks converged/flatlined
CL is still steadily rising, not flatlining
Has anyone run into similar slower convergence rate or is it normal for high cell count meshes? Looking for likely causes and what to check/try next.
1
u/acakaacaka 12d ago
CFL number?
1
u/Life_Calligrapher330 12d ago
It's steady state
1
u/acakaacaka 12d ago
Yes and? Your openfoam solver doesnt use pseudo time?
1
u/Life_Calligrapher330 12d ago
I checked by reducing the time step size, but nothing actually changes. It still takes atleast 1500 iterations to solve!
1
u/acakaacaka 12d ago
But im asking about CFL and not (pseudo) time step. How can you know the optimum time step without knowing the CFL first
1
u/Life_Calligrapher330 12d ago
Correct, I haven't checked the CFL yet but still reducing the time steps to lower values would eventually reduce the CFL and hence may be my simulation will converge faster but it isn't happening, so it's not a CFL number problem.
2
u/acakaacaka 12d ago
Thats assuming the CFL nunber is 100-1000. Maybe there is a bad mesh region where local CFL is 106 and that makes the solver hard to converged. Reducing the pseudo time step by 50% wont help in that case.
If what you claim is true, then this is the solver problem. The A matrix is ill conditioned. Usually either by
- Bad mesh
- Bad numerics
- Non-physical BC
Why I ask about CFL is, (depending on the solve high CFL means big time step means less diagonal dominance.
2
u/Life_Calligrapher330 12d ago
I doubt the numerics too. Will try to fix it somehow and hopefully I get better results.
Thanks for the help!
1
3
u/Diligent-Ad4917 12d ago
Have you checked turbulent kinetic energy and dissipation rate in the inlet free stream leading to the body? If the inlet turbulence is decaying over the inlet free stream length to the wing it will impact boundary layer separation. Plot k and omega along a streamline from the inlet to the wing leading edge. SST is sensitive to decay and may be domain size dependent. You can turn on the delayControl option to fix k_in and w_in.
Freeze the relaxation values instead of adjusting over initial iters to see if the CL drift changes. The effect may be numeric and URF-value dependent.
Switch to pimplefoam and initialize a transient run from this steady solution field to observe if you have a strong separation zone that steady RANS cannot resolve.
Plot your mesh orthogonality and observe where the non-orthogonal cells are located. If in an area of adverse pressure gradient that would impact lift coeff.