[chandra shekhar pant]

Dear Foamers,


I am trying to run 3D aerofoil in OpenFoam, the mesh I had created in the gmsh (attached herewith). In this case the flow features looks fine, but the Uz component of velocity is not converging (residual not going down). The flow is in x-direction. Snapshot of the residual, gmsh file, boundary condition, checkMesh log is attached.



Can it be inferred that my mesh in z direction is not ok? Or in other words I haven't been able to export the mesh in z-direction?


Any help or comment is highly welcomed.


Thanks a lot!

[Krao]

Hi Chandra Shekar,

your cheeckMesh results actually looks good. If you think it is upto mesh you can try running 'checkMesh -allTopology -allGeometry' once. This gives much more detailed mesh report. Apart from meshing there are lot of other factors, which influences the simulation. The initial conditions, the turbulence model you are using, the solution algorithm, the solvers you are using to solve the matrices., etc. With so less detail, nothing much can be added.

From the figure it can be assumed that you are using k-omega/k-omega SST model. So, check your yPlus values, whether it is in accordance with the model demand. Start, your simulation with no turbulence, with lower order grad schemes and lower your relaxation factors. Once you think the simulation is going well/converging, introduce turbulence, then change to higher order schemes and finally you can increase your relaxation factors as well.

Also, you should always post your simulation report for at least 5-6 steps so that, one can see how your simulation is behaving. For example, if your simulation is doing several iterations to solve each variables, then you can think about increasing the minimum number of iterations, or you may chose different solver for the particular variable in fvSolutions. Hope the above information helps, and please go through all the above mentioned points in detail.

K. Rao

[chandra shekhar pant]

Dear K Rao,


Many thanks for your inputs. When I checked the complete report of the checkMesh by using "checkMesh -allTopology -allGeometry", it shows an error, which I don't understand.

Yes, you are correct I am using k-\omega SST model, the fvSchemes and fvSolutions are attached herewith. To make my initial simulations stable, I am using very high value of \omega. The boundary conditions for the k and \omega are also attached.


I don't understand your quote "Also, you should always post your simulation report for at least 5-6 steps so that, one can see how your simulation is behaving. For example, if your simulation is doing several iterations to solve each variables, then you can think about increasing the minimum number of iterations, or you may chose different solver for the particular variable in fvSolutions" ...?



Meanwhile, I also tried with the laminar case, but in that case also the Uz component and Pressure were not converging.



Waiting for your more valuable inputs.


Thanks a lot!

[chandra shekhar pant]

I think you are saying about the solver output, if this is correct, please find it herewith. otherwise please correct me. Thank again!

[Krao]

I don't understand your quote "Also, you should always post your simulation report for at least 5-6 steps so that, one can see how your simulation is behaving. For example, if your simulation is doing several iterations to solve each variables, then you can think about increasing the minimum number of iterations, or you may chose different solver for the particular variable in fvSolutions" ...?

The following part is from your fvSolutions, there you can think of changing the solver or smoother, I mean. There are several tutorial cases for airfoil you can see those and decide, what best suits you. You can define min number of iterations as well.


"U.*"
{
solver smoothSolver;
smoother symGaussSeidel;
tolerance 1e-6;
relTol 0;
};
p
{
solver GAMG;
smoother GaussSeidel;
tolerance 1e-6;
relTol 0.1;
}

Also, you should always post your simulation report for at least 5-6 steps

Time = 0.0005

smoothSolver: Solving for Ux, Initial residual = 0.00413651, Final residual = 0.000105736, No Iterations 3
smoothSolver: Solving for Uy, Initial residual = 0.00103482, Final residual = 2.60759e-05, No Iterations 3
smoothSolver: Solving for Uz, Initial residual = 0.00279737, Final residual = 7.51683e-05, No Iterations 3
GAMG: Solving for p, Initial residual = 0.000224203, Final residual = 1.78668e-06, No Iterations 7
GAMG: Solving for p, Initial residual = 2.12721e-05, Final residual = 8.85287e-07, No Iterations 3
GAMG: Solving for p, Initial residual = 4.0315e-06, Final residual = 6.96086e-07, No Iterations 3
time step continuity errors : sum local = 2.71219e-09, global = 5.98377e-10, cumulative = 6.74512e-09
smoothSolver: Solving for omega, Initial residual = 5.2679e-06, Final residual = 3.65494e-08, No Iterations 3
smoothSolver: Solving for k, Initial residual = 0.00374982, Final residual = 7.93574e-05, No Iterations 3
ExecutionTime = 630.86 s ClockTime = 632 s


Finally you are using second order fvSchemes, it is always good to have the final solution with those schemes. But if you are not sure, start with lower order schemes and then finally you can go one step at a time.

To make my initial simulations stable, I am using very high value of \omega.

I don't know anything about the above mentioned statement, I usually calculate those and input the value, whatever I get. Maybe a 10% more sometimes.

These are all I can add as of now, please revisit your case thoroughly, by considering the above mentioned steps.

[Krao]

Originally Posted by chandra shekhar pant

I think you are saying about the solver output, if this is correct, please find it herewith. otherwise please correct me. Thank again!

If you see the report, you can clearly see something unusual with the pressure solver. It is taking 40+ iterations, while the other solvers require, 2-3 iterations. Check this out using some other solver/smoother. But I would check my yPlus and I would see if I have done proper refinements at crucial parts like trailing edge or in the wake etc.

[chandra shekhar pant]

Dear K Rao,


Many thanks for your input and the help. I had searched the tutorial for airfoil cases and found these schemes, fvsolution etc. the most appropriate. The values for the yplus are:
y (min): 0.005793
y (max): 3.22308
Y(avg): 0.619564
I think these lie with the specified range? Yes, you are correct initially it was taking too many iterations for the pressure since I have inputted the nNonOrthogonalCorrectors 2. But after time 1.2 you can clearly see that the no of iterations are in the range of 6-12, that's not high I guess.



But yes, again you are correct that pressure seems to have problems as the residual for the pressure is not falling as expected.



My ultimate goal is to run this case for the interPhaseChangeFoam which is inherently unsteady. As you have suggested in the earlier post that before going for the unsteady or the complicated solvers, go for the SIMPLE one, thus I tried this first one. But you can see that even this is not working properly.

I really can't see what is missing or not correct in this simplified case.



I think some way I am missing some thing in the mesh part, otherwise this should not happen, what you say? or any other advice or comment are welcomed.


Thank again for your time!

[Krao]

As of now I don't have much to add. I have a case where the simulation is dependent on the size of simulation domain. If it is too small, then my results are scattered. So, check whether the simulation domain is large enough, and there are no effects of re-circulation of flow.

Also, if your residuals are well converged, you cannot say the results are 100% true. You need to do grid independence study. Also, use probes like velocity, pressure in the wake region, see whether the probes are converging. If you are interested in calculating force coefficients, then check whether those variables are converging.

Best wishes,
K. Rao