How accurate are my results if the solution has not converged??? It is not divergent however and the solution seems to have converged to a point but Fluent has still not said that "Solution Converged".

By plotting contour plots the Mach no decreases where the static pressure increases indicating a shock wave occurs. However, can I be sure that the results on the scale for the plot are accurate? i.e. are they accurate enough to say that "the contours give the impression that a shock wave occurs but more refinement of the mesh is needed in order to get a convergent solution."

...Fluent has still not said that "Solution Converged"...

Exactly. This is where we should try to avoid putting all faith in the software. Fluent is just a calculator, a PDE solver if you may. There are limits set for convergence in the Solve -> Monitors -> Residual panel. When this limit is reached, a "Solution is converged" message is mechanically printed to stdout.

In other words, Fluent does not have an AI. There is no procedure that checks whether the results are meaningful in the physical sense. We should use our discretion based on the knowledge of the physical features of the flow being simulated and then decide whether convergence has been realized.

Ok thanks. In this sense, convergence has been realised and it is simply that my limit is a different value. (If I understand you correctly)

Do you have any suggestions for the limits to use for M0.8, M1.2 and M3.0 at 11km? I am using the defaults at present.

Well, if the results physically make sense and you've checked all other possible ways to ensure that convergence is definite (for instance, in fluid flow through conduits etc. you would check if mass/volume fluxes are conserved etc.) then yes, you have a converged solution.

With regards to your second question, I have to say I really cannot give you an answer, primarily because I do not work in that area. So sorry about that. You should wait and see if someone else can help you out.

Good Luck!

Best Regards,

Srinath Madhavan

Hi Chris! I work in aerospace field. So if you have some question let me know...Actually one thing I want to suggest is to check aerodynamic forces convergence. I study transonic flutter and I monitor lift and drag value to judge convergence. Luca

Hey Luca. I am modelling flow over the aim9x sidewinder missile at M0.8, M1.2 and M3 in horizontal flight at altitiude of 11km. See "RE: Fluent Read Error" and "RE: My Solution Wont Converge". If you need anymore information just email me on ct_con@hotmail.com

Thanks for your advice, I will plot the life and drag monitors as suggested today and lt you know how it goes.

Am I right in saying that Fluent will only say "solution is converged" when the solution converges to the limit set in solve>controls>solution panel.

Fluent only checks convergence on flow-residuals. Even if residuals are quite low (about 1e-7, 1e-8) aerodynamic forces may vary a little. That's why I check for lift convergence. Typically I get convergence on lift od order 1e-7 when residuals are about 1e-10. I want to assure convergence on aerodynamic forces because correct forces-behaviour description is my main target (as yours I suppose). Luca

Yes I am considering the aerodynamic forces around the missile and will be comparing my results in Fluent to theory. Thanks for the advice. I will try setting the resuiduals as you have suggested and look for converence.

Chris

You're right Luca. Having low residuals only means that the difference between the value of the solution at the n-th iterate and at the (n-1)-th iterate is low. Nothing else.

A good choice is to use a sort of "combined approach". I mean, you can still use residuals as a convercence criterion, combining it with physical analysis of the results.

I'd think FLUENT uses a convergence criterion (10^-3) which is far too large, above all in steady cases. A good approach is to set a very low or zero value as convergence criterion and iterate until all residuals stay flat for a reasonably high number of iteration. When this condition is reached, it's time to check the results from a physical point of view.

Moreover, you should also check, to be rigorous:

- Grid independence: a solution can be considered as "converged" only if it doesn't change anymore if you refine the grid.

- Convergence in time, for unsteady cases.

A good book for all these questions is the well known:

J.H. Ferziger, M. Peric, Computational Methods for Fluid Dynamics, Spriger, Berlin.

Best regards,

ap

Hei Ap form PoliTO I'm Luca from PoliMi, do you remember of me? Yes you're completely right. To be honest I disactivated residual check and I have a scheme function which checks convergence on forces. When convergence is reached, Fluent stops iterating. Hope to hear you soon. P.S Regarding that problem I talked to you about Fluent forces, the Fluent support was not succesfull. The problem is solved in Fluent 6.2. Luca

Hi Luca! Sure, I remember you. How are you?

Thank you for the information about the FLUENT 6.1 bug.

In this period I'm giving a deep look to OpenFOAM because its code is completely open and very well structured.

FLUENT gives me some (ehm...many ) problems implementing models for granular flows using UDF, so I'm thinking to change.

ap

Just curious ap, Have you tried MFix?

Yes, I used MFIX. It's a very good code, but it implements only few turbulence models (k-eps only, if I'm not wrong), and it's not able to manage complex grids created in commercial meshing tools.

OpenFOAM is able to convert grids generated with many CAD and meshing tools like GAMBIT and it's a more general and complete tool with a wide range of models.

Best regards, ap