[karchouille]

Hello everyone,

I have made many researches about my issue but none of them was satisfying. I am currently testing a three-element wing with segregated flow model, but I can't decide if the solution is well converged or not. Indeed, the lift curve seems pretty steady but the residuals remain high and fluctuating (see enclosed images).
My questions are :
- Is the calculation well converged even if the residuals are high and fluctuating ?
- Can I then rely on the lift value given by the lift plot ?

Thank you in advance.

[fluid23]

There are a lot of obvious problems just from what you have shown.

1. 600-700 iterations is never going be enough for this kind of analysis.

2. The one mesh image you show raises some concerns. I don't see any near wall refinement (prism mesh). Check to see that your wall y+ values are appropriate for your turbulence wall model. If you used the default, all y+ should be between 1 and 5 or 30 and 60 to 120 depending on the particulars of your flow.

3. It is very possible that this flow is too unsteady to approximate with a steady analysis. You will probably need to consider time averaging a transient solution to get better results.

4. The wake will have a significant impact on airfoil performance, you should be refining the mesh in the wake to capture this influence. There are several options for doing this, consult the help documentation for details.

[fluid23]

To answer your questions directly...

1. It can be, but yours is almost definitely not converged. To answer this question yourself you can turn on temporary storage, step 1 iteration then create a threshold in a scalar scene to find cells with high residuals that may need further refinement. If they are not near your area of interest then you might be able to justify not resolving them.

2. No.

[bluebase]

Hi Karchouille,

Is the calculation well converged even if the residuals are high and fluctuating ?

Well, i guess, it cannot converge any further in the current setup. So you can consider it as "converged". Please mind, that in StarCCM, the usual residual monitors are normalized. The absolute residual sum may be some where else.
Nevertheless, as a rule of thumb, the residuals should drop by three magnitudes to have a well converged solution (in enginering problems). Therefore, no, it's probably is not a good solution.
Your mesh clearly shows, that you cannot get a good solution with it. Do some research on boundary layer flows. I strongly suggest you, to include a proper boundary layer mesh consisting of prism elements. If you have prism layers, then they seem too few, more layers probably are required. Check also y+ range depending on how much of the flow regime of the boundary layer you want to model.

Can I then rely on the lift value given by the lift plot ?

By just one plot (and one mesh/time step setting), no you cannot rely on that only.
You probably should do some mesh dependency study, and maybe time step dependence study to analyse the impact on the predicted lift.
Only then you can have an impression how much you can rely on the predicted lift. Ideally, for two meshes of different densities, the lift doesn't change. In that case, you can assume, that the model's solution is mostly independent from numerics.


Depending on the importance of your results, reducing the degree of modeling turbulence (going in the direction of LES) might improve the representation of the real flow... of course at considerable costs...


More over, you might want to compare your calculated lift force with some similar cases from text books; just to check plausibility.


Best regards,
Sebastian

[karchouille]

Hi,

Thank you very much for your quick and very useful replies. Sorry for my late one but I spent all this time searching information about wall treatment,Y+, residuals, convergence, etc.

So I checked the wall Y+ values on the whole part and indeed there were very high values like 300 or something like this. I have then adjusted my prism layers to both cover all the boundary layer and ensure a wall Y+ value between 1 and 5 on every surface of the part. The flow model I have choosen is : Steady, Segregated, Realizable K-Epsilon with Two Layer All y+ wall treatment.
I have refined the mesh, especially in the wake region with a volumetric control.

All these settings allowed my calculation to converge way faster but my residuals are still remaining pretty high, especially the Turbulent Dissipation Rate (10 for TDR, 0.001 for the others). Note that I showed non-normalized values.
The drag and lift are still decreasing after several hundreds iterations with an oscillation. So I tried to run an unsteady calculation but the results are still irregular.

Do you think there is something to improve concerning the mesh or did I just choose a bad model for the flow ?

[bluebase]

Hi kachouille,


regarding the mesh, i don't know what could be improved, because i don't have a good enough idea about the flow around the foils.
However, you can try to figure out yourself what needs to be improved in the following way.


There is the option "Tempory storage retained" in every solver tree, such as segregated flow. It's usually at the end of the list of options in the solver object. Check the respective check box.
When this option is active, intermediate quantities, such as gradients and residual fields are kept in memory after each iteration step. This do cost memory, so take care if memory is limited.
These temporary fields (field functions) can be used to assess which parts of the mesh have locally (absolutely) high residuals, and where a gradient isn't resolved good enough.
So, check temporary storage retained, make a scene, plot residuals, later plot gradient of relevant quantities such as dissipation rate. Find areas of highest residuals and gradients, and refine if necessary, or add more prism layers. A threshold part (derived part) might be helpful too.


There is also a way to use such gradient fields as input for a field function to calculate the local mesh base size. This field function can then be fed to the automatic mesher to form an adaptive mesh. There was something in the manual, search for "Field function mesh refinement".
As refinement field function, i had some success in the past to use a logarithm from a problematic gradient field, such as constant * 10^(-log($anyGradient)). Enclose it in a min, and max statement to have some limiters.



Best regards,
Sebastian

[karchouille]

Hi,

I spent many hours refining and optimizing the mesh by analyzing the residuals and their location around the part. Now my residuals decrease signficantly, the convergence happens way faster and the results seem coherent.

Thank you so much for you help !

Loic

[karchouille]

Hello,

Unfortunately, I have encountered another issue concerning the residuals on my external flow simulation. The residuals have not decreased by 3 magnitudes, but when I plot the non-normalized ones, they seem pretty good except the Specific Dissipation Rate (see enclosed screenshots). The lift plot oscillates a little bit, but around the same value (-160N).
These oscillations made me think the flow I tried to simulate was unsteady, so I ran an unsteady simulation but the results were totally absurd.

Thanks to the "temporary storage retained" method with segregated flow, I managed to compute X Y and Z momentum on a scalar scene and they are all below E-06 on the whole part. The Turbulent Kinetic Energy is pretty good as well, there are just some cells with high values but they are not impactant in the results. However the Specific Dissipation Rate has higher values around interfaces between the three wings and the endplate. I showed the mesh at these interfaces and I noticed that the prism layer total thickness is reduced as it approches the interfaces (see screenshots).

So my questions are :

- Do you think this high SDR around interfaces is impactant on the final result ? I think so, but I am not sure about this.

- Is the prism layers total thickness reduction source of this high SDR?

- If yes, do you think adding a chamfer or a fillet at the interfaces could help the prism layer thickness remaining the same over the corner ?

I tried to show as much screenshots as possible to illustrate my problem, but I can send more if needed.

The parameters I'm using are :

- Segregated flow
- Steady state
- Constant density (Mach number << 0.3)
- K-Omega SST turbulence
- Low Y+ wall treatment (All Y+ values are between 0.5 and 7)
- Polyhedral mesh with 4,115,442 cells
- 20 prism layers, 8mm thickness on the whole part

Best regards,

Loic