[frossi]

Hi,

1) when I perform a grid independence study, do I only change the size of the elements in the core mesh? Or I also change the size of the elements on the airfoil?

2) In my case, when I use larger elements I get some faceting on the leading edge of my wing. If my results are the same with and without faceting, then is it right to assume that the mesh as converged, despite faceting?

3) Also, after I reduce the element size, my result do not change in only one direction (increase only or decrease only), but they increase and decrease randomly. Is this normal or I should expect the results to go in one direction only ?


Best regards.

[ghorrocks]

1) Ideally you change all the mesh. But that is not always possible so sometimes some judgement is required. But certainly you refine the mesh in all dimensions at critical parts of the geometry.

2) Possibly. Again, that is a judgement call based on what the results look like and what you expect the flow to do.

3) I do not understand this question.

[frossi]

My run is a 3D wing simulation.

1) My problem is that my computer can feasibly run a mesh of no more that 6 million elements. So, my main concern was to accurately mesh the leading edge of the wing (picture 1) so that there is no faceting and the curve is circular. Once I get a circular leading edge with no faceting, I used 3.8 million elements, leaving very large elements in the core of the mesh not to exceed the 6 million mark. If i further refine the leading edge, the element count will pass the 6 million. So, to do my mesh convergence study, I leave the elements on the wing the same, and I only change the elements of the core mesh (making them smaller), because the core mesh is the only thing I can still change. But my doubt was that the core mesh may not be such a game changer, since lift and drag are dependent on pressure on the wing surface, and so i believe that the convergence study would be better if i mainly change the elements on the wing surface rather than the core mesh. Does my reasoning make sense? But in this way i would have element count problems (too many for my computer).

Do you consider this an acceptable mesh convergence study, considering I am just decreasing the size of the core mesh (since by judging from the screen, the wing mesh looks fine enough)?
And what is your suggestion to present a decent mesh convergence study for my case? (It'a 3D wing simulation)


2) For what you didnt understand I meant:
How should the mesh convergence graph look? Should it be one single trend (graph 1), or the calculated value can increase and decrease until it levels out (graph 2)?


3) As you can see I am using 8 inflation layers to make sure the size of the last inflation element is the same size as the adjacent core mesh. Are 8 inflation layers good or i should use more/less?



Thank you for your time and help.

[ghorrocks]

1) This is suggesting that this model is too large for the computer you have at the accuracy you are looking for. This is no surprise - that is why serious CFD is done on supercomputers, not desktops.

2) Mesh refinement tends to have two sections: The grossly underrefined section where the results bounce up and down radically with each refinement. And then the convergent section where a nice, monotonic run to convergence is seen. If you are getting results bouncing around it suggests you are in the "grossly underrefined" section.

But be aware that issues other than the mesh can distort this. A key factor here is separations and vortex shedding - that needs to be resolved by appropriate choice of turbulence model, not mesh refinement.

3) You results are suggesting you are still some way off a mesh independant solution. But they could also be suggesting you are having separation and/or vortex shedding. Have a look at the results and check for separations. And also try more inflation layers to see the effect.

[frossi]

This is the 2D view of my wing. As you can see, it looks like separation occurs only at the trailing edge, but I think it is almost negligible (correct me if I am wrong). Or is it possible that thinner inflation layers are required to capture a smaller separation? Because as far as I can tell from my results, it looks like flow is not separating from the wing except the small part in the trailing edge. I also attached the graph of my results as the core mesh is refined. it looks like the change in lift is random.

Re is 1,000,000 (so it should be turbulent, since turbulent flow is Re > 500,000 for external flow)
I am using a Spalart-allmaras model
the veolocity of the flow is low (44 m/s)
the wing angle of attack is also low (5 deg)

What puzzles me is that my residuals for continuity and velocities increase! So if my residuals increase, i think there is something wrong somewhere. But the geometry is fine, and the conditions i set look good.
Since residuals are the error in the equation being solved, if they increase it means that the error increase and the result is further from being true. In fact, this is the first time ever that the value of my residuals increase. Any idea why? Or residuals are allowed to increase?

Also, will I ever be able to get a good answer considering the limitations listed before? And to get an idea, how many elements are you talking about when you refer to a reliable simulation (from experience)? around 5 million, or more than 10?



Thank you and best regards.

[ghorrocks]

Your residuals do not converge probably because of the separation at the trailing edge. It is likely this is transient.

Your mesh refinement study is not broad enough. Normally when you do a mesh refinement study you double or halve the element edge length. This leads to refinements in node numbers typically 8x for each refinement. Your refinements are too close to be useful. But the fact that the results are jumping around for very similar meshes suggest you are a long way away from a mesh refined result.

There is no overall guide for node count to give a good result, it is so dependent on so many things. You really do need to check for every application.

[frossi]

you are right. I replaced the rounded trailing edge with a sharp edge. After running the simulation again, lift seems to be converged. It keeps oscillating with changes of 1%. Are these changes low enough so that I can consider it converged?

Although lift is now converged, my residuals keep increasing. In fact, mass flow rate through the domain is more than 1% of what comes in. If i am right, it should be less than 1%. What do you think causes the residuals to increase? I am still not able to figure out why.

[Lazarus]

Originally Posted by frossi

Hi,

1) when I perform a grid independence study, do I only change the size of the elements in the core mesh? Or I also change the size of the elements on the airfoil?

2) In my case, when I use larger elements I get some faceting on the leading edge of my wing. If my results are the same with and without faceting, then is it right to assume that the mesh as converged, despite faceting?

3) Also, after I reduce the element size, my result do not change in only one direction (increase only or decrease only), but they increase and decrease randomly. Is this normal or I should expect the results to go in one direction only ?


Best regards.

Hi guys,

I have a problem similar to yours and I have been looking for the correct answer for days. I can not go to high mesh numbers because of limited computer source.

Anyway, I'm doing grid independence study for ship maneuvering simulation. As you mentioned, when I make a refinement to be r = 1.4(grid refinement ratio) just on the core mesh, for example, the number of mesh is 1.2M coarse, 2M in medium and 2.7M in fine. I am not sure if this increase is a little less and whether or not I have done the grid independence work correctly. If you have any information on this issue, will you inform me?

Thanks in advance.

Lazarus

[ghorrocks]

The difference in your mesh sizes is borderline as to whether it will be enough to really get a good handle on your mesh sensitivity. Rather than doing the mesh sensitivity study on the full design can you do it on a small section? Or a simpler design? Then you should be able to refine the mesh a large amount, if required. Once you have determined the mesh requirements on the small model you will not require a mesh sensitivity study on the full model.