[Wingman]

Hi,

I'm doing a CFD Analysis on an airfoil. I'm trying to make a Grid Independence Study. My instructor told me to have the tolerances for lift, drag and momentum 1e-2, 1e-4 and 1e-2 respectively.

I'm using fixed velocity (15 m/s), fixed angle (0 deg), fixed far-field size (100c), fixed wall spacing (6e-6), max y+ (0.47), e.t.c. but change of mesh density. - I'm using the k-w SST model for the grid convergence study.

The first figure attached is the lift and drag as function of the cell count.
The second figure is how many tolerances the previous results are from the densest grid results.
The graph below (in both figures) says how long time the run took. I will have to make it 130 times - So I really need to know when I have acceptable grid.

How can I be sure I have converged results? - Data is available on the attached Excel file.

Thanks in advance.

[Hamidzoka]

Hi
Practically thete is not any grid independent solution. As you move on with smaller grids the results vary at some extend. The selected mesh size and the parameter which is used to qualify a mesh independent solution usualy depends on the phenomenon to be studied.
Whatever it is, 130 runs for a grid independce study does not make scence.
It seems pressure distribusions on airfiol sides will be a good indication of convergence when there is no flow separation.
Another important issue is computational costs. You should answer that what computational costs are affidable at your side.

[flotus1]

A common problem when searching for a "grid independent" solution -lets rather call it a grid sensitivity analysis- is that the solutions on different grids are not obtained with the same level of accuracy.
This might be the case in your analysis because initially the results seem to stabilize and then begin to deviate for very high cell counts. Have you made sure that the iterative error is negligible throughout your analysis? Did you use some fixed residual limit to stop the iterations? It might be advisable to simply run the iterations until the residuals level out for the mesh sensitivity analysis.
Additionally, you should run at least one similar analysis for a case with high AoA.

What does your grid look like? Where exactly did you put the additional cells for your analysis? Feel free to share some pictures. Btw: which solver are you using?

[Wingman]

Originally Posted by Hamidzoka

Hi
Practically thete is not any grid independent solution. As you move on with smaller grids the results vary at some extend. The selected mesh size and the parameter which is used to qualify a mesh independent solution usualy depends on the phenomenon to be studied.
Whatever it is, 130 runs for a grid independce study does not make scence.
It seems pressure distribusions on airfiol sides will be a good indication of convergence when there is no flow separation.
Another important issue is computational costs. You should answer that what computational costs are affidable at your side.

I'm not doing 130 runs for the grid independence study. When I've found acceptable grid I will use that to run 26 different angles (-5° up to 20° with 1° increment) using five different models. (k-w SST, k-w SST Low Reynolds, SST Transition, k-kl-w and Inviscid) for comparison. Resulting in 130 runs. Thats why I want to believe I have acceptable model. I will hopefully be able to compare them to real data soon.

I'm actually expecting flow separation due to geometry, so I'm not sure I can count on the Cp plot to find convergence?

Originally Posted by flotus1

A common problem when searching for a "grid independent" solution -lets rather call it a grid sensitivity analysis- is that the solutions on different grids are not obtained with the same level of accuracy.
This might be the case in your analysis because initially the results seem to stabilize and then begin to deviate for very high cell counts. Have you made sure that the iterative error is negligible throughout your analysis? Did you use some fixed residual limit to stop the iterations? It might be advisable to simply run the iterations until the residuals level out for the mesh sensitivity analysis.
Additionally, you should run at least one similar analysis for a case with high AoA.

What does your grid look like? Where exactly did you put the additional cells for your analysis? Feel free to share some pictures. Btw: which solver are you using?

I'm using 1e-6 for everything... x/y velocity, continuity, lift, drag, momentum, energy, omega e.t.c. and using 2000 iteration when doing the grid convergence study. The lift, drag and momentum stabilize in all runs but the solver uses 2000 iterations.

I'm using Matlab to run ICEM CFD and Ansys Fluent through batch mode. I'll leave some pictures of some of the meshes. (4585 cells, 77077 cells and 1952085 cells)

[Wingman]

More Figures (Reached Maximum attachments)

[Wingman]

More Figures (Reached Maximum attachments)

[flotus1]

My initial guess would have been that fluent does not converge to a sufficient level within 2000 iterations with these kinds of meshes, especially the finer ones. There are quite a few high aspect ratio cells and volume jumps could be high.
Do you use double precision for fluent? What is the output of fluent when you click on "mesh->check" with the finest mesh loaded?

[arjun]

Originally Posted by flotus1

My initial guess would have been that fluent does not converge to a sufficient level within 2000 iterations with these kinds of meshes, especially the finer ones. There are quite a few high aspect ratio cells and volume jumps could be high.
Do you use double precision for fluent? What is the output of fluent when you click on "mesh->check" with the finest mesh loaded?

That is quite possible for various reasons.

[FMDenaro]

I agree, using any iterative method on via via refined grids requires to be careful in the convergence threshold. Double precision is also mandatory in such case.

[Wingman]

Originally Posted by flotus1

My initial guess would have been that fluent does not converge to a sufficient level within 2000 iterations with these kinds of meshes, especially the finer ones. There are quite a few high aspect ratio cells and volume jumps could be high.
Do you use double precision for fluent? What is the output of fluent when you click on "mesh->check" with the finest mesh loaded?

Hello guys, thanks for your replies and sorry for my late response. I am using double precision and the residual in each run appears to be flat, except for high angle of attack.

But what do you mean by 'these kind of mesh'? Most tutorials I've seen do similar meshes? Is there some other mesh technique I should go for? I've been trying to minimize the aspect ratio, but when aiming for y+ < 1, the aspect ratio increases.

Here is the mesh check comment from Fluent on the densest mesh. (A mesh I could never use for my analysis)

Originally Posted by Ansys Fluent

Checking mesh..................
WARNING: The mesh contains high aspect ratio quadrilateral,
hexahedral, or polyhedral cells.
The default algorithm used to compute the wall
distance required by the turbulence models might
produce wrong results in these cells.
Please inspect the wall distance by displaying the
contours of the 'Cell Wall Distance' at the
boundaries. If you observe any irregularities we
recommend the use of an alternative algorithm to
correct the wall distance.
Please select /solve/initialize/repair-wall-distance
using the text user interface to switch to the
alternative algorithm.
...................
Done.

Mesh Quality:
Orthogonal Quality ranges from 0 to 1, where values close to 0 correspond to low quality.
Minimum Orthogonal Quality = 5.60777e-01
Maximum Aspect Ratio = 1.25190e+03

I've been thinking of a O shaped farfield - with O shaped O-Grid block around the airfoil. Inside the O-grid I've been thinking about using Triangle Mesh and Outside having a Quadrilateral mesh. (See sketch in Attachment).

I've also attached an result example from previous model.

[flotus1]

But what do you mean by 'these kind of mesh'?

In this particular case:

• High aspect ratio cells in the free stream region (not those near the wall that cause the warning in fluent, they are ok)
• presumably rather high volume jumps
• high number of cells

You can improve on the first two points by carefully choosing mesh topology and bunching laws and parameters in ICEM. The worse these values are, the more iterations you need.
And just to be on the safe side you should do what the fluent mesh warning tells you.

You will still be left with the third point on the list and there is obviously no way around it for a mesh sensitivity analysis. It just takes more iterations to obtain the solutions on finer meshes. From my experience, 2000 Iterations are simply not enough for 2D meshes with more than 1e6 cells when you need to be sure that the iterative error is negligible.
When you say your residuals "appear to be flat" how exactly does this look like for finer grids? The magnitude of the residuals should drop below 1e-14 with high quality quad meshes and double precision.
In addition to checking the residuals you should also check the trend of lift and drag coefficients over the iterations.

[juliom]

I think you are mixing to many things at the same time. Although these papers are "old" I strongly encourage you to read them:
1.- Further discussion of numerical errors in CFD; Ferziger, Joel H, PERIĆ, MILOVAN 1996

2.- Perspective: a method for uniform reporting of grid refinement studies Roache, Patrick J

It is important to reduce the other source of error before claiming grid independent solution. If you are using a time dependent solution then you need to make sure that you are comparing them all at the specific time. In contrast if you are using a steady state approach then, the iterative error must be small enough (O) 10^-14. double precision is also encourage...