[Reoyo]

Hello everybody,

I am trying to perform a sensibility anaylsis about different ways to model boundaries for unbounded flows, and I am getting some results I cannot explain. I whish I could get some help on that.

The situation I am studying is a compressible, Euler's inviscid flow around a NACA 0012 airfoil.

I created two different meshes with two differet extensions:

• First one is just extended 2 chords away from the airfoil
• The second one is extended 20 chords away.

I know that 2 chords-size domain is not big enough for modeling an unbounded domain, but is what I am trying to demostrate.

I also apply two different sets of boundary conditions:

• In the first set non-reflective boundary conditions are applied to all the boundary.
• In the second set, non reflective boundary condition at inlet, and pressure outlet fixed (this BC allows to propagate velocity and speed sound/thermodinamic state throught outlet, but not pressure).

__________________________________________________ ___________

What I finally ran is four simulations, all possible combinations of domain sizes and sets of boundary conditions, and the discussion now is focused on the Drag and Lift coefficients I got from them:

• 2 chord-size domain with non-reflective boundary conditions.
• 2 chord-size domain with non-reflective outlet and fixed outlet pressure.
• 20 chord-size domain with non-reflective boundary conditions.
• 20 chord-size domain with non-reflective outlet and fixed outlet pressure.

Actually, what I expected is that in the small domain, results are more sentitive to the variation of boundary conditions, while in the big domain its sensituvity is reduced, since the boundary is big enough to disipate these non-idealities.


However, I find that in the results of the two small domain simulations are very similar, and there is a big difference in therms of drag coefficieet between the big and small domains. Please, see attached the screenshoots of pressure field (note that in Euler´s inviscid flow all the drag is created by statuc pressure differences) in some of these cases:

2 CHORD MESH - ALL NON-REFLECTIVE BC--------->Cd=0.0174
20 CHORD MESH - ALL NON-REFLECTIVE BD-------->Cd=0.0075

Searching for drag coefficient of NACA0012 profile at an attack angle off 5º, Cd(5º) must be around 0.007... So, what is clear is that the domain size id perturbing my results.

In the attached pictures you can see that the high pressure area in the trailing edge is smaller in small domain case... And of couse, it is created by my "artificial" boundary.

But, among other ones, my question is: How can I explain that even applying non-reflective boundary conditions in a smal domain I got such sifferent results?
Could anybody suggest any reference about domain size in unbounded flow models?

Thank you so much in advance!

C.Reoyo

[FMDenaro]

But such comparison of the domain of different size is performed by retaining the same grid resolution? You need to have exactly the same grid around the profile to make the comparison meaningful

[Reoyo]

Hello FMDenarom

Yes, the mesh around the airfoil is exactly the same in both cases. I created the big mesh by extending the small one without modifying it, so that I could perform the analysis without the mesh factor influence.

Regards!

[flotus1]

And lets not forget that you should reduce the iterative error as far as possible when making such comparisons. I tend to run this kind of simulation until the residuals level out at the maximum possible numerical accuracy.
In fact, controlling all other sources of errors in a simulation is key when trying to isolate the influence of one particular error source.

[Reoyo]

Hello flotus1,

Yes, I ran the simulation for a really high number of iterations... The reported values for Cd kept constant in half of the number of iterations i let the simulation run.

But, again, thank you for your advice. I will keep it!

Regards

[FMDenaro]

Well, non-reflective BC.s are always approximated by the characteristic theory for one-dimensional flows. Spurious effects due to several factors are still present. Do you see the same discrepancy also for other quantities other than Cd?

[Reoyo]

I computed three different results: Cd, Cl and Cp.

-According Cd, the differences I already explained.

-According Cp along the lenght of the airfoil and Cp is tricky....
Cl is almost the same value in both meshes, but the evolution of Cp is slightly different. The pressure gradient that the airfoil is creating both above and below it is higher in the 20 chord size mesh (therefore, higher values for Cp are plotted). Despite of that, at the time to compute Cl, the higher gradients above and below the profile compensate themselves, getting, finally, a simular value of Cl.
[I hope that it will be explained clear enough. Summarizing, pressure gradients are higher in the bigger mesh].

Thank you so much for your support, FMDenaro. I really appreciate it!

Regards

[FMDenaro]

I suppose you are working in subsonic regime so that both inflow and outflow have mixed set of conditions. What are you prescribing?

[Reoyo]

Yes, the flow is subsonic everywhere.

I am working with Fluent, and it has the BC called "Pressure far-field". By making the product between the speed and normal vector at each boundary cell face, the software automatically knows if it is an outlet or outlet face, so does it wheter if it is either subsonic or supersonic.

Then, the software knows which Riemann invariants must fix from the inner domain and which ones from the outer domain [All the far flow variables are intered. It just decides how to use them]
__________________________________________________ ____________

Just in order to give more information, in the attached picture you can see how the values at the boundary [Pf, Ufn, af] are obtained in each case (subsonic inlet and subsonic outlet).

[Pc, Ucn, ac] are the flow variables at the center of the boundary cell C, in a collocated mesh sheme; and [Pinf, Uinfn, ainf] are the far-field flow variables.
__________________________________________________ ___________

But going deeper in this issue, I realised two aspects:

• As you can see in the picture attached, the boundary condition is modifying the flow solution due to its proximity of the gradients... That was almost clear.

• Checking in Fluent Help, I found that "To effectively approximate true infinite-extent conditions, you must place the far-field boundary far enough from the object of interest. For example, in lifting airfoil calculations, it is not uncommon for the far-field boundary to be a circle with a radius of 20 chord lengths."

https://www.sharcnet.ca/Software/Flu...ug/node239.htm


So, at first sight, the answer to my question could be: "Yes, the non-reflective boundary condition is affecting to your flow because you did not fulfill the developer advice".

But just in case somebody knows/is interested in that.... Why the non-reflective boundary conditions affect the flow if the domain boundary is not big enough (or at least the way that Fluent calculates it).

Thank you so much again FMDenaro!

Regards

[FMDenaro]

The answer requires to know exactly which and how the non-reflective BC.s are implemented in Fluent. Riemann invariants exist only in specific hypothesis and other settings are possible.
I suggest to post in the Fluent forum where persons that are experts in this software can help

[Reoyo]

Ok, I will post it there. Now I am very intrigued about it.

But, again, thank you so much for all your support!

regards