[DeadLee]

Originally Posted by Moreza7

I should check that are the B.Cs correct?

We already said:

- your BCs are correct
- to extend spanwise direction
- that 2D LES is meaningless because turbulence is 3D so don't expect good results

Then you started talking about 2D-3D and other stuff, if this is not relevant to the first question (Why is 2D LES in Fluent not giving good results?) don't talk about it because it's too confusing. Your english is not the problem.

[Moreza7]

Originally Posted by DeadLee

We already said:

- your BCs are correct
- to extend spanwise direction
- that 2D LES is meaningless because turbulence is 3D so don't expect good results

Then you started talking about 2D-3D and other stuff, if this is not relevant to the first question (Why is 2D LES in Fluent not giving good results?) don't talk about it because it's too confusing. Your english is not the problem.

OK. Sorry if I confused you.
Best regards

[DeadLee]

Originally Posted by Moreza7

OK. Sorry if I confused you.
Best regards

No worries, good luck!

[flotus1]

Let me state the obvious, just in case: when expanding the 2D domain to the third dimension, this third dimension needs to be adequately resolved by the mesh for LES to do its magic. Just stretching out 1-5 cells won't work.

[Moreza7]

Originally Posted by flotus1

Let me state the obvious, just in case: when expanding the 2D domain to the third dimension, this third dimension needs to be adequately resolved by the mesh for LES to do its magic. Just stretching out 1-5 cells won't work.

Thank you. I'll check this.
But today a guy checked the velocity contours and told me that the high drag coefficient is probably due to the premature transition and separation of the flow (you can see that the flow separates very soon close the leading edge) and this is due to the use of central difference scheme upstream of the transition region which causes numerical trip of the boundary layer. Is that right?

Kind regards.

[FMDenaro]

Originally Posted by Moreza7

Thank you. I'll check this.
But today a guy checked the velocity contours and told me that the high drag coefficient is probably due to the premature transition and separation of the flow (you can see that the flow separates very soon close the leading edge) and this is due to the use of central difference scheme upstream of the transition region which causes numerical trip of the boundary layer. Is that right?

Kind regards.

I don't see the meaning of the statement of this guy. LES requires accurate discretizations and the second order central discretization was the hystorical scheme used.
Again, you miss the key point. The 2D or quasi 2D approximation forces the vorticity to have the direction normal to the plane and no action of the stretching appears. Without stretching the energy has a different way of distributing along the length scale. For example, in a 2D flow you can see small vortices merging in larger.
Try to extend the third dimension to a reasonable lenght and use a step size dz+=O(20-30). Only then we can discuss.

[Moreza7]

Originally Posted by FMDenaro

I don't see the meaning of the statement of this guy. LES requires accurate discretizations and the second order central discretization was the hystorical scheme used.
Again, you miss the key point. The 2D or quasi 2D approximation forces the vorticity to have the direction normal to the plane and no action of the stretching appears. Without stretching the energy has a different way of distributing along the length scale. For example, in a 2D flow you can see small vortices merging in larger.
Try to extend the third dimension to a reasonable lenght and use a step size dz+=O(20-30). Only then we can discuss.

Thank you dear FMDenaro.

My friend sent me a PDF which has more details about the LES of this airfoil. You can download it here:
http://www.tfd.chalmers.se/~lada/pos.../simon_lic.pdf

He said that his comments on the central difference scheme is from this paper you can check it in the following sections that I quoted some of them:
4.4 Discretisation Schemes of the Convective Terms (Page: 17)

When the momentum equations are discretised in space using the central difference scheme (CDS), considerable unphysical oscillations are present all over the computational domain (see Fig. 4). The CDS is often used in LES because of its non-dissipative and energy-conserving properties. However, the scheme is also known to produce these odd-even oscillations (grid-to-grid oscillations or wiggles) when the resolution is poor.
To remove the unphysical oscillations in front of the airfoil and upstream of the transition region, a bounded second-order upwind discretisation scheme (the van Leer scheme) is used in this region.

Also:
4.8.2 Transition (Page: 27)

When alpha is larger than approximately 0.6 in the mixed scheme (see Eq. 34 and Table 2), the non-dissipative effects of the CDS give rise to numerical oscillations and the boundary layer is tripped numerically.

I think his deduction based on these paragraphs is not reasonable enough.

I kbow it's not a pure 3D simulation and the papers claimed this. It's a quasi-3D simulation
Now I'm running the 3D LES with 33 nodes in spanwise direction and the length of 3% of the chord length and waiting for the results. Although you told that it needs a wider spanwise extent, but I have to choose this length because I need to compare the results with a reference simulation and they claimed that for 33 nodes, the 3% extent had better results that 8%. Also my computational power is very limited and I can't have more than 4 million cells.


The 3% length is adapted from the paper. You can check the following sections:
4.5.1 The resolution and extension in the spanwise direction (Page: 20)
4.8.3 Resolution in the streamwise and spanwise directions (Page: 29)

Best Regards

[FMDenaro]

Originally Posted by Moreza7

Thank you dear FMDenaro.

My friend sent me a PDF which has more details about the LES of this airfoil. You can download it here:
http://www.tfd.chalmers.se/~lada/pos.../simon_lic.pdf

He said that his comments on the central difference scheme is from this paper you can check it in the following sections that I quoted some of them:
4.4 Discretisation Schemes of the Convective Terms (Page: 17)
Also:
4.8.2 Transition (Page: 27)
I think his deduction based on these paragraphs is not reasonable enough.

LES is based on a basic assumption, the SGS model must account for the required energy transfer, that is both the inertial and disispative unresolved parts. The oscillation caused by central discretization is a different issue of numerical character. But in no way that implies that a bounded scheme must be used in LES. This is somehow a conflict of two different actions the limiter acting for numerical reason and the SGS model for the unresolved components. Usually the result is a very excess of dissipation.
The reason why the bounded scheme is present in Fluent is only one: to satisfy the users to get some solution, no matter of the accurate physical meaning.
But if your LES setup is correct and the grid is suitable, the unbounded scheme must work.

[Moreza7]

Originally Posted by FMDenaro

LES is based on a basic assumption, the SGS model must account for the required energy transfer, that is both the inertial and disispative unresolved parts. The oscillation caused by central discretization is a different issue of numerical character. But in no way that implies that a bounded scheme must be used in LES. This is somehow a conflict of two different actions the limiter acting for numerical reason and the SGS model for the unresolved components. Usually the result is a very excess of dissipation.
The reason why the bounded scheme is present in Fluent is only one: to satisfy the users to get some solution, no matter of the accurate physical meaning.
But if your LES setup is correct and the grid is suitable, the unbounded scheme must work.

Thanks a lot for your great replies.
I'm using unbounded central difference scheme now and I'm agree with you that Fluent just wants to give the user a solution while the LES needs accuracy. The funny thing is that by enabling LES and Smagorinsky subgrid scale model, it says that it must be used with bounded scheme!

After the new simulation results are ready, I'll post the results.

Best regards.

[FMDenaro]

Originally Posted by Moreza7

Thanks a lot for your great replies.
I'm using unbounded central difference scheme now and I'm agree with you that Fluent just wants to give the user a solution while the LES needs accuracy. The funny thing is that by enabling LES and Smagorinsky subgrid scale model, it says that it must be used with bounded scheme!

After the new simulation results are ready, I'll post the results.

Best regards.

You can force Fluent to use unbounded central scheme for LES. However, I suggest also to use the dynamic Smagorinsky model.

[Moreza7]

Originally Posted by FMDenaro

You can force Fluent to use unbounded central scheme for LES. However, I suggest also to use the dynamic Smagorinsky model.

Thank you dear FMDenaro! I'm using dynamic Samgorinsky model.

I just noticed something weird!
When I use Convective Outlet B.C for velocity + homogeneous Neumann B.C for pressure at the outlet boundary, the outlet mass flow is lower than the inlet mass flow. (The difference is about 0.5 kg/s and the total mass flow is about 50 kg/s)




But when I use the same B.C for the velocity, but Dirichlet B.C for pressure, the inlet and outlet mass flows are equal. It seems that there's a problem with the Neumann B.C for the pressure.

is that OK?


Best Regards

[MikeBravo]

Hi Moreza,

I think it is important that you look at time-averaged LES results. Your initial post was a snapshot of the LES, which can't be compared to RANS, even after you run the 3D domain. This will at least partially explain the differences in pressure and mass flows you observe. A 1% fluctuation in mass flow is not surprising, but the time-average fluctuation should be 0%.

I didn't see where anyone mentioned, but if you want to predict the transition of laminar to turbulent flow, it will be important to check that the eddy viscosity is very low in the laminar region for your mesh. Dynamic Smagorinsky should accomplish this, but I do not think it is a given. Here is a useful paper on the matter: https://web.stanford.edu/group/ctr/R.../09_sayadi.pdf

[Moreza7]

Originally Posted by MikeBravo

Hi Moreza,

I think it is important that you look at time-averaged LES results. Your initial post was a snapshot of the LES, which can't be compared to RANS, even after you run the 3D domain. This will at least partially explain the differences in pressure and mass flows you observe. A 1% fluctuation in mass flow is not surprising, but the time-average fluctuation should be 0%.

I didn't see where anyone mentioned, but if you want to predict the transition of laminar to turbulent flow, it will be important to check that the eddy viscosity is very low in the laminar region for your mesh. Dynamic Smagorinsky should accomplish this, but I do not think it is a given. Here is a useful paper on the matter: https://web.stanford.edu/group/ctr/R.../09_sayadi.pdf

Thank you very much dear Mike, your comments were really helpful I didn't know about the effect of subgrid scale model on the tranaition. However I used Dynamic Smagorinsky model.

And about the mass flow out, it's strange for me why while using the Drichlet boundary condition, mass flow does not oscillate and it only oscillates while using Nuemann B.C.

Best regards.

[FMDenaro]

How could you prescribe a Dirichlet BC at the outlet if the flow is unsteady ...

[Moreza7]

Originally Posted by FMDenaro

How could you prescribe a Dirichlet BC at the outlet if the flow is unsteady ...

Thanks for the reply.
I know the pressure outlet B.C in Fluent as Dirichlet because in the Docs it is given:

Pressure outlet boundary conditions require the specification of a static (gauge) pressure at the outlet boundary. The value of the specified static pressure is used only while the flow is subsonic. Should the flow become locally supersonic, the specified pressure will no longer be used; pressure will be extrapolated from the flow in the interior.

So as the flow is subsonic, the pressure at the outlet is set to the gauge pressure which is constant.

This is what I understand from the Docs. So if i'm wrong or it's a misunderstanding of the text by me, please correct me.

[FMDenaro]

Originally Posted by Moreza7

Thanks for the reply.
I know the pressure outlet B.C in Fluent as Dirichlet because in the Docs it is given:


So as the flow is subsonic, the pressure at the outlet is set to the gauge pressure which is constant.

This is what I understand from the Docs. So if i'm wrong or it's a misunderstanding of the text by me, please correct me.

Be aware, the set of BCs for the compressible subsonic flows is specified by one Dirichlet condition at the outlet but the other required BCs cannot be prescribed as Dirichlet.

[Moreza7]

Originally Posted by FMDenaro

Be aware, the set of BCs for the compressible subsonic flows is specified by one Dirichlet condition at the outlet but the other required BCs cannot be prescribed as Dirichlet.

Thank you dear FMDenaro.
Which boundary condition do you prefer for this problem at the outlet?
Is Neumann the best choice?

[FMDenaro]

Originally Posted by Moreza7

Thank you dear FMDenaro.
I'm talking about the outlet B.Cs Other B.Cs for the pressure are set to Neumann. Which boundary condition do you prefer for this problem at the outlet? Is Neumann the best choice?

I am also talking about the BCs for the outlet. For compressible subsonic flows you can fix a condition for the pressure (Dirichlet) but the other variables must be let free to develop from the interior, according to the characteristic theory

[Moreza7]

Originally Posted by FMDenaro

I am also talking about the BCs for the outlet. For compressible subsonic flows you can fix a condition for the pressure (Dirichlet) but the other variables must be let free to develop from the interior, according to the characteristic theory

Thank you.
The misunderstanding of your message is due to my poor English. Sorry for that.
So, I think I must go with Neumann B.Cs...

[MikeBravo]

Originally Posted by beeshma123

What might be a base separation the third way to consider? How about we accept that the harmony length is ONE. What's more, what number of cell layers in z-heading do we need to use for a genuinely decent goal of the 3d stream?

I'm not sure what you mean in your first question. But for the z-direction, if a scale-resolving simulation is done (i.e. LES), the length should be sufficient to capture the largest eddies, and the number of cells should be enough to keep the cell aspect ratio as close to 1 as possible as the filter shape can dampen turbulence in certain directions. Ideally z+ = y+ < 1.