[Anna Tian]

Hi,

I have Ma=0.15 in my project and Re=4 millions in my project. If I keep both Y+ and aspect ratio at good values, the grids number will be too high. So I may have to scale it to a smaller size. But Re will decrease with scaling. I have no idea about whether that will bring any inaccuracy or not. Does anyone have any experience about how to deal with this problem?

Btw, I don't expect boundary layer separation in my case. But I'd also like to know how to deal with this problem if I have BL separation which could be influenced by Re.

And how much could I scale? Could I scale it by 1000 times smaller?

[lovecraft22]

You mean you want to scale your geometry? Or am I missing something?

[flotus1]

Scaling the size of your flow problem wont get you anywhere.
You have to keep the relevant dimensionless numbers constant (at least Ma and Re in your case) which will lead to the exact same prerequisites for the discretization, regardless of the size.

But I doubt that you really have a constraint on the aspect ratio of the cells. In the boundary layer of flows with high Reynolds numbers, it is normal to have cells with high aspect ratios. Enabling double precision and checking the wall-normal distance makes aspect ratios of 10000:1 or even higher no problem, at least in Fluent. But any other CFD software should be able to handle this aswell.
High aspect ratio cells would only cause problems in the free-stream region of the flow.

[Anna Tian]

Originally Posted by lovecraft22

You mean you want to scale your geometry? Or am I missing something?

Yes. I'd like to scale my geometry.

[Anna Tian]

Originally Posted by flotus1

Scaling the size of your flow problem wont get you anywhere.
You have to keep the relevant dimensionless numbers constant (at least Ma and Re in your case) which will lead to the exact same prerequisites for the discretization, regardless of the size.

But I doubt that you really have a constraint on the aspect ratio of the cells. In the boundary layer of flows with high Reynolds numbers, it is normal to have cells with high aspect ratios. Enabling double precision and checking the wall-normal distance makes aspect ratios of 10000:1 or even higher no problem, at least in Fluent. But any other CFD software should be able to handle this aswell.
High aspect ratio cells would only cause problems in the free-stream region of the flow.

Thanks for your answer. But you know, for airfoil CFD, people likes to use C-block mesh. So at the wake area, the aspect ratio will also be very high. That is the free stream area. Any idea or experience about treating this problem?

[levivad]

as previously said you need to keep Re and Ma numbers constant to have correct results (like in wind tunnels).

My 2 cents are to have the mesh at the wake slowly grow as distance from the airfoil increases. do a mesh study (not sure it'll be much quicker)

[lovecraft22]

As already said that will take you nowhere: the smaller the geometry the smaller the mesh size will have to be. Besides, by doing that, you'll lose the Re and Ma analogy…

If it is a full airplane you may want to consider using a symmetry plane. If is it just a wing and you're not interested in 3D structures then you may want to try a 2D simulation. Otherwise… no way of reducing the number of cells unless you increase your finest cell size.

[Anna Tian]

Originally Posted by lovecraft22

As already said that will take you nowhere: the smaller the geometry the smaller the mesh size will have to be. Besides, by doing that, you'll lose the Re and Ma analogy…

If it is a full airplane you may want to consider using a symmetry plane. If is it just a wing and you're not interested in 3D structures then you may want to try a 2D simulation. Otherwise… no way of reducing the number of cells unless you increase your finest cell size.

Thanks. So I not only need to keep Re the same but also Ma.

I use the experimental data from the book 'THEORY OF
WING SECTIONS'. I'd like to know which page of this book tells the Mach number in its experiment for NACA 2412. I looked for this condition for quite a long time in that book but didn't find out that value. Could you tell at which page could I find the Mach value of its experiment?

[Anna Tian]

Originally Posted by levivad

as previously said you need to keep Re and Ma numbers constant to have correct results (like in wind tunnels).

My 2 cents are to have the mesh at the wake slowly grow as distance from the airfoil increases. do a mesh study (not sure it'll be much quicker)

Thanks. So I not only need to keep Re the same but also Ma.

I use the experimental data from the book 'THEORY OF
WING SECTIONS'. I'd like to know which page of this book tells the Mach number in its experiment for NACA 2412. I looked for this condition for quite a long time in that book but didn't find out that value. Could you tell at which page could I find the Mach value of its experiment?

[Anna Tian]

Originally Posted by flotus1

Scaling the size of your flow problem wont get you anywhere.
You have to keep the relevant dimensionless numbers constant (at least Ma and Re in your case) which will lead to the exact same prerequisites for the discretization, regardless of the size.

But I doubt that you really have a constraint on the aspect ratio of the cells. In the boundary layer of flows with high Reynolds numbers, it is normal to have cells with high aspect ratios. Enabling double precision and checking the wall-normal distance makes aspect ratios of 10000:1 or even higher no problem, at least in Fluent. But any other CFD software should be able to handle this aswell.
High aspect ratio cells would only cause problems in the free-stream region of the flow.

Do I need to keep Ma number the same? I heard about that if the mach number is much lower than supersonic, then it won't have a influence on the drag coefficient。

[gfoam]

Yes you're right, for example if you have M<=0.3 in the whole domain and you don't have zones with higher mach numbers you can cosideer it as a incompressible flow, and the Cl, CD and Cm coefficients will be the same if you model the flow as a compressible one or not. regards.
Gonzalo