[mrwts]

Hello everybody!

How can I calculate the Reynolds Number in Fluent?
Which specific values should I use in order to calculate that value and present the results for further comparison.

I've been working on an airfoil numerical validation using a NASA provided grid. According to their data, the Mach Number is equal to 0.15 and the Reynolds Number per chord equals 6 Million (under standard conditions). The simulation is run using Sutherland's Model for density. Nevertheless, if using standard values my calculations yield a Reynolds number of 3 Million and if using the Reference Values given by Fluent it yields 5 Million.

How can I know which values should I use? And for CD and CL what is the influence that Reynolds Number will have on their values? (considering a 1 million or 3 million deviation)

[shereez234]

Originally Posted by mrwts

Hello everybody!

How can I calculate the Reynolds Number in Fluent?
Which specific values should I use in order to calculate that value and present the results for further comparison.

I've been working on an airfoil numerical validation using a NASA provided grid. According to their data, the Mach Number is equal to 0.15 and the Reynolds Number per chord equals 6 Million (under standard conditions). The simulation is run using Sutherland's Model for density. Nevertheless, if using standard values my calculations yield a Reynolds number of 3 Million and if using the Reference Values given by Fluent it yields 5 Million.

How can I know which values should I use? And for CD and CL what is the influence that Reynolds Number will have on their values? (considering a 1 million or 3 million deviation)

Hello, I actually had the same confusion when I did this. You are right the reynolds number based on Chord Length of 1 is = 3 million.

To answer your questions:


1)
- Fluent does not give a reynolds number calculation tool or output.
- As you know by now Re = Rho * Cref * Velocity / Dynamic Viscocity

2) How much does it affect this particular simulation: I quote the NASA website from which you read this validation case:

"but were at a lower Re of 3 million. Lift data are not affected too significantly between 3 million and 6 million, but drag data are (e.g., according to McCroskey, tripped CD,0 at Re=3 million is about 10% higher than tripped CD,0 at Re=6 million) "

Oh and if you actually want to compare with them Use 6 million that's the advice I can give. because I am sure they used 6 million and not 3 million.
Here is their input file ( which again you can find on the same website).

NACA 0012
XMACH ALPHA BETA REUE,MIL TINF,DR IALPH IHSTRY
0.1500 10.0000 0.0000 6.0000 540.0000 0 0

3) How to achieve Re = 6 million?
Well it's easy
- either you can scale the chord length twice so Cref = 2m
- Or you can change the viscosity ( halve it)
I personally scale the chord length ( I prefer that way rather than playing with viscosity which is nonphysical in my head)

[mrwts]

Originally Posted by shereez234

How to achieve Re = 6 million?
Well it's easy
- either you can scale the chord length twice so Cref = 2m
- Or you can change the viscosity ( halve it)
I personally scale the chord length ( I prefer that way rather than playing with viscosity which is nonphysical in my head)

I actually had the same idea about halving the viscosity, but it didn't seem physically correct to me either.

Considering the first scenario, when you scale the chord length twice (Cref = 2m) that would mean, in the Fluent interface, to set the reference value for the area to 2 m2 instead of 1 m2 (by default). Am I right? Or does Fluent uses a different value to calculate the Cd and Cl? Otherwise, as long as I understand, it wouldn't affect at all the Cd and Cl calculation.

In order to get a reliable comparison (under the CFD community standards), considering that I am having troubles dealing with the Re number confusion, is it acceptable to just take into account that 10% increase and just subtract it from the value obtained or it would be better to achieve the 6 million value for Re? What is more recommended?

I am trying to improve Cd and Cl by using heat transfer, so I would like to have a exact base values to compare with. Thank you in advance.

[shereez234]

Originally Posted by mrwts

I actually had the same idea about halving the viscosity, but it didn't seem physically correct to me either.

Considering the first scenario, when you scale the chord length twice (Cref = 2m) that would mean, in the Fluent interface, to set the reference value for the area to 2 m2 instead of 1 m2 (by default). Am I right? Or does Fluent uses a different value to calculate the Cd and Cl? Otherwise, as long as I understand, it wouldn't affect at all the Cd and Cl calculation.

In order to get a reliable comparison (under the CFD community standards), considering that I am having troubles dealing with the Re number confusion, is it acceptable to just take into account that 10% increase and just subtract it from the value obtained or it would be better to achieve the 6 million value for Re? What is more recommended?

I am trying to improve Cd and Cl by using heat transfer, so I would like to have a exact base values to compare with. Thank you in advance.

1) You are right. Fluent uses Reference Area and Reference Length for CD and CL calculation. However, if you have want to have chord length of 2m and A = 2m your mesh should represent the same length. You can't just change the Cref and Sref to any value you want you should change it to represent real length of airfoil in the domain.

So what this means is scale your mesh twice to make Cref and Aref from 1 to 2 and import to fluent again. ( because when you change Chord length your Y height of first cell changes, think about it).

2) if you want to get the exact CL and CD, make sure >>>

a) you trailing edge spacing in the mesh is small enough.
b)you use the actual grid elements ( I think 240,000 elements?)
c) your Y+ = 1
d) Turbulent Visocity levels are initialized correct ( I think it was T.V.R = 0.009 at the inlet and Turbulent Intensity = 0.052 % at the inlet).

Regards
Shereez

[shereez234]

Originally Posted by shereez234

1) You are right. Fluent uses Reference Area and Reference Length for CD and CL calculation. However, if you have want to have chord length of 2m and A = 2m your mesh should represent the same length. You can't just change the Cref and Sref to any value you want you should change it to represent real length of airfoil in the domain.

So what this means is scale your mesh twice to make Cref and Aref from 1 to 2 and import to fluent again. ( because when you change Chord length your Y height of first cell changes, think about it).

2) if you want to get the exact CL and CD, make sure >>>

a) you trailing edge spacing in the mesh is small enough.
b)you use the actual grid elements ( I think 240,000 elements?)
c) your Y+ = 1
d) Turbulent Visocity levels are initialized correct ( I think it was T.V.R = 0.009 at the inlet and Turbulent Intensity = 0.052 % at the inlet).

Regards
Shereez

Oh hey I forgot you are using the provided grid. You should be fine then. Just scale the grid twice and give the correct turbulence at the inlet.