[jai174121]

Hi Guys

Im trying to simulate flow over a 3D Cylinder (pictures of the mesh generated using ICEM CFD are attached aswell as results). Im using the standard K-omega model for Re=3900 however when I go ahead and import the mesh into Fluent and check the quality of the mesh I get the following message:

The mesh contains very high aspect ratio 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.

I discard the message and start the simulation, the results i get for cd mean value is greatly over predicted at 3.72 when it should be around 1.32.

The mesh has 441680 nodes and an aspect ratio of 404!

I would be grateful for any help that anyone can offer im really confused at the moment and urgently need to attain some good results.

How can I can reduce the aspect ratio ? What else can I do to obtain a lower cd and cl value?

[`e`]

First of all, address the error message Fluent is providing you. If you can't fix your mesh; perhaps use a simpler O-grid type mesh. This mesh type performs well for both URANS and LES turbulence models for cylinder in cross-flow (2-D and 3-D). Furthermore, start with 2-D simulations to tune the settings (there's plenty of results from simulations and experiments in the literature at Re = 3900).

[jai174121]

Thanks for your reply e

Ive spent the last week generating simpler meshes as shown attached but Im still getting overpredicted cd values. For 2D cases all meshes attain reasonable cd values (0.95 to 1.4). Cl values are also reasonable for both 3D and 2D URANS cases. I used the standard k-omega model (altered y+ to be around 30 close to the cylinder wall) as well as the transitional k-kl-omega model (y+ around 1 clsoe to the cylinder).

However im not sure what Im doing wrong so I'll quickly run through my case:
Simulation type 3D Unsteady Double Precision Pressure based and implicit
Re=3900
Diameter of cylinder= 1
u=1
mu=0.00025641
Density=1

Model - k-omega standard (other models were used but still yielded same results)

Turbulence Intensity - 5%
Turbulent viscosity ratio = 10

Solving for 1000 timesteps, 0.233 time step size and 20 iterations per time step.

Any advice would be greatly appreciated.

Thanks (Screenshots are attached)

[Far]

what are your reference values?

[jai174121]

Ok so I made a silly mistake and left the area as 1 when simulating for a 3D case, now changing to its correct value of 11.5 m^2 the mean drag coefficient is around 0.36 now.

For the other reference values:

Density = 1
Enthalpy = 0
Length = 1
Pressure = 0
Temperature = 288.16
Velocity=1
Viscosity=0.00025641
Ratio of specific heats = 1.4

[Far]

The mesh contains very high aspect ratio 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.

This message requires a little bit background of CFD and numerical methods. Without going into those details, I would suggest "Don't care about these warnings..." unless you have high aspect ratio elements in far-field, interfaces etc...

Take a look at this two part tutorial https://www.youtube.com/watch?v=anTkWfMyEPM

[Far]

Originally Posted by jai174121

Ok so I made a silly mistake and left the area as 1 when simulating for a 3D case, now changing to its correct value of 11.5 m^2 the mean drag coefficient is around 0.36 now.

is this the correct value at Re = 3900?

[jai174121]

Thanks for the link Far

Unfortunately no its not the correct value for Re=3900 URANS it should be around 0.98.

I calculated the area of the cylinder using (2*pi*r*h + 2*pi*r^2). Where r is 0.5 and h is 3.14.

Any ideas on what I could be doing wrong?

[ssss]

Why 2*pi*r^2? In my opinion that area should not be taken into account

[Far]

Originally Posted by jai174121

Thanks for the link Far

Unfortunately no its not the correct value for Re=3900 URANS it should be around 0.98.

I calculated the area of the cylinder using (2*pi*r*h + 2*pi*r^2). Where r is 0.5 and h is 3.14.

Any ideas on what I could be doing wrong?

It should be the plane area normal to flow direction. Since this is cylinder, so no more thoughts. Just use diameter * height

[jai174121]

Yep thank you that worked.