Flow around an circular cylinder
 

Hello everbody,

im working in a project at my university. And a part of this project is to simulate a flow around a circular cylinder.


My main problem is that i can not reach the values for the drag coefficent that i read in Schlichting.
cd(Re=300) = 0.729 | stationary
cd(Re=300) = 1.32 | instationary




1. The mesh

I Meshed everything in ICEM as octree mesh and put some prism elements around the cylinder.

http://s1.directupload.net/images/140325/lie69z47.png

2. CFX

Steady State

ref Pressure = 1 bar
T.Model = SST

Boundarys:
Inlet - v = 1,46 m/s
Outlet = 0 bar
Sides = Symetry
Zylinder = Wall no slip
Top and Bottom = Wall free slip

Transient

same as in steady state and i calculated with an Stroudhal number of 0.2 for the transient Setup:

Simulation Time 0.01 s
Timestep Size 0.0041 s (~25 steps)


Now the Problem:

For Steady state i get a cd value of 0.83
And for Transient i get an cd value of 1.1

I think both of the simulations are setup wrong because when i take a look at the pressure distribution it doesnt look like something i expect.

http://s14.directupload.net/images/140325/tsiuvgwh.png



Where did i make the mistake? Why is there no karman street like in this video http://www.youtube.com/watch?v=BVyu4UEiB1k ?

Is maybe just my simulation time not long enougth?

Or is my reference Re Value wrong?

I calculatet the Re and cd Value with a specific length = (diameter * length)

FAQ: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

A few things:

- Your boundary layer mesh looks very coarse. You should start by checking the Y-plus on the cylinder wall (should be <1-2 for SST).
- Regenerate the mesh using a smaller growth ratio for the boundary layers (try 1.1-1.2).
- Make sure you have enought layers around the cylinder to cover the whole height of the boundary layer.

Cheers.

http://s7.directupload.net/images/140326/hag8zp2q.png

I think this looks better :)

But there is still the possibillity to improve, maybe behind the cylinder.
Is my y+ ok for SST with auto wall treatment?

Yes, that looks much better. But you might still be a bit coarse - you will need to do a sensitivity check to find out.

Your y+ means that the automatic wall treatment will be integrating to the wall at all locations. You should be OK here, but again, a sensitivity check is the best way to be sure.

In a tutorial they initilaize the u velocity with (step(y/1[m])+ 0.5)*xvelociy
I Know what the step function do but what means the y and why Do they use this for initilaizing?

The y/1[m] bit converts y as a value with units of metres to a value with no units. The step function requires an argument which is unitless.

Is the value of y the max. y value of my domain in meter? They dont specify y in one of their expressions.

Why do they set up the Initial value with a step function? Whats the benefit of it?
Is it wrong to initilize just with my x_velocity?



- Im confused!

No, y is a field variable and takes the value of the y coordinate of that point. So it varies at each point of the domain.

I suspect they use this initial condition to give the flow a strong asymmetry to start the vortex street off. This is probably not required and I would start as you have assuming just a constant X velocity. I would only artificially introduce an asymmetry if it is really required.

thank you very mutch :)