Hi!

I am simulating flow over a cylinder and want to get drag coefficient at various reynolds numbers. I modelled 2-D cylinder by making a circular hole in a rectangle and applied no slip boundary condition over the spherical hole. Also I applied velocity inlet and pressure outlet boundary condition. Now the problem is I am getting drag coefficient with a deviation of 20-40% from the experimental results. For example, I am getting Cd = 0.6 at Re = 1000, which should be 1 according to experimental results. I used standard k-e turbulence model.

Please help.

-Avijit

Have u checked grid convergence ? make a mesh which is twice as finer and run the same simulation and see if you get the same results

are you checking your residuals ?

Domain size might be another issue , is your domain big enough

check the above 3 these might lead you onto the right path

-Ajay

you should also check the values of y+ and y* over the cylinder's surface, and adjust them to the values sugested by fluent (see user's guide) for k-e model...

I forgot to tell that im using Ansys Flotran (7.1) and not Fluent. Also I am new to CFD so would like to clearify ur points.

1. what do u mean by grid convergence? As far as I know ur solution is said to be converged if pressure, velocity, k and e coefficients become smooth and constant in the convergence monitor (graph between Normalised rate of change and cumulative iteration number). In my case k and e coefficients become smooth but pressure and velocity coefficients become unstable (their shape become something like this /\/\/\/\/\/).

2. As far as meshing is concerned I think I have made it fine enough. Now my computer (P4- 2GHz, 256Mb RAM) is taking 20 minutes to do 1000 iterations. I have also checked the solution by both mapped and un-mapped (unstructured) meshing. But the results are coming almost the same.

3. What do u mean by "residuals" ?

4. I think my domain size is big enough. Outer domain size is 50m x 100m and diameter of cylinder = 1m.

Thanks a lot

-Avijit

Grid convergence is getting the same solution for a more finer grid usually u mesh it twice as fine and if u find the results to be the same as befor ethen you have grid convergence.

-> Are you doing an unsteady case ? or a steady one? if it is unsteady then try using smaller time steps.

^^^^^^ in the velocity and pressure should be smooth i guess , If you are doing a steady case then due to vortex shedding u would get ^^^^^^

residuals are same as your convergence monitors. Make sure that you give low values for your convergence criteria . continuity should be less than 10-3 at least.

-Ajay

Hi Ajay,

I am still getting /\/\/\ in velocity and pressure. how can i make it smooth?

also i checked my Y+ values, they r within 7. is it ok? i have noticed one thing that the variation of Y+ is within the nearest but one set of elements around the cylinder. do i have to make my mesh more fine?

avijit

Avjit Try reducing the time step to smaller values till u get a smooth variation I dont have much idea about K-E model so cant answer ur other question -Ajay

I am working on similar problems in Fluent. The flow field is periodically steady behind a cylinder so I think it reasonable for the pressure field to oscillate periodically around a constant value when you time achieved infinity. Did you try enhanced wall treatment and check the options of pressure gradient and thermal effect? It is also important that you set appropriate boundary conditions (turbulence level, turbulence length scale, etc.). I do not know how you calculate drag coeff. If you are reporting from Fluent, one has to choose the right referenc values. According to my experience, ANSYS can not have meshes as fine as Fluent and it does not give good values for my simulation.

Hi Zhihua,

thanks for ur advice. I am new to CFD so can u elaborate more on "enhanced wall treatment" and "boundary conditions (turbulence level, turbulence length scale, etc.)" Are u talking about the inlet kinetic energy and inlet kinetic energy dissipation rate epsilon ?

what should be their approx values.

-Avijit

When you defined your viscouse model, you will find 3 selections under: near wall treatment under the k-epsilon model. The first one is application to high Re flow (if you read some old paper, you will find all authors use it at Re>10^5). I am not sure about the second one. The 3rd one,that is enhanced wall treatment, considers the effect of large pressure gradient of the wall so I think it more appropriate for flow across blunt bodies.

About boundary conditions, Yes, I am talking about the inlet k and epsilon value. Currently I am setting the turbulence intensity to 1% and turbulence length scale to 0.07D. The 1% value is a low turbulence value for wind tunnels. It should be close to the value in the experiment to be compared wiht. The formula of estimating the tur. length scale is available in Fluent manual, where all the tur. models are discussed. It also discusses the near wall treatment. I think it helpful if you read it.

My CD at Re=600 is 1.13.

i made some changes in inlet kinetic energy boundary conditions. after doing that i got better results but the convergence monitors showed very unstable values for Press, Velocity ,ENDS and ENKE. is it correct?

The pressure and velocity will surely oscillate around a constant value due to the periodically steady vortex shedding behind the cylinder. I suggest compare the local friction coefficient and local pressure coefficient with experimental values in literature to make sure you get the right answer. The accuracy can also be improved by using second-order differential method. Good luck!

[yhy20081016]

Flow past cylinder is a challenging case for CFD. You should understand the physics if you want to simulate it reasonably. For instance, at Re=1000, the attached boundary layer on the cylinder is laminar; the boundary layer separates at about 82deg and the wake is turbulent. However, you cannot simply employ a turbulence model like k-epsilon to compute the flow; using a turbulence model makes the boundary layer separation point moves to the rear side (>90deg), and hence the wake is much narrower than reality, and therefore the drag is much smaller than reality. In reality, the separation point does not move to the rear side until much higher Reynolds number (about 2.5E5; "the drag crisis":at this Reynolds number, boundary layer transitions occur and the boundary layer becomes turbulent).