[Scabbard]

Dear all,

I just start to use Star-ccm+. I try to simulate a flow past a stationary cylinder at Re=1e05. However, the result I got is quite different from the experiment. The previous experiment shows the Cd is around 1.1, my simulation result is around 0.55.

Here is the information of my cases,

Mesh:

cylinder diameter: 0.1m
flow velocity:1m/s
Re=1e05
Thickness of near wall prism layer 2e-05 (y+=1)
Aref 0.0314m/s^2 (the front area, my cylinder height is 0.314m)
timestep 0.0005s
simulation time: 10s

The flow inlet boundary is located 10D upstream from the centre of the cylinder and the flow outlet boundary is located 25D downstream from the center of the cylinder. The top and bottom boundaries are located at a distance of 10D from the center of the cylinder.

Mesh pictures are in attached


Models:
Three Dimensional
Gradient
Implicit Unsteady
Liquid (H2O)
Segregated flow
Constant density
Turbulent
Large Eddy Simulation
Dynamic Smagorinsky Sugird Scale
Low y+ Wall Treatment

Cd properties
Coordinate System : Laboratory
Direction:[1.0,0.0,0.0]
Force Option:Pressure+Shear ( I try only Pressure but there is no different and I don't know which option should I choose)
Reference Pressure: 0Pa
Reference Density: 997.561kg/m^3
Reference Velocity: 1m/s
Reference Area:0.0314m^2
Parts： cylinder

Boundary

cylinder: no-slip wall
inlet:velocity inlet
outlet pressure outlet
front,back,top, down: symmetry

I make first several time step interaction 150, the change it to 20, make the continuity residual close to 1e-04

I try the mesh polyheral mesh with 70w cell however the Cd is 0.55 which just half of the experiment result.

Could Anyone give me some recommendations about which setting is wrong in my case?
Many thank with your kindly help.

Here is my simulation case, I am using version 9.04.011-R8
https://docs.google.com/file/d/0B1v8...RmclRscHM/edit


Best Regards,
Scabbard

[FMDenaro]

I have first a simple question, are you sure you are reproducing the actual conditions realized in the experiment?

Then, to have a good resolution of the boundary layer you need to put 3-4 grid nodes within y+ <1

[Scabbard]

Originally Posted by FMDenaro

I have first a simple question, are you sure you are reproducing the actual conditions realized in the experiment?

Then, to have a good resolution of the boundary layer you need to put 3-4 grid nodes within y+ <1

Dear Filippo Maria Denaro,

The experiment result is infinite cylidner test. According to my literature review, when cylinder height= pi*D, it can be consider as infinite.

I will have a try with put 3-4 gird nodes within y+<1.

However, I think will this several layer cause 50% error?

Many thanks for your help.

Best Regards,
Scabbard

[FMDenaro]

Originally Posted by Scabbard

Dear Filippo Maria Denaro,

The experiment result is infinite cylidner test. According to my literature review, when cylinder height= pi*D, it can be consider as infinite.

I will have a try with put 3-4 gird nodes within y+<1.

However, I think will this several layer cause 50% error?

Many thanks for your help.

Best Regards,
Scabbard

well, 1) consider the inlet velocity in the experiment, do you reproduce the same profile?? 2) are you sure the spanwise extension in the experiment is disregardable?

Finally, the wall stress must be computed quite accurately, therefore putting only a node at y+=1 is not sufficient

[Scabbard]

Originally Posted by FMDenaro

well, 1) consider the inlet velocity in the experiment, do you reproduce the same profile?? 2) are you sure the spanwise extension in the experiment is disregardable?

Finally, the wall stress must be computed quite accurately, therefore putting only a node at y+=1 is not sufficient

Dear FMDenaro,

1) yes the velocity reproduce the same profile, uniform flow.
2) According to the literature 3.14D is enough

I am now trying to add 3-4 layer within y+<1 and look through the result

Because current result is 50% error by chance, this make me thinking some setting may be set wrong value in my case.

Many thx for your kindly help.

Best Regards,
Scabbard

[flotus1]

How did you estimate a suitable time step size for your case?
Did you use periodic boundary conditions for the two side walls? If you use symmetry boundary conditions instead, the axial extent of the computational domain has do be even higher than the 3.14*D usually recommended.
And even though the wall yplus of your mesh may be below 1, the xplus and zplus values seem to be way too high for a wall-resolved LES. Even the cells far away from the wall seem to have an aspect ratio that is too high for LES.
Are you sure that you have the computational resources to perform a valid LES with high Reynolds numbers?
BTW: polyhedrons are not the best choice for LES, hexahedrons perform better.

[Scabbard]

Originally Posted by flotus1

How did you estimate a suitable time step size for your case?
Did you use periodic boundary conditions for the two side walls? If you use symmetry boundary conditions instead, the axial extent of the computational domain has do be even higher than the 3.14*D usually recommended.
And even though the wall yplus of your mesh may be below 1, the xplus and zplus values seem to be way too high for a wall-resolved LES. Even the cells far away from the wall seem to have an aspect ratio that is too high for LES.
Are you sure that you have the computational resources to perform a valid LES with high Reynolds numbers?
BTW: polyhedrons are not the best choice for LES, hexahedrons perform better.

Dear flotus,

I try to make the CFL around 1. also I tried to simulate this case by k epsilon with periodic boundary and les with periodic boundary. However, the Cd turn to 0.41... still to far from 1.1

Best Regards,
Scabbard

[Scabbard]

Dear all.

I try to use the structure mesh and k-epsilon to simulate this case, get Cd same around 0.54.

I define the reference area = diameter of the cylinder*height of the cylinder.

Could you tell me which setting is wrong? I am really sick of this, everything seems right except the result...

here is the case:
https://drive.google.com/file/d/0B1v...ew?usp=sharing

Best regards,
Scabbard

[FMDenaro]

Trying to reproduce exactly an experiment requires to be sure of all the relevant factors, looking only to integral quantities is somehow misleading... for example, the experiment reproduces some measure of velocity in time?
Are you able to compare the experimental and the numerical inflow profiles?
From you results I see oscillations that appear too regular for a turbulent flow, the vortex shedding seems almost laminar...

[Scabbard]

Originally Posted by FMDenaro

Trying to reproduce exactly an experiment requires to be sure of all the relevant factors, looking only to integral quantities is somehow misleading... for example, the experiment reproduces some measure of velocity in time?
Are you able to compare the experimental and the numerical inflow profiles?
From you results I see oscillations that appear too regular for a turbulent flow, the vortex shedding seems almost laminar...

Dear FMDenaro,

For a flow past a infinite cylinder. The Cd won't change too much from re 3900 to re 3*10e5, it should be around 1. If there is a factor of 2 involved, it seems like I am making a consistent mistake somewhere. However, I cannot find where is the mistake.

For the oscillations appear too regular, this is because the simulation method is URANS. If it is the LES, it won't be oscillated like this.

Many thx,
Scabbard

[FMDenaro]

Originally Posted by Scabbard

Dear FMDenaro,

For a flow past a infinite cylinder. The Cd won't change too much from re 3900 to re 3*10e5, it should be around 1. If there is a factor of 2 involved, it seems like you are making a consistent mistake somewhere. However, I cannot find where is the mistake.

For the oscillating too regular, this is because the simulation method is URANS. If it is the LES, it won't be oscillated like this.

Many thx,
Scabbard

Ok, in terms of URANS is acceptable, could you plot the LES result?... again, to understand the problem in your code you cannot debug your solution from an integral parameter but you need to assess if the setup of the problem is correctly reproducing your experiment. Check the velocity field and the boundary conditions to assess that the experiment is well reproduced.

I assume that in the experiment a "noise" is introduce into the velocity, depending on the turbulence intensity generated. If you simply set a plug inflow velocity, the LES would not reproduce the correct evolution around the cylinder.
Finally, computing the wall stress correctly requires a fully resolved boundary layer over the cylinder that requires a huge number of computational nodes

[Scabbard]

Originally Posted by FMDenaro

Ok, in terms of URANS is acceptable, could you plot the LES result?... again, to understand the problem in your code you cannot debug your solution from an integral parameter but you need to assess if the setup of the problem is correctly reproducing your experiment. Check the velocity field and the boundary conditions to assess that the experiment is well reproduced.

I assume that in the experiment a "noise" is introduce into the velocity, depending on the turbulence intensity generated. If you simply set a plug inflow velocity, the LES would not reproduce the correct evolution around the cylinder.
Finally, computing the wall stress correctly requires a fully resolved boundary layer over the cylinder that requires a huge number of computational nodes

Dear FMDenaro,

The LES result is in attached.

Because I also simulated this in Fluent and openFoam. They all generate more or less Cd around 1, but star ccm give a value around 0.54. I am quite confused about where is the mistake I make in the Star-ccm+.

The computational nodes is not a big problem for me.

Best Regards,
Scabbard

[FMDenaro]

I suggest to check the effect of the SGS model, you can perform a no-model LES turning off the model.
Furthermore, be sure that the discretization used by star-ccm+ is fully second order in time and space.
The Cd is computed in the code or you are post-processing the data?

[Scabbard]

Originally Posted by FMDenaro

I suggest to check the effect of the SGS model, you can perform a no-model LES turning off the model.
Furthermore, be sure that the discretization used by star-ccm+ is fully second order in time and space.
The Cd is computed in the code or you are post-processing the data?

Dear FMDenaro,
I almost followed a master dissertation about using star ccm+ simulating a flow past a cylinder

http://www.diva-portal.org/smash/get...FULLTEXT01.pdf

The Cd is computed in the code. However I also get the force on the cylinder, I use Cd=Fd/(0.5*density*inlet velocity^2*reference area) reference area= diameter of the cylinder * height of the cylinder, I get same value around 0.55

I guess I make some mistake about some constant settings. But I think I follow all the Star ccm tutorial and this dissertation suggestion. This make me crazy.

Best Regards,
Scabbard

[FMDenaro]

Again, in my opinion checking the quality of a LES solution only by a derived integral quantity is not correct...first you have to assess if the resolved fields are congruent. That requires statistical analysis and checking for average profiles, energy spectra, correlation, and so on...
Then, Cl and Cd quantity can be computed in a post-processing implemented by you.
Maybe your LES solution is correct and for some reason you just get a wrong Cd by star-ccm+

[kykim]

the Cd value is almost exactly half of tje solution. How about check wether coefficients for calculating Cd is the same or not

[Scabbard]

Originally Posted by kykim

the Cd value is almost exactly half of tje solution. How about check wether coefficients for calculating Cd is the same or not

Dear kykim,

I try simulate the Re=10000 and 3900 case, perfectly match the experiments results. How ever only this 1e05, no matter how fine the mesh i make, still got around 0.5. I think 1 million mesh for k-e or k-omega sst is a fine enough mesh...

Best Regards,
Scabbard

[kykim]

The grid is fine enough if you use RANS. However you said that you use LES at first. what exactly do you use? if you use LES then I recommed to see instanteneous or averaged field. you have to check not just Cd but the the field of simulation is reasonable or not.

[Scabbard]

Originally Posted by kykim

The grid is fine enough if you use RANS. However you said that you use LES at first. what exactly do you use? if you use LES then I recommed to see instanteneous or averaged field. you have to check not just Cd but the the field of simulation is reasonable or not.

Dear kykim,

After I got wrong result, I tried to simulate this case in both steady and unsteay in these days( k-e and k-omega) how ever both of them I got Cd around 0.55

Best Regards,
Scabbard

[jsb12136]

Originally Posted by Scabbard

Dear kykim,

After I got wrong result, I tried to simulate this case in both steady and unsteay in these days( k-e and k-omega) how ever both of them I got Cd around 0.55

Best Regards,
Scabbard

I got the exactly same results with you. Do you know how to solve this problem now? My Cd is always around 0.5 no matter how I change the settings. I have been struggling on this problem for a long time.