- **OpenFOAM Running, Solving & CFD**
(*http://www.cfd-online.com/Forums/openfoam-solving/*)

- - **Circular Cylinder at low Reynold number mesh and non orthogonal corrections**
(*http://www.cfd-online.com/Forums/openfoam-solving/58891-circular-cylinder-low-reynold-number-mesh-non-orthogonal-corrections.html*)

Hello everybody,
I try to sHello everybody,
I try to solve the benchmark proposed ans studied by Schäfer and Turek in this paper. I have found some linked topic here and here, but they don't really answer my questions. For the moment, I consider the first case proposed in the benchmark (steady simulation, parabolic input velocity with max 0,3m/s leading to a Reynold number around 20). You will find here some pictures of typical meshes I use: http://www.cfd-online.com/OpenFOAM_D...ges/1/7647.png http://www.cfd-online.com/OpenFOAM_D...ges/1/7649.jpg And the "annoying" results: http://www.cfd-online.com/OpenFOAM_D...ges/1/7648.png As one can see, the velocity field is not really physical as the flow don't want to enter the fine mesh surrounding the cylinder. I use icoFoam with steadyState time integration scheme. The initial condition are zero velocity and pressure fields (according to the description of the benchmark). I'm doing one time step (Is the steady solution independant of the size of the time step ?). For PISO algorithm I tried many solution with high number of orthogonal and nonOrthogonal correctors (let's say respectively 300 and 20)...leading to more time expensive computation but not really better results. I also checked the mesh with the checkMesh utility: Mesh non-orthogonality Max: 44.01408683 average: 11.32517179 Non-orthogonality check OK. My question are the following: 1 - is it absolutely necessary to compute first a solution with potential foam (as proposed in one of the thread)?...I think it will not really respect the benchmark proposed I my case. 2 - Do you see any mistake in my procedure? 3 - Is they a way to link the non-orthogonality results obtained by checkMesh to the number of orthogonal and nonOrthogonal correctors. 4 - Other question : in the paper by Schäfer and Turek they speak about a recirculation area that as to be measured. What is this? Is they an easy way to automatically measure this in OpenFoam (not seeing the results in paraFoam)? Thank you for any help or comments. |

1) No, it is no need to comput1) No, it is no need to compute potential solution - this may only improve solution convergence
2) YOU SHOULD NOT USE icoFoam with steady-state time integration scheme, because icoFoam uses TRANSIENT prec-vel coupling algo, PISO 3) Your mesh thikness in Y-direction is too small, mesh thikness should be about 50-100 diamterers of cylinder (character length). what is your BC's on upper and lower walls? opt. number of non orthogonal correctors is 1-3 4) I can't donload papers by your references |

the solver icoFoam isn't statithe solver icoFoam isn't stationary ! this solver needs an time integration scheme, because it solves the isothermal incompressible Navier-Stokes-equation ! so it also need time-steps !
Get some Books about "Fluidmechanics" and "wake flow around a circular cylinder" there you find many specifications about "recirculation area" ! Can you send me the paper per email ? I can't open the link ! astadfm@gmx.de |

Thank you for the hints.
1 Thank you for the hints.
1 - Ok, It was what I was thinking about potential solution. 2 - Not use icoFoam means use something like simpleFoam ? 3 - The mesh thikness, is, I admit, really not enough to avoid influence of boundary conditions on the flow around the cylinder, especially with the no-slip boundary condition I impose...but this is how the problem is defined in the paper (hope the link will work now). |

2 - yes, use simpleFoam with t2 - yes, use simpleFoam with turbulence "off" and
turbulenceModel "laminar" (file constant/turbulenceProperties) 3 - for freestream boundary i'm using pressureInletOutletVelocity for U and outletInlet for p. And, of course, if you want to compare your results with those in paper, you must use BC's from paper 4 - the link work |

Hello again,
I try for the Hello again,
I try for the moment two strategies in parallel, with, for both, initial state computed by potential foam solver. with simpleFoam (steadyState for time integration, output specified through the use of inletOutlet, laminar flow without any turbulence as a model): The results are the following http://www.cfd-online.com/OpenFOAM_D...ges/1/7674.png http://www.cfd-online.com/OpenFOAM_D...ges/1/7675.png They are not so bad. Unfortunately in notice two problems : - The computation blows up after the first time step (does it really make sense to make more than one time step, as steadyState is for static case).
- The drag coefficient obtain is around 82...far from the 5.5 awaited.
with icoFoam: I run the computation with an Euler time integration scheme. This seems to behave as awaited. Unfortunately, the Drag coefficient exhibits the following shape when drawing respect to time (the value at the end is not so bad, as one awaited around 5.5). http://www.cfd-online.com/OpenFOAM_D...ges/1/7676.jpg I think this is linked to the computation of pressure, no ? When one plot the pressure respect to time, one see a kind of "slow" diffusion. So my question are the following : - Can one rely on the computation at the first time step (for both icoFoam and simpleFoam) ?
- Is the behavior shown here normal ?
- How to avoid the computation divergence (if possible) for simpleFoam.
Thank you again for your help and advices ! |

Hello everybody,
In fact, iHello everybody,
In fact, it seems that, according to results from F. Bos computing the drag coefficient for a circular cylinder that the big overestimate at the beginning with icoFoam is a normal behavior before convergence In the following, you will find different numerical experiments: - Time integration schemes: Euler, backward and Crank-Nicholson. Euler seems to give the better results.
- Grad schemes: one can't notice significant differences between Gauss linear and least squares.
- Time step: the results given are not really significant as for time step 0.001 (res. 0.005) one save is made each 10 (res. 2) times steps.
- Initialization: use of potentialFoam really smooth the solution for the first time steps.
http://www.cfd-online.com/OpenFOAM_D...ges/1/7682.png http://www.cfd-online.com/OpenFOAM_D...ges/1/7683.png http://www.cfd-online.com/OpenFOAM_D...ges/1/7684.png http://www.cfd-online.com/OpenFOAM_D...ges/1/7685.png So, I think that I will use icoFoam, let it run a certain time and take the final value - which is close to the one expected at first glance - for the drag coefficient. I remain interested by any comments and/or remarks. |

All times are GMT -4. The time now is 07:08. |