CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (https://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Question about unsteady flow past a cylinder (https://www.cfd-online.com/Forums/openfoam-solving/115472-question-about-unsteady-flow-past-cylinder.html)

rogerliu April 1, 2013 00:43
Question about unsteady flow past a cylinder
 
In this case, I want to simulate unsteady flow past a cylinder at Re=4000.
I have the following questions:
1) how to set ''unsteady'' in OpenFOAM;
2) for the turbulent model, which wall function I should choose? Depends on what?

Thanks!

immortality April 1, 2013 04:01
1) you should choose an unsteady incompressible solver like icoFoam.
2)it depends on the turbulent model.which one you choosed?copy the files from a like turbulent tutorial.

haakon April 1, 2013 05:01
  1. My personal opinion is that icoFoam is only for testing and educational purposes, even if you are only doing a laminar simulation (i.e. not use a turbulence model). The reason for this is that for example pisoFoam allows more control over the solution process, by allowing two different specifications for linear solvers for the different stages in the PISO-loop/non-northogonal corrections. I use this by specifying a non-zero relative tolerance for p (f.ex. relTol = 0.05), and then (of course) specify zero relative residual for pFinal (relTol = 0). So choose pisoFoam as solver and use a time integrator different than steadyState, and you are ready to go with an unsteady simulation.
  2. First I suggest that you consider whether you need a turbulence model or not at all. At Re = 4000 the boundary layer and separation point is still laminar, and turbulence is only found in the farfield wake region. That means that you have large regions of laminar flow, and a transition to turbulent flow in the wake. There are not many (if some at all) RANS models capable of capturing this behaviour. If you are desperat I suggest that you go for a LES simulation. However, if you have access to a decent workstation, or best, compute cluster, resolving all turbulence scales directly (aka. laminar simulations) might be the best solution. The computational demand for this should not be too big. One show-stopper is of course that the nature of this flow is 3D...


All times are GMT -4. The time now is 11:43.