**** Entered By: rlange @ 12/16/2005 01:48 PM ****
Q. How can I do a CFD simulation that demonstrates vortex shedding?
A.
Vortex shedding is the continuance of a flow disturbance initiated by some instability in the system or surroundings. In a CFD simulation, the disturbance can be initiated in the computer simulation through numerical roundoff error, but more typically it must be introduced through the setup of the analysis.
One approach is to perform the analysis in two stages. Consider the classic geometry often used for illustrating vortex shedding, that of flow past a cylinder. The problem domain should extend a length of at least 10 characteristic diameters downstream, and up to 30 is reasonable, especially for the higher Reynolds number cases. The CFX outlet boundary condition of average static pressure is best for these simulations. During the first stage, the cylinder is rotated (i.e. it spins with a moving wall condition) and a solution obtained (this could be done in pseudo time, rather than real time). This becomes the initial condition for the vortex shedding analysis itself. Upon restart, the cylinder rotation is set to zero, and all other boundary conditions are maintained. It should then take a few cycles to get to "steady" behavior.
Next, how do we capture this phenomenon? A suitable time step as well as a suitable frequency at which to save results must be chosen. The dimensionless cylinder shedding frequency is known as the Strouhal number: St= fD/U, where f is the shedding frequency, D the characteristic diameter, and U is the velocity. From Frank White's Viscous Fluid Flow, Figure 18 (Figure 18 is an attachment to this solution: StvsRe.pdf), which relates the Strouhal number to the Reynolds number, we know that the Strouhal number for RE=150 is about 0.2, for example. Actually, this value of 0.2 is pretty accurate up to a Reynolds number of 100,000.
So fD/U = 0.2, and with, say, D~.2 ft and U=.006895 ft/sec, we
**** Entered By: rlange @ 12/16/2005 01:48 PM **** Q. How can I do a CFD simulation that demonstrates vortex shedding? A. Vortex shedding is the continuance of a flow disturbance initiated by some instability in the system or surroundings. In a CFD simulation, the disturbance can be initiated in the computer simulation through numerical roundoff error, but more typically it must be introduced through the setup of the analysis. One approach is to perform the analysis in two stages. Consider the classic geometry often used for illustrating vortex shedding, that of flow past a cylinder. The problem domain should extend a length of at least 10 characteristic diameters downstream, and up to 30 is reasonable, especially for the higher Reynolds number cases. The CFX outlet boundary condition of average static pressure is best for these simulations. During the first stage, the cylinder is rotated (i.e. it spins with a moving wall condition) and a solution obtained (this could be done in pseudo time, rather than real time). This becomes the initial condition for the vortex shedding analysis itself. Upon restart, the cylinder rotation is set to zero, and all other boundary conditions are maintained. It should then take a few cycles to get to "steady" behavior. Next, how do we capture this phenomenon? A suitable time step as well as a suitable frequency at which to save results must be chosen. The dimensionless cylinder shedding frequency is known as the Strouhal number: St= fD/U, where f is the shedding frequency, D the characteristic diameter, and U is the velocity. From Frank White's Viscous Fluid Flow, Figure 18 (Figure 18 is an attachment to this solution: StvsRe.pdf), which relates the Strouhal number to the Reynolds number, we know that the Strouhal number for RE=150 is about 0.2, for example. Actually, this value of 0.2 is pretty accurate up to a Reynolds number of 100,000. So fD/U = 0.2, and with, say, D~.2 ft and U=.006895 ft/sec, wesee that the vortex shedding frequency will be about 0.007 cycles/sec. So the period for one cycle is about 150 seconds. A time step of 6 seconds would yield 25 time steps per cycle. Better visualizations would be obtained with 60 time steps/cycle. The remaining modeling methods should introduce as little numerical diffusion as possible. So certainly, with lower Reynolds number, turbulence should be turned off. 

