# Transient Flow Simulation Ahmed Body

 Register Blogs Members List Search Today's Posts Mark Forums Read

 July 1, 2021, 14:03 Transient Flow Simulation Ahmed Body #1 New Member   Join Date: Feb 2021 Posts: 7 Rep Power: 4 Hello, I'm trying to conduct a transient flow simulation using an Ahmed body on fluent. I expect the total time will be approximately 20 seconds and my velocity input 20m/s but i'm unsure how to determine the appropriate time step, number of iterations and max number of iterations per timestep. thanks for reading Last edited by FinlayEeles; July 1, 2021 at 17:07.

 July 2, 2021, 01:29 #2 Senior Member   Kira Join Date: Nov 2020 Location: Canada Posts: 436 Rep Power: 7 Hello, You should look into the Courant number/CFL condition to find the appropriate time step. Courant number is a dimensionless quantity and can be stated as follows: C = a * (Δt/Δx), where a is the velocity magnitude, Δt is the timestep and Δx is the length between mesh elements. It follows from the numerical diffusion coefficient that for any explicit simple linear convection problem, the Courant number must be equal or smaller than 1, otherwise, the numerical viscosity would be negative, i.e. C< or = 1. As for iterations per timestep, you should aim for this value to be 3-5 per timestep.

 July 2, 2021, 02:48 #3 Super Moderator     Alex Join Date: Jun 2012 Location: Germany Posts: 3,344 Rep Power: 45 So much for explicit schemes. For implicit ones without stability constraints, the time step size is dictated by the shortest events you want to capture. Or the ones that your simulation approach needs to resolve in order to work as designed, e.g. when doing LES. Let's say you are doing URANS simulations. An initial guess for the frequency of the largest vortices shedding at the bluff body comes from a Strouhal Number ~0.2. Divide that by 20-50, and you have a good initial guess for a time step size. The number of iterations per time step is is kind of tied to your time step size. Larger time step -> more inner iterations. For pure aerodynamic simulations, you should aim for around 5-10 inner iterations. If you can't get convergence within that window, it is usually better to decrease the time step size instead of increasing the number of inner iterations.

July 2, 2021, 07:06
#4
New Member

Join Date: Feb 2021
Posts: 7
Rep Power: 4
Quote:
 Originally Posted by aero_head Hello, You should look into the Courant number/CFL condition to find the appropriate time step. Courant number is a dimensionless quantity and can be stated as follows: C = a * (Δt/Δx), where a is the velocity magnitude, Δt is the timestep and Δx is the length between mesh elements. It follows from the numerical diffusion coefficient that for any explicit simple linear convection problem, the Courant number must be equal or smaller than 1, otherwise, the numerical viscosity would be negative, i.e. C< or = 1. As for iterations per timestep, you should aim for this value to be 3-5 per timestep.

My mesh has different mesh sizes depending on the part of the air box. Varying from fairly large to 10mm in the wakebox and 1mm around the legs. When calculating the courant number where would i obtain the length between mesh elements from as my mesh isnt uniform.

July 2, 2021, 07:10
#5
New Member

Join Date: Feb 2021
Posts: 7
Rep Power: 4
Quote:
 Originally Posted by flotus1 So much for explicit schemes. For implicit ones without stability constraints, the time step size is dictated by the shortest events you want to capture. Or the ones that your simulation approach needs to resolve in order to work as designed, e.g. when doing LES. Let's say you are doing URANS simulations. An initial guess for the frequency of the largest vortices shedding at the bluff body comes from a Strouhal Number ~0.2. Divide that by 20-50, and you have a good initial guess for a time step size. The number of iterations per time step is is kind of tied to your time step size. Larger time step -> more inner iterations. For pure aerodynamic simulations, you should aim for around 5-10 inner iterations. If you can't get convergence within that window, it is usually better to decrease the time step size instead of increasing the number of inner iterations.
What i'm attempting to do is witness stable asymmetric flow caused by the flow reattachment on the rear slant.
I think in order to do this i may have to have a period of time where there is a flow to the side of the body to force the wake structure to be asymmetric, then hopefully once i remove the pertubation the flow will stay in an asymmetric mode.
I know it's possible with the notchback body, i'm just struggling to witness anything other than perfectly symmetric wake structures.

 Tags transient 3d