Best practice for transient simulations?
 

Hi,

I'm going to be modelling a transient external aerodynamics flowfield. To start I made a mesh (in ICEM CFD) that I thought had reasonable element sizings and clusterings. But to make sure I do things correctly and accurately in CFX I have a few questions:

1. Initially, I shall run a steady-state simulation with this mesh as this will be needed as the initial conditions of the transient simulation. However, although the flowfield is transient (I do not know at this stage the frequency of the transient flowfield features) should I conduct a series of steady state simulations with ever increasing mesh resolutions to get a mesh independent result and thereby obtaining a mesh that I can be confident to return a good transient result?

2. Or should a mesh independent solution be obtained during the transient solution? However, I'm thinking that the mesh refinements could be depenedent upon the time. And in at this stage the mesh from the steady state solution would no be that important.

3. Once the mesh independence is assessed the time step indepenence must be conducted. Should this be conducted by refining the physical timestep or the transient timestep? I think it would be a long process if both had to be assessed.

I'd be interested in the process/sequence of these assessments that other people use to make sure that I get solution independent meshes and times for my transient simulations.

Thanks

Is the transient flow caused by vortex shedding? If so then you will not get steady state simulations to converge. In this case the only use for steady state simulations is to use upwinding advection (which puts so much damping into it that it should converge but be quite inaccurate) to get an initial condition for the transient simulation.

So Q1 - No, it cannot be done for the reason I explain above.
Q2 - Yes, this is what is required.
Q3 - Yes. As you will only be doing a transient simulation you only have the transient simulation to determine. But it will have some coupling to the mesh - as the mesh resolves smaller features you will need a smaller timestep to resolve these smaller features. So when you change the mesh, scale the timestep to keep the Courant number about the same.

Glenn, thanks for your comments.

Yes, vortex shedding is occuring in a couple of places because of the geometry of the object in the flowfield.

I'll now have to find out what an apporopriate Courant number is (<= 1?) for this case and change the timestep accordingly as the as element size decreases. However, in the Courant equation would I use for delta_X the minimum element spacing in the entire domain, which possibly would be the first element height on the wall boundaries?

No, you should establish what Courant number to use by a sensitivity analysis. You should be able to use a Courant number quite a bit higher than 1, but exactly how much higher you will have to determine. Then when you check other mesh sizes you can scale the timestep keeping the Courant number constant. Then it you want to be thorough you can check timestep size again as the best timestep size will probably have moved a bit.

Courant number is a variable available in the solver and post-processing. Use either the maximum Courant number or the RMS average Courant number.

Hi - a question about Courant number. When you say use either RMS or Maximum, what exactly do you mean? I'm running a sim at the moment, the RMS is 16, and the Max is 102. I read somewhere saying the Courant number should preferably not be in the 100s...does that mean Max or RMS?

The maximum Courant number allowable is problem dependent, so general figures are useless. You have to establish what Courant number your simulation likes to run at by a sensitivity analysis.