Steady State as Initial Conditions for Navier Stokes+Heat Eq

[selim]

Hallo,

I want to use the steady state as the initial condition for the transient calculations.
I am using compressible Navier Stokes+Heat Equation (with Elmer Front)

I could not find any tutorial and also in the documentation.

Your help will be appreciated.
Thanks a lot,
Selim

[Takala]

Hi,

here is a quote from the old list, I hope it helps you:

Hi Eelis,

Eelis Takala wrote:
> Hi,
>
> is it possible to first calculate a steady state analysis and then calculate a transient analysis by using the steady state as initial value. For example to bend a beam in steady state mode using some force conditions and then release it in transient mode.
>
>
Sure. Just restart from steady state and the solution will be taken as
the initial condition for any further run (may it be transient or
againsteady state).
Just use the keywords

Restart File = "your_previosly_obtained.result"
Restart Position = 1 ! may be a higher number, if more Steady State
iterations have been run, else take 0 to read in latest


Best,

Thomas

[raback]

Another possibility is to use really large time-steps at the beginning which effectively make the equation steady-state. This makes it possible to have the initalization within the same simulation. However, often there is no steady-state solution and solving with long time-steps will not result into convergence. The remedy for this is to make, for example, viscosity dependent on the timestep size. This could be done by the following defenitions:

In Simulation section add some long timesteps in the start

Timestep Sizes(2) = 1000 0.01
Timestep Intervals(2) = 2 1000

and in Material section make the viscosity linearly dependent on the timestep size

Viscosity = Variable "timestep size"
Real MATC "1.23e-2*tx"

So here at timestep size 0.01 the viscosity would be 1.23e-4 etc.

BR, Peter

[cadmonkey]

G'day, I'm new to Elmer and trying to figure this out.

I tried what raback mentioned, with a long initial time step, seems to work, however its only outputting the initial "big guess" time-steps and not the refined time-steps. This is what the "simulation" part of my file looks like, it runs the first 20 seconds in 1 second intervals to get an initial flow field, then refines to 0.08 second steps (I'm trying to simulate von Karman vortex streets off the back of a bluff body):

Simulation
Max Output Level = 4
Coordinate System = Cartesian
Coordinate Mapping(3) = 1 2 3
Simulation Type = Transient
Steady State Max Iterations = 1
Output Intervals = 1
Timestepping Method = BDF
BDF Order = 2
Timestep intervals(2) = 20 1600
Timestep Sizes(2) = 1 0.08
Solver Input File = case.sif
Post File = case.ep
End

How can I get it to save all timesteps and not just the first ones?

[Juha]

Hi,

The "Output Intervals" keyword is also an array when "Timestep Intervals" in an array,
e.g. try
Output Intervals(2) = 1 1

BR, Juha

[cadmonkey]

That worked, cheers!

What do you guys use to mesh for transient cases like von Karman streets where you want a high level of refinement around vorticity but not elsewhere? Previously I was using Gerris which could easily adapt its mesh according to local vorticity at each timestep.