It is sometimes necessary to initialize a transient 2-way FSI
case using a previous steady-state 2-way FSI solution. In general this
is necessary when the initial (steady state) fluid field which acts as
the starting point for the transient simulation produces deformations in
the structure, or when a pre-loaded structure produces deformation that
should be accounted for in the fluid field. Pipes which operate at
high pressures are a common case when this type of initialization may be
necessary. Without appropriate initialization the pipe expansion that
would otherwise occur in the first timestep can induce large pressure
changes in the fluid, causing the solver to fail.
In structural
simulations a common approach is to solve a steady-state step, which is
actually a Transient Dynamic simulation with Time Integration turned off
(TIMINT,OFF), followed by a transient step (TIMINT,ON) all in one
simulation. In other words there are multiple SOLVE commands in one
input file. Note that this is not a valid approach for FSI simulations.
The general solution procedure is as follows:
1. Solve a fluids-only steady-state analysis to use as the initial guess for the steady-state FSI analysis.
However, you can often skip this step, especially when the expected deformations are small.
2. Solve a steady-state 2-way FSI simulation.
On
the structural side this should be defined as a Flexible Dynamic
simulation with Time Integration effects turned off. On the CFX side
define this as a steady-state simulation, using the initial guess from
step 1 if necessary. Steady-state FSI simulations should be solved
using a single Coupling Step, but with enough stagger loops to fully
converge the solution. The number of coupling steps is controlled by
the `Coupling Time Duration` and `Coupling Time Steps` settings in
CFX-Pre (corresponding to MFTI and MFDT). Set both of these values to 1
[s] (this value is arbitrary). The `Coupling Initial Time` should be
Automatic, do not specify a value. On the CFX side the `Maximum Number
of Iterations` now refers to the number of iterations per stagger, so a
sensible value might be 5. The CFX timestep is used only by CFX and has
its normal meaning. Now set the Maximum, Minimum and Target Stagger
Loops. A maximum of 100, a minimum of 20 and a target of 100 are
reasonable values. The target value will not be used. The solution
will now proceed for one coupling step with at least 20 stagger loops
and 5 CFX iterations per stagger (so at least 100 CFX iterations total).
If the convergence criteria has been met the solution will stop here,
otherwise it will continue until a maximum of 100 stagger loops.
If
structural loads are applied in Simulation, other than those loads
transferred through the FSI interfaces, they should be specified such
that they are constant for the first 1 [s] of the simulation
(corresponding to the steady-state part of the simulation) and then vary
as necessary during the transient part of the simulation, which will
begin after 1 [s]. Hence transient structural loads should be specified
at this stage of the procedure and should be offset in time to account
for the time covered by the steady state simulation. If the structural
loads are ramped during the steady-state part of the simulation, they
should reach their final value well before the end of the steady-state
simulation to allow time for the fluid field to respond and reach a
steady solution.
Check that you have obtained a converged steady-state solution before proceeding.
3.
Set up the CFX side as a transient FSI simulation `as normal`. Note
that the transient simulation will now start from 1 [s] instead of 0
[s]. This is because ANSYS controls the transient timestep, and ANSYS
sees the true transient simulation as a restart from an earlier
transient solution that finished after 1 [s]. Any time-dependent
quantities in CFX should account for this.
4. Generate the .mf file.
To
do this, define a run in the CFX Solver Manager. Pick the transient
CFX def file from step 3. On the Multifield tab pick the `MFX Run Mode`
as `Process Input File only`. Pick the `ANSYS Input File` as the input
file used in step 2. Enable `Restart ANSYS Run` and pick the `Previous
Run DB` as the db file written out when step 2 completed (it will be in
the <name>_001.ansys directory). Click Start Run and you should
get a new run directory containing a short .mf file.
5. Manually edit the .mf file.
Insert the command TIMINT,ON so that ANSYS will now solve a true transient.
Insert
the command DELTIM,<VAL>,0,0 where <VAL> is the `Coupling
Time Steps` value set in CFX-Pre for the transient simulation. Setting
a DELTIM value less than the Coupling Time Steps value will cause
sub-cycling in the ANSYS solver. This is generally not necessary since
the "Coupling Time Steps" value is usually limited by the fluid
timescale and is therefore small enough to avoid the need for
sub-cycling in ANSYS. There are some cases where this is not true.
6. Define the transient 2-way FSI run.
Pick
the transient CFX def file from step 3 and the steady-state CFX res
file from step 2. On the Multifield tab pick the `MFX Run Mode` as
`Start ANSYS and CFX`. Pick the`ANSYS Input File` as the .mf file you
just edited. Disable `Process ANSYS Input File`. Enable `Restart ANSYS
Run` and pick the `Previous Run DB` as the db file written out when 2
completed (it will be in the <name>_001.ansys directory). Start
the run.
Source: http://www.eureka.im/4057.html
