Below is an outline of the steps for solving a time-dependent problem that differ from the usual problem setup steps.
Determine which parameters in your problem are time-dependent. These can be material parameters (such as density) or boundary conditions.
In the Create a new task menu, specify a time-dependent problem, and define the geometry type, and so on, in the usual way.
Time-dependent problem(s) To set a time-dependent material parameter or a time-dependent boundary condition, the steps are slightly different:
For a time-dependent material parameter, follow these steps to define the parameter’s value as
: Go to the menu appropriate for setting the value of this parameter. For instance, if the parameter is density, select the Density menu item in the Material data menu.
Density Click the button at the top of the Ansys Polydata menu to enable the time-dependence inputs.
The button will change to to indicate that the time-dependence inputs are enabled.
Select the menu item appropriate for the time-dependent parameter. For density, this would be Modification of density.
Modification of density Enter
when Ansys Polydata prompts for the New
value. Click to accept this new value.
A menu will appear from which you will select the function
. The available functions are the same as those used
for evolution, and are described in Available Evolution Functions. If several parameters are time-dependent, a different function
can be chosen for each one. Select Upper level menu to complete the specification.
Click the button again to disable the inputs for time dependence.
The button will change to to indicate that the time-dependence inputs are disabled.
For a time-dependent boundary condition, follow these steps to define the parameter’s value as
: Select Flow boundary conditions or Thermal boundary conditions, as appropriate, from the sub-task menu.
Select the boundary condition you want to set, and click Modify.
Click the button at the top of the Ansys Polydata menu to enable the time-dependence inputs.
The button will change to to indicate that the time-dependence inputs are enabled.
Select the type of boundary condition you want to impose. For instance, for a flow boundary condition, you might choose Normal and tangential velocities imposed (vn, vs).
After you enter the value (
) of each numerical parameter
(such as 
) associated
with this boundary condition, clicking Upper level menu will cause a menu to appear, from which you can select the function 
. The available functions
are the same as those used for evolution, and are described in Available Evolution Functions. If several parameters are time-dependent, a different function
can be chosen for each one. Note that boundary conditions can be position-dependent and time-dependent. That is,
may be a constant, or a function of coordinates. Select Upper level menu to complete the specification.
Click the button again to disable the inputs for time dependence.
The button will change to to indicate that the time-dependence inputs are disabled.
Repeat this step for each time-dependent parameter.
Continue setting up the problem, following the usual procedures.
After all sub-tasks have been defined, select Numerical parameters from the F.E.M. Task Menu.
Numerical parameters In the Numerical parameters menu, select Modify the transient iterative parameters. This will bring up the Transient iterative parameters menu, which contains the following items:
Modify the initial time value
This allows you to modify the time at which the time-marching procedure starts. The initial time corresponds to
in Equation 29–2. The vector 
is initialized
to a default initial solution calculated by Ansys Polyflow (time-dependent
parameters will then be evaluated at 
), unless you choose to read an initial
solution from a file (that is, start from a results file, as described
in Starting an Ansys Polyflow Calculation from an Existing Results File). The default value of the initial time is
. Modify the upper time limit
This item allows you to specify the time at which the solution procedure stops.
Modify the initial value of the time-step
Use this item to set the initial time step
. The first solution
is calculated at 
. The initial value of the time step will be used
during the first three time steps; that is, 
and 
are equal to 
unless the simulation
does not converge, in which case the time step is usually divided
by 2. Thereafter, the time step size will be controlled automatically
by Ansys Polyflow according to Equation 29–9. Since accuracy cannot be checked for the first
three time steps, it is recommended that a small value of the initial
time step be used. The default value for the initial time step is
, and is, in general, a good choice, although this
parameter depends upon the time scale of the process; it may become
inappropriate for very fast or very slow processes. Modify the min value of the time-step
Ansys Polyflow will stop if the new value of
is less
than this allowed minimum value. Modify the max value of the time-step
This is the maximum time-step size that Ansys Polyflow will accept. The default value is 0.25. You will want to modify this value in certain cases:
when you want to solve a problem with a constant time step. It is sufficient to assign a unique value for both the minimum and the maximum time step, and to select a large value for the tolerance.
when you want result output files at more time intervals than you would get with the default time step. Set the maximum value for the time step to a smaller value than the default to achieve this.
for very slow processes when you do not need to get the results every quarter second.
Modify the tolerance
The tolerance,
, represents the maximum admissible relative
truncation error in the numerical solution 
with reference to the exact solution 
. The choice of
depends on the time-integration
method and can have a significant effect on computation cost and accuracy.
The automatic control of time step 
is directly
related to 
. Too small an 
can result in overly expensive
computation, although a high time-accuracy can be reached. On the
other hand, setting 
too large can cause one or more of the
following problems: significant departure from the assumptions used in the model derived from the theory of Theory
oscillatory behavior (in the case of the Crank-Nicolson and Galerkin methods)
divergence of nonlinear problems (due to the fact that Equation 29–8 will no longer be dominated by the mass matrix terms)
The default value of
is 0.01, which is usually the optimal value
for the Crank-Nicolson method and the implicit Euler method. For the
Galerkin method, a value between 0.001 and 0.01 is suggested. When solving a blow molding or thermoforming case with the shell model, the solver evaluates the actual volume of material at each time step. Although variation during one time step is bounded by the set tolerance, it may happen that, after a large number of steps, the overall variation of the volume of material exceeds the set tolerance. When this happens, it is recommended that you rerun the calculation with a more severe tolerance (for example, 0.001 or less).
Modify the max number of successful steps
This item allows you to set the maximum number of successful (that is, converged) steps. The computation will be stopped when this number is reached even if the upper time limit has not yet been reached. The default value is 200. Note that you can always restart the scheme from the results file in order to continue the time-marching scheme without losing the benefit of the previous solutions. See Starting an Ansys Polyflow Calculation from an Existing Results File for more information on these file types.
In the same menu, you can also specify the time-marching scheme using one of the following items:
Use of the implicit Euler method (the default scheme)
Use of the Galerkin method
Use of the Crank-Nicolson method
See Time-Marching Schemes for details of these methods.
In the same menu, you can also enable or disable the prediction of the velocity field:
Enable/Disable prediction of velocity field
In many processes, inertia terms are small compared to viscous forces; often they are even completely ignored. If this is the case, control of the accuracy for the time integration of the momentum equation will require very small time steps, which is usually not justified. It is therefore recommended to disable the accuracy check for the time integration of the momentum equation by selecting the Enable/Disable prediction of velocity field option. This is especially recommended for blow molding applications involving contact detection with extremely large variations of the velocity field at extremely short time scales. See Time Dependence and Contact Handling for details.