8.7非线性瞬态分析步骤帮助学习

Many of the tasks that you need to perform in a nonlinear transient analysis are the same as (or similar to) those that you perform in nonlinear static analyses (described in Performing a Nonlinear Static Analysis) and linear full transient dynamic analyses (described in Structural Static Analysis). However, this section describes some additional considerations for performing a nonlinear transient analysis. Remember that the Solution Controls dialog box, which is the method described in Performing a Nonlinear Static Analysis, cannot be used to set solution controls for a thermal analysis. Instead, you must use the standard set of ANSYS solution commands and the standard corresponding menu paths.

8.7.1. Build the Model

This step is the same as for a nonlinear static analysis. However, if your analysis includes time-integration effects, be sure to include a value for mass density [MP,DENS]. If you want to, you can also define material-dependent structural damping [MP,DAMP].

8.7.2. Apply Loads and Obtain the Solution

1. Specify transient analysis type and define analysis options as you would for a nonlinear static analysis:

 New Analysis or Restart [ANTYPE]  Analysis Type: Transient [ANTYPE]  Large Deformation Effects [NLGEOM]  Large Displacement Transient (if using the Solution Controls

dialog box to set analysis type)

2. Apply loads and specify load step options in the same manner as you would for a linear full transient dynamic analysis. A transient load history usually requires multiple load steps, with the first load step typically used to establish initial conditions (see the Basic Analysis Guide). The general, nonlinear, birth and death, and output control options available for a nonlinear static analysis are also available for a nonlinear transient analysis. In a nonlinear transient analysis, time must be greater than zero. See Transient Dynamic Analysis for procedures for defining nonzero initial conditions.

For a nonlinear transient analysis, you must specify whether you want stepped or ramped loads [KBC]. See the Basic Analysis Guide for further discussion about ramped vs. stepped loads.

You can also specify dynamics options: alpha and beta damping, time integration effects, and transient integration parameters.

ALPHAD,

, Command(s): BETAD

TIMINT, TINTP

Main Menu> Solution> Analysis Type> Sol'n Control ( : Transient Tab)

Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Damping

Main Menu> Solution> Unabridged Menu> Load Step Opts> Time/Frequenc> Time Integration

GUI:

An explanation of the dynamics options follows.



Damping

Rayleigh damping constants are defined using the constant mass [ALPHAD] and stiffness [BETAD] matrix multipliers. In a nonlinear analysis the stiffness may change drastically - do not use BETAD, except with care. See Damping for details about damping.



Time Integration Effects [TIMINT]

Time integration effects are ON by default in a transient analysis. For creep, viscoelasticity, viscoplasticity, or swelling, you should turn the time integration effects off (that is, use a static analysis). These time-dependent effects are usually not included in dynamic analyses because the transient dynamic time step sizes are often too short for any significant amount of long-term deformation to occur. Except in kinematic (rigid-body motion) analyses, you will rarely need to adjust the transient integration parameters [TINTP], which provide numerical damping to the Newmark and HHT methods. (See your Theory Reference for the Mechanical APDL and Mechanical Applications for more information about these parameters.)

ANSYS' automatic solution control sets the defaults to a new time integration scheme for use by first order transient equations. This is typically used for unsteady state thermal problems where θ = 1.0 (set by SOLCONTROL, ON); this is the backward Euler scheme. It is unconditionally stable and more robust for highly nonlinear thermal problems such as phase changes. The oscillation limit tolerance defaults to 0.0, so that the response first order eigenvalues can be used to more precisely determine a new time step value.

Note: If you are using the Solution Controls dialog box to set

solution controls, you can access all of these options [ALPHAD, BETAD, KBC, TIMINT, TINTP, TRNOPT] on the Transient tab. 3. Write load data for each load step to a load step file.

Command(s):

LSWRITE GUI:

Main Menu> Solution> Load Step Opts> Write LS File

4. Save a backup copy of the database to a named file.

Command(s):

SAVE GUI:

Utility Menu> File> Save As

5. Start solution calculations. Other methods for multiple load steps are described in \"Getting Started with ANSYS\" in the Basic Analysis Guide.

Command(s):

LSSOLVE GUI:

Main Menu> Solution> Solve> From LS Files

6. After you have solved all load steps, leave SOLUTION.

Command(s):

FINISH GUI:

Close the Solution menu.

8.7.3. Review the Results

As in a nonlinear static analysis, you can use POST1 to postprocess results at a specific moment in time. Procedures are much the same as described previously for nonlinear static analyses. Again, you should verify that your solution has converged before you attempt to postprocess the results. Time-history postprocessing using POST26 is essentially the same for nonlinear as for linear transient analyses. See the postprocessing procedures outlined in Transient Dynamic Analysis.

More details of postprocessing procedures can be found in the Basic Analysis Guide.