Mechanical APDL Structural Analysis Guide

For details on commands and menu paths

for defining these loads, see...

Load Type Category

Applying Inertia Loads in the Basic Analysis

Guide

Inertia

Loads

Gravity, Spinning, and so on

2.2.4.2.1. Applying Loads Using TABLE Type Array Parameters

You can also apply loads using TABLE type arra y parameters. For details on using tabular boundary
conditions, see Applying Loads Using TABLE Type Array Parameters in the Basic Analysis Guide.

In a structural analysis, valid primary variables are TIME, TEMP, and location (X,Y, Z).

When defining the table, TIME must be in ascending order in the table index (as in any table array).

You can define a table arra y parameter via command or interactively. For more information on defining
table arra y parameters, see the ANSYS Parametric Design Language Guide.

2.2.4.3. Calculating Inertia Relief

You can use a static analysis to perform inertia relief calculations, which calculate the accelerations that
will counterbalance the applied loads. You can think of inertia relief as an equivalent free-body analysis.

Your model should meet the following requirements:

• The model should not contain axisymmetric or generalized plane strain elements, or nonlinearities.
  Models with a mixture of 2-D and 3-D element types are not recommended.


• Symmetry models are not valid for inertia relief analysis.


• Data required for mass calculations (such as density) must be specified.


• Specify only the minimum number of displacement constraints - those required to prevent rigid-body
  motion. Three constraints (or fewer, depending on the element type) are necessary for 2-D models
  and six (or fewer) are necessary for 3-D models. Additional constraints, such as those required to
  impose symmetry conditions, are permitted, but check for zero reaction forces at all the constraints
  to make sure that the model is not overconstrained for inertia relief.


• The loads for which inertia relief calculations are desired should be applied.

Issue the IRLF command before the SOLVE command as part of the inertia load commands.

Command(s):IRLF,1
GUI: Main Menu> Solution> Load Step Opts> Other> Inertia Relief

Inertia Relief for Substructures

For substructures, inertia relief calculations (MATRIX50) use the equations described in Inertia Relief in
the Mechanical APDL Theory Reference. ANSYS obtains the mass matrix of a substructure via matrix re-
duction to condense it to the master nodes (MASTER). The inertia relief calculations in a substructure
are therefore consistent with the reduced mass contribution at the master nodes.

The IRLF command has no effect in the generation pass of a substructure. If you intend to perform in-
ertia relief calculations on a substructure, do not apply DOF constraints (D) on the substructure during
its generation pass; instead, apply them during the use pass. (Otherwise, the substructure reduction

Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential information

Performing a Static Analysis