logic condenses out the mass associated with the constrained DOFs in the generation pass, and the
inertia relief calculations in the use pass of the substructure reflect the condensed mass distribution.)
The choice of master nodes during the generation pass will have a critical effect on how well the mass
is represented in the condensed substructure mass matrix. When you choose the Master Degrees of
Fr eedom nodes to represent a 'bounding box' of the model, the substructure’s inertia relief calculations
should closely represent that of the model. To verify your Master dof selections, check the reaction
forces (PRRSOL in /POST1) to ensure they are close to zero.
In the expansion pass, precalculation of masses for summary printout (IRLF,-1) occurs only on elements
that are part of the substructure.
2.2.4.3.1. Inertia Relief Output.
Use the IRLIST command to print the output from inertia relief calculations. This output consists of the
translational and rotational accelerations required to balance the applied loads and can be used by
other programs to perform kinematics studies. The summary listing of mass and moments of inertia
(produced during solution) is accurate, not approximate. The reaction forces at the constraints will be
zero because the calculated inertia forces balance the applied forces.
Inertia relief output is stored in the database rather than in the results file (Jobname.RST). When you
issue IRLIST, ANSYS pulls the information from the database, which contains the inertia relief output
from the most recent solution [SOLVE].
Command(s):IRLIST
GUI:No GUI equivalent.
2.2.4.3.2. Using a Macro to Perform Inertia Relief Calculations
If you need to do inertia relief calculations frequently, you can write a macro containing the above
commands. Macros are described in the ANSYS Parametric Design Language Guide.
2.2.5. Solve the Analysis
You are now ready to solve the analysis.
- Save a backup copy of the database to a named file. You can then retrieve your model by reentering
the ANSYS program and issuing RESUME.
Command(s):SAVE
GUI: Utility Menu> File> Save as - Start solution calculations.
Command(s):SOLVE
GUI: Main Menu> Solution> Solve> Current LS - If you want the analysis to include additional loading conditions (that is, multiple load steps), you
will need to repeat the process of applying loads, specifying load step options, saving, and solving
for each load step. (Other methods for handling multiple load steps are described in Loading in the
Basic Analysis Guide.) - Leave SOLUTION.
Command(s):FINISH
GUI:Close the Solution menu.
Release 15.0 - © SAS IP, Inc. All rights reserved. - Contains proprietary and confidential informationStructural Static Analysis