Page 75 - Using ANSYS for Finite Element Analysis A Tutorial for Engineers

62 • Using ansys for finite element analysis
mode shapes are to be calculated, you would choose a modal analysis.
You can perform the following analysis types in the ANSYS program:
static (or steady-state), transient, harmonic, modal, spectrum, buckling,
and substructuring. Not all analysis types are valid for all disciplines.
Modal analysis, for example, is not valid for a thermal model. The analy-
sis guide manuals in the ANSYS documentation set describe the analysis
types available for each discipline and the procedures to do those anal-
yses. Analysis options allow you to customize the analysis type. Typical
analysis options are the method of solution, stress stiffening on or off,
and Newton–Raphson options. To define the analysis type and analy-
sis options, use the ANTYPE command (Main Menu > Preprocessor >
Loads > Analysis Type > New Analysis or Main Menu > Preprocessor >
Loads > Analysis Type > Restart) and the appropriate analysis option
commands (TRNOPT, HROPT, MODOPT, SSTIF, NROPT, etc.). For
GUI equivalents for the other commands, see their descriptions in the
ANSYS Elements Reference. If you are performing a static or full tran-
sient analysis, you can take advantage of the Solution Controls dialog
box to define many options for the analysis. For details about the Solution
Controls dialog box, see Solution. You can specify either a new analy-
sis or a restart, but a new analysis is the choice in most cases. A single
frame restart that allows you to resume a job at its end point or abort
point is available for static (steady-state), harmonic (2D magnetic only),
and transient analyses. A multi-frame restart that allows you to restart an
analysis at any point is available for static or full transient structural anal-
yses. See Restarting an Analysis for complete information on performing
restarts. The various analysis guides discuss additional details necessary
for restarts. You cannot change the analysis type and analysis options
after the first solution. A sample input listing for a structural transient
analysis is shown next. Remember that the discipline (structural, thermal,
magnetic, etc.) is implied by the element types used in the model.
ANTYPE, TRANS TRNOPT, FULL NLGEOM, ON
Once you have defined the analysis type and analysis options, the
next step is to apply loads.
Some structural analysis types require other items to be defined first,
such as master degrees of freedom and gap conditions. The ANSYS Struc-
tural Analysis Guide describes these items where necessary.

2.2.2.3 applying loads

The word loads as used in ANSYS documentation includes boundary con-
ditions (constraints, supports, or boundary field specifications), as well as