In this step, the SOLUTION processor defines the analysis type and analysis options, apply loads, specify load step options, and initiate the finite element solution. You can also apply loads via the PREP7 preprocessor.
Specify the analysis type based on the loading conditions and the response you wish to calculate. For example, if natural frequencies and mode shapes are to be calculated, you would choose a modal analysis. You can perform the following analysis types in the 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 analysis guides in the documentation set describe the analysis types available for each discipline and the procedures to do those analyses.
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 analysis options, issue the ANTYPE command ( or ) and the appropriate analysis option commands (TRNOPT, HROPT, MODOPT, NROPT, etc.). For GUI equivalents for the other commands, see the documentation for the given command in the Command Reference.
If you are performing a static or full transient 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 analysis or a restart, but a new analysis is the norm in most cases. A multiframe restart that enables you to restart an analysis at any point is available for static and transient (full or mode-superposition method) analyses. For more information, see Restarting an Analysis. The various analysis guides provide more specific information about restart requirements. You cannot change the analysis type and analysis options after the first solution.
An example input listing for a structural transient analysis is shown below. Remember that the discipline (structural, thermal, magnetic, etc.) is implied by the element types used in the model.
ANTYPE,TRANS TRNOPT,FULL NLGEOM,ON
After 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 Structural Analysis Guide describes these items where necessary.
The word loads as used in the documentation includes boundary conditions (constraints, supports, or boundary field specifications) as well as other externally and internally applied loads. Loads are divided into these categories:
DOF Constraints
Forces
Surface Loads
Body Loads
Inertia Loads
Coupled-field Loads
You can apply most of these loads either on the solid model (keypoints, lines, and areas) or the finite element model (nodes and elements). For details about the load categories and how they can be applied on your model, see Loading in this manual.
Two important load-related terms you need to know are load step and substep. A load step is simply a configuration of loads for which you obtain a solution. In a structural analysis, for example, you may apply wind loads in one load step and gravity in a second load step. Load steps are also useful in dividing a transient load history curve into several segments.
Substeps are incremental steps taken within a load step. You use them primarily for accuracy and convergence purposes in transient and nonlinear analyses. Substeps are also known as time steps - steps taken over a period of time.
Note: The program uses the concept of time in transient analyses as well as static (or steady-state) analyses. In a transient analysis, time represents actual time, in seconds, minutes, or hours. In a static or steady-state analysis, time simply acts as a counter to identify load steps and substeps.
Load step options are options that you can change from load step to load step, such as number of substeps, time at the end of a load step, and output controls. Depending on the type of analysis you are doing, load step options may or may not be required. The analysis procedures in the analysis guide manuals describe the appropriate load step options as necessary. See Loading for a general description of load step options.
Issue the SOLVE command to initiate solution calculations. When you issue the command, the program takes model and loading information from the database and calculates the results.
The program writes the results to the results file (Jobname.rst, Jobname.rth, or Jobname.rmg) and also to the database. The only difference is that only one set of results can reside in the database at one time, while you can write all sets of results (for all substeps) to the results file.
You can conveniently solve multiple load steps (LSSOLVE). Solution discusses this and other solution-related topics.