To apply loads and obtain a solution, you need to enter the ANSYS solution processor. Issue the /SOLU command or pick in the GUI.
From the solution processor, you can apply loads, initial velocities, constraints, and DOF coupling to the model. The following sections describe this process.
In an explicit dynamic analysis, all loads must be specified over time using component logic or part IDs, array parameters, and the EDLOAD command. (In the GUI, load options are found under .) Basic input for this command is a component name or part number and two array parameter names or a load curve ID number (LCID). The component specified must contain the nodes or elements on which the load is being applied. The array parameters specified must contain time varying load data (one array for time values and one array for the corresponding load values; the two arrays must be the same length). As an alternative to inputting the array parameters on the EDLOAD command, you can define the load curve using the EDCURVE command () and input the load curve ID on EDLOAD. Valid loads are shown in the table below.
Table 3.1: Loads Applicable in an Explicit Dynamics Analysis
| Load Type | Label |
|---|---|
| Displacements | UX, UY, UZ |
| Rotations | ROTX, ROTY, ROTZ |
| Forces | FX, FY, FZ |
| Moments | MX, MY, MZ |
| Velocities | VX, VY, VZ |
| Accelerations (on nodes) | AX, AY, AZ |
| Base Accelerations | ACLX, ACLY, ACLZ |
| Angular Velocities | OMGX, OMGY, OMGZ |
| Temperature | TEMP |
| Pressures (applied to elements) | PRESS |
| Displacements on Rigid Bodies | RBUX, RBUY, RBUZ |
| Rotations on Rigid Bodies | RBRX, RBRY, RBRZ |
| Velocities on Rigid Bodies | RBVX, RBVY, RBVZ |
| Forces on Rigid Bodies | RBFX, RBFY, RBFZ |
| Moments on Rigid Bodies | RBMX, RBMY, RBMZ |
| Angular Velocities on Rigid Bodies | RBOX, RBOY, RBOZ |
Note: We recommend that you specify velocity time histories instead of displacement time histories. A piecewise linear displacement time history may lead to discontinuous velocities and infinite accelerations.
The load symbol will appear automatically on the active graphics window. The load symbol is erased automatically when you replot. To turn the display of this symbol on or off, issue EDFPLOT (or pick in the GUI).
To visualize the applied load curve, use the EDPL command (or pick in the GUI).
For more detailed information on applying loads with the EDLOAD command, see General Loading Options.
In the ANSYS LS-DYNA program, initial velocities are defined using the EDVEL and EDPVEL commands. You can use these commands to apply both translational and rotational velocities to various entities. Use EDVEL to apply velocities to a nodal component or to a single node; use EDPVEL to apply velocities to a part or part assembly.
The EDVEL and EDPVEL commands provide two
methods for specifying rotational velocities, Option =
VGEN and Option = VELO. The VGEN method applies a rigid
body rotation to the specified entity around a specified axis. The VELO method
applies the rotational velocities directly to each node's rotation degree of
freedom. Since only shell and beam elements have rotation degrees of freedom, the
rotations input with the VELO method are only applicable to
SHELL163 and BEAM161
elements.
You can access all the initial velocity options in the GUI by picking . For more information on how to apply initial velocities, see Initial Velocity.
In addition to loads and initial velocities, constraints can also be applied to the model. Using the D command, you can apply constraints only to the displacement (UX, UY, UZ) and rotation (ROTX, ROTY, ROTZ) degrees of freedom; the constraint value must be zero. (In the GUI, pick .)
Other specialized types of constraints are also available in an explicit dynamic analysis (such as symmetry boundary planes and welded constraints). See Constraints and Welds for more information.
DOF coupling (CP command) and constraint equations (CE command) are also allowed in an explicit dynamic analysis. (In the GUI, pick .) Coupling is allowed only for the UX, UY, and UZ degrees of freedom. Constraint equations are allowed only for the UX, UY, UZ, and ROTX, ROTY, ROTZ degrees of freedom. For more information, see Coupling and Constraint Equations.
If you're working with noisy data (such as an earthquake excitation), you may want to "smooth" that data to a set of data that provides an accurate approximation of the data points.
To smooth data, you must first create four arrays. The first two arrays should contain the noisy data from the independent and the dependent variables. The second two arrays will be used to store the smoothed data. After these arrays are created, you then smooth the data using the EDNDTSD command (). See Data Smoothing later in this document for more information on data smoothing.
Table 3.2: LS-DYNA Solution and Output Control Options shows some basic LS-DYNA solution and output controls that you should specify for an explicit dynamic analysis.
The above table does not show all controls available in an explicit dynamic analysis. However, most of the default settings for the LS-DYNA control options (output controls, file controls, damping options, etc.) are sufficient for most explicit dynamic analyses and need not be modified.
A brief description of those options that are recommended follows:
Termination Time [TIME]
This option specifies time at the end of the analysis.
Substep Output Controls [EDRST]
This option specifies the number of results written to the Jobname.RST file. Because explicit dynamics analyses are only solved over very small time increments (i.e., 1e-7 seconds), only a relatively small number of solutions should be written to the Jobname.RST file.
Output Interval [EDHTIME]
This option specifies the number of output steps for the history file (Jobname.HIS). The history file results are typically saved for a small subset of nodes or elements [EDHIST], but at a much higher frequency than the results file (Jobname.RST) results.
After you have specified all loading and solution and output controls, save a backup copy of the database to a named file (SAVE command or in the GUI). Next, start the solution calculations (SOLVE command or in the GUI).
For more details on explicit dynamic solution controls and other solution features, see Solution Features later in this document.