3.2. Apply Loads and Obtain the Solution

To apply loads and obtain a solution, you need to enter the ANSYS solution processor. Issue the /SOLU command or pick Main Menu> Solution 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.

3.2.1. Loads

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 Main Menu> Solution> Loading Options> Specify Loads.) 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 (Main Menu> Solution> Loading Options> Curve Options) 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 TypeLabel
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 BodiesRBOX, 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 Main Menu> Solution> Loading Options> Show Forces in the GUI).

To visualize the applied load curve, use the EDPL command (or pick Main Menu> Solution> Loading Options> Plot Load Curve in the GUI).

For more detailed information on applying loads with the EDLOAD command, see General Loading Options.

3.2.2. Initial Velocities

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 Main Menu> Solution> Initial Velocity. For more information on how to apply initial velocities, see Initial Velocity.

3.2.3. Constraints

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 Main Menu> Solution> Constraints> Apply.)

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.

3.2.4. DOF Coupling

DOF coupling (CP command) and constraint equations (CE command) are also allowed in an explicit dynamic analysis. (In the GUI, pick Main Menu> Preprocessor> Coupling/Ceqn.) 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.

3.2.5. Data Smoothing

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 (Main Menu> Solution> Loading Options> Smooth Data). See Data Smoothing later in this document for more information on data smoothing.

3.2.6. Specify Explicit Dynamics Controls

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.

Table 3.2:  LS-DYNA Solution and Output Control Options

Option Command GUI Path
Termination Time TIME Main Menu> Solution> Time Controls> Solution Time
SHELL/BEAM Output EDINT Main Menu> Solution> Output Controls> Integ Pt Storage
Substep Output Controls EDRST Main Menu> Solution> Output Controls> File Output Freq
Output Interval (History File) EDHTIME Main Menu> Solution> Output Controls> File Output Freq
Energy Options EDENERGY Main Menu> Solution> Analysis Options> Energy Options

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.

3.2.7. Save Database and Solve

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 Utility Menu> File> Save as in the GUI). Next, start the solution calculations (SOLVE command or Main Menu> Solution> Solve in the GUI).

For more details on explicit dynamic solution controls and other solution features, see Solution Features later in this document.


Release 18.2 - © ANSYS, Inc. All rights reserved.