Use the Rigid Body Rotation tool   to specify the rotation of a rigid body (or bodies) in radians. This command rotates the selected rigid body(ies) around the x-axis, y-axis, or z-axis of the global coordinate system according to the rotation curve you enter.

Select the rigid body(ies) to be rotated, specify the axis of rotation, and define the times and magnitudes of the rotation curve in a table. For more complex rotations, break the rotation down into its x-, y-, and z-components and define separate rigid body rotation objects for rotation around each axis.

During the solution, the LS-DYNA solver applies a force to rotate the rigid body(ies) according to the rigid body rotation direction(s) and curve(s) you entered. It starts each rotation curve at the birth time and stops it at the death time.

Details of "Rigid Body Rotation"

Specify the input parameters for the Rigid Body Rotation tool:

Tabular Data for Rigid Body Rotation

Use this table to enter a rotation curve that specifies how the selected rigid body(ies) rotate. At each step in the curve, enter the time and magnitude of rotation.

Adding Time Steps to the Rigid Body Rotation Curve

You can manually enter a Time and Magnitude of rotation in the row marked with *. Alternatively, you can copy and paste pairs of time and magnitude values from a spreadsheet into that row.

The system adds these values to the table according to their Time value.

Graph of Rigid Body Rotation Curve

The Graph panel plots the rotation curve that you defined under Tabular Data. Click the check box next to Magnitude [rad] in the Tabular Data table to toggle the display of this curve.

Use the Rigid Body Angular Velocity tool   to set the angular velocity of the rigid body in radians per second . This command applies an angular velocity to the selected rigid body(ies) around the x-axis, y-axis, or z-axis of the global coordinate system according to the angular velocity curve you specify.

Select the rigid body(ies) to which an angular velocity is applied, specify the axis of rotation, and define the angular velocity curve (that is, the times and magnitudes of angular velocity) in a table. For more complex rotation patterns, break the angular velocity down into its x-, y-, and z-components and define separate rigid body angular velocity objects for the angular velocity around each axis.

During the solution, the LS-DYNA solver applies a force to the rigid body to rotate it according to the angular velocity direction(s) and curve(s) you entered. It starts to execute each angular velocity curve at the birth time and stops it at the death time.

Details of "Rigid Body Angular Velocity"

Specify the input parameters for the Rigid Body Angular Velocity tool:

Tabular Data for Rigid Body Angular Velocity

Use this table to enter the angular velocity curve, which specifies how the system applies angular velocities to the selected rigid body(ies). Enter the Time in seconds and the Magnitude of the angular velocity in radians per second. See Tabular Data for Rigid Body Rotation for more information.

Graph of Rigid Body Angular Velocity Curve

The Graph panel plots the angular velocity curve that you defined under Tabular Data. Click the check box next to Magnitude [rad/s] in the Tabular Data table to toggle the display of this curve.

Use the Rigid Body Force tool   to apply a force to a rigid body. This command applies a force in the x, y, or z direction to the center of mass of the selected rigid body(ies), according to the force curve you specify.

Select the rigid body(ies) to which a force is applied, specify the direction, and define the force curve (that is, the times and magnitudes at which force is applied) in a table. You can decompose a force vector into its x, y, and z components and define separate rigid body force objects for each component.

During the solution, the LS-DYNA solver applies a force to the rigid body according to the force direction(s) and curve(s) you entered. The solver starts to execute each force curve at the start time under Tabular Data and stops it at the end time.

Details of "Rigid Body Force"

Tabular Data for Rigid Body Force

Use this table to enter the force curve, which specifies how the system applies a force to the selected rigid body(ies). Enter the Time in seconds and the Magnitude of the force in Newtons. See Tabular Data for Rigid Body Rotation for more information.

Graph of Rigid Body Force Curve

The Graph panel plots the force curve that you defined under Tabular Data. Click the check box next to Magnitude [N] in the Tabular Data table to toggle the display of this curve.

Use the Rigid Body Moment tool   to apply a moment to a rigid body. This command applies a moment in the x, y, or z direction to the selected rigid body(ies), according to the moment curve you specify.

Select the rigid body(ies) to which a moment is applied, specify the direction, and define the moment curve (that is, the times and magnitudes at which a moment is applied) in a table. You can decompose a moment vector into its x, y, and z components and define separate rigid body moment objects for each component.

During the solution, the LS-DYNA solver applies a moment to the rigid body according to the direction(s) and curve(s) you entered. The solver starts to execute each moment curve at the start time under Tabular Data and stops it at the end time.

Details of "Rigid Body Moment"

Tabular Data for Rigid Body Moment

Use this table to enter the moment curve, which specifies how the system applies a moment to the selected rigid body(ies). Enter the Time in seconds and the Magnitude of the force in Newton-meters. See Tabular Data for Rigid Body Rotation for more information.

Graph of Rigid Body Moment Curve

The Graph panel plots the moment curve that you defined under Tabular Data. Click the check box next to Magnitude [N·m] in the Tabular Data table to toggle the display of this curve.

Use the Rigid Body Constraint tool   to constrain the motion of a rigid body. This tool allows you to specify the degrees of freedom for the selected rigid body(ies). You can constrain their movement in the x, y, or z direction and their rotation around the global x, y, or z axis.

Details of "Rigid Body Constraint"

Use the Master Rigid Body tool   to link two or more rigid bodies together. The rigid bodies must be connected by a mesh.

In the Mechanical workbench, the components of a larger body can be grouped together. When this group contains rigid bodies, the LS-DYNA solver merges the rigid bodies and computes a single solution for them. By using the Master Rigid Body tool, you can pick which rigid body in this group is assigned boundary conditions (the master rigid body). The solver applies any rigid body boundary conditions to the master rigid body you select. The master rigid body leads the movement of the rigid bodies that are connected to it by a mesh. The connected rigid bodies are constrained to move with the master rigid body.

Use the Merge Rigid Bodies tool to combine rigid bodies that are not connected by a mesh.

Details of "Master Rigid Body"

Select the master rigid body.

Use the Rigid Body Property tool   to set the following rigid body properties:

The Rigid Body Property tool allows you to set the mass, center of mass, and mass moment of inertia of a rigid body. When scoping a body to the geometry, the name of the Body is displayed, and the properties X,Y,Z coordinates, mass, and moments of inertia are filled accordingly from the values in the Geometry object. You can change the center of mass by scoping a geometric entity to the Location. When scoping multiple geometric entities, the equivalent center of mass is computed. The equivalent center of mass is the weighted mean of the center of gravity times the mass of all geometric entities. If you change the mass, the mass moments of inertia will be multiplied by the ratio between the new entered mass by the already scoped bodies mass.

Use the Explicit Rigid Bodies tool   to identify body(ies) that are treated as being rigid in an LS-DYNA Explicit analysis and flexible in other types of analyses.

Details of "Explicit Rigid Bodies"

Select the body(ies) that are treated as rigid during an Explicit analysis.

Use the Merge Rigid Bodies tool   to combine multiple rigid bodies together into a single rigid body. The rigid bodies do not have to be adjacent.

Ordinarily, the LS-DYNA solver considers each rigid body separately. By using the Merge Rigid Body tool, you can combine the selected rigid bodies into a single body. All rigid body boundary conditions are applied to the master rigid body. The slave rigid bodies are constrained to move with the master rigid body.

Details of "Merge Rigid Bodies"

Select the Master Rigid Body and at least one Slave Rigid Body.

Use the Rigid Body Additional Nodes tool   to create additional nodes in the mesh between adjacent rigid and flexile bodies. This adds rigid nodes to the flexible body, which creates a better connection and prevents deformation between the rigid and flexible bodies.

Details of "Rigid Body Additional Nodes"

Under Geometry, select the desired rigid body. Under Nodes, select the desired entities (non-body geometry scopings or nodes) to be added to the selected rigid body. The system adds nodes to the mesh for the selected entities.

To insert a box in an LS-DYNA analysis, right-click the system and select Insert > Box.

Two types of boxes exist: Standard and SPH. The Standard box is a stationary box. At this time, its function is to limit the SPH or SPG computation to particles that are within the box at the beginning of the simulation.

For the Standard box, the input parameters are:

The SPH box is a standard box that can move over time and is used only for SPH calculations. The SPH Box Motion Controls section in the Details panel allows you to specify the motion Type as a Displacement or Velocity. The direction of the box motion is defined by the Coordinate System and the Component. You can define time-dependent velocity or displacement for the box motion by entering tabular data.

You can define any number of Standard and SPH boxes in an analysis. In conjunction with the Use Box analysis setting, the following rules govern the solver's use of the boxes defined in the analysis.

When an Imported Displacement is added to an LS-DYNA analysis, the keyword written to the input file is determined by the Displacement Type field. The two keyword options are Boundary Prescribed Final Geometry and Initial Foam Reference Geometry.

When selecting the displacement for each component in the Data View worksheet, the Free option available for other types of analyses is not shown as it is not applicable when using these LS-DYNA keywords.

When the Displacement Type is set to Initial Foam Reference Geometry the Tabular Loading field is hidden. The rate at which the displacement is applied is determined by the solver in this case.

The Displacement Type Initial Foam Reference Geometry is only applicable to a subset of materials. Refer to the description of *Initial_Foam_Reference_Geometry in LS-DYNA Keyword User's Manual Volume I for a list of the supported material types.