General information about Results can be found in Review Results in the Mechanical User's Guide.
The following structural result types are available as results of an explicit dynamic analysis:
Structural Probes - Limited in Explicit Dynamics to: Deformation, Strain, Stress, Position, Velocity, Acceleration, Energy, Reaction Force, Reaction Moment, Joints. Limited in LS-DYNA to: Deformation, Stress, Velocity, Acceleration, Joint, Spring, Beam.
Once a solution is available you can display contour results or animate them to review the response of the structure through time.
Note: For an Explicit Dynamics analysis, there is no results interpolation between the results sets. Specifying a time in the GUI will display results for the closest results set.
The Scoping Method for Explicit Dynamics results cannot be set to Path or Surface for Particle bodies.
When post-processing any Force result in a 2d plane strain analysis, note that the result has units of force per length, even though the display shows a unit of force. The unit of length is always that of the solver unit (always mm for an Explicit Dynamics analysis), and not that of the Mechanical display unit. If the Mechanical display unit is changed, e.g. from metric to U.S. Customary, no conversion of the data with respect to the length unit will occur from mm to inches, and the result will remain in the solver unit of length (mm).
Eroded nodes can be toggled on or off in the graphics display.
Note: Reaction Forces and Moments Probes are computed by the Explicit Dynamics solver per boundary condition. The boundary condition itself will be assigned to the associated nodes of the scoped geometry or named selection. The boundary condition treatment depends on the behavior of the body:
If the boundary condition is applied to a flexible body: each node will record its own reaction force or moment, which is directly derived from the necessary impulse correction on the node.
If the boundary condition is applied to a rigid body: the impulse correction will be computed for the full rigid body. Subsequently the impulse (and thus force and moment reaction) will be distributed across the associated nodes in the scope of the boundary condition. Be aware that multibody rigid parts can be constrained by applying the boundary condition to one of the rigid bodies, but the reaction will be distributed across all nodes of this multibody part, which may yield results that are not immediately clear.
In case of overlapping boundary conditions the sum of reaction force and moment will be recorded on the node. In this case the actual exact contribution per boundary condition may be lost. For example: an edge with two boundary conditions like simply supported and fixed rotation will show reaction forces and moments for both boundary conditions, although the actual contribution to moment reaction comes from the fixed rotation and the actual contribution to reaction forces comes from the simply supported boundary condition.
Note: A remote displacement boundary condition is only indirectly associated with the scoped nodes. Since it is applied to the actual remote point location, which can not be selected as geometry, the scoped nodes just follow the imposed boundary condition. This means that the total reaction force and/or moment are computed on the internal node that is associated with the remote point location. Subsequently, the reaction force and moment will be distributed over the nodes in the scope of the remote point.
As a result, there are two ways to visualize the reaction probe: by selecting the boundary condition or by selecting the geometry of the associated scope. If there is no overlapping scope, the two methods will yield the same result. However, if there is overlap in scope, or the remote displacement is scoped to a rigid body with other boundary conditions or joints, the sum of reaction forces and probes will differ between location method boundary condition and geometry.
Probes can be used to display the variation in specific results over the saved time points in the analysis. The frequency at which data is available is defined in the Save Results On option of the analysis settings. This data should be specified prior to a solve.
Note: Probe results are not valid for Eulerian bodies.
You can use a Solution Information object to track, monitor, or diagnose problems that arise during a solution.
The display of shells may become distorted if they experience large deformations or rotations. A workaround for this is to disable Shell Thickness by toggling in the Style group of the Display tab. Or, set the Workbench variable UsePseudoShellDisp = 1 by selecting from the File tab. It may be necessary to toggle the deformation scaling from True Scale to Undeformed to True Scale again (see Scaling Menus for Deformed Shapes under the Result Context tab). Note that this option requires True Scaling to work properly.
Additional results specific to an Explicit Dynamics analysis are available via user defined results.
Mechanical supports the ability to review the results of a simulation that uses the LS-DYNA solver. Other information about results specific to the LS-DYNA analysis system can be found in Accessing Results in the LS-DYNA User's Guide. Additionally, results can be viewed with the LS-Prepost application that is included in the Ansys installation.