- Mode
- Displacement
Node-based displacements from a static analysis are used to initialize the Explicit node positions. These displacements are converted to constant node-based velocities and applied for a pre-defined time in order to obtain the required displaced coordinates. During this times, element stresses and strains are calculated as normal by the Explicit solver. Once the displaced node positions are achieved, all node-based velocities are set to 0 and the solution is completely initialized. This option is applicable to unstructured solids (hexahedral and tetrahedral), shells, and beams.
- Time Step Factor
The initial time step from the explicit solution is multiplied by the time step factor. The resulting time is used with the nodal displacements from the Ansys Mechanical analysis to calculate constant nodal velocities. These nodal velocities are applied to theExplicit model over the resulting time in order to initialize the Explicit nodes to the correct positions.
- Material State
Node-based displacements, element stresses and strains, and plastic strains and velocities from an Implicit solution are used to initialize an Explicit analysis at cycle 0. This option is applicable to results from a linear static structural, nonlinear static structural, or transient dynamic Mechanical system. The Ansys solution may be preceded with a steady-state thermal solution in order to introduce temperature differences into the solution. In this case, the accompanying thermal stresses due to the thermal expansion coefficient will be transferred but may dissipate since the thermal expansion coefficient is not considered in an Explicit analysis. This option is only applicable to unstructured solid elements (hexahedral and tetrahedral).
- Pressure Initialization
- From Deformed State
The pressure for an element is calculated from its compression, which is determined by the initial displacement of the element's nodes. This is the default option and should be used for almost all Implicit-Explicit analyses.
- From Stress State
The pressure for an element is calculated from the direct stresses imported from the implicit solution. This option is only available for materials with a linear equation of state. If the pressure for an element is already initialized, this calculation will be ignored. This is for a pre-stress analysis from an Implicit solution that has been initialized from an INISTATE command and has an .rst file with all degrees of freedom fixed.
- Time
The time at which results are extracted from the Implicit analysis.