Dynamic explicit analysis (Abaqus)

You can perform both Dynamic Explicit and Axisymmetric Dynamic Explicit analyses.

A Dynamic Explicit analysis analyzes large models with relatively short dynamic response times and extremely discontinuous events or processes. A Dynamic Explicit analysis allows for the definition of very general contact conditions. It uses a consistent, large-deformation theory (models can undergo large rotations and large deformation) and can use a geometrically linear deformation theory (strains and rotations are assumed to be small).

The options on the Dynamic Explicit Analysis tab correspond to the parameters for the Abaqus *DYNAMIC, EXPLICIT keyword.

Supported elements

For a list of supported elements, see Abaqus elements.

Boundary conditions

For boundary conditions that are applied during an explicit dynamic response step, use a field to define a time-dependent boundary constraint.

If you specify boundary conditions for an explicit dynamic response step without a field, the software applies the boundary conditions instantaneously at the beginning of the step. Because a dynamic explicit analysis does not allow jumps in displacement, the software ignores the value of a nonzero displacement boundary condition that you specify without a field, and enforces a zero velocity boundary condition.

Supported boundary constraints

Loads

You can apply concentrated nodal forces or moments to the displacement or rotation degrees of freedom (DOF1 through 6), as well as distributed pressure forces or body forces. As with boundary conditions used in an explicit dynamic response step, loads you apply during a dynamic response step should use a field to define a time-dependent load. If you specify loads for the explicit dynamic response step without a field, the software applies the loads instantaneously at the beginning of the step.

Supported loads

Mass scaling

You can define mass scaling for Abaqus Dynamic Explicit analyses using the Mass Scaling modeling object. Mass scaling is often used in for computational efficiency in quasi-static analyses and in dynamic analyses that contain a few very small elements that control the stable time increment.

You can define a mass scaling factor as fixed or variable.

Fixed mass Scaling

Fixed mass scaling is performed once at the beginning of the step for which it is specified. You can either define a mass scaling factor directly, or you can define a desired minimum stable time increment for which the solver determines the mass scaling factors.

Fixed mass scaling provides a simple way to modify the mass properties of a quasi-static model at the beginning of an analysis or to modify the masses of a few small elements in a dynamic model so they do not control the stable time increment size. Because the software performs the scaling operation only once at the beginning of the step for which the mass scaling is defined, fixed mass scaling is computationally efficient.

Variable mass scaling

For variable mass scaling, you define a minimum stable time increment. The solver automatically calculates and applies the mass scaling factors throughout the step. If you specify both variable and fixed mass scaling in a step, the software uses the fixed mass scaling to scale the original mass of the elements once at beginning of the step. It then uses the variable mass scaling to further scale the elements at the beginning and periodically during the step.

Corresponds to the Abaqus *VARIABLE MASS SCALING and *FIXED MASS SCALING keywords.

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file as the work and displayed partAbaqus as the specified solverDynamic Explicit as the specified analysis typeDynamic Explicit Analysis as the specified solution type

Learn more

Nonlinear analyses (Abaqus)

Axisymmetric analysis (Abaqus)

Modal steady-state dynamic analysis (Abaqus)

Modeling cohesive behavior in Abaqus contact analyses

Modeling abstractions (Abaqus)

User-defined progressive failure analysis (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Dynamic explicit analysis (Abaqus), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });