Enforced acceleration (Abaqus)

In the Abaqus environment, you can use the Enforced Acceleration command to apply an acceleration to the selected degrees of freedom of the specified region's nodes. Enforced acceleration is widely used in analyses that involve time-dependent simulations.

The options in the Enforced Acceleration Constraint dialog box correspond to the Abaqus *BOUNDARY, TYPE=ACCELERATION keyword

Methods

You can apply an enforced acceleration using one of these methods:

• Magnitude and direction—Lets you input the magnitude of an acceleration and define its direction by specifying a vector.

• Normal—Lets you select element or geometry faces to define an enforced acceleration normal to that surface.

• Components—Lets you specify the acceleration on a set of nodes in the translational degrees of freedom (DOF1 to DOF3) and/or the rotational degrees of freedom (DOF4 to DOF6).

When you export or solve a solution that contains an enforced acceleration, the software writes out the *BOUNDARY, TYPE=ACCELERATION keyword in your Abaqus input file. If the type of the acceleration is set to either Magnitude and Direction or Normal, the software also uses a *TRANSFORM keyword to write out a local Cartesian coordinate system for the acceleration.

• For Magnitude and Direction type accelerations, the Z-axis of this coordinate system aligns with the vector that you specified to define the direction of the acceleration.

• For Normal type acceleration, the Z-axis of this coordinate system is normal to the selected entities on which you defined the acceleration, such as element faces.

For both Magnitude and Direction and Normal type accelerations, the software uses the *NSET keyword to group the nodes associated with each local coordinate system. The acceleration is then prescribed in the Z-direction (DOF3) in the magnitude you specified in the Enforced Acceleration Constraint dialog box.

Define an acceleration that varies with time

Use the Field option in the Enforced Acceleration Constraint dialog box to set a time-dependent acceleration constraint.

For example, for DOF3, specify the following values that vary over time in a table:

Row ID	time (sec)	acceleration (mm/sec^2) *
1	1	0
2	2	0.15
3	3.5	0.25
4	7	0.45

When you export or solve a solution that contains an enforced acceleration that varies over time, the software writes the *AMPLITUDE keyword to the Abaqus input file.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed part Abaqus as the specified solver Abaqus Structural analysis with the Visco, Implicit Dynamic, or Direct Cyclic step typeNote: Not available in linear perturbation analyses (Static Perturbation, Buckling Perturbation, Frequency Perturbation, Complex Eigenvalue Extraction, Transient Modal Dynamics, and Response Spectrum) or the General (Static) step
Command Finder	Enforced Acceleration
Simulation Navigator	In the appropriate step, right-click Constraint Container→New Constraint→Enforced Acceleration

How do I

Define enforced acceleration using magnitude and direction (Abaqus)

Define enforced acceleration using components (Abaqus)

Define normal enforced acceleration (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Enforced acceleration (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 } });