Enforced velocity (Abaqus)

Use the Enforced Velocity Constraint command to prescribe a velocity to the selected degrees of freedom of a specified region's nodes. Velocity is widely used in analyses that involve time-dependent simulations, such as General (quasi-static), Dynamic Implicit, Dynamic Explicit, and Dynamic Coupled Thermal-Stress steps.

The options in the Enforced Velocity Constraint dialog box correspond to the Abaqus *BOUNDARY, TYPE=VELOCITY keyword.

Methods

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

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

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

• Components — Lets you specify the velocity 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 velocity, the software writes the *BOUNDARY, TYPE=VELOCITY keyword to the Abaqus input file. If the type of the velocity 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 load.

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

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

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

Define a velocity that varies with time

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

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

Row ID	time ('sec)	**Velocity (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 velocity that varies over time, the software writes out the *AMPLITUDE keyword in your Abaqus input file.

Importing velocity data

Velocity data is always imported as component-type velocity. For example, the prescribed velocity of 2.5 mm/sec in a normal-type velocity constraint is imported as a component-type velocity where 2.5 mm/sec is assigned to DOF3 and applied to a group of 10 nodes. The local nodal coordinate systems (defined in the *Transform keyword) are also read and associated to the nodes.

Degree of freedom	Velocity (mm/sec)
DOF1
DOF2
DOF3	2.5
DOF4
DOF5
DOF6

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and the displayed partAbaqus as the specified solverAbaqus Structural analyses except linear perturbation analyses (Static Perturbation, Buckling Perturbation, Frequency Perturbation, Complex Eigenvalue Extraction, Transient Modal Dynamics, and Response Spectrum)
Command Finder	Enforced Velocity
Simulation Navigator	In the appropriate step, right-click Constraint Container→New Constraint→Enforced Velocity

How do I

Define enforced velocity using magnitude and direction (Abaqus)

Define enforced velocity using components (Abaqus)

Define normal enforced velocity (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Enforced velocity (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 } });