Initial conditions (Abaqus)

Use the Initial Conditions command in an Abaqus solution to define:

• Initial velocities for specified degrees of freedom.When initial velocities are given for dynamic analysis, they should be consistent with all of the constraints on the model, especially time-dependent boundary conditions. Abaqus ensures that they are consistent with boundary conditions and with multi-point and equation constraints but does not check for consistency with internal constraints, such as incompressibility of the material. If a conflict exists, boundary conditions take precedence over the initial conditions.

• Initial temperatures for multiple regions. You can set initial temperature conditions for multiple regions in the model. Setting initial condition temperature is available at the solution level.

The options in the Initial Conditions dialog box correspond to the Abaqus *INITIAL CONDITIONS, TYPE=VELOCITY and *INITIAL CONDITIONS, TYPE=TEMPERATURE keywords.

Methods for setting transient initial conditions

You can apply a velocity initial condition using one of these methods:

• Velocity - Magnitude and direction — Lets you input the magnitude of an initial velocity (translational) and specify its direction by creating a vector. The software creates a nodal Cartesian coordinate system where the velocity vector points towards the local Z-direction. Because Abaqus requires that initial velocities be defined with respect to the global coordinate system, when you export or solve a solution, the software writes out the velocity components in the global (Cartesian) coordinate system (that is, the velocity vector is decomposed into X, Y, and Z components). In addition, for reference only, the software writes the local Cartesian coordinate system for the load using a *TRANSFORM keyword.

• Velocity - Normal — Lets you select element or geometry faces to define an initial velocity normal to that surface. The software creates a nodal coordinate system where the Z-direction indicates the direction of the velocity. It writes each individual local nodal coordinate system using the *TRANSFORM keyword. The software exports the nodal velocity in the global coordinate system.

• Velocity - Components — Lets you specify the initial 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).

You can apply this type of constraint	To this geometry or FEM entity
Velocity - Magnitude and direction****Velocity - Component	curvepointmesh pointpolygon facepolygon edgenode
Velocity - Normal	curvepointmesh pointpolygon facepolygon edgeelement

Graphical symbol

In the graphics window, a symbol represents a transient initial condition. It also denotes the displacement and velocity conditions for each axis.

Displacement and velocity conditions at all six degrees of freedom

In the symbol	Indicates
At the tip
A circle	An initial displacement along that axis.
A cone	An initial velocity along that axis.
In the middle of the symbol
Two circles	An initial displacement about that axis.
Two cones	An initial velocity about that axis.

The length of each axis in the symbol is scaled relative to the maximum value along or about that axis.

Where do I find it?

Application	Pre/Post
Prerequisites	A Simulation file as the work part and the displayed partAbaqus as the specified solver For a transient initial condition, Abaqus Structural, Dynamic Explicit, Coupled Thermal-Structural, or Dynamic Coupled Thermal-Structural as the specified analysis typeFor a temperature initial condition, all Abaqus analysis types
Command Finder	Initial Conditions
Simulation Navigator	For a transient initial condition, in the appropriate step, right-click Constraint Container→New Constraint→Initial ConditionsFor a temperature initial condition, in the solution, right-click Constraint Container→New Constraint→Initial Conditions

How do I

Define transient initial conditions using magnitude and direction (Abaqus)

Define transient initial conditions using components (Abaqus)

Define normal transient initial conditions (Abaqus)

Define temperature initial conditions (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Initial conditions (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 } });