Boundary Conditions

Boundary conditions are used to prescribe values of basic solution variables; for example, displacements and rotations in stress/displacement analysis. The following boundary conditions are available in the Nonlinear Structural Analysis workbench:

Creating Displacement Boundary Conditions: Defines the time history of displacement degrees of freedom on a geometry selection.

Creating Clamp Boundary Conditions: Fully constrains a geometry selection in all directions.

Importing Restraints: Imports a restraint definition from GPS into your analysis.

You apply environmental actions, such as boundary conditions, to supports (geometrical features) on your model. The supports that are available include points/vertices, curves/edges, surfaces/faces, or volumes/parts. In addition, point, line, or surface groups that were created from a mesh part are also valid supports. You can either select the support and then set the boundary condition specifications or set the boundary condition specifications and then select the support. Table 9–1 summarizes the supports to which each type of boundary condition can be applied.

Table 9–1 Supports for boundary conditions.

Boundary Condition Point, Vertex, or Point Group Curve, Edge, or Line Group Surface, Face, or Surface Group Volume, Part, or Body Other Supports
Displacement GPS User-defined Restraint
Clamp GPS Clamp


Creating Displacement Boundary Conditions

Displacement boundary conditions constrain the movement of selected degrees of freedom to zero or to a prescribed displacement history.

You can apply displacement boundary conditions only in mechanical steps.

The magnitude of a displacement boundary condition can vary with time during a step according to an amplitude definition (see Amplitudes for more information on defining amplitudes). If an analysis includes multiple general static steps, you can specify a “fixed” displacement boundary condition in the second or later general static step. Applying a fixed displacement boundary condition holds the selected degrees of freedom at their final position from the previous general static step.

You can prescribe the time variation of the magnitude of a displacement boundary condition in a user subroutine, which is sometimes preferable when the time history of the magnitude is complex. You can also apply knowledgeware techniques to control the value of a displacement boundary condition (for more information, see Applying Knowledgeware).

By default, displacement components are associated with the global, rectangular Cartesian axis system. You can specify a local coordinate system for the definition of displacement boundary conditions, and you can define the local system as a Cartesian, cylindrical, or spherical axis system. Local coordinate systems are defined in the CATIA Part Design workbench.

Displacement boundary conditions can be applied to point/vertex, curve/edge, surface/face, or body supports; to a point, line, surface, or body group; to a virtual part; or to a rigid coupling feature or a smooth coupling feature. When you select the support, you can also select an existing user-defined restraint from a different analysis case that was created in the Generative Structural Analysis workbench. The new displacement boundary condition is applied to the same region as the user-defined restraint created in the Generative Structural Analysis workbench. You can modify the region only by modifying the original user-defined restraint feature in the Generative Structural Analysis workbench.

Note:  For static analyses, make sure you define sufficient boundary conditions to prevent rigid body modes from occurring in your model.

This task shows you how to create a displacement boundary condition on geometry.

  1. Click the Displacement Boundary Condition icon .

    The Displacement BC dialog box appears, and a Displacement object appears in the specification tree under the Boundary Conditions objects set for the current step.

  2. You can change the identifier of the boundary condition by editing the Name field.

  3. Select the geometry support (a point, an edge, a surface, a body, a user-defined restraint, a coupling feature, or a virtual part that you created in the Generative Structural Analysis workbench). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the boundary condition to all supports simultaneously. You can also select an appropriate group.

    The Supports field is updated to reflect your selection.

  4. Toggle on Fix at Current Position if you want to “freeze” the selected degrees of freedom at their final values from the previous general static step. This option is available only if the current step is a general static step and is preceded by another general static step.

  5. Toggle on a degree of freedom to constrain it, and enter a value for the degree of freedom in the appropriate text field. The text field is not available if you chose to fix the degrees of freedom at their final values from the previous general step. Toggle off a degree of freedom to leave it unconstrained.

  6. Right-click on the text field for a degree of freedom to add knowledgeware controls to the selected field (for more information, see Applying Knowledgeware).

  7. Click More to access additional displacement boundary condition options.

    1. Toggle on Selected amplitude, and select an amplitude from the specification tree to define a nondefault time variation for the displacement boundary condition.

      If you do not specify an amplitude in a Nonlinear Structural case, the reference magnitude is applied linearly over the step (Ramp).

    2. Toggle on Selected local system, and select a coordinate system to define local directions.

    3. If desired, change the local orientation from Cartesian to Cylindrical or Spherical. See Using Local Coordinate Systems for more information.

    4. Toggle on Apply user subroutine to define a nonuniform variation of the displacement boundary condition magnitude throughout the step in user subroutine DISP. For more information, see Using User Subroutines.

    5. The propagation status shows the following:

      • Whether the boundary condition was Created in this step or Propagated into this step.

      • Whether the boundary condition is Active or Inactive.

  8. Click OK in the Displacement BC dialog box.

    Symbols representing the constrained degrees of freedom are displayed on the geometry.

Creating Clamp Boundary Conditions

Clamp boundary conditions fully constrain the movement of all degrees of freedom to zero.

You can apply clamp boundary conditions only in mechanical steps.

Clamp boundary conditions can be applied to point/vertex, curve/edge, surface/face, or body supports; to a point, line, surface, or body group; to a virtual part; or to a rigid coupling feature or a smooth coupling feature. When you select the support, you can also select an existing clamp from a different analysis case that was created in the Generative Structural Analysis workbench. The new clamp boundary condition is applied to the same region as the clamp created in the Generative Structural Analysis workbench. You can modify the region only by modifying the original clamp feature in the Generative Structural Analysis workbench.

Note:  For static analyses, make sure you define sufficient boundary conditions to prevent rigid body modes from occurring in your model.

This task shows you how to create a clamp boundary condition on geometry.

  1. Click the Clamp Boundary Condition icon .

    The Clamp BC dialog box appears, and a Clamp object appears in the specification tree under the Boundary Conditions objects set for the current step.

  2. You can change the identifier of the boundary condition by editing the Name field.

  3. Select the geometry support (a point, an edge, a surface, a body, a clamp, a virtual part, or a coupling feature that you created in the Generative Structural Analysis workbench). Any selectable geometry is highlighted when you pass the cursor over it. You can select several supports to apply the boundary condition to all supports simultaneously. You can also select an appropriate group.

    The Supports field is updated to reflect your selection.

  4. Click More to view the propagation status of the boundary condition. The propagation status shows the following:

    • Whether the boundary condition was Created in this step or Propagated into this step.

    • Whether the boundary condition is Active or Inactive.

  5. Click OK in the Clamp BC dialog box.

    Symbols representing the constrained degrees of freedom are displayed on the geometry.

Importing Restraints

Imported restraints enable you to incorporate a restraint definition from GPS into your analysis. Imported restraints can be oriented using rectangular coordinate systems only, and the following restraint types are available for import:

  • Clamp

  • Surface slider

  • Ball joint

  • Slider

  • Pivot

  • Sliding pivot

  • User-defined restraint

  • Iso-static restraint

This task shows you how to import a restraint definition into your analysis.

  1. Click the Imported Restraint icon .

    The Imported Restraint dialog box appears, and an Imported Restraint object appears in the specification tree under the Boundary Conditions objects set for the current step.

  2. You can customize the name of the imported restraint by editing the Name field. By default, Nonlinear Structural Analysis uses the name of the restraint it imports as the basis for the name of the imported restraint; for example, if you import Bearing Restraint.1 into your analysis, Nonlinear Structural Analysis uses the name Bearing Restraint-1 for the imported restraint object.

  3. Select the restraint feature or restraint set that you want to import. Any selectable geometry is highlighted when you pass the cursor over it.

    The Supports field is updated to reflect your selection.

  4. Click More to view the propagation status of the imported restraint. The propagation status shows the following:

    • Whether the imported restraint was Created in this step or Propagated into this step.

    • Whether the imported restraint is Active or Inactive.

  5. Click OK in the Imported Restraint dialog box.

    Symbols representing the constrained degrees of freedom are displayed on the geometry.