To create or edit a connector displacement boundary condition:

Display the connector displacement boundary condition editor using one of the following methods:

To create a new connector displacement boundary condition, follow the procedure outlined in “Creating boundary conditions,” Section 16.8.2 (Category: Mechanical; Types for Selected Step: Connector displacement).

To edit an existing connector displacement/rotation boundary condition using menus or managers, see “Editing step-dependent objects,” Section 3.4.12. To edit the region to which the boundary condition is applied, see “Editing the region to which a prescribed condition is applied,” Section 16.8.4.

If you are creating the boundary condition in a buckling step, select the Use BC for option that specifies the calculations for which you want the boundary condition used. For more information, see “Boundary conditions,” in “Eigenvalue buckling prediction,” Section 6.2.3 of the ABAQUS Analysis User's Manual.

If a Method field appears toward the top of the editor, click the arrow to the right of the field, and select one of the following:

Select Specify Constraints if you want to specify values for particular components of relative motion.

Select Fixed at Current Position if you want to fix the components of relative motion at their final values from the previous general step.

The Method option appears in the editor only if both methods are valid for the selected step.

If a Distribution field appears in the editor, click the arrow to the right of the field, and select one of the following:

Select Uniform to define a uniform boundary condition.

Select User-defined to define the boundary condition in user subroutine DISP. See the following sections for more information:

• “Specifying general job settings,” Section 18.6.6

• “DISP,” Section 1.1.4 of the ABAQUS User Subroutines Reference Manual

The Distribution option appears in the editor only if you are creating the boundary condition or editing the boundary condition in the step in which it was created. This option is unavailable if you select the Fixed at Current Position method or if you are performing an ABAQUS/Explicit analysis.

If you are defining the boundary condition directly in the editor (and not in user subroutine DISP), perform the following steps:

Use the appropriate method to define the boundary condition. Only components common to all of the selected wires are available in the editor.

If no text fields appear next to each component of relative motion:

Toggle on a component of relative motion to fix the value either at zero (if you are defining a component of relative motion in the initial step) or at its final value at the end of the previous analysis step (if you are defining the component of relative motion in the second analysis step or in a later step.)

Toggle off a component of relative motion to leave the component of relative motion unconstrained.

If text fields appear next to each component of relative motion:

Toggle on a component of relative motion to constrain the component of relative motion. The text field becomes available in which you can specify a value for the component of relative motion. If you are creating the boundary condition in this step, a default value of zero appears in the text field. If you are modifying the boundary condition in this step, the value propagated from the previous step appears in the text field.

Toggle off a component of relative motion to leave the component of relative motion unconstrained. If you toggle off a component of relative motion after modifying the default or propagated value in the text field, the modified value is lost. If you toggle that component of relative motion back on, the default or propagated value reappears in the text field.

Click the arrow to the right of the Amplitude field, and select the amplitude of your choice from the list that appears. Alternatively, you can click Create to create a new amplitude. (See Chapter 38, “The Amplitude toolset,” for more information.)

Click OK to save your data and to exit the editor.

If you are defining the boundary condition in user subroutine DISP, perform the following steps:

If desired, use the following techniques to define displacement. Only components common to all of the selected wires are available in the editor.

Toggle on a component of relative motion to constrain the component of relative motion. If you are in the initial step, that component of relative motion is set to zero. If you are in any step other than the initial step, a text field becomes available in which you can specify a value for the component of relative motion.

Toggle off a component of relative motion to leave the component of relative motion unconstrained.

Data that you enter in the editor for particular degrees of freedom are passed into the user subroutine.

Click OK to save your data and to exit the editor.

Enter the Job module and display the job editor for the analysis job of interest. (For more information, see “Creating, editing, and manipulating jobs,” Section 18.5.)

In the job editor, click the General tab, and specify the file containing the user subroutine that defines the boundary condition. For more information, see “Specifying general job settings,” Section 18.6.6.

Note:  You can specify only one user subroutine file in the job editor; if your analysis involves more than one user subroutine, you must combine the user subroutines into one file and then specify that file.