# Creating connector sections for assembled, complex, and basic connection types

 The connector section editor allows you to specify assembled, complex, or basic connection types; connector behaviors; and section data to include in the section definition. For more information, see Connector elements.
 Related Topics Understanding connector sections and functions Connector section editors Using the connector section editors Connectors
1. From the main menu bar, select ConnectorSectionCreate.

 Tip: You can also create a connector section using the tool in the Interaction module toolbox.

A Create Connector Section dialog box appears.

2. Enter a section name. For more information about naming objects, see Using basic dialog box components.

3. Choose one of the following connection categories:

• Choose Assembled/Complex to use either predefined combinations of basic connection types or complex connection types.

Click the arrow next to the Assembled/Complex type text field, and select the desired connection type from the list that appears.

• Choose Basic to use translational and rotational connection types.

1. If desired, click the arrow next to the Translational type text field, and select the connection type from the list that appears.

2. If desired, click the arrow next to the Rotational type text field, and select the connection type from the list that appears.

You can select one translational type, one rotational type, or one translational and one rotational type to define the connector section.

Abaqus/CAE displays the available and constrained components of relative motion (CORM) for the connection type that you have selected. In addition, you can click to see a schematic drawing of the connection type along with the Abaqus idealization of the connection.

For a description of assembled, complex, and basic connection types, see Connection types.

4. Click .

The connector section editor appears.

Note:

You can display help on a particular editor feature by selecting HelpOn Context from the main menu bar and then clicking the editor feature of interest. For more information on editor features, see Using the connector section editors.

5. To edit the connection type, click to the right of the connection type to display the connector section type editor. Select the connection type as described above. You must delete all behaviors from the editor before you can edit the connection type.

6. On the Behavior Options tabbed page, you can add, delete, and change behaviors as follows:

Adding behaviors

Click on the right side of the editor to display a list of available behaviors. Select the behaviors needed to define your connector section. You can define multiple behaviors of the same type for some behaviors. When you select a behavior, its name appears in the Behavior Options list, and data fields associated with the behavior appear in the data area in the bottom half of the editor. Use the data fields to enter information for the currently selected behavior. For more information, see Using the connector section editors.

Deleting behaviors

In the Behavior Options list, select the behavior that you want to delete, and click on the right side of the editor. This procedure removes the behavior from both the behavior options list and the connector section definition.

Changing behavior data

In the Behavior Options list, select the behavior whose data you want to change. When the data fields associated with the behavior appear in the bottom half of the window, change the information that you have entered for the behavior as desired.

7. On the Table Options tabbed page, you can specify behavior settings for the regularization (Abaqus/Explicit analyses only) and the extrapolation of tabular data for all of the behavior options in a connector section. Alternatively, you can specify behavior settings for individual behavior options. The button is available on the Behavior Options tabbed page for selected behavior options. Behavior settings for individual behavior options take precedence over the connector section behavior settings. For more information, see Specifying behavior settings for tabular data, and Defining connector behavior using tabular data.

Specify behavior settings on the Table Options tabbed page as follows:

1. In the Regularization portion of the page, specify the settings for the regularization of tabular data in an Abaqus/Explicit analysis. By default, Abaqus/Explicit regularizes the data into tables that are defined in terms of even intervals of the independent variables.

• Toggle on Regularize data to regularize tabular data.

• Toggle off Regularize data to turn off regularization of the tabular data and use the data that you define directly.

2. If you want to regularize tabular data, specify the error tolerance.

• Choose Use default to use the default value of 0.03.

• Choose Specify, and enter a value for the error tolerance.

3. In the Extrapolation portion of the page, specify the method for the extrapolation of tabular data. The data points that you enter make up a nonlinear curve in the constitutive space. By default, Abaqus extrapolates the dependent variables as constant values that correspond to the end points of the curve outside the specified range of the independent variables.

• Choose Constant to use constant extrapolation of the dependent variables outside the specified range of the independent variables.

• Choose Linear to use linear extrapolation of the dependent variables outside the specified range of the independent variables.

8. The Section Data tabbed page becomes available for the following connection types:

• For the Flow-Converter or Retractor connection type, enter the following section data:

Node b material flow scaling factor

Enter the scaling factor, $βs$, associated with the material flow at node b. Node b refers to the second point of a wire used to model a connector in Abaqus/CAE. The default value is 1.

For more information, see FLOW-CONVERTER and RETRACTOR.

• For the Slip Ring connection type, enter the following section data:

Mass per unit reference length

Enter the mass per unit reference length of belt material.

Contact angle around node b

The contact angle refers to the angle made by the belt wrapping around node b. Node b refers to the second point of a wire used to model a connector in Abaqus/CAE.

For an Abaqus/Standard analysis you must specify the contact angle directly. For an Abaqus/Explicit analysis you can specify the contact angle directly, or you can let Abaqus calculate the contact angle based on the configuration of your model:

• To let Abaqus calculate the contact angle, select Compute.

• To specify the contact angle directly, select Specify and enter the contact angle in degrees.

For more information, see SLIPRING.

9. Click to save the data and to exit the editor.