To create a load, boundary condition, or field, select Create from the appropriate menu in the main menu bar. A Create dialog box will appear in which you can provide a name for the prescribed condition and choose the type of the prescribed condition that you want to create.
When you click Continue in the Create dialog box, you are prompted to select the region or connectors to which you want to apply the prescribed condition, unless the prescribed condition is applied to the whole model. You should apply connector loads and connector boundary conditions only to the available components of relative motion of a connector. If you are selecting multiple connectors, you should ensure that all of the connectors have the available components of relative motion for which you are defining loads and boundary conditions. Once you have selected the region or connectors, an editor appears in which you can specify additional information about the prescribed condition, such as its magnitude.
The top panel of each prescribed condition editor displays the name and type of the prescribed condition, the analysis step you are currently in, and the region of the model or the connectors to which the prescribed condition will be applied. If you are editing a prescribed condition in the step in which it was first created, an Edit Region button appears next to the Region field or an Edit button appears next to the Connectors field; these buttons allow you to edit the region or connectors to which the prescribed condition is applied. If the prescribed condition is applied to the whole model, the Edit Region and Edit buttons are not applicable and, hence, do not appear. (For more information, see “Editing the region to which a prescribed condition is applied,” Section 16.8.4, and “Respecifying the connectors to which a load or boundary condition is applied,” Section 16.8.5.)
The format of the rest of the editor depends on the type of prescribed condition you are defining and on the step specified at the top of the editor. For example, the editor for concentrated forces is shown in Figure 16–2.
This editor contains special text fields in which you can specify the components of the force in the 1-, 2-, and 3-directions. The editor also contains an Amplitude text field that allows you to vary the magnitude of the prescribed condition as a function of time. You can accept either the default amplitude or select an amplitude that you have defined using the Amplitude toolset. (For more information, see Chapter 39, “The Amplitude toolset.”)You can specify the coordinate system in which you will apply the following loads or boundary conditions:
Concentrated force loads
Moment loads
General and shear surface tractions
General shell edge loads
Inertia relief loads
Displacement/rotation boundary conditions
Velocity/angular velocity boundary conditions
Acceleration/rotational acceleration boundary conditions
If the load or boundary condition allows you to specify the coordinate system, you can select an existing datum coordinate system or you can accept the global coordinate system. If the desired datum coordinate system does not exist, you can create it using the Datum toolset. (For more information, see “Creating datum coordinate systems,” Section 40.9.) Alternatively, you can refer to an ABAQUS/Standard user subroutine that defines the coordinate system (see “ORIENT,” Section 25.2.14 of the ABAQUS Analysis User's Manual).
Note: If you delete or suppress the datum coordinate system, the orientation of the load or boundary condition reverts to the global coordinate system.
The rules for creating and modifying fields vary depending on the field type:
Some fields require that you specify only the initial conditions. You can create and edit this type of field only in the initial step. ABAQUS computes subsequent values for the field as the analysis progresses. Currently, initial velocity is the only field of this type that is supported. For more information, see “Initial conditions,” Section 19.2.1 of the ABAQUS Analysis User's Manual.
You can create temperature fields for any step in the analysis. You can define the temperatures for the current model either by entering the values for the desired steps or by reading the temperature values computed by ABAQUS in a previous analysis with thermal components. For more information, see “Temperature,” in “Predefined fields,” Section 19.6.1 of the ABAQUS Analysis User's Manual.
Note: If you do not define initial values for a field, that field is assumed to have a value of zero at the start of the analysis.
Once you have created a prescribed condition, you can modify the prescribed condition in the following ways:
You can modify some or all of the data that you entered in the editor when you created the prescribed condition.
You can use the managers to modify the stepwise history of the prescribed condition. (For more information, see “What are step-dependent managers?,” Section 3.4.2.)
To display help on a particular manager or editor feature, select Help
On Context from the main menu bar and then click the feature of interest.
