To create a submodel boundary condition:

From the list of steps, select the step during which the submodel boundary condition will be applied.

From the Category field, select Other.

From the Types for Selected Step field, select Submodel and click Continue.

From the model, select the regions to which the boundary condition will be applied. In most cases you apply the boundary condition to the edges and faces that were created when you cut away regions from the global model. You can prescribe other boundary conditions to the same regions; for example, a symmetry boundary condition. The prescribed boundary conditions take precedence over the submodel boundary condition.

From the Edit Boundary Condition dialog box that appears, do the following:

In the Driving region field, do one of the following:

Select Automatic to allow ABAQUS/CAE to create the driving region by searching all regions in the global model that lie in the vicinity of the submodel.

Select Specify to specify a set name that will be used as the driving region. You must give the complete name of the set. The syntax for the set name is assembly_name.part_name-1.set_name, assuming that you are defining the driving region on the first instance of the part.

If you are driving a solid submodel with a shell global model, you must enter the maximum value of the shell thickness in the global model in the Shell thickness field.

In the Exterior tolerance field, do the following:

Enter the absolute exterior tolerance. This is the absolute value by which a driven node of the submodel may lie outside the elements of the global model. The default value is the relative exterior tolerance.

Enter the relative exterior tolerance. This is the fraction of the average element size in the global model by which a driven node of the submodel may lie outside the elements of the global model. The default value is .05.

For more information, see “Submodeling,” Section 10.2.1 of the ABAQUS Analysis User's Manual.

If you are driving a solid submodel with a solid global model or if you are driving a shell submodel with a shell global model, you must enter a comma-separated list indicating the degrees of freedom that are being driven; for example, 1,2,3. You cannot leave this field blank.

If you are driving a solid submodel with a shell global model, you can provide the thickness of the center zone size around the shell midsurface. The default value is 10% of the maximum shell thickness in the global model as defined in the Shell thickness field.

In the Global step number field, enter an integer representing the step number in the global analysis from which the values of the driven variables will be read.

If the time period of the submodel analysis is different from the time period of the global analysis, you can choose to scale the time period of the global step to match the time period of the submodel step. For example, ABAQUS determines the displacements of the global model at a time 20% into the global step and applies those displacements at a time 20% into the submodel step.

If you do not choose to scale the time period of the global step to match the time period of the submodel step, ABAQUS applies the displacements of the global model at the same time during the submodel step. For example, ABAQUS determines the displacements of the global model one second into the global step and applies those displacements one second into the submodel step. This behavior is probably not desired if the two time periods are different. You choose to scale the time period by toggling on Scale time period of global step to time period of submodel step.