Prescribed Displacement/Rotation
The Prescribed Displacement/Rotation node adds a point, edge, boundary, or domain condition to a model where the displacements and rotations are prescribed in one or more directions.
With this condition it is possible to prescribe one or more displacement components, as well as one or more rotational components, leaving the shell free to deform or rotate in the remaining directions. It is also possible set maximum and minimum limits for the displacements, so that for example a one-sided support can be modeled.
Coordinate System Selection
Select the coordinate system to use for specifying the prescribed displacement/rotation. The coordinate system selection is based on the geometric entity level.
Domains (Plate Interface)
From the Coordinate system list select from:
Global coordinate system (the default)
Shell Local System
Boundaries (Shell and Plate Interfaces)
From the Coordinate system list select from:
Global coordinate system (the default)
Boundary System (a predefined normal-tangential coordinate system)
Shell Local System
Edges (Shell Interface)
From the Coordinate system list select from:
Global coordinate system (the standard global coordinate system).
Local edge system (the default).
Points (Shell and Plate Interfaces)
From the Coordinate system list select from:
Global coordinate system (the default)
Shell Local System
Face Defining the Local Orientations
This setting is used in conjunction with a Local edge system and Shell Local System. If displacement or rotations is prescribed for an edge or point which is shared between boundaries, the local system can be ambiguous. Select the boundary which should define the local system. The default is Use face with lowest number.
Prescribed Displacement
For the displacement in each direction, select a setting from the list — Free, Prescribed, or Limited. Select:
Free (the default) to leave the displacement component unconstrained.
Prescribed to constrain the displacement component to a given value. Enter a scalar value for the component of the prescribed displacement u0.
Limited to set a maximum and a minimum limit for the displacement component. Enter values for the maximum displacement u0,max and the minimum displacement u0,min. By default, they are set to Inf and -Inf, which corresponds to no active constraint.
If any displacement component is set to Limited, an additional section Limited Displacement is visible. Select the Method used to implement the weak inequality constraint — Penalty or Augmented Lagrangian. For both methods, enter a Penalty factor kp.
By default, the Penalty method is suggested, which in principle enforces the maximum and minimum limits for the displacement by adding nonlinear springs with a stiffness equal to kp when the limits are exceeded. This method is usually robust, but the accuracy is directly dependent on the chosen penalty factor.
The Augmented Lagrangian method adds extra degrees of freedom to improve the accuracy of the constraint. Here, the penalty factor is a numerical parameter, and has less impact on the accuracy of the constraint compared to when using the penalty method. The implementation of the augmented Lagrangian method puts no restrictions on the solver sequence, but for good convergence, proper scaling of the extra degrees of freedom can be important.
The default value for the Penalty factor kp depends on to what type of entity the Prescribed Displacement/Rotation node is added. In the expressions below, <phys> is the tag of the physics interface, and <pd> is the tag of the Prescribed Displacement/Rotation node.
For points, the default expression is 100*<phys>.Eequ*<phys>.<pd>.charLen
For boundaries, the default expression is 100*<phys>.Eequ/<phys>.<pd>.charLen
Here, the terms point, edge, and boundary refer to the actual physical entities represented by the chosen geometric entities. For instance, in a 2D axisymmetric component, the circumferential direction is only implicitly modeled, and thus the physical entity level of the shell is interpreted as one level higher than the chosen geometric entity level. The highest entity level in the 2D Plate interface is interpreted as a boundary.
The variable <phys>.<pd>.charLen is equal to thickness of the shell or plate.
Prescribed Rotations
Select a prescribed rotation from the By list — Free, Rotation, or Normal vector. Select:
Free (the default) to leave the rotations unconstrained.
Rotation to activate a prescribed rotation in a certain direction. Enter a value or expression for the prescribed rotation, θ, about the tangential directions t1 and t2 of the shell local system. The rotation is always interpreted the with respect to the shell local system, and independent of the Coordinate System Selection.
For geometric linearity, select one or both of the Free rotation around t1 direction and Free rotation around t2 direction check boxes to remove the constraint for the corresponding rotation component. If unchecked, the rotations are constrained to either the input value or to the default zero rotation. The status of the check boxes has no effect when the geometric nonlinearity is activated under the study settings. This is because the constraints for different rotation components are not independent of each other in the case of finite rotations.
In 2D axisymmetry, there is only one input, the Prescribed rotation around the out-of-plane direction, Θ.
Normal vector to describe the rotation by prescribing the shell normal vector in the deformed configuration. Enter the components of the Prescribed normal vector N0.
Constraint Settings
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box.
In the COMSOL Multiphysics Reference Manual:
When Individual dependent variables is selected in the Apply reaction terms on list, the constraint forces are applied directly on the degrees of freedom, which are the displacements along the global coordinate axes. If you use this setting together with a local coordinate system, the results will be inconsistent since the constraint forces will not match the constraint orientation.
You can add a Harmonic Perturbation subnode for specifying a harmonic variation of the values of the prescribed displacements in a frequency domain analysis of perturbation type.
Location in User Interface
Context Menus
Ribbon
Physics tab with Shell selected:
Physics tab with Plate selected: