The Shell and Plate Interfaces
The Shell (shell) interface (), found under the Structural Mechanics branch () when adding a physics interface, is used to model structural shells on boundaries in 3D or 2D axisymmetry. Shells are thin flat or curved structures, having significant bending stiffness. The interface uses shell elements of the MITC type, which can be used for analyzing both thin (Kirchhoff theory) and thick (Mindlin theory) shells.
The Plate (plate) interface (), found under the Structural Mechanics branch () when adding a physics interface, provides the ability to model structural plates in 2D. Plates are thin flat structures with significant bending stiffness, being loaded in a direction out of the plane.
The Shell interface is for 3D and 2D axisymmetry models.
The Plate interface is for 2D models — domains are selected instead of boundaries, and boundaries instead of edges. Otherwise the Settings windows are similar to those for the Shell interface.
The Linear Elastic Material is the default material model. It adds a linear elastic equation for the displacements and has a Settings window to define the elastic material properties. With this material model, the material is assumed to be homogeneous through the thickness of the shell.
When this interface is added, these default nodes are also added to the Model BuilderLinear Elastic Material, Thickness and Offset, Free (a boundary condition where edges are free, with no loads or constraints), and Initial Values. Then, from the Physics toolbar, add other nodes that implement, for example, boundary conditions. You can also right-click Shell or Plate to select physics features from the context menu.
Settings
The Label is the default physics interface name.
The Name is used primarily as a scope prefix for variables defined by the physics interface. Refer to such physics interface variables in expressions using the pattern <name>.<variable_name>. In order to distinguish between variables belonging to different physics interfaces, the name string must be unique. Only letters, numbers, and underscores (_) are permitted in the Name field. The first character must be a letter.
The default Name (for the first physics interface in the model) is shell or plate.
Sketch
In the Sketch section, a conceptual sketch of the degrees of freedom in the Shell and Plate interfaces appears.
Axial Symmetry Approximation
Select Circumferential mode extension to prescribe a circumferential wave number to be used in eigenfrequency or frequency-domain studies. When selected, enter the Azimuthal mode number m.
For more information, see Circumferential Displacement and Out-of-Plane Waves in the Structural Mechanics Theory chapter.
Eigenfrequency Analysis of a Free Cylinder: Application Library path Structural_Mechanics_Module/Verification_Examples/free_cylinder.
Structural Transient Behavior
From the Structural transient behavior list, select Include inertial terms (the default) or Quasistatic. Use Quasistatic to treat the dynamic behavior as quasi static (with no mass effects; that is, no second-order time derivatives). Selecting this option gives a more efficient solution for problems where the variation in time is slow when compared to the natural frequencies of the system. The default solver for the time stepping is changed from Generalized alpha to BDF when Quasistatic is selected.
For problems with creep, and sometimes viscoelasticity, the problem can be considered as quasistatic. This is also the case when the time dependence exists only in some other physics, like a transient heat transfer problem causing thermal strains.
Fold-line Settings
The fold-line limit angle α is the smallest angle between the normals of two boundaries that makes their intersection to be treated as a fold line. The normal to the shell is discontinuous along a fold-line. Enter a value or expression in the α field. The default value is 0.001 radians (approximately 0.06 degrees). The value must be larger than 0, and less than π/2, but angles larger than a few degrees are usually not meaningful.
Since the rotational degrees of freedom have different meaning across a fold line, they are separate degrees of freedom, which a joined by a constraint. This constraint is, as default, implemented as a pointwise constraint. Select Use weak constraints to use a weak constraint instead.
Default Through-thickness Result Location
Enter a number between -1 and 1 for the Local z-coordinate [-1,1] for thickness-dependent results Z. The value can be changed from 1 (downside) to +1 (upside). The default is +1. A value of 0 means the midsurface of the shell. This is the default position for stress and strain evaluation during the results analysis. During the results and analysis stage, the coordinates can be changed in the Parameters section in the result features.
Advanced Settings
To display this section, click the Show More Options button () and select Advanced Physics Options in the Show More Options dialog box. Normally these settings do not need to be changed.
The Use MITC interpolation check box is selected by default, and this interpolation, which is part of the MITC shell formulation, should normally always be active.
For the Plate interface, the Use 3D formulation check box is used to select whether six or three variables are used in the formulation. For geometrically nonlinear analyses, or when in-plane (membrane) forces are active, six variables must be used. This check box is selected by default.
In order to maintain the property that the shell normal has unit length, a constraint is applied on the shell normal displacement degrees of freedom in each node. This constraint is, as default, implemented as a pointwise constraint.
Select a Normal constraint typePointwise constraint or Weak constraint. Switching to weak constraints may be necessary if weak constraints are used for other boundary conditions. A mesh node cannot have a combination of pointwise and weak constraints.
When a pointwise constraint is used, you can also select a Constraint methodNodal or Elemental. In the nodal method, one constraint per node is generated. When the elemental method is used, one constraint is generated per node in each element and the duplicates are removed during the constraint elimination pass. In most cases, the nodal method is preferable. Not only are fewer constraints generated, but also the risk that the constraints are conflicting due to variations of the normal direction in adjacent elements is eliminated.
You can choose how extra ODE variables added by some features are grouped in the Dependent Variables node of a generated solver sequence.
Select the Rigid materials check box to group variables added by Rigid Material nodes.
Select the Rigid connectors check box to group variables added by Rigid Connector nodes.
Select the Attachments check box to group variables added by Attachment nodes.
The selections made here can be overridden by the settings in the Advanced section of the Rigid Material, Rigid Connector or Attachment features.
Automated Model Setup
This section will only be displayed if a mesh on NASTRAN® format, containing RBE2 elements, has been imported in an Import node under Mesh. The purpose is to automatically create rigid connectors from RBE2 elements in the NASTRAN file.
An RBE2 element represents a rigid connection between a set of mesh nodes. This means that it can, and often does, connect elements from different physics interfaces.
In the menu in the section title, you can select Create Rigid Connectors from RBE2. The effect is that one rigid connector will be created for each RBE2 element in the imported file. This will happen for all physics interfaces in the Interfaces list. Supported interfaces are: Solid Mechanics, Shell, Beam, and Multibody Dynamics. If there are RBE2 elements spanning more than one physics interface, they will be automatically connected.
The created rigid connectors will have point, edge, and boundary selections as inferred from the nodes in the RBE2 element and the mesh connectivity. The ‘independent node’ of the RBE2 element is used as center of rotation for the rigid connector.
The Automated Model Setup section is present in the Solid Mechanics, Shell, and Beam interfaces. In a model that contains several physics interfaces, you should use the automated model setup from only one of them, and make sure that all the involved interfaces are selected in the Interfaces list.
Discretization
Select the order of the Displacement fieldLinear or Quadratic. The degrees of freedom for the displacement of the shell normals will always have the same shape functions as the displacements.
Dependent Variables
Both interfaces define two dependent variables (fields) — the displacement field u and the field of normal displacements ar. The names can be changed, but the names of fields and dependent variables must in general be unique within a model. If you intentionally use the same name for fields from different physics interfaces, these degrees of freedom are treated as being the same. This can be used when mixing different type of structural mechanics interfaces, where you often want the displacements to be the equal.
Vibrations of a Disk Backed by an Air-Filled Cylinder: Application Library path Structural_Mechanics_Module/Acoustic-Structure_Interaction/coupled_vibrations_manual
Pinched Hemispherical Shell: Application Library path Structural_Mechanics_Module/Verification_Examples/pinched_hemispherical_shell