The Solid Mechanics Interface

The interface (

), found under the branch (

) when adding a physics interface, is intended for general structural analysis of 3D, 2D, or axisymmetric bodies. In 2D, plane stress, plane strain, or generalized plane strain assumptions can be used. The Solid Mechanics interface is based on solving the equations of motion together with a constitutive model for a solid material. Results such as displacements, stresses, and strains are computed.

The functionality provided by the Solid Mechanics interface depends on the products you are using. The Acoustics Module, MEMS Module, and Structural Mechanics Module add several features, for example geometric nonlinearity and advanced boundary conditions such as contact, follower loads, and nonreflecting boundaries.

The default material is a Linear Elastic Material. With either the Nonlinear Structural Materials Module or the Geomechanics Module, the physics interface is extended with more materials, for example, material models for plasticity, hyperelasticity, creep, and concrete. You can also add your own material models using an External Stress-Strain Relation


	For a detailed overview of the functionality available in each product, visit https://www.comsol.com/products/specifications/

When this physics interface is added, these default nodes are also added to the — , (a boundary condition where boundaries are free, with no loads or constraints), and . Then, from the toolbar, you can add other nodes that implement, for example, solid mechanics material models, boundary conditions, and loads. You can also right-click to select physics features from the context menu.

Settings

The is the default physics interface name.

The 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 field. The first character must be a letter.

The default (for the first physics interface in the model) is solid.

2D Approximation


	From the 2D approximation list, select Plane strain, Plane stress, or Generalized Plane Strain. Plane strain is relevant when the 2D model can be considered as a cut through an object that is infinitely long in the out-of-plane direction or as a soft object confined between rigid walls. The strain in the out-of-plane direction is assumed to be zero. Plane stress is relevant for structures that are thin in the out-of-plane direction, such as a thin plate. When using plane stress, the Solid Mechanics interface solves for the out-of-plane strain displacement derivative, , in addition to the displacement field u, in order to fulfill the condition that there is no stress in the thickness direction. The generalized plane strain condition is similar to plane strain, but allows for a nonzero out-of-plane strain. It is representative for the central parts of a long object, which is stress free at the ends. In this case, you can choose between two assumptions: a uniform out-of-plane strain, or a full linear distribution of the out-of-plane strain. The latter assumption corresponds to bending in the out-of-plane direction, and is used when the Enable out-of-plane bending check box is selected. For more information see the theory section. When combining Solid Mechanics with other types of physics, there is often an assumption that the out-of-plane extension is infinitely long. This is the case in, for example, Acoustic-Structure interaction problems. In these cases, Plane strain is usually the correct choice. Select Out-of-plane mode extension (time-harmonic) to prescribe an out-of-plane wave number to be used in mode analysis, eigenfrequency, and frequency domain studies. When selected, enter the Out-of-plane wave number kz. The input value will only be taken into account in eigenfrequency and frequency domain studies. For mode analysis, the out-of-plane wave number is computed as an eigenvalue. For more information, see Out-of-Plane and Circumferential Modes in the Structural Mechanics Theory chapter.

Axial Symmetry Approximation


	Select Circumferential mode extension (time-harmonic) to prescribe a circumferential wave number to be used in eigenfrequency or frequency domain studies. When selected, enter the Circumferential mode number m. For more information, see Out-of-Plane and Circumferential Modes in the Structural Mechanics Theory chapter.


	Eigenfrequency Analysis of a Free Cylinder: Application Library path Structural_Mechanics_Module/Verification_Examples/free_cylinder.

Thickness


	For 2D components, enter a value or expression for the Thickness d. The default value of 1 m is suitable for plane strain models, where it represents a unit-depth slice, for example. For plane stress models, enter the actual thickness, which should be small compared to the size of the plate for the plane stress assumption to be valid. When manually combining Solid Mechanics with other physics interfaces, you must make sure that the same thickness assumption is used everywhere. In most cases, the default settings will be correct since interfaces which do not have an explicit thickness property will implicitly assume unit thickness. Use a Change Thickness node to change thickness in parts of the geometry if necessary.

Structural Transient Behavior

From the list, select or . Use to treat the dynamic behavior as quasistatic (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 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.

Transient Solver Settings

In this section, you can add instructions used when generating the solver sequence for a wave-propagation transient problem. Select the check box to activate this functionality.

Enter the in the model, fmax,sol.

Select the (method) as or . The option is in general not recommended for wave problems.

The generated solver will be adequate in most situations if the computational mesh also resolves the frequency content in the model. Note that any changes made to these settings (after the model is solved the first time) will only be reflected in the solver if or is selected in the study.

For highly nonlinear problems set up with user-defined terms, manual tuning of the solver may be necessary. In nonlinear models, the maximum frequency to resolve should be selected based on the number of harmonics to be resolved.

Reference Point for Moment Computation

Enter the coordinates for the xref (variable refpnt). The resulting moments (applied or as reactions) are then computed relative to this reference point. During the results and analysis stage, the coordinates can be changed in the section in the result nodes.

Typical Wave Speed for Perfectly Matched Layers

The typical wave speed cref is a parameter for the perfectly matched layers (PMLs) if used in a solid wave propagation model. The default value is solid.cp, the pressure-wave speed. To use another wave speed, enter a value or expression in the field.

Note: This section is only available with COMSOL products that include PMLs (see https://www.comsol.com/products/specifications/).

Port Sweep Settings

Select to enable the option. This option is used to compute the full scattering matrix when Port conditions are used. For more details see The Port Sweep Functionality subsection. The section only exists for 3D geometries.

Automated Model Setup

This section will only be displayed if a mesh on NASTRAN® format, containing RBE2 elements, has been imported in an node under . 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 drop-down menu in the section title, you can select . 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 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 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 list.

Discretization

In the Solid Mechanics interface, you can choose not only the order of the discretization, but also the type of shape functions: Lagrange or serendipity. For highly distorted elements, Lagrange shape functions provide better accuracy than serendipity shape functions of the same order. The serendipity shape functions will however give significant reductions of the model size for a given mesh containing hexahedral, prism, or quadrilateral elements.

The default is to use shape functions for the . Using shape functions will give what is sometimes called constant stress elements. Such a formulation will for many problems make the model overly stiff, and many elements may be needed for an accurate resolution of the stresses.

Dependent Variables

The physics interface uses the global spatial components of the u as dependent variables. The default names for the components are (u, v, w) in 3D. In 2D the component names are (u, v), and in 2D axisymmetry they are (u, w). You can however not use the “missing” component name in the 2D cases as a parameter or variable name, since it is still used internally.

You can change both the field name and the individual component names. If a new field name coincides with the name of another displacement field, the two fields (and the interfaces which define them) share degrees of freedom and dependent variable component names. You can use this behavior to connect a Solid Mechanics interface to a Shell directly attached to the boundaries of the solid domain, or to another Solid Mechanics interface sharing a common boundary.

A new field name must not coincide with the name of a field of another type (that is, it must contain a displacement field), or with a component name belonging to some other field. Component names must be unique within a model except when two interfaces share a common field name.


	In the COMSOL Multiphysics Reference Manual see Table 2-4 for links to common sections and Table 2-5 to common feature nodes. You can also search for information: press F1 to open the Help window or Ctrl+F1 to open the Documentation window.

•

Domain, Boundary, Edge, Point, and Pair Nodes for Solid Mechanics

•

Solid Mechanics Theory

•

Selecting Discretization

•

Stresses in a Pulley: Application Library path

•

Eigenvalue Analysis of a Crankshaft: Application Library path