Section Stiffness
The Section Stiffness material model provides a way of directly entering the stiffness or compliance of a shell without direct knowledge about the cross-section thickness and material distribution. Its main purpose is for entering homogenized properties of for example perforated or corrugated sheets.
Since only the stiffness, but not the section geometry is known, it is not possible to deduce the stresses. You can however provide an expression for stress computation based on the computed section forces.
In many cases, the properties of the shell cross section are anisotropic. All input data are interpreted along the local directions specified in the Coordinate System Selection section.
By adding the following subnodes to the Section Stiffness node you can incorporate other effects:
•
Thermal Expansion (for Materials)
•
Initial Stress and Strain
•
External Stress
•
Damping
Section Properties
From the Specify list, select Effective stiffness or Effective flexibility in order to specify the representation of the section stiffness.
For Effective stiffness, enter the Extensional stiffness matrix, DA; Bending-extensional stiffness matrix, DB; Bending stiffness matrix, DD; and Shear stiffness matrix, DAs.
For Effective flexibility, enter the Extensional flexibility matrix, Da; Bending-extensional flexibility matrix, Db; Bending flexibility matrix, Dd; and Shear flexibility matrix, Das.
If required, enter also the Translational inertia, I0; Rotational-translational inertia matrix, I1; and Rotational inertia matrix, I2. The translational inertia is the average mass per unit area. As long as the shell is not thick or shear flexible, the two latter contributions to the inertia can usually be ignored. If the mass distribution of the shell is symmetric with respect to the midplane, then I1 is identically zero.
The default for all section properties is to take the values From material. Any one of the matrices can also be User defined.
The inertia matrices are needed only for dynamic analysis. They are also used when computing mass forces for gravitational or rotating frame loads, and when computing mass properties (Computing Mass Properties).
Stress Evaluation Properties
If you want a certain stress value to be computed, you can enter a linear relation between section forces and stress here.
Enter an In-plane force factor, SN. This is a matrix which transforms the local membrane force (N11, N22, N12) into a local in-plane stress (s11, s22, s12).
Enter a Moment factor, SM. This is a matrix which transforms the local bending moment (M11, M22, M12) into a local in-plane stress (s11, s22, s12).
Enter an Out-of-plane force factor, SQ. This is a matrix which transforms the local shear force (Q1, Q2) into a local transverse shear stress (s13, s23).
Shear Correction Factor
Enter the shear correction factors for transverse shear k23 and k13.
When computing the contribution from shear stiffness to the total virtual work, it is necessary to take into account that the shell approximation assumes that shear stresses and strains in the thickness direction are constant, whereas in reality the distribution is more complicated. The shear correction factors are used to compensate for this, so that the total strain energy density is correct. When operating with stiffness and flexibility matrices, this correction can also be built directly into the matrices DAs and Das. Is so, set both shear correction factors to 1.
Geometric Nonlinearity
The settings in this section control the overall kinematics, the definition of the strain decomposition, and the behavior of inelastic contributions, for the material.
Select a Formulation — From study step (default), Total Lagrangian, or Geometrically linear to set the kinematics of the deformation and the definition of strain. When From study step is selected, the study step controls the kinematics and the strain definition.
•
With the default From study step, a total Lagrangian formulation for large strains is used when the Include geometric nonlinearity check box is selected in the study step. If the check box is not selected, the formulation is geometrically linear, with a small strain formulation.
To have full control of the formulation, select either Total Lagrangian, or Geometrically linear. When Total Lagrangian is selected, the physics will force the Include geometric nonlinearity check box in all study steps.
When inelastic deformations are present, such as for plasticity, the elastic deformation can be obtained in two different ways: using additive decomposition of strains or using multiplicative decomposition of deformation gradients.
Select a Strain decomposition — Automatic (default), Additive, or Multiplicative to decide how the inelastic deformations are treated. This option is not available when the formulation is set to Geometrically linear.
•
When Automatic is selected, a multiplicative or additive decomposition is used with a total Lagrangian formulation, depending on the Include geometric nonlinearity check box status in the study step.
•
Select Additive to force an additive decomposition of strains.
•
Select Multiplicative to force a multiplicative decomposition of deformation gradients. This option is only visible if Formulation is set to Total Lagrangian.
The Strain decomposition input is only visible for material models that support both additive and multiplicative decomposition of deformation gradients.
•
There are some cases when a small strain formulation could be useful for a certain domain, even though the study step is geometrically nonlinear. One such case is contact analysis, where the study step is always geometrically nonlinear, but where a geometrically linear formulation is sufficient for the material.
•
When a multiplicative decomposition is used, the order of the subnodes matters. The inelastic deformations are assumed to occur in the same order as the subnodes appear in the model tree.
See Lagrangian Formulation, Deformation Measures, and Inelastic Strain Contributions in the Structural Mechanics Theory chapter.
See Modeling Geometric Nonlinearity in the Structural Mechanics Modeling chapter.
See Study Settings in the COMSOL Multiphysics Reference Manual.
Location in User Interface
Context Menus
Shell>Material Models>Section Stiffness
Plate>Material Models>Section Stiffness
Ribbon
Physics tab with Shell selected:
Boundaries>Material Models>Section Stiffness
Physics tab with Plate selected:
Domains>Material Models>Section Stiffness