Safety
Use the Safety subnode to set up variables which can be used to check the risk of failure according to various criteria. It can be used in combination with Linear Elastic Material, Nonlinear Elastic Material, and Layered Linear Elastic Material. Four different variables describing the failure risk are defined, as described in Table 4-2.
You can add any number of Safety nodes to a single material model. The contents of this feature do not affect the analysis results as such, so you can add Safety nodes after having performed an analysis, and just do an Update Solution in order to access to the new variables for result evaluation.
Table 4-2: Variables for Safety Factor Evaluation
Variable
Description
Criterion Fulfilled
Criterion violated
Failure index, FI
For a linear criterion, this is the ratio between the computed value and the given limit.
FI<1
FI>1
Damage index, DI
A binary value, indicating whether failure is predicted or not. DI is based on the value of FI.
DI=0
DI=1
Safety factor, SF
For a linear criterion, this is 1/FI.
SF>1
SF<1
Margin of safety, MoS
SF-1
MoS>0
MoS<0
For orthotropic and anisotropic failure criteria, the directions are given by the coordinate system selection in the parent node.
When you add a Safety node in one of the Shell, Layered Shell, or Membrane interfaces, a default plot with the failure index is generated. Such plots are placed in a group named Failure Indices. The label of these plots is derived from the label of the corresponding Safety node.
The Safety node is only available with some COMSOL products (see https://www.comsol.com/products/specifications/)
Shell Properties
This section is only present when Safety is used as a subnode to:
•
Linear Elastic Material in the Layered Shell interface. See the documentation for the Safety node in the Layered Shell chapter.
•
Layered Linear Elastic Material in the Shell interface. See the documentation for the Safety node in the Shell and Plate chapter.
•
Layered Linear Elastic Material in the Membrane interface. See the documentation for the Safety node in the Membrane chapter.
Failure Model
Select a Failure Criterion. The available choices depend on the physics interface, as indicated in Table 4-3.
Table 4-3: Available Failure Criteria by Physics Interface
Criterion
Solid Mechanics
Shell, Plate
Layered Shell
Membrane
Beam, Pipe Mechanics
Truss
von Mises
X
X
X
X
X
X
Tresca
X
X
X
X
X
X
Rankine
X
X
X
X
X
X
St. Venant
X
X
X
X
X
X
Mohr-Coulomb
X
–
–
–
–
–
Drucker-Prager
X
–
–
–
–
–
Bresler-Pister
X
X
–
–
–
–
Willam-Warnke
X
X
–
–
–
–
Ottosen
X
X
–
–
–
–
Jenkins
X
X
X
X
–
–
Waddoups
X
X
X
X
–
–
Azzi-Tsai-Hill
Plane stress
X
X
X
–
–
Norris
Plane stress
X
X
X
–
–
Tsai-Hill
X
X
X
X
–
–
Hoffman
X
X
X
X
–
–
Tsai-Wu Orthotropic
X
X
X
X
–
–
Zinoviev1
–
X
X
–
–
–
Hashin-Rotem1
–
X
X
–
–
–
Hashin1
–
X
X
–
–
–
Puck1
–
X
X
–
–
–
LaRC031
–
X
X
–
–
–
Tsai-Wu Anisotropic
X
X
X
X
–
–
User defined
X
X
X
X
X
X
1) Requires the Composite Materials Module
•
When Failure Criterion is von Mises, enter Tensile strength σts.
•
When Failure Criterion is Tresca, enter Tensile strength σts.
•
When Failure Criterion is Rankine, enter Tensile strength σts and Compressive strength σcs.
•
When Failure Criterion is St. Venant, enter Ultimate tensile strain εts and Ultimate compressive strain εcs.
•
When Failure Criterion is Mohr-Coulomb, select Material parameters — Cohesion and angle of friction or Tensile and compressive strengths to determine the type of input data.
When Cohesion and angle of friction is used, enter Cohesion c and Angle of internal friction φ.
When Tensile and compressive strengths is used, enter Tensile strength σts and Compressive strength σcs.
In either case, you can select Include elliptic cap to limit the allowed compressive stress. When selected, enter the Elliptic cap parameters pa and pb.
•
When Failure Criterion is Drucker-Prager, select Material parameters — Drucker-Prager parameters, Tensile and compressive strengths, or Mohr-Coulomb parameters to determine the type of input data.
When Drucker-Prager parameters is used, enter Drucker-Prager alpha coefficient α and Drucker-Prager k coefficient k.
When Tensile and compressive strengths is used, enter Tensile strength σts and Compressive strength σcs.
When Mohr-Coulomb parameters is used, enter Cohesion c and Angle of internal friction φ.
In either case, you can select Include elliptic cap to limit the allowed compressive stress. When selected, enter the Elliptic cap parameters pa and pb.
•
When Failure Criterion is Bresler-Pister, enter Tensile strength σts, Compressive strength σcs, and Biaxial compressive strength σbc.
•
When Failure Criterion is Willam-Warnke, enter Tensile strength σts, Compressive strength σcs, and Biaxial compressive strength σbc.
•
When Failure Criterion is Ottosen, enter the Compressive strength σcs, Ottosen parameters a and b, the Size factor k1, and the Shape factor k2.
•
When Failure Criterion is Jenkins, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy.
•
When Failure Criterion is Waddoups, enter Ultimate tensile strains εts, Ultimate compressive strains εcs, and Ultimate shear strains γss. All entries have three components, related to the principal axes of orthotropy.
•
When Failure Criterion is Azzi-Tsai-Hill, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy.
•
When Failure Criterion is Norris, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy.
•
When Failure Criterion is Tsai-Hill, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy. Select the Use plane stress formulation check box to assume plane stress conditions, see The Tsai–Hill Criterion.
•
When Failure Criterion is Hoffman, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy.
•
When Failure Criterion is Tsai-Wu Orthotropic, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy. Select the Use plane stress formulation check box to assume plane stress conditions, see The Orthotropic Tsai–Wu Criterion.
•
When Failure Criterion is Zinoviev, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy.
•
When Failure Criterion is Hashin-Rotem, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy.
•
When Failure Criterion is Hashin, enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy. Select the Use plane stress formulation check box to assume plane stress conditions, see The Hashin Criterion.
•
When Failure Criterion is Puck:
-
Enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy.
-
Enter the Fiber failure data: Ultimate tensile strain in longitudinal direction, εts1, and Ultimate compressive strain in longitudinal direction, εcs1. Also, enter the fiber material properties Young’s modulus of fiber in longitudinal direction, Ef1, and In-plane Poisson’s ratio of fiber, νf12. Enter a Mean stress magnification factor, mf. The default value is 1.3, a value commonly assumed for GFRP. For CFRP, the value 1.1 has been suggested.
-
Enter the Interfiber failure data: Linear degradation stress, σ1D. Also, enter the Slope of in-plane fracture envelope, tension, ptl, and the Slope of in-plane fracture envelope, compression, pcl. The default values are 0.3 and 0.25, respectively. These values are common for GFRP. For CFRP, the values 0.35 and 0.3 have been suggested.
•
When Failure Criterion is LaRC03:
-
Enter Tensile strengths σts, Compressive strengths σcs, and Shear strengths σss. All entries have three components, related to the principal axes of orthotropy. Also, enter the Ultimate tensile strain in longitudinal direction, εtsl.
-
Enter the In situ transverse tensile strength, , and In situ in-plane shear strength, . For both parameters, the default is to compute the value from the data given above, as indicated by the selections From transverse tensile strength and From in-plane shear strength respectively. You can also take the values From material, or select User defined to enter own expressions.
-
Enter Young’s modulus in longitudinal direction, E1, Young’s modulus in transverse direction, E2, In-plane Poisson’s ratio, ν12, and In-plane shear modulus, G12. For all four parameters, the default selection is From parent, indicating that the values are taken from the linear elastic properties in the parent node. You can also take the values From material, or select User defined to enter own expressions.
-
Enter the Fracture plane angle under transverse compression, α0. The default value is 53°. Also enter the Fracture plane search angle, Δα. The default value is 3°. Under combined loading, the fracture plane angle will differ from α0, and a numerical search for the critical angle is performed in the range 0 < α < α0. The step in the search is Δα.
•
When Failure Criterion is Tsai-Wu Anisotropic, enter Second rank tensor, Voigt notation f, and Fourth rank tensor F. Enter the components of the tensors with respect to the directions of the coordinate system in the parent node, see The Anisotropic Tsai–Wu Criterion.
•
When Failure Criterion is User defined, you enter two expressions describing the Failure criterion g(S), used in the failure index, and the Safety factor sf(S). As an example, if you would like to replicate the von Mises Isotropic criterion with tensile strength 350 MPa, you could enter g(S) as solid.mises/350[MPa]-1 and sf(S) as 350[MPa]/(solid.mises+eps).
For all input fields, the default is to take the value From material. Change to User defined to enter other values or expressions.
For a detailed description of the various criteria, see Safety Factor Evaluation in the Structural Mechanics Theory chapter.
Location in User Interface
Context Menus
Solid Mechanics>Linear Elastic Material>Variables>Safety
Solid Mechanics>Nonlinear Elastic Material>Variables>Safety
Shell>Linear Elastic Material>Variables>Safety
Shell>Layered Linear Elastic Material>Variables>Safety
Layered Shell>Linear Elastic Material>Variables>Safety
Plate>Linear Elastic Material>Variables>Safety
Membrane>Layered Linear Elastic Material>Variables>Safety
Membrane>Linear Elastic Material>Variables>Safety
Membrane>Nonlinear Elastic Material>Variables>Safety
Beam>Linear Elastic Material>Variables>Safety
Truss>Linear Elastic Material>Variables>Safety
Pipe Mechanics>Fluid and Pipe Materials>Variables>Safety
Ribbon
Physics tab with Linear Elastic Material, Layered Linear Elastic Material, Nonlinear Elastic Material, or Fluid and Pipe Materials node selected in the model builder tree:
Attributes>Variables>Safety