Once the crack mesh is generated, you can apply loads and constraints, then solve the analysis. Then, once the solution is done, you can analyze the stress and deformation pattern around the crack. For meshes defined by the Semi-Elliptical Crack object or the Arbitrary Crack object, you can apply the loads on the crack face top and bottom discontinuity plane using nodal named selections.
For the Semi-Elliptical Crack object, the application defines the internally generated crack mesh after the initial base mesh. The base mesh generation is based on a different set of requirements and constraints than the crack mesh. As a result, the crack mesh, generated using the Hex dominant mesh method, may not perfectly match the boundaries of the fracture affected zone. Because they may not match perfectly, kinematic constraints are required to establish a connection between base mesh and crack mesh in the boundaries of the fracture affected zone, which is accomplished using the multi-point constraint (MPC) contact. A contact pair is created at the interface of the crack and base meshes, with contact surface created at the interface on the buffer zone side of the base mesh and target surface created at the interface on the fracture affected zone side of the hex dominant mesh. When the solution is performed using internally-generated crack meshes, the MPC contact region is automatically created and sent to the solver.
Important: For Arbitrary Cracks as well as analytical cracks (ring, corner, etc.), the application does not create a contact pair when the Mesh Method property is set to .
Note: Static Structural and Transient Structural analyses are the only analyses supported for fracture mechanics calculations. However, the mesh with cracks is also supported with a static structural analysis linked to an upstream steady state thermal or transient thermal analysis.
Also, all loads and boundary conditions applicable to the static structural analysis are applicable with the existence of crack in the solution.
Although you can add Fracture and crack objects of any definition to a Modal analysis or a Mode Superposition (MSUP) Transient analysis, the application does not compute fracture parameters during the solution.
Computation of Fracture Parameters
The stress and deformation pattern around the crack is not sufficient to evaluate the catastrophic failure of the structure. The computation of fracture parameters and its comparison against fracture toughness is necessary for designing safe structures.
To compute fracture parameters for all cracks defined under the Fracture folder, the Fracture property in the Fracture Controls of the Analysis Settings must be set to . This entry is visible only if the Fracture folder exists in the model. By default, the application does not compute fracture parameters for Material Force and T-Stress. You need to set their properties under the Fracture Controls of the Analysis Settings to .
The computations used for fracture analysis include Stress Intensity Factors (SIFS), J-Integral (JINT), Energy Release Rates, Material Force, T-Stress and C*-Integral. The Mode 1 Stress Intensity Factor (K1), Mode 2 Stress Intensity Factor (K2), Mode3 Stress Intensity Factor (K3), and T-Stress are computed along the crack front using the interaction integral method. The Mode 1 Energy Release Rate (G1) and Mode 2 Energy Release Rate (G2), Mode 3 Energy Release Rate (G3) and Total Energy Release Rate (GT) are computed using the Virtual Crack Closure Technique (VCCT) along the crack front.
Note: The Energy Release Rate parameters, which are specific to the Pre-Meshed Crack object, are computed using the Virtual Crack Closure Technique (VCCT). When the VCCT technique is used, a specific mesh pattern composed of hexahedral shapes along the crack front is recommended for better accuracy. For more information, see Understanding Fracture Mechanics in the Fracture Analysis Guide.
The JINT result is a mixed mode result and is also computed along the crack front using
the domain integral method. The fracture parameters, for all cracks defined under the fracture
folder, are automatically computed and stored in the results file when the
Fracture property in the Fracture Controls category of Analysis Settings is set to
. The SIFS and JINT results are calculated for all cracks defined
under the Fracture folder. The VCCT results are calculated only if the crack mesh generated is
of lower order (dropped midside nodes). Material Force and T-Stress results are calculated
only when their respective control is set to Yes in the Fracture Controls category of Analysis Settings. You can direct
the fracture parameter computation for all cracks to use symmetry by setting the all
cracks symmetric variable to active with a value of 1 in the Variable Manager. For
more information, see Setting Variables. Fracture parameter calculation based on
SIFS supports linear isotropic elastic material behavior. VCCT based fracture parameter
calculation supports linear isotropic elastic, anisotropic elastic and orthotropic elastic
material behavior. J-Integral based and T-stress based fracture parameter calculation supports
isotropic elastic and isotropic plastic material behaviors. Material force based fracture
parameter calculation supports linear isotropic elastic, isotropic hardening plasticity,
kinematic hardening plasticity and isotropic hyperelastic material behaviors. C*-Integral
based fracture parameter calculation supports secondary (steady-state) creep material behavior
and it is computed along the crack front using the domain integral method. You can exclude
computation of any fracture parameter (except VCCT) by setting its respective control in the
Fracture Controls category of
Analysis Settings to .
Note: If you get the following message:
The fracture parameters computed during solution may be incorrect. Check the Solver Output on the Solution Information object for possible causes.
Check for the following:
A contact might have been created in the region of the crack contours.
A load might have been applied in the region of the crack contours that is not supported in the fracture parameter computation. Try replacing it with a Direct FE load. You can also replace the normal Pressure loads using the Applied By property option, .