Go to a section topic:
General Assumptions and Limitations
Review the following for the use of the SMART Crack Growth feature:
Only supports Static Structural analyses.
Supports 3-D crack growth only.
Supports Mixed Mode Crack Growth for Mode I and II only. If using J-Integral as Crack Growth Criterion, then only straight (Mode I) crack growth is supported.
Supports higher order tetrahedron mesh. To use it with a hex-dominant base mesh ( any analytical crack objects only) you need to set the Fracture object property Re-mesh Hex-dominant to Tetrahedral to . This will re-mesh the bodies scoped to the analytical crack objects using tetrahedrons when (right-click) menu option is executed.
Material behavior is assumed to be linear elastic isotropic.
Fatigue crack growth is based on Paris' Law.
Plasticity effects, nonlinear geometry effects, load-compression effects, and crack-tip-closure effects are not considered.
Supports the Bonded, No-Separation, Frictionless, Rough, and Frictional contact Type property options with CONTA174 and TARGE170 when they remain outside the remeshing zone during the simulation. SMART does not support any contact element inside the remeshing zone.
Function based loads and tabular loads with time as independent variable are not supported for fatigue crack growth analysis.
Step-based loading is not supported for both Static and Fatigue crack growth analyses.
Node- and element-based components are not maintained after remeshing. Therefore, Ansys recommends that you use the option of the Define By property to define the load in a multi-step analysis.
Does not currently support Point Mass or Distributed Mass.
Only supports the following Imported Loads:
Imported Pressure
Imported Force
Imported Displacement
Imported Body Temperature
Imported Initial Stress
Does not currently support Hydrostatic Pressure.
Either SIFS or J-Integral fracture parameter can be computed in one solution.
Restarting the analysis is currently not supported.
When the crack grows to the point of breaking the structural component apart, all solution results are set to zero and no crack-front information is reported.
Graphics Limitation: During your analysis, if your SMART crack grows from one body to another body, you need to scope the corresponding bodies to a Material Assignment object and assign them with the same material using Material Name property. This in turn facilitates the proper display of the crack front contour result in the graphics window.
Postprocessing Limitations
Note the following SMART Crack Growth postprocessing limitations:
Probes scoped to the same body as a SMART Crack Growth object will not evaluate.
The Crack Extension probe displays the sum of the crack extension increments from only those substeps in which crack extension increment information has been saved. That is, if crack results are not written for each specified Substep, as is the case when Analysis Settings > Output Controls property Store Results At is not set to All Time Points (or using the OUTRES,CINT,Value command snippet) in a Static Structural environment, the application does not display the entire crack extension for the Crack Extension probe. It is because these values are derived from the summation of results stored in the results file instead of the summation of results over all solved sub-steps. This same behavior is found with Total Number of Cycles probe result. Even if you issue additional OUTRES commands through the Commands (APDL) object, Ansys recommends that you issue OUTRES,CINT,ALL to specify all time points,
Multiple SMART Crack Growth Objects
Make sure of the following setting when you have specified multiple SMART Crack Growth objects:
Each crack specified on the model must be associated with an unique SMART Crack Growth object (1:1 ratio).
The Crack Growth Option property must be set to the same option ( or ) for all SMART Crack Growth objects.
The Failure Criteria Option property must be set to the same option ( or ) when the Crack Growth Option property is set to for all SMART Crack Growth objects.
The Crack Growth Methodology property must be set to the same option ( or ) when the Crack Growth Option property is set to for all SMART Crack Growth objects.
Note: The SMART Crack Growth feature uses local re-meshing and adaptation techniques and therefore has restrictions for the crack extension size.
For example, the feature might modify your entries in the Min Increment of Crack Extension or Max Increment of Crack Extension properties for either Crack Growth Methodology, either or .
The default value considered for the Max Increment of Crack Extension property is 1.5 times of the element size near the crack front. For manual entry, you can specify a value up to 2 times the element size for the Conservative Mesh Coarsening option. And, for the and settings for the Mesh Coarsening property, you can specify a value up to 3 times the element size.
The default value considered for the Min Increment of Crack Extension property is 0. The default behavior during the solution is if any crack extension is less than 0.02 times the element size, the Mechanical APDL solver sets the crack extension to 0. You can change the default by specifying any value between 0 and the Max Increment of Crack Extension property value.
When the Crack Growth Methodology property is set to , and you enter a number of cycles that is too large or too small, then the algorithm automatically re-defines the number of cycles according to the crack for each crack growth sub-step according to the crack extension limits.. The re-defined value of number of cycles is a multiple (n times or 1/n times) of user-defined number of cycles value.