5.5.5.2. SMART Crack-Growth Assumptions and Limitations

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 only. To use it with a hex-dominant base mesh (analytical crack objects only) you need to set the Fracture object property Re-mesh Hex-dominant to Tetrahedral to Entire Part. This will re-mesh all parts associated with the bodies scoped to the analytical crack objects using tetrahedrons when Generate All Crack Meshes (right-click) menu option is executed.

  • Material behavior is assumed to be linear elastic isotropic.

  • When the Crack Growth Option property is set to Fatigue, crack growth is based on one of the following crack growth laws only:

    • Paris' Law

    • Tabular Fatigue Law

    • Forman equation

    • NASGRO Equation Version 3

    • NASGRO Equation Version 4

    • Walker Equation

    Note:  In the Engineering Data workspace, you can also include a fatigue crack-closure function with either Paris’ Law or the Tabular Fatigue Law. Supported functions include Elber Crack-Closure, Schijve Crack-Closure, Newman Crack-Closure, or Polynomial Crack-Closure.

  • When the Crack Growth Option property is set to Static, you can only specify the failure criteria (Failure Criteria Option property) as either Stress Intensity Factor (default) or J-Integral.

  • The following are not considered:

    • Large deflection/deformation

    • Finite-rotation effects

    • Crack-tip plasticity effects

    • Load-compression effects

  • 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 created by the loads and boundary conditions, are not maintained during SMART associated remeshing by default. Alternatively, you can use the Tabular Data option of the Define By property to define the load in a multi-step analysis.

  • To update node- and element-based Named Selections during SMART Crack Growth associated re-meshing, set the Preserve During Solve property to Yes.

  • 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.

  • 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.

  • Loads applied using the Surface Effect option of the Applied By property are not supported near the crack contours or inside the SMART associated re-meshing zone. They can be specified on the faces away from the re-meshing zone.

Graphical Display Limitations

Note the following SMART Crack Growth graphical display limitations:

  • 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.

  • When you set the Scoping Method property of the Fracture Tool object to Result File Item, probe results may not highlight crack face top and bottom nodes in the Geometry window.

Postprocessing Limitations

Note the following SMART Crack Growth postprocessing limitations:

  • Results and probes must be scoped to bodies only if the bodies will have mesh changes due to SMART Crack growth. Therefore, if you scope any result or probe on a vertex, edge, or face of a body that experiences a mesh change, such results or probes may not be evaluated. This limitation is due to changing mesh of the body. This limitation also applies to probes scoped to boundary conditions (via the Location Method property).

  • Non-fracture related probe results 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 (Fatigue or Static) for all SMART Crack Growth objects.

  • The Failure Criteria Option property must be set to the same option (SIFS or J-Integral) when the Crack Growth Option property is set to Static for all SMART Crack Growth objects.

  • The Crack Growth Methodology property must be set to the same option (Life Cycle Prediction or Cycle By Cycle) when the Crack Growth Option property is set to Fatigue 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 Life Cycle Prediction or Cycle By Cycle.

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 reference front element size (computed by the application), 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.

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 Moderate and Aggressive settings for the Mesh Coarsening property, you can specify a value up to 3 times the element size.

When the Crack Growth Methodology property is set to Cycle By Cycle, 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.