Nonlinear adaptivity refers to the capability of the solution process to adapt to changing conditions during a nonlinear analysis. The solution process uses a feedback mechanism to discretely or continuously adjust some internal parameters automatically so that an accurate and convergent solution is obtained.
A simple example of an adaptive process is the automatic time-stepping capability (AUTOTS,ON) that adjusts the time step suitably during the solution based on a set of internal parameters. No user intervention is required.
Adaptive meshing is another example of an adaptive process. In highly nonlinear problems, excessive deformation can cause parts to distort and/or fail. Examples include industrial applications involving:
Extrusion – The billet undergoes excessive deformation due to the flow of material into the die.
Gasket sealing – The gasket material is forced into narrow cavities to create a seal (a process known as gap filling).
Fracture mechanics – Localized high-stress and high-deformation fields around the crack-tip area can lead to part failure.
Adhesive debonding – High adhesion strength between soft materials can lead to localized high stresses and strains near the debonding cohesive zones.
Modeling such applications using the conventional finite element method can result in excessive mesh distortion, leading to convergence failure. Manual intervention to correct mesh distortion is not a viable option, requiring significant time and resources. In such cases, nonlinear adaptive-meshing techniques reduce the time and effort required to obtain accurate and convergent solutions.
Nonlinear mesh adaptivity (also available in Ansys Mechanical) modifies the mesh automatically based on specified criteria. Mesh modifications occur by splitting and/or morphing or by general remeshing. Loads, boundary conditions, contact conditions, solutions variables, etc., are seamlessly transferred to the new mesh as the solution progresses. The capability supports both local and global remeshing.
The ability to apply loading and constraint directly on the initial mesh for each load step (rather than on the new generated mesh) is useful if you want to set up some loading for all load steps in advance but the loading information is available based on the initial mesh only. Loads and constraints applied on the initial mesh are mapped and transferred to the current mesh for each specified load step. Initial-mesh loading and constraint also supports limited large-deflection effects (NLGEOM, ON).
You can also use nonlinear mesh adaptivity to alleviate convergence problems due to mesh distortion and/or improve local mesh density-dependent solution accuracy when hexahedron-dominant (hex-dom) meshes are used. The NLAD-ETCHG procedure converts hex-dom meshes to tetrahedral meshes so that the analysis can proceed to capture subsequent deformations accurately.
Adequate representation of the boundary throughout the deformation history can be difficult unless the initial mesh is carefully crafted. The NLAD-GPAD capability enables you to preserve the mesh/geometry relationship during deformation by maintaining a boundary representation (bRep) object and remeshing to it when required. NLAD-GPAD is initiated via the Ansys Mechanical Workflow for Nonlinear Adaptivity (Adaptivity Remeshing Controls in the Mechanical User's Guide) and cannot be initiated from within Mechanical APDL.
For contact-based cohesive zone modeling (CZM) problems, where the mesh can be too coarse to capture the local debonding behavior properly or high adhesion exists between two soft materials, you can use nonlinear adaptivity to capture the stress gradients and improve solution accuracy. The program modifies the mesh locally based on a combination of contact-based (NLADAPTIVE,,ADD,CONTACT,CZM) and mesh-quality-based criteria.
Element-removal-based criterion allows adaptive removal of elements during the solution. As with conventional nonlinear mesh adaptivity, the mapping of boundary conditions and loads is done automatically on the body with removed elements, followed by the mapping of solution variables and subsequent residual rebalancing. Element removal may be interpreted as an EKILL-like procedure for nonlinear problems within the solution itself – generalized to any state of deformation of the body and characterized by complete equilibrium states.
If you prefer to modify or repair meshes using other ANSYS, Inc. or third-party products, Mechanical APDL offers a manual rezoning capability, enabling you to import those meshes to continue the analysis.