The Nonlinear Adaptive Region condition enables you to change the mesh during the solution phase to improve precision without incurring a great deal of computational penalties. The Nonlinear Adaptive Region feature is completely automatic. It does not require any user input during the solution phase. It acts as a remesh controller based on certain criteria. The criteria determine whether or not the mesh requires modification and, if so, which parts need to be modified. This feature is based on load stepping, requiring you to define a number of steps for your analysis, while also allowing you to activate and/or deactivate the feature on a per step basis.
This condition may be useful for nonlinear problems that experience convergence difficulties or accuracy issues because of elemental distortions. Large deformation problems are best suited to the use of the condition.
The Nonlinear Adaptive Region condition requires the following settings.
The Large Deflection property must be set to in the Solver Controls category of the Analysis Settings.
The Store Results At property must be set to in the Output Controls category of the Analysis Settings.
Note the following limitations for this condition.
Is not supported for:
Distributed ANSYS Solver
Convergence
Cannot be used in combination with the following features/conditions on the same part:
Cyclic Symmetry
Contact Formulations: Normal Lagrange (3D), MPC, and Beam
Contact Behaviors: Auto Asymmetric
Point Mass, Beam Connection, Joints, Spring, and Bearing
Remote Force, Remote Displacement, Moment, Thermal Condition, and Remote Point
Spatially varying boundary conditions
Cannot be used in combination with the following boundary conditions:
Coupling
Constraint Equation
The following materials properties are not supported:
Cast Iron
Concrete
Cohesive Zone
Damage
Microplane
Shape Memory Alloy
Swelling
When linking analyses, you cannot apply the solution phase modified mesh to the linked system.
When using the Nonlinear Adaptive Region during the restart of an analysis, the Nonlinear Adaptive Region object does not support Named Selections if your model contains a mesh change prior to the restart point.
If your analysis failed to converge and you are adding a new Nonlinear Adaptive Region object, it is necessary that the contact object property, Behavior, was set to either or for the initial solution that was processed.
When the option is specified for the Criterion property:
does not support high order elements for 2D analyses.
does not support self-contact for 3D analyses.
cannot be used in the combination with Weak Springs (COMBIN14 element type).
Because this condition causes mesh changes during the course of the solution process, there are result scoping limitations.
Only Body scoping is permitted (for bodies whose meshes will change). Therefore, if you scope any result or probe on a vertex, edge, or face of a body that experiences a mesh change, the analysis will not solve. This limitation is a result of the base mesh of the body being represented by nodes only. This limitation also applies to probes scoped to boundary conditions (via Location Method property).
Element selection on a result is not supported.
Does not support the multiple result set options of the By property: / or /.
Penetration plot following remesh may show the curve discontinuity.
Is not supported when transferring the deformed geometry and mesh of a Deformation result.
When using the Deformation result tracker to graph displacement, note there is a display limitation for the graph. The tracker reads and displays data contained in the jobname.nlh file. This file contains incremental displacement data collected after re-meshing occurs. That is, the re-meshed model is considered as a new reference.
Nonlinear Adaptive Region is available for Static Structural analyses.
The following section outlines the common characteristics that include application requirements of the condition, support limitations, as well as loading definitions and values.
Dimensional Types
3D Simulation: Supported for linear tetrahedral elements.
2D Simulation: Supported.
Geometry Types: Geometry types supported for the Nonlinear Adaptive Region condition include:
Solid: Supported.
Surface/Shell: Not Supported.
Wire Body/Line Body/Beam: Not Supported.
Topology: The following topology selection options are supported for Nonlinear Adaptive Region.
Body: Supported.
Face: Not Supported.
Edge: Not Supported.
Vertex: Not Supported.
Nodes: Not Supported.
Elements: Supported - for element-based Named Selections only.
Note:
Elements must be of the same element type, material, nodal orientation, and element orientation.
If two regions with different element or material attributes require re-meshing, you must impose nonlinear adaptive regions separately.
To apply a Nonlinear Adaptive Region:
On the Environment context toolbar: click Conditions>Nonlinear Adaptive Region. Or, right-click the Environment tree object or the Geometry window and select Insert>Nonlinear Adaptive Region.
Specify the Scoping.
Note: You can scope multiple Nonlinear Adaptive Regions to the same entity to give yourself more control on multiple load step settings that are local to the Nonlinear Adaptive Region condition.
Specify the Criterion: options include , , and .
| If Energy... | If Box... | If Mesh... |
|---|---|---|
|
Define an Energy Coefficient value. The
Energy Coefficient must be non-negative. Default
numeric value is |
Define the following properties. The origin of Coordinate System gives the minimum values of the box, and the Length property provides the diagonal length of box. Length values must be positive numbers.
The Box option defines a region on the model | Nonlinear Adaptivity Controls become available in the Analysis Settings. The Criterion is recommended.
|
Specify the Check At property as either or .
Enter the Value property based on the Check
At property selection. This value must be an integer. Default integer
value is 1.
Specify the Time Range property as or . If Manual, specify Start Time and End Time values. The start and end time values regulate the effective range of possible remeshing. No remeshing will occur at a time outside of this range.
When the condition is defined, the Graph and Tabular Data windows provide a right-mouse click option to (or ) the condition for a desired load step. No remeshing will occur at the deactivated load step as the NLADAPTIVE command is set to OFF. The default setting is Activated. For a restart analysis, the application sets the newly added Nonlinear Adaptive Region to Deactivated.

Note: You may wish to review the Activation/Deactivation of Loads topic in the Step Controls section of the Help. The Nonlinear Adaptive Region condition is displayed in the graph for the Analysis Settings object.
The selections available in the Details view are described below.
| Category | Fields/Options/Description |
|---|---|
| Scope |
Scoping Method, options include:
You may wish to review the Mechanical APDL References and Notes at the bottom of the page for specific command execution information regarding these selections. |
| Definition |
Criterion: options included , , or .
Check At: options included or .
Value: This property further defines the Check
At property. The default value is Time Range: options included or . When specified as , you need to enter a and . The value must be larger than the value. Suppressed: Include ( - default) or exclude () the condition. |
Following the solution process, to determine if the mesh was changed:
Select the Solution object or a Result object, the Tabular Data window displays the substeps with a changed mesh (Changed Mesh column = ).
Select the Solution Information object and set the Solution Output property to . A chart displays. Remesh Points are shown by solid orange vertical lines.
Create a User Defined Result (using the PNUMELEM Expression) to view the new elements that have relatively larger element identities than the original element identities. You can duplicate this result and specify a ( property) for a result prior to a remesh and one at a remesh point, and using the Viewports feature, directly compare the (before and after) elements in the graphics window.
The following Mechanical APDL commands, element types, and considerations are applicable for this condition.
The Nonlinear Adaptive Region is applied with the NLADAPTIVE command.
When the Scoping property is defined as , the Nonlinear Adaptive Region condition uses the CM command to create the Nonlinear Adaptive Region component.
When the Scoping property is defined as a , the Nonlinear Adaptive Region condition uses the CMBLOCK command to create the Nonlinear Adaptive Region component.
The CMSEL,ALL command and the ESEL,ALL command are issued at beginning of the NLADAPTIVE command.
During a Structural Analysis, the Nonlinear Adaptive Region is applied using the PLANE182 (2-D Low Order), PLANE183 (2-D High Order), and SOLID285 (3-D Linear Tetrahedral) element types.
When a Nonlinear Adaptive Region is scoped to a body/element, the associated part is meshed with SOLID285 element type if they are linear tetrahedral.
When a Nonlinear Adaptive Region is deactivated for certain steps, the NLADAPTIVE command is set to be OFF in the corresponding load steps. Relatively, an activated Nonlinear Adaptive Region sets the NLADAPTIVE command to be ON.
When a Nonlinear Adaptive Region is applied, the ETCONTROL ,SET command is not issued.
The purpose of nonlinear adaptive region is to repair a distorted mesh in order to overcome convergence problems caused by the distortion. It is effective only when the mesh distortion is caused by a large, nonuniform deformation. Nonlinear adaptive region cannot help if divergence occurs for any other reason such as unstable material, unstable structures, or numerical instabilities.
Unstable Material
Most nonlinear material models, especially those employing hyperelastic materials, have their own applicable ranges. When a deformation is too large or a stress state exceeds the applicable range, the material may become unstable. The instability can manifest itself as a mesh distortion, but nonlinear adaptive region cannot help in such cases. While it is sometimes difficult to determine when material is unstable, you can check the strain values, stress states, and convergence patterns. A sudden convergence difficulty could mean that material is no longer stable. The program also issues a warning at the beginning of the solution indicating when hyperelastic material could be unstable, although such a warning is very preliminary and applies only to cases involving simple stress states.
Unstable Structures
For some geometries and loads, a deformation may cause a "snap-through," or local buckling. Such behavior can also manifest itself as a mesh distortion, but one that nonlinear adaptive region cannot repair. The effect is usually easy to detect by closely checking the deformed region or the load-versus- time (displacement) curve.
Numerical Instabilities
A condition of numerical instability can occur when a problem is nearly overconstrained. The constraints can include kinematic constraints such as applied displacements, couplings, and constraint equations, and volumetric constraints introduced by fully incompressible material in mixed u-P elements. In many cases, numerical instability is apparent even in the early stages of an analysis.