Nonlinear Adaptive Region

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.

Requirements

The Nonlinear Adaptive Region condition requires the following settings.

Preprocessing Support Limitations

Note the following limitations for this condition.

Post Processing Support Limitations

Because this condition causes mesh changes during the course of the solution process, there are result scoping limitations.

Analysis Types

Nonlinear Adaptive Region is available for Static Structural analyses.

Common Characteristics

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

Geometry Types: Geometry types supported for the Nonlinear Adaptive Region condition include:

Topology: The following topology selection options are supported for Nonlinear Adaptive Region.

Condition Application

To apply a Nonlinear Adaptive Region:

  1. 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.

  2. 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.


  3. Specify the Criterion: options include Energy, Box, and Mesh.

    If Energy...If Box...If Mesh...

    Define an Energy Coefficient value. The Energy Coefficient must be non-negative. Default numeric value is 1.

    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.

    • Coordinate System (default is Global Coordinate System)

      If you select a local coordinate system, it must be a Cartesian coordinate system and may not include rotation angles.

    • Length X

    • Length Y

    • Length Z (for 3D)

    The Box option defines a region on the model

    Nonlinear Adaptivity Controls become available in the Analysis Settings.

    The Mesh Criterion is recommended.

    For 3D Analyses

    Define a Skewness Value for the mesh elements. The value must be between 0 (equilateral) and 1 (degenerate). A larger value reduces the chance of a remesh to take place. The default value is 0.9.

    For 2D Analyses

    Specify a Maximum Corner Angle for the mesh elements. The value must be between 0° - 180°. The default setting is 160°.

  4. Specify the Check At property as either Equally Spaced Points or Specified Recurrence Rate.

  5. Enter the Value property based on the Check At property selection. This value must be an integer. Default integer value is 1.

  6. Specify the Time Range property as Entire Load Step or Manual. 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.

  7. When the condition is defined, the Graph and Tabular Data windows provide a right-mouse click option to Deactivate (or Activate) 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.


Details View Properties

The selections available in the Details view are described below.

CategoryFields/Options/Description
Scope

Scoping Method, options include:

  • Geometry Selection: Default setting, indicating that the condition is applied to a geometry or geometries, which are chosen using a graphical selection tools.

    • Geometry: Visible when the Scoping Method property is set to Geometry Selection. Displays the type of geometry (Body) and the number of geometric entities (1 Body, 2 Bodies) to which the condition has been applied using the selection tools.

  • Named Selection: Indicates that the geometry selection is defined by a Named Selection.

    • Named Selection: Visible when the Scoping Method property is set to Named Selection. This field provides a drop-down list of available user–defined element-based (only) Named Selections.

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 Energy, Box, or Mesh.

Energy

If Energy is selected, you need to enter an Energy Coefficient.

Energy Coefficient: This criterion checks the strain energy of any element that is part of the defined component using the following calculation. A component is defined as the assembly of all scoped elements.

where:

  • Ee = strain energy of single target element.

  • c1 = user input energy coefficient.

  • Etotal = total strain energy of the component.

  • NUME = number of elements of the component.

If this criterion is satisfied at an element, the program refines the element. A smaller Energy Coefficient improves the potential to trigger the mesh regeneration for the same loads.

Box

If Box is selected, the following additional properties require entries:

  • Coordinate System (default is Global Coordinate System): defines the minimum values of the box.

  • Length X: defines the diagonal length on global X axis.

  • Length Y: defines the diagonal length on global Y axis.

  • Length Z (for 3D): defines the diagonal length on global Z axis

Mesh

If Mesh is selected, the Options property displays and based on your analysis, whether it is 3D or 2D, the option is read-only and either Skewness (3D only) or Shape (2D only).

For 3D analyses, you need to enter a Skewness Value for the mesh elements. The element skewness is defined as:

Skewness = (Vreg - Vel) / Vreg

Where:

Vel is the volume of the element under calculation and Vreg is the volume of the standard tetrahedral linear element located in the same sphere as the element under calculation. When the element under calculation has an ideal shape (that of a standard tetrahedral element), Vreg = Vel and Skewness Value = 0.

When the element under calculation has the least ideal shape (that of a flat element), Vel = 0 and Skewness Value = 1.

Therefore, for the linear tetrahedral element, Skewness Value is always between 0 and 1, with 1 being a flat element. The default value is 0.9. The recommended Skewness Value is approximately 0.85 to 0.9.

For 2D analyses, the Shape setting also includes the Maximum Corner Angle property. The entry range for this property is 0° - 180°. The default setting of 160° is recommended. An element is remeshed when any of its corner angles reach the specified value.

Check At: options included Equally Spaced Points or Specified Recurrence Rate.

Value: This property further defines the Check At property. The default value is 1.

Time Range: options included Entire Load Step or Manual. When specified as Manual, you need to enter a Start Time and End Time. The End Time value must be larger than the Start Time value.

Suppressed: Include (No - default) or exclude (Yes) the condition.

View Changed Mesh Results

Following the solution process, to determine if the mesh was changed:

Mechanical APDL References and Notes

The following Mechanical APDL commands, element types, and considerations are applicable for this condition.

Nonlinear Adaptive Region Solving Limitations

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.


Release 18.2 - © ANSYS, Inc. All rights reserved.