Adaptive meshing

Adaptive meshing is an iterative solution process that you can use to improve the quality of a mesh by selectively refining the mesh in areas in which selected error values, such as strain energy, are highest. Adaptive meshing helps you to produce a mesh that is sufficiently detailed in the appropriate areas, such as in regions where higher stress concentrations occur, while controlling the overall cost of the analysis.

You can use the Adaptivity solution process to do the following:

• Specify accuracy parameters to identify regions within the existing mesh that have high error values.

• Iteratively refine the mesh in those regions to reduce the error values.

Adaptivity requires an existing solution

You create an Adaptivity solution process within the context of an existing solution. Only certain solvers and solution types support adaptive meshing. For more information, see Supported solution types for adaptive meshing.

Before each iteration, the software solves the model using the current mesh. It uses these results to determine the areas of the mesh that need to be refined.

Note:

For structural solutions, if the solution on which you define the Adaptivity process has existing results, you can use those results as the starting point for the adaptive process. However, if you decide to use existing results, you should be sure that those results are up-to-date and appropriate for the model.

Adaptive refinement process

In each iteration during an Adaptivity solution process, the software compares the generated or existing results to the specified accuracy parameters in the Adaptivity Meta Solution dialog box. If the calculated error values are higher than the accuracy parameters you specified, the software refines the mesh based on the criteria you specified in the Mesh Parameters group of options. For more information, see Understanding the adaptive refinement process.

The software continues the process of solving the model and remeshing until it reaches the maximum number of specified iterations or until the solution converges. It determines convergence by comparing the specified accuracy parameters to the calculated error values. If the calculated values are equal to or less than the specified accuracy parameters, the software considers the solution to be converged.

Singularity detection

Singularities occur when infinite stresses prevent the solution from converging. In an Adaptivity solution process, you can have the software automatically detect and remove singularities or you can manually specify locations where you believe a singularity will occur. For more information, see Singularities in adaptive meshing.

Limiting mesh refinement

You can use the Adaptivity Zone command to create refinement or suppression zones to control the extent of the mesh refinement.

• To refine the mesh only within a specific region of the model, such as an area where you expect high stress values, create a Refinement type of adaptivity zone. For more information, see Refining specific parts of an adaptive mesh.

• To exclude a region of the mesh from refinement, such as an area where you expect low stress values, create a Suppression type of adaptivity zone. For more information, see Excluding parts of the model from adaptive meshing.

Adaptive meshing output

When the software completes the final iteration, it saves several different types of output. This output includes the following:

• The solution results, including the error listing for the final iteration only.If the solve fails during an iteration, the software asks whether you want to keep the mesh associated with the failed solve.

• The final mesh.

• A summary of the adaptive analysis that provides detailed information, including:The maximum actual value for each accuracy parameter at each iteration. The software reports a single value for the entire model for absolute errors, such as strain energy or steady stress error percentage.The total number of iterations.The total number of elements and nodes in the mesh at each iteration.Whether or not the solution converged.

• A log file that includes information about each iteration, such as the total number of elements and nodes and the computed accuracy parameters, as well as whether the model has converged. The software automatically creates this log file when you solve an adaptivity solution.

You can also select the Keep Solver Output Files for All Iterations option in the Adaptivity Meta Solution to retain copies of all solver files for each iteration. This allows you to view data about the model from each iteration.

Viewing adaptivity results in post processing

After the Adaptivity iterations are complete, you can review the results of the adaptive solution in the Post-Processing Navigator. For example, you can create contour plots of the strain energy error as well as the stress or temperature errors. You can also create contour plots of the mesh refinement level results.

For more information, see Viewing adaptive meshing results.

Adaptive meshing considerations and limitations

• You can use adaptive meshing only on meshes that are fully associated to the underlying CAD geometry. If you try to run an Adaptivity solution process on a mesh that contains manual modifications, such as nodes that you have repositioned with the Move Node command, the adaptive meshing process does not work correctly.

• You should create only geometry-based boundary conditions on models on which you intend to use adaptive meshing. During the adaptive iterations, Pre/Post deletes any boundary conditions that are defined directly on nodes or elements.

Where do I find it?

Adaptivity solution process

Application	Pre/Post
Prerequisite	A Simulation file as the displayed part and the work partSimcenter Nastran, MSC Nastran, Simcenter 3D Multiphysics, Simcenter 3D Thermal, Abaqus, or ANSYS as the specified solver
Simulation Navigator	Right-click the Simulation file→New Solution Process→Adaptivity
Menu	Insert→Adaptivity Setup

Solve an adaptivity solution

Application	Pre/Post
Prerequisite	A Simulation file as the displayed part and the work partSimcenter Nastran, MSC Nastran, Simcenter 3D Multiphysics, Simcenter 3D Thermal, Abaqus, or ANSYS as the specified solverAn existing adaptivity solution
Simulation Navigator	Right-click the adaptivity solution→Solve

Adaptivity Zone

Application	Pre/Post
Prerequisite	A Simulation file as the displayed part and the work partSimcenter Nastran, MSC Nastran, Simcenter 3D Multiphysics, Simcenter 3D Thermal, Abaqus, or ANSYS as the specified solver
Simulation Navigator	In the appropriate Adaptivity solution process node, right-click the Zones folder→New

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Adaptive meshing, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });