Polygon geometry

When you create a FEM file, if you select the Associate to Master Part option in the New FEM dialog box, the software automatically creates polygon geometry from the geometry in your CAD model. The polygon geometry is a faceted representation of the geometry in the master part. Polygon geometry allows you to:

• Tailor the geometry to fit the needs of your CAE analysis without modifying the CAD part. This means you can make changes to the polygon geometry even though you may not own the CAD part.

• Repair issues with the CAD geometry, such as eliminate narrow regions, that can prevent the software from meshing or solving your model.

Note:

Working with polygon geometry in the FEM file is different from working with the idealized part. For more information, see Comparing geometry idealization and geometry abstraction.

Understanding faceting and polygon geometry creation

When the software creates the polygon geometry, it tessellates the CAD geometry with triangular facets. This tessellation occurs on the precise CAD geometry. In general, the polygon geometry is initially a one-for-one representation of the CAD geometry. That is, for every body, face, and edge in your CAD geometry, the software creates a corresponding polygon body, polygon face, and polygon edge in the FEM file. Specifically:

• Every facet point in the polygon model is located on the precise CAD geometry.

• At each facet point, the software also extracts the surface normal from the precise CAD geometry. These surface normals are part of the polygon geometry even though they are not displayed in the graphics window.

• At each edge, the software stores multiple normals to represent multiple, connected faces.

When you generate a mesh, these facet points and surface normals allow the software to infer node locations on the polygon geometry. Specifically, the software infers curved facets if the normals at the facet points show that the precise CAD geometry is not planar. The software uses this information to locate the nodes in the surface mesh so that the actual chordal faceting tolerance is not an issue during mesh generation.

In some cases with particularly complex geometry, the software may be unable to generate a complete, faceted representation of the CAD geometry. This can occur when the software encounters certain types of pathological issues in the CAD geometry, such as data inconsistencies or problems with the tessellation. In those cases, the resulting polygon geometry may contain missing faces. When this occurs, you can use the Face Repair command in the Polygon Geometry group to construct a new face. You can also check the syslog (select Help→Log File), which lists the coordinates of the geometry regions that contain such data inconsistencies.

Situations in which the software cannot infer the original CAD surfaces during meshing

In some cases, the software is unable to infer node locations on the polygon geometry and instead creates the node locations on the facets themselves. This causes the mesh to follow the facets and not the original CAD geometry. This typically occurs in regions of the model:

• That originally contained CAD surfaces that the software could not tessellate.

• Where the software abstracted the CAD geometry to eliminate problematic geometry, such as collapsing edges or the automatic insertion of seams along cylinders to facilitate meshing. For more information about the geometry abstraction process, see Understanding the geometry abstraction process.

• Where you have made significant modifications to the polygon geometry, such as those which result from the use of mesh mating conditions (particularly on curved geometry), or in areas where you have used any of the manual abstraction commands in the Polygon Geometry group.

• Where the software has made modifications to the polygon geometry, such as the automatic insertion of seams along cylindrical surfaces to facilitate meshing.

Note:

When you create a mesh on your FEM, the software does not access the original CAD geometry. The mesh is created only on the polygon geometry.

Repairing areas in which the mesh follows the facets

If your model contains regions in which node locations deviate significantly from the underlying CAD geometry, you can use the Node Proximity to CAD Geometry option in the Model Check dialog box to move those nodes. The Node Proximity to CAD Geometry option lets you both evaluate the proximity of nodes to the underlying CAD geometry and then adjust the location of any nodes the software identifies as lying outside the specified Proximity Tolerance.

Note:

You must have the idealized part loaded to use the Node Proximity to CAD Geometry option.

For more information, see Controlling the proximity of nodes to the CAD Geometry.

Controlling the default naming of polygon bodies

You can use a Customer Default to control whether the software uses the names of existing assembly components to name the related polygon bodies.

• If you select this default, the software uses the assembly component's name as the root name for the associated polygon bodies.

• If you do not select this default, the software uses the root name POLYGON BODY for all polygon bodies.

Although you can always later rename polygon bodies with more descriptive strings, you can use the default to give the bodies more meaningful default names.

To access this option:

1. Choose File→Utilities→Customer Defaults.

2. In the Customer Defaults dialog box, select Simulation→Pre/Post→General.

3. On the FE Model Create tab, either select or clear the Assign Assembly Component Names for Polygon Bodies check box.

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Related Topics

Generating surface wrap bodies and meshes

Polygon geometry, 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 } });