Geometry abstraction, polygon geometry, and convergent geometry > Polygon geometry and abstraction

Understanding CAD issues reported during FEM creation

This software uses the Parasolid modeling kernel for its geometric data. When you work with CAD geometry, you work with bodies, faces, and edges. Internally, the bodies, faces, and edges are represented by series of mathematical equations. When you create a shaded display of your model, Parasolid generates facets (triangles) from those equations so you can visualize the model.

CAD geometry may contain issues

When you create a FEM file, the software uses the facets from the CAD geometry faces to create the polygon geometry that is used in a FEM file in Pre/Post. However, in some cases, there may be issues with the CAD geometry's facet data. Problems with the CAD facet data can occur for a variety of reasons. For example:

They can occur when you import geometry you created in a different CAD system. In these cases, the software may introduce local tolerances to account for misaligned geometry.
They can occur from CAD operations, such Sew or variable radius blends, that approximate the input geometry with “tolerant” edges. While “precise” edges lie between two adjacent faces within the floating-point tolerance (0.00001 mm), tolerant edges typically have tolerances between 0.01 and 0.001 mm. For more information on tolerant edges, see How edges are represented in a solid model, Continuity in NX, and Modeling tolerance values.

CAE operations, however, have different requirements for facet data than Modeling operations. Specifically:

A model must be fully stitched or “watertight” (have no free edges, no internal cracks, and no voids) for you to generate a mesh. Although a CAD model may appear to be fully stitched when you visually inspect the model, there may still be issues at the facet-level that result in free edges.
All edges must be precise edges for CAE analysis. Tolerant edges are not valid for CAE operations.

Note:

You can use the Examine Geometry command in Modeling (on the Analysis menu) to identify issues with the CAD geometry before you create a FEM file.

For more information, see Examine Geometry dialog box and Solid Analysis Errors.

When you create a FEM file, the software tries to create polygon geometry that meets the requirements of a CAE analysis. As it creates the polygon geometry, the software evaluates the quality and consistency of the CAD facet data. When the software encounters problems with the facet data, it reports the issues to the syslog files and may ignore the associated faces. Once it has generated the polygon geometry, the software tries to repair any gaps or voids caused by ignoring the problem faces. During the repair process, the software tries to:

Stitch together any free edges by replacing or collapsing curves.
Fill any void areas with facets based on the maximum area plane. The software uses the color blue to indicate these areas.
Resolve consistency issues between facets, facet points, and the edge-face topology.

The goal of the repair process is to create a fully stitched model. However, the software is not always able to automatically repair the polygon geometry.

Note:

The software does not perform any geometry abstraction when it creates the polygon geometry from the CAD geometry.

Reported CAD issues should be investigated

Although the software resolves as many of the CAD issues as it can when it creates the FEM file, you should investigate any CAD issues reported in the syslog, particularly if you plan further design iterations. For example, CAD issues can prevent you from generating a tetrahedral mesh on your part. Even if you can generate a mesh on your part, CAD issues can prevent the polygon geometry and/or the mesh from successfully updating when later geometry changes occur.

Summary of commonly reported CAD issues

Error Message	Explanation
“CAD face produces an open loop.”	The outer boundary of the CAD face is not closed. This error message is usually issued when the software is unable to close the loop.
“CAD face has faceting issues.”	There are two scenarios in which the software generates this message:The CAD face is comprised of overlapping facets or contains a facet edge that is shared by more than two facets.The CAD face contains a facet point that does not belong to the face.
“CAD face has ambiguities creating loop.”	The software cannot determine the outer boundary of the CAD face.
“CAD face loop has self intersection”	The outer boundary of the CAD face contains a region in which the boundary crosses over upon itself.
“CAD face is degenerate (2A/P<tol).”	The CAD face is very thin and narrow, like a sliver or a spike. This occurs on faces where 2* the area of the face divided by its perimeter is less than the software's internal facet body tolerance. The facet body tolerance is set to a heuristically determined value. You cannot modify the facet body tolerance.Note: In most cases, you can safely ignore this message.

Identifying the location of CAD issues in Modeling

In the syslog, the software lists the following information for each identified CAD issue:

The internal and Parasolid IDs for the CAD face and associated facet.
The X, Y, Z coordinates where the issue occurs.

To view the syslog, select Log File from the Help menu.

Once you have the coordinates where the issue occurs, you can use the Point command in Modeling to create a point at that X, Y, Z location. This helps you locate the problem area so you can inspect it more closely. You can also use options in the Examine Geometry dialog box (available from the Analysis menu) in Modeling to locate tiny (sliver or spike) faces. See Examine Geometry options and Solid Analysis Errors for more information.

Strategies for repairing reported CAD issues

The strategy you should choose to repair reported CAD issues depends upon whether you need your FEM file to update in the event of a later geometry change.

If you need your FEM file to update with geometry changes, such as when you are performing a series of parametric studies, you should correct the CAD issues on the original CAD geometry itself. See Repairing reported CAD issues in Modeling for more information.
If you do not need your FEM file to update to account for geometry changes, you can correct any issues on the polygon geometry itself. For example:If your model contains free edges, you can use the Stitch Edge command to stitch selected edges together. See Stitching edges for more information.If your model contains voids, you can use the Face Repair command to create new polygon faces to fill those voids. See Creating faces from existing boundaries for more information.

Repairing reported CAD issues in Modeling

In Modeling, you can use the full complement of CAD creation and modification commands to repair any identified CAD issues. While there are many ways to repair CAD issues, the following workflow provides one possible method for repairing a CAD issue.

Switch to Modeling.
Create points at the X, Y, Z locations reported in the syslog. Note: You can also use the Examine Geometry command on the Analysis menu to gather further data about the CAD issue.
Carefully inspect the region of the model where the CAD issue occurs.
Use the Extract command (available from the Insert→Associative Copy menu) to extract the problem face and neighboring faces into their own sheet body. See Extract Geometry for more information.
In the new sheet body, use the appropriate Modeling commands to repair the problem. For example, you can remove the problem face and then recreate it.
Once you are satisfied that you have a good representation of the geometry, you can use the Patch (available from the Insert→Combine Bodies menu) command to overlay the repaired geometry in the sheet body over the problem geometry in the original solid body. See Patch for more information.
Return to Pre/Post and display the FEM file. The software automatically uses the modified CAD geometry to update the polygon geometry in the FEM file.

Learn more

Geometry abstraction and polygon geometry

Polygon geometry

Polygon geometry versus lightweight facet bodies

How edges are represented in a solid model

Modeling tolerance values

Comparing geometry idealization and geometry abstraction

Understanding the geometry abstraction process

Displaying suppressed edges in polygon geometry

Checking CAE model consistency

Naming of polygon bodies, meshes, and properties

Tools for identifying and repairing polygon body problems

Synchronizing polygon body names and attributes to the CAD geometry

Controlling polygon body tessellation

Polygon body update process

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area