Geometry Power Tools`

The geometry power tools, shown in Fig. 1. are located on the Tree View window under the blue geometry tab. The Geometry Power Tool provides several diagnostic tests to identify and repair problems in your CAD model prior to meshing including.

Fig. 1. Geometry Power Tools

Diagnostic tests include:

Small Features: Small curves and surfaces and volumes.
Bad Angles: Near tangent angles at curves and vertices.
Geometric Traits: Identifies common geometric traits such as holes, blends, chamfers, etc.
Assembly Checks: Gaps, overlaps and misalignments between multiple parts.
Tetmesh Poor Quality Predictions: Machine learning tool to predict poor quality tet mesh.
Part Classification: Machine learning tool to classify parts into common mechanisms.

This tool analyzes geometry for various characteristics that may affect meshing outcomes and aid in simplification and defeaturing. It also contains a powerful toolkit of geometry modification methods to fix these problems. Many of the common geometry clean-up tools are available from this tool without the need to search through the command panels for relevant operations.

The geometry power tool includes a window that lists results from geometry analysis in a tree format. In addition, a solution window can be displayed that will display specific suggested geometry solutions for the currently selected entity.

Suggested Usage

The following is a suggested workflow for using the geometry power tool:

Enter volumes to analyze: Enter or pick the volume IDs you wish to analyze in the field labeled Volume ID(s). By default, all volumes will be analyzed. For large or complex assemblies, consider selecting only a few volumes at a time to avoid long analysis times.
Enter a small curve threshold: The value entered in the field labeled Small Curve Threshold defines the basis for what is considered "small" for most geometry tests. If Cubit already has more than one volume defined, a default value for small curve threshold will be computed as 0.25*mesh_size. To update the default small curve threshold for the current volumes, select the Auto button. If no mesh size is currently defined, an autosize factor of 2.5 will be used to compute a mesh size. (Equivalent to vol all size auto factor 2.5).
Select diagnostics to perform: Selecting the Options... button will display a list of available diagnostics grouped by category, as shown in Fig. 2. By default all diagnostics are selected. Some diagnostics may not apply to specific geometry, or may only need to be run once per geometry. To avoid long analysis times, select only diagnostics that are relevant for your current problem scope. Clicking on the box by each test will select or deselect it. Categories of diagnostics may also be selected or deselected in a similar manner. All diagnostics may be selected or deseleted using the Select All and Select None buttons at the bottom of the panel. Threshold values used for some of the diagnostics can also be entered, including bad angle, chamfer thickness, blend or hole radius, cavity area and volume gap thresholds. Details on each of the diagnostics are described below. Select the Done button to return to the main Geometry power tool panel.
Analyze the geometry: Click the Analyze button to initiate an analysis of the selected diagnostics. The time taken for analysis will vary based on the number and complexity of volumes and the diagnostics selected.
Select an entity to examine: Once analysis is complete, the results will appear in the main window of the geometry power tool panel in the form of an expandable lists categorized by the selected diagnostics. Items in the list correspond to the selected tests. Expanding a list will display an ordered sub-list of geometry entities that have been identified by the test. Selecting one or more entities in one of the lists will also highlight the entities in the graphics window. Use shift-click or command/ctrl-click to select multiple entities in the list. Use the context menu (right click) to zoom or fly in, locate, draw or other methods to graphically examine the selected entities.
Choose a geometry repair solution: Multiple methods are provided for choosing and selecting a relevant geometry repair solution:
- Context Menu: Right clicking on an entity in the list will reveal a list of options that are normally relevant for the selected entity type. (See Fig. 3.) For example, selecting the Remove Surface... menu item will bring up the Remove Surface command panel pre-populated with the relevant entity. To execute the same operation on many entities at once, first select all relevant entities in the list.
- Show Solutions: Selecting the Show Solutions check box at the top of the results window will display an additional window, (See Fig. 4.) populated with relevant operations for the currently selected entity. Selecting a solution will display a preview of the operation in the graphics window. Double clicking the solution will execute the solution. A right click on the solution will show a context menu revealing the following options:
  - Execute: Execute the selected solution (same as double click).
  - Show More Solutions: Add additional solutions computed for attached entities if they exist. For example, if a small curve is selected, this option will include additional solutions in the window for its attached surfaces and vertices.
  - Open Command Panel Operation: Depending on the type of solution selected, the relevant command panel will appear pre-populated with the options called for in the solution. This provides the option to further customize the solution if the precise desired command is not displayed.
- Command Panel Buttons: The buttons at the bottom of the geometry power tool will display a specific geometry command panel. This can be useful if many similar operations are to be performed on different entities. A description of each is provided below.


Fig. 3. Geometry entity context menu in power tool	Fig. 4. Entitiy-specific solutions displayed in geometry power tool

Geometry Analysis Tools

The geometry power tools contain an array of tests that can be run on geometry to diagnose potential problems for mesh generation. To display a list of tests, click on the Show Options check box. By default all tests are selected and run on geometry. Some tests may not apply to specific geometry, or may only need to be run once per geometry (i.e. bad geometry definition test). Clicking on the box by each test will deselect it. The geometry analysis inputs and tests are summarized below:

Small Features.

Small features may be necessary and desirable in a model, but many times they are the result of poor geometry construction, or they may just not be important to the analysis. The small features tests look for small curves, small surfaces, and small volumes. These tests rely on the user-defined small curve threshold value defined at the top of the Geometry poert tool.

Small Curves - Small curves, including zero-length curves such as hardpoints, are compared directly against the small curve threshold value, and identified if they are less than or equal to the given value.
Small Surfaces - Small surfaces are identified based on area and hydraulic radius. Surface areas that are less than the square of the current mesh_size are identified as small. For surfaces where the hydraulic radius, defined as 4*surface_area/perimeter, is less than the small curve threshold are also identified as small.
Small Volumes - Small volumes are identified by their hydraulic radius, defined as 6*volume/surface_area.

Bad Angles

Small geometric angles at vertices and curves can sometimes over-constrain the resulting mesh resulting in poor element quality. These tests are controlled by the Bad Angle threshold value defined at the top of the Geometry power tool Options panel.

At Vertices - For vertices, the angle formed by two attached curves is measured. Vertices where angles less than the Bad Angle threshold. Fig. 5 shows an example of a bad angle where the resulting tet or hex mesh may result in poor mesh quality. Note that depending on how the angle is measured at the vertex, the small angle may be also be identified if 360. 0-angle is less than the Bad Angle threshold. The blunt tangency or collapse angle operations are useful for removing bad angles at curves.

Fig. 5. Bad Angle at Vertex Example

At Curves - For curves, the angle formed by two attached surfaces is measured. Similar to vertices, curves where angles less than the Bad Angle threshold are identified.
Tangential Intersections - A tangential intersection is formed when two parallel surfaces share an edge and have a 180 degree angle between them. The tangential intersection test is looking for the condition where two surfaces that meet tangentially share a common edge, and each of the surfaces has another edge which resides on a third face and forms a small angle. In the example shown in Fig. 6., Surface 1 and Surface 2 are tangential to each other and share a common edge. Both Surface 1 and 2 have another edge which resides on Surface 3 and forms a small angle at the vertex common to all three surfaces.

Fig. 6. Tangential Intersection Example

Traits

The tests in the Traits category, group entities according to a specific characteristic of the geometry such as its thickness or radius. Use the threshold values at the top of the Geometry power tools Options panel to set limits on values used to control entities returned from these tests. Geometry Traits include the following:

Close Loops - Close loops are identified by two curves on a single surface for which the shortest distance between them is less than the current mesh_size. Surfaces identified as close loops are ordered based on the minimum thickness of the surface between the loops. These surfaces and their immediate neighbors are often candidates for the remove surface command.

Fig. 7. Close Loop Example

Chamfer Chains - A chamfer surface can be identified as a narrow strip where its angle to neighboring surfaces is about 45 degrees as shown in Fig. 7. Chamfers often occur as a chain or connected set of surfaces and are grouped together in the power tool as a collection of surfaces that can be expanded and examined individually. Chamfer chains are ordered based on the narrow thickness of the surfaces illustrated in Fig. 8. Setting the Chamfer Thickness threshold in the Options panel will control which chamfer chains will be identified. The default value for Chamfer Thickness threshold is the current mesh_size Since chamfers with small thickness can effect the resulting size of the elements the remove surface option is often used to eliminate them.

Fig. 8. Chamfer Examples

Blend Chains - A blend surface serves as a smooth transition between two neighboring surfaces, such as a fillet as shown in Fig. 8. Blends are identified as surfaces having a constant radius along one of its parametric directions. Blends often occur as a chain or connected set of surfaces and are displayed as a collection of surfaces in the power tool that can be expanded and examined individually. Enter a Blend Radius threshold value at the top of Geometry power tools options panel to control the maximum radius of curvature for surfaces returned from this test. The default value for Blend Radius threshold is the current mesh_size. Resulting blend surfaces are ordered based upon their minimum radius of curvature. Blend chains can be candidates for the remove surface blend_chain or split surface commands.

Fig. 9. Blend Examples

Holes - Holes are a special category of Cavity (see below). They are collections of surfaces that are bounded by curves where the exterior angle is greater than 180 degrees and at least one of the surfaces have a radius of curvature less than the Hole Radius threshold. Figure 10 illustrates a hole that is comprised of a cylindrical surface and a planar circular surface. Resulting hole collections of surfaces are ordered based upon their cylindrical radius. Holes can be candidates for the remove surface cavity command.

Fig. 10. Hole Example

Cavities - Small cavities in a volume may be candidates for removal from the geometry. A cavity is defined as a collection of surfaces bounded by curves with an external angle greater than 180 degrees. Enter the Cavity Area threshold value at the top of the Geometry power tools Options panel. This value controls the maximum total surface area for a cavity identified from this diagnostic test. Since cavities may consist of many individual surfaces, the resulting ordered list displayed in the power tool includes sub-lists of surfaces that can be expanded and examined individually. Surfaces contained with cavities or holes can be candidates for the remove surface cavity command which will remove all surfaces in the cavity sumiluatneously.

Fig. 11. Cavity Example

Cone Surfaces- Cones are defined as any surface comprising exactly two curves where one of the curves is of zero length. Cone surfaces can often cause difficulty for surface meshing, and should be removed when possible. Surfaces identified as cones are ordered based on their surface area. Cone surfaces are good candidates for the tweak surface cone command.

Fig. 12. Cone Example

Bad Geometry Definition - Cubit uses third party libraries, such as ACIS from Spatial, Inc. for much of its geometric modeling capabilities. The bad geometry definition check calls internal validation routines in these libraries, when available, to check for errors in geometry definition. Entities indetified as "bad geometry" are usually candidates for the heal volume command. If the third party library does not provide validation capabilities, this check will not return anything. Note: ACIS is a trademark of Spatial.

Assembly Checks

Check the interactions between multiple volumes. Here we check for overlaps, gaps and misalignments between nearby volumes. It will also identify volumes that are in contact as well as entities that are ready for merging.

For assemblies of volumes, it is important to identify if volumes will be connected (imprinted and merged) are in contact, or separated by some distance. The Assembly Checks provide diagnostics and solutions to validate and resolve these interactions.

The Gaps, Overlaps and Misalignments diagnostics normally identify undesirable conditions that must be resolved prior to imprint and merge. Once resolved, the Volume Contacts and Mergable Geometry can be used to validate connections before and after imprinting and merging.

The Options panel also provides a way to estimate or manually set an imprint tolerance. Entities closer than this tolerance will be considered mergable when used with the tolerant imprint command. When the Tolerant Imprint checkbox is selected in the Options panel, the diagnostic tests that identify gaps, overlaps and misalignments will also use the specified tolerance when computing issues.

Volume Gaps - Lists volume pairs that are separated by a distance smaller than the Volume Gap tolerance specified in the Options panel, but are not in contact or overlapping. Gaps can result in parts that are not correctly merged and will not share nodes between volumes when meshed. Expanding a volume pair in the list will display individual surface pairs where gaps exist between the volumes. Fig. 13 illustrates a gap between two volumes. Gaps can be visualized using the Draw Volume Gap context menu, also shown in Fig. 13, where the surfaces that are within the gap tolerance are displayed in red. The tweak surface replace command can sometimes be used to correct overlaps.

Fig. 13. Volume Gap Example

Volume Overlaps - Lists volume pairs that are overlapping. Fig. 14. shows an example of a volume overlap. Overlapping volumes can result in sliver surfaces and bad element quality if they are not resolved prior to imprinting and merging. Overlaps can be displayed with the context menu item, Draw Volume Overlap which displays the overlap region in red. The remove overlap command or tweak surface replace commands can often be used to correct overlaps.

Fig. 14. Volume Overlap Example

Volume Misalignments - Misalignments are caused when neighboring volumes touch without overlap, but a small distance between neighboring vertices, curves or surfaces is identified. Fig. 15 shows an example of a misalignment. Misalignments can result in sliver surfaces and bad element quality if not resolved prior to imprinting and merging. The Volume Misalignments diagnostic test will list pairs of volumes that are misaligned. Expanding a volume pair will reveal entity to entity misalignments that were detected between the pair. Three categories of misalignments will be displayed, namely: vertex-vertex, vertex-curve and vertex-surface ordered by their misalignment distance. These indicate entity pairs that are closer than the Volume Gap tolerance that is set in the Options panel. The tweak surface replace command can often be used to correct misalignments.

Fig. 15. Volume Misalignment Example

Volume Contacts - Volumes that have surfaces in contact but not merged are displayed with this diagnostic test. This provides a way to distinguish volumes that are merged from those that are not and validate whether a contact state should exist between neighboring volumes. This list will include volume pairs that are touching including those that have been identified by the Volume Misalignment diagnostic test. Expanding a volume pair will reveal pairs of surfaces on different volumes that are in contact. If the contact state is not correct, normally an imprint and merge operation should be performed.
Mergable Geometry - Pairs of entities on neighboring volumes that are co-located are identified by this diagnostic test. This is normally used to verify that the expected set of surfaces are coincident prior to merging. Mergeable geometry pairs of surfaces, curves and vertices are displayed in this list. Lower order entities (ie. curves and vertices) will not be displayed if its parent geometry (ie. surface) is identified as mergeable. In most cases, lower order entities identified by this diagnostic indicate the existence of overlaps or misalignments and should be resolved before imprint and merging. Note that the default merge tolerance of 1e-6 is used to determine if entities are mergeable unless the Tolerant Imprint checkbox is selected in the Options panel and a user defined tolerance is set.

Geometry Repair Tools

The geometry repair tool buttons appear at the bottom of the Geometry Power Tool. Selecting one of these buttons will bring up the relevant command panel. Tools included in this panel have proven useful for geometry repair and defeaturing.

Split Surface Button

The split surface tool is used to split a surface into two surfaces. This is useful for blend surfaces, for example, where splitting a surface may facilitate sweeping. To select a surface for splitting, click on the surface in the tree view. To select multiple surfaces in the window, hold the CTRL key* while selecting surfaces (surfaces must be attached to each other). Then press the split surface button to bring up the Control Panel window with the ids of selected surfaces in the text input window. The split surface menu is located on the Control Panel under Geometry-Surface-Modify. You must press the Apply button for the command to be executed. You can also bring up the Split Surface menu by selecting surfaces in the tree view and selecting Split from the right click menu.

*Note: For Mac computers, use the command key (or apple key) to select multiple entities.

Heal Geometry Button

The healing function in CAE Fidesys is used to improve ACIS geometry that has been corrupted during file import due to differences in tolerances, or inherent limitations in the parent system. These errors may include: geometric errors in entities, gaps between entities, and the absence of connectivity information (topology). To heal a volume, select the volume in the geometry repair tree view. Then press the heal button. You may also press the heal button without a geometry selected in the window, and enter it later. The Control Panel window will come up under the Geometry-Volume-Modify option with the selected volume id highlighted. If no entity is selected, or if another entity type is selected, the input window will be blank. You can also open the healing control panel by selecting Heal from the right click menu in the geometry power tools window.

Tweak Surface or Curve Button

The tweak command is used to eliminate gaps between entities or simplify geometry. The tweaking commands modify geometry by offsetting, replacing, or removing surfaces, and extending attached surfaces to fill in the gaps. Tweaking can be applied to surfaces, and it can be applied to curves with a valence no more than 2 at each vertex. It can also be applied to some vertices. To tweak a surface, select the surface in the tree view. The Geometry-Surface-Modify control panel will appear with the selected surface id in the input window.

Tweaking is available for curves. Tweaking a curve creates a blended or chamfered edge between two orthogonal surfaces. The curve option is located on the Geometry-Curve-Modify panel under the Blend/Chamfer pull-down option.

Tweaking is also available for some vertices. Tweaking a vertex creates a chamfered or filleted corner between three orthogonal surfaces. The vertex option is located on the Geometry-Vertex-Modify panel under the Tweak pull-down menu.

Note: Only curves with valence 2 or less at each vertex are candidates for tweaking. Any other curve will cause the Geometry-Surface-Modify menu to appear.

Merge All Mergeable Entities Button

The merge command is used to merge coincident surfaces, curves, and vertices into a single entity to ensure that mesh topology is identical at intersections. Unlike other buttons on the geometry repair panel, the merge button acts as an "Apply" button itself. All geometry that is listed under "mergeable entities" will be merged.

Remove Entity Button

The remove button is used to simplify geometry by removing unnecessary features. To use the remove feature, click on the surface(s) in the Tree View. Right click and select the Remove Option, or click the Remove icon on the toolbar. The Control Geometry-Surface-Modify control panel will appear, with the surface ids in the input window. The Remove control panel can also be accessed from the right-click menu in the Geometry Power Tools window. Select options and press apply.

Regularize Entity Button

The regularize button is used to remove unnecessary topology. Regularizing an entity will essentially undo an imprint command.

Remove Slivers

The remove slivers button is used to remove surfaces with less than a specified surface area. When ACIS removes a surface it extends the adjoining surfaces to fill the gap. If it is not possible to extend the surfaces or if the geometry is bad the command will fail.

Auto Clean Geometry

The auto clean button is used to perform automatic cleanup operations on selected geometry. These automatic cleanup operations include forcing sweepable configurations, automatically removing small curves, automatically removing small surfaces, and automatically splitting surfaces.

Composite Button

The composite button is used to combine adjacent surfaces or curves together using virtual geometry . Virtual geometry is a geometry module built on top of the ACIS representation. Surfaces may be composited to simplify geometry in order to facilitate sweeping and mapping algorithms by removing constraints on node placement. It is important to note that solid model operations such as webcut, imprint, or booleans, cannot be applied to models that have virtual geometry. Both curves and surfaces may be composited.

Collapse Angle Button

The collapse angle button uses virtual geometry to collapse small angles. This is accomplished by partitioning and compositing surfaces in a way so that the small angle gets merged into a larger angle. Pressing the collapse button on the geometry power tools will open the collapse menu under Geometry-Vertex-Modify control panel. This panel can also be opened by selecting Collapse from the right click menu in the Geometry Tools window.

Collapse Surface Button

Pressing this button will open the collapse surface panel on the main control panel. The collapse surface function uses virtual geometry to eliminate small surfaces on the model to improve mesh quality. It is most useful for blend surfaces.

Collapse Curve Button

Pressing this button will open the collapse curve panel on the main control panel. The collapse curve command is used to eliminate small curves using virtual geometry.

Reset the Display Button

The reset graphics button will refresh the graphics window display.

Note: Pressing most of the geometry tool buttons on the panel will only bring up applicable command panels on the Control Panel. You must press the Apply button on the Control Panel to execute the command.

Context (Right Click Menu)

The following right click menu is available from the geometry power tools. Specific options depend on the type of entity selected.

Zoom To - Zoom to selected entity in the graphics window.
Reset Zoom - Reset graphics window zoom.
Fly-in - Animated zoom.
Locate - Labels the selected entities in the graphics window. Refresh screen to hide.
Draw - Displays only selected entities by themselves.
Draw Add - Adds the selected entity to the display without clearing .
Draw with Neighbors - Displays only selected entities with all attached neighbors.
Select Similar ... - Selects other entities in the same category that have the same geometry characteristic. For example, area, loop thickness, blend radius, angle at vertex, etc.
Clear Blend Chain - Available in Blend category. Selects surfaces in the same blend chain as the selected surface.
Clear Cavity/Hole - Available in Cavity/Hole category. Selects surfaces in the same cavity or hole collection as the selected surface.

Solution Options

Each of the following menu options are available based on the category and entity type selected. In each case they will open the relevant command panel pre-populated with the entity selected. Select multiple entities prior to selecting the context menu item below to execute the command on multiple entities simulaneously.