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Best Practice Guide for Exporting Solids from Unigraphics Using STEP

Overview

Things to do:

Try to eliminate modeling practices that led to the creation of unparamertized features. This will greatly reduce corrupt solids and will facilitate the repair of invalid geometry errors if they do occur.
Visually inspect the fully shaded Unigraphics solids to be translated. If any faces are "missing" they must be repaired or deleted from the model.
Save a copy of the part file with all of the blend features suppressed or deleted. The Unigraphics blend feature is not directly supported by STEP. The blend is approximated using B-Spline surfaces and may cause errors. If translations failures or errors occur using the original part with blends, translate the copy without blends.
Execute the File->Utilities->Part Cleanup command. The Part Cleanup option eliminates certain inaccessible objects from the part file. Specify the following clean up operations to be performed on the part:

Delete all empty groups, or all unnamed empty groups.
Turn off all object highlighting.
Delete all unused (un-referenced) objects.
Perform a clean up of Feature data.
Delete Invalid B-curves data (Not a visible option. Is preformed automatically.)

File->Utilities->Part Cleanup

Execute the Info->Analysis->Examine Geometry command. The Examine Geometry command lets you analyze solid bodies, faces, and edges for detection of corrupt data structures and geometric anomalies. The system cannot automatically correct errors, but highlights them, giving the user the "opportunity" to fix them. If a body is found to be invalid it means that further modeling operations or downstream operations (e.g., CAM and STEP) may fail. Click the Set All Checks button and Select All to fully analyze the geometry. Any errors returned in the Bodies and Faces sections must be repaired before exporting to STEP. See the Info->Analysis->Examine Geometry section below for details. The Examine Geometry options are:

Objects

Tiny
Misaligned

Bodies

Data Structures
Consistency
Face-Face Intersections
Sheet Boundaries

Faces

Smoothness
Self-Intersection
Spikes/Cuts

Edges

Smoothness
Tolerances

When translating to Catia, use a value of 0.00001 for the preprocessing (Unigraphics->STEP) Face/Edge B-spline approximation tolerance. This will be sufficient for generating STEP files to send to Catia systems whose modeling tolerance is significantly looser than the modeling tolerance used by Parasolid/Unigraphics
According to tests performed in Europe by ProSTEP, setting the Catia modeling space parameter to 2 meters will decrease errors when importing STEP files from Unigraphics and Pro/Engineer systems.
Import the STEP AP203 file back into Unigraphics for a "loop" test to be certain that the solid model data in the STEP file can be re-created in Unigraphics.

NOTE:

File -> Utilities -> Part Cleanup...

Figure 1 - Part Cleanup Option Dialog

You can specify which of the following clean up operations you would like performed on the part:

Delete all empty groups, or all unnamed empty groups.
Turn off all object highlighting.
Delete all unused (un-referenced) objects.
Perform a clean up of Feature data.
Delete Spreadsheet data
Delete Invalid B-curves data (automatic)

Delete Unused Objects

Clean Up Feature Data

Part Repaired

NOTE:

CAUTION: It is possible that during the attempt to correct mismatched data, the system will delete some individual solid objects from the part. However, the remainder of the solids and all other objects in the part are unaffected.

Deletion of Invalid B-curves

Solid Analysis

Info->Analysis->Examine Geometry

The system represents a solid or sheet body as a set of linked topological entities, such as faces, edges and vertices. The topological entities and the relationships between them define the connectivity of the body. Underlying the topological entities are geometrical entities which define the shape and location of the topological entities:

A vertex has point geometry underlying it.

An edge has curve geometry underlying it.

A face has surface geometry underlying it.

The topological structure must be consistent. e.g. the edges of a face must define closed loops and must meet at vertices.

The geometrical entities must be valid, e.g. they must not be self-intersecting. The geometry of any single face or edge must be G1 continuous (i.e. smooth).

The relationships between the geometrical entities must be consistent, e.g. a vertex must lie on the curves of the edges which meet at that vertex.

You may select as many bodies and/or faces as you like.

Data Structures

Consistency

The topological structure, to ensure that it is consistent.

The geometrical entities, to make sure they are valid and that faces and edges have G1 continuous geometry.

The geometrical entities, to ensure that they are consistent, i.e., that the point geometry of vertices lies on the edges and faces to which they are linked; that edge geometry lies in the faces to which they are linked; and that edges intersect only at vertices.

Face-Face Intersections

It is possible to inadvertently create face-face inconsistencies during modeling. For example, suppose you hollowed a cube to a thickness of 1 mm, then blended one of the outer edges to a radius of 5 mm. The inner shell then intersects the outer shell, and the model is invalid.

Face-face inconsistencies can often be remedied by further modeling operations. In the above example, the model can be made valid by blending the inner edge.

Face Smoothness

Face Self-Intersection

Info->Analysis->Examine Geometry...

Examine Geometry

The system cannot automatically correct such conditions, but it highlights them, giving you the opportunity to fix them yourself. If a body is found to be invalid it means that further modeling operations or downstream operations (e.g., CAM) may fail. It does not mean that your part file or your Unigraphics session is corrupted.

NOTE: For an analysis of the error conditions presented through this option, see the section, Solid Validity Errors, in the Error Messages chapter of the Unigraphics Modeling User Manual.

Choosing Examine Geometry displays the following dialog (Figure 1).

The Examine Geometry dialog lets you specify which tests to perform. The default is that all test options are disabled. Use the Set All Checks button to select all tests, and the Clear All Checks button to disable all tests. Once you have selected the desired tests and clicked the OK button, a dialog displays to let you select the geometry you wish to examine.

NOTE: When used with Info->Analysis->Examine Geometry, the Class Selection Select All option highlights only entities that are visible in the graphics window. If you have made Hidden Edges invisible, they will not be selected, and will not be used in the analysis.

Once you have selected the geometry, the system runs the chosen tests. After the selected tests are complete, the results are displayed in the Information window (Figure 2).

Figure 2 The Examine Geometry Dialog

Highlight Results

Figure 3 - Highlights Results Window

The Highlight Results dialog lets you highlight in the graphics window the objects found to have possible problems. Only those tests that you chose and which detected problems are enabled on this dialog. On selecting a test option from the Highlight Results dialog, and choosing OK, the geometry in the graphics window corresponding to the test is highlighted. The highlighted objects are easily visible: curves, solid faces and bodies have a temporary box drawn around them with asterisks at each corner; solid edges are highlighted with temporary asterisks at each vertex (continuous or circular edges have one asterisk). With the aid of these highlights, you can locate and zoom in on an area to examine it closely. The highlighting persists, even if you go to another function to edit the geometry. You can erase the highlighting with a Refresh or a Fit.

Objects

Tiny

curves, edges and bodies for which the diagonal length of a box enclosing the object is less than the specified distance tolerance

faces whose surface area is less than the specified distance tolerance, squared

faces whose area to perimeter ratio is such that 2 times the area, divided by the perimeter is less than the specified distance tolerance (this detects sliver faces)

Tiny

Highlight Results

Misaligned

For each object, a vector is obtained as follows:

lines - a vector in the direction of the line

arcs and circles - a vector normal to the plane of the curve

planes - the normal vector

cylinders, cones, tori, surfaces of revolution - the axis vector

extruded surfaces - the extrusion vector

Objects for which the vector is almost, but not exactly, parallel to XC, YC or ZC are flagged as misaligned. The number of incidences of misaligned geometry is reported in the Information window. To highlight the misaligned geometry in the graphics window, click the Misaligned option on the Highlight Results dialog.

Bodies

Data Structures

Consistency

This option checks:

that the topological structure is consistent

that the geometrical objects are valid and that faces and edges have G1 continuous geometry

that the geometrical objects are consistent; that is, the point geometry of vertices lies on the edges and faces to which they are linked; that edge geometry lies in the faces to which they are linked; and that edges intersect only at vertices

Face-Face Intersections

It is possible to inadvertently create face-face inconsistencies during modeling. For example, suppose you hollowed a cube to a thickness of 1mm, and then blended one of the outer edges to a radius of 5mm. The inner shell then intersects the outer shell, and the model is invalid.

Face-face inconsistencies can often be remedied by further modeling operations. In the above example, the model can be made valid by blending the inner edge.

The results of this test are reported in the Information window. Faces that intersect incorrectly are highlighted in the graphics window if requested from the Highlight Results dialog.

Sheet Boundaries

Highlight Results

Faces

Smoothness

This function performs a check of face smoothness, and that the geometry of the face selected is G1 continuous. (This option applies to free-form features only.) It also checks that the edge geometry lies on the face geometry. The results of the check are reported in the Information window. Any unsmooth face is highlighted when requested from the Highlight Results dialog.

Self-intersection

This function performs a check for faces that self-intersect. The results of the check are reported in the Information window. Any self-intersecting face found is highlighted when requested from the Highlight Results dialog.

Spikes/Cuts

Figure 4 - Spikes and Cuts

This function performs a search for all of the faces that contain spikes or cuts in the selected bodies. The number of such faces is reported in the Information window. Each face found to contain a spike or cut is highlighted when requested from the Highlight Results dialog.

Edges

Smoothness

This function searches for all edges whose adjoining faces do not join smoothly. The number of unsmooth edges are reported in the Information window. Each unsmooth edge is highlighted when requested from the Highlight Results dialog.

Tolerances

Distance

Threshold Tolerance Values

The values that appear in the Distance and Angle fields are used as a benchmark for some of the Examine Geometry tests. The values displayed in these fields the first time you enter the dialog are those specified in Preference->"Modeling. You are free to enter your own values, which will persist through the rest of the session.

Error Messages

Info->Analysis->Examie Geometry

Message	Comments
Data structure is corrupt	Serious condition. Use Undo and repeat the analysis.
Invalid geometry detected	An inconsistency was found in a topological structure. Use Undo and repeat the analysis.
Missing geometry detected Degenerate geometry detected	A topological entity (which is highlighted) lacks geometry. Use Undo and repeat the analysis.
Self-intersecting geometry detected	(Relevant to free form features.) A point of self-intersection is highlighted. Sometimes results if you make a mistake while creating a free form feature, e.g. incorrectly selecting curves. Can also be introduced by an offsetting operation. Recreate the free form feature if possible.
Geometry not G1 continuous	The geometry of a face or edge (highlighted) is not G1-continuous. (Relevant to free form features.)
Self-intersecting face detected	The face (highlighted) edges intersect at a point where there is no vertex.
Size box violation	Modeling operations are designed to work in a volume of 1000m x 1000m x 1000m centered on the origin of the absolute CSYS
Face-face inconsistency	An intersection of two faces was found which is not coincident with an edge. Corrective modeling is sometimes possible. In other cases (especially sewn bodies) the body may still be valid. If you cannot see an obvious face-face intersection.proceed with caution.

For more information on the "Part Cleanup" and "Examine Geometry" commands and using the STEP translators, please see the Unigraphics Online Documentation.

Last updated on May 28, 1998

Steven L. Alexander (STEP Master) is the maintainer of this Page.

Comments and suggestions are welcome. Phone: 1-765-451-7008

slalexan@mail.delcoelect.com