STEP  

• General STEP options:
  • Detailed report,
  • Geometric Validation Properties (GVP),
  • Groups (Selection Sets).
• Import STEP options:
  • Continuity optimization of curves and surfaces,
  • Assemblies physical structure,
  • Insert existing component,
• Export STEP options:
  • Application Protocol (AP),
  • Units,
  • Show/NoShow,
  • Header of the STEP file,
  • Assemblies.

General

Detailed report

By default, the report file contains a Detailed Conversion chapter. Click to clear the Detailed Report option to remove this chapter from the report file.

Geometric Validation Properties (GVP)

This functionality is available in STEP AP214 and AP203 ed2, i.e. Geometric Validation Properties are attached at product level, according to Recommended Practices for Geometric Validation Properties 2nd Extension March 24, 2006  

When the Geometric Validation Properties option is selected, the Tolerances button becomes available.
It opens a dialog box where you can define the tolerances for the GVP checking.
The dialog box looks like this if you have selected Standard Scale:

and like this if you have selected Small Scale:

• The first tolerance is the percentage of variation of volume or area allowed. Default value: 1%.
• The second tolerance is the maximum error for the center of gravity.
  Default value: 1mm for the Standard Scale and 0.01mm for the Small Scale.
• Click Default Values to revert to the default values (1 and 1mm or 0.01 mm).

For import:

• Geometric validation properties are computed for each solid, shell, product or instance, and this information is written in the report file.
• For each solid, shell, product or instance, the report file gives the computed geometric validation properties:

• Centroid: coordinates of the center of gravity (applies to solid, shell, product or instance),
• Area: area of the entity (wetted area for solids) (applies to solid, shell or product),
• Volume: volume of the entity (for solids only) (applies to solid or product).

• If the imported STEP file contains geometric validation properties, these properties are read. This information is written in the report file.
• For each read geometric validation properties, the report file gives the status of comparison between read and computed properties, with the following information: 

• Centroid deviation error (distance measure) (applies to solid, shell, product or instance),
• Surface area difference value and error ratio (applies to solid, shell or product),
• Volume difference value and error ratio (applies to solid or product).

• A global status for the conversion is given, together with the maximum deviations found. 

These properties are completed with the estimation of their computation errors for each solid and each shell.
The estimation of the computation error on the area or the volume is provided as a relative value.
The estimation of the computation error on the centre of gravity is provided as an absolute value for each coordinate and a bounding box of the entity.

Example of a report file:

• ratios (Volume difference and Surface area difference) are lower than 1%.
• and the centroid deviation is lower than 1 mm.

If all status are ok, the global status is ok too.
The maximum deviation found for each comparison (centroid, area and volume) is given in the report file with the corresponding entities (the maximum deviations found do not necessarily apply to a single object).
This functionality involves a slight performance loss, due to the properties computation cost.

For export:

• The exported STEP file includes geometric validation properties for each solid, shell, product or instance, according to STEP AP214 and AP203 ed2 and the CAX-IF recommended practices.
• For each solid, shell, product or instance, the report file gives the computed geometric validation properties:

• Centroid: coordinates of the center of gravity (applies to solid, shell, product or instance),
• Area: area of the entity (wetted area for solids) (applies to solid, shell or product),
• Volume: volume of the entity (for solids only) (applies to solid or product).

• These properties are completed with the estimation of their computation errors for each solid and each shell.
  The estimation of the computation error on the area or the volume is provided as a relative value.
  The estimation of the computation error on the centre of gravity is provided as an absolute value for each coordinate and a bounding box of the entity.

Example of a report file:

Groups (Selection Sets)

By default, this option is selected:

• at import, Groups found in the STEP file are translated into Selection Sets.
• at export, Selection Sets found in the CATIA file are exported as Groups in the STEP file. Refer to the STEP: Export chapter for more information (Miscellaneous section).

However, importing or exporting Groups may be time consuming. Click to clear this option and de-activate the processing of Groups.

Import

Continuity optimization of curves and surfaces

This setting allows a better user control over the number of curves and surfaces that are created during the process of importing STEP data into V5:

V5 requires its geometry to be C2-continuous. When non C2-continuous geometry must be imported from a STEP file, this geometry (curves, surfaces) is broken down into a set of contiguous geometries, each of them being C2-continuous. This is what happens when the No Optimization option is chosen. 

However, this can produce an increase of the size of the resulting data, because more curves/surfaces are created. In order to limit this drawback, two other modes are optionally offered. 

In those modes, the STEP interface tries to limit the splitting of curves and surfaces by modifying their shape slightly, so that they become C2-continuous while remaining very close to their original shape. 

In order to guarantee that the deformation is not excessive, a maximum deviation parameter is used. When in Automatic  optimization mode, this maximum deviation is read into the STEP file itself, in the STEP parameter that documents the precision of points in the file. In this mode, the value read from the STEP file is then corrected so that it remains comprised between 10E-2 and 10E-3. This guarantees an optimization that remains compatible with the precision for the data that was set by the emitting system. 

Last, if this strategy is not enough, you can choose the Advanced optimization mode, in which an arbitrary deviation value can be entered. 

You can find useful information in the report file. Please see the Report file section in the STEP Import chapter in this User's Guide.

The Automatic optimization proposes:

• No approximation, thus this option does not create a significant deformation and keeps the internal BSpline structure (equations and knots).
• A continuity optimization is performed within the deformation tolerance used for optimizing BSplines, comprised between 0.001mm and 0.01mm (depending on the tolerance value defined within the imported STEP file) on:

• BSpline surfaces,
• BSpline boundary curves (3D and P-curves when available),
• BSpline independent 3D curves,

• The parameters box cannot be activated

This option softens the effect C2 cutting of faces and boundaries (which is mandatory in V5) without any significant geometric deformation

If you select No optimization:

• No optimization is performed on BSplines (neither curves nor surfaces).
• Elements are cut at  discontinuity points to suit the modeler (exact mathematic continuity). This may result in a dramatic number of faces and boundary curves, data of poor quality and poor performances in further use in V5.

If you select Advanced optimization:

• No approximation. The internal BSpline structure (equations and knots) is kept,
• A continuity optimization is performed on:

• BSpline surfaces,
• BSpline boundary curves (3D and P-curves when available),
• BSpline independent 3D curves,

• but the deformation tolerance is set by the user (see Parameters).

With this option, you can enter a larger tolerance value which may enhance the optimization impact (resulting in less C2 cutting on faces).

Click Parameters to access advanced optimization options and tolerances.
The dialog box looks like this if you have selected Standard Scale:

and like this if you have selected Small Scale:

User-defined Tolerance

Note that the tolerance is shared by the optimization process (in all cases), the Curves and surfaces approximation and the Topological reduction of boundaries if you have selected those check boxes.
For example, you have a deformation tolerance of 0.001mm and you have selected Curves and surfaces approximation.
The tolerance for the optimization will be 50%, i.e. 0.0005mm and that of the Curves and surfaces approximation will also be 50%.
Thus, the number of cuts of the faces will vary according to the value entered, and according to the number of check boxes selected.

• Deformation: maximum deformation (in millimeter) allowed in the optimization of curves and surfaces:  

  • For the Standard Scale, it ranges between 0.0005 and 0.1 mm. The default deformation is 0.003mm.  
  • For the Small Scale, it ranges between 5e-006 mm and 0.001 mm. The default deformation is 3e-005mm.

Click Default Value to revert to the default value.

User-defined Advanced Option: Curves and surfaces approximation:

• By default, this option is not selected.
• BSpline surfaces and curves continuity is optimized,
• In addition, Bspline curves and surfaces approximation is performed,
• It is possible to enter a user value for Deformation,
• This option may change the internal structure of BSplines (equations and knots),
• This option usually results in a significant decrease in the number of faces cuttings.

Assemblies physical structure

This option enables the processing of sub-assemblies of an imported assembly.
By default, it is not selected. A CATProduct file containing the whole assembly structure and a CATPart file for each part of the assembly are created.
If you select this option, a CATProduct file containing the sub-assembly structure is created for each node of the whole assembly while a CATPart file is created for each part of the whole assembly.

Insert existing component

This option appears only if both the V5 - STEP AP203 Interface and the V5 - STEP AP214 Interface and the MULTICAx STEP Plug-in exist on the machine. By default it is not selected. Select it to activate the MultiCAD mode.

Export

Application Protocol (AP)

The data contained in a CATPart or CATProduct document will be saved in STEP AP203 or AP214 formats. For more information about STEP AP203, AP203 with extensions, AP203 edition 2 and STEP AP214, refer to Exporting CATPart or CATProduct Data to a STEP AP203 / AP214 File. 

Units

Show/NoShow

By default, those options are not active.
A CATPart to export may contain:

• visible entities placed in the Show space,

• hidden entities placed in the NoShow space. By default, they are not exported.

• hidden entities placed in layers that are not visualized (for more information, see Using Visualization Filters). Visualization filters are now taken into account: by default, entities placed in non-visualized layers are no longer exported.

Select the Export also NoShow entities option to export all entities belonging to both the "Show" and the "NoShow" spaces.
Select the Export non-visualized layers option to export also all entities belonging to those layers.

Note that the entities placed in the NoShow or in non-visualized layers are exported as if they were visible entities. This means that reading back a STEP file generated with the Export also NoShow entities or the Export also non-visualized layers option will make those previously hidden entities visible.

STEP export manages invisibility in assemblies as follows:

• invisible instances of a product or a component are not exported,

• an instance is considered as invisible for export in a given product or component if it is invisible in all instances of this given product or component.

For example:

Let's consider the instances of AAA in the products above:

• AAA is considered as visible for export in Product10, because it is visible in at least on instance of Product10.
• AAA is considered as invisible for export in Product9 as it is invisible in all instances of Product9.

• AAA is visible in both instances of Product10, as AAA was considered as visible for export in the initial Product10.
• There is no instance of AAA in Product9 as AAA was invisible in that product.

Header of the STEP file

Click Define... to define the header of the STEP file:
Fill in the form displayed as required. Click Default Values to revert to the Default Values of the header.

The header of the exported file looks like this:

Assemblies

Select the required option to select the export mode. 

• One STEP file: one STEP file only containing the structure and geometry of the components.
  
• Links to CATIA: a STEP file containing structure and entities PRODUCT_DEFINITION_WITH_ASSOCIATED_DOCUMENT which have a link with CATPart files.
• External references to STEP : 

• one STEP file containing the structure
• and a STEP file for each component 
  The STEP file names, for each component, have the same name as the components.
  the structure and the component STEP files are generated in one shot, in the same location.

• External references to CATIA: one STEP file containing the assembly structure with external links to CATPart, CATShape, model V4, .cgr, .wrl files, according to AP214 and AP203 edition 2 external references mechanism.

The External References functionality is available only with AP214 and AP203 edition 2. 
A STEP file cannot refer to a STEP assembly file.
This summary table shows you all the possible combinations within the first two frames, Export : Application Protocol and Export : Assemblies. 

(1) = reference of the Application Protocol Config Control Design (AP203)
(2) = reference of the Application Protocol Core Data for Automotive Mechanical Design Processes (AP214)
(3) = Export of the Structure and Geometry of a CATProduct into one file only
(4) = Export of the Structure and Geometry of a CATProduct into different files
(5) = Export of the Structure only of a CATProduct
(6) = Export of the Structure of a CATProduct with links to CATIA for the geometry.