CATIA - GENERATIVE DRAFTING 1 Product (GD1)

General Issues

Managing CATDrawing Documents in ENOVIAVPM If you use the command Load PDM Context in ENOVIAVPM context with VPM 1.5PTF18, a new CATProduct will be created in V5, instead of the assembly data being loaded in the CATProduct which is already opened and linked to the CATDrawing. On this level, use the following methodology: do not open the CATProduct before using the command Load PDM Context on the CATDrawing.
This behavior is corrected on VPM 1.5PTF19 and later PTFs.
Dimensions upper text For ANSI or ASME drawings created with V5R7SP1 or earlier: existing dimensions upper text may swap from edge to center.
Dimension line/Extension line thickness For drawings created with R6GA and R6SP1, dimensions thickness may change when opening the drawing.

Workaround: To bypass this problem, go to Edit > Search. In the Advanced tab, select Drafting for the workbench and Dimension for the type, and click the Search button. Select the dimensions to modify and click OK. In the contextual menu, choose Properties, and then in the Dimension line tab, set the line thickness.

Section views Patterns are not applied to sections which are tangent to 3D faces.
Annotation thickness When swapping from one CATDrawing document based on a standard containing thicknesses definition (standards created or updated in V5R9 or on a higher level), to a CATDrawing document based on a standard that does not contain thicknesses definition, the first display of this second drawing may sometimes show incorrect annotation thicknesses (dimensions, datum features leaders, datum target leaders and roughness symbol leaders). The following displays will show correct thicknesses.
Workarounds: To handle the problem, the recommended methods are the following: just activate (or deactivate) the Analysis Display Mode and Create Detected Constraints icons. Or, use the Force Update command (enter: c: Force Update in the Power Input field), if you do not mind updating generated views.

Even more efficient, just upgrade the standard to a level containing thicknesses definition. To do that, just click the Update button available in the Page Setup dialog box.
Dimension and dress-up parameters In versions prior to V5R14, when using styles parameters such as leader symbols or head/tail arrows symbols, SymetricCircle and Circle were inverted. For instance, when choosing SymetricCircle in styles, the annotation was displayed with Circle extremity and when choosing Circle in styles, the annotation was displayed with SymetricCircle extremity.

Example when creating annotation with SymetricCircle as parameter:

            Prior V5R14                                           From V5R14

Symbols Circle and SymetricCircle were inverted when creating the following annotations:

  • Coordinate dimension
  • Text
  • Table
  • Datum features
  • Datum target
  • Tolerance
  • Balloon
  • Roughness symbol
  • Welding symbol
  • Arrow

Symbols Circle and Symetric Circle were not inverted when creating the following annotations:

  • Length/Distance dimension
  • Angle dimension
  • Radius dimension
  • Diameter dimension
  • Chamfer dimension

We advise you to check in the standard files the symbols specified for the annotations mentioned in the first list:

  1. When using a symbol other than Circle and SymetricCircle: no modification required
  2. When using Circle or SymetricCircle:
  • The specified symbol is the one expected for the annotation: no modification required, newly created annotation displays the right symbol.
  • The specified symbol is not the one expected for the annotation: invert the symbols, then upgrade standard files to make sure the appropriate styles are used.

Note that only newly created annotations listed above will be impacted. Those created with versions prior to V5R14 will not.

Import from 3DXML
/ save as 3DXML
  • Texts in TrueType Font (TTF) are temporarily generated as Exact geometry (i.e. as true text objects) 3DXML. When 3DXML file is imported into a .CATDrawing document, in some cases, text objects visualization might be incorrect. Normal visualization behavior for .CATDrawing document is a WYSIWYG mode where text objects are generated as tessellated elements.
  • Text blanking is not taken into account in 3DXML.
  • When 3DXML files are imported into a .CATDrawing document, the overlay mechanism might not work as expected and therefore, some elements might be hidden instead of being displayed in foreground.
Views of products having layer filters activated When updating views of a product whose visualization has been filtered using “Layer filters”, the view will represent the filtering of the product that was active the last time the product parts were saved.

In order to take benefit of a change in the filtering of the product (either after a change of part layers, or a change of the filter itself) it is required that the parts be saved with this new filtering active.
Representation of fillets in Drafting views obtained by copying-pasting As Result the CATIA V4 solid Fillet surfaces do not exist as such in CATIA V4 models.
As a result, in Drafting views obtained by copying-pasting As Result the CATIA V4 solid, fillets cannot be represented using the following representation types: Symbolic, Approximated Original Edges, Project Original Edges.
They can only be represented using the Boundaries representation type.
You can workaround this by copying-pasting As Spec the CATIA V4 solid to a CATIA V5 part.
Updating assembly views Updating assembly views with the Enable occlusion culling option selected will result in a CPU loop on UNIX operating systems.

This impacts views that represent several CATParts (i.e. views of CATProducts or CATProcess containing more than 1 part), and are either:

  • Exact mode views
  • CGR mode views (wherein, the occlusion culling is part of the default processing of CGR mode views)

Therefore, as a bypass, we recommend to:

  • Modify the default setting by clearing the Enable occlusion culling check box in  Tools > Options > Mechanical Design > Drafting > View.
  • Clear the Enable occlusion culling check box in the properties of the view generated using the Exact view of View generation mode.
  • Use Approximate view generation mode instead of CGR mode.

Open Issues

None  

Documentation Addenda

V4/V5 Standard Mapping During a 2D conversion V4 to V5, V4 annotations and V4 dimensions are migrated in V5 with the same property as V4 or according the V5 2D standard defined in a *.XML file.
V4 2D standard defined in the V4 project file can not be converted as a *.XML file.

The following document was created to help V4 customers to set all V5 parameters in this file before starting 2D migration.

V4V5_standard_mapping_V07.pdf