IGES: Export

 

This task shows you how to save in IGES format the data contained in a CATPart, CATProduct or a CATShape document.

However, if you re-import an IGES file made from a CATShape, you will create a CATPart.

  • IGES 5.3 (year 2000-compliant) is the standard supported.
  • Only ASCII 1-byte characters are supported.

The table entitled What about the Elements You Export  ? provides information on the entities you can export.

You can find further information in the Advanced Tasks:

and in the Customizing 3D IGES Settings chapter.

Statistics about each export operation can be found in the report file created.

  1. Open the CATPart or CATProduct document to be saved in IGES format.

  2. Select the File > Save As... command.
    The Save As dialog box is displayed.

  3. Specify the name of the document in the File name:  field.

  4. Set the .igs extension in the Save as type field.

  5. Click the Save button to confirm the operation.

    A progress bar is displayed.
    You can use the Cancel button to interrupt the transfer at any time.

 

  • In V5, documents can be exported to files with the extension "igs".
  • The part number of the CATProduct is exported as the Product identification for Receiver.
  • The name of the author and of the organization can be exported to the Global Section of the IGES file.
  • Layer None is translated into layer 10000 in the IGES file.
Several 3D IGES export options can be customized:

Report File

After the exporting data to 3D IGES files, V5 generates:

  • a report file (name_of_file.rpt) where you can find references about the quality of the transfer 
  • and an error file (name_of_file.err) .

These files are created in a location referenced by 

  • the USERPROFILE variable on NT. Its default value is
     
    on NT (user being you logon id)
  • the HOME variable on UNIX. Its default value is $HOME/CATReport on UNIX.

What About the Elements You Export?


  • If the representation mode is "Surface", the topology of solids and shells is lost during the export.
    As a consequence, you have a group of surfaces called an Geometrical set.
    If you make an Import with Join, you can get a Close Body.
  • When a CATProduct is exported, its possible .igs components are not stored in the .igs file.
    If a CATProduct references V4 models, they are exported to the .igs file as IGES entities (product references).
    Each component of a CATProduct document is translated by a subfigure definition / singular
    subfigure instance in the .igs file.
  • Only V4 models referenced in a V5 CATProduct are exported to an .igs file.
  • You can choose the export unit.
  • Alternative representations that can be selected using Manage Representations are not taken into
    account during STEP exports. The main representation is always exported.
 
  • The name of the elements to export must be in ASCII format.
  • Overridden faces colors are supported.
  • You export the final construction object, i.e. the whole specification tree and its history up to the feature at
    the bottom of the specification tree and not the current feature: for example, you wish to export
    the specification tree up to Pocket.1 only.
    In this case, although Pocket.1 is the current feature, you will export all elements of
    the specification tree including Copy of Pad.1.
    If you want to limit your export to Pocket.1, you have to make sure that it is the feature at the
    bottom of the specification tree, like this:
The list below shows the IGES element numbers corresponding to the element types in Part Design.
  V5 Element

IGES Element

  null 0
  circle circular arc 100 However, in B-Spline mode (see options), all planes and surfaces are exported to rational B-Spline surfaces (128) and all curves, circles and lines are exported to B-Spline curves (126)
  curve, line, circle composite curve 102
  curve conic arc - ellipse 104 form 1 However, in B-Spline mode (see options), all planes and surfaces are exported to rational B-Spline surfaces (128) and all curves, circles and lines are exported to B-Spline curves (126)
  point, curve copious data 106 form 2
  plane unbounded plane 108 form 0 Construction unbounded planes (supporting faces) are exported as type 108, forme 0.
Independant unbounded planes are not exported.

However, in B-Spline mode (see options), planes and surfaces are exported to rational B-Spline surfaces (128) and all curves, circles and lines are exported to B-Spline curves (126)

  line line 110 form 0
  Semi-bounded lines line 110 form 1
  Unbounded lines line 110 form 2
  point point 116

A point belonging to a sketch is exported only if the sketch contains only points.

  surface ruled surface 118 However, in B-Spline mode (see options), all planes and surfaces are exported to rational B-Spline surfaces (128) and all curves, circles and lines are exported to B-Spline curves (126)
  surface surface of revolution 120
  surface tabulated cylinder 122
  matrix transformation matrix 124
  curve rational B-spline curve 126
  surface rational B-spline surface 128
  surface boundary curve on parametric surface 142 In standard export mode:

If the surface support is of B-Spline type and C2 continuous, both representation of boundaries are defined (2D parametric and 3D model space). Otherwise, only the 3D representation is defined.

In B-Spline mode all surfaces are exported as B-Spline surfaces (with 2D and 3D boundary representations). Those boundaries are ordered and oriented.

  surface trimmed (parametric) surface 144
  Solid

 

Manifold Solid B-Rep Object Entity 186 form 0 To export those entities, the Representation mode: Solid - Shell option must be active. It requires IGES 5.3 or higher.

All those new IGES entities have not been "tested" (IGES Norm 5.3) and the IGES/PDES Organization recommends that special consideration be given when implementing certain untested entities. Therefore if you do not know whether the receiver system will recognize those entities, we recommend that you do not use this option.

For Loops, only the 3D Representation is exported

  Plane Surface (support of Face) Plane Surface Entity 190 form 0
  Solid (Closed) Shell

 

Closed Shell Entity 514 form 1
  Independent Shell

 

Open Shell Entity 514, Form 2
  Face in a Shell

 

Face Entity 510 form 1
  Face Loop

 

Loop Entity 508 form 1
  List of Loop Edges Edge Entity 504 form 1
  List of Start/End Loop Edges Vertices Vertex Entity 502 form 1
  Long names (more than 8 characters) Name Property Entity 406 form 15
  Color color definition 314