IGES: Import

This task shows you how to import into a CATPart document the data contained in an IGES file.

Once imported, the data can be handled just as if it were created as a CATPart.
The main purpose of such an import is to be able to create shells from IGES faces but you may also find it
useful for re-using face contours in the Sketcher application, deforming NURBs in Generative Shape Design or
using faces in other V5 applications.

The table entitled What about the elements you import ? provides information on the entities you can import.
You can find further information in the Advanced Tasks:

and in the Customizing 3D IGES Settings chapter.
Statistics about each import operation can be found in the report file created.

The function "Insert / Existing Component" for IGES files is provided by the MULTICAx IGES plug-in
and requires a MultiCad license. 
  1. Select the File > Open command.
    The File Selection dialog box is displayed.

  2. If the directory contains many different types of files you may wish to set the .igs extension in the Files of type field.
    This displays all files with the extension "igs" contained in the selected directory.

awarning.gif (1007 bytes) In Version 5, both files with the extension "igs" and IGS can be imported to a CATPart document.
  1. Select the .igs file of your choice and click Open.

    A progress bar is displayed.
    You can use the Cancel button to interrupt the transfer at any time.
    This creates a new document similar to a CATPart document in all respects and containing all surfaces
    and 3D wireframe geometry. The data is now available in your session.
    • Some invalid geometries may be detected.
    • The reference planes are hidden at import.
Several 3D IGES import options can be customized:

Report File

After the recovery of 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 
    Profiles\\user\\Local Settings\\Application \Data\\Dassault Systemes\\CATReport
    on NT (user being you logon id)
  • the HOME variable on UNIX. Its default value is $HOME/CATReport on UNIX.
Always check the report and error files after a conversion !
Some problems may have occurred without been visually highlighted.
Example of a report file:

Example of an error file:


Report messages

  Here are some of the messages that may appear:
  • Too many cuts on face boundary.
    Tip : Use topological reduction option (in IGES) or curve optimization (in IGES or STEP) - see User's Guide
    These options are accessible via the Tools/Options/Compatibility/IGES or
    dialog boxes, in the Continuity optimization of curves and surfaces section.
    Select the Advanced optimization option and push the Parameters... button.
    For more information, click on the link on IGES above.
  When the Continuity optimization of curves and surfaces/Advanced optimization option
in Tools/Options/Compatibility/IGES is active, the following warning messages may appear in the report file:
  • The BSpine Surface is not C1: Approximation of the surface is impossible!
    This is just a warning, the surface is imported but is not approximated.
  • The deformation found of the surface approximation (which is calculated by isoparameters) is : xx millimeters.
    This indicates that the real deformation found is higher than the Deformation value you have entered in
    the Parameters box and that the approximation could not be performed. When this occurs for several entities,
    you will find the following information message at the end of the report file:
  • For a better approximation of BSpline surfaces, you can use a "Curves and surfaces approximation"
    Deformation value of at least : xx millimeters
    You can enter this value in the Parameters box of the
    Continuity optimization of curves and surfaces/Advanced optimization
    option in Tools/Options/Compatibility/IGES.

Invalidity in Input Geometry

  When invalidities are detected in the input geometry, all the invalid faces
(and all the elements of their geometry)
are put in a specific Geometrical set named invalid Input Geometry.
These faces are shown as invalid in the report file.
For each invalidity detected, a specific label points to the face concerned. 
These labels are put in an Annotation Set.xx.
  • Deleting an invalid element does not automatically delete the corresponding Annotation Set.
  • Only one feature Annotation Set is created at the root of the specification tree, with all the invalidity descriptions.
  • Annotation Sets are not exported to IGES, but they can be saved in the CATPart.

What about the Elements You Import?

The following points should be remembered:
  • The IGES standards 5.2 and 5.3 are supported. The latter is year 2000-compliant.
  • Trimmed and bounded surfaces are transformed into faces.
  • Solids and volumes are imported as joined shells as well as text, annotations and 2D geometry are not converted.
  • The tolerance used is the default tolerance defined in the Part Design session.
  • Properties such as the original colors, the show status, names (if they exist) are maintained in your session.
  • IGES files must contain only ASCII 1-byte characters.

Processing of layers:

  • If the IGES file contains a layer 10000, this layer is tranlated into layer None in V5.
  • A layer with a name greater or equal to 1000 is translated into a layer named with the last three digits, e.g. layer 3250 is translated into layer 250.

Processing of names:

  • Non ASCII characters are replaced with 1-byte characters, either a similar one, e.g. a 'e' with an accent is replaced with a plain 'e' (with no accent), or by an em dash '_'.
  • If an IGES entity has a pointer to a "Property Name Entity",
    the value of this property will be assigned to the name of the V5 entity.
  • If the IGES entity has no pointer to a "Property Name Entity" and
    if its "Directory Entry" field #18 is not blank the V5 name will be computed
    by appending field #18 and #19 of the  "Directory Entry".
  • If the entity has neither a "Property Pointer" nor a non-blank field #18 an automatic name will be generated.
  • Product Identification for Receiver (Global Section, Field #12) will be used as
    the Part Number in the Product Properties and as display and storage names in V5.
    For example, if the file MyFile.igs has a product identification IGES_Sample,
    the storage name will be IGES_Sample.CATPart (not MyFile.CATPart)

Processing of Group Associativity:

The Group Associativity, in the IGES Norm, is mapped with the type 402 (ASSOCIATIVITY INSTANCE ENTITY).
There are four form numbers which specify group associativities :

Form Meaning
1 Unordered group with back pointers

Unordered group without back pointers

14 Ordered group with back pointers
15 Ordered group without back pointers

For each Group Associativity pointing to a list of entities in the IGES file, a selection set is created.
This selection set is named with the name of the pointed GROUP entity and includes all pointed entities.

  • This applies to known Group Associativity forms (Type 402 - forms 1, 7, 14 and 15) only.  
  • A Selection set pointing to another Selection set cannot be created.
  • When a group is pointed by a second group, the entities of the first group will be pointed by a first
    Selection set (mapping the first group) and by a second Selection set mapping the second group
    (including others entities of the second group).
  • Only logically dependant IGES entities (Status Number 3-4 = "02" in D.E. section) can be mapped in a Selection set.
  • The Import Group option activates or de-activates the creation of Selection Sets.

Processing of 308/408 IGES entities

Processing of trimmed surfaces

IGES Trimmed surfaces are defined by a support surface and one or more boundaries.

For Trimmed parametric surfaces, the curves of boundaries can have two representations: one in the model space (3D curves) and another in the parametric space (2D or P-Curves).

3D Curves can be used on every type of surfaces.
2D curves can be used on B-Spline surfaces (IGES type 128), Ruled surfaces (IGES type 118 - if the surface is continuous in curvature and not closed) and Revolution surfaces (IGES types 120/122);
2D curves must be parametric lines (IGES type 110) or P-Nu(r)bs (IGES type 126).

The choice of the curves representation to process depends on the user preferences and on the IGES file contents. In some IGES files, a representation can be incorrect.

See Representation for Boundaries of Faces in IGES customizing section to learn more about the management of boundaries representations.


To make sure the elements you need to handle in your session are those you expected,
here is a list presenting the IGES data supported when imported into a CATPart document:

IGES Element

V5 Element Notes
  null 0
  circular arc 100 circle
  composite curve 102 curve, line, circle
  conic arc - ellipse 104 form 1 curve
  copious data 106 forms 1-3,15 point, curve
  unbounded plane 108 form 0 plane From V5R12, even independent planes 108 form 0 are imported.

Independent planes 108 form 0 will be displayed as a small square in CATIA

  bounded plane 108 form 1 plane
  line 110 form 0 line
  semi-bounded line 110 form 1 line
  unbounded line 110 form 2 line
  parametric spline curve 112 curve
  parametric spline surface 114 surface
  point 116 point
  ruled surface 118 surface
  surface of revolution 120 surface
  tabulated cylinder 122 surface
  direction entity 123 direction  
  transformation matrix 124 matrix
  rational B-spline curve 126 curve
  rational B-spline surface 128 surface Rational B-spline surfaces are also recognized as planes or cylinder according to their geometrical properties..
  offset curve 130 curve, line, circle
  offset surface 140 surface
  boundary (of skin) 141 either included in the translation of a bounded surface, or curve, line, circle if the transfer of the bounded surface has failed If the surface is not of type BSpline and C2 continuous, only the Geometry type curves "Curve on a parametric surface" and "Boundary" are taken into account for face creation. 2D Parametric type curves are ignored.
  curve on parametric surface 142 either included in the translation of a trimmed surface, or curve, line, circle if the transfer of the trimmed surface has failed If the surface is not of type BSpline and C2 continuous, only the Geometry type curves "Curve on a parametric surface" and "Boundary" are taken into account for face creation. 2D Parametric type curves are ignored.
  bounded surface (of skin) 143 surface
  trimmed (parametric) surface 144 surface
  manifold solid B-rep
(consisting of shell
edge list
vertex list)
186 form 0
(514 form 1
510 form 1
508 form 1
504 form 1
502 form 1)
joined shell Creation of a geometrical set or PartBody per shell.

Creation of a PartBody if the shell is closed.

  plane surface entity 190 form 0-1   All the surfaces are faces support surfaces : they must be used with entities of type 143, 144 and 510.

Those surfaces are infinite (not limited).

If a face, supported by one of those surfaces, cannot be correctly imported, the "invalidFace" created by CATIA V5 and containing surfaces and curves could present visualization problems on infinite surfaces graphic representation.

  right circular cylindrical surface entity 192 form 0-1  
  right circular conical surface entity 194 form 0-1  
  toroidal surface entity 198 form 0-1  
  subfigure definition (detail) 308 see singular subfigure instance
  color definition 314 color
  associativity instance (group) 402 forms 1,7,14,15 selection set See the Group Associativity
  singular subfigure instance (ditto) 408 simple elements or CATParts See the processing of 308/408 IGES entities.