STEP: Import

This task shows you how to import to a CATPart or CATProduct document
the data contained in a STEP AP203 / AP214 file. 

It is also possible to insert a STEP file as an existing component in a CATProduct. 
Regarding AP214, both STEP AP 214 IS and STEP AP 214 DIS files are read.

The level of Recommended Practices published by the CAx Implementor Forum applied by the translator at import and export are the following :
 

  • Recommended Practices for External References with References to the PDM Schema Usage Guide
    Release 2.1 January 19, 2005  

  • Recommended Practices for Colours and Layers
    September 24th , 2001  

  • Recommended Practices for Geometric Validation Properties
    2nd Extension March 24, 2006  

  • Recommended Practices for Assembly Validation Properties
    August 17th, 2007

  • See also:
    CAx Implementor Forum
    http://www.cax-if.de
    http://www.cax-if.org
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 STEP Settings chapter.

Statistics about each import operation can be found in the report file and the error file.


  1. Depending on your configuration:

    Click the Open icon  or select the File > Open command.
    The File Selection dialog box is displayed.
    or

    Insert/Existing component command.
    The File Selection dialog box is displayed.

  2. Set the .stp or .step extension in the Files of type field.  

    This displays all .stp or .step files contained in the selected directory :

  3. Select the .stp or .step file of your choice (MoldedPart.stp, in our example) and click Open.

    A progress bar is displayed.
    You can use the Cancel button to interrupt the transfer at any time.
What is then displayed depends on the contents of the STEP file.
  • For the File/Open command:
    • If the STEP file contains a normalized assembly structure,
      a CATProduct document is created.
    • If the STEP file does not contain any geometrical and topological data,
      the components will be visible only  in the Specification Tree.
    • If the STEP file contains also geometrical and topological data,
      all the components will be present in the Geometry Space and in the Specification Tree. 
    • If the STEP file contains only geometrical and topological data, a CATPart document is created.

The geometrical elements of the faces, which could not be transferred,
are created in the NO SHOW space. In the NO SHOW space, you can
visualize the Surface supports and the 3D Curves).

  • For the Insert/Existing component command:
    • if the STEP file contains no assembly information, it is converted to a CATPart,
    • if the STEP file contains assembly information, it is converted to a CATProduct
      referencing several CATPart documents.

The resulting document is inserted in the current CATProduct document,
and the graphic window is updated (specification tree and geometry).
  • The reference to the STEP file is lost, so any update of the STEP file will have no effect
    in the CATProduct.
 
  • For both commands:
    • The reference planes are hidden.
    • A Geometrical Set is always created. It may be empty:
      • it will contain the valid surfaces imported, if any.
      • it is empty if there is no valid surfaces, e.g. when the element imported is a solid,
        or when all surfaces are invalid.
      • invalid surfaces are sent to a specific Geometrical Set (FaceKO#xxx)
Several STEP options can be customized:

Report file

After the recovery of STEP files, the system generates:

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

These files are created in a location referenced by the CATReport variable. Its default value is 

  • Profiles\user\Local Settings\Application Data\Dassault Systemes\CATReport on Windows (user being you logon id)
  • and  $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 

Note that the conversion summary in the report file takes assemblies into account.


Legend

  • OK = Transferred
  • KO = Not Transferred
  • NS = Unsupported
  • OUT = Out Of Size
    "OUT" entities are OUT of model size. Most of the time, these entities are curves
    and they are out of the V5 model space. These entities are not created.
  • DEG = Degenerated
    • "DEG" entities are degenerated entities. They are solids (MANIFOLD_SOLID_BREP) or
      Shells (OPEN_SHELL), or Curves (LINE, CIRCLE,...).
      Degenerated solids are incomplete solids (at least one Face misses)
  • INV = Invalid
    "INV" entities are Invalid entities, that is to say their description within the STEP file
    is invalid (STEP syntax rules are not respected,...). These entities are not created.

Example of error file:

E:\Report\pm6-hc-214.err

Input FileName : G:\Equipe_STEP\STEP\PDES-Prostep\Tr8\Prod\pm6-hc-214.stp
Output FileName : 


============================================
*** = Processing new independent element
* = Intermediate processing
!! = Independent element K.O.
! = Intermediate error
--------------------------------------------
<I> = Information
<W> = Warning
<E> = Error
--------------------------------------------
[0000] = Message identifier : 0000
[T=xxx] = Entity Type Step : xxx
[#0000] = Entity identifier number : 0000
============================================
Actual display level : Customer
 

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 Tools/Options/Compatibility/STEP 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 STEP above.
  • <W> [0904] The face #xx was splitted into nn CATIA V5 faces
    This message indicates that a STEP face has been split into several V5 faces to comply with V5 data structure.
  When the Continuity optimization of curves and surfaces/Advanced optimization option in
Tools/Options/Compatibility/STEP 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/STEP.

What About The Elements You Import ?

The attributes of products are taken into account as follows:
STEP   V5     
PRODUCT.ID   Part Number
PRODUCT.DEFINITION.ID   Definition
PRODUCT.NAME   Nomenclature
PRODUCT.DESCRIPTION   Description 
PRODUCT_DEFINITION_FORMATION_WITH_SPECIFIED_SOURCE.MAKE_OR_BUY   Source
PRODUCT_DEFINITION_FORMATION.ID   Revision

The attributes of instances of products are taken into account as follows:

STEP   V5
NEXT_ASSEMBLY_USAGE_OCCURRENCE.ID   Component/Instance name
NEXT_ASSEMBLY_USAGE_OCCURRENCE.DESCRIPTION   Component/Description
 

Groups

  • For each APPLIED_GROUP_ASSIGNMENT pointing to a group and a list of entities in the STEP file,
    a Selection Set is created.  This Selection Set is named with the name of the pointed GROUP entity
    and includes all pointed entities.
  • The transfer of groups can be activated/de-activated via the Groups (Selection Sets) option.

Layers

The number of the layer imported is defined by STEP PRESENTATION_LAYER_ASSIGMENT.ID. This is a string representing an integer. If this integer is higher than 1000, the number of layer will be imported as 0.

STEP Part 42 Entities Imported into V5R6 and Higher 

 

I=Implemented NI=Not yet implemented N/A=Not applicable according to the standard

       

Shape Representation

geometrically
bounded
wireframe

geometrically
bounded
surface

edge-based
wireframe

shell-based
wireframe

manifold
surface

faceted
brep

advanced
brep

High Level Entities

geometric_curve_set

geometric_set

edge_based_
wireframe_model

shell_based_
wireframe_model

shell_based_
surface_model

faceted_brep
brep_with_voids

manifold_solid_brep
brep_with_voids

                              Entity

Point

cartesian_point

I

 I I I I NI I

point_on_curve

 NI NI

N/A

N/A

 NI

N/A

N/A

point_on_surface

N/A

N/A

N/A

N/A

 NI

N/A

 NI

point_replica

 NI NI NI NI

N/A

N/A

 NI

degenerate_pcurve

N/A

N/A

N/A

N/A

 NI

N/A

 NI
 

Curve

line

 I I I I I

N/A

 I

circle

 I I I I I

N/A

 I

ellipse

 I I I I I

N/A

 I

hyperbola

 I I I I I

N/A

 I

parabola

 I I I I I

N/A

 I

polyline

 I I I I I

N/A

 I

b_spline_curve (+ rational)
b_spline_curve_with_knots

 I I I I I

N/A

 I

uniform_curve (+rational)

 NI NI NI NI NI

N/A

 NI

quasi_uniform_curve (+rational)

 I I I I I

N/A

 I

bezier_curve

 I I I I I

N/A

 I

trimmed_curve

 I I

N/A

N/A

N/A

N/A

N/A

composite_curve

 I I

N/A

N/A

N/A

N/A

N/A

composite_curve_on_surface

N/A

 NI

N/A

N/A

N/A

N/A

N/A

boundary_curve
outer_boundary_curve

N/A

 NI

N/A

N/A

N/A

N/A

N/A

pcurve

 NI

N/A

N/A

N/A

 NI

N/A

 NI

surface_curve

 I

N/A

N/A

N/A

  

N/A

  

offset_curve_3D

 NI

N/A

 NI NI NI

N/A

 NI

curve_replica

 NI

N/A

 NI NI NI

N/A

 NI
 

Surface

plane

N/A

 I

N/A

N/A

 I NI I

cylindrical_surface

N/A

 I

N/A

N/A

 I

N/A

 I

conical_surface

N/A

 I

N/A

N/A

 I

N/A

 I

spherical_surface

N/A

 I

N/A

N/A

 I

N/A

 I

toroidal_surface

N/A

 I

N/A

N/A

 I

N/A

 I

degenerate_toroidal_surface

N/A

 I

N/A

N/A

 I

N/A

 I

surface_of_linear_extrusion

N/A

 I

N/A

N/A

 I

N/A

 I

surface_of_revolution

N/A

 I

N/A

N/A

 I

N/A

 I

b_spline_surface
b_spline_surface_with_knots

N/A

 I

N/A

N/A

 I

N/A

 I

uniform_surface

N/A

 NI

N/A

N/A

 NI

N/A

 NI

quasi_uniform_surface

N/A

 I

N/A

N/A

 I

N/A

 I

bezier_surface

N/A

 I

N/A

N/A

 I

N/A

 I

rectangular_trimmed_surface

N/A

 I

N/A

N/A

N/A

N/A

N/A

curve_bounded_surface

N/A

 I

N/A

N/A

N/A

N/A

N/A

rectangular_composite_surface

N/A

 NI

N/A

N/A

N/A

N/A

N/A

offset_surface

N/A

 I

N/A

N/A

 I

N/A

N/A

surface_replica

N/A

 NI

N/A

N/A

 NI

N/A

N/A

Topology

vertex_point

N/A

N/A

 I I I

N/A

 I

edge_curve

N/A

N/A

 I I I

N/A

 I

oriented_edge

N/A

N/A

N/A

 I I

N/A

 I

vertex_loop

N/A

N/A

N/A

 NI NI

N/A

 NI

poly_loop

N/A

N/A

N/A

 NI

N/A

 NI

N/A

edge_loop

N/A

N/A

N/A

 I I

N/A

 I

face_bound
face_outer_bound

N/A

N/A

N/A

N/A

 I NI I

face_surface

N/A

N/A

N/A

N/A

 I I

N/A

advanced_face

N/A

N/A

N/A

N/A

 I NI I

oriented_face

N/A

N/A

N/A

N/A

 NI

N/A

N/A

vertex_shell

N/A

N/A

N/A

 NI

N/A

N/A

N/A

wire_shell

N/A

N/A

N/A

 NI

N/A

N/A

N/A

connected_edge_set

N/A

N/A

I

N/A

N/A

N/A

N/A

open_shell

N/A

N/A

N/A

N/A

 I

N/A

N/A

oriented_open_shell

N/A

N/A

N/A

N/A

N/A

N/A

N/A

closed_shell

N/A

N/A

N/A

N/A

I

 NI I

oriented_closed_shell

N/A

N/A

N/A

N/A

N/A

 NI I
manifold_solid_brep N/A N/A N/A N/A N/A N/A I
brep_with_voids N/A N/A N/A N/A N/A N/A I
faceted_brep N/A N/A N/A N/A N/A

I

N/A