DXF/DWG: Import

This task lets you quickly see how to import or to insert the 2D geometric data
contained in a DXF file into a CATDrawing document.
Once imported, the data can be handled and edited just as if they had been created
in a Drafting session using 2D geometry creation commands.
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:

Statistics about each import operation can be found in the report file created.
Open your session (Open your CATDrawing document if you want to insert a DXF file.).

  1. To import an existing DXF/DWG file, select the File > Open items or
    To insert a DXF/DWG file in an existing CATDrawing document, select the Tools > Import From File.
    The File Selection dialog box is displayed:

  2. Select the .DXF/.DWG extension from the field called Files of type.
    All .DXF/.DWG files contained in the selected directory are now displayed.

  3. Click the .DXF/.DWG file of your choice.

  4. Click Open.

    • In import mode, a CATDrawing file is created which contains all the geometry included in the DXF/DWG file. This CATDrawing file becomes the current document.
    • In insertion mode, the geometry of the DXF/DWG file is created in the current drawing.
 

Import of multiple viewports and layouts

The default behavior has been improved for better results.
If the model is referenced, at least partially, by one or several viewports, the model is not created in a sheet of its own.
Only layouts are created. They will contain eventual viewports.
In this case, select the option Keep model space to force the creation of the model space in its own sheet.
CATIA does not create empty viewports or layouts.
Viewport with a not null twist angle (group code 51) are not correctly handled during import.
 

Format

V5 determines systematically and automatically the most suitable format (A0 ISO, A1 ISO, etc.)
for each sheet (layout) i.e. V5 chooses the smallest format in which the drawing can be totally included:

  • If the standard is ISO, V5 chooses the format among A0, A1, A2, etc.
  • If the standard is ANSI,  V5 chooses the format among A, B, C, etc.
  • If no standard format fits the sheet, the format is set to the largest one i.e. A0 ISO and
    made invisible with a message "No standard format can be applied to this sheet" in the report file.
  • If you are not satisfied with this automatic result, use the Page Setup command to modify the format.

Information on what has been determined automatically is written in the report file:

For more information on Formats,
see the Defining a Sheet chapter in the Generative Drafting User's Guide.
 

Code pages

DBCS (Double Byte Character Set) Supported Code Pages are:

  • 932 (Japanese)
  • 936 (Simplified Chinese)
  • 950 (Traditional Chinese)
949 (Korean) is not supported.
 

Customization

Import of a DXF/DWG file can be improved by customization:

DXF/DWG specific import settings are:

  • Standards. The lists of attributes are not the same in V5 and AutoCAD.
    A DXF mapping standard file is used to come as close as possible to the AutoCAD attributes,
    or to switch them to V5 attributes. 
  • Unit of the file

The definitions of dimensions are not the same in V5 and AutoCAD.
This option is used to give priority either to the graphic closeness or to the re-usability in V5. 

Report File

After the recovery of DXF/DWG files, the system generates:

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

This file is created in a location referenced by 

  • the CATUserSettingPath 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  file after a conversion ! Some problems may have occurred without been visually highlighted.

What About The Elements You Import ?


 		 Version 5 supports the import DXF/DWG formats version 12,13, 14 and AutoCAD2000, AutoCAD2000i, AutoCAD2002, AutoCAD2004, AutoCAD2005, AutoCAD2006 and AutoCAD2007.

To make sure the elements you need to handle in your session are those you expected,
here is a list presenting the DXF/DWG data supported  when imported into a CATDrawing file.

  DXF/DWG element DXF/DWG sub-type  V5 element Notes
 

Geometry
  point Point
  line Line
  ray None
  xline None
  circle Circle
  arc Arc
  ellipse Ellipse
  polyline/2D polyline/
lightweight polyline		 non adjustable width,
made of line segments		 Polyline Not editable in V5
  non adjustable width,
made of line and arc segments		 segments and arc
with no structure		 Structure is lost
  adjustable width Filled area (pattern) Structure is lost
  fit curve Polyline
  mline Lines Structure and closing attributes are lost
  spline NURBS Not editable in V5
  3D face none
  3D solid none
 

Annotations
  text Text
  mtext Text Changing fonts, changing attributes and
line break are not taken into account
  Arc aligned text none
  rtext none
  dimensions aligned,
linear and rotated,
radius and diameter,
angular,  ordinate (x or y)		 According to option:

dimension or 

details or 

geometry+texts

 See dimensions

In a few "dimensions" cases, the text of the
dimension can be a text with an associative link

In all "dimensions" cases, the geometry support is
in No Show
  leader Line + text DXF Leaders are imported as simple lines.
The arrow head and the line under the text are lost
  tolerance none
  hatch non-associative Filled area (pattern)
  associative Filled area (pattern) The contour of the hatch is created in the No Show
and the associativity is created with this hidden contour.
  solid Filled area (colored)
  block attribute Text
  Structures
  block Detail
(2D component)		 The details are created in a new Detail Sheet
named "Imported Details".
  insert (Block Reference) Ditto
(instance of 2D component)		 If the insert is defined with different scales,
on x-axis and y-axis, no detail instance is created
but only the geometry is transferred.
  external reference     not supported
  group none The structure of the group is lost whereas its contents
is transferred
  viewport View see  above
  Layout (paper space)   Sheet see  above
  OLE frame none
proxy Detail The proxy is converted into standard elements (lines, arcs, texts, …) that are imported at the place of the proxy.
The proxy must contain its graphic representation.
The graphic representation must be consistent with the proxy.
  region none
  Attributes
  color Color see Standards
  Line weight Line thickness see Standards
  line type Line type see Standards
  point markers Point type Markers may be different since V5 and
AutoCAD do not have the same markers.
  layer Layer Invisible layers are gathered in a filter
named Invisible Imported Layers.

Visible layers are gathered in a filter
named Visible Imported Layers.
  layer name     When an AutoCAD layer has a name that corresponds to a number between 0 and 999, this layer will be imported as a V5 layer with the number associated:
  • if a V5 layer with the same number already exists, the AutoCAD layer is imported in this V5 layer, without changing its name.
  • if there is no V5 layer with the same number, the AutoCAD layer is imported in a new V5 layer, with the same name as in AutoCAD.

If the AutoCAD layer has a name that does not match any number in the available range, the layer is mapped on the first existing V5 layer that has the same name, or a new one is created on the first available V5 layer number with the AutoCAD layer name.

  font Font see Standards
  Pattern Pattern Automatic mapping 
  BYBlock attribute Attribute The value of the attribute of the block is
set to a default value
  BYLAYER attribute Attribute The value of the attribute of the layer is
applied to each element imported