DXF/DWG: Export

• Drawing Interchange Format (DXF) files enable the interchange of drawings between
  Generative Drafting Version 5 and Version 4 or with other programs.
• DXF files correspond to ASCII format and DWG to binary format.
• V5 provides a simple method to export the data contained in a CATDrawing document
  either in a DXF file or in a DWG file.V5 supports DXF/DWG formats version 12, 13, 14 and AutoCAD2000.

• Trouble Shooting,
• Best Practices,
• FAQ,
• VBScript Macros.
• and in the Customizing DXF/DWG Settings chapter.

1. Select the File, Save As item.

   The Save As dialog box is displayed:

2. Change the Format type into DXF type.

3. Enter the file name.

4. Click Save.

• If the current unit belongs to the metric system (millimeter, centimeter, meter, ...)
  the export unit is the millimeter.
• If the current unit belongs to the Anglo-Saxon system (inch, foot, ...) the export unit is the inch.

So select the required type of session unit to export your data in one system or the other.

Limitations in the case of a multi-sheet drawing:

• When there are several sheets, the name of the file really created is not that entered by the user in the
  Save as dialog box, since it is concatenated with that of the sheet. Therefore,  it is not possible to check
  if a file with the same name already exists and any existing file will be overwritten without warning.
• If one of the sheets contains no geometry, no DXF file is created.
• The number of characters of the name of the result file is limited to 150.
• If the name of a sheet contains one of the following characters or a
  blank space, the character will be replaced with _ (underscore).

• exported sheets (in the case of a multi-sheet drawing)
• version
• export mode

After the exporting data to 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 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.

Both export options:

• If the sheet to export contains no geometry, or only non supported entities, no DXF/DWG file is generated.
• The visual clipping of views is not yet supported.
• Show/No Show:
  The V5 elements placed in the No Show are not exported. The visible elements are exported.
• Filters:
  To avoid missing geometries at export, we recommend that you activate either the filter All Visible or the filter None.
• Generative raster views are never exported.

Semantic export option only:

• If the check box Export dimensions as Dimensions is not selected, all dimensions are exported as graphic blocks and are editable as such.
• If the check box Export dimensions as Dimensions is selected, dimensions are exported as follows:
  • Circular, linear and angular dimensions are exported as true dimensions and editable as such.
  • The texts of those dimensions are exported with the STANDARD style and the isocp.shx font.
  • The tolerances of dimensions are now exported.
  • The "upper" and "down" texts are not taken into account.
  • Dual values are not exported.
  • Circular extension lines are not exported.
  • Half-dimensions are exported as graphic blocks.
  • Chamfer dimensions are exported as graphic blocks.
  • Dimensions that cannot be exported semantically are exported as graphic blocks.
• Layers are automatically exported.
  See Export layer name or Export layer number for more information.

• Texts:
  • All texts are exported as texts (even dimension texts and annotations) with a fit justification,
  • All texts are exported with the STANDARD style and the isocp.shx font with the exception of geometric
    tolerance symbols that are exported with the GDT specific style and gdt.shx font, with the corresponding mapping.
  • The symbols diameter Ø, degree °, plus/minus ± are inserted with the standard tags. 
  • Unicode characters are exported with the \U+ tag.
    You have to redefine the STANDARD style in AutoCAD to reference an unicode font.

Structures

The graphical representation of each file is transferred to the space of the AutoCAD model

The structure is not exported. 

The above applies to CGR, approximate, exact views.

Attributes

Exported implicitly through the graphic representation of text.

Annotations

Circular

Angular

The geometrical basic elements of each representation are exported

Semantic mode:

Linear, angular and circular dimensions are exported as such.
On option, each graphical representation of the elements is exported to an INSERT/BLOCK

Each graphical representation of the elements is exported to an INSERT/BLOCK

Geometry

2D POLYLINE

If the Version is set to DXF/DWG R12 or R13, they are exported as 2D POLYLINE.

If the Version is set to DXF/DWG R14 or above:

• Splines or NURBS originated from Interactive Drafting and Splines originated from exact views of Generative Drafting are exported into DXF Splines (with consistent graphical attribute such as color, line thickness and line type).

• The Spline or NURBS inside a 2D Component are not managed (they are still exported as 2D POLYLINE).

Only the generative exact view can contain Spline or NURBS.

Miscellaneous