About Exporting Drawings to DXF or DWG Files
You can export drawing data to the DXF and DWG formats of AutoCAD version 2018 or earlier. Version 2018 of the DXF and the DWG file formats is the default for export.
The Creo Parametric Interface for DWG uses RealDWG technology.
You can use the File > Save As > Save a Copy command to export drawings to the DXF and DWG formats. If you use File > Save As > Export, you can preview the current export settings of the drawings before you export them as publish deliverables to the DXF or the DWG format. If the drawings do not suit your requirements, the Export Setup tab enables you to modify their export settings before you export them. You can change the export settings in the Export Environment for DXF or the Export Environment for DWG dialog box. Additionally, you can set the preferred_export_format configuration option to dxf or dwg and click File > Save As > Quick Export to directly export the drawings to these formats without changing their export settings.
The Export Environment for DXF and the Export Environment for DWG dialog boxes display options specific to the respective file types and the type of entities these file types support for export. These options depend on the additional configuration options that you set. Standard Creo colors, layers, and line styles map automatically to standard default AutoCAD properties. You can also manually map these properties and text fonts. By default, all text is exported based on the font and character coding. However, you can configure Creo to stroke text characters during export to AutoCAD.
The Model Tree hierarchy of assemblies and components can be included in the file for export. In the Export Environment for DXF or the Export Environment for DWG dialog box, you can specify that the assembly structure for export as nested blocks.
The log files created during the export contain details about the export such as the file versions, the configuration options settings, the assembly structure representations as blocks or layers, the export of text as text or geometric entities, and so on. You can verify and edit the information in the Information Window and save the log files after the export. The details of the export are as follows:
Splines or B-splines are exported to the DXF format as splines.
Construction lines are exported to the DXF format as XLINEs.
Draft hatches are exported to the DXF format as hatches. Draft hatches create AutoCAD UDF hatches.
Multiple-line note is exported to the DXF and DWG file formats as a single MTEXT entity or as multiple TEXT entities.
Ellipses are exported as ellipses.
Notes with leaders are exported as AutoCAD leadered notes.
Tables are exported as AutoCAD tables.
Unicode characters are exported as is to the DXF versions below 2007 when the intf2d_out_acad_unicode configuration option is set to yes.
DWG and DXF Blocks
Using the intf_out_layer configuration option, you can export the user-defined symbols and drawing groups through DXF and DWG as blocks, making it is easier to modify the exported drawings. Two-dimensional representations of individual components with their drafting entities for each view within an assembly are also translated as blocks.
Use the Intf2d_out_acad_norm_annot_block configuration option to export annotations with multiple normal leaders to DWG and DXF as blocks.