Importing a DXF or DWG Drawing File
When you import DXF or DWG data into a drawing:
Draft entities are created using the units in the drawing setup file. For example, if the drawing setup file sets the units to inches, and the DXF or DWG data is in millimeters, the units are converted to inches during the translation.
DXF or DWG file values do not override all settings in the drawing setup file. For example, differences can exist in arrow size and style, text size, and parallel or horizontal dimensioning.
The arrow style of a dimension is stored in the BLOCK SECTION of a DXF file and is treated as part of the dimension picture. The Creo application, by default, does not retrieve any data from the dimension picture to recreate the dimension. Therefore, the arrow style of the dimension is lost when you import it.
AutoCAD entities that are on a blanked layer are imported and placed on a blank layer, after which you can change the display of this layer.
DXF blocks with symbols, and other details, especially of assemblies, are imported as separate symbols when you set the dxf_block_to_pro_symbol configuration option to yes.
A separate symbol definition is created for each block instance and placed in the appropriate location.
Specifying different 3D rotations for the block of drafting entities creates several block instances for each block definition. However, the 3D orientation property of the DXF block definition is not maintained. Yet each block instance is placed appropriately so that each block instance reflects its intended appearance when placed and viewed on a drawing sheet in AutoCAD.
Dimensions associated with draft entities before import retain their association to the same entities after the import of the DXF and DWG files. You can link nonassociative dimensions to the relevant draft entities after import. If there are geometry changes after import, you can recalculate dimension values before you associate dimensions with entities that are closest to the dimension witness lines.
The imported drawing can consist of 2D entities and 3D solids. The 3D solid entities are converted to components of an assembly. You can skip the 3D data in the file to selectively import the 2D data.
The imported drawing can have more than one layout or drawing sheet and can exist as a multiple-sheet drawing. The imported file can have both model space and paper space.
For a DXF file with multiple drawing sheets of variable size, the size of each drawing sheet in the imported drawing is maintained after import. If you set the intf_use_variable_size configuration option to no, for each sheet of the drawing, a standard-size drawing sheet that is nearest in size to the original drawing sheet is created.
You can import multiple-line text from a DXF file, with each line of the text in a different font, as multiple single-line notes or as a single multiple-line note. The fonts and styles of the multiple-line text are preserved in the single-line notes.
You can create a Draft View with related imported annotations. When importing DXF or DWG files, select the Import associative dimensions option. In the imported file, select all the annotations that need to be related to the draft view, along with the draft geometry chosen for the creation of the draft view. Ordinate dimensions are not imported as associative when importing DXF or DWG files. Hence, they cannot be associated with a draft view during its creation, but they can be related to an existing draft view.