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DXF/DWG File Export Options

Set options when you export drawing documents as DXF or DWG files.

To set the DXF or DWG file export options:

  1. Click File, Save As.

  2. Select Dxf (*.dxf) or Dwg (*.dwg) file for Save as type, then click Options.

  3. In the Export Options dialog box, select from the options described below, then click OK.

  4. Click Save to export the document.

Version. Select the type supported by the target system. The SolidWorks DXF and DWG file translators support all AutoCAD® versions up to and including AutoCAD 2007.

Fonts. Select either TrueType or AutoCAD STANDARD only. If you select AutoCAD STANDARD only, the drawFontMap.txt mapping file is used. See AutoCAD Font Support for details.

Line styles. Select AutoCAD Standard Styles to map SolidWorks line fonts to the original AutoCAD stock line types. Line font weight is mapped to the closest AutoCAD line weight value. AutoCAD line weight value mapping is only supported for AutoCAD Version setting R2000 and higher. Select SolidWorks Custom Styles to use the SolidWorks line styles.

Custom Map SolidWorks to DXF/DWG. Implements mapping. See DXF/DWG File Mapping.

  • Don't show mapping on each save. Prevents the SolidWorks To DXF/DWG Mapping dialog box from appearing every time you save a drawing with Custom Map SolidWorks to DXF selected. The map file specified in the Map file box is used.

  • Map file. Select a previously saved map file, or browse to the desired file.

Scale output 1:1. Exports the drawing using a model geometry scale of 1:1 and enables the Base scale list. The paper or sheet scale is not normally used when you enable this option.

  • Select Warn me if enabled to see a warning message. You can turn the warning off in the warning dialog box, and this option allows you to turn it back on.

  • Base scale. Refers to the basis used for the 1:1 scale output of the geometry, based on the various drawing view scales on the sheet. If you have a view selected, the view scale and count values for this selected view appear in the Base scale list. If no view is selected, the view scale with the highest count is displayed by default. Count indicates the number of occurrences of this scale in the drawing document.

Views are grouped by scale. If you select 1:1 Scale output, the group with the largest number of views is exported with 1:1 scale, and the remaining views are scaled correspondingly. If the drawing contains no views, the sheet is exported with 1:1 scale.

End Point Merging options

  • Enable merging. If enabled, specify the tolerance within which gaps between line endpoints are eliminated.

  • High quality DWG export. Available when Enable Merging is selected. Exports at a higher level of quality but can increase the time required to export.

Spline export options

  • Export all splines as splines

  • Export all splines as polylines. Splines display as polylines in AutoCAD.

Multiple sheet drawing. If your drawing document contains more than one drawing sheet, choose from:

  • Export active sheet only

  • Export all sheets to separate files. The filenames are serialized (00_<filename>.dwg, 01_<filename>.dwg, etc.)

  • Export all sheets to one file



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