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:
Click File,
Save As.
Select Dxf (*.dxf)
or Dwg (*.dwg) file for Save as type, then click Options.
In the Export
Options dialog box, select from the options described below, then
click OK.
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
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