You can set file export
options
when you export SOLIDWORKS drawing documents as .dxf or
.dwg files.
To select these options when saving a file as a
.dxf or .dwg file:
In
the Save As dialog box, click Options.
3DEXPERIENCE
Users: If the Save As New
dialog box appears, click Save to This
PC.
Specify
options and save the
file.
General Options
| Version |
Selects the target AutoCAD® version. |
| Fonts |
Select one of the following:
|
AutoCAD Standard Only
|
Uses the
drawfontmap.txt
mapping file.
|
|
TrueType
|
|
|
| Line Styles |
Select one of the following:
|
AutoCAD Standard Styles
|
Maps SOLIDWORKS line fonts to AutoCAD stock line types. For AutoCAD version R2000 and later, also maps line font weight to the closest AutoCAD line weight value.
|
|
SOLIDWORKS Custom Styles
|
Uses SOLIDWORKS software line styles.
|
|
Custom Map SOLIDWORKS to DXF/DWG
| Enable |
Exports mapping specified in the selected map file. |
| Map file |
Specifies the default target map file. |
| Don't show mapping on each save |
When you select a map file, suppresses the SOLIDWORKS to DXF/DWG Mapping dialog box when you export. |
Scale output 1:1 (Drawings only)
| Enable |
Exports the drawing using a model geometry scale of 1:1 according to your selected base scale. The paper or sheet scale is not normally used when you enable this option.
|
| Base scale |
Selects 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 selected a view, the base scale options include the View scale and Count values for the view. Otherwise, the view scale with the highest count is displayed. Count indicates the number of occurrences of this scale in the drawing document. Views are grouped by scale. If you enable 1:1 scaled output, the group with the largest number of views is exported with a 1:1 scale, and the remaining views are scaled correspondingly. If the drawing contains no views, the sheet is exported with a 1:1 scale.
|
| Warn me if enabled |
Displays a warning message when you enable sheet scaling. If you turn off these warning messages when one appears, you can turn them on again from this option.
|
Scale Output 1:1 Warning Message Options
| Disable
1:1 Scale |
Turn off the export scale option
for this and subsequent export operations. |
| Don't
warn me about this any more in this SOLIDWORKS
session |
Turn off the warning message. You
can turn it back on in the DXF/DWG File
Export Options. |
This
warning message appears
when
exporting DXF/DWG files with Save
As:
- If you click Options in the Save As dialog box and select Scale output 1:1, the option is observed and no warning is
issued.
- In subsequent exports, if you:
- Do not click Options, a warning is issued
- Do click Options, no warning is issued (You do not have to
select anything in the Export
Options dialog box, only open it and click OK.)
- If you select Don't warn me about this any more in this SOLIDWORKS
session in the warning dialog box, no warning appears for
subsequent exports. To turn the warning back on, click Options in the Save As dialog box and select Warn me if enabled.
End point merging
| Enable merging |
Eliminates gaps between line endpoints for gaps less than the specified tolerance. |
| High quality DWG export |
Exports at a higher level of quality. Selecting this option might increase the export time.
|
Spline export options
| Export all splines as splines |
|
| Export all splines as polylines |
Displays splines as polylines in AutoCAD. |
Multi sheet drawing
| Export active sheet only |
|
| Export all sheets to separate files |
Writes each drawing sheet to a file of the specified file
name, prepended by a number. For example, 00_filename.dwg and 01_filename.dwg. |
| Export all sheets to one file |
|
| Export all drawing sheets to paper space |
Exports drawing sheets to paper space rather than model space. |