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
2D drafting apps such as
DraftSight®
and
AutoCAD. |
View export options
Export views as blocks |
Exports
geometry in drawing
views
as blocks. |
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. |