Selecting Base Scale for Exporting SOLIDWORKS Drawings to DXF/DWG

When exporting SOLIDWORKS drawings to DXF/DWG format, scale factor needs to be taken into consideration to avoid incorrect dimensions and a potential loss of material.

Changing scale in a SOLIDWORKS drawing view does not affect dimensions displayed as they are parametrically linked to the part or the assembly file shown in the view.  It is expected in SOLIDWORKS that drawing views with different scale factors show the same model dimensions.  This concept of multiple scales does not apply to DXF/DWG files where scale change does affect model dimensions.  When SOLIDWORKS drawings are exported to DXF/DWG format, all drawing views and sheet-format items are converted using a single scale factor.  If SOLIDWORKS drawing includes views of different scales, some of them will inevitably measure incorrectly when converted to DXF/DWG format.

In the SOLIDWORKS ‘Save As’ dialog, the Options button becomes available after the file type is selected for the export.  In the export options for DXF/DWG files, it is not sufficient to enable scale output 1:1 because the result of the conversion also depends on the selected base scale.  For example, selecting the base scale of 1:2 means that the content of the drawing will be enlarged two times (2:1) during the conversion so that any views with the scale 1:2 end up with the 1:1 output in the DXF/DWG file, measuring correctly.  However, the same base scale of 1:2 applied to SOLIDWORKS views that are scaled differently (eg. 1:4) will produce incorrect dimensions when those views are measured in the DXF/DWG file.

The pull-down menu for base scale lists all scale factors found in the sheet format and in all views present in the drawing, showing the number of views using the same scale.

SolidWorks Export Options

If the export option ‘Warn me if enabled’ is selected, a warning comes up when different scales are found in the drawing, indicating that some items will measure incorrectly in the DXF/DWG file.

SolidWorks Warning – DXF export

Views using the same scale as the base scale for the export produce correct measurements in DXF/DWG file.  Views whose scale is different than the base scale measure incorrectly after the export.

Scale options for exporting SOLIDWORKS drawing to DXF/DWG

Measured in DXF/DWG file, view whose scale did not match the base scale used in the export has incorrect dimensions

To avoid incorrectly scaled geometry in DXF/DWG Export

It is suggested to:

1. Apply the same scale to all views of the drawing being exported to DXF/DWG format
2. Select view scale as a base scale for the export as opposed to selecting sheet scale

A step further would be to apply the same scale to all views and the sheet format.  There is no other way to predict or pre-set base scale for DXF/DWG conversion.  Some users like to apply scale factor of 1:1 to all views and the sheet format, which eliminates a chance for error in SOLIDWORKS drawings exported to DXF/DWG format.  SOLIDWORKS users that regularly convert drawings to DXF/DWG format typically have a drawing template with the sheet scale set to 1:1 scale.