Creating DXF Files In SolidWorks

3D (-1)

(Exporting 2D DXF files) We design in a 3D world, but many parts are manufactured from flat sheet. The flat pattern of a sheet metal part and flat plates used in weldments are examples. Laser and waterjet cutters of flat parts may want to use a DXF file instead of native geometry. Let’s look at several ways to create DXF files.

Option 1 File > Save As > DXF is the most general method. The dialog at the right requires several inputs from the user: Be sure to select a view that is normal to the flat part and deselect the others. The output alignment tools specify the X and Y axes and whether the part is flipped on an axis.
Option 2 For an inherently flat part or an unfolded sheet metal part, right click on the face and select Export to DXF/DWG from the context menu. In this case, there’s no dialog to select a view because the face determines the view. This workflow is a little faster.
Option 3 You can also right click the Flat Pattern feature in the Feature Manager to see a different dialog. For cutting only, just select Geometry as the entities to export and set Output Alignment as desired.  

There’s yet another way to do this. One of our customers wanted to make a SolidWorks drawing as an intermediate step, but the title block, dimensions and annotations were exported to the DXF and interpreted by the laser cutter as actual geometry.

There’s a solution: Create a second sheet and edit Sheet Properties so no format is displayed. Set the sheet scale to 1:1. Return to Sheet 1, select the Flat Pattern view and Control-C to copy it. There may be a warning that not all items in the view can be copied, but ignore it. Change to Sheet 2, left click anywhere on the sheet and Control-V to paste a copy of the flat pattern view. Now delete any dimensions and annotations. Right click the bend lines and Hide. There will be a message that bend notes will be hidden as well. Click Yes to continue. The desired result is Sheet2 that contains nothing but the outline geometry of the flat pattern, with no notes, annotations, title block etc.

Finally File > Save As > DXF, click the Options button and select “Export active sheet only” > OK > Save

The drawing now serves two purposes: Sheet1 is fully dimensioned and annotated as a design document, while Sheet2 is never printed but used only for DXF export.


Art Woodbury is an Applications Engineer  at CAPINC, a SolidWorks Value Added Reseller with locations across New England. He is a regular contributor to their CAPINC University blog.

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