Understanding DXF/DWG Layer Mapping for Sheet Metal
Understanding DXF/DWG Layer Mapping for Sheet Metal
Mapping entities by type to a specific color and line format layers is a useful tool when converting SOLIDWORKS files to 2D drawing exchange formats like DXF or DWG. Groups of entities can be assigned to specific layers. Named layers are commonly used by CNC sheet metal cutting post-processing software to assign processing methods automatically. For example, post-processing software can be configured to always scribe/etch entities assigned to a DXF layer named SCRIBE. With a little bit of up-front configuring, SOLIDWORKS makes it easy to map entities to specific layers repeatedly when converting from SOLIDWORKS Sheet Metal to DXF or DWG files.
System Options
A quick change to SOLIDWORKS System Options is required to activate the SOLIDWORKS To DXF/DWG Mapping.
1. Select Tools > Options > System Options.
2. Select the Export category.
3. From the File Format dropdown list, select DXF/DWG.
4. For Custom Map SOLIDWORKS to DXF/DWG, turn on Enable Map file.
5. The file location will populate automatically the first time a mapping file is created and saved. This location can also be changed on-the-fly for different DXF/DWG requirements.
6. Click OK to save the options changes.
DXF/DWG Output Options
With a sheet metal part open, either right-click a face of the part and select Export to DXF/DWG or select Save As from the File dropdown list and then select DXF or DWG as the file type.
In the Properties Manager, select Sheet Metal as the Export type and then select which Entities To Export.
For this example:
Geometry = the edges of all visible geometry (perimeter and holes)
Bend Lines = all sheet metal bends
Sketches = the visible sketch on the center of the part (sketches must be visible to map using Sketches)
Click the Green Checkmark to accept the options.
Defining the Mapping Layers
Once you accept the DXF/DWG Output options, a dialog opens to configure the layers. After defining the layers the first time, you can then use Save Map File… to save a template and map entities repeatably.
1 Define Layers:
The Define Layers section are the layers you want to create in your DXF/DWG. To create a new layer, enter any text to name the Layer, select a color from the color pallet, then select a Line Style from the dropdown list.
For this example, we created CUT, SCRIBE, BEND-UP, and BEND-DOWN
2 Map Entities:
The Map Entities section allows you to map SOLIDWORKS Entities To Export to the DXF/DWG Define Layers created in the left column.
For this example, we assigned Geometry to the CUT layer, Sketches to the SCRIBE layer, and the Bend lines to their associated BEND-UP and BEND-DOWN layers. To map both bend directions to the same layer, simply select the same Define Layer from the Layer dropdown list (center column).
Once satisfied with your selections click OK to create the DXF/DWG with the mapped layers.
Map Colors (right column) can be used to map a specific SOLIDWORKS color to a different color in the DXF/DWG. For example, you could map Black to White or Green to Red using the Map Colors section.
Click Save Map File… to save the Define Layers for use later. Click Load Map File… to switch between mapping templates with different Define Layers.
Review the DXF/DWG File
The DXF/DWG is created with the correct layer names, colors, and line styles.
Final Note
To repeatably create DXF/DWG files with the same mapped layers, make sure to activate Enable Map file and set the file location to your saved mapping file.
If you will always use the same mapping file and no longer want to see the SOLIDWORKS to DXF/DWG Mapping dialog which displays the layer configuration, then activate the option Don’t show mapping on each save. SOLIDWORKS will then use the specified mapping file to map all entities to the Define Layers.
