9 Replies Latest reply on Mar 15, 2018 12:56 PM by Tom Schrei

    Soldworks DXF Mapping- Layers????! HOW!!!?

    Tom Schrei

      Here at my work we etch sheet metal on our CNC Apelio. We can etch using layers. The Etching needs be on level 10 and red in color. Can anyone help me? If you can take this part and save a map. that would be awesome. There is nothing on the web about this!

        • Re: Soldworks DXF Mapping- Layers????! HOW!!!?
          Bob Van Dick

          Is this what you were looking for?

          • Re: Soldworks DXF Mapping- Layers????! HOW!!!?
            Shaodun Lin

            Hi Tom:

             

            Have you tried this:

            2014 SOLIDWORKS Help - Mapping Entities When Saving Drawings as .DXF or .DWG Files

             

            Mapping Entities When Saving Drawings as .DXF or .DWG Files

            You can map SolidWorks drawing entities and colors when you save drawings as .dxf or .dwg files to configure these entities and colors in the target files.

            You can map SolidWorks entities to layers, colors, or line styles you specify in the SolidWorks to DXF/DWG Mapping dialog box. You can also map exported colors.

            1. From a SolidWorks drawing, click File > Save As and select .dwg or .dxf as the file type.
            2. Click Options.
            3. For Custom map SolidWorks to DXF/DWG, select Enable and clear Don't show mapping on each save.
            4. Click OK.
            5. Type a name for the file, select a file location, and click Save.The SolidWorks to DXF/DWG Mapping dialog box appears.dwgdxfmappingdialogboxtorn.gif
            6. In the SolidWorks to DXF/DWG Mapping dialog box, specify the mappings:
              • Click Load Map File to upload mappings from a file.
              • Manually specify layers, map entities, or color mappings.
            7. To save DXF/DWG export map file settings, click Save Map File.
            8. Click OK.

             

            Saving and Loading Map Entities

            When exporting drawings as .dxf or .dwg files, you can save .dxf or .dwg entity property mappings in a map file and load them the next time you save a SolidWorks drawing to either file type.To save or load entity property mappings when exporting SolidWorks drawings to .dwg or .dxf files:

            1. Follow the main procedure for mapping entities through step 5.
            2. Save or load entity and color mappings:
              • From the SolidWorks to DXF/DWG Mapping dialog box, specify layers, and map colors and entities, and click Save Map File to save property mappings.
              • Click Load Map File to load previously saved property mappings.
            3. Browse to a folder and enter a file name.
              • Click Save to save property mappings to a map file.
              • Click Open to load a map file with saved property mappings.
            4. Click OK to close the SolidWorks to DXF/DWG Mapping dialog box and export the file.

            Defining Layers

            When exporting drawings as .dxf or .dwg files, you can define layers in the SolidWorks to DXF/DWG Mapping dialog box.To add or edit a layer:

            1. Follow the main procedure for mapping entities through step 5.
            2. Under Define Layers, select the row for the layer and do the following:
              1. Click in the Layer column and type a number or name for the new layer.
              2. Click in the Color column for the layer and select an item from the grid.
              3. Click in the Line Style column for the layer, and select a line style.
            3. Repeat Step 2, as required, to specify other layers.
            4. Specify map entities or colors as required.
            5. To save DXF/DWG export map file settings, click Save Map File.
            6. Click OK.

            Mapping Entities

            When exporting drawings as .dxf or .dwg files, you can map entities in the SolidWorks to DXF/DWG Mapping dialog box.To map entities:

            1. Follow the main procedure for mapping entities through step 5.
            2. Under Map Entities, select the row for the entity and do the following:
              1. Click in the Layer column and select a layer.You must define the layers before you can map the entities.
              2. Click in the Color column for the layer and select an item from the grid.
              3. Click in the Line Style column for the layer, and select a line style.
              4. Click in the Entity column, and select an entity to map.
            3. Repeat Step 2, as required, to map other entities.
            4. Specify map colors as required.
            5. To save DXF/DWG export map file settings, click Save Map File.
            6. To apply the mapping file settings only to those entities whose layers are not defined as SolidWorks drawing file layers, click Only map entities that are not on SolidWorks layers.
            7. Click OK.

             

            Mapping Colors

            When exporting drawings as .dxf or .dwg files, you can define the color mapping from SolidWorks to the target file in the SolidWorks to DXF/DWG Mapping dialog box.To map colors when saving drawings as .dxf or .dwg files:

            1. Follow the main procedure for mapping entities through step 5.
            2. Under Map Colors, specify a color mapping:
              1. Click the next empty row in the SolidWorks swcolorscolumkn.gif column, and select a color from the grid for the source file.
              2. Click in the DXF/DWG dxfcolors.gif column and select mapped color for the target file.
            3. Repeat Step 2, as required, to map other colors.
            4. To save DXF/DWG export map file settings, click Save Map File.
            5. Click OK.
            • Re: Soldworks DXF Mapping- Layers????! HOW!!!?
              Kevin Chandler

              Hello,

               

              I think the issue is the different approach to layers in the two programs.

              SolidWorks follows AutoCAD in naming a layer. They're may be some internal layer index, but only the layer name is exposed and that's the working handle.

               

              In the layer list screen shots, the "10" layer is an absolute number. It's the tenth layer.

              To get ten layers in SolidWorks, you have to add ten named layers.

               

              To get the mapping to work (I think), you'll need nine layers so that you can assign named layer "10"  for the entities to be mapped to the tenth (layer count) layer.

               

              Cheers,

               

              Kevin