Support Sheet: DWG/DXF Import for SolidWorks _____________________________________________________________________ The following example illustrates the different steps involved in importing a DWG/DXF Import for SolidWorks DWG/DXF into SolidWorks. Use the Recommended AutoCAD settings If the DWG/DXF was created in AutoCAD, please ensure that you are using the recommended AutoCAD settings (i.e. please read Javelin FAQ on Recommended AutoCAD settings) Drag and drop the DWG/DXF into SolidWorks from Windows Explorer You can also open a DWG/DXF in SolidWorks, from the main menu click File, Open. The DWG/DXF Import Wizard is launched automatically when you drag and drop a DWG/DXF into SolidWorks. DXF/DWG Import Wizard Overview The DXF/DWG import wizard imports DXF or DWG files into SolidWorks by guiding you through required steps. You have the option of importing to either a drawing or a part. If you import to a drawing, the layer, color, and line style information in the DXF or DWG file is also imported. Import to a new drawing Generally, we recommend importing to a new drawing instead of importing to a new part. This is because most DWG/DXF files contain title blocks, annotations and other information that is not needed in a part. Once you have imported into a drawing you can copy the geometry from the drawing into a part sketch. DXF/DWG Import - Document Settings You can set the drawing document options using this dialog box, which appears only if you import to a new drawing document. SolidWorks attempts to make the best settings based on the imported file data, but you can adjust the options as necessary. IMPORTANT: Select the Show preview check box to see a preview of the drawing on the drawing sheet. DXF/DWG Import - Drawing Layer Mapping You can set the drawing sheet format using this dialog box, which appears only if you import to a new drawing document. After I import a DWG/DXF into SolidWorks I get a “dimensions that differ from the actual measured value” error message. What does this mean? The SolidWorks preference is to leave the dimscale factor = 1. If you get this error message, usually it means that the dimscale factor was changed in some or all the views. Constrain All You can set relations on the sketch entities of an unconstrained imported DXF or DWG file. To solve relations in an imported drawing: Click Tools, Relations, Constrain All. The SolidWorks software adds all the apparent relations and reports the number of relations that are added. IMPORTANT: You should do a “Constrain All” right after importing a DWG/DXF, since this option is no longer available once you start working with the document. Attach Dimensions You can attach the dimensions to the nearest reasonable sketch entities all at once. To attach dimensions: With an imported .DXF or .DWG drawing document active, click Tools, Dimensions, Attach Dimensions (this converts the AutoCAD dimensions into SolidWorks driving dimensions). IMPORTANT: For this to work you must have the AutoCAD parameter Dimasso "dimension associative" = ON. Hide any layers that you will not be using Generally, all you need to see are the dimensions and the geometry (i.e. you don’t need title blocks, center marks, annotations) Copy the geometry and dimensions into a Part Sketch If you want to use a drawing profile in a Part Sketch you can select the geometry and dimensions in a drawing then click Copy, open a Part Sketch and click Paste. You can also use the “Insert Drawing” command; however, the “Insert Drawing” command does not copy dimensions. I can not copy a drawing into a Part Sketch, I get a “cannot complete copy” error message. What does this mean? SolidWorks will not allow you to copy annotations into a Part Sketch. Usually, this means that you have selected some annotations. Make sure that you only select geometry and dimensions when you copy. Make sure that all annotations are in a separate layer so that you can hide them. I copied a drawing profile into a Part Sketch, how can I translate the entire Sketch to the Part origin? When I try to drag the Sketch it changes shape. Your Sketch changes shape, because your Sketch does not have all the necessary relations. The best way to move the Sketch to the origin is to use the command “Tools, Sketch Tools, Modify”. This command can be used to translate a Sketch to the origin or any other location. To use it from the main menu click Tools, Sketch Tools, Modify. While the Modify Sketch dialog box is open, you can the drag the Sketch and you will see that the Sketch does not change shape when you move it (i.e. the entire Sketch moves). Think of this as a translate command. Click on View, Origins. Now you can drag the Sketch into the Part origin. I copied the drawing profile into a Part Sketch, what do I do next? Depending on the application you may want to use this Sketch as a layout Sketch, or maybe you want to use it to model a Part (i.e. you can extrude, or revolve it).