SOLIDWORKS drawing view with assembly components displayed in different colours or line types
In a SOLIDWORKS drawing view, assembly components can be displayed in different colours using layers. Additionally, the type and thickness of the component edges can be specified using RMB option ‘Component Line Font.’
The Layers toolbar/dialog box can be activated from the View > Toolbars menu. Click New to add a layer and specify layer name, colour and line style.
Select the FeatureManager design tree of the drawing, expand the drawing view and expand the assembly to access assembly components. With the assembly component selected in the design tree, use the layer toolbar to assign a layer to the component. The assembly component immediately adopts the layer colour.
To change the line type and thickness of the component edges, right-click on it and select the option Component Line Font.
In the Component Line Font dialog, specify the line type and thickness using one of the following options:
- Use document defaults – line selection set in Tools > Options > Document Properties > Line Font.
- With the option ‘Use document defaults cleared,’ specify line style and thickness, or
- With the option ‘Use document defaults cleared,’ set line style and/or thickness to ‘Default’ to apply the line font of the layer selected in the Layer drop-down menu.
Additionally, select to apply these component settings to all views or to the selected views only (‘From selection’).
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