Create Overlay drawing views using positional representations to show an assembly in multiple positions in a single view. You can also create an Overlay to emphasize certain parts or components by showing them as solid lines or shaded, while the rest of the components appear dashed. This method does not require a positional representation to create an Overlay.
Overlay views are available for unbroken base, projected, and auxiliary views. Each overlay view can reference a view representation independent of the parent view.
In the drawing browser, overlay views are shown as child nodes to the parent view. You can right-click an overlay view node to open the model file using the representation set by the overlay view.
Add dimensions between different positional representation overlays in the master view to show the distance a component has moved. Drawing dimensions automatically update if the model position changes.
Guidelines for Working with Overlay Views
- In the assembly, create view representations that show only components of interest. For an uncluttered overlay view, specify a view representation when placing the overlay view.
- An overlay view can be associative to a defined view representation.
- A positional representation can be used in multiple overlay views. In the assembly file, create as many positional representations as necessary to show different positions.
- To change to a different positional representation for an overlay view, delete the overlay view and specify a new positional representation when placing a new overlay view.
- If you delete a positional representation in the model, the drawing view reverts to the master positional representation.
- Overlay views cannot be moved from their parent views or copied. The parent view can be moved or copied but overlay views are not included.
- The view can be different from the parent view, and each overlay view can use a different view representation.
Create Overlay Views
- On the ribbon, click
Place Views tab
Create panel
Base, and then in the Drawing View dialog, specify the assembly file and the view representation.
- On the ribbon, click
Place Views tab
Create panel
Overlay, and then click the base view.
- In the Overlay View dialog, do one of the following:
- On the Positional Representation box, click the arrow and select a positional representation.
- On the View Representation box, click the arrow and select a view representation.
- Edit the overlay view as desired.
- (Optional) Use Positional Representations to add additional overlay views to the base view to show the assembly in various positions.
- (Optional) Create additional projected and auxiliary views and create overlay views for each.
Edit Overlay Views
You use the Edit Overlay dialog to edit overlay views. If you want to use a different positional representation for the overlay view, delete the overlay view and recreate the view, specifying the positional representation in the Drawing View dialog.
- Right-click an overlay view in the drawing browser and select Edit View.
- In the Overlay View dialog:
- On the View Representation box, click the arrow and specify a view representation. If desired, enable Associative to update the view when changes are made to the view representation in the assembly environment.
- In the Label box:
- Clear the Use Positional Rep Name check box to enter a new name or accept the default.
- If appropriate, click Toggle Label Visibility to change the visibility of the view label.
- Click Edit View Label to edit the view label in the Format Text dialog.
- In the Display box, select:
- Tangent Edges to show tangent edges.
- Foreshortened to shorten the length of tangent edges to distinguish them from visible edges.
- Work Features to display them on the view.
- In the Style box, select:
- Hidden Lines, Remove Hidden Lines, or Shaded display style.
- Style from Base to show the overlay view in the same line style as the parent view.
- For Layer, click the arrow and select:
- As Overlay to set view items to the line style specified by the Layer style.
- As Part to show standard lines styles used in the part model. Components marked as Reference displays in the reference layer style.