To Work with Surfaces in Drawing Views

How to show and hide surfaces for best results in drawing views and to support annotations.

When you create a view of a part file that contains only surfaces, only the surfaces that are set to Visible appear in the drawing view. After view creation, any surfaces in the corresponding part file that are set to Invisible will no longer display in the drawing file.

After you create a drawing view, you can include or exclude surfaces from drawing views. Files that contain only surfaces automatically include the surfaces in a drawing view.

A drawing view can include open or closed surfaces, model surfaces, thickened surfaces, or derived surfaces. A drawing view cannot include construction surfaces. You must first use Copy Object to place construction surfaces to the part environment before including them in a drawing view.

Drawing Views of Models with a Mixture of Solids and Surfaces

The workflow differs according to the combination of bodies and surfaces in a file:

• When creating a view of a part or (in Inventor) assemblies that contain parts with a solid body and one or more surfaces, surfaces are excluded from the view by default. You can include or exclude individual surfaces from a view. New surfaces added to the part file must be manually included to show in the view.
• For a part with only surface bodies but no solid body, all surfaces are included by default in a drawing view. You can include or exclude individual surfaces from the view. New surfaces added to the part file are automatically added to the view.
• Assemblies (not available in Inventor LT) that contain parts with only surfaces do not automatically recover surfaces in drawing views. You must include them manually.

Surfaces in Child Views

After you create a base (parent) view in which you have included or excluded surfaces, newly created child views inherit the same visibility characteristics.

If a child view already exists, including or excluding surfaces on the parent view does not update the child view. You must include or exclude surfaces in each child view individually.

In Inventor, in assemblies with a mixture of surfaces and solid parts, surfaces are not automatically included in drawing views. You must include them manually.

In section and breakout views, hatching does not show on regions defined by a surface. Hatching is visible only on a solid body.

Edges and Annotations for Surfaces

You can apply edge properties to surface edges and model edges.

After a surface is included in a view, you can apply annotations to surface view edges. Surfaces are not counted separately from the part for parts list quantities.

Create Views Containing both Solid Bodies and Surfaces

By default, when you create a view of a part that contains solid bodies and surfaces, the view contains solid bodies but no surfaces.

Inclusion or exclusion of surfaces in child views is the same as the base (parent) view. If you include or exclude surfaces in a parent view after child views are created, they are not reflected in the child views.

1. On the ribbon, click Place Views tab Create panel Base.
2. In the Drawing View dialog, select a part (or assembly file in Inventor) that contains parts with a mixture of solids and surfaces.
3. On the Component tab, specify view Orientation, Scale, Label, and Style.
4. On the Options tab, specify Reference Data, a Positional Representation (if applicable) and Display preferences. Click OK to create the view. (In Inventor LT, on the Options tab, specify Display preferences, and click OK to create the view. By default, the view contains solid bodies, but no surfaces.)
5. In the browser, expand the file folder and right-click a surface. On the context menu, select Include to add the surface to the view.
6. (Optional) Continue to create views and add surfaces to views as needed.
7. (Optional) To remove a surface from a view, right-click the surface in the browser and clear the Include check mark.

Create Views Containing Surfaces but No Solid Bodies

After you create a view that contains surfaces but no solids, the view in the graphics window automatically includes surfaces. Surfaces are included in dependent views based on their inclusion or exclusion from the base (parent) view.

1. On the ribbon, click Place Views tab Create panel Base.
2. In the Drawing View dialog, click the arrow on the File box, and select a part file that contains only surfaces.
3. On the Component tab, specify view Orientation, Scale, Label, and Style.
4. On the Options tab, specify Reference Data, a Positional Representation (if applicable) and Display preferences. Click OK. (In Inventor LT, on the Options tab, specify Reference Data and Display preferences. Click OK.)
5. On the Options tab, specify Display preferences. Click OK.
6. If appropriate, right-click a surface in the browser and clear the Include check mark to remove the surface from the view.
7. (Optional) In a drawing of an assembly, use Include to add surfaces to drawing views manually.
8. Continue to create views as needed.