New Sheet Metal Commands in Inventor 2008 (Avatech Tricks Tutorial)

The Flange tool's new Loop option and the Annotation Panel's Bend Notes are great ways to work effectively with sheet metal.

First start with a sheet metal template and create a sketch that you will turn into a face. Mine is 6" X 3". Use the Face tool on the Sheet Metal Features toolbar to create a sheet metal face by adding thickness to a sketched profile. If it is the first feature created, it is the base feature.

Next set your sheet metal style. Notice that you have multiple gauges defined in the template. Select your own or simply use Inventor's default size. Use the Sheet Metal Styles tool on the Sheet Metal Features toolbar to edit the style options and parameters for a sheet metal part. Most of these options and parameters apply to the entire part.

By default there are no defined styles. Simply enter the thickness of your metal.

Use the Face tool on the Sheet Metal Features toolbar to add a sheet metal face and a bend to an existing sheet metal face. You can specify the depth and the angle of the flange and whether it is created inside or outside the existing face. You can also specify the width or offset of the new flange.

This creates the base face.

Face dialog box with included options.

After creating the face, use the Flange tool from the Sheet Metal panel bar.

Choose the Loop option.

1. Click the Flange tool.

2. The Flange command initializes with the Edge Select Mode button active, and you are prompted to select an edge. Instead, select the Loop Select Mode button. You are now prompted to select a loop. The flange around the edge loop will be formed using the values you enter and using the corner option specified by the sheet metal style or as optionally altered on the Corner tab.

3. Set a distance for the height of the flange.

4. Specify an angle for the flange (if other than the default of 90 degrees).

The Green preview indicates allowable values.

Now that you have your folded version, you need to create a flat pattern for manufacturing.

Use the Flat Pattern tool on the Sheet Metal Features toolbar to create a flat pattern of a sheet metal model. Before you create the flat pattern, you should select the desired base face. Autodesk Inventor unfolds the part using the selected face as the base face. Note: Preselect a curved face to create a flat pattern from a part converted to sheet metal created using only conical or cylindrical features.

Selected base face prior to unfolding.

Representation of the flat pattern.

Annotating Flat Patterns
Once you have a drawing ready to create views, notice the Flat Pattern Option in the View Creation dialog box.

Drawing view option found in View Creation of IDW/DWG.

Now that a view of the flat pattern is created, use the Bend Note command (found under the Drawing Annotation panel and submenu under Hole/Thread Notes) and select the bend lines displayed in the view. A bend note adds fabricating information to sheet metal bend centerlines. Bend notes are associated with a drawing view. Each individual bend centerline is treated as an individual bend object in the drawing (with respect to both bend notes and bend tables).

Found under the Drawing Annotation panel and submenu under Hole/Thread Notes.

As you can see, Inventor provides efficient tools designed to make engineering sheet metal components and annotations faster and easier, allowing you to focus on the design rather than feature creation. The figure below shows an example of the detailed Sheet Metal component.

Flat pattern, detail, and ISO view.