This chapter explains how to create sheet metal drawings. Gauges for sheet metal are presented along with bend radii, flanges, tabs, reliefs, and flat patterns.
Sheet Metal Drawings
Figure 13-1 shows a 3D solid model of a sheet metal part and a dimensioned orthographic drawing of that part. The orthographic drawing was created from the 3D model. The following sections explain how to create the 3D sheet metal drawing.
Exercise 13-1Creating a 3D Sheet Metal Drawing
Create a new drawing using the Sheet Metal (mm).ipt format.
See Figure 13-2. The Sketch panels will appear. See Figure 13-3. Sheet metal drawings are initiated as 2D sketches, then developed using a combination of Sketch and Sheet Metal panel tools.
Click the Start 2D Sketch tool, select the XY plane, and use the Two Point Rectangle tool and draw a 20 × 50 rectangle.
Move the cursor into the area of the ViewCube and click the icon that looks like a house (the Home tool).
Right-click the mouse again and select the Finish 2D Sketch option.
The Sheet Metal panels will appear. See Figure 13-4. Not all tools will be active at this time, but they will become active as the drawing progresses.
Select the Sheet Metal Defaults option located on the Setup panel under the Sheet Metal tab.
The Sheet Metal Defaults dialog box will appear. See Figure 13-5. The Sheet Metal Defaults dialog box is used to define the thickness, material, and bend characteristics of the part.
Inventor has many default values already in place. Figure 13-5 shows that the default thickness is 0.500 mm. Sheet metal is manufactured in standard thicknesses. Figure 13-6 is a partial listing of available standard sheet metal thicknesses in inches, and Figure 13-7 is a partial listing of sheet metal thicknesses in millimeters.
Figure 13-5 lists 0.500 mm as a standard thickness, so this default value will be used for this example. Click the checkmark in the Use Thickness from Rule box. There should be no checkmark in the box. Set the Material Style for Aluminum-6061.
Accept the 0.500 mm Thickness value, then click OK.
Select the Face tool from the Create panel located under the Sheet Metal tab.
Select the sketch, and click OK.
The 20 × 50 panel will now have a thickness of 0.50. See Figure 13-8.
Bend Radii
As sheet metal is bent, the inside surface is subjected to compression, and the outside surface to tension. These forces cause the material to stretch slightly.
To edit the bend radius for a sheet metal part:
Click the Sheet Metal Defaults tool listed under the Sheet Metaltab.
Click the pencil icon next to the Sheet Metal Rule box in the Sheet Metal Defaults dialog box. See Figure 13-9.
The Style and Standard Editor dialog box will appear. See Figure 13-9.
Click the Bend tab. See the bottom dialog box in Figure 13-9.
The Relief Depth and Minimum Remnant values shown on the Style and Standard Editor dialog box are calculated based on the thickness value specified in the Sheet Metal Defaults dialog box. This defines the Relief Depth as 0.50 mm.
The default values for Bend Radius and Relief Shape will be accepted for this example.
Click the Done box. The Sheet Metal Defaults dialog box will appear.
Note
Reliefs are added to bends in sheet metal parts to prevent tearing as the bend is created.
Click the Cancel box. (No changes were made to the bend parameters.)
Flanges
A flange is a rim formed on the edge of sheet metal for strength.
A rim formed on the edge of sheet metal for strength.
Right-click the mouse and select the Flange tool.
The Flange dialog box will appear. See Figure 13-10.
Set the length of the flange for 20 mm, accept the 90.0° Flange Angle, and select the lower rear edge of the sketch.
The lower edge was chosen because the flange total height is to be 20 mm. If the upper edge was chosen, the total height would be 20.5, the flange height plus the material thickness. Figure 13-11 shows the flange orientation resulting from edge selection.
Use the Flip Direction button to change the flange orientation if necessary.
Click Apply and then Cancel. Figure 13-12 shows the resulting flange.
Tabs
Tabs are similar to flanges, but tabs do not run the entire length of the edge, as flanges do. Tabs are created using a new sketch plane, and the Two Point Rectangle tool located under the Sketch tab. See Figure 13-13.
A feature similar to a flange but that does not run the entire length of the edge.
Zoom the part so that the top-edge surface is identifiable; select the top-edge surface of the vertical flange, right-click the mouse, and select the New Sketch option.
Use the Two Point Rectangle tool located on the Draw panel under the Sketch tab to draw a rectangle from the back edge of the vertical flange as shown.
Use the Dimension tool to size and locate the tab in accordance with the dimensions given in Figure 13-13.
Right-click the mouse and select the Finish 2D Sketch option.
Select the Face tool, and define the tab as the Profile.
An area cut out of material to allow it to be bent.
Inventor’s default relief value is equal to the thickness of the sheet metal material. Figure 13-13 shows the relief that was automatically created as the tab was formed.
Holes
Holes are added to sheet metal parts in the same manner as they are added to 3D models. See Figure 13-14.
Create a new sketch plane on the top surface of the tab.
Use the Point, Center Point tool to define a center point.
Use the Dimension tool to dimension the center point location.
Right-click the mouse, and select the Finish 2D Sketch option.
Use the Hole tool on the Modify panel under the 3D Model tab panel to create the hole.
In this example, a Ø5.00 hole was created located 5 from each edge of the tab.
Corners
Both internal and external corners are created using the Corner Round tool found on the Sheet Metal panel bar.
Click the Corner Round tool on the Modify panel under the Sheet Metal tab.
The Corner Round dialog box will appear. See Figure 13-15.
Set the Radius value for 5 mm and click the Selected option in the Corner Round box.
Cuts may be any shape, other than a hole, that passes through the sheet metal. In this example a rectangular shape is used. See Figure 13-16.
Reorient the part, create a new sketch plane, and sketch a rectangle as shown. Use the Dimension tool to size and locate the rectangle.
Right-click the mouse and select the Finish 2D Sketch option.
The Sheet Metal panel bar will appear.
Select the Cut tool from the Modify panel.
The Cut dialog box will appear.
Select the rectangle as the Profile.
Ensure that the direction of the cut is correct, and click the OK box.
The rectangular area will be removed. The depth of the cut will automatically be set for the thickness value.
Select the Corner Round tool and set the Radius value for 2 mm.
Select the four inside corners of the rectangular cut.
Click the OK button on the Corner Round dialog box.
Cuts through Normal Surfaces
Normal surfaces are surfaces that are perpendicular to each other. Cuts in normal surfaces are made by making intersecting cuts in both surfaces. See Figure 13-17.
Create a new sketch plane on the vertical flange as shown, and sketch a rectangle.
Ensure that the rectangle extends beyond the rounded edge of the surface.
Use the Dimension tool to locate and size the rectangle.
Right-click the mouse and select the Finish 2D Sketch option.
Use the Cut tool to remove the rectangle.
Create another new sketch plane on the horizontal flange, and use the Dimension tool to size and locate the rectangle.
Right-click the mouse and select the Finish 2D Sketch option.
Click the Cut tool.
The Cut dialog box will appear.
Click the Cut Across Bend box, then click OK.
Hole Patterns
A hole pattern is created from an existing hole. See Figure 13-18.
Create a new sketch plane on the horizontal flange.
Use the Point, Center Point tool and create a hole on the flange.
Use the Dimension tool to locate the center point.
Right-click the mouse and click the Finish 2D Sketch option.
Click the Hole tool on the Sheet Metal panel.
The Hole dialog box will appear.
Set the Termination for Through All and the hole’s diameter for 2.
Click OK.
The dimensions for the hole come from the dimensions given in Figure 13-1.
Click the Rectangular tool located on the Pattern panel under the Sheet Metal tab.
The Rectangular Pattern dialog box will appear.
Define the Ø2 hole as the Feature.
Click the arrow under the Direction 1 heading, then the top front edge of the part. Use the Flip Direction button to change direction if necessary.
Set the number of holes under Direction 1 for 4 and the spacing for 8 mm.
Click the arrow under the Direction 2 heading, and click the left front edge of the part to define the direction.
Set the number of holes for 2 and the distance for 8 mm.
Click OK.
Flat Patterns
Flat patterns of 3D sheet metal parts can be created using the Create Flat Pattern tool. See Figure 13-19.
Click the Create Flat Pattern tool.
A flat pattern will automatically be created.
Punch Tool
The Punch Tool is used to create various shapes in sheet metal parts. Because sheet metal parts are thin, many shapes are created by punching through the material. Sheet metal is placed in a press and a tool with the desired shape is inserted. The press then presses down quickly, piercing the sheet metal with the punch tool to create the desired shape.
To Use the Punch Tool
Draw a 4-in.× 6-in. rectangle using the Sheet Metal (in).ipt format. It is presented in an isometric orientation.
Create another New Sketch plane on the front surface of the rectangular part and locate a center mark 3.00 from the left edge and 2.00 from the top edge.
Right-click the mouse and select the Finish 2D Sketch option.
This chapter defined and illustrated how to create sheet metal drawings from 3D models and orthographic drawings. Features of sheet metal parts such as bend radii, flanges, tabs, and reliefs were presented, and flat patterns were created. The use of the Punch Tool was also illustrated.
Chapter Test Questions
Multiple Choice
Circle the correct answer.
1. How thick is a piece of #12 gauge sheet metal?
a. 0.4600 in.
b. 0.0808 in.
c. 0.0571 in.
d. 0.0050 in.
2. How thick is a piece of #30-gauge sheet metal?
a. 0.1443 in.
b. 1/8 in.
c. 0.0100 in.
d. 0.0031 in.
3. The thickness of a piece of sheet metal is defined using which tool?
a. Sheet Metal Defaults
b. Face
c. Fold
d. Hem
4. A small piece of bent material that does not run the entire length of an edge is called a
a. Flange
b. Tab
c. Relief
d. Contour
5. Which of the following materials is not available in the Material option of the Sheet Metal Defaults dialog box?
a. Steel, Mild
b. Aluminum-6061
c. Brass, Soft
d. Plexiglas
True or False
Circle the correct answer.
1. True or False: In the English unit system, the higher the sheet metal gauge number, the thinner the material.
2. True or False: A cut made next to a tab to allow for smooth bending is called a relief.
3. True or False: As sheet metal is bent, the inside surface is subjected to compression, and the outside surface to tension.
4. True or False: Normal surfaces are surfaces located 60° apart.
5. True or False: Punch tools can be used to create slots and keyholes.
Chapter Projects
Project 13-1
Redraw the sheet metal parts in Figures P13-1A through P13-1F using the given dimensions. Use the default values for all bend radii and reliefs.
Project 13-2: Inches
Design and draw a box (similar to that shown in Figure P13-2) that has a capacity of
100 cubic centimeters and is a cube.
4 fluid ounces.
100 cubic centimeters and is rectangular with the length of one side twice the length of the other.
125 cubic inches and is a cube.
125 cubic inches and is rectangular with the length of one side 1.5 times the length of the other.