SOLIDWORKS Exercise 1

Sheet Metal Bracket

Exercise 1: Create this part using the provided information below.

Sheet Metal
Bracket

Design Intent The design intent for this part is as follows:

1. The material is 14 gauge steel.
2. All bends = R2.54mm.
3. Dimensions given define the inside of the bracket.
4. The part is symmetrical about the default reference planes.
This exercise uses the following skills:
 Base Flange/Tab
 Cuts in Sheet Metal
Units: MMGS
Procedure
1 New part.
Begin a new document using the Part_MM template.
2 Base Flange.
Create the sketch for the Base Flange on the Front Plane to
appropriately match the views in the drawing provided.
Ensure the material is added in the correct direction to meet the stated
design intent.
3 Add cuts and chamfers.
Add Extruded Cut and Chamfer features to complete the part.

1
Exercise 2 SOLIDWORKS
Flange Features

Exercise 2: Use flange features to create the

Flange Features part as shown.
This exercise uses the following
skills:
 Base Flange/Tab
 Sheet Metal Parameters
 Using Tables
 Edge Flanges
 Tab Features
 Flatt-Pattern Feature
Units: MMGS
Procedure
1 New part.
Begin a new part document using the Part_MM template.
2 Sketch.
Sketch the profile as shown on the Front Plane.

3 Base Flange.
Click Base Flange/Tab .
Direction1: Blind, 75mm.
Click Use Gauge Table. Select SAMPLE TABLE - ALUMINUM.

2
SOLIDWORKS Exercise 2
Flange Features

4 Sheet Metal Parameters.

Use the following settings for the sheet metal
parameters:
 Thickness = Gauge 18
 Bend Radius = 3mm
 Bend Allowance = K-Factor (read from the
table)
 Auto Relief = Obround, Use relief ratio: 0.5

Click OK .

5 Optional: Modify appearance.

Clear any selections by clicking in empty space in the graphics area.

Click the tab for Appearances, Scenes, and Decals in the Task
Pane.
Expand Appearances, Painted and select Powder Coat.
Press ALT while dragging the aluminum powdercoat appearance onto
the part.
Tip Using the ALT key during the drag and drop opens the appearances
PropertyManager.
Use the PropertyManager to
change the color of the
appearance and apply it to the
entire part .

Click OK .

3
Exercise 2 SOLIDWORKS
Flange Features

6 Edge Flange.
Click Edge Flange .
Click the edge as shown.
Tip It doesn’t matter if an inside or
outside edge is selected.
Move the cursor to the right and
click again to define the
direction for the flange.
Tip The arrows in the graphics area
can be used to change the
direction and length of the
flange, or use the options under Flange Length in the
PropertyManager.
7 Additional edges.
Pick the two additional edges at
the back of the part as shown.

8 Adjust Edge Flange settings.

Use the following settings for
the edge flange feature:
 Gap Distance = 0.25mm

 Angle: 90deg

 Flange Length: Blind,

22mm
 Measured from:
Outer Virtual Sharp
 Flange Position:
Material Inside
 Trim Side Bends: Checked

Click OK .

4
SOLIDWORKS Exercise 2
Flange Features

9 New sketch.
Create a sketch on the right face as
shown.

10 Extruded Cut.
Click Extruded Cut .
Use Through All to cut away the corner of the Base Flange.

Click OK .
11 Edge Flange.
Create a new Edge Flange feature from the angled edges as shown.
Use the following settings:
 Angle: 90deg

 Flange Length: Blind, 22mm

 Measured from: Outer Virtual Sharp

 Flange Position: Material Inside
 Trim Side Bends: Cleared

Click OK .

5
Exercise 2 SOLIDWORKS
Flange Features

12 Evaluate reliefs.
Relief cuts were automatically
created for the edge flange. The
default sheet metal parameters are set
for Obround.
For this feature, we will override the
default sheet metal parameters to use
a Tear relief type.

13 Edit Edge-Flange2.
Click the last Edge-Flange feature and
Edit Feature .
Click Custom Relief Type.
Select Tear, and the Extend type.

Click OK .

6
SOLIDWORKS Exercise 2
Flange Features

14 Add a Tab.
Sketch the rectangular profile on the bottom inside face as shown.

Click Base Flange/Tab .

Ensure Merge Result is checked. Click OK .

The thickness and direction is automatically determined by the existing
geometry.
15 Evaluate Flat Pattern.
Toggle flat display or Flatten the part to evaluate the Flat Pattern.

16 Save and close the part.

7
Exercise 3 SOLIDWORKS
Edit Flange Profile

Exercise 3: Use flange features to create the part

Edit Flange as shown.
Profile This exercise uses the following
skills:
 Base Flange/Tab
 Tab Features
 Edge Flanges
 Editing the Flange Profile
 Flat-Pattern Feature
Units: MMGS
Procedure
1 New part.
Begin a new part document using the Part_MM template.
2 Sketch.
Sketch the profile as shown on the
Front Plane.
3 Base Flange.
Click Base Flange/Tab .
Direction1: Midplane, 35mm.
Click Use Gauge Table. Select
SAMPLE TABLE - STEEL.

4 Sheet Metal Parameters.

Use the following settings for the sheet metal parameters:
 Thickness = Gauge 18
 Bend Radius = 2.54mm
 Bend Allowance = K-Factor (read
from the table)
 Auto Relief = Obround, Use relief
ratio: 0.5
Click Reverse direction to apply the
material above the sketch lines.

Click OK .

8
SOLIDWORKS Exercise 3
Edit Flange Profile

5 Add a Tab.
Sketch the profile as shown and use it for
a Tab feature.
6 Mirror Tab.
Mirror Tab1 over the Right Plane.

7 Edge Flange.
Click Edge Flange .
Click the edge as shown.
Click again to define the direction for the
flange.

8 Edit Flange Profile.

In the PropertyManager, click Edit Flange Profile.
Drag the ends of the flange profile to break the endpoint attachment.
Modify and dimension the profile as shown.

9
Exercise 3 SOLIDWORKS
Edit Flange Profile

9 Edge Flange Settings.

Click Back in the Profile Sketch dialog to return to the
PropertyManager.
Set the Angle to 90deg and the Flange Position to
Material Inside .

Click OK .
10 Mirror Edge Flange.
Mirror Edge-Flange1 over the Front Plane.

11 Add holes.
Click Hole Wizard from the Features toolbar.
Use the following settings:

Hole Type: Hole

Standard: ANSI Metric
Type: Drill sizes
Size: Ø5.0
End Condition: Up to Next
Tip Since the Hole Wizard does not include the Link to Thickness option,
Up to Next can be used to ensure the hole only cuts through one
material thickness.

10
SOLIDWORKS Exercise 3
Edit Flange Profile

12 Hole positions.
Click the Positions tab.
Click 3D Sketch.

Add sketch points Coincident to the arc

centers of each tab and edge flange.

Click OK .
13 Evaluate the flat pattern.

14 Save and close the part.

11
Exercise 4 SOLIDWORKS
Sheet Metal Box

Exercise 4: Use flange features to create the part as

Sheet Metal Box shown.
This exercise uses the following skills:
 Base Flange/Tab
 Miter Flanges
 Editing Sheet Metal Parameters
 Flat-Pattern Feature
Units: MMGS

Procedure
1 New part.
Begin a new part document using the Part_MM template.
2 Sketch.
Sketch the profile as shown on the Front
Plane.
3 Sheet metal plate.
Click Base Flange/Tab .
Click Use Gauge Table. Select SAMPLE
TABLE - STEEL.

4 Sheet Metal Parameters.

Use the following settings for the sheet metal parameters:
 Thickness = Gauge 14
 Bend Radius = 2.54mm
 Bend Allowance = K-Factor (read from the table)
 Auto Relief = Obround, Use relief ratio: 0.5
Click Reverse direction to extrude the plate forward from the Front
Plane.

Click OK .
5 Optional: modify part appearance.
Change the color of the part as desired.

12
SOLIDWORKS Exercise 4
Sheet Metal Box

6 New reference plane.

The sides of the box will be created with a
miter flange feature. The profile for a
miter flange must be created normal to an
existing edge at an end point.

Create a Plane using the edge and

endpoint shown as references.

Tip The Plane command can be found on

the Features toolbar in the Reference
Geometry flyout.

7 Sketch on Plane1.
Create the profile as shown on Plane1.

Right View

8 Miter Flange.
Click Miter Flange .
Select the edges as shown and use
the following settings:
 Flange location =
Material Inside
 Gap distance = 0.25mm

Click OK .

Tip The initial edge that is selected - the inside or outside edge of the plate -
is determined by the relations in the profile sketch. The additional
edges selected for the feature must be connected to the initial edge.

13
Exercise 4 SOLIDWORKS
Sheet Metal Box

9 Edit sheet metal parameters.

Click the Sheet-Metal folder and
Edit Feature .
Change the Thickness to be 12 Gauge and the
Bend Radius to be 5.080mm.

Click OK .
10 Flat Pattern.
Examine the flat pattern.

11 Save and close the part.

14
SOLIDWORKS Exercise 5
Assorted Framing Hangers

Exercise 5: Use the accompanying graphics and

Assorted stated design intent to create the parts.
Framing This exercise uses the following
Hangers skills:
 Base Flange/Tab
 Edge Flanges
 Cuts in Sheet Metal

Design Intent The design intent for all parts is as follows:

1. Material is 18 gauge steel
2. All bends = R1.905mm
3. All holes = Ø5mm
4. Hole positions can be estimated
5. Part is symmetrical

Post Cap

15
Exercise 5 SOLIDWORKS
Assorted Framing Hangers

Joist Hanger 1

Joist Hanger 2

16