Activity 1: Create features for the gas pedal

In this activity, you open the gas pedal sample file and save it to a personal project. You create a loft feature to connect the larger profile on the gas pedal base to the smaller one on the foot support, using a centerline to control the shape. You add a web feature to the loft, to give it additional strength. You then add a rib to the gas pedal base to provide it with additional support.

Note: Web and rib features cannot be created alone and must intersect with solid model geometry on both ends.

gas pedal model and with added features

Gas Pedal starting model (left), and with added features (right)

Prerequisites

Fusion is started.
Data file location: Samples > Basic Training > 04-Modeling > Gas Pedal.f3d

Steps

Open the starting model, Gas Pedal, from the Basic Training folder in the Data Panel
1. If the Data Panel is not currently shown, click Show Data Panel at the top of the screen.
2. The top level (home view) of the Data Panel is divided into two subsections: ALL PROJECTS and SAMPLES. Scroll down until you reach SAMPLES.
3. Double-click the Basic Training folder to open it.
4. Double-click the 04 - Modeling folder to open it.
5. Double-click the Gas Pedal model to open it in the canvas.
  
  Note: When you open a sample design in Fusion for the first time, it appears in the Model workspace.
Identify a personal project in which to save the starting shape models. Sample models are read-only and must be saved to a personal project.
1. Click File > Save as .
2. Enter a name, such as Gas Pedal, in the name field.
3. Expand the arrow button next to the Location field.
4. Locate and click on an existing project, or click New Project to start a new project.
Identify or create a folder in which to save the starting shape models.
1. Double-click on a folder in the project to select it, or create a new folder.
2. To create a new folder, click New Folder.
3. Type a name, such as Create tools for the folder.
4. Press Enter.
5. Double-click the folder to make it the current file saving location
6. Click Save
Create the loft feature. Use the larger I-shaped face on the bottom of the pedal base body, and the smaller I-shaped face on the bottom of the foot support body, as the Profiles. Use the Loft Centerline sketch as the Centerline Guide Type.
1. In the Browser, expand the Sketches folder, then click the visibility eye associated with Loft Centerline to make the Loft Centerline sketch visible.
2. Click (Design > Solid > Create > Loft) to activate the Loft tool.
3. In the Loft dialog, confirm that Select associated with Profiles is active, then click on the I-shaped face on the base of the pedal base.
4. Rotate the model so that you can see the bottom of the foot support body and click on the I-shaped face.
  
  Note: Although the shape of these two faces is the same, the dimensions are different. The Loft tool creates a feature with a smooth transition from one dimension to the other.
5. In the Loft dialog, click Centerline associated with the Guide Type to activate it, then select the Loft Centerline sketch in the canvas.
  
  Note: The Loft tool creates the feature as soon as you select the sketch in the canvas.
6. Click OK to close the Loft dialog.
Create a 2 mm thick Web feature to support the new loft feature, using the 11 sketch lines that intersect with the loft.
1. In the Browser, in the Sketches folder, click the visibility eye associated with Web to make the Web sketch visible.
2. Click Design > Solid > Create > Web to activate the Web tool.
3. On the model in the canvas, click on the 11 sketch lines that intersect with the loft to select them.
  
  Note: The sketch edges don’t need to be coincident with the edges of the feature.
4. Set the Thickness to 2 mm to see a preview of the web.
  
  Tip: When the thickness is non-zero, curves can only be selected while you hold Ctrl (Windows) or Command (MacOS).
5. Confirm that Depth Options is set to To Next, so the web feature extends downwards as far as the loft feature surface, then click OK to close the dialog.
  
  Note: When Extend Curves is selected, the curves are extended to the first surface they encounter. If the original curve is too short, the web feature is extended. If it is too long, the web feature still ends at the first surface it encounters. In this example, it doesn’t matter whether Extend Curves is selected or not.
Create a rib to support the pedal base, 7.5 mm thick, that extends to both surfaces to which the Rib sketch is attached.
1. In the Sketches folder, make the Rib sketch visible.
2. Click Design > Solid > Create > Rib to activate the Rib tool.
3. Click on the angled sketch line, to select it as the Curve.
4. Set the Thickness to 7.5 mm to see a preview of the rib.
5. Confirm that Thickness Options is Symmetric, and Depth Options is To Next, so the rib is symmetrical about the rib sketch and extends to both surfaces, then click OK to close the dialog.
Go to Activity 4 to check your modifications.

Activity 1 summary

In this activity, you created a loft feature to connect the gas pedal base to the foot support. You added a web feature to the loft, to give it additional strength. You then added a rib to the gas pedal base to provide it with additional support.

You accomplished this task using the following tools:

Loft
Web
Rib