4.1.2: How to create an engineering drawing

Why are engineering drawings important?

Engineering drawings are essential tools for effective communication between machinists, engineers, and other teams. These detailed illustrations ensure that designs can be accurately interpreted and manufactured. Additionally, they provide a reliable way to document your work, which is critical for troubleshooting failures, implementing revisions, or maintaining records for future use (1).

Key components of engineering drawings include:

• Bill of Materials (BOM): This section lists all components required for the assembly of your design, ensuring proper identification and sourcing of parts.

• Title Block: Found within the drawing template, this block includes essential details such as your name, the part name, and tracking information like dates or revision numbers.

Many organizations, including NC State, have standardized templates for engineering drawings, ensuring consistency and adherence to specific guidelines. Using these templates ensures your work meets professional and institutional standards.

References 

(1) Inodvance. The Importance of Technical Drawings in Engineering. https://blog.indovance.com/importanc...ical-drawings/ (accessed 2024-11-19).

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Step 0 - Model Your Part And Familiarize yourself with drawing tools

Before creating an engineering drawing in Fusion 360, you must have a completed 3D model. Ensure that your part, such as the phone holder, is fully modeled and saved.

• Save Your Design: The design must be saved locally or uploaded to Fusion 360's cloud storage.

• Verify Accessibility: To confirm your part is accessible for creating a drawing, check if it is discoverable in the Fusion 360 Data Panel.

  • To access the Fusion 360 Data Panel, click on the 3x3 grid of boxes in the top left.  This will show all files saved to your cloud.   

 

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Step 1 - Start Creating a Drawing

1. Open the File dropdown menu in the top-left corner of the Fusion 360 interface (Figure 1).

2. Scroll to the bottom of the menu and select Drawing.

   • From the submenu, click From Design.

3. This will open the drawing workspace, where you can create an engineering drawing based on any saved design.

Figure 1.)  The dropdown menu in Fusion 360 showing the option to create a drawing and change workspaces.

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Step 2 - Modify Sheet Settings

1. Change the Sheet Size:

   • Fusion 360 defaults to an A3-size sheet.

   • To modify the sheet size:

     • Hover over the Sheet Size in the workspace.

     • Click the option to change the sheet size, which appears on the right.

   • If you want to use a custom template:

     • Go to the File menu and select New Drawing Template.

     • Use the menu on the right to import your own template, such as company or school-specific designs.

note: For this tutorial, the standard A3-size paper will be used.

2. Fill Out the Title Block:

   • Hover over the Title Block until it highlights, then click on it.

   • This will open editable text boxes for you to input information such as the title, author, and date.

   • You can also import custom title blocks using the same process for templates.

Figure 2.)  Clicking on the title block in Fusion 360 opens a menu for editing its attributes, such as title, author, and date.  All blue text boxes are editable.

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Step 3 - Import the Principal View

1. Insert the Base View:

   • Click the Base View tool in the drawing menu.

   • This allows you to insert the principal view of your part.

2. Select the Principal View:

   • Choose the view that shows the most shared dimensions, as all subsequent views will be derived from this.

3. Adjust View Settings:

   • In the Drawing View menu on the right:

     • Set Tangent Edges to Full Length.

     • Set the Style to Visible and Hidden Edges.

     • Enable Center Marks for round cuts.

These settings ensure that the part is displayed clearly, making it easier to dimension in the following steps.

Figure 3.)  A principal view added to the document in Fusion 360, showing the base view with visible and hidden edges, full-length tangent edges, and center marks enabled.

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Step 4 - Insert Projected Views

1. Select the Projected Views Tool:

   • Click the Projected Views tool, located next to the Base View tool in the drawing menu.

2. Choose the Principal View:

   • Select the principal view placed in the previous step.

3. Place Additional Views:

   • Use the tool to place front, top, and isometric views in the workspace.

   • The orientation of these views will depend on their relation to the principal view.

4. Adjust View Settings (Optional):

   • By default, projected views inherit the settings of the principal view, such as tangent edges and style.

   • If needed, you can adjust these settings individually for each view.

Figure 4.)  A document showing correctly inserted projected views, including front, top, and isometric views, all derived from the principal view.

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Step 5 - Dimension Your Views

1. Select the Dimension Tool:

   • To begin dimensioning, select the Dimension Tool from the drawing menu.

2. Apply Dimensions:

   • Click on two points or vectors to dimension the distance or angle between them.

3. Dimensioning Best Practices:

   • The goal of dimensioning is to clearly convey all necessary measurements to the reader, particularly for machining.

   • Avoid overdimensioning, as it can lead to confusion. Ensure each dimension is specified only once.

4. Using Auto Dimension (Optional):

   • Fusion 360 offers an Auto Dimension feature, but it is not recommended.

   • Auto dimensioning doesn’t consider the reader’s perspective and may result in dimensions that are difficult to read or incorrectly placed.

   • While it produces a technically correct dimensioned drawing, it may not be as clear or accurate as manually placed dimensions. However, it can be useful in some cases for quick drafts.

Note:  Dimensions can be edited after they are placed, including from the auto dimension tool.

Figure 5.)  A properly dimensioned sketch of the phone holder, with clear and precise dimensions applied to all relevant features.

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Step 6 - Export the Drawing

You can export your drawing as a PDF using one of the following methods:

Option 1: Using the Export Tool

1. Navigate to the Export tool in the drawing menu.

2. Select PDF from the dropdown menu.

3. In the menu on the right:

   • Specify the sheets you wish to include in the PDF.

   • Click OK to confirm your selection.

4. In the file-saving menu that appears:

   • Click the three dots to choose the save location.

   • Ensure Save to My Computer is checked.

   • Click Save to complete the export.

Option 2: Using the Print Option

1. Open the File menu in the top-left corner and select Print.

2. In the Printer dropdown menu, select Print to PDF.

3. Choose the file location, name the file, and click Save to finalize the export.