Drawing Orthographic Views with Dimensions

1. From 3D Model to 2D Drawing

A 2D drawing in Fusion 360 is not a separate, disconnected file. It's a dynamic representation of your 3D model, presented in a traditional engineering format. The goal is to create a set of scaled, dimensioned views that provide all the necessary information to manufacture a part.

A typical drawing includes:

• Orthographic Views: Standard front, top, and side views.
• Isometric View: A 3D view to help with visualization.
• Dimensions: Measurements defining the geometry.
• Title Block: A frame containing metadata like the part name, author, scale, and material.

Here is an example of a complete technical drawing created within Fusion 360:

2. Creating a Drawing: The Fundamental Workflow

We will use the 90-degree bracket you designed in the previous lesson as our example piece. Please open that Fusion 360 design file now.

The process of creating a drawing involves four main steps: setting up the sheet, placing views, adding dimensions, and finalizing the details. We'll use a video to guide us through most of the process.

3. Your Turn: Create a Drawing of Your Bracket

Now, let's apply what you've just seen to your own bracket design. Follow these steps in Fusion 360.

Step 1: Initiate the Drawing

As shown in the video, navigate to File > New Drawing > From Design. This will open the Create Drawing dialog.

Before you click OK, it's crucial to set your standards correctly.

• Standard: Choose ASME (American Society of Mechanical Engineers) or ISO (International Organization for Standardization). ASME typically defaults to inches and third-angle projection (the standard in the US), while ISO uses millimeters and first-angle projection. For DIY projects, either is fine, but consistency is key. Let's stick with ASME.
• Units: You can select in or mm.
• Sheet Size: Choose a size that suits your needs, like 8.5 x 11 in for a standard home printer.

Important Note: As another expert, Tyler Beck, points out in his video "Getting Started in 2d Drawings", Fusion 360 does not currently allow you to change the fundamental Standard (ASME/ISO) after a drawing is created. You must get this right from the start.

Step 2: Place Your Views

1. Base View: Fusion will prompt you to place the base view. In the dialog box, set the Orientation to Front. Choose a suitable Scale (e.g., 1:2 or 1:1) so the views will fit comfortably on the page. Click to place this view, perhaps in the lower-left corner.
2. Projected Views: Select the Projected View tool. Click on your base view first, then move your mouse and click to place the following:
   • A Top View directly above the base view.
   • A Right-Side View directly to the right of the base view.
   • An Isometric View in the upper-right corner.
3. Press Enter to confirm the placement. Your projected views are now intelligently linked to the base view.
4. Style Adjustment: Double-click the isometric view. Change its Style to Shaded to give it a more realistic, 3D appearance.

Step 3: Add Dimensions

This is where the drawing becomes a useful plan.

1. Activate the Dimension tool (shortcut: D).
2. Add the key dimensions to your orthographic views. Your goal is to provide enough information for someone to understand the part's geometry without needing the 3D model. Be sure to dimension:
   • Overall length, width, and height.
   • The bracket_thickness parameter.
   • The position and diameter of the holes (hole_diameter).
   • The diameter of the countersinks (countersink_diameter).
   • The radius of the main fillet you added for strength.

Tip: Avoid redundant dimensions. If you've dimensioned the bracket's width on the top view, you don't need to dimension it again on the front view.

4. The Power of Parametric Design: The Model-Drawing Link

Here is where the digital workflow vastly outperforms manual drafting. Your drawing is not static; it is directly linked to your 3D model.

Now, try this yourself:

1. Go back to the browser tab with your 3D bracket model.
2. Open the parameters dialog (Modify > Change Parameters).
3. Change a key dimension. For example, change bracket_width from 30mm to 50mm. Save the design.
4. Switch back to the browser tab with your drawing. You should see a warning icon indicating that the reference model has changed.
5. Click the update icon at the top of the window.

Observe how all your views and dimensions update automatically to reflect the change. This single feature eliminates countless hours of manual redrawing and ensures your plans always match your part.

5. Finalizing and Exporting

Finally, you need to prepare the drawing for use.

• Title Block: Double-click the title block at the bottom right. Fusion auto-fills some information, but you can edit the fields to add details like a project name or material.
• Export: To print your drawing or share it, you can export it as a PDF. Go to File > Print. You can choose to print to a physical printer or use a "Print to PDF" option, which most operating systems provide. This creates a clean, scalable document you can use in your workshop.

Conclusion

Excellent work. You have successfully translated a 3D component into a professional 2D technical drawing. You now possess a complete workflow: from conceptual 3D design to a practical, manufacturable plan.

Key Takeaways:

• The Drawing workspace in Fusion 360 creates a set of linked, scaled views of a 3D model.
• The workflow involves creating a Base View and then using the Projected View tool to generate aligned orthographic and isometric views.
• The Dimension tool is used to annotate the views with the necessary manufacturing information.
• The drawing is parametrically linked to the 3D model, allowing for automatic updates when the design changes—a massive advantage over traditional methods.

Next Lesson Preview:
You've designed individual components (brackets) and now you can create plans for them. In our next lesson, we will combine these skills to model a simple mixed-material project: a small shelf that uses the very type of 3D printed brackets you've been designing. This will be a great opportunity to practice assembly design and see how your 3D printed parts and wooden components come together in a complete project.