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Lesson 8

Dimensioning and Annotating Drawing Views

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Hello! Welcome back to our final lesson on OnShape CAD fundamentals.

In our last session, you successfully created a multi-view drawing, placing the standard orthographic and isometric views for your screw part. This laid the visual foundation for your engineering drawing. Now, it's time to add the most critical information: the data that tells a machinist exactly how to make the part.

Today's lesson addresses the learning outcome: Apply dimensions and annotations to drawing views to fully define a part. We will cover the tools and, more importantly, the strategies for adding dimensions, notes, and other symbols to create a complete, professional manufacturing blueprint. This skill is the final piece of the puzzle in creating the portfolio-quality documentation you're aiming to produce.

1. The Goal: Creating a "Fully Defined" Drawing

Before we start clicking buttons in Onshape, let's revisit the purpose of a drawing from a design engineer's perspective. A drawing is "fully defined" when a manufacturer can create the part without making any assumptions or needing to ask you questions. Every feature's size, shape, and location must be controlled unambiguously.

Achieving this requires a strategy:

  • Clarity over clutter: Dimensions should be placed on the view where the feature is shown most clearly. Avoid placing dimensions on hidden lines if possible.
  • No redundancy: A feature should only be dimensioned once. Stating the same dimension in multiple ways can lead to confusion and errors, especially if the design is updated.
  • Communicating Design Intent: Your dimensioning scheme should reflect how the part functions. For example, dimensioning features from a common datum (a reference surface) often relates to how the part is mounted or assembled.

Take a look at the drawing below. Notice how the dimensions are organized, easy to read, and logically grouped. This level of professionalism is what we are working towards.

Technical Drawing of a Mechanical Shaft in Onshape
This drawing is an excellent example of a fully defined part. Dimensions are clear, and annotations provide necessary manufacturing details without cluttering the views.

2. Adding Dimensions and Annotations in Onshape

Onshape provides a powerful set of tools for dimensioning and annotating your drawings. The best way to get an overview of these tools in action is to see them demonstrated.

The following video continues from where we left off in the last lesson, focusing now on adding supplemental geometry, dimensions, and notes.

Onshape - Drawings Overview - How to Create New Drawings, Views, and Dimensions

This video, 'Onshape - Drawings Overview', provides a practical demonstration of the core dimensioning and annotation workflow. Pay close attention to the different types of dimensions used and how notes are added.

Please watch the following segments: 05:08 - 06:56: This part covers adding supplemental geometry like center marks and centerlines, which are essential for dimensioning to holes and cylindrical features. 06:56 - 14:29: This is the main segment. It demonstrates the use of the Dimension tool for various cases (linear, radial), how to add symbols (like the diameter symbol), creating ordinate dimensions, and adding text notes.

Onshape Crankshaft Drawing with Dimensions and Annotations
The crankshaft drawing from the video demonstrates the application of linear, radial, chamfer, and ordinate dimensions to define a complex part.

3. A Deeper Dive into Dimensioning Tools

The video gave you a great tour. Now, let's organize those concepts and point you to the definitive reference for when you need more detail. The Onshape Help documentation on Dimensions is an exhaustive resource. We won't read it all, but I'll guide you to the most important parts.

Dimensions

The Onshape Help page titled 'Dimensions' is your comprehensive guide. We'll use it as a reference to solidify your understanding of the tools shown in the video.

You don't need to read this entire document now, but be aware of its contents. Specifically, scan through the sections on: Dimension: The general-purpose tool, activated with the 'd' shortcut. Chamfer dimension: For specifying chamfers. Line-to-line angular dimension: For angles. Radial and Diameter dimension: For arcs and circles. Ordinate dimension: A powerful method for dimensioning from a common zero-point. Dimension palette: The pop-up menu for adding tolerances, symbols, and text.

Key Dimensioning Tools:

  • The General Dimension Tool (Shortcut: d): As you saw, this is your primary tool. It's context-sensitive:

    • Click a line to get its length.
    • Click a circle to get its diameter.
    • Click an arc to get its radius.
    • Click two parallel lines to get the distance between them.
    • Click two non-parallel lines to get the angle.

  • Specific Dimension Types: For some features, it's better to use a dedicated tool from the Dimension tool's dropdown menu. The Chamfer Dimension tool is a good example, as it creates a standard callout like "0.5 X 45°".

  • The Dimension Palette: This is arguably one of the most important features for creating professional drawings. After placing a dimension, hover over it and click the small palette icon that appears (or just double-click the dimension). This opens a dialog where you can:

    • Add Prefixes and Suffixes (e.g., 4X to indicate four identical features, or TYP for "typical").
    • Insert Symbols like diameter (⌀), depth (↧), or plus/minus (±).
    • Define Tolerances (which we will cover in detail in a later module).
    • Add parentheses to create a reference dimension.
Test your understanding!

You've dimensioned a hole with a diameter of '10 mm'. You want to indicate that this is a repeating feature on 4 identical holes in your part. What is the most efficient way to annotate this using the Dimension Palette without adding extra text notes?

Show answer

The most efficient and standard way is to double-click the '⌀10' dimension to open the palette and add 4X (with a space) to the Prefix text field. The resulting dimension will read 4X ⌀10, clearly communicating the quantity to the manufacturer.

4. Your Turn: Fully Define the Screw Part

Let's apply these skills to the drawing you created in the last lesson. Our goal is to add the essential dimensions to fully define your screw part.

  1. Open your Onshape document and go to the drawing tab for your screw.
  2. Add a Centerline:
    • In the toolbar, find the centerline tool (it looks like a long dash and a short dash). Use the Edge to Edge Centerline option.
    • In the Front View, select the left vertical edge of the screw and the right vertical edge. A centerline will appear down the middle. This is the axis of revolution and is critical for dimensioning cylindrical parts.
  3. Apply Key Dimensions:
    • Activate the Dimension tool (shortcut: d).
    • Overall Length: In the Front View, dimension the overall length of the screw from end to end.
    • Head Height: In the Front View, dimension the height of the screw head.
    • Shaft Diameter: In the Front View, dimension the distance between the two outer vertical lines of the shaft.
    • Head Diameter: In the Top View (the circle), dimension the diameter of the head.
  4. Add a Chamfer Dimension:
    • From the dimension tool dropdown, select Chamfer dimension.
    • In the Front View, click the angled chamfer line at the tip of the screw, then click the adjacent horizontal line. Place the dimension callout.
  5. Refine with the Dimension Palette:
    • Your shaft and head diameter dimensions probably look like simple numbers (e.g., "0.25"). This is not standard.
    • Double-click the Head Diameter dimension. In the Dimension Palette, click the Symbol dropdown and insert the Diameter (⌀) symbol. It should now read "⌀...".
    • Do the same for the Shaft Diameter in the Front View.
  6. Add a Note:
    • In the toolbar, click the Note icon (A).
    • Click somewhere in an empty space on your drawing.
    • Type a simple material note, for example: MATERIAL: 304 STAINLESS STEEL. Click the green checkmark to confirm.

Take a step back and look at your drawing. It now contains not just the shape, but the specific, actionable information needed to manufacture it.

Conclusion

Congratulations on completing the OnShape CAD Fundamentals module! You now possess the core skills to take a 3D part from a concept to a fully detailed 2D engineering drawing.

Here are your key takeaways from this lesson:

  • A drawing is fully defined when it contains all the information needed for manufacturing, with no ambiguity.
  • Onshape's General Dimension tool (d) is your primary tool, while specific tools exist for features like chamfers.
  • Annotations like centerlines and notes provide context that dimensions alone cannot.
  • The Dimension Palette is essential for adding professional details like symbols, tolerances, and quantity callouts, which communicate your design intent.

You have built a strong foundation in using the CAD tool. In our next module, "Engineering Workflow and System Design," we will shift our focus from how to use the tools to why and when. We will begin to simulate a real-world project workflow, starting with the most critical first step: writing clear design requirements and specifications. This will lay the groundwork for our first major portfolio project.