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Lesson 24

Assembly Drawing and Bill of Materials

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Hello! Welcome back to the course.

In our last session, you did an excellent job bringing your design to life by building a fully functional 3D assembly of the linear actuator. By mating all the components and creating a screw relation, you've created a virtual prototype that simulates the core mechanism.

Today, we'll take that 3D model and create the kind of documentation that is essential in any professional engineering environment. Our learning outcome is to create an assembly drawing including standard views and a preliminary Bill of Materials (BOM). This bridges the gap between the 3D design and the real-world need for manufacturing, assembly, and procurement information. Your background in mechanical engineering means you're already familiar with the purpose of these documents; today, we'll focus on the specific Onshape tools and workflow to generate them efficiently.

We will cover:

  1. Creating a new drawing sheet and placing standard orthographic and isometric views of your assembly.
  2. Defining and inserting an exploded view to clearly show how the components fit together.
  3. Generating an automatic Bill of Materials (BOM) table.
  4. Adding callouts (balloons) to link the BOM to the parts in your views.

Let's get started on creating a key deliverable for your portfolio.

1. Creating the Drawing and Placing Standard Views

The first step in any documentation process is to set up your drawing sheet and place the primary views. In Onshape, drawings exist in their own tab within your document and are directly linked to your Part Studios and Assemblies. Any changes you make to the 3D model will be flagged for updating in the drawing, ensuring your documentation stays in sync with your design.

The goal is to produce a drawing like the one below, with clear views and a table of parts.

Onshape Assembly Drawing with Bill of Materials (BOM)
This image shows a typical Onshape assembly drawing. It includes an isometric view with balloon callouts and a corresponding Bill of Materials (BOM) table that lists all the components.

Let's watch a video that covers the fundamentals of creating a drawing and placing these initial views.

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

This video from the Creo Parametric channel provides a concise overview of the drawing creation process in Onshape. Pay close attention to how new drawing sheets are made and how the first views are placed.

Please watch from the beginning to 04:20. This will cover: Creating a new drawing and selecting a template. Inserting a part or assembly and placing the base (front) view. Projecting the top and right views from the base view. Inserting a separate, independent isometric view.

Your Task: Create the Base Drawing

Now it's your turn. Follow these steps in your Onshape document for the linear actuator project:

  1. Click the + icon in the bottom-left corner and select Create Drawing.
  2. When prompted for a template, select the Onshape tab and choose an ANSI template (e.g., ANSI B, inch or mm depending on your design). ANSI is the standard for US-based engineering. Click OK.
  3. The "Insert view" dialog will open automatically. Select your top-level linear actuator assembly.
  4. Place the Base View: Set the View orientation to Front. Place this view on the lower-left side of your sheet. This will be your primary view.
  5. Project Orthographic Views: Without exiting the tool, move your cursor above the base view to project a top view, and to the right of the base view to project a right view. Click to place each one. These views are now linked to the base view.
  6. Place the Isometric View: Click the Insert View tool again. Select your assembly, but this time set the View orientation to Isometric. You might want to adjust the View scale to fit it nicely in the top-right corner. It's common practice to change the display style of this view by right-clicking it and selecting Show/hide > Show shaded view to make it look more realistic.

You should now have a drawing sheet with the standard three orthographic views and one isometric view.

2. The Exploded View: Deconstructing the Assembly

For assemblies, an exploded view is invaluable. It shows how components are assembled and is almost always included in assembly instructions and design documentation. In Onshape, you first define the exploded state in the assembly environment and then place it as a special view in your drawing.

This process is covered in the following video.

Onshape - How to Create Exploded Views | Assemblies and Drawings

This video, also from Creo Parametric, demonstrates the two-stage process for creating an exploded view drawing. First, you'll see how to define the explode steps in the assembly, and then how to use that state in a drawing.

Watch the video from the beginning until 07:30. The first part (up to 06:00) takes place in the Assembly tab, showing how to pull components apart in sequence. The second part shows how to insert this 'Explode' state into a Drawing tab.

Your Task: Create and Place an Exploded View

Part A: In the Assembly Tab

  1. Go back to your main Assembly tab.
  2. On the right side of the screen, find and click the Exploded views icon.
  3. Click Add exploded view.
  4. Now, create the exploded state. Click a component (like a screw or bracket), and use the manipulator to drag it along an axis away from the main assembly. Each movement creates an "Explode step."
  5. Continue this process for several key components until the assembly is clearly "opened up." You can select multiple identical parts (like all the screws) to move in a single step.
  6. Once you are satisfied, click Done. You can double-click the "Explode 1" state in the panel to see it again.

Part B: Back in the Drawing Tab

  1. Return to your drawing tab.
  2. Click the Insert View tool.
  3. In the dialog, select your assembly.
  4. Now, find the dropdown menu labeled Explode/Position. Select Explode 1 (or whatever you named your exploded view).
  5. Place this new, exploded isometric view on your drawing sheet. This will be the view we use for our BOM callouts.

3. Bill of Materials (BOM) and Callouts

The Bill of Materials is the master parts list for your design. Onshape automatically generates this table from the assembly, listing every part and its quantity. Callouts, or balloons, are numbered labels that link each part in the drawing view to its corresponding line item in the BOM.

Your Task: Add the BOM and Callouts

  1. Insert the BOM Table:

    • Find the BOM table icon in the toolbar.
    • Onshape will prompt you to select the assembly for which to generate the BOM (it's usually pre-selected if you only have one).
    • Click to place the table, typically in the top-left or bottom-right corner of the drawing sheet. The table will automatically populate with item numbers, quantities, and part names.

  2. Add Callouts:

    • Click the Callout tool in the toolbar.
    • In your exploded isometric view, click on the edge of a part, then click again to place the balloon. The number in the balloon will automatically correspond to the item number in the BOM table.
    • Add callouts for several, if not all, of the parts in your exploded view. Try to arrange them neatly around the view.

For a text-based reference on this process, you can consult the official Onshape learning materials.

BOMs and Callouts - Introduction to Drawings

The Onshape Learning Center provides a self-paced course on drawings. This specific section covers BOMs and Callouts and can serve as a great written reference for the video you just watched.

Navigate to the section titled 'Notes and Tables' and find the lesson 'BOMs and Callouts'. Skim through this to reinforce your understanding of how to insert the BOM table and apply the callouts.

Test your understanding!

After placing your BOM, you realize it only shows 'Item', 'Quantity', and 'Part number'. Your company's standard requires a 'Material' column as well. How would you add this column to the BOM table on your drawing?

Show answer

You would need to edit the BOM table. You can typically do this by right-clicking on the BOM table and looking for an option like 'Properties' or by selecting the table and using a context menu. In Onshape, you can simply right-click a column header in the BOM table and choose 'Add column'. A dialog will appear allowing you to select from various part properties, including 'Material', to add to the table. This is powerful because the material data is pulled directly from the properties you assigned to each part in its Part Studio.

Conclusion

Congratulations! You have now created a complete, professional-grade assembly drawing. This document clearly communicates the design's form, the relationship between its parts, and the list of components required to build it. This is a critical skill for any design engineer and a fantastic piece to include in your portfolio.

Key Takeaways:

  • Assembly drawings are created in a dedicated Drawing tab and are parametrically linked to your 3D models.
  • The standard layout includes orthographic views (front, top, side) for dimensioning and an isometric view for visualization.
  • Exploded views must first be defined in the Assembly environment before they can be placed in a drawing.
  • The Bill of Materials (BOM) is automatically generated from the assembly data, saving significant time and reducing errors.
  • Callouts are used to link the parts shown in a view directly to their item numbers in the BOM table.

Preview of the Next Lesson:
With this lesson, you've completed the fundamentals of Onshape CAD: sketching, part modeling, assembling, and creating drawings. You now have the core skills to model and document a mechanical design. In our next module, we'll step back and look at the bigger picture of the engineering workflow. We will start at the very beginning of a project by learning how to write clear design requirements and specifications for a mechanical system. This will set the stage for our future projects and align with the goal of simulating a real-world engineering process.