Day 29 of Learn Fusion 360 in 30 Days for Complete Beginners! – 2023-24 EDITION – Introduction to Autodesk Fusion’s Drawing Workspace

Drawing Demo File

Use the Day #1 toy block for this lesson. If you have not completed Day #1, use the file here: https://a360.co/39UUWLw

Select the Fusion ‘share link‘ above > select the ‘Open in Fusion’ button > select ‘Open’ when prompted. This will open the demo file in your Autodesk Fusion application. Everything is set up and ready to use with the tutorial.

Key Terminology for Drawing Workspace in Autodesk Fusion

• Drawing Workspace: The area in Fusion 360 where 2D drawings are created from 3D models.
• Base View: The initial view of the 3D model from which other views are derived in the drawing.
• Projected View: Additional views generated from the base view, including front, top, right, and isometric views.
• Section View: A cut-through view showing the internal features of a part or assembly.
• Detail View: An enlarged view of a specific area to highlight intricate details.
• Auxiliary View: A view that is projected perpendicularly to a selected edge or face, often used for inclined surfaces.
• Bill of Materials (BOM): A table listing all the components, materials, and quantities used in the assembly.
• Title Block: A section of the drawing that contains important information such as the drawing title, author, date, and scale.
• Annotations: Notes and symbols added to the drawing to provide additional information, such as dimensions, tolerances, and material specifications.
• Dimensions: Numerical values that define the size and location of features on the drawing.
• Tolerances: Allowable variations in dimensions to ensure proper function and fit of the parts.
• Symbols: Graphical representations used to convey specific information, such as surface finish, welds, and geometric dimensioning and tolerancing (GD&T).
• Drawing Sheet: The physical or virtual paper on which the drawing is created, defined by its size and layout.
• Views: Different orientations of the 3D model displayed on the drawing sheet.
• Centerlines and Center Marks: Lines and marks used to indicate the center of holes, arcs, and other symmetrical features.
• Templates: Predefined drawing formats that can be reused to maintain consistency across multiple drawings.

Transcript

Welcome to Day #29 of Learn Fusion 360 in 30 days!

Fusion’s Drawing workspace lets you quickly create manufacture drawings from design or animation files.

A “drawing” is a collection of sheets that document a design using scaled 2D orthographic and isometric views, along with annotations and tables, to assist in manufacturing.

Let’s use the toy block from Day 1.

There are a couple of ways to create a new drawing. In the Data Panel, we can right-click and select “New Drawing from Design.”

With the file open, we can go to File, New Drawing, and select “From Design.”

Lastly, we can select the Drawing Workspace from the workspace dropdown menu, and choose “From Design”.

In the “Create Drawing” dialog, we can choose whether to create the drawing automatically or manually. The Automatic creation is a powerful new addition to Fusion that generates your drawing in a few minutes. However, this is not available to the free Personal Use license, so we’ll briefly look at this workflow at the end of this video.

Let’s proceed with the “traditional” method of manually creating a drawing.

In the case of our Toy block, we only have one component so we can leave this set to the “Full assembly” option. If we had a design file with many components, we could select components or use “Visible only” to automatically select all visible components.

The drawing option will only have “Create New” if this is the first drawing created with the associated file. If you’ve already started one you could choose from an existing drawing.

Drawing templates allow us to start with a custom title block, borders, document and sheet settings, and more.

We’ll start with a new blank drawing using the “From Scratch” option.

We can then define our desired drafting standards, units of measure, and sheet size. In many cases, these will be determined by the manufacturer, company preference, or location.

Note that we can always change the units of measure after starting the drawing.

Let’s leave these set to the defaults and select OK.

Upon entering the Drawing workspace, we’re prompted to place the “Base View.”

In a 2-dimensional drawing, a base view is the direct projection of the 3D design. After you click to place a base view on a sheet, you can generate additional projected, section, and detail views from it.

However, you’ll see that we can change the orientation, scale, style, and visibility before we place the base view.

Let’s make sure this is set to the Front view and we’ll click anywhere on the drawing sheet to place the base view… and we’ll click OK to close the dialog.

Once a view is placed on the sheet, we can click and drag on the view to reposition it.

Most manufacture drawings will include orthographic views to share the necessary dimensions and details.

Orthographic projection is a way of representing a 3D object by using multiple 2-dimensional views of the object. 

We’ll use the “Projected View” option to create the additional orthographic views. Once active, we need to select a base view to create the projections.

We then get a preview of the projected view as we drag around our mouse cursor.

Let’s click to place a projected view above the base view. We’ll repeat this below the base view…. and to the right of the base view.

We can also create a 3D isometric view by placing one in the lower right corner.

After placing the views, we’ll want to press the Enter key or select the checkmark.

Before we add the necessary dimensions to our drawing, we’ll want to consider what style and edge visibility are necessary.

Because we have internal components, such as the cylinders, we’ll want to keep them visible on at least one view.

At any time, we can double-click on any view to edit the settings.

One important thing to note is that changing our base view will change all other views. For example, double-click the base view and change the style to Visible Edges only.

Notice how all five views are updated.

Contrary, we can select one of the projected views to change the settings on an individual view. This will not affect the other views.

For example, we’ll change the right-side view to include “Visible and Hidden edges.”

Let’s also select our isometric view and change the style to “Shaded.” 

Notice this shades our toy block with the previously applied red appearance.

We can click and drag to move this to the upper right corner.

Let’s also leave more space between our orthographic views. You’ll find that because these are driven from our base views, they are connected and need to stay in line with the base view, which is a good practice to follow when creating scaled drawings for manufacturing.

Before we go any further, let’s save our drawing.

Notice that Fusion’s drawings place us in a new tab and we’re able to create and save as many drawing files as needed.

Another important callout is the ability to create additional drawing sheets at the bottom. Hobbyists on the free personal Use license are limited to one drawing sheet per drawing.

When using the other Fusion licenses, you can select the plus button to generate new drawing sheets, allowing you to document other parts of the design as needed.

You can also right-click on the drawing sheets to duplicate, rename, delete, print, or export them.

Under the Create Menu, you’ll find additional drawing options such as the ability to create section views, detail views, and more advanced view types.

However, I want to bring your attention to the Create Sketch feature.

At times, you may need to add custom geometry or documentation using sketches. It’s important to note that sketches in the Drawing workspace are for documentation objects only. You will not see constraints and many of the other sketching tools. These sketches are not the same as the sketches you create in the Design workspace.

We’re now ready to add dimensions to our 2D drawing.

Fusion offers many types of dimension tools that can help dimension-specific geometry.

Most of the time you’ll start with the standard Dimension tool that creates dimensions based on the geometry you select. Dimension can be activated with the shortcut letter “D” or from the Dimension menu.

Once active, select points, edges, or existing dimensions on the sheet. Fusion will attempt to guess the most appropriate dimension type based on your selection.

To start, let’s dimension our length and width on the base view.

Remember we added a small fillet to the top of the block, which means if we select the left edge our dimension will not be correct. We can instead select the top edge and bottom edge. Notice our dimension moves with our mouse cursor as we drag to the left. Click with your mouse again to place dimensions.

The dimension tool remains active. Let’s select the bottom line to define the length.

Once that is placed, let’s select the corner edge and the inside wall, defining the wall thickness of our block.

On our top view, let’s define the diameter of the nub.

If you have trouble finding the desired dimension type, remember you can utilize a specific dimension type from the menu, such as the diameter dimension tool.

This will limit your selection to only items that accept a diameter dimension.

You will also find that zooming in on the drawing can make it easier to select the specific points of your drawing.

We also need to define how far the center of the nub is from the edge. With the regular Dimension tool, let’s select the center of the nub, followed by one of the edges of the block.

At any time, we can delete dimensions if needed. Press the escape key to clear out the dimension tool, select the dimension, and press the Delete key.

Let’s define our wall thickness on the right side view instead of the bottom view.

Take a minute to dimension the diameter of the inside cylinders. 

We’ll now add a Detail View because our fillets are hard to see.

With Detail View active, we’ll select the base view, which allows us to select the desired area.

Select the corner of the block. Then, define the size of the detailed view. Let’s ensure it’s large enough to encompass the full corner and top nub and we’ll click again to place the circle.

Once the size is determined, we need to place our detailed view. Let’s place it below the isometric view.

We’ll make the style Visible Edges Only, and we’ll also change the scale to 8:1 so it’s easier to see.

This time let’s use the Radius dimension tool to define the two radii on the detailed view. Radius dimension makes it easier to select the fillet, without having to worry about selecting the other object snaps.

A typical 2D manufacturing drawing will list all of the necessary dimensions without repeating dimensions or listing items that would be known dimensions.

As a challenge, consider what remaining dimensions are needed to manufacture the toy block. Let me know in the comments below!

Let’s quickly cover a few last items to consider when working on 2D drawings.

First, you’ll notice that Fusion automatically filled out our Title block. This contains information about the design you are documenting, as well as a border.

At any time, double-click on the title block to edit the details.

You can also create templates and reuse title blocks, which is helpful in a commercial environment where consistency is critical.

We can also add text and notes to the drawing, calling out critical manufacturing details. This could be used for specific tolerances or other important annotations.

In the toolbar, you’ll find many industry symbols to add to your drawing sheets. Call out surface textures, welds, and so on.

You will also find Fusion offers the ability to create parts lists and tables, helping list out all of the necessary parts when working with multi-part assemblies.

Lastly, getting your Fusion drawing to the Manufacturer or factory – or simply in your own hands – is a critical step.

Personal Use license holders are limited to the print functionality. However, all other license types can export drawings as common file extensions such as PDF, DWG, or DXF. You can also export your tables and parts list to CSV files, allowing you to open them in Microsoft Excel or similar software.

As promised, let’s briefly take a look at the newer Automatic drawing creation. From the Create Drawing dialog, we’ll select Automatic instead of manual.

After selecting OK, Fusion will take up to a few minutes to generate the drawing.

You’ll find the progress in the Job Status dialog under the Drawing Automation section.

Once complete, we can open the drawing. We’re provided with different dimensioning strategies to choose from, and we can adjust the dimension density.

This process can help you reduce errors and time spent on tedious, repetitive tasks and lets you create consistent, pre-configured drawings at the push of a button.

The optional use of templates allows you to create additional drawings even faster without the need to adjust drawing settings and preferences.

Once created, Automated drawings are the same as Manual 2D drawings.  You can continue to edit them as needed.

You now know the basics of creating a 2D manufacturer drawing in Autodesk Fusion!

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I’ll see you on the final day, day #30 where we’ll look at Autodesk Fusion’s Animation Workspace.

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