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Drawings

Learn to create 2D drawings from a model or animation. This guide covers concepts of creating drawings, how-to add dimensions, balloons and annotations, and how-to create a BOM.

Overview

Start with this overview of the drawing tools and features available in Fusion 360.

  •  Dimension drawings with dimensioning tools

  • BOM, balloons, and parts lists

How to's

Learn to generate 2D drawings from models.  These videos provide everything you need to start a drawing, add dimensions, create views, and create a BOM.

  • Start a drawing

  • First drawing views

  • Add additional views

  • Add dimensions

  • Exploded view drawing and BOM

Hands-on Exercises

Now you’re ready to put your skills into practice.  Try these hands-on exercises to get started.

  • Create a drawing

  • Projected views and detailed views

  • Text and leader notes

Creating a Drawing

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Goals:

Understand how to create drawings by:

  1. Saving the Model
  2. Initiating a New Drawing
  3. Choosing the Assembly
  4. Committing a Base View

Instructions:

Step 1: Save the Model

With the Utility Knife design open, do the following:

  1. If the model is "Read Only" (indicated in the title bar), click File > Save As. Note: Even if a model is not "Read Only," you may wish to use the Save As command to preserve the original version of the model. Though a history of revisions is maintained, and you can revert to the original configuration, you might want to keep your changes confined to a new and separate version of the model.
  2. Optionally, create a new Project to store your training models. Click + Project to do so, specify the project name, and press Enter. After a short pause, the new project becomes the active project, and a blank file list appears on the right side of the Save dialog.
  3. Optionally, create a new folder within the project to store your training models. Click + Folder to do so, specify a folder name, and press Enter. Double-click the new folder to make it the current file saving location.
  4. Click Save.

Step 2: Initiate a New Drawing

With the Utility Knife design open, do the following:

  1. Click on File in the top menu bar.
  2. Select New Drawing ->From Design from the File drop-down menu.

Step 3: Choose the Assembly

  1. Activate the Full Assembly option in the dialog (if it is not already checked).
  2. Select ASME from the Drawing Format drop-down list.
  3. Select in from the Units drop-down list.
  4. Ensure that the B (17in x 11in) option is selected for the Sheet Size.
  5. Click OK to initiate the drawing. Notice that a new file tab is automatically generated.

 

Note: If you uncheck Full Assembly in the New Drawing dialog, you can select individual or multiple components to create a drawing of part of the assembly.
Tip: When selecting multiple components, it helps to use Ctrl+click.

You can set the drawing format, units, and sheet size before you create a drawing. However, you cannot change the drawing format or units after you create the new drawing.

Step 4: Commit a Base View

  1. Move your cursor around the screen. Notice that the Base View preview is attached to the cursor.
  2. Click on the top left quadrant of the sheet to place the view.
  3. Click OK to commit the view.

 

Note: After the view is committed, the shaded preview matures into a 2D line drawing of the view.

Projected Views and Detail Views

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Goals:

  1. Create Projected Views
  2. Use View Properties to customize Layout Views
  3. Create Detail Views
  4. Moving objects

Instructions:

Creating Projected Views

Step 1: Initiate a Projected View

Now that we've created a base view of the model assembly, let's create projected views and edit their properties to create a complete drawing layout.

  1. From the View Toolbar, select Projected View.
  2. Click the base view to select it as the parent view from which the projected views will be created and associated.

Step 2: Place the Views

  1. Drag the cursor to the right of the base view, and notice that the projected view is previewed based on this alignment.
  2. Select (click) to the right of the existing base view to place a projected view.
  3. Select to the bottom of the existing base view to place a second projected view.
  4. Press Enter to finish the task.

 

Note: A projected view inherits all its properties from the parent. When the properties of the parent view change, the corresponding properties on the projected view also change. You can change the properties of a projected view by double-clicking it.

Step 3: Create an Isometric Base View

  1. From the View Toolbar, select Base View.
  2. Click to place the view in the lower right of the sheet layout, above the title block.
  3. Set the Orientation to NE Isometric.
  4. Press OK to commit the view.

Note: A projected view inherits all its properties from the parent. When the properties of the parent view change, the corresponding properties on the projected view also change. You can change the properties of a projected view by double-clicking it.

Editing the Layout Views

Step 1: Edit the Isometric Base View

Now that you have created a base view and several projected views of the model, let’s use the View Properties settings to further customize the view layouts.

  1. Double-click anywhere inside the selection boundary of the isometric view to activate it.
  2. In the View Properties dialog, select 1:1 from the Scale drop-down list to scale the base view.
  3. Click Close to accept the drawing view changes.

Step 2: Edit the Right Projected View

  1. Double-click anywhere inside the selection boundary of the right projected view to activate it.
  2. In the View Properties dialog, select Visible and hidden edges from the Style drop-down list to display hidden lines in this view.
  3. Click Close to accept the drawing view changes.

 

Note: Once the projected view properties are changed, they no longer inherit the settings of the base view. If you change the properties back to “From parent,” they will once again inherit properties from the parent view.

Step 3: Edit the Bottom Projected View

Now that you have created a base view and several projected views of the model, let’s use the View Properties settings to further customize the view layouts.

  1. Double-click anywhere inside the selection boundary of the bottom projected view to activate it.
  2. In the View Properties dialog, select Full Length from the Tangent Edges drop-down list to display full length tangent edges in this view.
  3. Click Close to accept the drawing view changes.

Creating a Detail View

A detail view is a projected view that shows a specific portion of a view at an enlarged scale.

  1. From the View toolbar, select Detail View.
  2. Select the right side projected view as the parent view.
  3. Click the center point for the detail boundary (as shown in the image below).
  4. Click again to specify the size of the detail view boundary.
  5. Click to place the detail view in a clear area of the drawing sheet.
  6. In the View Properties dialog, select 2:1 from the Scale drop-down list to make the detail
    view larger.
  7. Click OK to generate the detail view.

Moving Objects

  1. Click anywhere on an object to select it. 
  2. Click the gray grip at the center of the object.
  3. Click a new location for the object.
    Note: The Move action works the same way for all views, text objects, dimensions, and balloons.

4. Move around the objects on your drawing so that they are nicely spaced, leaving the top right portion of the drawing space open. We will place a Parts List there later.

 

By now, your drawing should look something like this:

 

Text and Leader Notes

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Goals:

  1. Create Text
  2. Create Leader Notes
  3. Reposition Annotation and Edit Text

Instructions:

Step 1: Create Text

  1. In the Annotation toolbar, click Text.

2. Select two corners below the Front View to create a text box.  

3. Type the text, Front View into the text box.

4. Select anywhere outside of the text box to commit the action.

5. Repeat the process to add text below the other views (except for the Detail A, which is already labeled). Type the following text, respectively, into the three additional text boxes:

  • Bottom View
  • Right View
  • NE Isometric View

Step 2: Create Leader Notes  

  1. In the Annotation toolbar, click Leader Note.
  2. Click the blade in the bottom view to place the start of the leader.
  3. Click outside of the view to place the end of the leader.
  4. Type the text, Steel Blade.
  5. Select anywhere outside of the text box to commit the action.

 

Tip: When selecting a part, you'll see green shapes on the object. These are called Object Snap points, and they help you specify a precise point on the object (like an endpoint, a midpoint, or a center point).

Step 3: Reposition Leader Notes

  1. Click on the leader note to activate it.
  2. Click any of the gray grips to move the leader note to a new location.
  3. Click anywhere outside the leader note to commit the action.

Step 4: Edit Text

  1. Double-click on the leader note to activate the text editor.
  2. Click and drag the width slider icon (  ) to the right to format the text into 2 lines.
  3. Click anywhere outside of the text box to commit the action.