From a 3D model of a gearbox, create a package of drawings of the whole assembly and its individual parts.

Open the gearbox model and create a named view

Open the design file for the gearbox and create a named view of the crank arm that you'll use in a later step.

If the Data Panel is not open, click Show Data Panel .
In the Data Panel, open 7_Drawings from Projects > Samples > Workshops & Events > Adoption Path > Mechanical Assembly > 7_Drawings. The design appears on the Autodesk Fusion canvas.
From the navigation bar at the bottom of the Fusion design window, click Look At.
Select a face on the crank arm.

The display changes to a side view of the assembly.
In the browser, expand the Named Views folder.
In the browser, right-click the Named Views folder and select New Named View.
In the browser, click the label for the new named view, and change it from Named View to Crank Arm.
At the top of the Fusion design window, click Save.

Create a new drawing from the gearbox model

In this step, you create a 2D drawing package from the gearbox model and specify drawing settings.

From the workspace drop-down menu, choose Drawing > From Design.
In the Create Drawing dialog, specify the following values:
- Select Full Assembly.
- Set Drawing to Create New.
- Set Template to From Scratch.
  
  As an alternative, you can use a saved template with a custom title block and logo.
- Set Standard to ASME.
- Set Units to In.
- Set Sheet Size to D (34in x 22in).
- Click OK.
  
  A drawing sheet appears, with a front view of the assembly attached to the cursor.
In the Drawing View dialog, specify the following values:
Move the cursor to the left side of the drawing sheet, and click to place the base view there.
In the Drawing View dialog, click OK. A drawing of the view appears on the drawing sheet.

To the left of the drawing sheet, the browser lists all the parts in the assembly. By toggling the light bulb next to a part, you can show or hide it in the drawing.

Create projected views of the assembly

In your drawing, create projected views from the base view.

In the Drawing workspace, choose Drawing Views > Projected View.
Click the base view to select it.
Place a projected view above the base view.
Place another projected view to the right of the base view.
Place a third projected view diagonally up and to the right of the base view.
Press Enter. The three projected views now appear as drawings.
Click the base view to select it. A small square appears.
Drag the small square to move the base view down and to the left. When you move the base view, the projected views move with it.

Create a large isometric view on a new sheet

Add a drawing sheet and create a large isometric view of the whole assembly. Edit the view and then move the new sheet to the front of the drawing package.

Click Add Sheet in the lower-left corner of the window.

A new sheet appears on the canvas. Thumbnails show the collection of sheets.
Choose Drawing Views > Base View.
In the Drawing View dialog, specify the following values:
- Set Orientation to NW Isometric.
- Set Style to Visible Edges.
- Set Scale to 3:1.
- Set Tangent Edges to Off.
- Leave Interference Edges and Thread Edges unselected.
Move the cursor to the center of the drawing sheet, and click to place the view.
In the Drawing View dialog, click OK. The drawing appears.
Right-click the canvas and select Edit View from the Marking menu.
Click the view to select it.
In the Drawing View dialog, make the following changes:
- Set Style to Shaded.
- Set Tangent Edges to Shortened.
In the lower-left corner of the window, drag the thumbnail of the new sheet to the left so that it comes first in the sheet order.

Create a new sheet for views of the crank arm

Use the named view of the crank arm you defined earlier to create base and projected views of that part on a new sheet.

Click Add Sheet in the lower-left corner of the window.
Choose Drawing Views > Base View.
In the Drawing View dialog, specify the following values:
- Set Orientation to Crank Arm (the named view you defined earlier).
- Set Scale to 3:1.
Move the cursor to the left side of the drawing sheet, and click to place the view.
Click OK. The drawing appears.
In the browser, right-click the Crank Arm component and select Suppress All Except Selected. All parts of the assembly except the crank arm disappear from the drawing.
Choose Drawing Views > Projected View.
Create projected views of the crank arm as you previously did for the whole assembly.

Create a section view of the assembly

Using the drawing sheet with projected views of the assembly, create a section view.

Click the thumbnail of the drawing sheet with the projected views of the assembly.

The drawing sheet fills the canvas.
Choose Drawing Views > Section View.
Click the top view to select it.
Select starting and ending points to designate a line running through the middle of the view.
Press Enter.
Move the cursor below the parent view, and click to place the section view there.

Placement of the section view determines its orientation. For example, if you place the section view above the parent view, it is oriented in the opposite direction.
Click OK. The section view appears with a label.

Note: When creating a section view, you can selectively turn off objects to be cut in the Drawing View dialog. For example, to leave the small bushings uncut, deselect them.

Create a detail view

Using the base view of the assembly, create a detail view. A detail view is an enlarged section of the drawing.

From the navigation bar, use the Pan and Zoom tools to focus on the base parent view of the assembly.
Choose Drawing Views > Detail View.
Click the parent view to select it.
In the Drawing View dialog, set Scale to 2:1.
Click a center point and drag outward to draw a circle that encompasses the area for the detail view, to the right of the assembly.

An enlarged section appears.
Drag the enlarged section to locate it, and click to place it.
Click OK. The detail view appears with a label.
Select the view, and use the gray square to move the view away from the circle.
To enlarge the circle on the parent view, drag the circle outward.

The detail view is automatically updated to include the area from the enlarged circle.

Create center marks and centerlines

Use the Centerlines command to add centerlines and center marks to the crank arm drawing views.

Click the thumbnail for the crank arm views to display that drawing sheet on the canvas.
Choose Centerlines > Center Mark.
Select the outside perimeter of the left circular end of the crank arm and the inner circles of the right end.

Center marks appear across all the circles on the left side and the two inner circles on the right side.
Choose Centerlines > Centerline.
Select the top and bottom linear edges of the end of the crank arm. A centerline appears halfway between the two edges.
Lengthen the centerline by dragging the handles on each end.

Create annotations

Add dimension annotations and a text leader to the top view of the crank arm.

Use the navigation controls to bring the top view of the crank arm into focus.
Click Annotation Settings at the bottom of the screen.
Using the Annotation Settings menu, specify the following values:
- Set Annotation Font to Arial.
- Set Annotation Text Height to 0.24 in.
- Set Linear Unit Format to Decimal.
- Set Linear Decimal Precision to 0.1.
- Set Angular Decimal Precision to 0.1.
- Leave Decimal Annotation Unit and Display Trailing Zeros unselected.
Choose Dimensions > Dimension.
Select the objects, points, and edges for which dimensions are needed in your drawing.

The Dimension command creates the most appropriate dimension type for each of your selections.

Although the Dimensions menu contains separate commands for linear, aligned, angular, radius, and diameter dimensions, the Dimension command is a "smart" command that chooses the appropriate dimension type. Fusion also allows you to create baseline, chain, and ordinate dimensions.
Choose Text > Leader.
Select the centerhole on the right end of the crank arm.
Drag to create the leader line, and click to specify the text location.
In the text box that appears, type Press Fit.
Click to finalize the leader.

NOTE You can also use the Symbols menu to annotate the drawing with surface texture symbols, feature control frames, and datum identifiers.

Add a bill of materials (BOM)

Create a parts list on the drawing sheet and show which parts of the drawing correspond to the items in the list.

Select the thumbnail of the drawing sheet with different views of the whole assembly.
Choose BOM > Parts List.
Move the cursor to the upper-right corner of the drawing sheet, and click to place the automatically generated parts list.
Choose BOM > Balloon.
Select each of the components in the drawing to place balloon references that correspond to the BOM.
Choose BOM > Renumber Balloons.
Select each balloon from left to right to renumber them in sequence. The BOM is automatically resequenced to match the new numbers.
Choose BOM > Align Balloons.
Select all the balloons, and then press Enter.
Select a starting point and an ending point for the alignment.

Save the drawing and create output

Save your drawing and then output a PDF file. The drawing updates when you revise the assembly.

Click Save, choose a location, and save the drawing. The drawing is associated with the assembly.
Choose Output > Output PDF.

You can also choose to create DWG output from the drawing, and you can create a template for customizing future drawings.
In the Output PDF dialog, set Range to All Sheets.
Navigate to a location to save the PDF file.

If you open a drawing after revising the corresponding assembly, click the warning icon at the top of the screen to update the drawing.

Inserting hardware from McMaster Carr

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