In this activity, you will create a drawing view from an existing part and place part drawing views.

Prerequisites

Download and open main-pump-body.f3d.

Steps-by-step:

Create a drawing from the part in main-pump-body.f3d.
1. Click the Workspaces tab and navigate to Drawing.
2. Select From Design.
3. Keep all the defaults in the Create Drawing dialog and click OK.
Place a Base View.
1. Since you started this drawing from an existing design, the Base View command is active.
2. In the Drawing View dialog, keep the Orientation as Front.
3. Set the Style to Visible Edges.
4. Set the Scale to 1:2.
5. Keep all the Edge Visibility as default.
6. Move the view to the upper left corner of the drawing and click to place the view.
7. In the Drawing view dialog, click OK.
Place a Projected View.
1. Select the Projected View command.
2. Select the base view that was just created.
3. Pull your mouse away to see a preview of the Projected View. (Notice how moving the mouse around the Base View changes the orientation of the Projected View you will create).
4. Move your mouse to the right of the base view and click to place the view.
5. Select the check mark to finish placing the view.
Place a Section View.
1. Select the Section View command.
2. Select the Projected View as the view you want to create a section view from.
3. Click above the view in the center of the part.
4. Draw a vertical line through the entire part.
5. Select the Check Mark that is over your line.
6. Pull the pointer to the right of the Projected View to see a preview of your Section View.
7. Click to place your Section View.
8. Keep all the defaults in the Drawing View dialog and click OK.
Place another Section View.
1. Select the Section View command.
2. Select the Base View as the view you want to create a section view from.
3. Click the left side of the Base View, right above the feet.
4. Draw a horizontal line over the left foot.
5. Select the Check Mark that is over your line.
6. Pull the pointer below the Base View to see a preview of your Section View.
7. Click to place your Section View.
8. Change the Scale to 1:1 and click OK.
Place a Detail View.
1. Select the Detail View command.
2. Select the Base View as the view you want to create a Detail View from.
3. Select the top hole in the Base View to start the Detail View.
4. Pull the pointer away from the whole to create a circle around the feature.
5. When you think the circle is big enough, click again to create a preview.
6. Move the pointer to the bottom-right corner of the drawing and click to place the view.
7. Keep all the defaults in the drawing view dialog and click OK.

Activity 1 summary

In this activity, you created a drawing and placed four views.

Placed views before and after

Before drawing views (left). After drawing views (right).

Intro to Fusion drawings for manufacturing

Objectives

Prerequisites

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