- 4-1 Introduction
- 4-2 Third- and First-Angle Projections
- 4-3 Fundamentals of Orthographic Views
- 4-4 Drawing Orthographic Views Using SolidWorks
- 4-5 Section Views
- 4-6 Drawing a Section View Using SolidWorks
- 4-7 Aligned Section Views
- 4-8 Broken Views
- 4-9 Detail Views
- 4-10 Auxiliary Views
- Chapter Projects
This chapter is from the book
This chapter is from the book
This chapter is from the book
4-6 Drawing a Section View Using SolidWorks
This section will show how to draw a section view of an existing model. In this example, the model presented as P4-22 in the Chapter Projects was used to demonstrate the concepts.
Start a new drawing using the Drawing format.See the previous section on how to create orthographic views using SolidWorks. Select the A (ANSI) Landscape format and select the ANSI standards.
Click the Model View tool on the View Layout panel.
In the Part/Assembly to Insert box click Browse.. . .See Figure 4-44. The Open box will appear. See Figure 4-45.
Figure 4-44
Click the model to be used to draw orthographic views, and click Open.In this example the model is called BLOCK, 3 HOLES. The dimensions for the BLOCK, 3 HOLES can be found in Figure P4-22.
A rectangular outline will appear defining the boundaries of the orthographic view. By default, this will be a front view. In this example we want a top view.
Click the Top view tool.See Figure 4-46.
Locate the top orthographic view on the drawing screen and click the mouse.
Add a center mark to the Ø30 hole.See Figure 4-47.
Click the View Layout tab and click the Section View tool.The orthographic view will be outlined by a dotted line.
Select a horizontal cutting plane line.
Define the location of the cutting plane line by moving the cursor to the approximate midpoint of the left vertical line of the orthographic view.The system will automatically jump to the line’s midpoint. A filled square icon will appear.
Click the green OK check mark.
Move the cursor downward.The section view will appear and move with the cursor. See Figure 4-48.
Select an appropriate location and click the mouse.
Click the Flip direction box if necessary.See Figure 4-49.
Add centerlines.
Click the green OK check mark.
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More than one section view may be taken from the same model. See Figure 4-50.
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The section views shown in Figure 4-50 use a hatching pattern made from evenly spaced 45° lines. This is the most commonly used hatch pattern for section views and is designated as ANSI 31 in the ANSI hatch patterns. SolidWorks can also draw section views using one of five different styles. See Figure 4-51.
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To Change the Style of a Section View
- Move the cursor into the area of the section view and right-click the mouse.
A listing of tools will appear, and the Display Style box will appear.
- Click the mouse again in the section view area to remove the list of tools.
- Click one of the boxes in the Display Style box.
Figure 4-52 shows two of the styles available: shaded with edge lines, and shaded. The hidden lines removed style is used for all other illustrations in this chapter.
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