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# Getting Started

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## 1-9 Sample Problem SP1-1

Figure 1-23 shows a 2D shape sketched using the Line tool. The dimensions are in millimeters. This section will explain how to draw the shape.

1. Start a New Part document, select the Front Plane, and create a Sketch plane.

See Figure 1-24.

1. Define the dimensional units as millimeters, MMGS.

See Figure 1-25.

1. Click the Line tool.

2. Select the origin as the starting point for the first line.

See Figure 1-26.

1. Sketch the general shape as shown.

Note the double circle relation icon that appears when the end of the last horizontal line drawn is located on the starting point of the first line. This is the Concentric relation icon. The Concentric icon indicates that the two points occupy the same location. The midpoint of the right-side vertical line is also defined.

1. Click the Smart Dimension tool and dimension the shape as shown by clicking each line and entering the given dimensional value. See Figure 1-27.

SolidWorks is sensitive to how the dimensions are entered. See Figure 1-28. Note that when the vertical 40 dimension was added to the right side of the shape the adjacent horizontal 40 line moved upwards. This means that the two horizontal 40 lines are no longer aligned. The right 40 line must be fixed in place so that it remains aligned with the other horizontal 40 line when the vertical 40 dimension is added. The vertical 40 dimension will then move the bottom of the slot downwards.

### To Fix a Line in Place

1. Use the Undo tool to remove the vertical 40 dimension.

2. Click the right horizontal 40 line.

3. Click the Make Fixed tool.

The Make Fixed tool’s icon is an anchor. When the Make Fixed tool is activated, an anchor icon will appear below the line.

1. Use the Smart Dimension tool and add a vertical 40 dimension as shown.

The horizontal line at the bottom of the slot will move, accepting the 40 dimensional changes. The two horizontal lines remain aligned.

### Sketch Relations

Figure 1-29 shows a view of the object with and without Sketch Relations.

To remove the Sketch Relations icon:

1. Click the View tab at the top of the screen.

2. Click the Hide/ Show option.

3. Click the Sketch Relations option.