- 1-1 Introduction
- 1-2 Starting a New Drawing
- 1-3 SolidWorks Colors
- 1-4 Creating a Fully Defined Circle
- 1-5 Units
- 1-6 Rectangle
- 1-7 Moving Around the Drawing Screen
- 1-8 Orientation
- 1-9 Sample Problem SP1-1
- 1-10 Creating 3D Models
- 1-11 Saving a Document
- 1-12 Lines and Angles – Sample Problem SP1-2
- 1-13 Holes
- Chapter Projects
This chapter is from the book
This chapter is from the book
This chapter is from the book
1-4 Creating a Fully Defined Circle
In this section we will sketch a circle to help understand the difference between a fully defined and an under defined Part.
Start a New Part drawing and click the Top plane tool as defined in Figure 1-4.
Click the Sketch tab. (It may already be activated.)
Click the Circle tool.
Locate the cursor on the origin, click the mouse, and drag the cursor away from the origin center point.
Note that the Coincident relationship symbol appears next to the origin, indicating that the center point of the circle is located on the origin.
Click the mouse to define a sketch radius for the circle.
This is a temporary radius, that is, a sketched radius, and is not the final radius. The circle will be blue, indicating that it is not fully defined. See Figure 1-9.
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Click the Smart Dimension tool on the Sketch panel.
Click the circle and move the cursor away from the circle.
A dimension will appear. See Figure 1-10.
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Select a location for the dimension and click the mouse.
The circle will initially be blue, not fully defined, until the mouse is clicked, locating the circle’s dimension. When the mouse is clicked, the circle will turn black; it is now fully defined. We know the circle’s diameter and location.
When the mouse is clicked, the Modify dialog box will appear. The sketched diameter value will be listed in the box. This sketched diameter value is now the circle’s diameter until we enter a new value.
Enter a diameter value for the circle.
In this example a value of 2.00 was entered.
Click the green OK check mark in the Modify box to enter the diameter value.
Click the green OK check mark in the Manager area to finish defining the circle.
To Change an Existing Dimension
- Double-click the 2.00 dimension.
The Modify dialog box will reappear.
- Enter a new value.
In this example a value of 3.00 was entered. See Figure 1-11. The circle’s diameter will change to 3.00 and the circle’s color will remain black. The circle still is fully defined.
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Note that the words Fully Defined appear at the bottom of the screen.
The circle is fully defined because both its diameter and location are known. The location was fully defined when we located the circle’s center point on the origin. Every circle needs a locational value and a diameter value to be fully defined. The locational value may be linear, an X and Y component value, or polar, an angular and radius value.
Fully Defined Entities
To help understand when an entity is fully defined, sketch two circles, one with its center point on the origin and the other with its center point not on the origin. See Figure 1-12. Both circles are under defined because the diameter values have not been defined. Both circles are sketched circles.
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Use the Smart Dimension tool and define both their diameters as Ø2.00. The circle located on the origin will be black. It is fully defined. Both its diameter and location are known. The circle with its center point not located on the origin will remain blue. It is not fully defined. Its location is unknown. See Figure 1-13.
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Figure 1-14 shows the two Ø2.00 circles again. This time, dimensions have been added to the circle not located on the origin. The dimensions define the circle’s center point relative to the origin. It is now fully defined. Its color will change to black.
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Figure 1-15 shows the two Ø2.00 circles with an extra dimension. The 1.20 vertical dimension is not needed to define the location of the hole not centered on the origin. A 1.20 vertical dimension already exists. The 1.20 dimension is redundant, so the drawing lines change to yellow.
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Figure 1-15 also shows the Make Dimension Driven? dialog box. A driving dimension drives the shape and/or location of the object. If the driving dimension is changed, the shape or location will change. Driven dimensions are reference dimensions. They are sometimes added to a drawing for clarity. For example, a reference dimension could be used to show the overall value of a string of smaller dimensions. See Chapter 7, in this example it would be better to delete the extra 1.20 dimension. If you save it on the drawing, click the Make this dimension driven option and click OK. It will appear as a gray color. See Figure 1-16.
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