3-28 Curve Driven Patterns
Figure 3-54 shows a Ø4.00 inch ring with 12 holes though its side sur-
faces. The holes were created using the Curve Driven Pattern tool.
To Use the Curve Driven Pattern Tool – Example 1
See Figure 3-55.
1 Sketch the ring using the dimensions shown in Figure 3-54.
The outer diameter is Ø4.00, and the inner ring is Ø3.00. Both are cen-
tered on the origin working on the Top plane.
2 Extrude the ring a distance of 1.00.
3 Click the Front plane in the FeatureManager box, click the Plane
option under the Reference Geometry tool and create an offset plane
tangent to the front edge of the ring.
Ring
Origin
12 Holes
Figure 3-54
Front plane is located on the origin
Sketch the tool circles
Origin
Extrude a distance
of 1.00
Offset plane
Figure 3-55
202 Chapter 3 | Features
Figure 3-55 A normal view of Plane 1
Chapter 3
(Continued)
Use the Circle tool to sketch Ø.38 circle
Offset top plane
Offset distance is .50
Isometric View
Use the Extrude-Cut tool to
create the hole
Use the Circle tool to sketch
a Ø4.00 circle on the offset
plane, Plane 2
1. Click Insert
2. Click Pattern/
Mirror
Click Curve Driven Pattern
Chapter 3 | Features 203
Set for 12 holes
Check mark for equal spacing
Select the Ø.375 hole
Ring with 12 holes
Figure 3-55
(Continued)
The new plane is offset 2.00 from the origin, that is, from the center-
point of the ring. The new plane is defined as Plane 1 in this example.
4 Create a sketch plane on Plane 1, create a normal view to the plane,
and sketch a Ø0.375 circle 0.50 from the bottom edge of the ring.
5 Use the Extruded Cut tool and create a hole from the circle.
6 Click the Top plane in the FeatureManager box, click the Plane option
under the Reference Geometry tool, and create an offset Plane 0.50
above the initial Top plane used to create the ring.
In this example this plane is defined as Plane 2. Plane 2 is offset .50
from the initial top plane or halfway up the 1.00 thickness of the ring.
7 Create a sketch plane on Plane 2, and create a normal view.
8 Sketch a Ø4.00 circle on sketch plane, click the Exit Sketch icon, and
orientate the drawing to an isometric view.
204 Chapter 3 | Features
9 Click the Insert toolbar heading at the top of the screen, click the
Chapter 3
Pattern/Mirror option, and click the Curve Driven Pattern tool.
10 Select the hole as the Feature to Pattern, set the Number of
Instances to 12, click the Equal spacing box, and click OK.
11 Hide Planes 1 and 2, and the circle used to define the pattern.
To Use the Curve Driven Pattern Tool – Example 2
Figure 3-56 shows a part that has 12 holes offset 10 from the part’s outer
edge surface.
1 Use the given dimensions and draw the part as shown in Figure 3-56.
See Figure 3-57.
Figure 3-56
Chapter 3 | Features 205
Create a sketch
Profile plane
Centerpoint
for arc
Fillet
Locate the
centerpoint
of the arc by
touching the arc
with the cursor.
Create a Ø6.00
hole on the
horizontal
centerlines.
Use the Offset tool
to create a curve
line offset 10 from
the edge.
Figure 3-57
206 Chapter 3 | Features
Figure 3-57
Chapter 3
(Continued)
Number of copies
Activate Equal spacing
Feature
to pattern
2 Define a sketch plane on the top surface of the part and use the Offset
tool and create a curve offset 10 from the part’s outer edge.
Figure 3-57 shows a normal view of the top surface. The offset curve is
created using the Offset tool. Both the arcs and fillets can be offset to cre-
ate a continuous curve.
3 Draw a Ø6 hole centered on the intersection of the offset curve and the
horizontal center line of the part. The centerpoint is 40 from the part’s
origin.
4 Click the Insert toolbar heading at the top of the screen, click the
Pattern/Mirror option, and click the Curve Driven Pattern tool.
5 Select the hole as the Feature to Pattern, the offset curve as the Path,
and set the Number of Instances to 12; click the Equal spacing box,
and click OK.
Chapter 3 | Features 207
1 Create a new drawing, select the Top plane option, click the Sketch
tool, and set the units for millimeters (MMGS), and the Drafting
Standards for ANSI.
2 Use the Center Rectangle tool and sketch a rectangle about the origin.
3 Use the Smart Dimension tool and create an 80 3 80 square.
The square is centered about the origin.
4 Click the Exit Sketch option.
5 Click the View Orientation tool and select a Trimetric orientation.
6 Click the Features tab.
7 Click the Top plane option, click the Reference Geometry tool, and
select the Plane option.
A new plane, called Plane 1, will appear.
8 Offset Plane 1 60 from the top plane.
9 Right-click the mouse and click OK.
10 Right-click Plane 1 and click the Sketch option.
11 Use the Circle tool and sketch a circle centered about the origin in
Plane 1.
12 Use the Smart Dimension tool and dimension the diameter of the
circle to 50.0.
13 Click the Exit Sketch option and click the Lofted Boss/Base tool.
The Profiles box should turn on automatically; that is, it should be
blue in color.
14 Click the rectangle.
The rectangle may already have been selected.
15 Click the circle.
A preview of the lofted segment should appear.
16 Click the green OK check mark in the Loft PropertyManager box.
17 Right-click Plane 1 and select the Hide option.
18 Save the part as LOFT.
3-14 Shell
The Shell tool is used to hollow out existing solid parts. Figure 3-26 shows
a 35 3 40 3 60 box. It was created using the Corner Rectangle, Smart
Dimension, and Extruded Boss/Base tools.
Figure 3-26 A 40×60×35 Box
35
60 40
162 Chapter 3 | Features
Chapter 3
1. Click the Shell tool
2. Define Shell thickness
The resulting shell
4. Click
this face
3. Click this face
Figure 3-26
(Continued)
The Shell tool will be applied to the box.
1 Click the Features tab and click the Shell tool.
2 Define the shell thickness.
In this example, a thickness of 2.00 was selected.
3 Click the two faces of the box as indicated.
4 Click the green OK check mark.
Figure 3-27 shows two more examples of how the Shell tool can be
applied to parts.
Examples of Shell tool applications
Figure 3-27
Chapter 3 | Features 163
3-15 Swept Boss/Base
The Swept Boss/Base tool is used to sweep a profile along a path line. As
with the Lofted Boss/Base tool, existing shapes must be present before the
Swept Boss/Base tool can be applied. In this example, a Ø.50-inch circle
will be swept along an arc with a 2.50-inch radius for 120°. See Figure 3-28.
Create a Front plane, and
make it a Sketch plane
Sketched on
Top plane
Origin for both
planes
Origin
Sketched on
Top plane
Point 3
1. Use Centerpoint
Arc tool Point 2 Point 1
Set arc distance for 120º
Figure 3-28
164 Chapter 3 | Features
Figure P3-27 Figure P3-28
MILLIMETERS MILLIMETERS
Figure P3-29 Figure P3-30
INCHES (SCALE: 4 5 1) MILLIMETERS (SCALE: 2 5 1)
214 Chapter 3 | Features
Figure P3-31 Figure P3-32
MILLIMETERS MILLIMETERS
Figure P3-33 Figure P3-34
MILLIMETERS MILLIMETERS
Figure P3-35 Figure P3-36
MILLIMETERS MILLIMETERS
Chapter 3 | Features 215
Project 3-2:
A. Draw the following spring.
Diameter 5 2.00
Wire diameter 5 .125
Pitch 5 .375
Revolutions 5 16
B. Grind both ends to create a spring 2.00 long in its unloaded position.
Project 3-3:
A. Draw the following spring.
Diameter 5 25
Wire diameter 5 5 3 5 Square
Pitch 5 6
Revolutions 5 8
Figure P3-49 Figure P3-50 Figure P3-51
INCHES MILLIMETERS INCHES
Chapter 3 | Features 219
