3.4.3.2: Module 13 Arcs

13

Module 13 Arcs

Wally Baumback

Learning Outcomes

When you have completed this module, you will be able to:

1. Describe the geometry of an arc and how arcs are drawn in Inventor.
2. Describe how to snap to midpoints of lines.
3. Apply the CENTER POINT ARC command to draw arcs in 2D sketches.

Drawing Arcs

There are three commands available to draw arcs in Inventor. In this module, drawing arcs using the CENTER POINT ARC command will be taught. Similar to the CIRCLE command, the CENTER POINT ARC command also requires you to select the centre point and the radius. Drawing arcs additionally require you to locate the start point and end point or the arc. Arcs can be constructed clockwise or counterclockwise.

Geometry Lesson: Arcs

An ARC is defined as an open curve in which all points are the same distance from its centre point. Study the drawings in Figure 13-1 and 13-2.for a description of the geometry of an arc.

Figure 13-1
Geometry of an Arc – Part 1 Figure 13-2
Geometry of an Arc – Part 2

Inventor Command: CENTER POINT ARC

The CENTER POINT ARC command is used to draw an arc by entering the location of its centre point, radius, start point and end point.

Shortcut: A

WORK ALONG: Drawing Models with Arcs

Step1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Enter the NEW command to start a new part file using the template: Metric-Modules Part (mm).ipt.

Step 3

Save the file with the name: Inventor Workalong 13-1. (Figure Step 3A and 3B)

Figure Step 3A
3D Model – Home View [Click to see image full size] Figure Step 3B
Dimensioned Multiview Drawing [Click to see image full size] USER TIP: When drawing arcs, do your best to tie the centre point, the start point, and the end point to existing geometry. It will decrease the number of dimensions that are required to constrain the arc.

Step 4

Edit Sketch1. Project the Center Point onto the sketch.

Step 5

Draw a sketch of the Top view of the model. Apply all of the geometrical and dimensional constraints to fully constrain it. (Figure Step 5)

Figure Step 5 [Click to see image full size]

AUTHOR’S COMMENTS: Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.

Step 6

Extrude the sketch in the positive Z direction. (Figure Step 6)

Figure Step 6

Step 7

Start a new sketch on the right side as shown in the figure. (Figure Step 7)

Figure Step 7

Step 8

Enter the CENTER POINT ARC command and when prompted for the centre point, right click the mouse. In the Right-click menu, select Midpoint. (Figure Step 8)

Figure Step 8

Step 9

Move the cursor onto the vertical edge. When the green snap icon appears, click the left mouse button. (Figure Step 9)

Figure Step 9

Step 10

Move the cursor approximately 10 mm along the edge and when the Snap onto icon displays, click the mouse. (Figure Step 10)

Figure Step 10

Step 11

Move the cursor to the other side of the centre and when the Snap onto icon displays, click the mouse. (Figure Step 11)

Figure Step 11

Step 12

Press F8 to display the constraint icons. (Figure Step 12)

Figure Step 12

Step 13

Move the cursor onto the Coincident icon and note the display of two coincident icons. (Figure Step 13)

Figure Step 13

AUTHOR’S COMMENTS: When two constraint icons display, it means that the endpoint of the arc is exactly on the line and the line is exactly on the endpoint of the arc.

AUTHOR’S COMMENTS: Note that the bottom endpoint of the arc is not constrained with a Coincident constraint.

Step 14

In the Graphic window, right click the mouse. In the Right-click menu, click Create Constraint and then Coincident. (Figure Step 14)

Figure Step 14

Step 15

Select the edge for the first point. (Figure Step 15)

Figure Step 15

Step 16

For the second point, move the cursor onto the endpoint of the arc. When a small red point will displays, click the mouse. (Figure Step 16)

Figure Step 16

Step 17

Press F8. Locate the cursor onto the Coincident icon and note the display of two coincident icons. (Figure Step 17)

Figure Step 17

AUTHOR’S COMMENTS: Both ends of the arc are now geometrically constrained to the edge of model.

Step 18

The arc should now display purple indicating it is fully constrained. (Figure Step 18)

Figure Step 18

Step 19

Finish the sketch and extrude the arc by using the Cut option. (Figure Step 19)

Figure Step 19 [Click to see image full size]

Step 20

Start a new sketch on the front side. (Figure Step 20)

Figure Step [Click to see image full size]

Step 21

Draw a line perpendicular from the midpoint of the edge. (Figure Step 21)

Figure Step 21

AUTHOR’S COMMENTS: Ensure that you snap to the midpoint of the edge.

Step 22

Change the line to a construction line by selecting the line and then click the Construction icon. (Figure Step 22A, 22B, and 22C)

Figure Step 22A Figure Step 22B Figure Step 22C

Step 23

Offset the construction line on each side. (Figure Step 23)

Figure Step 23

Step 24

Insert two dimensions. (Figure Step 24)

Figure Step 24

Step 25

Draw an arc locating the centre at the end of the construction line. (Figure Step 25)

Figure Step 25

Step 26

Insert the required dimensions to constrain the sketch. (Figure Step 26)

Figure Step 26

Step 27

Enable the display of the constraint icons. (Figure Step 27)

Figure Step 27

Step 28

Use what you learned in Step 14 to 17, create the additional Coincident constraints to fully constrain the sketch. (Figure Step 28)

Figure Step 28

Step 29

Extrude the sketch to complete the model. (Figure Step 29)

Figure Step 29

Step 30

Change the colour to: Titanium – Polished. (Figure Step 30).

Figure Step 30

Step 31

Save and close the file.

Key Principles

Key Principles in Module 13

1. There are three commands available to draw arcs in Inventor. Similar to the CIRCLE command, the CENTER POINT ARC command also requires you to select the location of the centre point and the radius. Drawing arcs additionally requires you to locate the start point and end point or the arc. Arcs can be constructed clockwise or counterclockwise.
2. When drawing arcs, do your best to tie the centre point, the start point, and the end point to existing geometry. This will decrease the number of dimensions that are required to constrain the arc.

Lab Exercise 13-1

Time allowed: 45 minutes.

Part Name	Project	Units	Template	Color	Material
Inventor Lab Lab 13-1	Inventor Course	Inches	English-Modules Part (in).ipt	Chrome – Polished	N/A

Step 1

Project the Center Point onto the Base sketch.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size] Figure Step 2B
Suggested Base Sketch
– Right Side – YZ Plane

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3 Solid Model – Home View

Lab Exercise 13-2

Time allowed: 45 minutes.

Part Name	Project	Units	Template	Color	Material
Inventor Lab Lab 13-2	Inventor Course	Millimeters	Metric-Modules Part (mm).ipt	Copper – Satin	N/A

Step 1

Project the Center Point onto the Base sketch.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size] Figure Step 2B
Suggested Base Sketch –
Front – XZ Plane

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3
Completed Solid Model –
Home View