Skip to main content
Workforce LibreTexts

3.3: Module 14 Revolving

  • Page ID
    19878
  • \( \newcommand{\vecs}[1]{\overset { \scriptstyle \rightharpoonup} {\mathbf{#1}} } \) \( \newcommand{\vecd}[1]{\overset{-\!-\!\rightharpoonup}{\vphantom{a}\smash {#1}}} \)\(\newcommand{\id}{\mathrm{id}}\) \( \newcommand{\Span}{\mathrm{span}}\) \( \newcommand{\kernel}{\mathrm{null}\,}\) \( \newcommand{\range}{\mathrm{range}\,}\) \( \newcommand{\RealPart}{\mathrm{Re}}\) \( \newcommand{\ImaginaryPart}{\mathrm{Im}}\) \( \newcommand{\Argument}{\mathrm{Arg}}\) \( \newcommand{\norm}[1]{\| #1 \|}\) \( \newcommand{\inner}[2]{\langle #1, #2 \rangle}\) \( \newcommand{\Span}{\mathrm{span}}\) \(\newcommand{\id}{\mathrm{id}}\) \( \newcommand{\Span}{\mathrm{span}}\) \( \newcommand{\kernel}{\mathrm{null}\,}\) \( \newcommand{\range}{\mathrm{range}\,}\) \( \newcommand{\RealPart}{\mathrm{Re}}\) \( \newcommand{\ImaginaryPart}{\mathrm{Im}}\) \( \newcommand{\Argument}{\mathrm{Arg}}\) \( \newcommand{\norm}[1]{\| #1 \|}\) \( \newcommand{\inner}[2]{\langle #1, #2 \rangle}\) \( \newcommand{\Span}{\mathrm{span}}\)\(\newcommand{\AA}{\unicode[.8,0]{x212B}}\)

    14

    Module 14 Revolving

    Wally Baumback

    Learning Outcomes

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

    1. Describe a centerline object and explain how it is inserted and used in a 2D Sketch.
    2. Describe how a Base sketch is revolved with and without the use of a centerline to create a solid model.
    3. Apply the REVOLVE command to create a solid model from a Base sketch.

    Revolving

    When drawing symmetrical objects it is much easier to create the model by revolving the Base sketch around an axis rather then extruding it. The axis, which can be one of the lines in the sketch or a centerline, must always be located in the centre of the symmetrical model. The sketch can be revolved any angle between 0 and 360 degrees.

    In this module, the basic features of the REVOLVE command are taught. The Inventor Advanced book will cover the more advanced features.

    The models in Figure 14-1 and 14-2 were created by revolving the same Base sketch around an axis. Take note how the two solid models that were created using the same sketch are quite different. In Figure 14-1, the line on left side of the sketch was used as the axis while in Figure 14-2, it was the centerline that was used as an axis or revolution.

    14-1.jpg
    Figure 14-1
    A 2D Sketch Revolved Around a
    Line in the Sketch
    14-2.jpg
    Figure 14-2
    The Same 2D Sketch Revolved
    around a Centerline

    Inventor Command: REVOLVE

    The REVOLVE command is used to create a solid model by revolving the Base sketch around an axis.

    Shortcut: R

    revolve.jpg

    Centerlines

    A centerline is a line with its properties set to act as a centerline. In the REVOLVE command, a centerline is automatically recognized as the axis for the revolution. The two methods of drawing a centerline, which is similar to drawing construction a line, are as follows:

    Method 1

    Draw the line using the LINE command and then select it. While it is selected, click the Centerline icon.

    Method 2

    Enable the Centerline icon and then draw the line, using the LINE command. The Centerline icon is shown in Figure 14-3. A centerline will display as the centerline linetype.

    14-3.jpg
    Figure 14-3
    Centerline Icon

    WORK ALONG: Revolving a Sketch Without using a Centerline

    Step 1

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

    Step 2

    Using the NEW command, start a new part file using the template: English-Modules Part (in).ipt.

    Step 3

    Save the file with the name: Inventor Workalong 14-1. (Figure Step 3A and 3B)

    work-along-3A-2-1.jpg
    Figure Step 3A
    3D Model
    work-along-3B-2-1.jpg
    Figure Step 3B
    Dimensioned Multiview Drawing [Click to see image full size]
    AUTHOR’S COMMENTS: In this and the next workalong, you will be constructing the same solid model. In this workalong without the use of a centerline, and the next workalong with the use of a centerline. Either method is an acceptable way of creating the solid model. These two workalongs will allow you to practice both methods.

    Step 4

    Start a new sketch on the Front or XZ Plane. Project the Center Point onto the sketch.

    Step 5

    Draw and dimension one-half of the Front view as shown in the figure. Ensure that the sketch is fully constrained (Figure Step 5)

    Fig-Step-5-7.jpg
    Figure Step 5
    AUTHOR’S COMMENTS: Note how the sketch is a profile of the object, that when revolved, will create the solid model. For now, ignore the centre hole and the 4 small holes. The line located in the centre of the model is used as the axis. The holes will be inserting after the sketch is revolved to complete the solid model.
    AUTHOR’S COMMENTS: Your geometrical and dimensional constrains may not match the figure exactly. Ensure that the sketch is fully constrained.

    Step 6

    In Model mode, enter the REVOLVE command. It will highlight the sketch automatically as the area to revolve. (Figure Step 6)

    Fig-Step-6-5.jpg
    Figure Step 6 [Click to see image full size]

    Step 7

    In the Revolve dialogue box, set the Extents to Full and enable the Axis icon. Select the line on the right side of the sketch as the axis. The Full setting means that it will be revolved 360 degrees. (Figure Step 7)

    Fig-Step-7-9.jpg
    Figure Step 7 [Click to see image full size]

    Step 8

    After you select the axis, the REVOLVE command will display the Base model as it is revolved. If this is the desired outcome, click OK. (Figure Step 8A and 8B)

    Fig-Step-8A-2.jpg
    Figure Step 8A [Click to see image full size]
    Fig-Step-8B-2.jpg
    Figure Step 8B

    Step 9

    Start a new sketch on the top plane of the model. (Figure Step 9)

    Fig-Step-9-9.jpg
    Figure Step 9

    Step 10

    Using what you learned in Module 12, draw a construction circle and four construction lines. Insert a dimension for the diameter of the circle. Ensure that the sketch is fully constrained. (Figure Step 10)

    Fig-Step-10-6.jpg
    Figure Step 10
    AUTHOR’S COMMENTS: Ensure that you snap the lines correctly when you draw them. If you don’t, you will have trouble fully constraining the sketch. If you have trouble doing this step, look at the workalong in Module12.

    Step 11

    Using the technique that you learned in Module 12, draw the 4 circles. Dimension one and constrain the additional 3 with an Equal constraint. (Figure Step 11A and 11B)

    Fig-Step-11A.jpg
    Figure Step 11A
    Fig-Step-11B.jpg
    Figure Step 11B
    AUTHOR’S COMMENTS: Your geometrical and dimensional constrains may not match the figure exactly. Ensure that your sketch is fully constrained.

    Step 12

    Extrude the four circles to the To Next extents. (Figure Step 12)

    Fig-Step-12-7.jpg
    Figure Step 12 [Click to see image full size]

    Step 13

    Start another sketch on the top plane and draw a circle by offsetting the outside diameter. Dimension the circle and extrude it to complete the model. (Figure Step 13)

    Fig-Step-13-9.jpg
    Figure Step 13 [Click to see image full size]
    AUTHOR’S COMMENTS: Using an offset, will automatically constrain the circle.

    Step 14

    Change the colour to: Aluminum – Polished. (Figure Step 14)

    Fig-Step-14-6.jpg
    Figure Step 14

    Step 15

    Save and close the file.

    WORK ALONG: Revolving a Sketch using a Centerline

    Step 1

    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: English-Modules Part (in).ipt.

    Step 3

    Save the file with the name: Inventor Workalong 14-2. (Figure Step 3)

    work-along-revolve-3.jpg
    Figure Step 3
    Dimensioned Multiview Drawing

    Step 4

    Start a new sketch on the Front or XZ Plane. Draw and dimension a line start it by snapping to the Center Point. Draw it 5 inches in the negative Y direction. This is the length of the model. This is centerline of the solid model. Change the line’s properties to a centerline. (Figure Step 4A and 4B)

    Fig-Step-4A-1.jpg
    Figure Step 4A
    Fig-Step-4B-1.jpg
    Figure Step 4B

    Step 5

    Draw and dimension one-half of the Front view as shown in the figure. (Figure Step 5A and 5B)

    Fig-Step-5A-2.jpg
    Figure Step 5A [Click to see image full size]
    work-along-5b.jpg
    Figure Step 5B [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

    Return to Model mode and enter the REVOLVE command. Since a centerline is part of the sketch, the REVOLVE command will automatically use it as the axis to revolve the sketch around. It will display the outcome of the revolution. (Figure Step 6)

    Fig-Step-6-revolve.jpg
    Figure Step 6 [Click to see image full size]

    Step 7

    In a new sketch, add the four smaller circles and extrude them to complete the model.

    Step 8

    Change the colour to: Aluminum – Polished. (Figure Step 8)

    work-along-fig-step-8-1.jpg
    Figure Step 8

    Step 9

    Save and close the file.

    Drafting Lesson: Cross Sections

    When a view of an object requires a clearer description of its interior or it is hard to dimension because of the hidden lines, a cross section view can be drawn in place of the normal multiview. See Figure 32-1

    Fig-32-1.jpg
    Figure 32-1
    Normal Front and Right Side View of an Object

    A cross section view, also called a section, is a view of the object as if it were cut along a cutting plane and the two pieces pulled apart exposing the inside of the object. See Figure 32-2 and 32-3.

    Fig-32-2-1.jpg
    Figure 32-2
    A Front view and Right
    Side Section View
    Fig-32-3-1.jpg
    Figure 32-3
    3D Model of the Object
    Showing it Cut on the
    Cutting Plane Line

    A cutting plane line is the line along the object where the cut would have been made. See Figure 32-2. The arrows point in the direction that you are looking when drawing the section view. The surfaces of the object that are solid, when cut, are crosshatched.

    Key Principles

    Key Principles in Module 14

    1. When drawing symmetrical objects, it is much easier to create the model by revolving the Base sketch around an axis rather then extruding it. The axis, which can be one of the lines in the sketch or a centerline, must always be located in the centre of the symmetrical MODEL.
    2. A centerline is a line with its properties set to act as a centerline.

    Lab Exercise 14-1

    Time allowed: 60 minutes.

    Part Name Project Units Template Color Material
    Inventor Lab Lab 14-1 Inventor Course Millimeters Metric-Modules Part (mm).ipt Copper – Polished N/A

    Step 1

    Project the Center Point onto the Base plane.

    Step 2

    Note the location of X0Y0Z0. Draw the Base sketch and revolve it create the Base model of the object shown below. Revolve it by using a line in the sketch. Do not draw a centerline. (Figure Step 2A and 2B)

    14-2-2A.jpg
    Figure Step 2A
    Dimensioned Multiview Drawing
    14-2-2B.jpg
    Figure Step 2B
    Suggested Base
    Sketch – Right Side –
    YZ Plane

    Step 3

    Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.

    Step 4

    Apply the colour shown above. (Figure Step 4A and 4B)

    14-1-4a-e1624569937583.jpg
    Figure Step 4A
    Completed Solid Model
    – Home View
    14-1-4b-e1624569950323.jpg
    Figure Step 4B
    Completed Model
    – Rear View

    Step 5

    Add the four small holes on a new sketch and extrude them.

    AUTHOR’S GEOMETRIC CONSTRAINS: The following figures shows the sketch’s construction method plus geometric and dimensional constraints suggested by the author to help you learn how to construct and constrain sketches. It is only the suggested method and if you can complete a fully constrained sketch using a different construction method and constraints, that is what is important. You may want to compare your construction method and constraints with the authors.
    AUTHOR’S COMMENTS: Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.
    Base-Skitch.jpg
    Base Sketch

    Lab Exercise 14-2

    Time allowed: 60 minutes.

    Part Name Project Units Template Color Material
    Inventor Lab Lab 14-2 Inventor Course Inches English-Modules Part (in).ipt Zinc N/A

    Step 1

    Project the Center Point onto the Base plane.

    Step 2

    Note the location of X0Y0Z0. Draw the Base sketch and revolve it create the Base model of the object shown below. Revolve it by using a centerline. (Figure Step 2A, 2B, 2C, 2D, and 2E)

    14-2-2A-1.jpg
    Figure Step 2A
    Dimensioned Multiview Drawing
    14-2-2B-1.jpg
    Figure Step 2B
    Suggested
    Base Sketch –
    YZ Plane
    14-2-2C.jpg
    Figure Step 2C
    Detail of Keyway
    14-2-2D-1.jpg
    Figure Step 2D
    Keyway is Flat Across the Top
    14-2-2E-1.jpg
    Figure Step 2E
    Solid Model – Home View

    Step 3

    Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.

    Step 4

    Apply the colour shown above. (Figure Step 4A and 4B)

    14-2-Fig-Step-4A-e1624570032272.jpg
    Figure Step 4A
    Completed Model –
    Home View
    14-2-Fig-Step-4B-e1624570055314.jpg
    Figure Step 4B
    Completed Model
    – Rotated View

    Step 5

    Add the four small holes and the key on new sketches and extrude them.

    AUTHOR’S GEOMETRIC CONSTRAINS: The following figures shows the sketch’s construction method plus geometric and dimensional constraints suggested by the author to help you learn how to construct and constrain sketches. It is only the suggested method and if you can complete a fully constrained sketch using a different construction method and constraints, that is what is important. You may want to compare your construction method and constraints with the authors.
    AUTHOR’S COMMENTS: Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.
    Base-Sketch-1-1.jpg
    Base Sketch
    Key-Sketch.jpg
    Key Sketch

    This page titled 3.3: Module 14 Revolving is shared under a CC BY license and was authored, remixed, and/or curated by Wally Baumback (BC Campus) .

    • Was this article helpful?