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3.1: Module 12 Circles

  • Page ID
    19876
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    12

    Module 12 Circles

    Wally Baumback

    Learning Outcomes

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

    1. Describe construction objects and their use in a 2D sketch.
    2. Describe drawing circles and offsets in a 2D sketch.
    3. Apply the CENTER POINT CIRCLE and OFFSET commands to complete 2D sketches.

    Geometry Lesson: Circles

    A circle is defined as a closed curve in which all points are the same distance from its centre point. The centre point is a single XY coordinate. A circle is 360 degrees and can be divided into four quadrants. All points on a circle are at a given distance from is centre point. The distance between any of the points and the centre is called the radius.

    Study the drawings in Figure 12-1, 12-2, 12-3, and 12-4 for a description of the geometry of a circle.

    12-1-2.jpg
    Figure 12-1
    Geometry of a Circle – Part 1 [Click to see image full size]
    12-2-2.jpg
    Figure 12-2
    Geometry of a Circle – Part 2 [Click to see image full size]
    12-3-3.jpg
    Figure 12-3
    Geometry of a Circle – Part 3 [Click to see image full size]
    12-4-3.jpg
    Figure 12-4
    Geometry of a Circle – Part 4

    Drafting Lesson: Reading Dimensions for Circles and Arcs

    When reading the dimensions for circles and arcs, consider the following: Circles are dimensioned as diameters. For example: 2.0 DIA.

    Arcs are dimensioned as radii. For example: 1.5 R

    When there is more than one circle of the same diameter, they are only dimensioned once. For example: 0.5 DIA., 4 PLACES

    Sometimes multiple arcs are dimensioned as typical (TYP.). For example: 2.0 R TYP. This simply means that there is at least one additional arc of the same size, See Figure 12-5.

    12-5-3.jpg
    Figure 12-5
    Typical Drawing

    Inventor Command: CENTER POINT CIRCLE

    The CENTER POINT CIRCLE command is used to draw a circle by entering the location of its centre point and its radius.

    Shortcut: C

    centre-pt-circle-1.jpg

    Inventor Command: OFFSET

    The OFFSET command is used to draw an object parallel to an existing object.

    Shortcut: O

    offset-1.jpg

    Construction objects are objects that are drawn in the sketch to assist you to complete the sketch but will be ignored by Inventor when the sketch is extruded or revolved to create the Base model. Geometrical and dimensional constraints can be applied to construction objects the same as they are to drawing objects. Construction objects and drawing objects only differ in the properties of the objects. They are both drawn and manipulated the same way in a 2D sketch.

    There are two methods of creating construction objects as follows:

    Method 1

    Enable the Construction icon, see Figure 12-6, and then draw the objects. All objects drawn while the Construction icon is enabled, will be created as construction objects.

    12-6-3.jpg
    Figure 12-6

    Method 2

    Draw the object with the Construction icon disabled. After the drawing object(s) is created, select it. While it is selected, click the Construction icon. Construction objects will appear as a dashed lines as shown in Figure 12-7.

    12-7-3.jpg
    Figure 12-7
    Construction Objects

    Geometrical-Constraints-2.jpg

    snap-symbols-6.jpg

    USER TIP: Some commands require you to select one or more drawing objects when there is no command active. For example, the DELETE command. The Status bar will display Ready when there is no command active. To select one object at a time, select the object by clicking it with the left mouse button. The selected object will highlight and change colour. To select more then one object at time, hold down either the CTRL or SHIFT key while selecting the objects. When all objects have been selected, click the command icon or enter the command on the command line.

    WORK ALONG: Drawing Circles and Cylindrical Models

    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 12-1. (Figure Step 3A and 3B)

    work-along-3a-2.jpg
    Figure Step 3A
    3D Model
    Home View [Click to see image full size]
    work-along-3b-2.jpg
    Figure Step 3B
    Dimensioned Multiview Drawing [Click to see image full size]

    Step 4

    Draw the Base sketch on the Top view. Since this is the XY plane (the default plane), use Sketch1.

    Step 5

    Project the Center Point onto the sketching plane.

    Step 6

    Enter the CENTER POINT CIRCLE command and draw a 4.0 inch diameter circle. Watch the Status bar. The first prompt will be to select the centre point for the circle. For the centre point location, snap to the Center Point that was projected onto the sketching plane. Select the radius by guessing 2 inches from the centre. (Figure Step 6)

    Fig-Step-6-3.jpg
    Figure Step 6
    AUTHOR’S COMMENTS: You can guess at the location of the radius since you will be constraining its size with a dimension later. Ensure that the green dot appears when you snap to the Center Point.

    Step 7

    Click the OFFSET command and when prompted, select the circle. Right-click the mouse. In the Right-click menu, ensure that Loop Select is enabled. Move the mouse towards the centre, guess at the diameter size of the 1.0 inch. (Figure Step 7A, 7B, and 7C)

    Fig-7A-1.jpg
    Figure Step 7A
    Fig-7B-1.jpg
    Figure Step 7B
    Fig-7C-1.jpg
    Figure Step 7C [Click to see image full size]
    AUTHOR’S COMMENTS: Using the OFFSET command to draw the two additional circles will automatically constrain their centre to the centre of the offset circle.

    Step 8

    Click the Construction icon to enable it. (Figure Step 8)

    Fig-Step-8-7.jpg
    Figure Step 8

    Step 9

    Using what you just learned, enter the OFFSET command and offset the large circle to draw the 3 inch diameter construction circle. (Figure Step 9)

    Fig-Step-9-7.jpg
    Figure Step 9
    AUTHOR’S COMMENTS: By inserting a construction circle, it will not be part of the extrusion later. Guess at the radius as you will be constraining its size with a dimension later.

    Step 10

    Click the Tools menu. Click the Applications Options icon to open the Applications Options dialogue box. Enable the Sketch tab. In the Display area, disable Axes. Click OK to close the dialogue box. (Figure Step 10A and 10B)

    Fig-Step-10A-3.jpg
    Figure Step 10A
    Fig-Step-10B-3.jpg
    Figure Step 10B [Click to see image full size]
    AUTHOR’S COMMENTS: I am having you disable the display of the axes as they get in the way of drawing this sketch. If you wish, you can leave them disabled or enable their display after you complete this workalong.

    Step 11

    Dimension the three circles. Press F8 to display the geometrical constraint icons. (Figure Step 11)

    Fig-Step-11-7.jpg
    Figure Step 11 [Click to see image full size]
    AUTHOR’S COMMENTS: Your sketch should be fully constrained.

    Step 12

    Using the LINE command, draw a line by first snapping to the Center Point and ending it by snapping onto the circle. Make sure that the Horizontal constraint icon displays when you are drawing the line. The constraint icons should appear similar to the figure. (Figure Step 12)

    Fig-Step-12-5.jpg
    Figure Step 12 [Click to see image full size]
    AUTHOR’S COMMENTS: Since the Construction Line icon is enabled from Step 8, this will be a construction line. In other words, used to construct and constrain the sketch but not included in the extruded.
    AUTHOR’S COMMENTS: Ensure that you snap to the Center Point and onto the circle circumference for the other end.

    Step 13

    Using the LINE command, draw three additional construction lines by first snapping to the Center Point and ending them by snapping onto the circle. The constraint icons should appear similar to the figure. (Figure Step 13)

    Fig-Step-13-7.jpg
    Figure Step 13
    AUTHOR’S COMMENTS: Your sketch should be fully constrained.

    Step 14

    Press F8 to display the constraint icons. (Figure Step 14)

    Fig-Step-14-4.jpg
    Figure Step 14

    Step 15

    Click the Construction icon to disable it.

    Step 16

    Enter the CENTER POINT CIRCLE command. With the cursor in the sketching window, right-click the mouse. In the Right-click menu, select Intersection. Select the construction circle and then the construction line. Notice how the cursor will display a plus sign beside it. When you select the line, the green snap indicator will display. Select a location for the radius of the circle by guessing at its size. (Figure Step 16A, 16B, 16C, and 16D)

    Fig-Step-16A-4.jpg
    Figure Step 16A
    Fig-Step-16B-4.jpg
    Figure Step 16B [Click to see image full size]
    Fig-Step-16C-1.jpg
    Figure Step 16C [Click to see image full size]
    Fig-Step-16D-1.jpg
    Figure Step 16D [Click to see image full size]

    Step 17

    Using what you just learned in Step 14, insert the 3 additional circles. For now, the diameter of the circles is not important. (Figure Step 17)

    Fig-Step-17-4.jpg
    Figure Step 17 [Click to see image full size]
    AUTHOR’S COMMENTS: Ensure that you snap to the intersection of the construction circle and the construction line when you locate the centre for each circle.

    Step 18

    Dimension one circle only. (Figure Step 18)

    Fig-Step-18-3.jpg
    Figure Step 18 [Click to see image full size]

    Step 19

    Ensure that there is no active command and select the Equal constrain icon. (Figure Step 19)

    Fig-Step-19-4.jpg
    Figure Step 19

    Step 20

    For the first circle, select the top (dimensioned circle) and for the second circle select one of the other circles. It will constrain the second circle as equal in size to the dimensioned circle. (Figure Step 20A and 20B)

    Fig-Step-20A-1.jpg
    Figure Step 20A [Click to see image full size]
    Fig-Step-20B-1.jpg
    Figure Step 20B [Click to see image full size]

    Step 21

    Using what you learned in Step 20, constrain the additional 2 circles with the Equal constraint to equal the dimensioned circle. The constraint icons should appear similar to the figure. (Figure Step 21)

    Fig-Step-21-4.jpg
    Figure Step 21 [Click to see image full size]

    Step 22

    Change the view to the Home view. The sketch should be fully constrained and display purple. (Figure Step 22)

    Fig-Step-22-3.jpg
    Figure Step 22 [Click to see image full size]

    Step 23

    Extrude the sketch as shown in the figure. (Figure Step 23A and 23B)

    Fig-Step-23A-1.jpg
    Figure Step 23A [Click to see image full size]
    Fig-Step-23B-1.jpg
    Figure Step 23B

    Step 24

    Start a new sketch on the top plane of the model. Using the OFFSET command, offset the outside diameter of the object to insert a 1.5 inch circle. Add the diameter dimension as shown in figure. (Figure Step 24)

    Fig-Step-24-3.jpg
    Figure Step 24
    AUTHOR’S COMMENTS: Since you used the OFFSET command to draw the circle, the centre of the circle will be automatically constrained and the sketch will be fully constrained.

    Step 25

    Extrude the sketch as shown in figure. (Figure Step 25)

    Fig-Step-25-3.jpg
    Figure Step 25 [Click to see image full size]
    AUTHOR’S COMMENTS: Notice how the Join icon is enabled. This is because you are joining onto the existing solid.

    Step 26

    Change the colour to: Chrome -Polished Black. (Figure Step 26)

    Fig-Step-26-3.jpg
    Figure Step 26

    Step 27

    Save and close the file.

    Key Principles

    Key Principles in Module 12

    1. Construction objects are objects that are drawn in the sketch to assist you in completing the sketch but will be ignored by Inventor when the sketch is extruded or revolved. Geometrical and dimensional constraints can be applied to construction objects the same as they are to drawing Construction objects and drawing objects only differ in the properties of the objects. They are both drawn and manipulated the same way in a 2D sketch.
    2. To select more then one object at time, hold down either the CTRL or SHIFT key while selecting the objects.

    Lab Exercise 12-1

    Time allowed: 45 minutes.

    Part Name Project Units Template Color Material
    Inventor Lab Lab 12-1 Inventor Course Millimeters Metric-Modules Part (mm).ipt Aluminum – Flat N/A

    Step 1

    Project the Center Point onto the Base plane.

    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)

    12-1-2A.jpg
    Figure Step 2A
    Solid Model – Home View
    12-1-2B.jpg
    Figure Step 2B
    Dimensioned Multiview Drawing [Click to see image full size]

    Step 3

    Apply the colour shown above. (Figure Step 3A and 3B)

    12-1-3A.jpg
    Figure Step 3A
    Solid Model – Home View
    12-1-3B.jpg
    Figure Step 3B
    Suggested Base Sketch –
    Front – XZ Plane

    Hint:

    The small holes do NOT go all the way through the flange.

    AUTHOR’S GEOMETRIC CONSTRAINTS: 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.

    base-sketch-1.jpg
    Base Sketch [Click to see image full size]
    sketch-2.jpg
    Sketch 2 [Click to see image full size]

    Lab Exercise 12-2

    Time allowed: 45 minutes.

    Part Name Project Units Template Color Material
    Inventor Lab Lab 12-2 Inventor Course Inches English-Modules Part (in).ipt White N/A

    Step 1

    Project the Center Point onto the base plane.

    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)

    12-2-2A.jpg
    Figure Step 2A
    Dimensioned Multiview Drawing [Click to see image full size]
    12-2-2B.jpg
    Figure Step 2B
    Suggested Base Sketch –
    Front – XZ Plane [Click to see image full size]

    Hint

    Draw the base sketch on the Front view or XZ plane.

    Step 3

    Apply the colour shown above. (Figure Step 3A and 3B)

    12-2-3A.jpg
    Figure Step 3A
    Completed Solid Model – Home View [Click to see image full size]
    12-2-3B.jpg
    Figure Step 3B
    Completed Solid Model – Bottom View [Click to see image full size]

    This page titled 3.1: Module 12 Circles is shared under a CC BY license and was authored, remixed, and/or curated by Wally Baumback (BC Campus) .

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