{"id":539,"date":"2021-05-13T22:29:21","date_gmt":"2021-05-13T22:29:21","guid":{"rendered":"https:\/\/opentextbc.ca\/autodesk\/chapter\/revolving\/"},"modified":"2021-11-05T17:26:32","modified_gmt":"2021-11-05T17:26:32","slug":"revolving","status":"publish","type":"chapter","link":"https:\/\/opentextbc.ca\/autodesk\/chapter\/revolving\/","title":{"raw":"Module 14 Revolving","rendered":"Module 14 Revolving"},"content":{"raw":"
\n

Learning Outcomes<\/p>\n\n<\/header>\n

\n\nWhen you have completed this module, you will be able to:\n
    \n \t
  1. Describe a centerline object and explain how it is inserted and used in a 2D Sketch.<\/li>\n \t
  2. Describe how a Base sketch is revolved with and without the use of a centerline to create a solid model.<\/li>\n \t
  3. Apply the REVOLVE command to create a solid model from a Base sketch.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

    Revolving<\/h1>\nWhen drawing symmetrical objects it is much easier to create the model by revolving<\/span> <\/em>the Base sketch around an axis<\/span> <\/em>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.\n\nIn this module, the basic features of the REVOLVE command are taught. The Inventor Advanced book will cover the more advanced features.\n\nThe 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.\n\n[caption id=\"attachment_1161\" align=\"aligncenter\" width=\"300\"]\"\" Figure 14-1
    A 2D Sketch Revolved Around a
    Line in the Sketch[\/caption]\n\n[caption id=\"attachment_1162\" align=\"aligncenter\" width=\"300\"]\"\" Figure 14-2
    The Same 2D Sketch Revolved
    around a Centerline[\/caption]\n\n
    \n

    Inventor Command: REVOLVE<\/p>\n\n<\/header>\n

    \n\nThe REVOLVE command is used to create a solid model by revolving the Base sketch around an axis.\n\nShortcut: R<\/strong>\n\n\"\"\n\n<\/div>\n<\/div>\n

    Centerlines<\/h1>\nA centerline<\/span> <\/em>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:\n

    Method 1<\/h2>\nDraw the line using the LINE command and then select it. While it is selected, click the Centerline icon.\n

    Method 2<\/h2>\nEnable 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.\n\n[caption id=\"attachment_1164\" align=\"aligncenter\" width=\"298\"]\"\" Figure 14-3
    Centerline Icon[\/caption]\n

    WORK ALONG: Revolving a Sketch Without using a Centerline<\/h1>\n

    Step 1<\/h2>\nCheck the default project and if necessary, set it to Inventor Course.\n

    Step 2<\/h2>\nUsing the NEW command, start a new part file using the template: English-Modules Part (in).ipt<\/span>.\n

    Step 3<\/h2>\nSave the file with the name: Inventor Workalong 14-1<\/span>. (Figure Step 3A and 3B)\n\n[caption id=\"attachment_1165\" align=\"aligncenter\" width=\"252\"]\"\" Figure Step 3A
    3D Model[\/caption]\n\n[caption id=\"attachment_1195\" align=\"aligncenter\" width=\"500\" class=\"page-break-after\"]\"\"<\/a> Figure Step 3B
    Dimensioned Multiview Drawing [Click to see image full size][\/caption]\n
    AUTHOR'S COMMENTS: <\/strong>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.\n<\/strong><\/div>\n

    Step 4<\/h2>\nStart a new sketch on the Front or XZ Plane. Project the Center Point onto the sketch.\n

    Step 5<\/h2>\nDraw and dimension one-half of the Front view as shown in the figure. Ensure that the sketch is fully constrained (Figure Step 5)\n\n[caption id=\"attachment_1167\" align=\"aligncenter\" width=\"335\"]\"\" Figure Step 5[\/caption]\n\n
    AUTHOR'S COMMENTS: <\/strong>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.<\/div>\n
    AUTHOR'S COMMENTS: <\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Ensure that the sketch is fully constrained.\n<\/strong><\/div>\n

    Step 6<\/h2>\nIn Model mode, enter the REVOLVE command. It will highlight the sketch automatically as the area to revolve. (Figure Step 6)\n\n[caption id=\"attachment_1168\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 6 [Click to see image full size][\/caption]\n

    Step 7<\/h2>\nIn 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)\n\n[caption id=\"attachment_1169\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 7 [Click to see image full size][\/caption]\n

    Step 8<\/h2>\nAfter 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)\n\n[caption id=\"attachment_1170\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 8A [Click to see image full size][\/caption]\n\n[caption id=\"attachment_1171\" align=\"aligncenter\" width=\"264\"]\"\" Figure Step 8B[\/caption]\n

    Step 9<\/h2>\nStart a new sketch on the top plane of the model. (Figure Step 9)\n\n[caption id=\"attachment_1172\" align=\"aligncenter\" width=\"446\"]\"\" Figure Step 9[\/caption]\n

    Step 10<\/h2>\nUsing 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)\n\n[caption id=\"attachment_1173\" align=\"aligncenter\" width=\"421\"]\"\" Figure Step 10[\/caption]\n\n
    AUTHOR'S COMMENTS:<\/strong>\u00a0Ensure 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.\n<\/strong><\/div>\n

    Step 11<\/h2>\nUsing 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)\n\n[caption id=\"attachment_1174\" align=\"aligncenter\" width=\"486\"]\"\" Figure Step 11A[\/caption]\n\n[caption id=\"attachment_1175\" align=\"aligncenter\" width=\"503\"]\"\" Figure Step 11B[\/caption]\n\n
    AUTHOR'S COMMENTS: <\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Ensure that your sketch is fully constrained.\n<\/strong><\/div>\n

    Step 12<\/h2>\nExtrude the four circles to the To Next extents. (Figure Step 12)\n\n[caption id=\"attachment_1176\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 12 [Click to see image full size][\/caption]\n

    Step 13<\/h2>\nStart 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)\n\n[caption id=\"attachment_1177\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 13 [Click to see image full size][\/caption]\n
    AUTHOR'S COMMENTS: <\/strong>Using an offset, will automatically constrain the circle.\n<\/strong><\/div>\n

    Step 14<\/h2>\nChange the colour to: Aluminum - Polished. (Figure Step 14)\n\n[caption id=\"attachment_1178\" align=\"aligncenter\" width=\"288\"]\"\" Figure Step 14[\/caption]\n

    Step 15<\/h2>\nSave and close the file.\n

    WORK ALONG: Revolving a Sketch using a Centerline<\/h1>\n

    Step 1<\/h2>\nCheck the default project and if necessary, set it to Inventor Course.\n

    Step 2<\/h2>\nEnter the NEW command to start a new part file using the template: English-Modules Part (in).ipt<\/span>.\n

    Step 3<\/h2>\nSave the file with the name: Inventor Workalong 14-2<\/span>. (Figure Step 3)\n\n[caption id=\"attachment_1183\" align=\"aligncenter\" width=\"437\"]\"\" Figure Step 3
    Dimensioned Multiview Drawing[\/caption]\n

    Step 4<\/h2>\nStart 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\u2019s properties to a centerline. (Figure Step 4A and 4B)\n\n[caption id=\"attachment_1184\" align=\"aligncenter\" width=\"248\"]\"\" Figure Step 4A[\/caption]\n\n[caption id=\"attachment_1185\" align=\"aligncenter\" width=\"409\"]\"\" Figure Step 4B[\/caption]\n

    Step 5<\/h2>\nDraw and dimension one-half of the Front view as shown in the figure. (Figure Step 5A and 5B)\n\n[caption id=\"attachment_1186\" align=\"aligncenter\" width=\"300\"]\"\"<\/a> Figure Step 5A [Click to see image full size][\/caption][caption id=\"attachment_1188\" align=\"aligncenter\" width=\"300\"]\"\"<\/a> Figure Step 5B [Click to see image full size][\/caption]\n
    AUTHOR'S COMMENTS: <\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.<\/div>\n

    Step 6<\/h2>\nReturn 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)\n\n[caption id=\"attachment_1189\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 6 [Click to see image full size][\/caption]\n

    Step 7<\/h2>\nIn a new sketch, add the four smaller circles and extrude them to complete the model.\n

    Step 8<\/h2>\nChange the colour to: Aluminum - Polished<\/span>. (Figure Step 8)\n\n[caption id=\"attachment_1190\" align=\"aligncenter\" width=\"288\"]\"\" Figure Step 8[\/caption]\n

    Step 9<\/h2>\nSave and close the file.\n

    Drafting Lesson: Cross Sections<\/h1>\nWhen 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\n\n[caption id=\"attachment_1191\" align=\"aligncenter\" width=\"224\"]\"\" Figure 32-1
    Normal Front and Right Side View of an Object[\/caption]\n\nA cross section<\/span> <\/em>view, also called a section<\/em><\/span>, 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.\n\n \n\n[caption id=\"attachment_1197\" align=\"aligncenter\" width=\"336\"]\"\" Figure 32-2
    A Front view and Right
    Side Section View[\/caption]\n\n[caption id=\"attachment_1198\" align=\"aligncenter\" width=\"240\"]\"\" Figure 32-3
    3D Model of the Object
    Showing it Cut on the
    Cutting Plane Line[\/caption]\n\nA cutting plane<\/span> <\/em>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.\n

    Key Principles<\/h1>\n
    \n

    Key Principles in Module 14<\/p>\n\n<\/header>\n

    \n
      \n \t
    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.<\/li>\n \t
    2. A centerline is a line with its properties set to act as a centerline.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

      Lab Exercise 14-1<\/h1>\nTime allowed: 60 minutes.\n\n\n\n\n
      Part Name<\/strong><\/td>\nProject<\/strong><\/td>\nUnits<\/strong><\/td>\nTemplate<\/strong><\/td>\nColor<\/strong><\/td>\nMaterial<\/strong><\/td>\n<\/tr>\n
      Inventor Lab Lab 14-1<\/td>\nInventor Course<\/td>\nMillimeters<\/td>\nMetric-Modules Part (mm).ipt<\/td>\nCopper - Polished<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

      Step 1<\/h2>\nProject the Center Point onto the Base plane.\n

      Step 2<\/h2>\nNote 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)\n\n[caption id=\"attachment_1200\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 2A
      Dimensioned Multiview Drawing[\/caption]\n\n[caption id=\"attachment_1201\" align=\"aligncenter\" width=\"162\"]\"\" Figure Step 2B
      Suggested Base
      Sketch - Right Side -
      YZ Plane[\/caption]\n

      Step 3<\/h2>\nApply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.\n

      Step 4<\/h2>\nApply the colour shown above. (Figure Step 4A and 4B)\n\n[caption id=\"attachment_1207\" align=\"aligncenter\" width=\"292\"]\"\" Figure Step 4A
      Completed Solid Model
      - Home View[\/caption]\n\n[caption id=\"attachment_1208\" align=\"aligncenter\" width=\"314\"]\"\" Figure Step 4B
      Completed Model
      - Rear View[\/caption]\n

      Step 5<\/h2>\nAdd the four small holes on a new sketch and extrude them.\n
      AUTHOR'S GEOMETRIC CONSTRAINS: <\/strong>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.<\/div>\n
      AUTHOR'S COMMENTS:\u00a0<\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.<\/div>\n\n[caption id=\"attachment_1220\" align=\"aligncenter\" width=\"500\"]\"\" Base Sketch[\/caption]\n

      Lab Exercise 14-2<\/h1>\nTime allowed: 60 minutes.\n\n\n\n\n
      Part Name<\/strong><\/td>\nProject<\/strong><\/td>\nUnits<\/strong><\/td>\nTemplate<\/strong><\/td>\nColor<\/strong><\/td>\nMaterial<\/strong><\/td>\n<\/tr>\n
      Inventor Lab Lab 14-2<\/td>\nInventor Course<\/td>\nInches<\/td>\nEnglish-Modules Part (in).ipt<\/td>\nZinc<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

      Step 1<\/h2>\nProject the Center Point onto the Base plane.\n

      Step 2<\/h2>\nNote 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)\n\n[caption id=\"attachment_1211\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 2A
      Dimensioned Multiview Drawing[\/caption]\n\n[caption id=\"attachment_1212\" align=\"aligncenter\" width=\"162\"]\"\" Figure Step 2B
      Suggested
      Base Sketch -
      YZ Plane[\/caption]\n\n[caption id=\"attachment_1213\" align=\"aligncenter\" width=\"458\"]\"\" Figure Step 2C
      Detail of Keyway[\/caption]\n\n[caption id=\"attachment_1214\" align=\"aligncenter\" width=\"443\"]\"\" Figure Step 2D
      Keyway is Flat Across the Top[\/caption]\n\n[caption id=\"attachment_1215\" align=\"aligncenter\" width=\"256\"]\"\" Figure Step 2E
      Solid Model - Home View[\/caption]\n\n \n

      Step 3<\/h2>\nApply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.\n

      Step 4<\/h2>\nApply the colour shown above. (Figure Step 4A and 4B)\n\n[caption id=\"attachment_1216\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 4A
      Completed Model -
      Home View[\/caption]\n\n[caption id=\"attachment_1217\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 4B
      Completed Model
      - Rotated View[\/caption]\n

      Step 5<\/h2>\nAdd the four small holes and the key on new sketches and extrude them.\n
      AUTHOR'S GEOMETRIC CONSTRAINS: <\/strong>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.<\/div>\n
      AUTHOR'S COMMENTS:\u00a0<\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.<\/div>\n\n[caption id=\"attachment_1219\" align=\"aligncenter\" width=\"462\"]\"\" Base Sketch[\/caption]\n\n[caption id=\"attachment_1221\" align=\"aligncenter\" width=\"474\"]\"\" Key Sketch[\/caption]","rendered":"
      \n
      \n

      Learning Outcomes<\/p>\n<\/header>\n

      \n

      When you have completed this module, you will be able to:<\/p>\n

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

        Revolving<\/h1>\n

        When drawing symmetrical objects it is much easier to create the model by revolving<\/span> <\/em>the Base sketch around an axis<\/span> <\/em>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.<\/p>\n

        In this module, the basic features of the REVOLVE command are taught. The Inventor Advanced book will cover the more advanced features.<\/p>\n

        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.<\/p>\n

        \"\"
        Figure 14-1
        A 2D Sketch Revolved Around a
        Line in the Sketch<\/figcaption><\/figure>\n
        \"\"
        Figure 14-2
        The Same 2D Sketch Revolved
        around a Centerline<\/figcaption><\/figure>\n
        \n
        \n

        Inventor Command: REVOLVE<\/p>\n<\/header>\n

        \n

        The REVOLVE command is used to create a solid model by revolving the Base sketch around an axis.<\/p>\n

        Shortcut: R<\/strong><\/p>\n

        \"\"<\/p>\n<\/div>\n<\/div>\n

        Centerlines<\/h1>\n

        A centerline<\/span> <\/em>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:<\/p>\n

        Method 1<\/h2>\n

        Draw the line using the LINE command and then select it. While it is selected, click the Centerline icon.<\/p>\n

        Method 2<\/h2>\n

        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.<\/p>\n

        \"\"
        Figure 14-3
        Centerline Icon<\/figcaption><\/figure>\n

        WORK ALONG: Revolving a Sketch Without using a Centerline<\/h1>\n

        Step 1<\/h2>\n

        Check the default project and if necessary, set it to Inventor Course.<\/p>\n

        Step 2<\/h2>\n

        Using the NEW command, start a new part file using the template: English-Modules Part (in).ipt<\/span>.<\/p>\n

        Step 3<\/h2>\n

        Save the file with the name: Inventor Workalong 14-1<\/span>. (Figure Step 3A and 3B)<\/p>\n

        \"\"
        Figure Step 3A
        3D Model<\/figcaption><\/figure>\n
        \"\"<\/a>
        Figure Step 3B
        Dimensioned Multiview Drawing [Click to see image full size]<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong>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.
        \n<\/strong><\/div>\n

        Step 4<\/h2>\n

        Start a new sketch on the Front or XZ Plane. Project the Center Point onto the sketch.<\/p>\n

        Step 5<\/h2>\n

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

        \"\"
        Figure Step 5<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong>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.<\/div>\n
        AUTHOR’S COMMENTS: <\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Ensure that the sketch is fully constrained.
        \n<\/strong><\/div>\n

        Step 6<\/h2>\n

        In Model mode, enter the REVOLVE command. It will highlight the sketch automatically as the area to revolve. (Figure Step 6)<\/p>\n

        \"\"<\/a>
        Figure Step 6 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 7<\/h2>\n

        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)<\/p>\n

        \"\"<\/a>
        Figure Step 7 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 8<\/h2>\n

        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)<\/p>\n

        \"\"<\/a>
        Figure Step 8A [Click to see image full size]<\/figcaption><\/figure>\n
        \"\"
        Figure Step 8B<\/figcaption><\/figure>\n

        Step 9<\/h2>\n

        Start a new sketch on the top plane of the model. (Figure Step 9)<\/p>\n

        \"\"
        Figure Step 9<\/figcaption><\/figure>\n

        Step 10<\/h2>\n

        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)<\/p>\n

        \"\"
        Figure Step 10<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:<\/strong>\u00a0Ensure 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.
        \n<\/strong><\/div>\n

        Step 11<\/h2>\n

        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)<\/p>\n

        \"\"
        Figure Step 11A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 11B<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Ensure that your sketch is fully constrained.
        \n<\/strong><\/div>\n

        Step 12<\/h2>\n

        Extrude the four circles to the To Next extents. (Figure Step 12)<\/p>\n

        \"\"<\/a>
        Figure Step 12 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 13<\/h2>\n

        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)<\/p>\n

        \"\"<\/a>
        Figure Step 13 [Click to see image full size]<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong>Using an offset, will automatically constrain the circle.
        \n<\/strong><\/div>\n

        Step 14<\/h2>\n

        Change the colour to: Aluminum – Polished. (Figure Step 14)<\/p>\n

        \"\"
        Figure Step 14<\/figcaption><\/figure>\n

        Step 15<\/h2>\n

        Save and close the file.<\/p>\n

        WORK ALONG: Revolving a Sketch using a Centerline<\/h1>\n

        Step 1<\/h2>\n

        Check the default project and if necessary, set it to Inventor Course.<\/p>\n

        Step 2<\/h2>\n

        Enter the NEW command to start a new part file using the template: English-Modules Part (in).ipt<\/span>.<\/p>\n

        Step 3<\/h2>\n

        Save the file with the name: Inventor Workalong 14-2<\/span>. (Figure Step 3)<\/p>\n

        \"\"
        Figure Step 3
        Dimensioned Multiview Drawing<\/figcaption><\/figure>\n

        Step 4<\/h2>\n

        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\u2019s properties to a centerline. (Figure Step 4A and 4B)<\/p>\n

        \"\"
        Figure Step 4A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 4B<\/figcaption><\/figure>\n

        Step 5<\/h2>\n

        Draw and dimension one-half of the Front view as shown in the figure. (Figure Step 5A and 5B)<\/p>\n

        \"\"<\/a>
        Figure Step 5A [Click to see image full size]<\/figcaption><\/figure>\n
        \"\"<\/a>
        Figure Step 5B [Click to see image full size]<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.<\/div>\n

        Step 6<\/h2>\n

        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)<\/p>\n

        \"\"<\/a>
        Figure Step 6 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 7<\/h2>\n

        In a new sketch, add the four smaller circles and extrude them to complete the model.<\/p>\n

        Step 8<\/h2>\n

        Change the colour to: Aluminum – Polished<\/span>. (Figure Step 8)<\/p>\n

        \"\"
        Figure Step 8<\/figcaption><\/figure>\n

        Step 9<\/h2>\n

        Save and close the file.<\/p>\n

        Drafting Lesson: Cross Sections<\/h1>\n

        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<\/p>\n

        \"\"
        Figure 32-1
        Normal Front and Right Side View of an Object<\/figcaption><\/figure>\n

        A cross section<\/span> <\/em>view, also called a section<\/em><\/span>, 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.<\/p>\n

         <\/p>\n

        \"\"
        Figure 32-2
        A Front view and Right
        Side Section View<\/figcaption><\/figure>\n
        \"\"
        Figure 32-3
        3D Model of the Object
        Showing it Cut on the
        Cutting Plane Line<\/figcaption><\/figure>\n

        A cutting plane<\/span> <\/em>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.<\/p>\n

        Key Principles<\/h1>\n
        \n
        \n

        Key Principles in Module 14<\/p>\n<\/header>\n

        \n
          \n
        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.<\/li>\n
        2. A centerline is a line with its properties set to act as a centerline.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

          Lab Exercise 14-1<\/h1>\n

          Time allowed: 60 minutes.<\/p>\n\n\n\n\n
          Part Name<\/strong><\/td>\nProject<\/strong><\/td>\nUnits<\/strong><\/td>\nTemplate<\/strong><\/td>\nColor<\/strong><\/td>\nMaterial<\/strong><\/td>\n<\/tr>\n
          Inventor Lab Lab 14-1<\/td>\nInventor Course<\/td>\nMillimeters<\/td>\nMetric-Modules Part (mm).ipt<\/td>\nCopper – Polished<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

          Project the Center Point onto the Base plane.<\/p>\n

          Step 2<\/h2>\n

          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)<\/p>\n

          \"\"
          Figure Step 2A
          Dimensioned Multiview Drawing<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2B
          Suggested Base
          Sketch – Right Side –
          YZ Plane<\/figcaption><\/figure>\n

          Step 3<\/h2>\n

          Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.<\/p>\n

          Step 4<\/h2>\n

          Apply the colour shown above. (Figure Step 4A and 4B)<\/p>\n

          \"\"
          Figure Step 4A
          Completed Solid Model
          – Home View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 4B
          Completed Model
          – Rear View<\/figcaption><\/figure>\n

          Step 5<\/h2>\n

          Add the four small holes on a new sketch and extrude them.<\/p>\n

          AUTHOR’S GEOMETRIC CONSTRAINS: <\/strong>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.<\/div>\n
          AUTHOR’S COMMENTS:\u00a0<\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.<\/div>\n
          \"\"
          Base Sketch<\/figcaption><\/figure>\n

          Lab Exercise 14-2<\/h1>\n

          Time allowed: 60 minutes.<\/p>\n\n\n\n\n
          Part Name<\/strong><\/td>\nProject<\/strong><\/td>\nUnits<\/strong><\/td>\nTemplate<\/strong><\/td>\nColor<\/strong><\/td>\nMaterial<\/strong><\/td>\n<\/tr>\n
          Inventor Lab Lab 14-2<\/td>\nInventor Course<\/td>\nInches<\/td>\nEnglish-Modules Part (in).ipt<\/td>\nZinc<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

          Project the Center Point onto the Base plane.<\/p>\n

          Step 2<\/h2>\n

          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)<\/p>\n

          \"\"
          Figure Step 2A
          Dimensioned Multiview Drawing<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2B
          Suggested
          Base Sketch –
          YZ Plane<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2C
          Detail of Keyway<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2D
          Keyway is Flat Across the Top<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2E
          Solid Model – Home View<\/figcaption><\/figure>\n

           <\/p>\n

          Step 3<\/h2>\n

          Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.<\/p>\n

          Step 4<\/h2>\n

          Apply the colour shown above. (Figure Step 4A and 4B)<\/p>\n

          \"\"
          Figure Step 4A
          Completed Model –
          Home View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 4B
          Completed Model
          – Rotated View<\/figcaption><\/figure>\n

          Step 5<\/h2>\n

          Add the four small holes and the key on new sketches and extrude them.<\/p>\n

          AUTHOR’S GEOMETRIC CONSTRAINS: <\/strong>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.<\/div>\n
          AUTHOR’S COMMENTS:\u00a0<\/strong>Your geometrical and dimensional constrains may not match the figure exactly. Just ensure that your sketch is fully constrained.<\/div>\n
          \"\"
          Base Sketch<\/figcaption><\/figure>\n
          \"\"
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