{"id":255,"date":"2021-05-14T20:46:11","date_gmt":"2021-05-15T00:46:11","guid":{"rendered":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/?post_type=chapter&p=255"},"modified":"2021-07-13T14:36:53","modified_gmt":"2021-07-13T18:36:53","slug":"work-features","status":"publish","type":"chapter","link":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/chapter\/work-features\/","title":{"raw":"Module 19 Work Features","rendered":"Module 19 Work Features"},"content":{"raw":"
\r\n

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

\r\n\r\nWhen you have completed this module, you will be able to:\r\n
    \r\n \t
  1. Describe and apply the POLYGON, TANGENT CIRCLE, and THREAD commands.<\/li>\r\n \t
  2. Describe work features including Work Points, Work Axes, and Work Planes and explain how they are used in model construction.<\/li>\r\n \t
  3. Describe and apply the WORK POINT, WORK AXIS, and WORK PLANE commands.<\/li>\r\n<\/ol>\r\n<\/div>\r\n<\/div>\r\n

    Geometry Lesson: Regular Polygons<\/h1>\r\nA polygon<\/span> <\/em>is defined as any plane figure bounded by straight lines. A regular polygon<\/span> <\/em>is a polygon that has equal angles, equal sides and can be inscribed in or circumscribed around a circle. The first eight regular polygons are shown in Figure 19-1.\r\n\r\n[caption id=\"attachment_1434\" align=\"aligncenter\" width=\"500\"]\"\" Figure 19-1
    Regular Polygons
    Work[\/caption]\r\n\r\nAny regular polygon can be inscribed in or circumscribed around a circle as shown, using a hexagon, in Figure 19-2.\r\n\r\n[caption id=\"attachment_1435\" align=\"aligncenter\" width=\"494\"]\"\" Figure 19-2
    Inscribed and Circumscribed Regular Polygon[\/caption]\r\n\r\nIt is important to understand and know the geometry involved to construct a triangle, square, hexagon, and octagon as shown in Figure 19-3. Study each one and try to understand how they are constructed and the angles used to construct them.\r\n\r\n[caption id=\"attachment_1436\" align=\"aligncenter\" width=\"615\"]\"\" Figure 19-3
    Geometry of Four Regular Polygons[\/caption]\r\n\r\n
    \r\n

    Inventor Command:\u00a0POLYGON<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe POLYGON command is used to draw a regular polygon on a 2D sketch. You can select the number of sides and choose between either an inscribed or a circumscribed polygon.\r\n\r\nShortcut: none<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n
    \r\n

    Inventor Command:\u00a0TANGENT CIRCLE<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe TANGENT CIRCLE command is used to draw a circle tangent to three lines.\r\n\r\nShortcut: none<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n
    \r\n

    Inventor Command: AUTO DIMENSION<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe AUTO DIMENSION command is used to add dimensions or constrains automatically to fully constrain a sketch.\r\n\r\nShortcut: none<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n

    Drawing Threads<\/h2>\r\nThe THREAD command is used to draw exterior threads or interior threads on a 3D solid model. See Figure 19-4 The threads created using the THREAD command are not actual threads constructed on the model. They are simply a graphical representation of the threads. A real life solid model created from the Inventor part would not be threaded. Actual threads can be created but this is a much more advanced feature that is taught in the Inventor Advanced book. The thread specifications can be applied to the thread in the sketch and then be used when creating the working drawing of the part.\r\n\r\n[caption id=\"attachment_1442\" align=\"aligncenter\" width=\"400\"]\"\" Figure 19-4
    External and Internal Threads[\/caption]\r\n\r\n
    \r\n

    Inventor Command: THREAD<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe THREAD command is used to draw a graphical representation of an outside or inside diameter thread. The thread specifications can also added to the thread properties.\r\n\r\nShortcut: none<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n

    WORK ALONG: Drawing Polygons and Threads - Part 1<\/h1>\r\n

    Step 1<\/h2>\r\nUsing the NEW command start a new part file using the template: English-Modules Part (in).ipt<\/span>.\r\n

    Step 2<\/h2>\r\nSave the file with the name: Inventor Workalong 19-1<\/span>. (Figure Step 2A, 2B, and 2C)\r\n\r\n[caption id=\"attachment_1444\" align=\"aligncenter\" width=\"189\"]\"\" Figure Step 2A
    3D Model -
    Home View[\/caption]\r\n\r\n[caption id=\"attachment_1445\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 2B
    Dimensioned Multiview Drawing[\/caption]\r\n\r\n[caption id=\"attachment_1446\" align=\"aligncenter\" width=\"452\"]\"\" Figure Step 2C
    Detail[\/caption]\r\n

    Step 3<\/h2>\r\nDraw the Base sketch on the Top or XY plane.\r\n

    Step 4<\/h2>\r\nProject the Center Point onto the Base sketch.\r\n

    Step 5<\/h2>\r\nEnter the POLYGON command and set the number of sides to 6. (Figure Step 5)\r\n\r\n[caption id=\"attachment_1447\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 5[\/caption]\r\n

    Step 6<\/h2>\r\nEnable the Circumscribed Polygon icon. Snap to the Center Point for the centre and select a radius of approximately 0.75 inches. (Figure Step 6)\r\n\r\n[caption id=\"attachment_1448\" align=\"aligncenter\" width=\"29\"]\"\" Fig Step 6[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>A circumscribed polygon is used in this sketch because the edge to edge dimension was given rather then corner to corner.<\/div>\r\n

    Step 7<\/h2>\r\nAdd the dimension from the Center Point to the left line. (Figure Step 7)\r\n\r\n[caption id=\"attachment_1449\" align=\"aligncenter\" width=\"293\"]\"\" Figure Step 7[\/caption]\r\n

    Step 8<\/h2>\r\nEnter the AUTO DIMENSION command. Note that one dimension or constraint is required to fully constrain the sketch. Click Apply. (Figure Step 8A, 8B, and 8C\r\n\r\n[caption id=\"attachment_1450\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 8A[\/caption]\r\n\r\n[caption id=\"attachment_1451\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 8B[\/caption]\r\n\r\n[caption id=\"attachment_1452\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 8C[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>This will add a constraint to fully constrain the sketch. The AUTO DIMENSION command is used to automatically add the dimensions or constraints to fully constrain it.<\/div>\r\n

    Step 9<\/h2>\r\nExtrude the hexagon in the negative Z direction. (Figure Step 9)\r\n\r\n[caption id=\"attachment_1453\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 9 [Click to see image full size][\/caption]\r\n

    Step 10<\/h2>\r\nStart a new sketch on the bottom side of the Base model. Enter the TANGENT CIRCLE command. When prompted, select any three edges. (Figure Step 10)\r\n\r\n[caption id=\"attachment_1454\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 10[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>Since you are inserting a circle tangent inside of a regular polygon, any three edges can be selected.<\/div>\r\n

    Step 11<\/h2>\r\nExtrude the circle 0.016 inches. Ensure that you enable the Join<\/span> icon and extrude it away from the bolt head. (Figure Step 11)\r\n\r\n[caption id=\"attachment_1455\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 11 [Click to see image full size][\/caption]\r\n

    Step 12<\/h2>\r\nStart a new sketch on the extruded circle. Draw and dimension a 1 inch circle using the centre of the circle to snap to. Extrude the circle 3 inches. (Figure Step 12A and 12B)\r\n\r\n[caption id=\"attachment_1456\" align=\"aligncenter\" width=\"363\"]\"\" Figure Step 12A[\/caption]\r\n\r\n[caption id=\"attachment_1457\" align=\"aligncenter\" width=\"225\"]\"\" Figure Step 12B[\/caption]\r\n

    Step 13<\/h2>\r\nUsing the CHAMFER command, chamfer the bottom of the bolt. (Figure Step 13)\r\n\r\n[caption id=\"attachment_1458\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 13 [Click to see image full size][\/caption]\r\n

    Step 14<\/h2>\r\nEnter the THREAD command. Enable the Location tab and set the Length to 1.5 and then select the cylinder as the face to thread. Do not close the dialogue box. (Figure Step 14)\r\n\r\n[caption id=\"attachment_1459\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 14 [Click to see image full size][\/caption]\r\n

    Step 15<\/h2>\r\nEnable the Specification tab. Set the thread specifications as shown in the figure. Click OK to execute the command. (Figure Step 15A and 15B)\r\n\r\n[caption id=\"attachment_1460\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 15A [Click to see image full size][\/caption]\r\n\r\n[caption id=\"attachment_1461\" align=\"aligncenter\" width=\"256\"]\"\" Figure Step 15B[\/caption]\r\n

    Step 16<\/h2>\r\nChange the view to the Home view and change the colour to: Metal-Brass<\/span>. (Figure Step 16)\r\n\r\n[caption id=\"attachment_1462\" align=\"aligncenter\" width=\"198\"]\"\" Figure Step 16[\/caption]\r\n

    Step 17<\/h2>\r\nSave and close the file.\r\n
    MUST KNOW:<\/strong> The threads created by the THREAD command are not actual threads constructed on the model. They are simply a graphical representation of the threads. A real life solid model created from the Inventor part file would not be threaded.<\/div>\r\n

    WORK ALONG: Drawing Polygons and Threads - Part 2<\/h1>\r\n

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

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

    Step 3<\/h2>\r\nSave the file with the name: Inventor Workalong 19-2<\/span>.\r\n

    Step 4<\/h2>\r\nUsing what you learned in the last workalong, construct the nut shown in the multiview drawing. (Figure Step 4A and 4B)\r\n\r\n[caption id=\"attachment_1463\" align=\"aligncenter\" width=\"408\"]\"\" Figure Step 4A
    Dimensioned Multiview Drawing[\/caption]\r\n\r\n[caption id=\"attachment_1464\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 4B 3D Model - Home View[\/caption]\r\n

    Step 5<\/h2>\r\nChange the colour to: Metal-Brass<\/span>. (Figure Step 5A and 5B)\r\n\r\n[caption id=\"attachment_1465\" align=\"aligncenter\" width=\"214\"]\"\" Figure Step 5A[\/caption]\r\n\r\n[caption id=\"attachment_1466\" align=\"aligncenter\" width=\"228\"]\"\" Figure Step 5B[\/caption]\r\n

    Work Features<\/h1>\r\nWork Features<\/em><\/span> consists of points, axes, and planes that can be inserted on a solid model or in Model space. They are used as a construction aids to draw the model. You can insert them when existing geometry cannot be used to add geometry. The three work features available in Inventor are the work point, the work axis, and the work plane. See Figure 19-5. This module is an introduction to work features only and will teach the user how to create and use them in part modeling. They are also used in assemblies.\r\n\r\n[caption id=\"attachment_1467\" align=\"aligncenter\" width=\"500\"]\"\" Figure 19-5
    Work Features[\/caption]\r\n

    Work Points<\/h2>\r\nA Work Point<\/span> <\/em>is a parametric construction point or a single XYZ location that is inserted and then used as a work feature. Once a Work Point is inserted on the model, it can be projected onto part faces, linear edges, or onto an arc or circle using the PROJECT GEOMETRY command. Work Points can also be constrained to the centre points of arcs, circles, and ellipses. In this module, inserting Work Points on the model or in 3D space will be taught.\r\n

    Work Axes<\/h2>\r\nA Work Axis<\/em><\/span> is a parametric construction line or two XYZ locations joined by a line that is inserted and then used as a work feature. Even though a Work Axis appears as a specified length, as far as Inventor is concerned, it is infinite in length and can be expanded to any length required.\r\n\r\nUse Work Axes when creating models to mark symmetry lines, centre lines, or distances between revolved feature axes. Work Axes can be used along the symmetry lines of circular features such as cylinders, shafts, or holes. They can also be created as a work axis on a linear edge, a sketch line, or a 3D sketch line.\r\n

    Work Planes<\/h2>\r\nA Work Plane<\/span><\/em> is parametric construction plane or four XYZ locations joined by lines inserted on the model or in model space and then used as a work feature. Even though a Work Plane appears as a rectangular plane of a given size, it is actually infinite in size and can be expanded to any size required.\r\n\r\nWork Planes can be placed at any orientation in space, offset from existing faces, or rotated around an axis or edge. A work plane can be used as a sketch plane and dimensioned or constrained to other features or components. Each work plane has its own internal coordinate system. The order in which geometry is selected determines the origin and positive directions of the coordinate system axes.\r\n
    \r\n

    Inventor Command: WORK POINT<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe WORK POINT command is used to insert a Work Point on the model or in Model space.\r\n\r\nShortcut:\u00a0. (period)<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n
    \r\n

    Inventor Command: WORK AXIS<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe WORK AXIS command is used to insert a Work Axis on the model or in Model space.\r\n\r\nShortcut:\u00a0\/ (forward slash)<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n
    \r\n

    Inventor Command: WORK PLANE<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe WORK PLANE command is used to insert a Work Plane on the model or in Model space.\r\n\r\nShortcut:] (right bracket)<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n

    WORK ALONG: Creating Work Features<\/h1>\r\n

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

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

    Step 3<\/h2>\r\nSave the file with the name: Inventor Workalong 19-3<\/span>.\r\n

    Step 4<\/h2>\r\nCreate the solid model shown in the figures. (Figure Step 4A and 4B)\r\n\r\n[caption id=\"attachment_1471\" align=\"aligncenter\" width=\"486\"]\"\" Figure Step 4A
    3D Model - Home View[\/caption]\r\n\r\n[caption id=\"attachment_1472\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 4B
    Dimensioned Multiview Drawing [Click to see image full size][\/caption]\r\n

    Step 5<\/h2>\r\nInsert a Work Point at the apparent intersection of two edges. Click the WORK POINT command and then Intersection of Two Lines. Select the edges shown in the figure. Note how they highlight and extend. (Figure Step 5A, 5B, and 5C)\r\n\r\n[caption id=\"attachment_1474\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 5A[\/caption]\r\n\r\n[caption id=\"attachment_1475\" align=\"aligncenter\" width=\"410\"]\"\" Figure Step 5B[\/caption]\r\n\r\n[caption id=\"attachment_1476\" align=\"aligncenter\" width=\"376\"]\"\" Figure Step 5C[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>The Work Point will be inserted at the apparent intersection of the two selected edges.<\/div>\r\n

    Step 6<\/h2>\r\nInsert a Work Point at the intersection of three planes. Click the WORK POINT command and then Intersection of Three Planes. Select the planes shown in the figures. (Figure Step 6A, 6B, 6C, 6D, and 6E)\r\n\r\n[caption id=\"attachment_1477\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 6A[\/caption]\r\n\r\n[caption id=\"attachment_1478\" align=\"aligncenter\" width=\"484\"]\"\" Figure Step 6B[\/caption]\r\n\r\n[caption id=\"attachment_1479\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 6C[\/caption]\r\n\r\n[caption id=\"attachment_1480\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 6D[\/caption]\r\n\r\n[caption id=\"attachment_1481\" align=\"aligncenter\" width=\"499\"]\"\" Figure Step 6E[\/caption]\r\n

    Step 7<\/h2>\r\nTo insert a Work Point at the midpoint of an edge. Click the WORK POINT command and then On Vertex, Sketch point, or Midpoint. Snap to the midpoint of the edge shown in the figure. The midpoint will highlight with a yellow work point symbol. Select it when it appears. (Figure Step 7A, 7B, and 7C)\r\n\r\n[caption id=\"attachment_1482\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 7A[\/caption]\r\n\r\n[caption id=\"attachment_1483\" align=\"aligncenter\" width=\"374\"]\"\" Figure Step 7B[\/caption]\r\n\r\n[caption id=\"attachment_2124\" align=\"aligncenter\" width=\"511\"]\"\" Figure Step 7C[\/caption]\r\n\r\n
    <\/div>\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>You should now have three Work Points inserted.<\/div>\r\n

    Step 8<\/h2>\r\nWork Features will display as items in the Browser bar. Note the three Work Points that you just inserted. The visibility of Work Features can be enabled or disabled in the Right-click menu. (Figure 8A and 8B)\r\n\r\n[caption id=\"attachment_1485\" align=\"aligncenter\" width=\"245\"]\"\" Figure Step 8A[\/caption]\r\n\r\n[caption id=\"attachment_1498\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 8B[\/caption]\r\n

    Step 9<\/h2>\r\nInsert a Work Axis on the centerline of the cylinder. Enter the WORK AXIS command and then Through Center of Circular or Elliptical Edge. Select the cylinder as shown in the figure. Note how the cylinder highlights. The axis will appear as a colored line. (Figure Step 9A, 9B, and 9C)\r\n\r\n[caption id=\"attachment_1486\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 9A[\/caption]\r\n\r\n[caption id=\"attachment_1487\" align=\"aligncenter\" width=\"314\"]\"\" Figure Step 9B[\/caption]\r\n\r\n[caption id=\"attachment_1488\" align=\"aligncenter\" width=\"235\"]\"\" Figure Step 9C[\/caption]\r\n

    Step 10<\/h2>\r\nInsert a Work Axis between two Work Points. Enter the WORK AXIS command and then Through Two Points. Select the Work Points on the front edge and the back corner. (Figure Step 10A, 10B, 10C, and 10D)\r\n\r\n[caption id=\"attachment_1489\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 10A[\/caption]\r\n\r\n[caption id=\"attachment_1490\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 10B[\/caption]\r\n\r\n[caption id=\"attachment_1491\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 10C[\/caption]\r\n\r\n[caption id=\"attachment_1492\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 10D[\/caption]\r\n

    Step 11<\/h2>\r\nInsert a Work Axis at the intersection of two non-parallel faces. Enter the WORK AXIS command and then Intersection of Two Planes. Select the face on the left side and then the face on the right side. The Work Axis will appear at the apparent intersection of the two faces. (Figure Step 11A, 11B, 11C, and 11D)\r\n\r\n[caption id=\"attachment_1493\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 11A[\/caption]\r\n\r\n[caption id=\"attachment_1494\" align=\"aligncenter\" width=\"400\"]\"\" Figure Step 11B[\/caption]\r\n\r\n[caption id=\"attachment_1495\" align=\"aligncenter\" width=\"388\"]\"\" Figure Step 11C[\/caption]\r\n\r\n[caption id=\"attachment_1496\" align=\"aligncenter\" width=\"400\"]\"\" Figure Step 11D[\/caption]\r\n

    Step 12<\/h2>\r\nWork Features will display as items in the Browser bar. Note the three Work Axes that you just inserted. (Figure Step 12)\r\n\r\n[caption id=\"attachment_1497\" align=\"aligncenter\" width=\"292\"]\"\" Figure Step 12[\/caption]\r\n

    Step 13<\/h2>\r\nInsert a Work Plane from an existing face and through a Work Axis at a specified angle. Enter the WORK PLANE command and then Plane. Select the face on the right side of the model and then select the Work Axis at the centre of the cylinder. Enter the angle between the new Work Plane and the face. In this case, 90 degrees or perpendicular. (Figure Step 13A, 13B, 13C, and 13D)\r\n\r\n[caption id=\"attachment_1501\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 13A[\/caption]\r\n\r\n[caption id=\"attachment_1502\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 13B[\/caption]\r\n\r\n[caption id=\"attachment_1503\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 13C[\/caption]\r\n\r\n[caption id=\"attachment_1504\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 13D[\/caption]\r\n

    Step 14<\/h2>\r\nInsert an offset Work Plane. Enter the WORK PLANE command and then Offset from Plane<\/span>. Select the face on the right side. Hold down the left mouse button and drag the plane into the model. The Offset dialogue box will display. Enter the offset distance of -1.25 inches. (Figure Step 14A, 14B, and 14C)\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>The offset is negative since that is the negative Z direction of the work plane.<\/div>\r\n\r\n[caption id=\"attachment_1505\" align=\"aligncenter\" width=\"247\"]\"\" Figure Step 14A[\/caption]\r\n\r\n[caption id=\"attachment_1506\" align=\"aligncenter\" width=\"345\"]\"\" Figure Step 14B[\/caption]\r\n\r\n[caption id=\"attachment_1507\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 14C[\/caption]\r\n

    Step 15<\/h2>\r\nMove the cursor to the edge of the newly inserted work plane and when the double arrow icon appears, press and hold down the left mouse button. While holding it down, drag it to enlarge the plane. Do this for all four corners. (Figure Step 15A and 15B)\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>To get the double arrow to appear, you sometimes have to move the cursor to the corner and click the mouse.<\/div>\r\n\r\n[caption id=\"attachment_1508\" align=\"aligncenter\" width=\"478\"]\"\" Figure Step 15A[\/caption]\r\n\r\n[caption id=\"attachment_1509\" align=\"aligncenter\" width=\"457\"]\"\" Figure Step 15B[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>Work axes and work planes can be expanded to any size you require.<\/div>\r\n

    Step 16<\/h2>\r\nInsert a Work Plane on a work axis and at an angle to an existing plane. Enter the WORK PLANE command and then Plane. Select the Work Axis shown in the figure. Select the bottom plane next and enter the angle of 90 degrees. (Figure Step 16A, 16B, 16C, 16D, and 16E)\r\n\r\n[caption id=\"attachment_1510\" align=\"aligncenter\" width=\"615\"]\"\" Figure Step 16A[\/caption]\r\n\r\n[caption id=\"attachment_1511\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 16B[\/caption]\r\n\r\n[caption id=\"attachment_1512\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 16D[\/caption]\r\n\r\n[caption id=\"attachment_1513\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 16E[\/caption]\r\n

    Step 17<\/h2>\r\nThe Browser bar should now appear as shown in the figure. (Figure Step 17)\r\n\r\n[caption id=\"attachment_1515\" align=\"aligncenter\" width=\"265\"]\"\" Figure Step 17[\/caption]\r\n

    Step 18<\/h2>\r\nDisable the visibility of all Work Features. Your solid model should appear as shown in the figure. (Figure Step 18)\r\n\r\n[caption id=\"attachment_1518\" align=\"aligncenter\" width=\"409\"]\"\" Figure Step 18[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>You will now be using the drawings shown in Figures 19-6 and 19-7 and inserting Work Features to add the detail on the model.<\/div>\r\n\r\n[caption id=\"attachment_1516\" align=\"aligncenter\" width=\"398\"]\"\" Figure 19-6
    Dimensioned Multiview Drawing[\/caption]\r\n\r\n[caption id=\"attachment_1517\" align=\"aligncenter\" width=\"500\"]\"\" Figure 19-7
    3D Model - Home View[\/caption]\r\n

    Step 19<\/h2>\r\nUsing the offset method, insert a Work Plane -2.25 inches from the right side face. Expand the size of the Work Plane. Start a new sketch on the Work Plane. (Figure Step 19A and 19B)\r\n\r\n[caption id=\"attachment_1519\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 19A[\/caption]\r\n\r\n[caption id=\"attachment_1520\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 19B[\/caption]\r\n

    Step 20<\/h2>\r\nEnter the TWO POINT RECTANGLE command and right click the mouse. Ensure that AutoProject is enabled. Draw a rectangle by snapping to the bottom right corner. Dimension the square and ensure it is fully constrained. Extrude the sketch. (Figure Step 20A, 20B, 20C, and 20D)\r\n\r\n[caption id=\"attachment_1521\" align=\"aligncenter\" width=\"134\"]\"\" Figure Step 20A[\/caption]\r\n\r\n[caption id=\"attachment_1523\" align=\"aligncenter\" width=\"368\"]\"\" Figure Step 20B[\/caption]\r\n\r\n[caption id=\"attachment_1524\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 20C[\/caption]\r\n\r\n[caption id=\"attachment_1525\" align=\"aligncenter\" width=\"394\"]\"\" Figure Step 20D[\/caption]\r\n

    Step 21<\/h2>\r\nStart a new sketch and draw two lines. Dimension and extrude it. (Figure Step 21A and 21B)\r\n\r\n[caption id=\"attachment_1526\" align=\"aligncenter\" width=\"469\"]\"\" Figure Step 21A[\/caption]\r\n\r\n[caption id=\"attachment_1527\" align=\"aligncenter\" width=\"448\"]\"\" Figure Step 21B[\/caption]\r\n

    Step 22<\/h2>\r\nInsert a Work Plane -0.375 inches in from the front face. (Figure Step 22)\r\n\r\n[caption id=\"attachment_1529\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 22[\/caption]\r\n

    Step 23<\/h2>\r\nDraw a triangle and insert two dimensions to fully constrain it. (Figure Step 23)\r\n\r\n[caption id=\"attachment_1530\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 23 [Click to see image full size][\/caption]\r\n

    Step 24<\/h2>\r\nExtrude the sketch 0.125 inches in both directions to complete the part. (Figure Step 24)\r\n\r\n[caption id=\"attachment_1531\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 24 [Click to see image full size][\/caption]\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>I placed the sketch at the centre of the rib so I extruded it one-half its width in both directions.<\/div>\r\n

    Step 25<\/h2>\r\nDisable the visibility of all Work Features. The completed solid model should appear as shown in the figure. (Figure Step 25)\r\n\r\n[caption id=\"attachment_1532\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 25[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>As you can see there are may ways to insert and use Work Features. Practice inserting them as you construct future models. Read Inventor's Help files if you have trouble.<\/div>\r\n

    Step 26<\/h2>\r\nChange to the Home view. (Figure Step 26)\r\n\r\n[caption id=\"attachment_1533\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 26 [Click to see image full size][\/caption]\r\n

    Step 27<\/h2>\r\nSave and close the part.\r\n

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

    Key Principles in Module 19<\/p>\r\n\r\n<\/header>\r\n

    \r\n
      \r\n \t
    1. The POLYGON command is used to draw a regular polygon on a 2D sketch. You can select the number of sides and choose between either an inscribed or a circumscribed polygon.<\/li>\r\n \t
    2. The threads created by the THREAD command are not actual threads constructed on the model. They are simply a graphical representation of the threads.<\/li>\r\n \t
    3. The TANGENT CIRCLE command is used to draw a circle tangent to three lines.<\/li>\r\n \t
    4. The AUTO DIMENSION command is used to add dimensions or constrains automatically to fully constrain a sketch.<\/li>\r\n \t
    5. The three Work Features available in Inventor are the Work Point, the Work Axis, and the Work Plane.<\/li>\r\n \t
    6. A Work Point is a parametric construction point or a single XYZ location that is inserted and then used as a Work Feature.<\/li>\r\n \t
    7. A Work Axis is a parametric construction line or two XYZ locations joined by a line that is inserted and then used as a Work Feature.<\/li>\r\n \t
    8. A Work Plane is parametric construction plane or four XYZ locations joined by lines inserted on the model or Model space and then used as a Work Feature.<\/li>\r\n<\/ol>\r\n<\/div>\r\n<\/div>\r\n

      Lab Exercise 19-1<\/h1>\r\nTime allowed: 90 minutes.\r\n\r\n\r\n\r\n\r\n
      Part Name<\/strong><\/td>\r\nProject<\/strong><\/td>\r\nUnits<\/strong><\/td>\r\nTemplate<\/strong><\/td>\r\nColor<\/strong><\/td>\r\nMaterial<\/strong><\/td>\r\n<\/tr>\r\n
      Inventor Lab Lab 19-1<\/td>\r\nInventor Course<\/td>\r\nMillimeters<\/td>\r\nMetric - Modules Part (mm).ipt<\/td>\r\nChrome - Black Polished<\/td>\r\nN\/A<\/td>\r\n<\/tr>\r\n<\/tbody>\r\n<\/table>\r\n

      Step 1<\/h2>\r\nDraw the Base sketch on the Front view.\r\n

      Step 2<\/h2>\r\nProject the Center Point onto the Base plane.\r\n

      Step 3<\/h2>\r\nNote the location of X0Y0Z0. Draw the necessary sketches and EXTRUDE them to produce the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. (Figure Step 3A, 3B, 3C, 3D, and 3E)\r\n\r\n[caption id=\"attachment_1535\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 3A
      3D Model - Orbited View[\/caption]\r\n\r\n[caption id=\"attachment_1536\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 3B
      3D Model - Home View[\/caption]\r\n\r\n[caption id=\"attachment_1537\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 3C
      Solid Model - Home View[\/caption]\r\n\r\n[caption id=\"attachment_1538\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 3D
      3D Model - Orbited View[\/caption]\r\n\r\n[caption id=\"attachment_1540\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 1E
      Left Side View - Multiview Drawing [Click to see image full size][\/caption][caption id=\"attachment_1541\" align=\"aligncenter\" width=\"500\"]      \"\"<\/a> Figure Step 1F
      Right Side View - Multiview Drawing [Click to see image full size][\/caption]\r\n

      Step 4<\/h2>\r\nCreate the fillets and chamfers after the model is totally constructed.\r\n

      Step 5<\/h2>\r\nApply the colour shown above.\r\n

      Lab Exercise 19-2<\/h1>\r\nTime allowed: 90 minutes.\r\n\r\n\r\n\r\n\r\n
      Part Name<\/strong><\/td>\r\nProject<\/strong><\/td>\r\nUnits<\/strong><\/td>\r\nTemplate<\/strong><\/td>\r\nColor<\/strong><\/td>\r\nMaterial<\/strong><\/td>\r\n<\/tr>\r\n
      Inventor Lab Lab 19-2<\/td>\r\nInventor Course<\/td>\r\nMillimeters<\/td>\r\nMetric - Modules Part (mm).ipt<\/td>\r\nChrome - Black Polished<\/td>\r\nN\/A<\/td>\r\n<\/tr>\r\n<\/tbody>\r\n<\/table>\r\n

      Step 1<\/h2>\r\nDraw the Base sketch on the Right Side view.\r\n

      Step 2<\/h2>\r\nProject the Center Point onto the Base plane.\r\n

      Step 3<\/h2>\r\nNote the location of X0Y0Z0. Draw the same model you just drew in Lab Exercise 19-1. In this exercise, REVOLVE the Base sketch and then add sketches and extrude them to complete the model. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. (Figure Step 3A, 3B, 3C, and 3D)\r\n\r\n[caption id=\"attachment_2125\" align=\"aligncenter\" width=\"305\"]\"\" Figure Step 3A
      3D Model - Orbited View[\/caption]\r\n\r\n[caption id=\"attachment_2126\" align=\"aligncenter\" width=\"305\"]\"\" Figure Step 3B
      3D Model - Home View[\/caption]\r\n\r\n[caption id=\"attachment_1543\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 3C
      Solid Model - Home View[\/caption]\r\n\r\n[caption id=\"attachment_1544\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 3D
      Solid Model - Orbited View[\/caption]\r\n\r\n[caption id=\"attachment_2127\" align=\"aligncenter\" width=\"709\"]\"\" Author's Base Sketch[\/caption]\r\n\r\n[caption id=\"attachment_2128\" align=\"aligncenter\" width=\"264\"]\"\" Author's Base Model[\/caption]\r\n

      Step 4<\/h2>\r\nCreate the fillets and chamfers after the model is totally constructed.\r\n

      Step 5<\/h2>\r\nApply the colour shown above.\r\n

      Lab Exercise 19-3<\/h1>\r\nTime allowed: 90 minutes.\r\n\r\n\r\n\r\n\r\n
      Part Name<\/strong>: Inventor Lab 19-3<\/td>\r\nProject<\/strong>: Inventor Course<\/td>\r\nUnits<\/strong>: Millimeters<\/td>\r\n<\/tr>\r\n
      Template<\/strong>: Metric - Modules Part (mm).ipt<\/td>\r\nColor<\/strong>: Galvanized (texture)<\/td>\r\nMaterial<\/strong>: N\/A<\/td>\r\n<\/tr>\r\n<\/tbody>\r\n<\/table>\r\n

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

      Step 2<\/h2>\r\nDraw the necessary sketches and extrude or revolve them to produce the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. (Figure Step 2A, 2B, 2C, 2D, and 2E)\r\n\r\n[caption id=\"attachment_1550\" align=\"aligncenter\" width=\"305\"]\"\" Figure Step 2A
      3D Model - Home View[\/caption]\r\n\r\n[caption id=\"attachment_1551\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 2B [Click to see image full size][\/caption]\r\n\r\n[caption id=\"attachment_1552\" align=\"aligncenter\" width=\"615\"]\"\" Figure Step 2C
      Suggested Base Sketch - Author's Base Model Top (XY) Plane[\/caption]\r\n\r\n[caption id=\"attachment_1553\" align=\"aligncenter\" width=\"615\"]\"\" Author's Base Sketch[\/caption]\r\n\r\n[caption id=\"attachment_1554\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 2D
      Solid Model - Home View
      With Work Planes[\/caption]\r\n\r\n[caption id=\"attachment_1555\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 2E
      Solid Model - Home View[\/caption]\r\n

      Step 3<\/h2>\r\nCreate the fillets and chamfers after the model is totally constructed.\r\n

      Step 4<\/h2>\r\nApply the colour shown above.","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 and apply the POLYGON, TANGENT CIRCLE, and THREAD commands.<\/li>\n
      2. Describe work features including Work Points, Work Axes, and Work Planes and explain how they are used in model construction.<\/li>\n
      3. Describe and apply the WORK POINT, WORK AXIS, and WORK PLANE commands.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

        Geometry Lesson: Regular Polygons<\/h1>\n

        A polygon<\/span> <\/em>is defined as any plane figure bounded by straight lines. A regular polygon<\/span> <\/em>is a polygon that has equal angles, equal sides and can be inscribed in or circumscribed around a circle. The first eight regular polygons are shown in Figure 19-1.<\/p>\n

        \"\"
        Figure 19-1
        Regular Polygons
        Work<\/figcaption><\/figure>\n

        Any regular polygon can be inscribed in or circumscribed around a circle as shown, using a hexagon, in Figure 19-2.<\/p>\n

        \"\"
        Figure 19-2
        Inscribed and Circumscribed Regular Polygon<\/figcaption><\/figure>\n

        It is important to understand and know the geometry involved to construct a triangle, square, hexagon, and octagon as shown in Figure 19-3. Study each one and try to understand how they are constructed and the angles used to construct them.<\/p>\n

        \"\"
        Figure 19-3
        Geometry of Four Regular Polygons<\/figcaption><\/figure>\n
        \n
        \n

        Inventor Command:\u00a0POLYGON<\/p>\n<\/header>\n

        \n

        The POLYGON command is used to draw a regular polygon on a 2D sketch. You can select the number of sides and choose between either an inscribed or a circumscribed polygon.<\/p>\n

        Shortcut: none<\/strong><\/p>\n

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

        \n
        \n

        Inventor Command:\u00a0TANGENT CIRCLE<\/p>\n<\/header>\n

        \n

        The TANGENT CIRCLE command is used to draw a circle tangent to three lines.<\/p>\n

        Shortcut: none<\/strong><\/p>\n

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

        \n
        \n

        Inventor Command: AUTO DIMENSION<\/p>\n<\/header>\n

        \n

        The AUTO DIMENSION command is used to add dimensions or constrains automatically to fully constrain a sketch.<\/p>\n

        Shortcut: none<\/strong><\/p>\n

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

        Drawing Threads<\/h2>\n

        The THREAD command is used to draw exterior threads or interior threads on a 3D solid model. See Figure 19-4 The threads created using the THREAD command are not actual threads constructed on the model. They are simply a graphical representation of the threads. A real life solid model created from the Inventor part would not be threaded. Actual threads can be created but this is a much more advanced feature that is taught in the Inventor Advanced book. The thread specifications can be applied to the thread in the sketch and then be used when creating the working drawing of the part.<\/p>\n

        \"\"
        Figure 19-4
        External and Internal Threads<\/figcaption><\/figure>\n
        \n
        \n

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

        \n

        The THREAD command is used to draw a graphical representation of an outside or inside diameter thread. The thread specifications can also added to the thread properties.<\/p>\n

        Shortcut: none<\/strong><\/p>\n

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

        WORK ALONG: Drawing Polygons and Threads – Part 1<\/h1>\n

        Step 1<\/h2>\n

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

        Step 2<\/h2>\n

        Save the file with the name: Inventor Workalong 19-1<\/span>. (Figure Step 2A, 2B, and 2C)<\/p>\n

        \"\"
        Figure Step 2A
        3D Model –
        Home View<\/figcaption><\/figure>\n
        \"\"
        Figure Step 2B
        Dimensioned Multiview Drawing<\/figcaption><\/figure>\n
        \"\"
        Figure Step 2C
        Detail<\/figcaption><\/figure>\n

        Step 3<\/h2>\n

        Draw the Base sketch on the Top or XY plane.<\/p>\n

        Step 4<\/h2>\n

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

        Step 5<\/h2>\n

        Enter the POLYGON command and set the number of sides to 6. (Figure Step 5)<\/p>\n

        \"\"
        Figure Step 5<\/figcaption><\/figure>\n

        Step 6<\/h2>\n

        Enable the Circumscribed Polygon icon. Snap to the Center Point for the centre and select a radius of approximately 0.75 inches. (Figure Step 6)<\/p>\n

        \"\"
        Fig Step 6<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>A circumscribed polygon is used in this sketch because the edge to edge dimension was given rather then corner to corner.<\/div>\n

        Step 7<\/h2>\n

        Add the dimension from the Center Point to the left line. (Figure Step 7)<\/p>\n

        \"\"
        Figure Step 7<\/figcaption><\/figure>\n

        Step 8<\/h2>\n

        Enter the AUTO DIMENSION command. Note that one dimension or constraint is required to fully constrain the sketch. Click Apply. (Figure Step 8A, 8B, and 8C<\/p>\n

        \"\"
        Figure Step 8A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 8B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 8C<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>This will add a constraint to fully constrain the sketch. The AUTO DIMENSION command is used to automatically add the dimensions or constraints to fully constrain it.<\/div>\n

        Step 9<\/h2>\n

        Extrude the hexagon in the negative Z direction. (Figure Step 9)<\/p>\n

        \"\"<\/a>
        Figure Step 9 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 10<\/h2>\n

        Start a new sketch on the bottom side of the Base model. Enter the TANGENT CIRCLE command. When prompted, select any three edges. (Figure Step 10)<\/p>\n

        \"\"
        Figure Step 10<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>Since you are inserting a circle tangent inside of a regular polygon, any three edges can be selected.<\/div>\n

        Step 11<\/h2>\n

        Extrude the circle 0.016 inches. Ensure that you enable the Join<\/span> icon and extrude it away from the bolt head. (Figure Step 11)<\/p>\n

        \"\"<\/a>
        Figure Step 11 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 12<\/h2>\n

        Start a new sketch on the extruded circle. Draw and dimension a 1 inch circle using the centre of the circle to snap to. Extrude the circle 3 inches. (Figure Step 12A and 12B)<\/p>\n

        \"\"
        Figure Step 12A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 12B<\/figcaption><\/figure>\n

        Step 13<\/h2>\n

        Using the CHAMFER command, chamfer the bottom of the bolt. (Figure Step 13)<\/p>\n

        \"\"<\/a>
        Figure Step 13 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 14<\/h2>\n

        Enter the THREAD command. Enable the Location tab and set the Length to 1.5 and then select the cylinder as the face to thread. Do not close the dialogue box. (Figure Step 14)<\/p>\n

        \"\"<\/a>
        Figure Step 14 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 15<\/h2>\n

        Enable the Specification tab. Set the thread specifications as shown in the figure. Click OK to execute the command. (Figure Step 15A and 15B)<\/p>\n

        \"\"<\/a>
        Figure Step 15A [Click to see image full size]<\/figcaption><\/figure>\n
        \"\"
        Figure Step 15B<\/figcaption><\/figure>\n

        Step 16<\/h2>\n

        Change the view to the Home view and change the colour to: Metal-Brass<\/span>. (Figure Step 16)<\/p>\n

        \"\"
        Figure Step 16<\/figcaption><\/figure>\n

        Step 17<\/h2>\n

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

        MUST KNOW:<\/strong> The threads created by the THREAD command are not actual threads constructed on the model. They are simply a graphical representation of the threads. A real life solid model created from the Inventor part file would not be threaded.<\/div>\n

        WORK ALONG: Drawing Polygons and Threads – Part 2<\/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 19-2<\/span>.<\/p>\n

        Step 4<\/h2>\n

        Using what you learned in the last workalong, construct the nut shown in the multiview drawing. (Figure Step 4A and 4B)<\/p>\n

        \"\"
        Figure Step 4A
        Dimensioned Multiview Drawing<\/figcaption><\/figure>\n
        \"\"
        Figure Step 4B 3D Model – Home View<\/figcaption><\/figure>\n

        Step 5<\/h2>\n

        Change the colour to: Metal-Brass<\/span>. (Figure Step 5A and 5B)<\/p>\n

        \"\"
        Figure Step 5A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 5B<\/figcaption><\/figure>\n

        Work Features<\/h1>\n

        Work Features<\/em><\/span> consists of points, axes, and planes that can be inserted on a solid model or in Model space. They are used as a construction aids to draw the model. You can insert them when existing geometry cannot be used to add geometry. The three work features available in Inventor are the work point, the work axis, and the work plane. See Figure 19-5. This module is an introduction to work features only and will teach the user how to create and use them in part modeling. They are also used in assemblies.<\/p>\n

        \"\"
        Figure 19-5
        Work Features<\/figcaption><\/figure>\n

        Work Points<\/h2>\n

        A Work Point<\/span> <\/em>is a parametric construction point or a single XYZ location that is inserted and then used as a work feature. Once a Work Point is inserted on the model, it can be projected onto part faces, linear edges, or onto an arc or circle using the PROJECT GEOMETRY command. Work Points can also be constrained to the centre points of arcs, circles, and ellipses. In this module, inserting Work Points on the model or in 3D space will be taught.<\/p>\n

        Work Axes<\/h2>\n

        A Work Axis<\/em><\/span> is a parametric construction line or two XYZ locations joined by a line that is inserted and then used as a work feature. Even though a Work Axis appears as a specified length, as far as Inventor is concerned, it is infinite in length and can be expanded to any length required.<\/p>\n

        Use Work Axes when creating models to mark symmetry lines, centre lines, or distances between revolved feature axes. Work Axes can be used along the symmetry lines of circular features such as cylinders, shafts, or holes. They can also be created as a work axis on a linear edge, a sketch line, or a 3D sketch line.<\/p>\n

        Work Planes<\/h2>\n

        A Work Plane<\/span><\/em> is parametric construction plane or four XYZ locations joined by lines inserted on the model or in model space and then used as a work feature. Even though a Work Plane appears as a rectangular plane of a given size, it is actually infinite in size and can be expanded to any size required.<\/p>\n

        Work Planes can be placed at any orientation in space, offset from existing faces, or rotated around an axis or edge. A work plane can be used as a sketch plane and dimensioned or constrained to other features or components. Each work plane has its own internal coordinate system. The order in which geometry is selected determines the origin and positive directions of the coordinate system axes.<\/p>\n

        \n
        \n

        Inventor Command: WORK POINT<\/p>\n<\/header>\n

        \n

        The WORK POINT command is used to insert a Work Point on the model or in Model space.<\/p>\n

        Shortcut:\u00a0. (period)<\/strong><\/p>\n

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

        \n
        \n

        Inventor Command: WORK AXIS<\/p>\n<\/header>\n

        \n

        The WORK AXIS command is used to insert a Work Axis on the model or in Model space.<\/p>\n

        Shortcut:\u00a0\/ (forward slash)<\/strong><\/p>\n

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

        \n
        \n

        Inventor Command: WORK PLANE<\/p>\n<\/header>\n

        \n

        The WORK PLANE command is used to insert a Work Plane on the model or in Model space.<\/p>\n

        Shortcut:] (right bracket)<\/strong><\/p>\n

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

        WORK ALONG: Creating Work Features<\/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 19-3<\/span>.<\/p>\n

        Step 4<\/h2>\n

        Create the solid model shown in the figures. (Figure Step 4A and 4B)<\/p>\n

        \"\"
        Figure Step 4A
        3D Model – Home View<\/figcaption><\/figure>\n
        \"\"<\/a>
        Figure Step 4B
        Dimensioned Multiview Drawing [Click to see image full size]<\/figcaption><\/figure>\n

        Step 5<\/h2>\n

        Insert a Work Point at the apparent intersection of two edges. Click the WORK POINT command and then Intersection of Two Lines. Select the edges shown in the figure. Note how they highlight and extend. (Figure Step 5A, 5B, and 5C)<\/p>\n

        \"\"
        Figure Step 5A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 5B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 5C<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>The Work Point will be inserted at the apparent intersection of the two selected edges.<\/div>\n

        Step 6<\/h2>\n

        Insert a Work Point at the intersection of three planes. Click the WORK POINT command and then Intersection of Three Planes. Select the planes shown in the figures. (Figure Step 6A, 6B, 6C, 6D, and 6E)<\/p>\n

        \"\"
        Figure Step 6A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 6B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 6C<\/figcaption><\/figure>\n
        \"\"
        Figure Step 6D<\/figcaption><\/figure>\n
        \"\"
        Figure Step 6E<\/figcaption><\/figure>\n

        Step 7<\/h2>\n

        To insert a Work Point at the midpoint of an edge. Click the WORK POINT command and then On Vertex, Sketch point, or Midpoint. Snap to the midpoint of the edge shown in the figure. The midpoint will highlight with a yellow work point symbol. Select it when it appears. (Figure Step 7A, 7B, and 7C)<\/p>\n

        \"\"
        Figure Step 7A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 7B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 7C<\/figcaption><\/figure>\n
        <\/div>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>You should now have three Work Points inserted.<\/div>\n

        Step 8<\/h2>\n

        Work Features will display as items in the Browser bar. Note the three Work Points that you just inserted. The visibility of Work Features can be enabled or disabled in the Right-click menu. (Figure 8A and 8B)<\/p>\n

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

        Step 9<\/h2>\n

        Insert a Work Axis on the centerline of the cylinder. Enter the WORK AXIS command and then Through Center of Circular or Elliptical Edge. Select the cylinder as shown in the figure. Note how the cylinder highlights. The axis will appear as a colored line. (Figure Step 9A, 9B, and 9C)<\/p>\n

        \"\"
        Figure Step 9A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 9B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 9C<\/figcaption><\/figure>\n

        Step 10<\/h2>\n

        Insert a Work Axis between two Work Points. Enter the WORK AXIS command and then Through Two Points. Select the Work Points on the front edge and the back corner. (Figure Step 10A, 10B, 10C, and 10D)<\/p>\n

        \"\"
        Figure Step 10A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 10B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 10C<\/figcaption><\/figure>\n
        \"\"
        Figure Step 10D<\/figcaption><\/figure>\n

        Step 11<\/h2>\n

        Insert a Work Axis at the intersection of two non-parallel faces. Enter the WORK AXIS command and then Intersection of Two Planes. Select the face on the left side and then the face on the right side. The Work Axis will appear at the apparent intersection of the two faces. (Figure Step 11A, 11B, 11C, and 11D)<\/p>\n

        \"\"
        Figure Step 11A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 11B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 11C<\/figcaption><\/figure>\n
        \"\"
        Figure Step 11D<\/figcaption><\/figure>\n

        Step 12<\/h2>\n

        Work Features will display as items in the Browser bar. Note the three Work Axes that you just inserted. (Figure Step 12)<\/p>\n

        \"\"
        Figure Step 12<\/figcaption><\/figure>\n

        Step 13<\/h2>\n

        Insert a Work Plane from an existing face and through a Work Axis at a specified angle. Enter the WORK PLANE command and then Plane. Select the face on the right side of the model and then select the Work Axis at the centre of the cylinder. Enter the angle between the new Work Plane and the face. In this case, 90 degrees or perpendicular. (Figure Step 13A, 13B, 13C, and 13D)<\/p>\n

        \"\"
        Figure Step 13A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 13B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 13C<\/figcaption><\/figure>\n
        \"\"
        Figure Step 13D<\/figcaption><\/figure>\n

        Step 14<\/h2>\n

        Insert an offset Work Plane. Enter the WORK PLANE command and then Offset from Plane<\/span>. Select the face on the right side. Hold down the left mouse button and drag the plane into the model. The Offset dialogue box will display. Enter the offset distance of -1.25 inches. (Figure Step 14A, 14B, and 14C)<\/p>\n

        AUTHOR’S COMMENTS:\u00a0<\/strong>The offset is negative since that is the negative Z direction of the work plane.<\/div>\n
        \"\"
        Figure Step 14A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 14B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 14C<\/figcaption><\/figure>\n

        Step 15<\/h2>\n

        Move the cursor to the edge of the newly inserted work plane and when the double arrow icon appears, press and hold down the left mouse button. While holding it down, drag it to enlarge the plane. Do this for all four corners. (Figure Step 15A and 15B)<\/p>\n

        AUTHOR’S COMMENTS:\u00a0<\/strong>To get the double arrow to appear, you sometimes have to move the cursor to the corner and click the mouse.<\/div>\n
        \"\"
        Figure Step 15A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 15B<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>Work axes and work planes can be expanded to any size you require.<\/div>\n

        Step 16<\/h2>\n

        Insert a Work Plane on a work axis and at an angle to an existing plane. Enter the WORK PLANE command and then Plane. Select the Work Axis shown in the figure. Select the bottom plane next and enter the angle of 90 degrees. (Figure Step 16A, 16B, 16C, 16D, and 16E)<\/p>\n

        \"\"
        Figure Step 16A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 16B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 16D<\/figcaption><\/figure>\n
        \"\"
        Figure Step 16E<\/figcaption><\/figure>\n

        Step 17<\/h2>\n

        The Browser bar should now appear as shown in the figure. (Figure Step 17)<\/p>\n

        \"\"
        Figure Step 17<\/figcaption><\/figure>\n

        Step 18<\/h2>\n

        Disable the visibility of all Work Features. Your solid model should appear as shown in the figure. (Figure Step 18)<\/p>\n

        \"\"
        Figure Step 18<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>You will now be using the drawings shown in Figures 19-6 and 19-7 and inserting Work Features to add the detail on the model.<\/div>\n
        \"\"
        Figure 19-6
        Dimensioned Multiview Drawing<\/figcaption><\/figure>\n
        \"\"
        Figure 19-7
        3D Model – Home View<\/figcaption><\/figure>\n

        Step 19<\/h2>\n

        Using the offset method, insert a Work Plane -2.25 inches from the right side face. Expand the size of the Work Plane. Start a new sketch on the Work Plane. (Figure Step 19A and 19B)<\/p>\n

        \"\"
        Figure Step 19A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 19B<\/figcaption><\/figure>\n

        Step 20<\/h2>\n

        Enter the TWO POINT RECTANGLE command and right click the mouse. Ensure that AutoProject is enabled. Draw a rectangle by snapping to the bottom right corner. Dimension the square and ensure it is fully constrained. Extrude the sketch. (Figure Step 20A, 20B, 20C, and 20D)<\/p>\n

        \"\"
        Figure Step 20A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 20B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 20C<\/figcaption><\/figure>\n
        \"\"
        Figure Step 20D<\/figcaption><\/figure>\n

        Step 21<\/h2>\n

        Start a new sketch and draw two lines. Dimension and extrude it. (Figure Step 21A and 21B)<\/p>\n

        \"\"
        Figure Step 21A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 21B<\/figcaption><\/figure>\n

        Step 22<\/h2>\n

        Insert a Work Plane -0.375 inches in from the front face. (Figure Step 22)<\/p>\n

        \"\"
        Figure Step 22<\/figcaption><\/figure>\n

        Step 23<\/h2>\n

        Draw a triangle and insert two dimensions to fully constrain it. (Figure Step 23)<\/p>\n

        \"\"<\/a>
        Figure Step 23 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 24<\/h2>\n

        Extrude the sketch 0.125 inches in both directions to complete the part. (Figure Step 24)<\/p>\n

        \"\"<\/a>
        Figure Step 24 [Click to see image full size]<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>I placed the sketch at the centre of the rib so I extruded it one-half its width in both directions.<\/div>\n

        Step 25<\/h2>\n

        Disable the visibility of all Work Features. The completed solid model should appear as shown in the figure. (Figure Step 25)<\/p>\n

        \"\"
        Figure Step 25<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>As you can see there are may ways to insert and use Work Features. Practice inserting them as you construct future models. Read Inventor’s Help files if you have trouble.<\/div>\n

        Step 26<\/h2>\n

        Change to the Home view. (Figure Step 26)<\/p>\n

        \"\"<\/a>
        Figure Step 26 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 27<\/h2>\n

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

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

        Key Principles in Module 19<\/p>\n<\/header>\n

        \n
          \n
        1. The POLYGON command is used to draw a regular polygon on a 2D sketch. You can select the number of sides and choose between either an inscribed or a circumscribed polygon.<\/li>\n
        2. The threads created by the THREAD command are not actual threads constructed on the model. They are simply a graphical representation of the threads.<\/li>\n
        3. The TANGENT CIRCLE command is used to draw a circle tangent to three lines.<\/li>\n
        4. The AUTO DIMENSION command is used to add dimensions or constrains automatically to fully constrain a sketch.<\/li>\n
        5. The three Work Features available in Inventor are the Work Point, the Work Axis, and the Work Plane.<\/li>\n
        6. A Work Point is a parametric construction point or a single XYZ location that is inserted and then used as a Work Feature.<\/li>\n
        7. A Work Axis is a parametric construction line or two XYZ locations joined by a line that is inserted and then used as a Work Feature.<\/li>\n
        8. A Work Plane is parametric construction plane or four XYZ locations joined by lines inserted on the model or Model space and then used as a Work Feature.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

          Lab Exercise 19-1<\/h1>\n

          Time allowed: 90 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 19-1<\/td>\nInventor Course<\/td>\nMillimeters<\/td>\nMetric – Modules Part (mm).ipt<\/td>\nChrome – Black Polished<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

          Draw the Base sketch on the Front view.<\/p>\n

          Step 2<\/h2>\n

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

          Step 3<\/h2>\n

          Note the location of X0Y0Z0. Draw the necessary sketches and EXTRUDE them to produce the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. (Figure Step 3A, 3B, 3C, 3D, and 3E)<\/p>\n

          \"\"
          Figure Step 3A
          3D Model – Orbited View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 3B
          3D Model – Home View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 3C
          Solid Model – Home View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 3D
          3D Model – Orbited View<\/figcaption><\/figure>\n
          \"\"<\/a>
          Figure Step 1E
          Left Side View – Multiview Drawing [Click to see image full size]<\/figcaption><\/figure>\n
          \"\"<\/a>
          Figure Step 1F
          Right Side View – Multiview Drawing [Click to see image full size]<\/figcaption><\/figure>\n

          Step 4<\/h2>\n

          Create the fillets and chamfers after the model is totally constructed.<\/p>\n

          Step 5<\/h2>\n

          Apply the colour shown above.<\/p>\n

          Lab Exercise 19-2<\/h1>\n

          Time allowed: 90 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 19-2<\/td>\nInventor Course<\/td>\nMillimeters<\/td>\nMetric – Modules Part (mm).ipt<\/td>\nChrome – Black Polished<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

          Draw the Base sketch on the Right Side view.<\/p>\n

          Step 2<\/h2>\n

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

          Step 3<\/h2>\n

          Note the location of X0Y0Z0. Draw the same model you just drew in Lab Exercise 19-1. In this exercise, REVOLVE the Base sketch and then add sketches and extrude them to complete the model. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. (Figure Step 3A, 3B, 3C, and 3D)<\/p>\n

          \"\"
          Figure Step 3A
          3D Model – Orbited View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 3B
          3D Model – Home View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 3C
          Solid Model – Home View<\/figcaption><\/figure>\n
          \"\"
          Figure Step 3D
          Solid Model – Orbited View<\/figcaption><\/figure>\n
          \"\"
          Author’s Base Sketch<\/figcaption><\/figure>\n
          \"\"
          Author’s Base Model<\/figcaption><\/figure>\n

          Step 4<\/h2>\n

          Create the fillets and chamfers after the model is totally constructed.<\/p>\n

          Step 5<\/h2>\n

          Apply the colour shown above.<\/p>\n

          Lab Exercise 19-3<\/h1>\n

          Time allowed: 90 minutes.<\/p>\n\n\n\n\n
          Part Name<\/strong>: Inventor Lab 19-3<\/td>\nProject<\/strong>: Inventor Course<\/td>\nUnits<\/strong>: Millimeters<\/td>\n<\/tr>\n
          Template<\/strong>: Metric – Modules Part (mm).ipt<\/td>\nColor<\/strong>: Galvanized (texture)<\/td>\nMaterial<\/strong>: N\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

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

          Step 2<\/h2>\n

          Draw the necessary sketches and extrude or revolve them to produce the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. (Figure Step 2A, 2B, 2C, 2D, and 2E)<\/p>\n

          \"\"
          Figure Step 2A
          3D Model – Home View<\/figcaption><\/figure>\n
          \"\"<\/a>
          Figure Step 2B [Click to see image full size]<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2C
          Suggested Base Sketch – Author’s Base Model Top (XY) Plane<\/figcaption><\/figure>\n
          \"\"
          Author’s Base Sketch<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2D
          Solid Model – Home View
          With Work Planes<\/figcaption><\/figure>\n
          \"\"
          Figure Step 2E
          Solid Model – Home View<\/figcaption><\/figure>\n

          Step 3<\/h2>\n

          Create the fillets and chamfers after the model is totally constructed.<\/p>\n

          Step 4<\/h2>\n

          Apply the colour shown above.<\/p>\n","protected":false},"author":1154,"menu_order":3,"template":"","meta":{"pb_show_title":"on","pb_short_title":"","pb_subtitle":"","pb_authors":[],"pb_section_license":""},"chapter-type":[],"contributor":[],"license":[],"class_list":["post-255","chapter","type-chapter","status-publish","hentry"],"part":232,"_links":{"self":[{"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/pressbooks\/v2\/chapters\/255","targetHints":{"allow":["GET"]}}],"collection":[{"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/pressbooks\/v2\/chapters"}],"about":[{"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/wp\/v2\/types\/chapter"}],"author":[{"embeddable":true,"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/wp\/v2\/users\/1154"}],"version-history":[{"count":25,"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/pressbooks\/v2\/chapters\/255\/revisions"}],"predecessor-version":[{"id":2196,"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/pressbooks\/v2\/chapters\/255\/revisions\/2196"}],"part":[{"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/pressbooks\/v2\/parts\/232"}],"metadata":[{"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/pressbooks\/v2\/chapters\/255\/metadata\/"}],"wp:attachment":[{"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/wp\/v2\/media?parent=255"}],"wp:term":[{"taxonomy":"chapter-type","embeddable":true,"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/pressbooks\/v2\/chapter-type?post=255"},{"taxonomy":"contributor","embeddable":true,"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/wp\/v2\/contributor?post=255"},{"taxonomy":"license","embeddable":true,"href":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/wp-json\/wp\/v2\/license?post=255"}],"curies":[{"name":"wp","href":"https:\/\/api.w.org\/{rel}","templated":true}]}}