{"id":242,"date":"2021-05-08T21:19:44","date_gmt":"2021-05-08T21:19:44","guid":{"rendered":"https:\/\/opentextbc.ca\/autodesk\/chapter\/extruding-part-1\/"},"modified":"2021-11-05T17:25:36","modified_gmt":"2021-11-05T17:25:36","slug":"extruding-part-1","status":"publish","type":"chapter","link":"https:\/\/opentextbc.ca\/autodesk\/chapter\/extruding-part-1\/","title":{"raw":"Module 5 Extruding – Part 1","rendered":"Module 5 Extruding – Part 1"},"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 dimensional constraints, linear dimensions, driving and driven dimensions.<\/li>\n \t
  2. Apply the GENERAL DIMENSION command to insert the necessary linear dimensions to fully constrain Base sketches.<\/li>\n \t
  3. Describe and apply the EXTRUDE command to extrude Base sketches to create the 3D Base model.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

    Dimensional Constraints<\/h1>\nUnlike geometrical constraints, that are used to apply geometrical relationships between the objects in the sketch, dimensional constraints <\/em><\/span>control and report the size of the geometry. Dimensional constraints are sometimes called parametric dimensions<\/em><\/span>. To fully constrain a 2D sketch, driving dimensions must be applied. A driving dimension <\/em><\/span>is a parametric dimension controlling the size of the object. Inventor will automatically change the overall model to conform to the driving dimensions maintaining the existing geometrical constraints that were assigned in the sketch. Objects of the sketch that are not dimensioned will change to adapt when a driving dimension is applied or an existing driving dimension is changed.\n\nAdd only the number of driving dimensions that are required to ensure that the model maintains the desired size and shape. Inventor will issue a warning when a dimension is added that over-constrains the sketch. Only driven dimensions will be allowed to be added to a fully constrained sketch.\n\nA driven dimension <\/em><\/span>is a non-parametric dimension that does not constrain the object. It only displays the current value of the geometry that it is applied to. Driven dimensions are automatically enclosed in parentheses to distinguish them from driving dimensions. You can add as many driven dimensions to the sketch as you wish.\n

    Base Model<\/h2>\nAfter the Base sketch is complete and is fully constrained, it is ready to be extruded or revolved to create the base model. The Base model <\/em><\/span>is the solid model created from the base sketch by extruding or revolving it. In this module, only extruding the Base sketch to create the Base model is taught. The simplest definition of an extrusion is it adds depth to the Base sketch to create the Base model. See Figure 5-1.\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"133\"]\"\" The Base Sketch[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"278\"]\"\" The Extrusion[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"286\"]\"\" The Base Model
    Figure 5-1[\/caption]\n\n
    \n

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

    \n\nThe EXTRUDE command is used to extrude a 2D sketch to create or edit a 3D solid model.\n\nShortcut: E<\/strong>\n\n\"\"\n\n<\/div>\n<\/div>\n

    Dimensioning Sketches<\/h2>\nThere are many different types of dimensions available to the operator to dimension sketches. The different dimensioning types will be taught throughout the Inventor book. In this module, inserting object linear dimensions is taught.\n

    Linear Dimensions<\/h2>\nA linear<\/span> <\/em>dimension is a dimension measuring the delta X <\/em><\/span>or the delta Y <\/em><\/span>distance between the two XY locations or endpoints of a line. See Figure 5-2. Linear dimensions are always either horizontal (delta X) or vertical (delta Y). A linear dimension cannot be used to dimension the true length of an inclined line. It will only dimension the true length of a line if the line is horizontal or vertical. If both endpoints of a line lie on the same axis, it can only be dimensioned in one delta direction. Since all lines that were drawn to this point in the book were either horizontal or vertical, linear dimensions will be used for all of the dimensions inserted in this module.\n\n \n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"321\"]\"\" Fig 5-2
    Linear Dimensions Applied to
    Horizontal and Vertical Lines[\/caption]\n

    Object Linear Dimensions<\/h2>\nTo insert an object linear dimension<\/em><\/span>, enter the GENERAL DIMENSION command and move the cursor onto the line to be dimensioned. When the two headed arrow icon appears, click the left mouse button to select the line as shown in Figure 5-3. After selecting the line, move the cursor in the direction to select the location of the dimension. Click the mouse at the desired location of the dimension.\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"211\"]\"\" Figure 5-3 Object Linear Dimension Icon[\/caption]\n\n
    \n

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

    \n\nThe GENERAL DIMENSION command is used to create driving or driven dimensions on a sketch.\n\nShortcut: D<\/strong>\n\n\"\"\n\n<\/div>\n<\/div>\n

    WORK ALONG:\u00a0Dimensioning and Extruding the Base Sketch<\/h1>\n

    Step 1<\/h2>\nUsing the OPEN command, open the part file: Inventor Workalong 04-1<\/span> that you completed in Module 4.\n

    Step 2<\/h2>\nChange to Sketch mode by editing Sketch1 in the Browser bar. Press F6 to change the view to the Home view. (Figure Step 2)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 2[\/caption]\n\n
    \n\nAUTHOR'S COMMENTS:<\/strong> Two lines of the sketch should appear purple and the remainder blue. The purple lines are constrained while the blue ones are not. The reason the two lines are constrained is because they have one endpoint snapped to the Center Point (X0Y0), which is constrained (projected) to the sketching plane. In this workalong, you will be adding dimensional constrains to fully constrain the sketch.\n\n\"\"\n\n<\/div>\n

    Step 3<\/h2>\nEnter the LOOK AT command and when prompted, select one of the lines on the sketch as shown in the figure. (Figure Step 3A and 3B)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"295\"]\"\" Figure Step 3A[\/caption]\n\n
    AUTHOR'S COMMENTS:<\/strong> For the beginner, it is sometimes easier to dimension the sketch while it is in a 2D view. While this step is not necessary, I used it here to show you different methods of working on the sketch.<\/div>\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 3B[\/caption]\n

    Step 4<\/h2>\nEnter the GENERAL DIMENSION command by pressing D on the keyboard. Move the cursor onto the left vertical line. When the Two Headed Arrow icon appears, select the line by clicking the left mouse button. (Figure Step 4)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"347\"]\"\" Figure Step 4[\/caption]\n\n
    AUTHOR'S COMMENTS:<\/strong> It is best to dimension starting at lines that snapped to the Center Point (X0Y0). Create dimensioned in both directions moving around the sketch until the sketch is fully constrained.<\/div>\n

    Step 5<\/h2>\nMove the cursor to the left and drag the dimension. Inventor will measure the delta Y length of the line, since it is a vertical line, and display its actual length. In this case, it is 6.0 inches long. Since that is the desired length, accept it by clicking the green Check icon. (Figure Step 5)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"570\"]\"\" Figure Step 5[\/caption]\n

    Step 6<\/h2>\nContinue to add linear dimensions to fully constrain your sketch. If the length of the lines are correct, accept the dimension. If they are incorrect, change the dimension in the edit box to the actual dimension of the line and then accept it by clicking the green Check icon. (Figure Step 6A, 6B, 6C, and 6D)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"368\"]\"\" Figure Step 6A[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"427\"]\"\" Figure Step 6B[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"418\"]\"\" Figure Step 6C[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"420\"]\"\" Figure Step 6D[\/caption]\n

    Step 7<\/h2>\nWhen complete, there should be six driving dimensions. (Figure Step 7)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"522\"]\"\" Figure Step 7[\/caption]\n

    Step 8<\/h2>\nAdd one more dimension as shown in the figure. Note that Inventor will issue a warning that the dimension over-constrains the sketch. Click the Accept button to add it as a driven dimension. (Figure Step 8A and 8B)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"212\"]\"\" Figure Step 8A[\/caption]\n\n
    AUTHOR'S COMMENTS:<\/strong> This step is not necessary to fully constrain the sketch. Driven dimensions are added for reference only.<\/div>\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 8B[\/caption]\n

    Step 9<\/h2>\nWithout entering a command, move the cursor onto the 2.000 dimension as shown in the figure. When the Move icon displays, click and hold the mouse button down and drag the dimension to the new location shown in the figure. (Figure Step 9A and 9B)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"365\"]\"\" Figure Step 9A[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"467\"]\"\" Figure Step 9B[\/caption]\n\n
    AUTHOR'S COMMENTS: <\/strong>I use the Move icon to centre the numbers in the dimensions after I complete the sketch. This is not a necessary step but makes the sketch appear more professional.<\/div>\n
    \n\nUSER TIP: <\/strong>Instead of clicking the green Check icon to accept the displayed dimension in the Edit Dimension dialogue box it is faster to press the Enter key.\n\n\"\"\n\n<\/div>\n

    Step 10<\/h2>\nThe completed sketch should appear as shown in the figures. (Figure Step 10A, 10B, and 10C)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"475\"]\"\" Figure Step 10A[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"363\"]\"\" Figure Step 10B[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"189\"]\"\" Figure Step 10C[\/caption]\n\n
    AUTHOR'S COMMENTS:<\/strong> All of the lines in your sketch should appear purple and the Status bar should display Fully Constrained as shown in Figure Step 10C.<\/div>\n

    Step 11<\/h2>\nPress F6 to change to the Home view. (Figure Step 11)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"568\"]\"\" Figure Step 11[\/caption]\n

    Step 12<\/h2>\nClick the LOOK AT command and change the view to the top or XY plane.\n

    Step 13<\/h2>\nPress F8 to display the geometrical constraint icons. You figure should appears similar as shown in the figure. (Figure Step 13)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"561\"]\"\" Figure Step 13[\/caption]\n\n
    AUTHOR'S COMMENTS:<\/strong> Your geometrical constrains may not match the figure exactly. Just ensure that the sketch is fully constrained.<\/div>\n

    Step 14<\/h2>\nEnter the EXTRUDE command. The Extrude dialogue box will display. The model being drawn is 5 inches high as shown in the figure. Set the Output box to Solid, the Extents to Distance of 5 and the Extrude Direction to positive Z as shown in the figures. (Figure Step 14A and 14B)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 14A[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 14B [Click to see image full size][\/caption]\n
    AUTHOR'S COMMENTS: <\/strong>Note that Inventor will, by default, attempt to extrude in the positive Z direction. This extrude direction can be reversed, when required.<\/div>\n

    Step 15<\/h2>\nThe completed solid model should now appear as shown in the figure. (Figure Step 15)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"320\"]\"\" Figure Step 15[\/caption]\n

    Step 16<\/h2>\nFind the Appearance pull-down menu and select the arrow to pull down the Color list. Ensure that the library: Inventor Material Library<\/span> is enabled at the bottom of the list. (Figure Step 16A and 16B)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 16A[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"305\"]\"\" Figure Step 16B[\/caption]\n

    Step 17<\/h2>\nIn the Appearance pull-down menu, select the color: Aluminum Polished<\/span> as shown in the figure. (Figure Step 17)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"279\"]\"\" Figure Step 17[\/caption]\n\n
    AUTHOR'S COMMENTS: <\/strong><\/strong>Ensure that you use the Appearance pull-down list and not the Material pull-down Figure Step 17<\/strong> list to the left of the Appearance pull-down list. The Material pull-down list will be covered in Module 20.<\/div>\n
    AUTHOR'S COMMENTS: <\/strong><\/strong>If your Inventor software does not include Inventor Material Library, you can use either the Autodesk Material Library or the Autodesk Appearance Library to set the colors specified in the book.<\/div>\n

    Step 18<\/h2>\nThe completed part or model should appear as shown in the figure. (Figure Step 18)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"304\"]\"\" Figure Step 18[\/caption]\n\n
    AUTHOR'S COMMENTS:\u00a0<\/strong>The colour only changes the model to appear as the assigned colour. It does not specify the material that the solid model is made from. That will be taught in Module 20.<\/div>\n

    Step 19<\/h2>\nSave and close the part file.\n
    \n\nMUST KNOW: <\/strong>A driving dimension is a parametric dimension controlling the size of the object. Inventor will automatically change the overall sketch to conform to the driving dimensions maintaining the existing geometrical constraints that were used in the design.\n\n[caption id=\"attachment_225\" align=\"aligncenter\" width=\"320\"]\"\" Driving Dimension[\/caption]\n\nA driving dimension is shown below. A driven dimension is a non-parametric dimension that does not constrain the object. It is inserted for reference only and is always displayed enclosed in brackets as shown below.\n\n[caption id=\"attachment_225\" align=\"aligncenter\" width=\"315\"]\"\" Driven Dimension[\/caption]\n\n<\/div>\n
    \n\nUSER TIP: <\/strong>When you open the Extrude dialogue box for the first time, the Marking menu will display on top of the extruded model. You will not be using that menu in the Inventor book.\n\n[caption id=\"attachment_614\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> [Click to see image full size][\/caption]<\/div>\n
    \n\nUSER TIP: <\/strong>Click the bottom right arrow and enable Pin Mini-Toolbar Position and Auto Fade.\n\n\"\"\n\nDrag the Marking menu to bottom right corner of the Graphic window. It will remain there for the duration while you working on the Inventor book. After you complete the book, you can use change the settings to use the menu any way the works for you.\n\n[caption id=\"attachment_227\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> [Click to see image full size][\/caption]<\/div>\n
    \n\nMUST KNOW: <\/strong>Knowing When the Sketch is Fully Constrained<\/strong><\/span> It is very important to know when a sketch is fully constrained. A fully constrained sketch is complete and is ready to be extruded or revolved to create or edit the solid model. When the colour scheme is set to High Contrast, the background is black and the lines that are constrained will display purple. The lines that are not yet constrained will display blue. When the sketch is fully constrained, all of the lines in the sketch will display purple. Inventor also reports the current constraint status on the Status bar. See the figures below.\n\n[caption id=\"attachment_231\" align=\"aligncenter\" width=\"400\"]\"\" Sketch Partially Constrained[\/caption]\n\n[caption id=\"attachment_231\" align=\"aligncenter\" width=\"400\"]\"\" Sketch Fully Constrained[\/caption]\n\nA special Pinned icon will display in Browser bar on sketches that are fully constrained as shown to the figures.\n\n\"\"\n\n<\/div>\n

    Key Principles<\/h1>\n
    \n

    Key Principles in Module 5<\/p>\n\n<\/header>\n

    \n
      \n \t
    1. Unlike geometrical constraints, that are used to apply geometrical relationships of the objects in a 2D sketch, dimensional constraints control and report the size of the geometry.<\/li>\n \t
    2. To fully constrain a 2D sketch, driving dimensions must be applied. A driving dimension is a parametric dimension controlling the size of the object. Inventor will automatically change the overall object to conform to the driving dimensions maintaining the existing geometrical constraints that were assigned in the sketch.<\/li>\n \t
    3. A driven dimension is a non-parametric dimension that does not constrain the sketch.<\/li>\n \t
    4. It is very important to know when the sketch is fully When it is fully constrained, the sketch is complete and it is ready to be extruded or revolved to create the Base model. When the background colour scheme is set to High Contrast the constrained lines will display purple and lines that are not yet constrained will display blue. When the sketch is fully constrained, all of the lines in the sketch will display purple.<\/li>\n \t
    5. After the Base sketch is complete and is fully constrained, it is ready to be extruded to create the Base model. The Base model is the solid model created from the Base sketch.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

      Lab Exercise 5-1<\/h1>\nTime allowed: 40 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 04-1<\/td>\nInventor Course<\/td>\nInches<\/td>\nEnglish-Modules Part (in).ipt<\/td>\n\u00a0Zinc Chromate 2<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

      Step 1<\/h2>\nOpen the file: Inventor Lab 04-1.ipt<\/span> that you saved in Lab Exercise 4-1 in Module 4.\n

      Step 2<\/h2>\nUsing the SAVEAS command, save the file with the name: Inventor Lab 05-1.ipt<\/span>.\n

      Step 3<\/h2>\nInsert the necessary driving dimensions to fully constrain the sketch. Add at least one driven dimension. (Figure Step 3A, 3B, and 3C)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 3A
      3D Model[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 3B
      Base Sketch Dimensioned[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 3C
      The Base Sketch Fully Constrained [Click to see image full size][\/caption]\n

      Step 4<\/h2>\nExtrude the sketch to create the Base model and apply the colour shown above. (Figure Step 4)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 4
      Completed
      3D Solid Model
      Home View[\/caption]\n\n
      AUTHOR'S GEOMETRIC CONSTRAINTS: <\/strong>The following figure shows the Base 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 used with the authors.[caption id=\"attachment_627\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> [Click to see image full size][\/caption]<\/div>\n

      Lab Exercise 5-2<\/h1>\nTime allowed: 40 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 04-2<\/td>\nInventor Course<\/td>\nInches<\/td>\nN\/A<\/td>\nChrome - Polished Blue<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

      Step 1<\/h2>\nOpen the file: Inventor Lab 04-2.ipt<\/span> that you saved in Lab Exercise 4-2 in Module 4.\n

      Step 2<\/h2>\nUsing the SAVEAS command, save the file with the name: Inventor Lab 05-2.ipt<\/span>.\n

      Step 3<\/h2>\nInsert the necessary driving dimensions to fully constrain the sketch and add at least two driven dimensions. (Figure Step 3A, 3B, and 3C)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 3A
      3D Mode[\/caption]\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 3B
      Base Sketch Dimensioned [Click to see image full size][\/caption][caption id=\"attachment_240\" align=\"aligncenter\" width=\"500\"]      \"\"<\/a> Figure Step 3C
      Base Sketch Fully Constrained [Click to see image full size][\/caption]\n

      Step 4<\/h2>\nExtrude the sketch to create the Base model and apply the colour shown above. (Figure Step 4)\n\n[caption id=\"attachment_240\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 4
      Completed 3D Solid Model
      Home View[\/caption]\n\n
      \n\nAUTHOR'S GEOMETRIC CONSTRAINS: <\/strong>The following figure shows the Base 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 used with the authors.\n\n[caption id=\"attachment_637\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> [Click to see image full size][\/caption]<\/div>","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 dimensional constraints, linear dimensions, driving and driven dimensions.<\/li>\n
      2. Apply the GENERAL DIMENSION command to insert the necessary linear dimensions to fully constrain Base sketches.<\/li>\n
      3. Describe and apply the EXTRUDE command to extrude Base sketches to create the 3D Base model.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

        Dimensional Constraints<\/h1>\n

        Unlike geometrical constraints, that are used to apply geometrical relationships between the objects in the sketch, dimensional constraints <\/em><\/span>control and report the size of the geometry. Dimensional constraints are sometimes called parametric dimensions<\/em><\/span>. To fully constrain a 2D sketch, driving dimensions must be applied. A driving dimension <\/em><\/span>is a parametric dimension controlling the size of the object. Inventor will automatically change the overall model to conform to the driving dimensions maintaining the existing geometrical constraints that were assigned in the sketch. Objects of the sketch that are not dimensioned will change to adapt when a driving dimension is applied or an existing driving dimension is changed.<\/p>\n

        Add only the number of driving dimensions that are required to ensure that the model maintains the desired size and shape. Inventor will issue a warning when a dimension is added that over-constrains the sketch. Only driven dimensions will be allowed to be added to a fully constrained sketch.<\/p>\n

        A driven dimension <\/em><\/span>is a non-parametric dimension that does not constrain the object. It only displays the current value of the geometry that it is applied to. Driven dimensions are automatically enclosed in parentheses to distinguish them from driving dimensions. You can add as many driven dimensions to the sketch as you wish.<\/p>\n

        Base Model<\/h2>\n

        After the Base sketch is complete and is fully constrained, it is ready to be extruded or revolved to create the base model. The Base model <\/em><\/span>is the solid model created from the base sketch by extruding or revolving it. In this module, only extruding the Base sketch to create the Base model is taught. The simplest definition of an extrusion is it adds depth to the Base sketch to create the Base model. See Figure 5-1.<\/p>\n

        \"\"
        The Base Sketch<\/figcaption><\/figure>\n
        \"\"
        The Extrusion<\/figcaption><\/figure>\n
        \"\"
        The Base Model
        Figure 5-1<\/figcaption><\/figure>\n
        \n
        \n

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

        \n

        The EXTRUDE command is used to extrude a 2D sketch to create or edit a 3D solid model.<\/p>\n

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

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

        Dimensioning Sketches<\/h2>\n

        There are many different types of dimensions available to the operator to dimension sketches. The different dimensioning types will be taught throughout the Inventor book. In this module, inserting object linear dimensions is taught.<\/p>\n

        Linear Dimensions<\/h2>\n

        A linear<\/span> <\/em>dimension is a dimension measuring the delta X <\/em><\/span>or the delta Y <\/em><\/span>distance between the two XY locations or endpoints of a line. See Figure 5-2. Linear dimensions are always either horizontal (delta X) or vertical (delta Y). A linear dimension cannot be used to dimension the true length of an inclined line. It will only dimension the true length of a line if the line is horizontal or vertical. If both endpoints of a line lie on the same axis, it can only be dimensioned in one delta direction. Since all lines that were drawn to this point in the book were either horizontal or vertical, linear dimensions will be used for all of the dimensions inserted in this module.<\/p>\n

         <\/p>\n

        \"\"
        Fig 5-2
        Linear Dimensions Applied to
        Horizontal and Vertical Lines<\/figcaption><\/figure>\n

        Object Linear Dimensions<\/h2>\n

        To insert an object linear dimension<\/em><\/span>, enter the GENERAL DIMENSION command and move the cursor onto the line to be dimensioned. When the two headed arrow icon appears, click the left mouse button to select the line as shown in Figure 5-3. After selecting the line, move the cursor in the direction to select the location of the dimension. Click the mouse at the desired location of the dimension.<\/p>\n

        \"\"
        Figure 5-3 Object Linear Dimension Icon<\/figcaption><\/figure>\n
        \n
        \n

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

        \n

        The GENERAL DIMENSION command is used to create driving or driven dimensions on a sketch.<\/p>\n

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

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

        WORK ALONG:\u00a0Dimensioning and Extruding the Base Sketch<\/h1>\n

        Step 1<\/h2>\n

        Using the OPEN command, open the part file: Inventor Workalong 04-1<\/span> that you completed in Module 4.<\/p>\n

        Step 2<\/h2>\n

        Change to Sketch mode by editing Sketch1 in the Browser bar. Press F6 to change the view to the Home view. (Figure Step 2)<\/p>\n

        \"\"
        Figure Step 2<\/figcaption><\/figure>\n
        \n

        AUTHOR’S COMMENTS:<\/strong> Two lines of the sketch should appear purple and the remainder blue. The purple lines are constrained while the blue ones are not. The reason the two lines are constrained is because they have one endpoint snapped to the Center Point (X0Y0), which is constrained (projected) to the sketching plane. In this workalong, you will be adding dimensional constrains to fully constrain the sketch.<\/p>\n

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

        Step 3<\/h2>\n

        Enter the LOOK AT command and when prompted, select one of the lines on the sketch as shown in the figure. (Figure Step 3A and 3B)<\/p>\n

        \"\"
        Figure Step 3A<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:<\/strong> For the beginner, it is sometimes easier to dimension the sketch while it is in a 2D view. While this step is not necessary, I used it here to show you different methods of working on the sketch.<\/div>\n
        \"\"
        Figure Step 3B<\/figcaption><\/figure>\n

        Step 4<\/h2>\n

        Enter the GENERAL DIMENSION command by pressing D on the keyboard. Move the cursor onto the left vertical line. When the Two Headed Arrow icon appears, select the line by clicking the left mouse button. (Figure Step 4)<\/p>\n

        \"\"
        Figure Step 4<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:<\/strong> It is best to dimension starting at lines that snapped to the Center Point (X0Y0). Create dimensioned in both directions moving around the sketch until the sketch is fully constrained.<\/div>\n

        Step 5<\/h2>\n

        Move the cursor to the left and drag the dimension. Inventor will measure the delta Y length of the line, since it is a vertical line, and display its actual length. In this case, it is 6.0 inches long. Since that is the desired length, accept it by clicking the green Check icon. (Figure Step 5)<\/p>\n

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

        Step 6<\/h2>\n

        Continue to add linear dimensions to fully constrain your sketch. If the length of the lines are correct, accept the dimension. If they are incorrect, change the dimension in the edit box to the actual dimension of the line and then accept it by clicking the green Check icon. (Figure Step 6A, 6B, 6C, and 6D)<\/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

        Step 7<\/h2>\n

        When complete, there should be six driving dimensions. (Figure Step 7)<\/p>\n

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

        Step 8<\/h2>\n

        Add one more dimension as shown in the figure. Note that Inventor will issue a warning that the dimension over-constrains the sketch. Click the Accept button to add it as a driven dimension. (Figure Step 8A and 8B)<\/p>\n

        \"\"
        Figure Step 8A<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:<\/strong> This step is not necessary to fully constrain the sketch. Driven dimensions are added for reference only.<\/div>\n
        \"\"
        Figure Step 8B<\/figcaption><\/figure>\n

        Step 9<\/h2>\n

        Without entering a command, move the cursor onto the 2.000 dimension as shown in the figure. When the Move icon displays, click and hold the mouse button down and drag the dimension to the new location shown in the figure. (Figure Step 9A and 9B)<\/p>\n

        \"\"
        Figure Step 9A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 9B<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong>I use the Move icon to centre the numbers in the dimensions after I complete the sketch. This is not a necessary step but makes the sketch appear more professional.<\/div>\n
        \n

        USER TIP: <\/strong>Instead of clicking the green Check icon to accept the displayed dimension in the Edit Dimension dialogue box it is faster to press the Enter key.<\/p>\n

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

        Step 10<\/h2>\n

        The completed sketch should appear as shown in the figures. (Figure Step 10A, 10B, and 10C)<\/p>\n

        \"\"
        Figure Step 10A<\/figcaption><\/figure>\n
        \"\"
        Figure Step 10B<\/figcaption><\/figure>\n
        \"\"
        Figure Step 10C<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:<\/strong> All of the lines in your sketch should appear purple and the Status bar should display Fully Constrained as shown in Figure Step 10C.<\/div>\n

        Step 11<\/h2>\n

        Press F6 to change to the Home view. (Figure Step 11)<\/p>\n

        \"\"
        Figure Step 11<\/figcaption><\/figure>\n

        Step 12<\/h2>\n

        Click the LOOK AT command and change the view to the top or XY plane.<\/p>\n

        Step 13<\/h2>\n

        Press F8 to display the geometrical constraint icons. You figure should appears similar as shown in the figure. (Figure Step 13)<\/p>\n

        \"\"
        Figure Step 13<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:<\/strong> Your geometrical constrains may not match the figure exactly. Just ensure that the sketch is fully constrained.<\/div>\n

        Step 14<\/h2>\n

        Enter the EXTRUDE command. The Extrude dialogue box will display. The model being drawn is 5 inches high as shown in the figure. Set the Output box to Solid, the Extents to Distance of 5 and the Extrude Direction to positive Z as shown in the figures. (Figure Step 14A and 14B)<\/p>\n

        \"\"
        Figure Step 14A<\/figcaption><\/figure>\n
        \"\"<\/a>
        Figure Step 14B [Click to see image full size]<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong>Note that Inventor will, by default, attempt to extrude in the positive Z direction. This extrude direction can be reversed, when required.<\/div>\n

        Step 15<\/h2>\n

        The completed solid model should now appear as shown in the figure. (Figure Step 15)<\/p>\n

        \"\"
        Figure Step 15<\/figcaption><\/figure>\n

        Step 16<\/h2>\n

        Find the Appearance pull-down menu and select the arrow to pull down the Color list. Ensure that the library: Inventor Material Library<\/span> is enabled at the bottom of the list. (Figure Step 16A and 16B)<\/p>\n

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

        Step 17<\/h2>\n

        In the Appearance pull-down menu, select the color: Aluminum Polished<\/span> as shown in the figure. (Figure Step 17)<\/p>\n

        \"\"
        Figure Step 17<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS: <\/strong><\/strong>Ensure that you use the Appearance pull-down list and not the Material pull-down Figure Step 17<\/strong> list to the left of the Appearance pull-down list. The Material pull-down list will be covered in Module 20.<\/div>\n
        AUTHOR’S COMMENTS: <\/strong><\/strong>If your Inventor software does not include Inventor Material Library, you can use either the Autodesk Material Library or the Autodesk Appearance Library to set the colors specified in the book.<\/div>\n

        Step 18<\/h2>\n

        The completed part or model should appear as shown in the figure. (Figure Step 18)<\/p>\n

        \"\"
        Figure Step 18<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:\u00a0<\/strong>The colour only changes the model to appear as the assigned colour. It does not specify the material that the solid model is made from. That will be taught in Module 20.<\/div>\n

        Step 19<\/h2>\n

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

        \n

        MUST KNOW: <\/strong>A driving dimension is a parametric dimension controlling the size of the object. Inventor will automatically change the overall sketch to conform to the driving dimensions maintaining the existing geometrical constraints that were used in the design.<\/p>\n

        \"\"
        Driving Dimension<\/figcaption><\/figure>\n

        A driving dimension is shown below. A driven dimension is a non-parametric dimension that does not constrain the object. It is inserted for reference only and is always displayed enclosed in brackets as shown below.<\/p>\n

        \"\"
        Driven Dimension<\/figcaption><\/figure>\n<\/div>\n
        \n

        USER TIP: <\/strong>When you open the Extrude dialogue box for the first time, the Marking menu will display on top of the extruded model. You will not be using that menu in the Inventor book.<\/p>\n

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

        USER TIP: <\/strong>Click the bottom right arrow and enable Pin Mini-Toolbar Position and Auto Fade.<\/p>\n

        \"\"<\/p>\n

        Drag the Marking menu to bottom right corner of the Graphic window. It will remain there for the duration while you working on the Inventor book. After you complete the book, you can use change the settings to use the menu any way the works for you.<\/p>\n

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

        MUST KNOW: <\/strong>Knowing When the Sketch is Fully Constrained<\/strong><\/span> It is very important to know when a sketch is fully constrained. A fully constrained sketch is complete and is ready to be extruded or revolved to create or edit the solid model. When the colour scheme is set to High Contrast, the background is black and the lines that are constrained will display purple. The lines that are not yet constrained will display blue. When the sketch is fully constrained, all of the lines in the sketch will display purple. Inventor also reports the current constraint status on the Status bar. See the figures below.<\/p>\n

        \"\"
        Sketch Partially Constrained<\/figcaption><\/figure>\n
        \"\"
        Sketch Fully Constrained<\/figcaption><\/figure>\n

        A special Pinned icon will display in Browser bar on sketches that are fully constrained as shown to the figures.<\/p>\n

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

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

        Key Principles in Module 5<\/p>\n<\/header>\n

        \n
          \n
        1. Unlike geometrical constraints, that are used to apply geometrical relationships of the objects in a 2D sketch, dimensional constraints control and report the size of the geometry.<\/li>\n
        2. To fully constrain a 2D sketch, driving dimensions must be applied. A driving dimension is a parametric dimension controlling the size of the object. Inventor will automatically change the overall object to conform to the driving dimensions maintaining the existing geometrical constraints that were assigned in the sketch.<\/li>\n
        3. A driven dimension is a non-parametric dimension that does not constrain the sketch.<\/li>\n
        4. It is very important to know when the sketch is fully When it is fully constrained, the sketch is complete and it is ready to be extruded or revolved to create the Base model. When the background colour scheme is set to High Contrast the constrained lines will display purple and lines that are not yet constrained will display blue. When the sketch is fully constrained, all of the lines in the sketch will display purple.<\/li>\n
        5. After the Base sketch is complete and is fully constrained, it is ready to be extruded to create the Base model. The Base model is the solid model created from the Base sketch.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

          Lab Exercise 5-1<\/h1>\n

          Time allowed: 40 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 04-1<\/td>\nInventor Course<\/td>\nInches<\/td>\nEnglish-Modules Part (in).ipt<\/td>\n\u00a0Zinc Chromate 2<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

          Open the file: Inventor Lab 04-1.ipt<\/span> that you saved in Lab Exercise 4-1 in Module 4.<\/p>\n

          Step 2<\/h2>\n

          Using the SAVEAS command, save the file with the name: Inventor Lab 05-1.ipt<\/span>.<\/p>\n

          Step 3<\/h2>\n

          Insert the necessary driving dimensions to fully constrain the sketch. Add at least one driven dimension. (Figure Step 3A, 3B, and 3C)<\/p>\n

          \"\"
          Figure Step 3A
          3D Model<\/figcaption><\/figure>\n
          \"\"
          Figure Step 3B
          Base Sketch Dimensioned<\/figcaption><\/figure>\n
          \"\"<\/a>
          Figure Step 3C
          The Base Sketch Fully Constrained [Click to see image full size]<\/figcaption><\/figure>\n

          Step 4<\/h2>\n

          Extrude the sketch to create the Base model and apply the colour shown above. (Figure Step 4)<\/p>\n

          \"\"
          Figure Step 4
          Completed
          3D Solid Model
          Home View<\/figcaption><\/figure>\n
          AUTHOR’S GEOMETRIC CONSTRAINTS: <\/strong>The following figure shows the Base 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 used with the authors.<\/p>\n
          \"\"<\/a>
          [Click to see image full size]<\/figcaption><\/figure>\n<\/div>\n

          Lab Exercise 5-2<\/h1>\n

          Time allowed: 40 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 04-2<\/td>\nInventor Course<\/td>\nInches<\/td>\nN\/A<\/td>\nChrome – Polished Blue<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

          Open the file: Inventor Lab 04-2.ipt<\/span> that you saved in Lab Exercise 4-2 in Module 4.<\/p>\n

          Step 2<\/h2>\n

          Using the SAVEAS command, save the file with the name: Inventor Lab 05-2.ipt<\/span>.<\/p>\n

          Step 3<\/h2>\n

          Insert the necessary driving dimensions to fully constrain the sketch and add at least two driven dimensions. (Figure Step 3A, 3B, and 3C)<\/p>\n

          \"\"
          Figure Step 3A
          3D Mode<\/figcaption><\/figure>\n
          \"\"<\/a>
          Figure Step 3B
          Base Sketch Dimensioned [Click to see image full size]<\/figcaption><\/figure>\n
          \"\"<\/a>
          Figure Step 3C
          Base Sketch Fully Constrained [Click to see image full size]<\/figcaption><\/figure>\n

          Step 4<\/h2>\n

          Extrude the sketch to create the Base model and apply the colour shown above. (Figure Step 4)<\/p>\n

          \"\"
          Figure Step 4
          Completed 3D Solid Model
          Home View<\/figcaption><\/figure>\n
          \n

          AUTHOR’S GEOMETRIC CONSTRAINS: <\/strong>The following figure shows the Base 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 used with the authors.<\/p>\n

          \"\"<\/a>
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