{"id":323,"date":"2021-05-18T14:16:31","date_gmt":"2021-05-18T18:16:31","guid":{"rendered":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/?post_type=chapter&p=323"},"modified":"2021-07-13T14:49:34","modified_gmt":"2021-07-13T18:49:34","slug":"2d-drawings-part-1","status":"publish","type":"chapter","link":"https:\/\/pressbooks.bccampus.ca\/autodeskinventor\/chapter\/2d-drawings-part-1\/","title":{"raw":"Module 24 2D Drawings - Part 1","rendered":"Module 24 2D Drawings – Part 1"},"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 2D drawing files, drawing sheets, and drawing sizes.<\/li>\r\n \t
  2. Describe and apply the commands BASE VIEW, PROJECTED VIEW, SECTION VIEW, and NEW SHEET to create multiview and isometric views of a solid model on a drawing sheet.<\/li>\r\n<\/ol>\r\n<\/div>\r\n<\/div>\r\n

    Drawing Files<\/h1>\r\nA drawing file<\/em><\/span> contains one or more drawing sheets on which 2 dimensional and\/or 3 dimensional scaled views of the solid models contained in part, assembly, or presentation files. The views can be created complete with hidden lines or shading. Annotation can be automatically or manually added to the views as required. A typical drawing sheet with an orthographic, section, and isometric view of a model is shown in Figure 24-1. Dimensioning, inserting text, and filling in the titleblock are taught in Module 25. When the drawing is complete, it can be printed or plotted on paper. A drawing file has the file extension .idw. IDW is an acronym for Inventor Drawing.\r\n\r\n[caption id=\"attachment_1773\" align=\"aligncenter\" width=\"615\"]\"\"<\/a> Figure 24-1
    A Typical Drawing Sheet in a Drawing File [Click to see image full size][\/caption]\r\n

    Model Views<\/h2>\r\nA model view<\/em><\/span> is a scaled view orientated at an angle and direction that the solid model or assembly is being viewed and displayed on the drawing sheet. There is no limit to the number of views or the number of solid models from part, assembly, or presentation files that can be placed on a drawing sheet. Views can also be automatically annotated or labeled. There are eight predefined views that you can select from when creating the view. The predefined views are the; base, projection, auxiliary, section, detail, broken, breakout, and overlay.\r\n

    The Base<\/h2>\r\nA Base view<\/span><\/em> is the first view created on the drawing sheet. It controls the scale, orientation, and location of the views projected from it. The orthographic and\/or isometric views in the drawing are created from the Base view. For example, if a multiview drawing was being created from a solid model, the Front view is created first as a Base view. The Front view would control the scale and location of the projected Top and Right Side views. See Figure 24-2. To change the scale of all views, only the scale of the Front (Base) view would have to be changed and the Top and Right Side views would automatically change scale to match. If the Front view was moved, the Top and Right Side views would move accordingly to keep their multiview position.\r\n\r\n[caption id=\"attachment_1774\" align=\"aligncenter\" width=\"421\"]\"\" Figure 24-2
    Multiview Drawing[\/caption]\r\n

    Projected Views<\/h2>\r\nA projected view<\/span><\/em> is a view projected from a Base view. The scale of a projected view cannot be set since the Base view that you projected it from controls its scale. The Base view also controls the orientation and location of the projected views.\r\n

    Drawing Sheets<\/h2>\r\nA drawing sheet<\/span><\/em> represents a blank piece of paper complete with titleblock and border. The size of drawing sheet can be set by the user. The sheet size can be a custom size set by you or one of the ANSI or ISO drawing sheet standards listed in the table shown in Figure 24-3.\r\n\r\nThere is no maximum number of drawing sheets that can be created for each drawing file but there must be at least one sheet. Sheets can be created or deleted but Inventor will NOT allow all of them to be deleted since one sheet must exist at all times.\r\n\r\nThe drawing sheet can be assigned a drawing border and a titleblock which can be created or edited by you. Custom drawing template files containing borders and titleblocks are supplied with the Inventor book.\r\n
    MUST KNOW:<\/strong> There is no maximum number of drawing sheets that can be created for each drawing file but there must be at least one sheet. One sheet must exist in each drawing file at all times.<\/div>\r\n

    ANSI and ISO Standard Drawing Sheet Sizes<\/h2>\r\n[caption id=\"attachment_2136\" align=\"aligncenter\" width=\"1292\"]\"\" Figure 24-3
    Standard ANSI and ISO Drawing Sheet Sizes[\/caption]\r\n

    View Style<\/h2>\r\nA view style<\/span><\/em> can be displayed in one of three different styles. The three styles are hidden line<\/em><\/span>, hidden line removed<\/em><\/span>, and shaded<\/span> <\/em>as shown in Figure 24-4. The style of a view can be changed as required after the view has been placed.\r\n

    View Scale<\/h2>\r\nThe scale<\/em> <\/span>of the view is a factor of the number that it is set to. For example, if the scale is set to 1 then the factor of 1 X 1 = 1, full scale or 1:1. If the scale is set to 2 then 2 X 1 = 2 or a scale of 2:1 which is twice the size of the original model. On the other hand, if the scale factor is set to 0.5 then 0.5 X 1 = 0.5 or the scale of 1:2 which would display the view one-half the size of the original model.\r\n\r\n[caption id=\"attachment_1777\" align=\"aligncenter\" width=\"496\"]\"\" Figure 24-3
    View Styles[\/caption]\r\n\r\n
    MUST KNOW:<\/strong> A drawing file contains one or more 2 dimensional drawing sheets on which a 2D and\/or 3D scaled views of solid models contained in part, assembly, and presentation files. A drawing file has the file extension .idw. IDW is an acronym for Inventor Drawing.<\/div>\r\n
    \r\n

    Inventor Command:\u00a0 BASE VIEW<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe BASE VIEW command is used to create a Base view of the solid model contained in a part, assembly, or presentation file on the drawing sheet. The scale, style, labeling, and orientation of the view can be set when the view is created.\r\n\r\nShortcut: none<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n
    \r\n

    Inventor Command: PROJECTED VIEW<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe PROJECTED VIEW command is used to create a projected view from a Base view. The style, labeling, and direction from the Base view can be set by you when the view is created.\r\n\r\nShortcut: none<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n
    \r\n

    Inventor Command: SECTION VIEW<\/p>\r\n\r\n<\/header>\r\n

    \r\n\r\nThe SECTION VIEW command is used to create a Section view from an existing view. The location, style, labeling, and direction from the selected view can be set by you when the view is created.\r\n\r\nShortcut: none<\/strong>\r\n\r\n\"\"\r\n\r\n<\/div>\r\n<\/div>\r\n
    USER TIP:<\/strong> ANSI is an acronym for American National Standard Institute. ANSI has set drawing standards that are widely adapted and followed by most companies working in English or Imperial measurements. To read more about ANSI see: http:\/\/www.ansi.org\/\r\nISO is an acronym for International Organization for Standardization. ISO has set the drawing standards that are widely adapted and followed by most companies working in Metric measurements. To read more about ISO see: http:\/\/www.iso.org\/iso\/en\/ISOOnline.frontpage<\/div>\r\n

    WORK ALONG: Creating 2D Drawings<\/h1>\r\n

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

    Step 2<\/h2>\r\nEnter the NEW command to start a new drawing file. Enable the English tab and select the template: Modules Drawing ANSI (in).idw<\/span>. (Figure Step 2)\r\n\r\n[caption id=\"attachment_1782\" align=\"aligncenter\" width=\"53\"]\"\" Figure
    Step 2[\/caption]\r\n\r\n
    AUTHOR'S COMMENTS:<\/strong> See the User Tip before WORKALONG: Creating 2D Drawings for a explanation of the acronyms ANSI and ISO.<\/div>\r\n

    Step 3<\/h2>\r\nWhen the drawing file is opened, it will display an A size drawing complete with border and titleblock. Save the file with the name: Inventor Workalong 24-1<\/span>. (Figure Step 3)\r\n\r\n[caption id=\"attachment_1783\" align=\"aligncenter\" width=\"615\"]\"\"<\/a> Figure Step 3 [Click to see image full size][\/caption]\r\n

    Step 4<\/h2>\r\nEnter the BASE VIEW command to create the Base view. It will open the Drawing View dialogue box. Set the Orientation (view) to Front and the Style to Hidden Line. Ensure that the dialogue box matches the figure. (Figure Step 4)\r\n\r\n[caption id=\"attachment_1784\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 4 [Click to see image full size][\/caption]\r\n

    Step 5<\/h2>\r\nClick OK. In the Open dialogue box, select the part: Inventor Workalong 22-1D.ipt<\/span>. (Figure Step 5)\r\n\r\n[caption id=\"attachment_1785\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 5 [Click to see image full size][\/caption]\r\n

    Step 6<\/h2>\r\nSelect the location for the Front view. Don't be too concerned where you locate it since it can be moved later. Try to locate it close to where it is shown in the figure. (Figure Step 6A and 6B)\r\n\r\n[caption id=\"attachment_1786\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 6A [Click to see image full size][\/caption][caption id=\"attachment_1787\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 6B [Click to see image full size][\/caption]\r\n

    Step 7<\/h2>\r\nEnter the PROJECT VIEW command and select the Base view as the view to project from. (Figure Step 7)\r\n\r\n[caption id=\"attachment_1788\" align=\"aligncenter\" width=\"217\"]\"\" Figure Step 7[\/caption]\r\n

    Step 8<\/h2>\r\nMove the cursor up to locate the Top view. Click the mouse at the desired location. Right click the mouse. In the Right-click menu, select Create. (Figure Step 8A and 8B)\r\n\r\n[caption id=\"attachment_1789\" align=\"aligncenter\" width=\"207\"]\"\" Figure Step 8A[\/caption]\r\n\r\n[caption id=\"attachment_1790\" align=\"aligncenter\" width=\"251\"]\"\" Figure Step 8B[\/caption]\r\n

    Step 9<\/h2>\r\nUsing what you just learned, use the PROJECT VIEW command to create the Right Side view. (Figure Step 9)\r\n\r\n[caption id=\"attachment_1791\" align=\"aligncenter\" width=\"500\"]\"\" Figure Step 9[\/caption]\r\n

    Step 10<\/h2>\r\nYour drawing should now contain the Top, Front and Right Side views of the part. (Figure Step 10)\r\n\r\n[caption id=\"attachment_1792\" align=\"aligncenter\" width=\"601\"]\"\"<\/a> Figure Step 10 [Click to see image full size][\/caption]\r\n

    Step 11<\/h2>\r\nEnter the PROJECT VIEW command. Select the Base view (Front view) and project an Isometric view from it. (Figure Step 11)\r\n\r\n[caption id=\"attachment_1793\" align=\"aligncenter\" width=\"506\"]\"\" Figure Step 11[\/caption]\r\n

    Step 12<\/h2>\r\nRight click the Isometric view. In the Right-click menu, click Edit View. (Figure Step 12)\r\n\r\n[caption id=\"attachment_1794\" align=\"aligncenter\" width=\"350\"]\"\" Figure Step 12[\/caption]\r\n

    Step 13<\/h2>\r\nIn the Edit View dialogue box enable the display View\/Scale label (turn the light bulb on). Set the Scale to 0.75:1, View Identifier to ISOMETRIC and the Style to Shaded. (Figure Step 13A and 13B)\r\n\r\n[caption id=\"attachment_1795\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 13A [Click to see image full size][\/caption][caption id=\"attachment_1796\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 13B [Click to see image full size][\/caption]\r\n

    Step 14<\/h2>\r\nRight click the file name in the Browser bar. In the Right-click menu, click New Sheet. An A size drawing sheet will display in the Graphic window. The new sheet will be labeled Sheet:2 and will display in the Browser bar. (Figure Step 14)\r\n\r\n[caption id=\"attachment_1797\" align=\"aligncenter\" width=\"170\"]\"\" Figure Step 14[\/caption]\r\n

    Step 15<\/h2>\r\nRight-click Sheet:2. In the Right-click menu, click Edit Sheet. In the Edit Sheet dialogue box, pull down the Size list and select B to change Sheet 2 to a B size. Ensure that Landscape is enable. (Figure 15A, 15B, and 15C)\r\n\r\n[caption id=\"attachment_1798\" align=\"aligncenter\" width=\"297\"]\"\" Figure Step 15A[\/caption]\r\n\r\n[caption id=\"attachment_1799\" align=\"aligncenter\" width=\"300\"]\"\" Figure Step 15B[\/caption]\r\n\r\n[caption id=\"attachment_1800\" align=\"aligncenter\" width=\"396\"]\"\"<\/a> Figure Step 15C [Click to see image full size][\/caption]\r\n

    Step 16<\/h2>\r\nUsing what you just learned, create a Base view of Top view of part: Inventor Workalong 22-1C.ipt that you created in Module 22. (Figure Step 16)\r\n\r\n[caption id=\"attachment_1801\" align=\"aligncenter\" width=\"615\"]\"\"<\/a> Figure Step 16 [Click to see image full size][\/caption]\r\n

    Step 17<\/h2>\r\nEnter the SECTION VIEW command. Move the cursor to the centre of the circle on the Top view until it displays the green snap circle. You may have to move the cursor touching the circle circumference and then move back to the centre. Do NOT select the green snap circle, wait until it displays. Move the cursor to the right and you will see a dashed line indicating an implied line which is orthographic or horizontal, in this case. move outside the view. The yellow grid snap circle will display. Select a location when the grid snap is displayed. (Figure Step 17A and 17B)\r\n\r\n[caption id=\"attachment_1802\" align=\"aligncenter\" width=\"274\"]\"\" Figure Step 17A[\/caption]\r\n\r\n[caption id=\"attachment_1803\" align=\"aligncenter\" width=\"278\"]\"\" Figure Step 17B[\/caption]\r\n

    Step 18<\/h2>\r\nMove the cursor across to the other side of the view and when the geometry constraint (horizontal) displays, select a location about the same distance from the view as you did for the other side of the view. Right-click the mouse. In the Right-click menu, select Continue. (Figure Step 18A and 18B)\r\n\r\n[caption id=\"attachment_1804\" align=\"aligncenter\" width=\"259\"]\"\" Figure 18A[\/caption]\r\n\r\n[caption id=\"attachment_1805\" align=\"aligncenter\" width=\"313\"]\"\" Figure 18B[\/caption]\r\n

    Step 19<\/h2>\r\nMove the cursor down and the section view will display. The Section View dialogue box will open. Set the dialogue box as shown in the figure. (Figure Step 19A and 19B)\r\n\r\n[caption id=\"attachment_1806\" align=\"aligncenter\" width=\"615\"]\"\"<\/a> Figure 19A [Click to see image full size][\/caption]\r\n\r\n[caption id=\"attachment_1807\" align=\"aligncenter\" width=\"294\"]\"\" Figure 19B[\/caption]\r\n

    Step 20<\/h2>\r\nUsing the BASE VIEW command, create an Isometric view and set the scale to 1.25:1. (Figure Step 20)\r\n\r\n[caption id=\"attachment_1808\" align=\"aligncenter\" width=\"615\"]\"\"<\/a> Figure Step 20 [Click to see image full size][\/caption]\r\n

    Step 21<\/h2>\r\nSave and close the drawing file.\r\n
    USER TIP:<\/strong> The default labels and colors can be configured for each drawing file. Originally, these setting came from the template file that you used to start the drawing file. Any changes that you make will only affect the current drawing file. Enter the DOCUMENT SETTINGS command. See figure right. To change the default labels of the sheets, simply edit the value as shown in the figure below. To change the background colour of the Sheet, the Sheet Outline, Highlight or Selection, select the one you want from the Color dialogue box. In this example, the colour of the sheet was change to white.\"\"\"\"\"\"\"\"<\/div>\r\n
    USER TIP:<\/strong> To move a view on the drawing sheet, move the cursor onto the view\u2019s border. When you are on the border, it will highlight as shown in Step 1. If the view is a base view or a projected view that has a view dependent on it, the Graphic cursor will display as shown on the left. If the view is a Base view or a projected view that does NOT have view dependent on it, the cursor will display as shown on the right. To move a view, simply press and hold down the left mouse button and drag it to desired location as shown in Step 2.<\/div>\r\n

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

    Key Principles in Module 24<\/p>\r\n\r\n<\/header>\r\n

    \r\n
      \r\n \t
    1. A drawing file contains one or more 2 dimensional drawing sheets on which a 2D and\/or 3D scaled views of solid models contained in part, assembly, and presentation files. A drawing file has the file extension .idw. IDW is an acronym for Inventor Drawing.<\/li>\r\n \t
    2. A Base view is the first view created by the user. It controls the scale, orientation, and location of the orthographic views projected from it.<\/li>\r\n \t
    3. A projected view is a view projected from a Base view. The scale of a projected view cannot be set since the Base view that you projected it from controls its scale. The Base view also controls the orientation and location of the projected views.<\/li>\r\n \t
    4. A drawing sheet represents a blank piece of paper complete with titleblock and border. The size of drawing sheet can be set by the user. The sheet size can be a custom size set by the user or one of the ANSI or ISO drawing sheet standards.<\/li>\r\n \t
    5. There is no maximum number of drawing sheets that can be created for each drawing file but there must be at least one sheet. One sheet must exist in each drawing file at all times.<\/li>\r\n \t
    6. A view style can be displayed in one of three different styles. The three styles are hidden line, hidden line removed, and shaded. The style of a view can be changed as required after the view has been placed.<\/li>\r\n \t
    7. The scale of the view is a factor of the number that it is set to.\r\n\r\n[caption id=\"attachment_1815\" align=\"aligncenter\" width=\"136\"]\"\" Move[\/caption]\r\n\r\n[caption id=\"attachment_1816\" align=\"aligncenter\" width=\"149\"]\"\" Project[\/caption]\r\n\r\n[caption id=\"attachment_1817\" align=\"aligncenter\" width=\"300\"]\"\" Step 1[\/caption]\r\n\r\n[caption id=\"attachment_1818\" align=\"aligncenter\" width=\"300\"]\"\" Step 2[\/caption]<\/li>\r\n<\/ol>\r\n<\/div>\r\n<\/div>\r\n

      Lab Exercise 24-1<\/h1>\r\nTime allowed: 2 hours.\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
      See Below<\/td>\r\nInventor Course<\/td>\r\nInches<\/td>\r\nSee Below<\/td>\r\nN\/A<\/td>\r\nN\/A<\/td>\r\n<\/tr>\r\n<\/tbody>\r\n<\/table>\r\n

      Step 1<\/h2>\r\nCreate the following drawings and ensure the following:\r\nA<\/strong> There is a separate file for each drawing sheet.\r\nB<\/strong> Create the same views as shown.\r\nC<\/strong> If the scale is not indicated, set it to full scale or 1:1.\r\nD<\/strong> Each drawing file has only one drawing sheet.\r\nE<\/strong> Save the drawing files with the Drawing Name shown for each part.\r\n\r\nPart:<\/strong> Base\r\nDrawing Size:<\/strong> B\r\nDrawing Name:<\/strong> Inventor Lab 24-1A.idw Part Name: Inventor Workalong 22-1A.ipt\r\n\r\nTemplate:<\/strong> English-Modules Drawing ANSI (in).idw (Figure Step 1A)\r\n\r\n[caption id=\"attachment_1819\" align=\"aligncenter\" width=\"615\"]\"\"<\/a> Figure Step 1A [Click to see image full size][\/caption]Part:<\/strong> Post\r\nDrawing Size:<\/strong> C\r\nDrawing Name:<\/strong> Inventor Lab 24-1B.idw\r\nPart Name:<\/strong> Inventor Workalong 22-1B.ipt\r\nTemplate:<\/strong> English-Modules Drawing ANSI (in).idw (Figure Step 1B)\r\n\r\n[caption id=\"attachment_1820\" align=\"aligncenter\" width=\"615\" class=\"page-break-after\"]\"\"<\/a> Figure Step 1B [Click to see image full size][\/caption]\r\nPart:<\/strong> Screw\r\nDrawing Size:<\/strong> A\r\nDrawing Name:<\/strong> Inventor Lab 24-1C.idw\r\nPart Name:<\/strong> Inventor Workalong 22-1E.ipt\r\nTemplate:<\/strong> English-Modules D\r\n\r\nrawing ANSI (in).idw (Figure Step 1C)\r\n\r\n[caption id=\"attachment_1821\" align=\"aligncenter\" width=\"500\" class=\"page-break-after\"]\"\"<\/a> Figure Step 1C [Click to see image full size][\/caption]Assembly:<\/strong> Tool Holder\r\nDrawing Size:<\/strong> A\r\nDrawing Name:<\/strong> Inventor Lab 24-1.idw\r\nPart Name:<\/strong> Inventor Workalong 22-1.iam\r\nTemplate:<\/strong> English-Modules Drawing ANSI (in).idw (Figure Step 1D)\r\n\r\n[caption id=\"attachment_1822\" align=\"aligncenter\" width=\"500\"]\"\"<\/a> Figure Step 1D [Click to see image full size][\/caption]","rendered":"
      \n
      \n

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

      \n

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

        \n
      1. Describe 2D drawing files, drawing sheets, and drawing sizes.<\/li>\n
      2. Describe and apply the commands BASE VIEW, PROJECTED VIEW, SECTION VIEW, and NEW SHEET to create multiview and isometric views of a solid model on a drawing sheet.<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

        Drawing Files<\/h1>\n

        A drawing file<\/em><\/span> contains one or more drawing sheets on which 2 dimensional and\/or 3 dimensional scaled views of the solid models contained in part, assembly, or presentation files. The views can be created complete with hidden lines or shading. Annotation can be automatically or manually added to the views as required. A typical drawing sheet with an orthographic, section, and isometric view of a model is shown in Figure 24-1. Dimensioning, inserting text, and filling in the titleblock are taught in Module 25. When the drawing is complete, it can be printed or plotted on paper. A drawing file has the file extension .idw. IDW is an acronym for Inventor Drawing.<\/p>\n

        \"\"<\/a>
        Figure 24-1
        A Typical Drawing Sheet in a Drawing File [Click to see image full size]<\/figcaption><\/figure>\n

        Model Views<\/h2>\n

        A model view<\/em><\/span> is a scaled view orientated at an angle and direction that the solid model or assembly is being viewed and displayed on the drawing sheet. There is no limit to the number of views or the number of solid models from part, assembly, or presentation files that can be placed on a drawing sheet. Views can also be automatically annotated or labeled. There are eight predefined views that you can select from when creating the view. The predefined views are the; base, projection, auxiliary, section, detail, broken, breakout, and overlay.<\/p>\n

        The Base<\/h2>\n

        A Base view<\/span><\/em> is the first view created on the drawing sheet. It controls the scale, orientation, and location of the views projected from it. The orthographic and\/or isometric views in the drawing are created from the Base view. For example, if a multiview drawing was being created from a solid model, the Front view is created first as a Base view. The Front view would control the scale and location of the projected Top and Right Side views. See Figure 24-2. To change the scale of all views, only the scale of the Front (Base) view would have to be changed and the Top and Right Side views would automatically change scale to match. If the Front view was moved, the Top and Right Side views would move accordingly to keep their multiview position.<\/p>\n

        \"\"
        Figure 24-2
        Multiview Drawing<\/figcaption><\/figure>\n

        Projected Views<\/h2>\n

        A projected view<\/span><\/em> is a view projected from a Base view. The scale of a projected view cannot be set since the Base view that you projected it from controls its scale. The Base view also controls the orientation and location of the projected views.<\/p>\n

        Drawing Sheets<\/h2>\n

        A drawing sheet<\/span><\/em> represents a blank piece of paper complete with titleblock and border. The size of drawing sheet can be set by the user. The sheet size can be a custom size set by you or one of the ANSI or ISO drawing sheet standards listed in the table shown in Figure 24-3.<\/p>\n

        There is no maximum number of drawing sheets that can be created for each drawing file but there must be at least one sheet. Sheets can be created or deleted but Inventor will NOT allow all of them to be deleted since one sheet must exist at all times.<\/p>\n

        The drawing sheet can be assigned a drawing border and a titleblock which can be created or edited by you. Custom drawing template files containing borders and titleblocks are supplied with the Inventor book.<\/p>\n

        MUST KNOW:<\/strong> There is no maximum number of drawing sheets that can be created for each drawing file but there must be at least one sheet. One sheet must exist in each drawing file at all times.<\/div>\n

        ANSI and ISO Standard Drawing Sheet Sizes<\/h2>\n
        \"\"
        Figure 24-3
        Standard ANSI and ISO Drawing Sheet Sizes<\/figcaption><\/figure>\n

        View Style<\/h2>\n

        A view style<\/span><\/em> can be displayed in one of three different styles. The three styles are hidden line<\/em><\/span>, hidden line removed<\/em><\/span>, and shaded<\/span> <\/em>as shown in Figure 24-4. The style of a view can be changed as required after the view has been placed.<\/p>\n

        View Scale<\/h2>\n

        The scale<\/em> <\/span>of the view is a factor of the number that it is set to. For example, if the scale is set to 1 then the factor of 1 X 1 = 1, full scale or 1:1. If the scale is set to 2 then 2 X 1 = 2 or a scale of 2:1 which is twice the size of the original model. On the other hand, if the scale factor is set to 0.5 then 0.5 X 1 = 0.5 or the scale of 1:2 which would display the view one-half the size of the original model.<\/p>\n

        \"\"
        Figure 24-3
        View Styles<\/figcaption><\/figure>\n
        MUST KNOW:<\/strong> A drawing file contains one or more 2 dimensional drawing sheets on which a 2D and\/or 3D scaled views of solid models contained in part, assembly, and presentation files. A drawing file has the file extension .idw. IDW is an acronym for Inventor Drawing.<\/div>\n
        \n
        \n

        Inventor Command:\u00a0 BASE VIEW<\/p>\n<\/header>\n

        \n

        The BASE VIEW command is used to create a Base view of the solid model contained in a part, assembly, or presentation file on the drawing sheet. The scale, style, labeling, and orientation of the view can be set when the view is created.<\/p>\n

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

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

        \n
        \n

        Inventor Command: PROJECTED VIEW<\/p>\n<\/header>\n

        \n

        The PROJECTED VIEW command is used to create a projected view from a Base view. The style, labeling, and direction from the Base view can be set by you when the view is created.<\/p>\n

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

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

        \n
        \n

        Inventor Command: SECTION VIEW<\/p>\n<\/header>\n

        \n

        The SECTION VIEW command is used to create a Section view from an existing view. The location, style, labeling, and direction from the selected view can be set by you when the view is created.<\/p>\n

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

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

        USER TIP:<\/strong> ANSI is an acronym for American National Standard Institute. ANSI has set drawing standards that are widely adapted and followed by most companies working in English or Imperial measurements. To read more about ANSI see: http:\/\/www.ansi.org\/
        \nISO is an acronym for International Organization for Standardization. ISO has set the drawing standards that are widely adapted and followed by most companies working in Metric measurements. To read more about ISO see: http:\/\/www.iso.org\/iso\/en\/ISOOnline.frontpage<\/div>\n

        WORK ALONG: Creating 2D Drawings<\/h1>\n

        Step 1<\/h2>\n

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

        Step 2<\/h2>\n

        Enter the NEW command to start a new drawing file. Enable the English tab and select the template: Modules Drawing ANSI (in).idw<\/span>. (Figure Step 2)<\/p>\n

        \"\"
        Figure
        Step 2<\/figcaption><\/figure>\n
        AUTHOR’S COMMENTS:<\/strong> See the User Tip before WORKALONG: Creating 2D Drawings for a explanation of the acronyms ANSI and ISO.<\/div>\n

        Step 3<\/h2>\n

        When the drawing file is opened, it will display an A size drawing complete with border and titleblock. Save the file with the name: Inventor Workalong 24-1<\/span>. (Figure Step 3)<\/p>\n

        \"\"<\/a>
        Figure Step 3 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 4<\/h2>\n

        Enter the BASE VIEW command to create the Base view. It will open the Drawing View dialogue box. Set the Orientation (view) to Front and the Style to Hidden Line. Ensure that the dialogue box matches the figure. (Figure Step 4)<\/p>\n

        \"\"<\/a>
        Figure Step 4 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 5<\/h2>\n

        Click OK. In the Open dialogue box, select the part: Inventor Workalong 22-1D.ipt<\/span>. (Figure Step 5)<\/p>\n

        \"\"<\/a>
        Figure Step 5 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 6<\/h2>\n

        Select the location for the Front view. Don’t be too concerned where you locate it since it can be moved later. Try to locate it close to where it is shown in the figure. (Figure Step 6A and 6B)<\/p>\n

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

        Step 7<\/h2>\n

        Enter the PROJECT VIEW command and select the Base view as the view to project from. (Figure Step 7)<\/p>\n

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

        Step 8<\/h2>\n

        Move the cursor up to locate the Top view. Click the mouse at the desired location. Right click the mouse. In the Right-click menu, select Create. (Figure Step 8A and 8B)<\/p>\n

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

        Step 9<\/h2>\n

        Using what you just learned, use the PROJECT VIEW command to create the Right Side view. (Figure Step 9)<\/p>\n

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

        Step 10<\/h2>\n

        Your drawing should now contain the Top, Front and Right Side views of the part. (Figure Step 10)<\/p>\n

        \"\"<\/a>
        Figure Step 10 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 11<\/h2>\n

        Enter the PROJECT VIEW command. Select the Base view (Front view) and project an Isometric view from it. (Figure Step 11)<\/p>\n

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

        Step 12<\/h2>\n

        Right click the Isometric view. In the Right-click menu, click Edit View. (Figure Step 12)<\/p>\n

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

        Step 13<\/h2>\n

        In the Edit View dialogue box enable the display View\/Scale label (turn the light bulb on). Set the Scale to 0.75:1, View Identifier to ISOMETRIC and the Style to Shaded. (Figure Step 13A and 13B)<\/p>\n

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

        Step 14<\/h2>\n

        Right click the file name in the Browser bar. In the Right-click menu, click New Sheet. An A size drawing sheet will display in the Graphic window. The new sheet will be labeled Sheet:2 and will display in the Browser bar. (Figure Step 14)<\/p>\n

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

        Step 15<\/h2>\n

        Right-click Sheet:2. In the Right-click menu, click Edit Sheet. In the Edit Sheet dialogue box, pull down the Size list and select B to change Sheet 2 to a B size. Ensure that Landscape is enable. (Figure 15A, 15B, and 15C)<\/p>\n

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

        Step 16<\/h2>\n

        Using what you just learned, create a Base view of Top view of part: Inventor Workalong 22-1C.ipt that you created in Module 22. (Figure Step 16)<\/p>\n

        \"\"<\/a>
        Figure Step 16 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 17<\/h2>\n

        Enter the SECTION VIEW command. Move the cursor to the centre of the circle on the Top view until it displays the green snap circle. You may have to move the cursor touching the circle circumference and then move back to the centre. Do NOT select the green snap circle, wait until it displays. Move the cursor to the right and you will see a dashed line indicating an implied line which is orthographic or horizontal, in this case. move outside the view. The yellow grid snap circle will display. Select a location when the grid snap is displayed. (Figure Step 17A and 17B)<\/p>\n

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

        Step 18<\/h2>\n

        Move the cursor across to the other side of the view and when the geometry constraint (horizontal) displays, select a location about the same distance from the view as you did for the other side of the view. Right-click the mouse. In the Right-click menu, select Continue. (Figure Step 18A and 18B)<\/p>\n

        \"\"
        Figure 18A<\/figcaption><\/figure>\n
        \"\"
        Figure 18B<\/figcaption><\/figure>\n

        Step 19<\/h2>\n

        Move the cursor down and the section view will display. The Section View dialogue box will open. Set the dialogue box as shown in the figure. (Figure Step 19A and 19B)<\/p>\n

        \"\"<\/a>
        Figure 19A [Click to see image full size]<\/figcaption><\/figure>\n
        \"\"
        Figure 19B<\/figcaption><\/figure>\n

        Step 20<\/h2>\n

        Using the BASE VIEW command, create an Isometric view and set the scale to 1.25:1. (Figure Step 20)<\/p>\n

        \"\"<\/a>
        Figure Step 20 [Click to see image full size]<\/figcaption><\/figure>\n

        Step 21<\/h2>\n

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

        USER TIP:<\/strong> The default labels and colors can be configured for each drawing file. Originally, these setting came from the template file that you used to start the drawing file. Any changes that you make will only affect the current drawing file. Enter the DOCUMENT SETTINGS command. See figure right. To change the default labels of the sheets, simply edit the value as shown in the figure below. To change the background colour of the Sheet, the Sheet Outline, Highlight or Selection, select the one you want from the Color dialogue box. In this example, the colour of the sheet was change to white.\"\"\"\"\"\"\"\"<\/div>\n
        USER TIP:<\/strong> To move a view on the drawing sheet, move the cursor onto the view\u2019s border. When you are on the border, it will highlight as shown in Step 1. If the view is a base view or a projected view that has a view dependent on it, the Graphic cursor will display as shown on the left. If the view is a Base view or a projected view that does NOT have view dependent on it, the cursor will display as shown on the right. To move a view, simply press and hold down the left mouse button and drag it to desired location as shown in Step 2.<\/div>\n

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

        Key Principles in Module 24<\/p>\n<\/header>\n

        \n
          \n
        1. A drawing file contains one or more 2 dimensional drawing sheets on which a 2D and\/or 3D scaled views of solid models contained in part, assembly, and presentation files. A drawing file has the file extension .idw. IDW is an acronym for Inventor Drawing.<\/li>\n
        2. A Base view is the first view created by the user. It controls the scale, orientation, and location of the orthographic views projected from it.<\/li>\n
        3. A projected view is a view projected from a Base view. The scale of a projected view cannot be set since the Base view that you projected it from controls its scale. The Base view also controls the orientation and location of the projected views.<\/li>\n
        4. A drawing sheet represents a blank piece of paper complete with titleblock and border. The size of drawing sheet can be set by the user. The sheet size can be a custom size set by the user or one of the ANSI or ISO drawing sheet standards.<\/li>\n
        5. There is no maximum number of drawing sheets that can be created for each drawing file but there must be at least one sheet. One sheet must exist in each drawing file at all times.<\/li>\n
        6. A view style can be displayed in one of three different styles. The three styles are hidden line, hidden line removed, and shaded. The style of a view can be changed as required after the view has been placed.<\/li>\n
        7. The scale of the view is a factor of the number that it is set to.
          \n
          \"\"
          Move<\/figcaption><\/figure>\n
          \"\"
          Project<\/figcaption><\/figure>\n
          \"\"
          Step 1<\/figcaption><\/figure>\n
          \"\"
          Step 2<\/figcaption><\/figure>\n<\/li>\n<\/ol>\n<\/div>\n<\/div>\n

          Lab Exercise 24-1<\/h1>\n

          Time allowed: 2 hours.<\/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
          See Below<\/td>\nInventor Course<\/td>\nInches<\/td>\nSee Below<\/td>\nN\/A<\/td>\nN\/A<\/td>\n<\/tr>\n<\/tbody>\n<\/table>\n

          Step 1<\/h2>\n

          Create the following drawings and ensure the following:
          \nA<\/strong> There is a separate file for each drawing sheet.
          \nB<\/strong> Create the same views as shown.
          \nC<\/strong> If the scale is not indicated, set it to full scale or 1:1.
          \nD<\/strong> Each drawing file has only one drawing sheet.
          \nE<\/strong> Save the drawing files with the Drawing Name shown for each part.<\/p>\n

          Part:<\/strong> Base
          \nDrawing Size:<\/strong> B
          \nDrawing Name:<\/strong> Inventor Lab 24-1A.idw Part Name: Inventor Workalong 22-1A.ipt<\/p>\n

          Template:<\/strong> English-Modules Drawing ANSI (in).idw (Figure Step 1A)<\/p>\n

          \"\"<\/a>
          Figure Step 1A [Click to see image full size]<\/figcaption><\/figure>\n

          Part:<\/strong> Post
          \nDrawing Size:<\/strong> C
          \nDrawing Name:<\/strong> Inventor Lab 24-1B.idw
          \nPart Name:<\/strong> Inventor Workalong 22-1B.ipt
          \nTemplate:<\/strong> English-Modules Drawing ANSI (in).idw (Figure Step 1B)<\/p>\n

          \"\"<\/a>
          Figure Step 1B [Click to see image full size]<\/figcaption><\/figure>\n

          Part:<\/strong> Screw
          \nDrawing Size:<\/strong> A
          \nDrawing Name:<\/strong> Inventor Lab 24-1C.idw
          \nPart Name:<\/strong> Inventor Workalong 22-1E.ipt
          \nTemplate:<\/strong> English-Modules D<\/p>\n

          rawing ANSI (in).idw (Figure Step 1C)<\/p>\n

          \"\"<\/a>
          Figure Step 1C [Click to see image full size]<\/figcaption><\/figure>\n

          Assembly:<\/strong> Tool Holder
          \nDrawing Size:<\/strong> A
          \nDrawing Name:<\/strong> Inventor Lab 24-1.idw
          \nPart Name:<\/strong> Inventor Workalong 22-1.iam
          \nTemplate:<\/strong> English-Modules Drawing ANSI (in).idw (Figure Step 1D)<\/p>\n

          \"\"<\/a>
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