An Inventor Project

An Inventor project is a user named process to logically organize, store, and manage the valid links to the files created for an undertaking. For each project a user created name and a home folder is assigned. Inventor creates a project file that contains the project’s parameters and the paths to the locations of the files in that project. There is no limit to the number of projects that can be created. Inventor assigns a shortcut for each project so that you can easily select the appropriate project when required.

A project should be created so that it has a logical connection between the files in it. For example, if you were designing and drawing an office chair, all the individual parts of that chair, the assembly drawings, the design data, and the 2D working drawings would be stored in a project that you might name ‘ Office Chair ‘.

When a project is created, Inventor automatically creates a project file and saves it in the home folder of the project. A project file is automatically given the extension .ipj and contains the project parameters data as shown in Figure 1-1. This file also specifies the paths to the templates and files in the project. The information, parameters and data contained in the project file can be edited as required.

Figure 1-1
Typical Project Parameter Data List

WORK ALONG: Creating the Project for the Inventor book

Step 1

Start Inventor and enable the Get Started tab. In the ribbon menu, click Projects. This will display the Projects window. (Figure Step 1)

Figure Step 1 [Click to see image full size]

Step 2

Click the New button along the bottom of the dialogue box. The Inventor project wizard window will open. Enable the New Single User Project button and then click Next. (Figure Step 2A and 2B)

Figure Step 2A

Figure Step 2B

Step 3

Name the project: Inventor Course. (Figure Step 3)

Figure Step 3

Step 4

Set the location for the Project (Workspace) Folder. To do that, click the Browse button (the one with the 3 dots at the right-hand of the Project (Workspace) Folder) window. In the Browse for Folder dialogue box, locate the folder: C:\CAD Courses\Inventor\Lab Exercises. Highlight it by selecting it and click OK. (Figure Step 4A and 4B)

Figure Step 4A

Figure Step 4B

Step 5

You should now see the Project (Workspace) Folder location as follows: C:\CAD Courses\Inventor\Lab Exercises (Figure Step 5)

Figure Step 5

Step 6

The Project File to be created will automatically be created by Inventor. (Figure Step 6)

Figure Step 6

Step 7

Check the completed page and ensure it matches the figure. Click the Finish button to complete the project setup. (Figure Step 7)

Figure Step 7

Step 8

The Project window will show the new project that you just created. Double click Inventor Course in the Projects name column and note how the check mark icon beside the Inventor Course project indicates it is the current project. (Figure Step 8)

Figure Step 8 [Click to see image full size]

Step 9

Down near the bottom, expand Folder Options and click the Templates folder to select it. (Figure Step 9)

Figure Step 9

Step 10

While the Templates folder is selected, right-click the mouse. In the right-click menu, click Edit. (Figure Step 10)

Figure Step 10

Step 11

Click the Browse icon. (Figure Step 11)

Figure Step 11

Step 12

In the Browse For Folder dialogue box, locate and select the Templates folder: C:\CAD Courses\Inventor\Templates (Figure Step 12)

Figure Step 12

Step 13

Click OK and the dialogue box will appear similar to the figure. (Figure Step 13)

Figure Step 13 [Click to see image full size]

Step 14

Click Apply and Done to complete the new project.

Step 15

Exit Inventor.

Step 16

Open Windows Explorer and locate the folder Lab Exercises in the folder list. The file Inventor Course.ipj, that was automatically created by Inventor in this workalong, should appear in the file list. (Figure Step 16)

Figure Step 16

Key Principles

Inventor’s Graphic Window

When a file is active, Inventor will display the Graphic window. The Graphic window has two different modes, the Sketch mode and the Model mode. The Sketch mode is used to create and edit 2D sketches that are then extruded or revolved to create 3D solid models. The Model mode is used to view, manipulate and modify 3D solid models. You can switch between these two modes to construct or edit and create the solid model. The mode that is currently displayed is called the current mode. The Model mode must be the current mode to save the file.

A 3D Solid Model

A 3D solid model, Figure 2-1, is the best possible computerized representation of a real object. A solid model can be colored or rendered plus the mass properties can be obtained from it. Mass properties are attributes such as volume, weight, surface area, moments of inertia, and centre of gravity. They are taught in Module 20.

Figure 2-1
A 3D Solid Model

An Inventor File

Regardless of the type of files that are created using Inventor, they are called files as compared to files created on a CAD system which are typically called drawings. A file can be a 3D solid model (called a part), an assembly, a presentation, or a drawing created in Inventor and saved in digital format. The four types of files, taught in this book, that Inventor can create and save are part files, assembly files, presentation files, and drawing files.

A Part File

A part file is one 3D solid model. A part file has the file extension .ipt which is an acronym for Inventor ParT. A part file can be used on its own, used to create a working drawing, used as part of an assembly file, or used as part of a presentation file. Assembly and presentation files are taught in Module 21 to Module 26.

Starting a New File

A new file is started using the NEW command. The NEW command forces you to select the template file that will be used to create the new file. Every new Inventor file must be created from an existing template file. The file currently being editing in Inventor is called the current file or sometimes the active file.

Templates

A template file is simply an Inventor file, set with the desired parameters by its creator, named, and saved. As part of the Inventor book there are two distinct sets of templates provided. One set is in english units and the other set is in metric units. The English templates use the base unit of inches and the metric templates use the base unit of millimeters. Template files can also contain modelling objects so that several similar parts can easily be started from a common pre-built unit.

Saving Files

Inventor keeps the current file in RAM memory. If the computer cashes or the power fails while the operator is working on a file, all the work on the file, since the last time it was saved, will be lost. When the file is saved it saves the current file that is in RAM memory onto the disk drive.

Ensure that the current file is saved frequently to avoid losing production time. You should get into the habit of saving the current file every 5 to 10 minutes.

Inventor’s Menus

Inventor has many different menus that are used by you to give instructions to Inventor while constructing and editing files. The Inventor menus taught in the Inventor book are the Pull-down menu, the Ribbon menu, the Quick Access toolbar, the Browser bar, and the Right-click menu.

Inventor’s Pull-Down Menu

To pull down Inventor’s Pull-down menu, click the File tab. If the pull down menu item has a small solid triangle at the end, it has a flyout menu associated with it. If you move the cursor on the triangle, the flyout menu will display. See Figure 2-2.

Figure 2-2
The Pull-Down Menu

Ribbon Menu

The Ribbon menu is used for most of your work in Inventor. See Figure 2-3.

Figure 2-3
A Typical Ribbon Menu

Browser Bar

The Browser bar displays the hierarchical structure of the model or assembly of the current file. It is your most important and most-used tool to create and modify objects within files. The Browser bar will be taught in more detail in future modules. It is normally docked on the left side of the Graphic window. See Figure 2-4.

Figure 2-4
Browser Bar

Figure 2-5 Right-click Menu

Right-Click Menu

When the right mouse button is clicked, it displays the Right-click menu. See Figure 2-5. It is sometimes called the Cursor menu since it displays at the current location of the cursor. This menu changes automatically depending on the current command or operation being performed. It usually takes the new user a bit of time to get used to using this menu.

Status Bar

The Status bar is permanently located along the bottom of the Graphic window. It displays the prompts that the current command is issuing, as shown in Figure 2-6, as well as the coordinate locations, as shown in Figure 2-7. These prompts help you understand what information Inventor requires and the cursor location, length, and angle in the current command.

Figure 2-6  Status Bar – Showing a Command
Prompt.

Figure 2-7 Status Bar – Showing Coordinate
Information

The Graphic Cursor

The Graphic cursor is used to select menu items or objects on the sketch or model. See Figure 2-8.

Figure 2-8
The Graphic Cursor

Dialogue Boxes

Inventor commands use many different dialogue boxes to obtain information to be used by the command or current operation. A typical dialogue box is shown in Figure 2-9.

Figure 2-9 A Typical Dialogue Box

The Mouse

Inventor is programed to use the three buttons on the mouse as follows:

Left Button:  This is the pick button. Use it to pick objects, pick menu items, or select locations on the sketch or model.

Middle Button:  The middle button or the wheel is used to zoom and pan around the Graphic window. This will be discussed in detail in Module 3.

Right Button:  The right button displays the Right-click menu. See Figure 2-10. The Right-click menu will change depending on the current command or operation being preformed. It is a very helpful menu and should be used as often as possible when working in Inventor.

Inventor Commands

An Inventor command is an instruction from you to Inventor instructing it what operation to perform. Commands can be entered by selecting an item from a Pull-down menu, a Right-click menu, an icon on a Toolbar, an item on the Panel menu, or entering a shortcut on the keyboard. Since there are usually many different ways of entering the same command, you should select the method that works the best for you. There is no right or wrong way to enter a command. You should experiment to find the fastest method to improve your drawing speed and productivity.

Ending the Current Command

When you enter a command, it becomes the current command or sometimes called the active command. Inventor must be instructed to end the current command. There are two methods available to do this. The first is to press the Esc key on the keyboard and the second is click to Done or Cancel on the Right-click menu as shown in Figure 2-10.

Figure 2-10 Ending a Command

Undo and Redo Commands

In the current file, any Inventor command or commands can be undone to reverse any changes that they may have made. To do this, click the Undo icon in the Quick Access toolbar as shown in Figure 2-11. Each click will undo the previous step. If the Undo icon was used to undo a command or a series of commands, it can be reversed by clicking the Redo icon. See Figure 2-12.

Fig 2-11 Undo Icon

Fig 2-11 Redo Icon

WORK ALONG: Creating and Saving a Part File

Step 1

Start Inventor and check the current project. If required, set it to Inventor Course. (Figure Step 1)

Figure Step 1

Step 2

Click the NEW command icon in the upper left corner of the screen or under the File tab. In the Create New File dialogue box, enable the folder: Templates – English. (Figure Step 2A and 2B)

Figure Step 2A

Figure Step 2B

Step 3

Select the template: Modules Part (in).ipt icon and click OK. (Figure Step 3)

Figure Step 3

Step 4

Inventor will display the Graphic window, in Sketch mode, as shown in the figure. (Figure Step 4)

Figure Step 4 [Click to see image full size]

Step 5

Click the Finish Sketch icon to change to Model mode. (Figure Step 5A and 5B)

Figure Step 5A

Figure Step 5B [Click to see image full size]

Step 6

Click the Save icon. It will open the Save As dialogue box. In the File name: box, enter the name: Inventor Workalong 02-1 and click Save. (Figure Step 6A and 6B)

Figure Step 6A

Figure Step 6B [Click to see image full size]

Step 7

The file name should now display on top bar of the Graphic window similar to what is shown in the figure. (Figure Step 7)

Figure Step 7

Step 8

Click the File tab and then the Close icon to close the current part file. (Figure Step 8)

Figure Step 8

Step 9

Click the Inventor icon to pull down the menu. On the Pull-down menu, click Exit Autodesk Inventor Professional to exit Inventor. (Figure Step 9)

Figure Step 9

WORK ALONG: Configuring and Working with Inventor’s Interface

Step 1

Start Inventor and check the current project. If required, set it to Inventor Course.

Step 2

Click the New icon. In the New File dialogue box, enable the folder: Metric Templates.

Step 3

Select the template: Module Part (mm).ipt. (Figure Step 3)

Figure Step 3

Step 4

Click Finish Sketch to exit Sketch mode. While in Model mode, save the part file with the name: Inventor Workalong 02-2. (Figure Step 4)

Figure Step 4 [Click to see image full size]

Step 5

Move the cursor onto the space between the plus (+) sign and the magnifying glass at the top of the Browser bar and press and hold the left mouse button down. While holding the button down, drag the Browser bar into the Graphic window. The Graphic window should appear similar to the figure. (Figure Step 5)

Figure Step 5 [Click to see image full size]

Step 6

Move the cursor onto the space between the plus (+) sign and the magnifying glass at the top of the Browser bar and press and hold the left mouse button down. While holding the button down, drag the Browser bar to the left until its colors fade. Release the left mouse button and the browser bar will dock on the left edge of the screen. (Figure Step 6)

Figure Step 6 [Click to see image full size]

Step 7

Click Sketch1 in the Browser bar to select it and right click the mouse. In the Right-click menu, click Edit Sketch. (Figure Step 7)

Figure Step 7

Step 8

The Graphic window will change to Sketch mode and should appear similar to the figure. (Figure step 8)

Figure Step 8 [Click to see image full size]

Step 9

Change to Model mode. Save and close the part file.

Key Principles

Viewing the 2D Sketch and 3D Model

In Sketch mode, you are viewing and working on a two dimensional plane. In Model mode, you are viewing and working in three dimensions the same way the human eye see real objects. It is essential for you to be able to change the viewing position of the 2D sketch and the 3D model as required. This is done by zooming, panning, and orbiting to change the viewpoint of the 2D sketch and the 3D model.

Zooming

Zooming is the process of changing the viewable size of the sketch or model to make it appear either smaller or larger. It is an important tool for you and is used extensively in the drawing and modeling process. As it is zoomed, the size of the sketch or model not changed, Inventor is simply adjusting the distance the object is from your eyes making it appear larger or smaller. I wondered why the Frisbee was getting bigger, and then it struck me…

Panning

Panning is the process of moving the sketch or model around the Graphic window without actually physically moving it from its location in space. It is an important tool for you and is used extensively while working in Inventor.

Orbiting

Orbiting is the process of changing the orientation of the sketch or model in relation to your eyes. Rather then changing the orientation of your eyes, Inventor orbits the sketch or model and your eyes remain stationary. The model and sketch are not physically rotated or their orientation in space changed. Orbiting is used extensively when working in Inventor.

Home View

The Home view is important to you while working in Inventor. It is the viewing position of the sketch or model to a known isometric view. This view re-establishes your bearings to better visualize the sketch or model because you are viewing it in a known viewing position.

WORK ALONG: Viewing the Model

Step 1

Start Inventor and check the current project. If required, set it to Inventor Course.

Step 2

Click the Open icon. In the Open dialogue box, select the file:

Inventor Workalong 03-1.ipt . Note how the file name will appear in the File name: box as shown in the figure. (Figure Step 2)

Figure Step 2 [Click to see image full size]

Step 3

If you are asked to convert the appearance, click Yes. (Figure Step 3).

Figure Step 3

Step 4

The part will open and display in Model mode and appear similar to the figure. (Figure Step 4).

Figure Step 4 [Click to see image full size]

Step 5

Move the cursor to approximately the centre of the solid model as shown in the figure. While keeping the cursor in the centre, rotate the mouse wheel back and forth. Note how the model appears larger and smaller. (Figure Step 5A and 5B)

Figure Step 5A

Figure Step 5B [Click to see image full size]

Step 6

Move the cursor near the model and press and hold the wheel down. A small Hand icon will replace the arrow cursor as shown in the figures. While the Hand icon is displayed, move the mouse to pan the model as shown. (Figure Step 6A, 6B, and 6C)

Figure Step 6A

Figure Step 6B

Figure Step 6C [Click to see image full size]

Step 7

Press F6 to return the model to its Home view. (Figure Step 7)

Figure Step 7 [Click to see image full size]

Step 8

Press F4 and hold it down. While holding it down, move the cursor outside the orbit circle, as shown below. The cursor will change as shown in the figures. Press and hold down the left mouse button. While holding it down, move the mouse and the model will orbit. (Figures 8A, 8B, and 8C)

Figure Step 8A

Figure Step 8B

Figure Step 8C

Step 9

Press F4 and hold it down. While holding it down, move the Graphic cursor somewhere inside the orbit circle. The icon will change in appearance as shown in the figures. Press the left mouse button and while holding it down, move the mouse. The model will orbit. (Figure Step 9A, 9B, and 9C)

Figure Step 9A

Figure Step 9B

Figure Step 9C

Step 10

Press F6 to return the model to its home view. (Figure Step 10)

Figure Step 10

Step 11

Close the part without saving it.

Key Principles

Geometry Lesson: Points and Lines

A point is defined as a single XY coordinate. It does not have width, height, or depth. A line is the shortest distance between two XY coordinates. Lines can be horizontal, vertical, or inclined. Lines that are the same distance apart are called parallel lines. Perpendicular lines are at right angles to each other or 90 degrees apart. See Figure 4-1 and 4-2.

Figure 4-1
Points and Lines [Click to see image full size]

Figure 4-2
Parallel and Perpendicular Lines [Click to see image full size]

The Cartesian Coordinate System

To accurately draw two dimensional (2D) Base sketches, you must understand the Cartesian Coordinate System.

Figure 4-3
The Cartesian Coordinate System [Click to see image full size]

The Cartesian Coordinate System consists of two numbered lines crossing perpendicular to one another at their zero values. The horizontal axis is the X axis and the vertical axis is the Y axis. See Figure 4-3. A coordinate value is assigned to each location on the current construction plane. Each coordinate value consists of a pair of numbers, the first is the X coordinate and the second is the Y coordinate, written X,Y. The X and Y values are separated by a comma. For example, X2,Y4 is the location 2 units to the right and 4 units up from X0,Y0 or 0,0.

The values can be either positive or negative. Positive numbers are default so the plus sign is not required. If the value is negative, the minus sign must precede the number. For example, -3,5 is X minus 3 and Y positive 5.

Parametric Solid Modeling

Inventor is a true Three Dimensional Parametric Solid Modeling system. A parametric solid model is a 3 dimensional solid model designed with geometrical and dimensional constraints rather then hard dimensions. A model designed in this way can then be modified by changing the dimensions, and/or constraints during or after the design is complete. When one or more constraints are modified, all other dependant constraints will automatically modify the model to conform to the new constraints. Geometric constraints are taught in this modules and dimensional constraints are taught in Module 5.

Geometrical Constraints

Geometrical constraints are used to apply geometrical relationships to the objects in the 2D sketch. They specify the geometrical relationship that the objects have to the sketching plane and to one another. Relationships like horizontal, vertical, parallel, or perpendicular are used. By applying geometrical constraints the number of dimensional constraints required to fully constrain the model is reduced. Applying the correct geometrical constraints prevents unwanted changes to a feature when geometry or dimensions are modified.

Since the geometrical constraint symbol displays and the constraints are automatically applied as the sketch is drawn, you have control on which constraints are applied to the objects as you are drawing the sketch. Constraints can be added while creating the sketch or by editing the sketch after the solid model is constructed. The geometrical constraints taught in this module are shown in Figure 4-4. Additional geometrical constraints will be taught throughout the Inventor book.

Figure 4-4
Geometrical Constraints

Projecting Reference Geometry

Projected reference geometry is geometry that has its position fixed relative to the sketching plane it resides on. Objects in the sketch are constrained with geometrical or dimensional constraints to the reference geometry to constrain it to the sketching plane. If the objects in the sketch are not constrained to the sketching plane, they will free float. A sketch that is not constrained to the sketching plane can never be fully constrained.

Inventor allows reference geometry to be projected in many different methods and uses. Many of these methods will be covered in the Inventor book. In this module, projecting the Center Point onto the plane of the Base sketch is taught.

Snapping

It is absolutely imperative that, when required, you snap to grids or locations on objects when drawing 2D sketches. Snapping to these locations ensures that the sketch is drawn accurately and constrained correctly. Inventor has many different snapping locations and they will be taught throughout the Inventor book. For now, the snap locations shown in Figure 4-5 should be used when drawing sketches. Study the figure before starting the workalong.

Figure 4-5
Snap Locations and Symbols

Lines

Lines are the drawing objects that are used the most when drawing 2D sketches. A line is defined as the shortest distance between two XY coordinate locations. Once a line is drawn, Inventor knows the location of its endpoints as well as the midpoint of the line. Other lines or drawing objects can be drawn by snapping to those locations. See Figure 4-6.

Figure 4-6
A Line

Base Sketch

The Base sketch is the first 2D sketch drawn in a new part. After the Base sketch is complete, it is extruded or revolved to create the Base model. Before drawing the Base sketch, you should study the model being constructed to determine the best plane to draw it on. The best view to use is the view with the most complex contour shape that does not contain arcs and curves. Draw the lines using lengths close to the finished dimensions. They do not have to be 100% accurate in length. The following rules should be followed when drawing the base sketch.

1. The objects in the sketch must meet exactly at their endpoints and cannot overlap.
2. The objects must form a perfect closed polygon and cannot contain any gaps.
3. The objects must have geometrical constraints applied to control the shape of the sketch.
4. Leave fillets and chamfers out of the original sketch. They can be added to the model after it is created. This is taught in Module 15.

X0Y0Z0

The two bold grid lines on the sketching plane represents the X and Y axis of the Cartesian Coordinate System. The axis lines display can be either enabled or disabled. It should currently be enabled. The horizontal line is the X axis and the vertical line is the Y axis. The point where they intersect is X0Y0Z0 of the sketch. Z is always zero since it is a 2D sketch.

The location of X0Y0Z0 on the Base sketch is a very important. You should pick its location on sketch carefully since it dictates the location of X0Y0Z0 on the completed model. See Figure 4-7.

Figure 4-7
X0Y0 Origin Location

The Coordinate System Indicator shows the X, Y, and Z axis. The arrows always point in the positive X, Y, and Z direction. The red arrow is the X axis , the green arrow is the Y axis, the blue arrow is the z axis. See Figure 4-8 and 4-9.

Figure 4-8
Coordinate System Indicator

Figure 4-9
The Graphic window in 2D Sketch Mode [Click to see image full size]

AUTHOR’S COMMENTS: Your Graphic window should appear black as shown in the upper figure below while the Graphic window figures shown in future modules in the Inventor book will have a white background as shown in the lower figure. I used the white background in the book because they displays better.

[Click to see image full size]

[Click to see image full size]

WORK ALONG: Drawing the Base Sketch

Step 1

Start Inventor. Ensure that the current project is Inventor Course.

Step 2

Click the NEW command and start a new part using the template: English-Modules Part (in).ipt.

Step 3

Change to Model mode by clicking in the Finish sketch icon.

Step 4

Save the part file with the name: Inventor Workalong 04-1. The Graphic window should appear similar to the figure. (Figure Step 4)

Figure Step 4 [Click to see image full size]

Step 5

Change to Sketch mode by right clicking Sketch1 in the Browser bar and click Edit Sketch. (Figure Step 5A and 5B)

Figure Step 5A

Figure Step 5B [Click to see image full size]

Step 6

The 3D model that you are constructing in this workalong is shown in the figure. (Figure Step 6A)

Figure Step 6A

Figure Step 6B

Step 7

Press F6 to change to the Home view. (Figure Step 7)

Figure Step 7 [Click to see image full size]

Step 8

Click the PROJECT GEOMETRY command. Note the Status bar, it displays the command prompt. Expand the Origin folder in the Browser bar and click Center Point. Press Esc to end the command and note that after you do that, the Status bar displays the Ready prompt. That means there is no current command. (Figure Step 8A, 8B, 8C, and 8D)

Figure Step 8A

Figure Step 8B

Figure Step 8C

Figure Step 8D

Step 9

Click the LOOK AT command. Move the cursor onto the Browser bar and click the XY Plane. The Graphic window will change to display the top view. Press Esc to end the command. (Figure Step 9A, 9B, and 9C)

Figure Step 9A

Figure Step 9B

Figure Step 9C [Click to see image full size]

Step 10

Press F8. It enables the display of the geometrical constraint icons. To this point, there is only one geometrical constraint applied to sketch. It is the Reference constrain that was applied when you projected the Center Point using the PROJECT GEOMETRY command in Step 8. (Figure Step 10)

Figure Step 10

Step 11

Press F9 to disable the display of the geometrical constraint icons.

Step 12

Move the cursor somewhere in the Graphic window and right click the mouse. In the Right-click menu, ensure that Snap to Grid is enabled. (Figure Step 12)

Figure Step 12

Step 13

Click the LINE command. Note the Status bar prompt. Move the cursor to X0Y0Z0 and hold it there. A green snap point will display. That means it is snapping to the Center Point geometry that was projected in Step 8. While the green snap point is displayed, click the left mouse button. (Figure Step 13A, 13B, and 13C)

Figure Step 13A

Figure Step 13B

Figure Step 13C

Step 14

Move the cursor about 4 inches along the positive X axis. Watch the Status bar and it will display the length of the line as the cursor is moved. When it is about 4 inches long and the Horizontal geometrical constraint symbol and the yellow snap point displays, click the left mouse button. (Figure Step 14A and 14B)

Figure Step 14A

Figure Step 14B

Step 15

Move the cursor about 2 inches in the positive Y direction. When the Perpendicular geometrical constraint symbol displays at the same time as the yellow grid snap point, click the left mouse button. (Figure Step 15A and 15B)

Figure Step 15A

Figure Step 15B

Step 16

Move the cursor about 2 inches in the negative X direction. When the Perpendicular constraint symbol displays and the yellow snap grid point displays, click the left mouse button. (Figure Step 16A and 16B)

Figure Step 16A

Figure Step 16B

Step 17

Move the cursor about 2 inches in the positive Y direction. When the Parallel constraint symbol and the yellow snap grid point displays, click the left mouse button. (Figure Step 17A and 17B)

Figure Step 17A

Figure Step 17B

Step 18

Move the cursor about 2 inches in the positive X direction. When the Perpendicular constraint symbol and the yellow snap grid point displays, click the left mouse button. (Figure Step 18A and 18B)

Figure Step 18A

Figure Step 18B

Step 19

Move the cursor about 2 inches in the positive Y direction. When the Perpendicular constraint symbol and the yellow snap grid point displays, click the left mouse button. (Figure Step 19)

Figure Step 19

Step 20

Move the cursor about 4 inches in the negative X direction. When the Perpendicular constraint symbol and the yellow snap grid point displays, on the Y axis, click the left mouse button. (Figure Step 20)

Figure Step 20

Step 21

Move the cursor to X0Y0Z0. When the green snap point and the Perpendicular constraint symbol displays, click the left mouse button. (Figure Step 21)

Figure Step 21

Step 22

Press Esc to end the LINE command. Note that the Status bar prompts Ready meaning there is no current command. (Figure Step 22)

Figure Step 22

MUST KNOW: When the Snap to Grid feature is enabled, the points selected will snap to locations on the grid. As a beginner, it is best to draw by snapping to the grid to control the location and size of the sketch.

Step 23

Click the LOOK AT command and change the view to the top or XY plane. If you have trouble, see Step 9.

Step 24

Press F8 to display the geometrical constraint icons. They should appear similar to the figure. (Figure Step 24)

Figure Step 24

Step 25

Move the cursor onto the Horizontal geometrical constraint icon. Note how the bottom line display red to indicate that the constraint is applied to that line. (Figure Step 25)

Figure Step 25

Step 26

Move the cursor onto a Parallel geometrical constraint icon and note how another Parallel geometrical constraint icon will highlight showing you which two icons match one another. Note how the two parallel lines will also highlight to indicate that the upper line is constrained to the lower line with a Parallel geometric constraint. (Figure Step 26)

Figure Step 26

Step 27

Move the cursor onto the Perpendicular geometrical constraint icon. Note how the two lines highlight. The vertical line is constrained perpendicular to the horizontal line. (Figure Step 27)

Figure Step 27

Step 28

Move the cursor onto the small square icon at the bottom right corner of the object. Note how two Coincident geometrical constraint icons will display indicating both line’s endpoints are at the exact same XY location. (Figure Step 28)

Figure Step 28

Step 29

Press F9 to disable the display of the geometrical constraint icons. Press F6 to display the Home view. The completed sketch should appear as shown in the figure. (Figure Step 29)

Figure Step 29 [Click to see image full size]

Step 30

Return to Model mode.

Step 31

Save and close the file.

AUTHOR’S COMMENTS: The final sketch is shown in black as your screen should. Note that two lines are purple and the remainder are blue. If the two lines do not display purple, redo the workalong. You will learn the importance of this in Module 5.

[Click to see image full size]

Deleting Lines

There are two methods to delete any unwanted drawing object.

Method 1

Ensure that there is no active command and without entering a command, select the drawing object with the cursor. If it is successfully selected, it will change colour. Right click the mouse. In the Right-click menu, click Delete as shown in Figure 4-9.

Figure 4-9
Deleting Lines

Method 2

Select the drawing object the same way as in Method 1. When the selected object changes colour, press the Delete key on the keyboard.

Key Principles

Lab Exercise 4-1

Time allowed: 40 minutes.

Step 1

Start a new part file with the template: English – Modules Part(in).ipt save the file with the name: Inventor Lab 04-1 as shown above.

Step 2

Project the Center Point onto the Base sketch.

Step 3

Draw the Base sketch for the 3D model shown below and apply all of the necessary geometrical constraints. Note the location of X0Y0Z0. (Figure Step 3A and 3B)

Figure Step 3A

Figure Step 3B
Base Sketch

AUTHOR’S GEOMETRIC CONSTRAINS: The following figure shows the Base sketch’s geometric 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 different construction methods and constraints, that is what is important. You may want to compare your construction method and constraints used with the authors.

Author’s Base Sketch

Lab Exercise 4-2

Time allowed: 40 minutes.

Step 1

Start a new part file with the template: English – Modules Part(in).ipt and save the file with the name: Inventor Lab 04-2 as shown above.

Step 2

Project the Center Point onto the Base sketch.

Step 3

Draw the Base sketch for the 3D model shown below and apply all of the necessary geometrical constraints. Note the location of X0Y0Z0. (Figure Step 3A and 3B)

Figure Step 3A

Figure Step 3B Base Sketch

AUTHOR’S GEOMETRIC CONSTRAINS: The following figure shows the Base sketch’s geometric 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 different construction methods and constraints, that is what is important. You may want to compare your construction method and constraints used with the authors.

Author’s Base Sketch

Dimensional Constraints

Unlike geometrical constraints, that are used to apply geometrical relationships between the objects in the sketch, dimensional constraints control and report the size of the geometry. Dimensional constraints are sometimes called parametric dimensions. 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 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.

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.

A driven dimension 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.

Base Model

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 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.

The Base Sketch

The Extrusion

The Base Model
Figure 5-1

Dimensioning Sketches

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.

Linear Dimensions

A linear dimension is a dimension measuring the delta X or the delta Y 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.

Fig 5-2
Linear Dimensions Applied to
Horizontal and Vertical Lines

Object Linear Dimensions

To insert an object linear dimension, 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.

Figure 5-3 Object Linear Dimension Icon

WORK ALONG: Dimensioning and Extruding the Base Sketch

Step 1

Using the OPEN command, open the part file: Inventor Workalong 04-1 that you completed in Module 4.

Step 2

Change to Sketch mode by editing Sketch1 in the Browser bar. Press F6 to change the view to the Home view. (Figure Step 2)

Figure Step 2

Step 3

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)

Figure Step 3A

Figure Step 3B

Step 4

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)

Figure Step 4

Step 5

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)

Figure Step 5

Step 6

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)

Figure Step 6A

Figure Step 6B

Figure Step 6C

Figure Step 6D

Step 7

When complete, there should be six driving dimensions. (Figure Step 7)

Figure Step 7

Step 8

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)

Figure Step 8A

Figure Step 8B

Step 9

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)

Figure Step 9A

Figure Step 9B

Step 10

The completed sketch should appear as shown in the figures. (Figure Step 10A, 10B, and 10C)

Figure Step 10A

Figure Step 10B

Figure Step 10C

Step 11

Press F6 to change to the Home view. (Figure Step 11)

Figure Step 11

Step 12

Click the LOOK AT command and change the view to the top or XY plane.

Step 13

Press F8 to display the geometrical constraint icons. You figure should appears similar as shown in the figure. (Figure Step 13)

Figure Step 13

Step 14

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)

Figure Step 14A

Figure Step 14B [Click to see image full size]

Step 15

The completed solid model should now appear as shown in the figure. (Figure Step 15)

Figure Step 15

Step 16

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

Figure Step 16A

Figure Step 16B

Step 17

In the Appearance pull-down menu, select the color: Aluminum Polished as shown in the figure. (Figure Step 17)

Figure Step 17

Step 18

The completed part or model should appear as shown in the figure. (Figure Step 18)

Figure Step 18

Step 19

Save and close the part file.

MUST KNOW: 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.

Driving Dimension

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.

Driven Dimension

USER TIP: 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.

[Click to see image full size]

USER TIP: Click the bottom right arrow and enable Pin Mini-Toolbar Position and Auto Fade.

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.

[Click to see image full size]

MUST KNOW: Knowing When the Sketch is Fully Constrained 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.

Sketch Partially Constrained

Sketch Fully Constrained

A special Pinned icon will display in Browser bar on sketches that are fully constrained as shown to the figures.

Key Principles

Lab Exercise 5-1

Time allowed: 40 minutes.

Step 1

Open the file: Inventor Lab 04-1.ipt that you saved in Lab Exercise 4-1 in Module 4.

Step 2

Using the SAVEAS command, save the file with the name: Inventor Lab 05-1.ipt.

Step 3

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

Figure Step 3A
3D Model

Figure Step 3B
Base Sketch Dimensioned

Figure Step 3C
The Base Sketch Fully Constrained [Click to see image full size]

Step 4

Extrude the sketch to create the Base model and apply the colour shown above. (Figure Step 4)

Figure Step 4
Completed
3D Solid Model
Home View

AUTHOR’S GEOMETRIC CONSTRAINTS: 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.

[Click to see image full size]

Lab Exercise 5-2

Time allowed: 40 minutes.

Step 1

Open the file: Inventor Lab 04-2.ipt that you saved in Lab Exercise 4-2 in Module 4.

Step 2

Using the SAVEAS command, save the file with the name: Inventor Lab 05-2.ipt.

Step 3

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

Figure Step 3A
3D Mode

Figure Step 3B
Base Sketch Dimensioned [Click to see image full size]

Figure Step 3C
Base Sketch Fully Constrained [Click to see image full size]

Step 4

Extrude the sketch to create the Base model and apply the colour shown above. (Figure Step 4)

Figure Step 4
Completed 3D Solid Model
Home View

AUTHOR’S GEOMETRIC CONSTRAINS: 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.

[Click to see image full size]

The Inventor book was written with competency based modules. What that means is that you have not completed each module until you have mastered it. The Competency Test module contains multiple choice questions and a comprehensive lab exercise to test your mastery of the set of modules that you completed. There are no answers or keys supplied in a Competency Test module since it is meant to be checked by your instructor. If there are any parts of this module that you have trouble completing, you should go back and reread the module or modules containing the information that you are having trouble with. If necessary, redo as many lab exercises required until you fully understand the material.

If you are Completing this book:

• Without the aid of an instructor, complete the written test and the lab exercise.
• In a classroom with an instructor, the instructor will give instructions on what to do after you have completed this module.

Multiple Choice Questions

Select the BEST answer.

1. What keyboard key is used to end the current command?
   1. CTRL
   2. TAB
   3. ESC
   4. SHIFT
   5. ENTER
2. An Inventor _______________is designed to logically organize, store and manage the valid links to the files that are created for each undertaking.
   1. 3D Model
   2. Project
   3. Design
   4. 2D Sketch
   5. Menu
3. What command is used to zoom the model or the 2D sketch to display the complete model or sketch in the graphic window?
   1. ZOOM
   2. PAN
   3. ISOMETRIC
   4. ZOOM ALL
   5. LOOK AT
4. What are all files created in Inventor called?
   1. Designs
   2. Drawings
   3. Files
   4. 3D Models
   5. 2D Sketches
5. What command is used to change the viewing position of the model or sketch to a known home view or isometric view?
   1. ZOOM
   2. PAN
   3. HOME VIEW
   4. ZOOM ALL
   5. LOOK AT
6. What is the name of the Inventor file that must be used by the operator when creating any new file?
   1. Design file
   2. Drawing file
   3. Model file
   4. Template file
   5. Sketch file
7. What term describes the process of applying geometrical relationships of objects to one another in a 2D sketch?
   1. Object snapping
   2. Dimensional constraints
   3. Parametric solid modeling
   4. Driven dimensions
   5. Geometrical constraints
8. What file extension is assigned to a part file?
   1. .IPT
   2. .IJP
   3. .IAM
   4. .IDW
   5. .IPN
9. When drawing a base sketch that must be extruded to create the solid model there is a list of rules that should be used. Which one of the following rules is false?
   1. Select the view with the most complex contour shape.
   2. Draw the lines using dimensions close to finished dimensions.
   3. The objects in the sketch must meet at their endpoints and cannot overlap.
   4. The objects in the sketch must have geometrical constraints applied to control the shape.
   5. The objects in the sketch cannot be a closed polygon.
10. What term describes the process of controlling and reporting the size of the geometry in a 2D sketch?
    1. Object snapping
    2. Dimensional constraints
    3. Parametric solid modeling
    4. Driven dimensions
    5. Geometrical constraints

Lab Exercise 6-1

Time allowed: 60 minutes.

Step 1

Start a new part file with the template: English- Modules Part(in).ipt, and save the file with the name: Inventor Lab 06-1, as shown above.

Step 2

Project the Center Point onto the Base sketch.

Step 3

Draw the Base sketch for the object shown in the figure and apply all of the necessary geometrical constraints to maintain the shape of the sketch. Note the location of X0Y0Z0. (Figures Step 3A and 3B)

Figure 3A
Base Sketch [Click to see image full size]

Figure Step 3B
3D Model [Click to see image full size]

Step 4

Insert the necessary driving dimensions to fully constrain the sketch. Add at least 1 driven dimension.

Step 5

Ensure that the sketch is fully constrained and all lines display purple. (Figure Step 5)

Figure Step 5
Fully Constrained Base Sketch [Click to see image full size]

Step 6

Extrude the sketch to complete the Base model and apply the color: Aluminum – Flat (Figure Step 6)

Figure Step 6
Completed Solid Model – Home View

Point to Point Linear Dimensions

A point to point linear dimension is a dimension measuring the delta X or the delta Y distance between two points of an existing object or objects. The points, which are normally the endpoints of a line, could also be centre points of circles or arcs as you will see in future modules. If the points both lie on the same X or Y axis, the dimension can only inserted in one direction. If the points do not lie on the same axis, you have the choice of inserting either the delta X or the delta Y dimension. See Figure 7-1. The three steps used to insert a point to point linear dimension are shown below.

Figure 7-1
Linear Dimensions Applied To an Inclined Line

Step 1

Step 2

Step 3

WORK ALONG: Constructing a Solid Model Using Multiple Sketches

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Enter the NEW command to start a new part file using the template: Metric-Modules Part (mm).ipt.

Step 3

Save the file with the name: Inventor Workalong 07-1. (Figure Step 3A and 3B)

Figure Step 3A
Solid Model – Home View

Figure Step 3B
Solid Model – Rotated View

Step 4

Edit Sketch 1 and enter the PROJECT GEOMETRY command and project the Center Point onto the sketching plane. Press Esc to exit the command. (Figure Step 4)

Figure Step 4

Step 5

Draw the Top view of the model starting at X0Y0Z0. This is the Base sketch. (Figure Step 5)

Figure Step 5

Step 6

Add 4 driving dimensions to fully constrain the sketch. Add 2 driven dimensions.

Step 7

Press F8 to display the constraints. (Figure Step 7)

Figure Step 7

Step 8

The sketch should now be fully constrained and all the lines display purple on a black background. (Figure Step 8)

Figure Step 8

Step 9

Press F6 to change the view to the Home view. Click the FINISH SKETCH command to return to Model mode. (Figure Step 9)

Figure Step 9

Step 10

Enter E to execute the EXTRUDE command and extrude the model 100 mm in the positive Z direction. (Figure Step 10)

Figure Step 10 [Click to see image full size]

Step 11

The solid model should appear as shown in the figure. (Figure Step 11)

Figure Step 11

Step 12

Click the 2D SKETCH icon and when prompted, select the right side plane as shown in the figure. Exit the command and the grid will display on the plane in Sketch mode. Press F6 to change to the Home view. (Figure Step 12A, 12B, and 12C)

Figure Step 12A

Figure Step 12B

Figure Step 12C

Step 13

Enter L for the LINE command and start the first endpoint of the line by snapping onto the plane edge line. (Figure Step 13)

Figure Step 13

Step 14

Draw three lines, applying perpendicular geometrical constraints and snapping back onto the edge. Guess at the length of the lines making them approximately the correct length. (Figure Step 14)

Figure Step 14

Step 15

Press F8 to display the constraint icons. (Figure Step 15)

Figure Step 15

Step 16

Enter D for the GENERAL DIMENSION command. Move the cursor to bottom corner of the model. When a small point highlights, click the mouse. (Figure Step 16)

Figure Step 16

Step 17

For the second point of the dimension, click the end of the line as shown in the figure. Locate and set the dimension to 25. (Figure Step 17A and 17B)

Figure Step 17A

Figure Step 17B

Step 18

Add two additional dimensions to fully constrain it. (Figure Step 18A, 18B, and 18C)

Figure Step 18A

Figure Step 18B

Figure Step 18C

Step 19

Enter E for the EXTRUDE command. (Figure Step 19)

Figure Step 19 [Click to see image full size]

Step 20

Set the Extents to To, the type to Cut and select the back face to locate where to extrude to. (Figure Step 20)

Figure Step 20 [Click to see image full size]

Step 21

Your model should appear as shown in the figure. (Figure Step 21)

Figure Step 21

Step 22

Click the 2D Sketch icon and select the top plane to start a new sketch. Orbit the model to match the figure. (Figure Step 22)

Figure Step 22

Step 23

On the sketch, draw a line across the corner. Make sure that you snap both ends of the line to the edges. Guess at the distance from the corner. (Figure Step 23)

Figure Step 23

Step 24

Draw a line on the opposite side and dimension both lines using four point to point dimensions. (Figure Step 24)

Figure Step 24 [Click to see image full size]

Step 25

Your sketch should be fully constrained as shown in the figure. (Figure Step 25)

Figure Step 25 [Click to see image full size]

Step 26

Press F8 to display the constraint icons. (Figure Step 26)

Figure Step 26 [Click to see image full size]

Step 27

Extrude the sketch using the To Next extents. Select the two profiles to extrude and ensure that you enable the Cut icon. (Figure Step 27)

Figure Step 27 [Click to see image full size]

Step 28

Change to the Home view by pressing F6. Change the colour of the completed model to color: Light Steel Blue. (Figure Step 28)

Figure Step 28

Step 29

Expand the Browser bar. You can see that the model hierarchy shows the three sketches and an extrusion of each one. (Figure Step 29)

Figure Step 29

Step 30

Save and close the file.

Key Principles

Lab Exercise 7-1

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the sketching plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
3D Model

Figure Step 2B
Suggested Base Sketch

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3
Completed Solid Model – Home View

AUTHOR’S GEOMETRIC CONSTRAINS: The following three figures shows the base and additional 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 sketches using different construction methods and constraints, that is what is important. You may want to compare your construction method and constraints used with the authors.

Author’s Base Sketch

Author’s Sketch

Author’s Sketch

Lab Exercise 7-2

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the base sketching plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A, 2B, and 2C)

Figure Step 2A
3D Model – Home View

Figure Step 2B
A Rotated View of the 3D Model

Figure Step 2C
Suggested Base View

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3
Completed Solid Model – Home View

Step 4

Save the file with the name: Inventor Lab 07-2 as shown above.

Author’s Base Sketch [Click to see image full size]

Author’s Sketch

Author’s Sketch

NOTE: If you understand multiview drawings, object lines, hidden lines, and you can draw the three standard views of an object, skip this module.

Multiview Drawing

The drafting and design world uses a system of representing a three- dimensional object by drawing two-dimensional views. It is called a multiview drawing. To explain this system of drawing, the object shown in Figure 8-1 will be used in this module. To draw a two-dimensional view of one side of the object, place a imaginary plane parallel to the side and project the view of the object perpendicular onto the plane. This is called orthographic projection. Imagine the plane to a sheet of glass. See Figure 8-2.

Figure 8-1
The 3D Model

Figure 8-2
Projecting the
Two-Dimensional View

The Glass Box Principle

To carry this principal further, place a plane on each side of the object for a total of six planes or sheets of glass to form a glass box. This is called the Glass Box Principle, see Figure 8-3. Picture unfolding the glass box onto a flat two-dimensional plane as shown in Figure 8-4. All six views are now visible at the same time.

Figure 8-3
The Glass Box Principle

Figure 8-4
The Glass Box Unfolded [Click to see image full size]

The Three Standard Views

In almost all objects, three views are adequate to describe it. In fact, there are many objects that only need two views and some that only need one view to describe it. The six views are Top, Front, Right Side, Left Side, Rear, and Bottom. The three standard views are the Top, Front, and Right Side. They must be drawn in the positions shown in Figure 8-5 and they must be aligned.

Figure 8-5
The Three Standard Views

Picking the Standard Three Views

The three standard views are always selected as shown in Figure 8-6.

Figure 8-6
Picking the Three Standard Views

Drawing the Views

Usually it is best to draw the view with the most irregular shape first and then project lines to the other two views. For the object in Figure 8-7, the front view should be drawn first and then the top and right side views are projected. Notice how the views have to align. Figure 8-7 shows two different methods of projecting lines from the top view to the right side view or vise versa. The distance between the views is not important.

Figure 8-7
Two Methods for View Layout and Alignment

Drafting Lesson Object and Hidden Lines

Lines and features that can be seen in the views are drawn with continuous or solid lines. They are called object lines. Even though they are called object lines, they can be circular in shape. To completely describe an object in a multiview drawing, the drafter must also show all lines or features that are hidden in that view. They are called hidden lines and their linetype is dashed. Study the multiview drawing below and take note how the holes going through the object are shown with hidden lines. See Figures 8-8 and 8-9.

Figure 8-8
The Model

Figure 8-9
The Multiview Drawing of the Model

Key Principles

Lab Exercise 8-1

Time allowed: 15 minutes.

Step 1

Sketch the Top, Front and Right Side views of the Object 8-1.

Step 2

Use one grid on the model equal to one grid on the drawing. See the example.

Step 3

When complete, check your answers at the end of this chapter.

Example

Object 8-1

Lab Exercise 8-2

Time allowed: 60 minutes.

Step 1

Sketch the Top, Front, and Right Side views of each model.

Step 2

Use one grid on the model equal to one grid on the drawing.

Step 3

Check your answers at the end of this chapter. Do not look at the answers until you have completed your sketch.

Object 8-2

Object 8-3

Object 8-4

Object 8-5

Object 8-6

Visualizing 3D Models

In the first six modules, all of the wireframe models that you constructed were referenced to a given 3D view of the model. Since most technical drawings used in the drafting and design world are 2D multiview drawings, 3D models must be able to be drawn using a multiview drawing as a reference to find the model’s shape and dimensions. To construct a 3D model, you must be able to mentally visualize the 3D model using a multiview drawing as a reference.

.A good way for you to learn to visualize a 3D model from a 2D multiview drawing is to first draw the model as an isometric drawing. By doing this, it is easier to form a mental image from the multiview drawing. After practicing this for while, you will be able to visualize and construct 3D models without drawing the isometric first.

Figure 9-1
An Isometric Drawing

An isometric drawing is a 2-dimensional drawing that has the XYZ axis drawn at 120 degrees apart as shown in Figure 9-1. In this module, drawing the isometric on an isometric grid will be taught. An isometric grid has the grid lines drawn at 120 degrees as shown in Figure 7-2. Figure 9-3 shows a rectangular box drawn on the isometric grid.

Figure 9-2
An Isometric Grid

Figure 9-3
A Rectangular Box Drawn on an Isometric Grid

WORK ALONG: Sketching an Isometric Drawing of a 3D Model – Part 1

This workalong demonstrates how the multiview drawing of the 3D model, shown in Figure 9-4, is drawn as an isometric drawing.

Figure 9-4
Multiview Drawing

Step 1

Using a pencil and eraser, complete this workalong to create the isometric sketch of the 3D model. (Figure Step 1)

Figure Step 1

Step 2

Sketch the rectangular box using the length, width, and height of the overall size of the 3D model. The overall size of the 3D model is 6 grids long, 5 grids wide and 5 grids high. (Figure Step 2)

Figure Step 2

Step 3

Cut the shape away, one view at a time. Draw the Front view first. (Figure Step 3A and 3B)

Figure Step 3A

Figure Step 3B

Step 4

In the Right Side view, remove the top left side of the object to match the multiview’s right side view. (Figure Step 4)

Figure Step 4

Step 5

In the Top view, remove the bottom right corner to complete the isometric drawing. (Figure Step 5A and 5B)

Figure Step 5A

Figure Step 5B

WORK ALONG: Sketching an Isometric Drawing of a 3D Model – Part 2

This workalong demonstrates how the multiview drawing of the 3D model, shown in Figure 9-5, is drawn as an isometric drawing.

Figure 9-5
Multiview Drawing

Step 1

Using a pencil and eraser, complete this workalong to create the isometric sketch of the 3D model. (Figure Step 1)

Figure Step 1

Step 2

The figures show the necessary steps. Try to complete the isometric without looking at the figure. (Figure Step 2A, 2B, 2C, and 2D)

Figure Step 2A

Figure Step 2B

Figure Step 2C

Figure Step 2D

Key Principles

Lab Exercise 9-1

Time allowed: 90 minutes.

Step 1

Using the 4 multiview drawings shown below, using pencil and eraser and the graph paper you printed, sketch the isometric drawing of each 3D model.

Step 2

Using what was just taught, draw isometric drawings of the four objects: Object 9-1 to Object 9-4. For the answers, see the end of this chapter. Try to visualize the 3D model by looking at the multiview drawing and then draw the isometric. Do not look at the answers until you have done your best to complete the isometric drawing of each object.

Object 9-1

Object 9-2

Object 9-3

Object 9-4

Object 9-1

Object 9-2

Object 9-3

Object 9-4

Object 9-1

Object 9-2

Object 9-3

Object 9-4

2D Sketching Planes

Up to this point in the book, the Base sketch has been drawn on the XY plane. The XY plane is the Top view of the model and the default plane as configured in the templates that are being used to complete the workalongs and lab exercises in the Inventor book. The models that have been constructed up to this point in the modules were all designed so that the Base sketch was drawn on the XY plane or the Top view. In this module, learning how to construct solid models by drawing the Base sketch on either the front or right side planes will be taught.

Inventor has p three predefined planes that can be used to draw the Base sketch. They are the XY, XZ, and YZ planes. The XY plane is the Top view, the XZ plane is the Front view and the YZ is the Right Side view of the model.

Keep in mind the rule that was taught in Module 4. ‘ It is best to draw the Base sketch on the plane that has the most complex contour. Contours with arcs and curves should be avoided ‘.

The Three Predefined Planes

To help visualize the three predefined planes used in Inventor, the 3D model shown in Figure 10-1 is used in this module. The glass box principle that was taught in Module 8 is used to help you visualize Inventor’s three predefined planes. See Figure 10-2.

Figure 10-1
The 3D Model

Figure 10-2 The Glass Box

Consumed and Unconsumed Sketches

A consumed sketch is a 2D sketch that has been extruded or revolved to create a 3D solid model. An unconsumed sketch is a 2D sketch that is blank or one that has not been extruded or revolved.

The Browser bar will display which sketches have been consumed and which ones are unconsumed. See Figure 10-3. Sketch1 is unconsumed while Sketch2, Sketch3, and Sketch4 have been extruded and are consumed.

Figure 10-3
Consumed and Unconsumed Sketches

USER TIP: A 2D sketch can be drawn in the orthographic view or in the 3D Home view. In fact, any 3D orbited view can be used. When drawing in a 3D view, it is always best to draw in the Home view since this helps you maintain a good mental picture of the model.

2D Orthographic View

3D Home View

WORK ALONG: Working with 2D Sketching Planes

Step 1

Start a new part file using the template: English-Modules Part (in).ipt.

Step 2

In Sketch mode, press F6 to change to the Home view. The Graphic window and the Browser bar will appear as shown in the figure. (Figure Step 2)

Figure Step 2 [Click to see image full size]

Step 3

In the Browser bar, expand the folder: Origin as shown in the figure. Place the cursor on the XY Plane. Note the orientation of the plane on the sketch. (Figure Step 3)

Figure Step 3 [Click to see image full size]

Step 4

Place the cursor on the XZ Plane in the Browser bar. Note the orientation of the plane on the sketch. The XZ Plane is the Front view. (Figure Step 4)

Figure Step 4 [Click to see image full size]

Step 5

Place the cursor on the YZ Plane in the Browser bar. Note the orientation of the plane on the sketch. This is the Right Side view. (Figure Step 5)

Figure Step 5 [Click to see image full size]

Step 6

Place the cursor anywhere in the Graphic window and right click the mouse. In the Right-click menu, click Finish 2D Sketch.

Figure 10-3
3D Model – Home View

Figure 10-4
Dimensioned Multiview Drawing [Click to see image full size]

Step 7

Save the part file with the name: Inventor Workalong 10-1. In Model mode, expand the folder: Origin in the Browser bar and right-click the XZ plane. In the Right-click menu, click New Sketch as shown in figure. (Figure Step 7)

Figure Step 7 [Click to see image full size]

Step 8

The Graphic window will change to Sketch mode. Change to the Home view. Note that in the Browser bar a new sketch will appear and named Sketch2. (Figure Step 8)

Figure Step 8 [Click to see image full size]

Step 9

Project the Center Point onto the sketch plane. Draw the Base sketch for the model applying all of the necessary geometrical constraints to maintain the shape of the sketch. Note the location of X0Y0Z0. Insert the necessary driving dimensions to fully constrain the sketch. (Figure Step 9)

Figure Step 9 [Click to see image full size]

Step 10

Press PAGE UP key to execute the LOOK UP/VIEW FACE command. Select one of the lines to change the sketch to the 2D view of the the XZ plane. Press F8 to display the geometrical constraint icons. They should appear similar to the figure. (Figure Step 10)

Figure Step 10 [Click to see image full size]

Step 11

Right-click anywhere in the Graphic window. In the Right-click menu, click Finish 2D Sketch to return to Model mode. (Figure Step 11)

Figure Step 11

Step 12

Save the part with the name: Inventor Workalong 10-1. Extrude the sketch to create the solid model as shown in figure. (Figure Step 12)

Figure Step 12

Step 13

Using the 2D SKETCH command, or even better the shortcut S, start a new sketch and select the right side as the plane to draw it on. (Figure Step 13)

Figure Step 13

Step 14

The grid will display on the right side. It will be Sketch3 in the Browser bar. (Figure Step 14)

Figure Step 14

Step 15

Draw three lines for the slot. Apply all of the necessary geometrical and dimensional constraints to fully constrain the sketch. (Figure Step 15)

Figure Step 15 [Click to see image full size]

Step 16

Press F8 to enable the display of the constraint icons. They should be similar to the figure. (Figure Step 16)

Figure Step 16

Step 17

Press F9 to disable the display of the constraint icons. Extrude the sketch using the To next. (Figure Step 17)

Figure Step 17

Step 18

Start a new sketch on the top plane as shown in the figure. (Figure Step 18)

Figure Step 18

Step 19

Draw the 2D sketch on the new sketching plane and insert the necessary dimensions to fully constrain it. (Figure Step 19)

Figure Step 19 [Click to see image full size]

Step 20

Extrude the top sketch to complete the solid model. (Figure Step 20)

Figure Step 20

Step 21

Change the view to the Home view and apply the color: Chrome – Polished Black. Orbit the model to check the bottom. (Figure Step 21)

Figure Step 21

Step 22

Save and close the file.

Key Principles

Lab Exercise 10-1

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the base sketching plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2B
Suggested Base Sketch – Front XZ Plane

Step 3

Apply the colour as shown above. (Figure Step 3)

Figure Step 3 Completed Solid Model – Home View [Click to see image full size]

Author’s Base Sketch [Click to see image full size]

Author’s Sketch [Click to see image full size]

Author’s Sketch [Click to see image full size]

Lab Exercise 10-2

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the base sketching plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2B
Suggested Base Sketch – Right Side YZ Plane

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3 Completed Solid Model – Home View [Click to see image full size]

Author’s Base Sketch [Click to see image full size]

Author’s Sketch [Click to see image full size]

If you are Completing this book:

• Without the aid of an instructor, complete the written test and the lab exercise.
• In a classroom with an instructor, the instructor will give instructions on what to do after you have completed this module.

Multiple Choice Questions

Select the BEST answer.

1. What view of the model is the XZ plane in Inventor?
   1. Left Side
   2. Right Side
   3. Top
   4. Bottom
   5. Front
2. Which one of Inventor’s menus shows if a sketch is consumed or unconsumed?
   1. Status bar
   2. Standard menu
   3. Browser bar
   4. Panel bar
   5. 2D Sketch panel
3. What command is used to draw a 2D Sketch on the existing solid model?
   1. NEW
   2. LOOK AT
   3. 2D SKETCH
   4. EXTRUDE
   5. LINE
4. Which plane is the default plane used in the templates supplied with the Inventor book?
   1. ZY
   2. XZ
   3. XY
   4. YX
   5. YZ
5. Which of the following best describes a consumed 2D sketch?
   1. It is blank.
   2. It has been extruded or revolved to create a 3D feature.
   3. It has been deleted.
   4. It cannot be edited.
   5. It has been dimensioned.
6. In Figure 11-1, what is the purpose of the middle icon in the EXTRUDE dialogue box?
   
   

   Figure 11-1
   1. Cut
   2. Subtract
   3. Add
   4. Join
   5. Intersect
7. What kind of dimension does a linear dimension insert?
   1. Line
   2. Object
   3. Horizontal only
   4. Vertical only
   5. Delta X or Delta Y
8. What view of the model is the XY plane in Inventor?
   1. Left Side
   2. Right Side
   3. Top
   4. Bottom
   5. Front
9. On the colour scheme High Contrast, what colour will the sketch appear when it is fully constrained?
   1. Black
   2. White
   3. Purple
   4. Blue
   5. Green
10. What view of the model is the YZ plane in Inventor?
    1. Rotated
    2. Right Side
    3. Top
    4. Bottom
    5. Front

Lab Exercise 11-1 Part B

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the Base sketch.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. Ensure that all lines on all sketches display purple on a black background. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Drawing [Click to see image full size]

Figure Step 2B
Suggested Base View –
Front – XZ Plane

Step 3

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

Figure Step 3A
Completed Solid Model –
Home View

Figure Step 3A
Solid Model – Rotated View

Figure Step 3A
Solid Model – Rotated View

Geometry Lesson: Circles

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

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

Figure 12-1
Geometry of a Circle – Part 1 [Click to see image full size]

Figure 12-2
Geometry of a Circle – Part 2 [Click to see image full size]

Figure 12-3
Geometry of a Circle – Part 3 [Click to see image full size]

Figure 12-4
Geometry of a Circle – Part 4

Drafting Lesson: Reading Dimensions for Circles and Arcs

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

Arcs are dimensioned as radii. For example: 1.5 R

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

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

Figure 12-5
Typical Drawing

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

There are two methods of creating construction objects as follows:

Method 1

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

Figure 12-6

Method 2

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

Figure 12-7
Construction Objects

WORK ALONG: Drawing Circles and Cylindrical Models

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Enter the NEW command to start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 12-1. (Figure Step 3A and 3B)

Figure Step 3A
3D Model
Home View [Click to see image full size]

Figure Step 3B
Dimensioned Multiview Drawing [Click to see image full size]

Step 4

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

Step 5

Project the Center Point onto the sketching plane.

Step 6

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

Figure Step 6

Step 7

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

Figure Step 7A

Figure Step 7B

Figure Step 7C [Click to see image full size]

Step 8

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

Figure Step 8

Step 9

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

Figure Step 9

Step 10

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

Figure Step 10A

Figure Step 10B [Click to see image full size]

Step 11

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

Figure Step 11 [Click to see image full size]

Step 12

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

Figure Step 12 [Click to see image full size]

Step 13

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

Figure Step 13

Step 14

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

Figure Step 14

Step 15

Click the Construction icon to disable it.

Step 16

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

Figure Step 16A

Figure Step 16B [Click to see image full size]

Figure Step 16C [Click to see image full size]

Figure Step 16D [Click to see image full size]

Step 17

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

Figure Step 17 [Click to see image full size]

Step 18

Dimension one circle only. (Figure Step 18)

Figure Step 18 [Click to see image full size]

Step 19

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

Figure Step 19

Step 20

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

Figure Step 20A [Click to see image full size]

Figure Step 20B [Click to see image full size]

Step 21

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

Figure Step 21 [Click to see image full size]

Step 22

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

Figure Step 22 [Click to see image full size]

Step 23

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

Figure Step 23A [Click to see image full size]

Figure Step 23B

Step 24

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

Figure Step 24

Step 25

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

Figure Step 25 [Click to see image full size]

Step 26

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

Figure Step 26

Step 27

Save and close the file.

Key Principles

Lab Exercise 12-1

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the Base plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Solid Model – Home View

Figure Step 2B
Dimensioned Multiview Drawing [Click to see image full size]

Step 3

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

Figure Step 3A
Solid Model – Home View

Figure Step 3B
Suggested Base Sketch –
Front – XZ Plane

Hint:

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

AUTHOR’S GEOMETRIC CONSTRAINTS: The following figures shows the sketch’s construction method plus geometric and dimensional constraints suggested by the author to help you learn how to construct and constrain sketches. It is only the suggested method and if you can complete a fully constrained sketch using a different construction method and constraints, that is what is important. You may want to compare your construction method and constraints with the authors.

Base Sketch [Click to see image full size]

Sketch 2 [Click to see image full size]

Lab Exercise 12-2

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the base plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2B
Suggested Base Sketch –
Front – XZ Plane [Click to see image full size]

Hint

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

Step 3

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

Figure Step 3A
Completed Solid Model – Home View [Click to see image full size]

Figure Step 3B
Completed Solid Model – Bottom View [Click to see image full size]

Drawing Arcs

There are three commands available to draw arcs in Inventor. In this module, drawing arcs using the CENTER POINT ARC command will be taught. Similar to the CIRCLE command, the CENTER POINT ARC command also requires you to select the centre point and the radius. Drawing arcs additionally require you to locate the start point and end point or the arc. Arcs can be constructed clockwise or counterclockwise.

Geometry Lesson: Arcs

An ARC is defined as an open curve in which all points are the same distance from its centre point. Study the drawings in Figure 13-1 and 13-2.for a description of the geometry of an arc.

Figure 13-1
Geometry of an Arc – Part 1

Figure 13-2
Geometry of an Arc – Part 2

WORK ALONG: Drawing Models with Arcs

Step1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Enter the NEW command to start a new part file using the template: Metric-Modules Part (mm).ipt.

Step 3

Save the file with the name: Inventor Workalong 13-1. (Figure Step 3A and 3B)

Figure Step 3A
3D Model – Home View [Click to see image full size]

Figure Step 3B
Dimensioned Multiview Drawing [Click to see image full size]

Step 4

Edit Sketch1. Project the Center Point onto the sketch.

Step 5

Draw a sketch of the Top view of the model. Apply all of the geometrical and dimensional constraints to fully constrain it. (Figure Step 5)

Figure Step 5 [Click to see image full size]

Step 6

Extrude the sketch in the positive Z direction. (Figure Step 6)

Figure Step 6

Step 7

Start a new sketch on the right side as shown in the figure. (Figure Step 7)

Figure Step 7

Step 8

Enter the CENTER POINT ARC command and when prompted for the centre point, right click the mouse. In the Right-click menu, select Midpoint. (Figure Step 8)

Figure Step 8

Step 9

Move the cursor onto the vertical edge. When the green snap icon appears, click the left mouse button. (Figure Step 9)

Figure Step 9

Step 10

Move the cursor approximately 10 mm along the edge and when the Snap onto icon displays, click the mouse. (Figure Step 10)

Figure Step 10

Step 11

Move the cursor to the other side of the centre and when the Snap onto icon displays, click the mouse. (Figure Step 11)

Figure Step 11

Step 12

Press F8 to display the constraint icons. (Figure Step 12)

Figure Step 12

Step 13

Move the cursor onto the Coincident icon and note the display of two coincident icons. (Figure Step 13)

Figure Step 13

Step 14

In the Graphic window, right click the mouse. In the Right-click menu, click Create Constraint and then Coincident. (Figure Step 14)

Figure Step 14

Step 15

Select the edge for the first point. (Figure Step 15)

Figure Step 15

Step 16

For the second point, move the cursor onto the endpoint of the arc. When a small red point will displays, click the mouse. (Figure Step 16)

Figure Step 16

Step 17

Press F8. Locate the cursor onto the Coincident icon and note the display of two coincident icons. (Figure Step 17)

Figure Step 17

Step 18

The arc should now display purple indicating it is fully constrained. (Figure Step 18)

Figure Step 18

Step 19

Finish the sketch and extrude the arc by using the Cut option. (Figure Step 19)

Figure Step 19 [Click to see image full size]

Step 20

Start a new sketch on the front side. (Figure Step 20)

Figure Step [Click to see image full size]

Step 21

Draw a line perpendicular from the midpoint of the edge. (Figure Step 21)

Figure Step 21

Step 22

Change the line to a construction line by selecting the line and then click the Construction icon. (Figure Step 22A, 22B, and 22C)

Figure Step 22A

Figure Step 22B

Figure Step 22C

Step 23

Offset the construction line on each side. (Figure Step 23)

Figure Step 23

Step 24

Insert two dimensions. (Figure Step 24)

Figure Step 24

Step 25

Draw an arc locating the centre at the end of the construction line. (Figure Step 25)

Figure Step 25

Step 26

Insert the required dimensions to constrain the sketch. (Figure Step 26)

Figure Step 26

Step 27

Enable the display of the constraint icons. (Figure Step 27)

Figure Step 27

Step 28

Use what you learned in Step 14 to 17, create the additional Coincident constraints to fully constrain the sketch. (Figure Step 28)

Figure Step 28

Step 29

Extrude the sketch to complete the model. (Figure Step 29)

Figure Step 29

Step 30

Change the colour to: Titanium – Polished. (Figure Step 30).

Figure Step 30

Step 31

Save and close the file.

Key Principles

Lab Exercise 13-1

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the Base sketch.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2B
Suggested Base Sketch
– Right Side – YZ Plane

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3 Solid Model – Home View

Lab Exercise 13-2

Time allowed: 45 minutes.

Step 1

Project the Center Point onto the Base sketch.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2B
Suggested Base Sketch –
Front – XZ Plane

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3
Completed Solid Model –
Home View

Revolving

When drawing symmetrical objects it is much easier to create the model by revolving the Base sketch around an axis rather then extruding it. The axis, which can be one of the lines in the sketch or a centerline, must always be located in the centre of the symmetrical model. The sketch can be revolved any angle between 0 and 360 degrees.

In this module, the basic features of the REVOLVE command are taught. The Inventor Advanced book will cover the more advanced features.

The models in Figure 14-1 and 14-2 were created by revolving the same Base sketch around an axis. Take note how the two solid models that were created using the same sketch are quite different. In Figure 14-1, the line on left side of the sketch was used as the axis while in Figure 14-2, it was the centerline that was used as an axis or revolution.

Figure 14-1
A 2D Sketch Revolved Around a
Line in the Sketch

Figure 14-2
The Same 2D Sketch Revolved
around a Centerline

Centerlines

A centerline is a line with its properties set to act as a centerline. In the REVOLVE command, a centerline is automatically recognized as the axis for the revolution. The two methods of drawing a centerline, which is similar to drawing construction a line, are as follows:

Method 1

Draw the line using the LINE command and then select it. While it is selected, click the Centerline icon.

Method 2

Enable the Centerline icon and then draw the line, using the LINE command. The Centerline icon is shown in Figure 14-3. A centerline will display as the centerline linetype.

Figure 14-3
Centerline Icon

WORK ALONG: Revolving a Sketch Without using a Centerline

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Using the NEW command, start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 14-1. (Figure Step 3A and 3B)

Figure Step 3A
3D Model

Figure Step 3B
Dimensioned Multiview Drawing [Click to see image full size]

Step 4

Start a new sketch on the Front or XZ Plane. Project the Center Point onto the sketch.

Step 5

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

Figure Step 5

Step 6

In Model mode, enter the REVOLVE command. It will highlight the sketch automatically as the area to revolve. (Figure Step 6)

Figure Step 6 [Click to see image full size]

Step 7

In the Revolve dialogue box, set the Extents to Full and enable the Axis icon. Select the line on the right side of the sketch as the axis. The Full setting means that it will be revolved 360 degrees. (Figure Step 7)

Figure Step 7 [Click to see image full size]

Step 8

After you select the axis, the REVOLVE command will display the Base model as it is revolved. If this is the desired outcome, click OK. (Figure Step 8A and 8B)

Figure Step 8A [Click to see image full size]

Figure Step 8B

Step 9

Start a new sketch on the top plane of the model. (Figure Step 9)

Figure Step 9

Step 10

Using what you learned in Module 12, draw a construction circle and four construction lines. Insert a dimension for the diameter of the circle. Ensure that the sketch is fully constrained. (Figure Step 10)

Figure Step 10

Step 11

Using the technique that you learned in Module 12, draw the 4 circles. Dimension one and constrain the additional 3 with an Equal constraint. (Figure Step 11A and 11B)

Figure Step 11A

Figure Step 11B

Step 12

Extrude the four circles to the To Next extents. (Figure Step 12)

Figure Step 12 [Click to see image full size]

Step 13

Start another sketch on the top plane and draw a circle by offsetting the outside diameter. Dimension the circle and extrude it to complete the model. (Figure Step 13)

Figure Step 13 [Click to see image full size]

Step 14

Change the colour to: Aluminum – Polished. (Figure Step 14)

Figure Step 14

Step 15

Save and close the file.

WORK ALONG: Revolving a Sketch using a Centerline

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Enter the NEW command to start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 14-2. (Figure Step 3)

Figure Step 3
Dimensioned Multiview Drawing

Step 4

Start a new sketch on the Front or XZ Plane. Draw and dimension a line start it by snapping to the Center Point. Draw it 5 inches in the negative Y direction. This is the length of the model. This is centerline of the solid model. Change the line’s properties to a centerline. (Figure Step 4A and 4B)

Figure Step 4A

Figure Step 4B

Step 5

Draw and dimension one-half of the Front view as shown in the figure. (Figure Step 5A and 5B)

Figure Step 5A [Click to see image full size]

Figure Step 5B [Click to see image full size]

Step 6

Return to Model mode and enter the REVOLVE command. Since a centerline is part of the sketch, the REVOLVE command will automatically use it as the axis to revolve the sketch around. It will display the outcome of the revolution. (Figure Step 6)

Figure Step 6 [Click to see image full size]

Step 7

In a new sketch, add the four smaller circles and extrude them to complete the model.

Step 8

Change the colour to: Aluminum – Polished. (Figure Step 8)

Figure Step 8

Step 9

Save and close the file.

Drafting Lesson: Cross Sections

When a view of an object requires a clearer description of its interior or it is hard to dimension because of the hidden lines, a cross section view can be drawn in place of the normal multiview. See Figure 32-1

Figure 32-1
Normal Front and Right Side View of an Object

A cross section view, also called a section, is a view of the object as if it were cut along a cutting plane and the two pieces pulled apart exposing the inside of the object. See Figure 32-2 and 32-3.

Figure 32-2
A Front view and Right
Side Section View

Figure 32-3
3D Model of the Object
Showing it Cut on the
Cutting Plane Line

A cutting plane line is the line along the object where the cut would have been made. See Figure 32-2. The arrows point in the direction that you are looking when drawing the section view. The surfaces of the object that are solid, when cut, are crosshatched.

Key Principles

Lab Exercise 14-1

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the Base plane.

Step 2

Note the location of X0Y0Z0. Draw the Base sketch and revolve it create the Base model of the object shown below. Revolve it by using a line in the sketch. Do not draw a centerline. (Figure Step 2A and 2B)

Figure Step 2A
Dimensioned Multiview Drawing

Figure Step 2B
Suggested Base
Sketch – Right Side –
YZ Plane

Step 3

Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.

Step 4

Apply the colour shown above. (Figure Step 4A and 4B)

Figure Step 4A
Completed Solid Model
– Home View

Figure Step 4B
Completed Model
– Rear View

Step 5

Add the four small holes on a new sketch and extrude them.

Base Sketch

Lab Exercise 14-2

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the Base plane.

Step 2

Note the location of X0Y0Z0. Draw the Base sketch and revolve it create the Base model of the object shown below. Revolve it by using a centerline. (Figure Step 2A, 2B, 2C, 2D, and 2E)

Figure Step 2A
Dimensioned Multiview Drawing

Figure Step 2B
Suggested
Base Sketch –
YZ Plane

Figure Step 2C
Detail of Keyway

Figure Step 2D
Keyway is Flat Across the Top

Figure Step 2E
Solid Model – Home View

Step 3

Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches.

Step 4

Apply the colour shown above. (Figure Step 4A and 4B)

Figure Step 4A
Completed Model –
Home View

Figure Step 4B
Completed Model
– Rotated View

Step 5

Add the four small holes and the key on new sketches and extrude them.

Base Sketch

Key Sketch

Fillets

A fillet is a tangent arc. A fillet is simply an arc which is tangent at both ends. It can be tangent to two lines, a line and an arc, or two arcs. Technically, it is a fillet when material is added to the object model and a round is when material is removed from the object. See Figure 15-1 and 15-2. Most CAD systems, including Inventor, use the term fillet for both.

There are two basic methods of inserting fillets in Inventor. In this module, inserting the fillets after the solid model is created will be taught. They are called features. In the Inventor Advanced book, drawing fillets on the 2D sketch will be taught. It is always better to insert the fillets as features since that makes them much easier to edit after the solid model is created.

Figure 15-1
Fillets Dimensioned in 2D

Figure 15-2
How Fillets Appear on the
Solid Model

Geometry Lesson Tangency – Part 1

A point of tangency is the theoretical point where a line joins an arc or where two arcs join each other making a smooth transition. A line tangent to a circle passes the circle and touches it on only one point on the circle. The point where they touch is called the point of tangency. See Figure 15-3.

Figure 15-3
Tangency – Part 1

WORK ALONG: Creating Models With Fillet Features

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Enter the NEW command to start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 15-1. (Figure Step 3A and 3B)

Figure Step 3A
3D Model

Figure Step 3B

Step 4

Draw the Base sketch on the Front view. Ensure that it is fully constrained. Extrude the sketch to create the Base model. (Figure Step 4A and 4B)

Figure Step 4A

Figure Step 4B

Step 5

Enter the FILLET command and in the Fillet dialogue box, click the radius to edit it. Change the radius to 1.50. (Figure Step 5)

Figure Step 5 [Click to see image full size]

Step 6

Click the Pencil icon to change to the Arrow icon. When the Plus icon appears beside the cursor, select the top left corner of the model. (Figure Step 6A and 6B)

Figure Step 6A [Click to see image full size]

Figure Step 6B

Step 7

Insert the same fillet on the opposite side of the model. (Figure Step 7)

Figure Step 7

Step 8

Start a new sketch and enter the CENTER POINT CIRCLE command. Right click the mouse. In the Right-click menu, select Center. Select the arc and draw a 1 inch Diam circle. Dimension and extrude it.(Figure Step 8A, 8B, 8C, and 8D)

Figure Step 8A

Figure Step 8B

Figure Step 8C

Figure Step 8D

Step 9

Start a new sketch. On it, draw and dimension the slot and extrude it. (Figure Step 9A and 9B)

Figure Step 9A [Click to see image full size]

Figure Step 9B

Step 10

Using what you just learned, insert the 1 inch radius fillets. (Figure Step 10)

Figure Step 10 [Click to see image full size]

Step 11

Insert the fillets as shown on the figures. Ensure that you set the correct radius for each fillet. (Figure Step 11A and 11B)

Figure Step 11A

Figure Step 11B

Step 12

Enter the FILLET command and in the Fillet dialogue box, set the Radius to 0.0875. Set the Select mode to Loop and select the edge as shown in the figure. (Figure Step 12)

Figure Step 12 [Click to see image full size]

Step 13

To complete the model, change the colour to: Chrome – Polished Black. (Figure Step 13)

Figure Step 13

Step 14

Save and close the file.

Chamfers

A chamferis similar to a fillet except instead of an arc being inserted, it inserts an inclined line. See Figure 15-4. Figure 15-5 shows a multiview drawing with the chamfers dimensioned. There are two basic methods of inserting chamfers in Inventor, the same as fillets. In this module, you will learn how to insert them as features after the solid model is created as shown in Figure 15-6.

Figure 15-4
Chamfers

Figure 15-5
Chamfers in a Multiview Drawing

Figure 15-6
Chamfers on the Solid Model

WORK ALONG: Creating Models with Chamfer Features

Step 1

Open the file: Inventor Lab 13-1.ipt that you created in Module 13.

Step 2

Using the SAVEAS command, save the file with the name: Inventor Workalong 15-2. (Figure Step 2A and 2B)

Figure Step 2A

Figure Step 2B
Dimensioned Multiview Drawing

Step 3

Enter the CHAMFER command. In the Chamfer dialogue box, ensure that the equal side icon and Edges icon are enabled. Set the distance to 1.0. Select the bottom right corner of the model. (Figure Step 3)

Figure Step 3 [Click to see image full size]

Step 4

Set the distance to 0.125 and insert the chamfer on the around the top as shown in the figure. (Figure Step 4)

Figure Step 4 [Click to see image full size]

Step 5

Using what you just learned, insert the fillet and chamfers on the model as shown in the figure. (Figure Step 5)

Figure Step 5

Step 6

Insert the 0.10 chamfers around the outside as shown in the figure. (Figure Step 6)

Figure Step 6 [Click to see image full size]

Step 7

The completed model should appear as shown in the figure. (Figure Step 7)

Figure Step 7

Step 8

Save and close the file.

Key Principles

Lab Exercise 15-1

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the Base plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produced the solid model shown in the figures. Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. (Figure Step 2A, 2B, and 2C)

Figure Step 2A
Dimensioned Multiview Drawing

Figure Step 2B
Suggested Base Sketch –
Front – XZ Plane

Figure Step 2C
3D Model – Home View

Step 3

Insert the fillets and chamfers as features after the model is constructed.

Step 4

Apply the colour shown above.

Lab Exercise 15-2

Time allowed: 30 minutes.

Step 1

Open the file: Inventor Lab 14-2.ipt that you created in Module 14.

Step 2

Using the SAVEAS command, save it with the name: Inventor Lab 15-2.

Step 3

Add the fillets and chamfers as features as shown in the figures. (Figure Step 3A, 3B, and 3C)

Figure Step 3A
Dimensioned Multiview Drawing

Figure Step 3B
Solid Model –
Home View

Figure Step 3C
Solid Model –
Rotated View

Competency Tests

The Inventor book was written with competency based modules. What that means is that you have not completed each module until you have mastered it. The Competency Test module contains multiple choice questions and a comprehensive lab exercise to test your mastery of the set of modules that you completed. There are no answers or keys supplied in a Competency Test module since it is meant to be checked by your instructor. If there are any parts of this module that you have trouble completing, you should go back and reread the module or modules containing the information that you are having trouble with. If necessary, redo as many lab exercises required until you fully understand the material.

If you are Completing this book:

• Without the aid of an instructor, complete the written test and the lab exercise.
• In a classroom with an instructor, the instructor will give instructions on what to do after you have completed this module.

Multiple Choice Questions

Select the BEST answer.

1. Which on of the following statements is true?
   1. Construction objects are drawn with the command CONSTRUCTION.
   2. Construction objects will not be used when the sketch is converted into a 3D feature.
   3. Construction objects cannot be used to constrain the sketch.
   4. Construction objects cannot be used as dimensional constraints.
   5. Construction objects will be used when the sketch is converted into a 3D feature.
2. When is it best to place fillets and chamfers on a solid model?
   1. The last thing you do to complete the solid.
   2. The first thing after the base sketch it is revolved.
   3. Before the base model is created.
   4. When the sketches are being created.
   5. The first thing after the base sketch is extruded.
3. Which snap mode is used to snap to the location where two object cross?
   1. On
   2. Midpoint
   3. Intersection
   4. Point
   5. Center
4. Which one of the following function keys, when pressed, enables the display of the constraint icons?
   1. F2
   2. F4
   3. F6
   4. F8
   5. F10
5. What two commands are used to create a solid model?
   1. REVOLVE AND OFFSET
   2. EXTRUDE and REVOLVE
   3. EXTRUDE and FILLET
   4. PROJECT and SOLID
   5. EXTRUDE and MODEL
6. Which key or keys, when pressed while you are selecting objects, will allow you to select more then one object in the selection set?
   1. Only TAB
   2. Either ALT or SHIFT
   3. Either CTRL or ALT
   4. Either TAB or CTRL
   5. Either CTRL or SHIFT.
7. What does the REVOLVE command do when it finds a centerline in the base sketch it is revolving?
   1. It automatically uses the centerline as the axis of revolution.
   2. It prompts you to select the axis of revolution.
   3. It extrudes the base sketch using it as the centre.
   4. It ignores the centerline.
   5. It allows you to select another axis as the axis of revolution.
8. Which snap mode is used when you want to snap to the centre of a line?
   1. On
   2. Midpoint
   3. Intersection
   4. Point
   5. Center
9. Which geometrical constraint is used to make 4 circles all the same diameter when only one of them is dimensioned?
   1. Tangent
   2. Concentric
   3. Coincident
   4. Center
   5. Equal
10. What one of the following is used to change the properties of a selected object from a drawing object to a construction object?
    1. Construction menu
    2. Construction icon
    3. Construction line
    4. Construction circle
    5. Construction object

Lab Exercise 16-1

Time allowed: 60 minutes.

Step 1

Note the location of X0Y0Z0. Draw the necessary sketches and revolve or extrude them to produce the 3D model. (Figure Step 1)

Figure Step 1
Dimensioned Multiview Drawing [Click to see image full size]

Step 2

Draw the base sketch on the Front view. (Figure Step 2)

Figure Step 2
Suggested Base Sketch –
Front View (XZ Plane)

Step 3

Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. Ensure that all objects, on all sketches, display purple on a black background.

Step 4

Create the fillets and chamfers after the solid model is totally constructed.

Step 5

Apply the colour shown. (Figure Step 5A, 5B, and 5C)

Figure Step 5A
Solid Model – Home View

Figure Step 5B
Solid Model – Rotated View

Figure Step 5C
Solid Model – Rotated View

Lab Exercise 16-2

Time allowed: 60 minutes.

Step 1

Note the location of X0Y0Z0. Draw the base sketch on the Right Side view and revolve it to create the base model. (Figure Step 1A, 1B, 1C, and 1D)

Figure Step 1A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 1B
Suggested Base
Sketch – Right Side
View (YZ Plane)

Figure Step 1C
Keyway Detail

Figure Step 1D Section Detail

Step 2

Draw the necessary sketches and extrude them to complete the model.

Step 3

Apply all of the necessary geometrical and dimensional constraints to fully constrain all sketches. Ensure that all objects, on all sketches, display purple on a black background.

Step 4

Create the fillets after the solid model is totally constructed.

Step 5

Apply the colour shown. (Figure Step 5A and 5B)

Figure Step 5A
Solid Model – Home View

Figure Step 5B
Solid Model – Rotated View

Drafting Lesson: Auxiliary Views

When a model has an inclined side, its plane is not parallel to the horizontal and vertical sides of the glass box. If the inclined view is drawn in one of the predefined views in a multiview drawing, some or all parts of the object will not be their true size and shape. To correct this, an auxiliary view is drawn instead of a predefined view. An auxiliary view is a view looking perpendicular to the inclined plane as shown in Figure 17-1.

Figure 17-1
An Auxiliary View [Click to see image full size]

Drafting Lesson: Broken Views and Break Lines

To simplify or speed up drawing some of the views of a multiview drawing are only partially drawn. In these cases, the cutoff (sometimes called the broken) portion of the view is not required for the reader to visualize the object. Auxiliary views are frequently cutoff. When a view is cutoff, a break line is drawn to indicate where the view was broken as shown in Figure 17-2. A short break line and a long break line are drawn differently as show in Figure 17-2.

Figure 17-2
Broken Views and Break Lines

Short Break

Long Break

An Example of Using Break Lines

Drawing and Dimensioning Inclined Lines

Drawing and dimensioning inclined lines in sketches is a simple operation in Inventor compared to most CAD systems. The reason for this is that you can guess at the angle when drawing the inclined line rather then entering the exact number of degrees. After the sketch is complete, the angle is dimensioned using the exact angle and Inventor will adjust the sketch to match.

Aligned Dimensions

An aligned dimension is a dimension measuring the true length of a line or the true distance between two points. See Figure 17-3. The extension lines will be perpendicular and the dimension line will be parallel to the line or an imaginary line between two points.

Figure 17-3
An Aligned Dimension

Placing an Aligned Dimension

To place an aligned dimension, enter the GENERAL DIMENSION command or the shortcut D and regardless if you are selecting a line, two points, or two lines to dimension, the same Aligned dimension icon will display as shown in Figures 17-4 and Figure 17-5.

Figure 17-4
Placing a Aligned
Dimension

Figure 17-5
Aligned
Dimension Icon

Angular Dimensions

An angular dimension is a dimension measuring the angle between two lines or the angle between the imaginary lines between three points. See Figure 17-6. The lines cannot be parallel to each other.

Figure 17-6 Angular Dimension

Placing an Angular Dimension

To place an angular dimension, enter the GENERAL DIMENSION command or the shortcut D and either select two lines or three points to place the angular dimension between.

The Two-Line Method

Select the first line. It will change colour. Move the cursor onto the second line and without selecting it, note how it changes colour. The Angular Dimension icon will display as shown in Figure 17-7. Select the second line. Drag the dimension to locate it. See Figure 17-8

Figure 17-7
Placing an Angular Dimension – Two line Method

Figure 17-8
The Angular Dimension – Two line Method

The Three-Point Method

Select the first two points and move the cursor onto the third point as shown in Figure 17-9. The second point MUST be the vertex of the angle. The Angular Dimension icon will display as shown in Figure 17-9. Select the third point and drag the angular dimension to the desired location. See Figure 17-10.

Figure 17-9
Placing an Angular Dimension – Three Point Method

Figure 17-10
The Angular Dimension – Three Point Method

WORK ALONG: Drawing Models that Contain Inclined Lines

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Using the NEW command start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 17-1. (Figure Step 3A, 3B, and 3C)

Figure Step 3A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 3B
Auxiliary View

Figure Step 3C
3D Model
Home View

Step 4

Start the Base sketch on the Front or XZ plane.

Step 5

Project the Center Point onto the sketch.

Step 6

Draw the three top lines of the Front view and dimension them. Ensure that the sketch is fully constrained. (Figure Step 6)

Figure Step 6

Step 7

Enter the OFFSET command. When prompted, select the top line. (Figure Step 7)

Figure Step 7

Step 8

Right click the mouse and in the Right-click menu, select Continue. Move the cursor down about 0.5 inches. The offset line will drag with it. Click to select the location. (Figure Step 8)

Figure Step 8

Step 9

Do the same for the other two lines. (Figure Step 9)

Figure Step 9

Step 10

Enter the TRIM command. When prompted, select the overlapping end of the lines on the top intersection. (Figure Step 10A and 10B)

Figure Step 10A

Figure Step 10B

Step 11

Enter the EXTEND command and extend the lines at the bottom intersection by selecting each of them. (Figure Step 11A and 11B)

Figure Step 11A

Figure Step 11B

Step 12

Add three dimensions for the 0.5 thickness. The sketch should be fully constrained. (Figure Step 12)

Figure Step 12

Step 13

Press F6 to return to Home view.

Step 14

Extrude the sketch. (Figure Step 14)

Figure Step 14

Step 15

Start a new sketch on the top plane. Draw three lines and add the dimensions to fully constrain the sketch. (Figure Step 15)

Figure Step 15

Step 16

Extrude the sketch using the cut option. (Figure Step 16)

Figure Step 16

Step 17

Start a new sketch on the inclined plane. Draw three construction lines and dimension them to locate the centre of the circles. Ensure that the lines are fully constrained. (Figure Step 17)

Figure Step 17

Step 18

Insert two circles locating their centers at the intersection of the construction lines. Dimension only one of them and then apply the Equal constrain to the other circle. (Figure Step 18)

Figure Step 18

Step 19

Draw a line from one circle to the other. Don’t worry about constraining them tangent at this time. Ensure that the Snap On icon appears when you select the endpoint of the lines. (Figure 19A and 19B)

Figure
Step 19A

Figure
Step 19B

Step 20

In the right-click menu, select Create Constrain – Tangent. (Figure Step 20).

Figure
Step 20

Step 21

Apply the Tangent constraint between the circle and the line. Repeat with the other circle. (Figure Step 21A and 21B)

Figure Step 21A [Click to see image full size]

Figure Step 21B [Click to see image full size]

Step 22

Trim the circles. This will take four steps. (Figure Step 22)

Figure Step 22

Step 23

Extrude the sketch. (Figure Step 23)

Figure Step 23

Step 24

Draw a 2D Sketch on the bottom plane. Using what you just learned, ensure that you constrain the lines tangent to the circles and then trim. (Figure Step 24A and 24B)

Figure Step 24A [Click to see image full size]

Figure Step 24B

Step 25

Extrude the sketch. (Figure Step 25)

Figure Step 25

Step 26

Insert the fillets and change to the color: Orange to complete the solid model. (Figure Step 26)

Figure Step 26

Step 27

Save and close the part file.

Key Principles

Lab Exercise 17-1

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the base plane.

Step 2

Note the location of X0Y0Z0. 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 and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2B
Suggested Base
Sketch – Front (XZ)
Plane

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3
Completed Solid Model
Home View

Author’s Base Sketch [Click to see image full size]

Step 4

Create all fillets after the solid model is totally constructed.

Lab Exercise 17-2

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the base plane.

Step 2

Note the location of X0Y0Z0. 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 and 2B)

Figure Step 2A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2B
Suggested Base Sketch –
Top (XY) Plane) [Click to see image full size]

Step 3

Apply the colour shown above. (Figure Step 3)

Figure Step 3
Completed Solid Model – Home View
Author’s

Step 4

Create all fillets after the solid model is totally constructed.

Author’s Base Sketch [Click to see image full size]

Methods of Selecting Objects

Figure 18-1 Methods of Selecting Objects

 Selecting Objects

Up to this point in the book, the only way that has been shown how to select objects was to pick them, one at a time. A quicker and more efficient method of selecting multiple objects is to use either a window or a crossing window. Study Figure 18-1 and start using windows and crossing windows when selecting multiple objects in both Sketch or Model mode.

AUTHOR’S COMMENTS: Construct the arc either clockwise or counterclockwise. Point 3 MUST always be on the circumference of the arc, between Point 1 and Point 2. See Figure 18-2.

Figure 18-2
Construction Techniques for Arcs

WORK ALONG: Drawing a Solid Model with Arcs and Rectangles

Step 1

Check the current project and if necessary, set it to Inventor Course.

Step 2

Using the NEW command, start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 18-1. (Figure Step 3A, 3B, 3C, and 3D)

Figure Step 3A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 3B
Dimensioned Detail Drawing [Click to see image full size]

Figure Step 3C
3D Model – Home View [Click to see image full size]

Figure Step 3D
3D Model – Rotated View [Click to see image full size]

Step 4

Start the Base sketch on the Front or XZ plane. Project the Center Point onto the sketch.

Step 5

Draw the four outside lines of the Base sketch. (Figure Step 5)

Figure Step 5

Step 6

Offset all four lines as shown in the figure. (Figure Step 6)

Figure Step 6

Step 7

Trim and dimension the sketch ensuring that it is totally constrained. (Figure Step 7)

Figure Step 7

Step 8

Press F6 to change the view to the Home view. All of the lines in the sketch should appear purple. Extrude the sketch. (Figure Step 8)

Figure Step 8

Sketching Without the Grid

Up to this point in the Inventor book, the grid display has been enabled in Sketch mode. To the more experienced operator, grid display can be disabled in Sketch mode. On some sketches, it is sometimes easier to draw without the grid getting in the way.

Step 9

Start a new sketch on the right side face as shown in the figure. (Figure Step 9)

Figure Step 9

Step 10

Using what you already learned, open the Application Options dialogue box.

Step 11

Enable the Sketch tab.

Step 12

In the Display area, disable Grid Lines. (Figure Step 12)

Figure Step 12

Step 13

Draw a construction line 0.5 inches below the top edge and dimension it. Ensure that it is fully constrained. (Figure Step 13)

Figure Step 13 [Click to see image full size]

Step 14

Click the THREE POINT ARC command. Snap the first point to one end of the construction line, snap the second point to the other end of the construction line. For the third point, snap it to the midpoint of the top edge. (Figure Step 14A, 14B, and 14C)

Figure Step 14A

Figure Step 14B

Figure Step 14C

Step 15

Using the CREATE CONSTRAIN command, apply the Tangent constraint to the arc and the top edge. This should fully constrain the sketch. (Figure Step 15)

Figure Step 15 [Click to see image full size]

Step 16

Extrude the sketch. (Figure Step 16A and 16B)

Figure Step 16A [Click to see image full size]

Figure Step 16B

Step 17

Using what you just learned, start a new sketch on the top of the model. On it, draw three construction lines and a three point arc. Ensure that the sketch is fully constrained. Extrude the sketch. (Figure Step 17A and 17B)

Figure 17A [Click to see image full size]

Figure 17B

Step 18

Start a new sketch on the lower plane. (Figure Step 18)

Figure Step 18

Step 19

On the sketch, using the TWO POINT RECTANGLE command, draw a rectangle by selecting two opposite corners. Guess at the location and size. (Figure Step 19)

Figure Step 19 [Click to see image full size]

Step 20

Insert four dimensions, one from each edge. Check to ensure that the sketch is fully constrained and extrude it. (Figure Step 20A and 20B)

Figure Step 20A [Click to see image full size]

Figure Step 20B

Step 21

Start a new sketch on the back plane and place a construction line as shown in the figure. Do not offset the edge. Ensure that you constrain the line perpendicular to the bottom or top edge. You can guess at the start point and the length of the line. (Figure Step 21)

Figure Step 21 [Click to see image full size]

Step 22

Change the property of the line to a construction line. Insert one circle at the each end of the line. Snap to the end of the line to locate the centre of the circles. (Figure Step 22)

Figure Step 22

Step 23

Using what you learned already, dimension one of the circles and then create an Equal constraint for the other one. Draw lines on either side of the circle. Ensure that you snap the end of the lines onto the circles. Constrain the lines to the circle with the Tangent constraint. Trim the circles. (Figure Step 23A, 23B, and 23C)

Figure Step 23A

Figure Step 23B

Figure Step 23C

Step 24

Draw a construction line from the end of the construction line at the top circle, constraining it perpendicular to one of the vertical lines. Draw it approximately 1 inch long. (Figure Step 24)

Figure Step 24

Step 25

Click the COPY command and select the two lines and the arcs as shown in the figure. Ensure that the Select icon is enabled. (Figure Step 25)

Figure Step 25 [Click to see image full size]

Step 26

Enable the From icon and select the end of the construction line for the From location. (Figure Step 26)

Figure Step 26 [Click to see image full size]

Step 27

Enable the To icon and select the other end of the construction line for the To location. (Figure Step 27)

Figure Step 27

Step 28

If you get the warning message, click Yes.

Step 29

Dimension the sketch until it is fully constrained. (Figure Step 29)

Figure Step 29 [Click to see image full size]

Step 30

Return to Model mode and extrude the slots. Extrude them 0.25 inches deep. (Figure Step 30)

Figure Step 30 [Click to see image full size]

Step 31

Start a new sketch on the bottom of the extruded slots. Enter the OFFSET command and right-click one of the arcs. In the Right-click menu, enable Loop Select. Select the other arc and the lines to complete the loop. (Figure Step 31A and 31B)

Figure Step 31A

Figure Step 31B

Step 32

Offset the slot towards the inside. Guess at the offset distance. (Figure Step 32)

Figure Step 32

Step 33

Dimension the offset. (Figure Step 33)

Figure Step 33

Step 34

Extrude the slot To Next. (Figure Step 34)

Figure Step 34

Step 35

Redo Step 31 to 34 on the other slot to complete the solid model.

Step 36

Set the colour to: Dark Red. (Figure Step 36)

Figure Step 36

Step 37

Save and close the file.

MUST KNOW: A window selects all of the objects that are totally inside of it defined by two user picks. A window always appears as a solid line and is created by picking the first point on the left and moving right to pick the second point.A crossing window selects all of the objects that are totally inside and the ones that cross it defined by two user picks. A crossing Window always appear as dashed lines and is created by picking the first point on the right and moving left to select the second point.

To select a window or crossing window, select the first point by moving the cursor to the desired location and press the left mouse button down. While holding it down, move to the cursor to second desired location and release the mouse button.

A Window

A Crossing Window

Key Principles

Lab Exercise 18-1

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the base plane.

Step 2

Note the location of X0Y0Z0. 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, and 2D)

Figure Step 2A
3D Model – Home View

Figure Step 2B
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 2C
Dimensioned Auxiliary View [Click to see image full size]

Figure Step 2D
Suggested Base Sketch –
Front (XZ) Plane

Step 3

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

Figure Step 3A
Solid Model – Home View

Figure Step 3B
Solid Model – Rotated View

Lab Exercise 18-2

Time allowed: 60 minutes.

Step 1

Project the Center Point onto the base plane.

Step 2

Note the location of X0Y0Z0. 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 and 2B)

Figure Step 2A
Suggested Base
Sketch – Right Side
(YZ Plane)

Figure Step 2B
Dimensioned Multiview Drawing

Author`s Base Sketch

Author’s Base Model

Step 3

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

Figure Step 3A
Solid Model – Home View

Figure Step 3B
Solid Model – Rotated View

Step 4

Create all fillets after the solid model is totally constructed.

Geometry Lesson: Regular Polygons

A polygon is defined as any plane figure bounded by straight lines. A regular polygon 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.

Figure 19-1
Regular Polygons
Work

Any regular polygon can be inscribed in or circumscribed around a circle as shown, using a hexagon, in Figure 19-2.

Figure 19-2
Inscribed and Circumscribed Regular Polygon

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.

Figure 19-3
Geometry of Four Regular Polygons

Drawing Threads

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.

Figure 19-4
External and Internal Threads

WORK ALONG: Drawing Polygons and Threads – Part 1

Step 1

Using the NEW command start a new part file using the template: English-Modules Part (in).ipt.

Step 2

Save the file with the name: Inventor Workalong 19-1. (Figure Step 2A, 2B, and 2C)

Figure Step 2A
3D Model –
Home View

Figure Step 2B
Dimensioned Multiview Drawing

Figure Step 2C
Detail

Step 3

Draw the Base sketch on the Top or XY plane.

Step 4

Project the Center Point onto the Base sketch.

Step 5

Enter the POLYGON command and set the number of sides to 6. (Figure Step 5)

Figure Step 5

Step 6

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)

Fig Step 6

Step 7

Add the dimension from the Center Point to the left line. (Figure Step 7)

Figure Step 7

Step 8

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

Figure Step 8A

Figure Step 8B

Figure Step 8C

Step 9

Extrude the hexagon in the negative Z direction. (Figure Step 9)

Figure Step 9 [Click to see image full size]

Step 10

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)

Figure Step 10

Step 11

Extrude the circle 0.016 inches. Ensure that you enable the Join icon and extrude it away from the bolt head. (Figure Step 11)

Figure Step 11 [Click to see image full size]

Step 12

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)

Figure Step 12A

Figure Step 12B

Step 13

Using the CHAMFER command, chamfer the bottom of the bolt. (Figure Step 13)

Figure Step 13 [Click to see image full size]

Step 14

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)

Figure Step 14 [Click to see image full size]

Step 15

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

Figure Step 15A [Click to see image full size]

Figure Step 15B

Step 16

Change the view to the Home view and change the colour to: Metal-Brass. (Figure Step 16)

Figure Step 16

Step 17

Save and close the file.

WORK ALONG: Drawing Polygons and Threads – Part 2

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Using the NEW command start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 19-2.

Step 4

Using what you learned in the last workalong, construct the nut shown in the multiview drawing. (Figure Step 4A and 4B)

Figure Step 4A
Dimensioned Multiview Drawing

Figure Step 4B 3D Model – Home View

Step 5

Change the colour to: Metal-Brass. (Figure Step 5A and 5B)

Figure Step 5A

Figure Step 5B

Work Features

Work Features 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.

Figure 19-5
Work Features

Work Points

A Work Point 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.

Work Axes

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. 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.

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.

Work Planes

A Work Plane 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.

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.

WORK ALONG: Creating Work Features

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Using the NEW command start a new part file using the template: English-Modules Part (in).ipt.

Step 3

Save the file with the name: Inventor Workalong 19-3.

Step 4

Create the solid model shown in the figures. (Figure Step 4A and 4B)

Figure Step 4A
3D Model – Home View

Figure Step 4B
Dimensioned Multiview Drawing [Click to see image full size]

Step 5

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)

Figure Step 5A

Figure Step 5B

Figure Step 5C

Step 6

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)

Figure Step 6A

Figure Step 6B

Figure Step 6C

Figure Step 6D

Figure Step 6E

Step 7

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)

Figure Step 7A

Figure Step 7B

Figure Step 7C

Step 8

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)

Figure Step 8A

Figure Step 8B

Step 9

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)

Figure Step 9A

Figure Step 9B

Figure Step 9C

Step 10

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)

Figure Step 10A

Figure Step 10B

Figure Step 10C

Figure Step 10D

Step 11

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)

Figure Step 11A

Figure Step 11B

Figure Step 11C

Figure Step 11D

Step 12

Work Features will display as items in the Browser bar. Note the three Work Axes that you just inserted. (Figure Step 12)

Figure Step 12

Step 13

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)

Figure Step 13A

Figure Step 13B

Figure Step 13C

Figure Step 13D

Step 14

Insert an offset Work Plane. Enter the WORK PLANE command and then Offset from Plane. 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)

Figure Step 14A

Figure Step 14B

Figure Step 14C

Step 15

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)

Figure Step 15A

Figure Step 15B

Step 16

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)

Figure Step 16A

Figure Step 16B

Figure Step 16D

Figure Step 16E

Step 17

The Browser bar should now appear as shown in the figure. (Figure Step 17)

Figure Step 17

Step 18

Disable the visibility of all Work Features. Your solid model should appear as shown in the figure. (Figure Step 18)

Figure Step 18

Figure 19-6
Dimensioned Multiview Drawing

Figure 19-7
3D Model – Home View

Step 19

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)

Figure Step 19A

Figure Step 19B

Step 20

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)

Figure Step 20A

Figure Step 20B

Figure Step 20C

Figure Step 20D

Step 21

Start a new sketch and draw two lines. Dimension and extrude it. (Figure Step 21A and 21B)

Figure Step 21A

Figure Step 21B

Step 22

Insert a Work Plane -0.375 inches in from the front face. (Figure Step 22)

Figure Step 22

Step 23

Draw a triangle and insert two dimensions to fully constrain it. (Figure Step 23)

Figure Step 23 [Click to see image full size]

Step 24

Extrude the sketch 0.125 inches in both directions to complete the part. (Figure Step 24)

Figure Step 24 [Click to see image full size]

Step 25

Disable the visibility of all Work Features. The completed solid model should appear as shown in the figure. (Figure Step 25)

Figure Step 25

Step 26

Change to the Home view. (Figure Step 26)

Figure Step 26 [Click to see image full size]

Step 27

Save and close the part.

Key Principles

Lab Exercise 19-1

Time allowed: 90 minutes.

Step 1

Draw the Base sketch on the Front view.

Step 2

Project the Center Point onto the Base plane.

Step 3

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)

Figure Step 3A
3D Model – Orbited View

Figure Step 3B
3D Model – Home View

Figure Step 3C
Solid Model – Home View

Figure Step 3D
3D Model – Orbited View

Figure Step 1E
Left Side View – Multiview Drawing [Click to see image full size]

Figure Step 1F
Right Side View – Multiview Drawing [Click to see image full size]

Step 4

Create the fillets and chamfers after the model is totally constructed.

Step 5

Apply the colour shown above.

Lab Exercise 19-2

Time allowed: 90 minutes.

Step 1

Draw the Base sketch on the Right Side view.

Step 2

Project the Center Point onto the Base plane.

Step 3

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)

Figure Step 3A
3D Model – Orbited View

Figure Step 3B
3D Model – Home View

Figure Step 3C
Solid Model – Home View

Figure Step 3D
Solid Model – Orbited View

Author’s Base Sketch

Author’s Base Model

Step 4

Create the fillets and chamfers after the model is totally constructed.

Step 5

Apply the colour shown above.

Lab Exercise 19-3

Time allowed: 90 minutes.

Step 1

Project the Center Point onto the Base sketch.

Step 2

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)

Figure Step 2A
3D Model – Home View

Figure Step 2B [Click to see image full size]

Figure Step 2C
Suggested Base Sketch – Author’s Base Model Top (XY) Plane

Author’s Base Sketch

Figure Step 2D
Solid Model – Home View
With Work Planes

Figure Step 2E
Solid Model – Home View

Step 3

Create the fillets and chamfers after the model is totally constructed.

Step 4

Apply the colour shown above.

Modifying Solid Models

The ability to modify solid models is as important to the drafter/designer as being able to construct models. Since most parts are modified after the initial design or revised and used in another project, it is very important that you can modify solid models rather then redraw them. The true power of Inventor is its ability to modify a solid and have it conform to the geometrical and dimensional constraints applied to it when it was constructed without having to redraw it. In this module, the basics of modifying solid models is taught. The Inventor Advanced book will cover the more advanced methods of modifying solid models.

Working with the Browser Bar

The Browser bar is used extensively as a tool to assist you when modifying solid models. It displays the work features and the part features for the current part.

Features

Work features are the basic sketching planes (XY, XZ, YZ), the axes (X, Y, Z) and the Center Point as shown in Figure 20-1.Part features are the 3D features added to the solid model in model construction. The part features for the active part are shown in Figure 20-2.

Figure 20-1
Work Features

Figure 20-2
Part Features

Edges and Faces

Edges are the lines, circles, or arcs located between the planes that form the solid model. Faces are the planes between the edges of the solid. A face can also be circular or cylindrical in shade, for example the hole in the model. Figure 20-3 shows each visible face of a solid model in a different colour.

Figure 20-3
Edges and Faces

WORK ALONG: Modifying a Solid Model

Step 1

Open the part file: Inventor Workalong 20-1.ipt. This is one of the parts that you received when you download your book. It should be in the folder: Lab Exercise. (Figure Step 1A and 1B)

Figure Step 1A

Figure Step 1B

Step 2

The Filter icon located at the top of the Browser bar allows you to enable or disable the visibility of the features in the Browser bar. Click the Filter icon. The filter list will display. (Figure Step 2A and 2B)

Figure Step 2A

Figure Step 2B

Step 3

Click Hide Work Features to enable it. The work features are now hidden for the current part. (Figure Step 3A and 3B)

Figure Step 3A

Figure Step 3B

Step 4

Since you want the work features to display most of the time, click the Filter icon again and disable the Hide Work Features. (Figure Step 4)

Figure Step 4

Step 5

The Part icon is the first icon inside the Browser bar window. It displays the name of the active part. (Figure Step 5)

Figure Step 5

Step 6

Right-click the part name. In the Right-click menu, click Expand All Children. Note how all the folders and part features will expand to display every feature in the current part. Right click the menu again and this time, click Collapse All Children. (Figure Step 6A, 6B, and 6C)

Figure Step 6A

Figure Step 6B

Figure Step 6C

Step 7

Right-click the part feature Extrusion1. In the Right-click menu, click Show Dimensions. Note how the 2D sketch dimensions and the extrusion dimension will display on the model. (Figure Step 7)

Figure Step 7 [Click to see image full size]

Step 8

Right-click Extrusion1 again. In the Right-click menu, click Edit Sketch. The Graphic window will change to Sketch mode and display the sketch. (Figure Step 8)

Figure Step 8

Step 9

Double click any dimension in the sketch and the Edit Dimension dialogue box will open as shown in the figure. You could now change the dimension, if required, which in turn will change the size of the model. Close the dialogue box without making any changes and return to Model mode. (Figure Step 9)

Figure Step 9

Step 10

Right-click Extrusion1. In the right-click menu, click Edit Feature. Since this feature is an extrusion, the Extrude dialogue box will open. If required, the extrude feature could be edited. Click the Cancel button to close it. (Figure Step 10A and 10B)

Figure Step 10A

Figure Step 10B [Click to see image full size]

Step 11

Right-click Extrusion3 as shown in the figure. In the right-click menu, click Find in Window. Note how the extrude on the left side will fully display in the window. This is a handy feature to use when your part is complicated or if you are using a part you are not familiar with. (Figure Step 11)

Figure Step 11

Step 12

Using what you learned in Steps 8 to 11, edit the sketch in Extrusion1 to match the dimensions shown in the figure. When you are done, click Finish Sketch to return to Model mode and the model will resize to reflect the changes you made to the dimensions. (Figure Step 12)

Figure Step 12

Step 13

Edit Extrusion1 to change the extrusion depth from 3 inches to 4 inches. Click OK. (Figure Step 13)

Figure Step 13 [Click to see image full size]

Step 14

Edit the dimensions in the sketch for the part feature Extrusion4 to the dimensions shown in the figure. Return to Model mode. (Figure Step 14A and 14B)

Figure Step 14A

Figure Step 14B

Step 15

Since Sketch1 is an unconsumed sketch, it can be deleted. Select it and right click it. In the Right-click menu, select Delete. (Figure Step 15)

Figure Step 15

Step 16

Expand the children. Change the name of Sketch2 to Base Sketch – Front View. (Figure Step 16A and 16B)

Figure Step 16A

Figure Step 16B

Step 17

Change the names of all the part features and their children to match the names in the figure. Change the name of the part to: Inventor Workalong 20-1 Finished.ipt as shown in the figure. (Figure Step 17)

Figure Step 17

Step 18

Move the cursor onto the End of Part icon and hold down the left mouse button. When the End of Part has a red rectangle around it, drag it to the location shown in the figure. (Figure Step 18A, 18B, and 18C)

Figure Step 18A

Figure Step 18B

Figure Step 18C

Step 19

Drag the End of Part icon back to the bottom of the part feature list in the Browser bar. (Figure Step 19A and 19B)

Figure Step 19A

Figure Step 19B

Step 20

Using the SAVEAS command, save the file with the name: Inventor Workalong 20-1 Finished. Close the part.

Measuring the Model

Inventor has four commands available to measure distances, angles, loops lengths and areas. They also allow the user to set the units and decimal precision of how it displays the answers. Answers can be accumulated. Measurements can be made in either 3D (Model mode) or 2D (Sketch mode).

WORK ALONG: Measuring a Solid Model

Step 1

Open part file: Inventor Workalong 20-1.ipt. (Figure Step 1)

Figure Step 1

Step 2

Click the MEASURE DISTANCE command. The Measure Distance dialogue box will display as shown in the figure. Move this dialogue box close to your model to make measuring easier. (Figure Step 2).

Figure Step 2

Step 3

Note that when you are in Measuring mode, the Graphic cursor appears as a ruler icon. The ruler icon indicates that you are measuring in document units. This will be covered in greater detail later in the module. (Figure Step 3)

Figure Step 3

Step 4

Move the cursor to the bottom left corner of the model and click the left mouse button. Note how it displays a small snap circle indicating that you are snapping to an exact endpoint. (Figure Step 4)

Figure Step 4

Step 5

When you snap to a location on the model, the XYZ coordinate location will display as shown in the figure. In this case, it is X0Y0Z0 of the model or the Center Point. (Figure Step 5)

Figure Step 5

Step 6

To clear the Measure Distance dialogue box and start a new measurement, click the small triangle inside the dialogue box. In the pull-down menu, select Restart. (Figure Step 6)

Figure Step 6

Step 7

Move the cursor to bottom right corner of the right side of the model. Click it to snap to the corner. The XYZ location will display in the dialogue box as shown in the figure. (Figure Step 7)

Figure Step 7

Step 8

Clear the dialogue box by clicking Restart. Measure the length of an edge. Move the cursor onto the left edge of the right side of the model as shown in the figure. (Figure Step 8)

Figure Step 8

Step 9

When you click the mouse, the length of the edge will display in the dialogue box. In this case, it is 3 inches long. (Figure Step 9)

Figure Step 9

Step 10

While the dialogue box is still displaying the length of the edge, click the opposite edge. Note how the dialogue box now displays both the length of the edge and the distance between the edges. A line showing the measured distance will display to show you what is being measured. (Figure Step 10)

Figure Step 10

Step 11

To measure a three dimensional distance, click the two corners shown in the figure. The 3D dimension between the corners will display as well as the XYZ location of the last corner and the delta XYZ distances. (Figure Step 11A and 11B)

Figure Step 11A

Figure Step 11B

Step 12

Measure the angle between the two edges by clicking the small triangle at the end of the dialogue box. In the pull-down menu, select Measure Angle. Select the two edges. The angle will display graphically and as an exact number in decimal degrees. (Figure Step 12A and 12B)

Figure Step 12A

Figure Step 12B

Step 13

Change the command to Measure Loop. Click the face on the Front view. Note how the complete loop (the perimeter) around the front plane will highlight and the loop distance of 22 inches will display in the dialogue box. (Figure Step 13A and 13B)

Figure Step 13A

Figure Step 13B

Step 14

Measure the area of the right side face by changing the command to Measure Area. Click the face on the right side and the area to be measured will highlight. The area will display in the dialogue box. Since there is a hole in this plane, the area will be measured minus the hole. (Figure Step 14A and 14B)

Figure Step 14A

Figure Step 14B

Step 15

Suppress the hole feature on the right side face so that you can measure the area of the face without subtracting the hole. Right-click the feature in the Browser bar. In the Right-click menu, select Suppress Feature. Note how Extrusion4 is now grayed out. (Figure Step 15)

Figure Step 15

Step 16

Using what you just learned, measure the area of the right-side minus the hole. After you measure it, unsuppress the hole feature. (Figure Step 16)

Figure Step 16

Step 17

Click Tools and then click Document Settings. This will open the Document Setting dialogue box for the current part. Do not make any changes at this time. Click Close to close the dialogue box. (Figure Step 17A and 17B)

Figure Step 17A

Figure Step 17B

Step 18

Enter the MEASURE command. Click the small triangle at the end. In the pull-down menu, select Precision and then 5 places. An example of an area measurement with a precision of 5 decimals points is shown in the figure.

Figure Step 18

Step 19

Change the precision to display All Decimals. A sample of an answer to an area measurement is shown in the figure. (Figure Step 19)

Figure Step 19

AUTHOR’S COMMENTS: When the precision is set to All Decimals, the Graphic cursor will change to the Micrometer icon as shown in Figure below.

Step 20

Change the precision back to three decimal places. (Figure Step 20)

Figure Step 20

Step 21

Change the colour to: Aluminum Cast. (Figure Step 21)

Figure Step 21

Step 22

Save and close the part.

Geometry Lesson: Physical Properties

Face Coloring

Sometimes it is helpful to be able to change the colour of a face. This is especially helpful when working with complex parts or to display different textures on a model. For example, this can happen during manufacturing when a part is cast and has machined surfaces. By applying the cast material to the part and then changing the faces of the machined areas to a polished texture/color, the model will appear more realistic.

A face colour overrides the part colour and, if applicable, the feature colour for selected faces. In this module, only faces coloring will be taught. The general rules when changing the colour of faces are:

1. A face colour overrides the part feature colour which in turn overrides the part colour.
2. If the part has been assigned a transparent colour, the face colour you apply will change the colour but it will be transparent.
3. If a thread texture is applied to the feature, a change to the face colour affects the base colour used in the thread texture.
4. If the face colour has been changed and the feature is colored as a pattern, the patterned features will not display the face colour.

Figure 20-3
Edges and Faces

Physical Properties

The physical properties of a solid model include the mass, volume, centre of gravity, and inertial properties. Using the physical properties helps you to evaluate how the designed model correlates to its physical counterpart. For example, the weight of a solid model made from different materials could easily be found.

Assigning the Material to the Model

Up to this point in the book, only colour or texture has been assigned to the solid model. In this module, assigning the actual material that the part is made from will be taught.

WORK ALONG: Coloring Faces and Working with Physical Properties

Step 1

Open part file: Inventor Workalong 20-1.ipt. (Figure Step 1)

Figure Step 1

Step 2

Click the right side face to select it and right click the mouse. In the Right-click menu, select Properties. In the Face Properties dialogue box, select: Blue – Wall Paint – Glossy. (Figure Step 2A, 2B, and 2C)

Figure Step 2A

Figure Step 2B

Figure Step 2C

Step 3

Using what you just learned, change three additional faces as shown in the figure to Green, Orange and Red. (Figure Step 3)

Figure Step 3

Step 4

Click the View tab. Click the CENTER OF GRAVITY command. Note how the Center of Gravity icon will display located at the centre of gravity or centroid of the model. It also displays the positive X, Y and Z axis. (Figure Step 4A and 4B)

Figure Step 4A

Figure Step 4B

Step 5

Rotate the model so that you can see the location of Center of Gravity icon from a better viewpoint . (Figure Step 5)

Figure Step 5

Step 6

Disable the display of the Center of Gravity icon.

Step 7

Right-click the part name in the Browser bar. In the Right-click menu, select iProperties. This will open the Properties dialogue box for the current part. (Figure step 7A and 7B)

Figure Step 7A

Figure Step 7B [Click to see image full size]

Step 8

Enable the Physical tab. Note how the material is shown as Default. Pull down the Material list and select: Aluminum 6061. (Figure Step 8)

Figure Step 8

Step 9

Change the Requested Accuracy to Very High. The Density box displays the density of the material: Aluminum 6061. (Figure Step 9)

Figure Step 9

Step 10

Using what you learned earlier in the workalong, open the Document Settings dialogue box and in the Units tab, change the Mass to gram. (Figure Step 10)

Figure Step 10

Step 11

Note how the mass (weight) is now displayed in grams. (Figure Step 11)

Figure Step 11

Step 12

Change the material to: Cast Steel. Note how the density and the mass change since steel is much denser then aluminum.

Step 13

Change the material back to: Aluminum-6061. Close the Properties dialogue box.

Step 14

Save and close the part.

Key Principles

Lab Exercise 20-1

Time allowed: 60 minutes.

Step 1

Open the part: Inventor Lab 19-3.ipt that you created in Module 19. (Figure Step 1)

Figure Step 1
Modified Solid Model

Step 2

Save the file as: Inventor Lab 20-1.

Step 3

Change the model colour to: Aluminum (Cast).

Step 4

Expand All the Children in the Browser bar.

Step 5

Edit the Base sketch and change the dimensions of the overall length from 180 to 200 and the overall width from 140 to 175 in the figure. (Figure Step 5)

Figure Step 5
Editing the Base Sketch [Click to see image full size]

Step 6

Edit the feature Extrusion1 and change the thickness of the base sketch from 15mm to 20 mm. Return to model mode.

Step 7

Using the next five figures below, change the colors of the machined faces shown to: Aluminum (Polished). (Figure Step 7A, 7B, 7C, 7D, and 7E)

Figure Step 7A
Solid Model – Colored Faces

Figure Step 7B
Solid Model – Colored Faces

Figure Step 7C
Solid Model – Colored Faces

Figure Step 7D
Solid Model – Colored Faces

Figure Step 7E
Solid Model – Colored Faces

Lab Exercise 20-2

Time allowed: 60 minutes.

Step 1

Open part: Inventor Lab 18-2.ipt that you created in Module 18. (Figure Step 1A and 1B)

Figure Step 1A
Solid Model – Home View

Figure Step 1B
Solid Model – Without the Small Fillets

Step 2

Save the file as: Inventor Lab 20-2.

Step 3

Change the colour to: Blue Gray (Light)

Step 4

Move the End of Part Icon up above the small fillets as shown below. (Figure Step 4)

Figure Step 4

Step 5

Find the following with a precision of 5 decimal points. (Figure Step 5)

Figure Step 5

A The XYZ coordinates of corner A.
____________________________

B The distance from corner B to corner C.
____________________________

C The distance from corner B to corner D.
____________________________

D The area of the shaded area the figure. Do NOT include the area of the cylinder. (Figure Step 5D)

____________________________

E The perimeter of the shaded plane. (Figure Step 5E)

____________________________

Figure Step 5D and 5E)

F The area of the shaded area of the figure WITHOUT the eight small holes. (Figure Step 5F)
____________________________

Figure Step 5F

Step 6

Move the End of Part icon back to bottom.

Step 7

Using the two figures, change the colors of the faces shown to: Blue Pastel. (Figure Step 7A and 7B)

Figure Step 7A
Solid Model – Colored Faces

Figure Step 7B
Solid Model – Colored Faces

Step 8

Set the material to: Cast Iron and find the following:

A The mass in pounds.
____________________________

B The mass in grams.
____________________________

Step 9

Save and close the part.

The Inventor book was written with competency based modules. What that means is that you have not completed each module until you have mastered it. The Competency Test module contains multiple choice questions and a comprehensive lab exercise to test your mastery of the set of modules that you completed. There are no answers or keys supplied in a Competency Test module since it is meant to be checked by your instructor. If there are any parts of this module that you have trouble completing, you should go back and reread the module or modules containing the information that you are having trouble with. If necessary, redo as many lab exercises required until you fully understand the material.

If you are Completing this book:

• Without the aid of an instructor, complete the written test and the lab exercise.
• In a classroom with an instructor, the instructor will give instructions on what to do after you have completed this module.

Multiple Choice Questions

Select the BEST answer.

1. When you are selecting objects with a window, which window selects all the objects that are totally inside it and the ones that it crosses?
   1. Square Window
   2. Crossing Window
   3. Extruded Window
   4. Rectangular Window
   5. Polygon Window
2. What is the name for two or more objects that are connected at their endpoints and then treated as one object in the OFFSET command?
   1. Loop
   2. Continuous
   3. Area
   4. Polyloop
   5. Window
3. What are the basic sketching planes (XY, XZ, YZ), the three axis (X, Y, Z) and the Center Point called?
   1. Work Planes
   2. Work Points
   3. Work Features
   4. Work Sketches
   5. Work Axis
4. What is the maximum number of sides that the POLYGON command can draw a regular polygon?
   1. 20
   2. 100
   3. 120
   4. 180
   5. 256
5. When the graphic cursor appears as a ruler, what units are you measuring in? Select the BEST answer.
   1. English Units
   2. Document Units
   3. System Units
   4. Metric Units
   5. Actual Units
6. What command is used to extend the length of an existing line or an arc?
   1. LENGTHEN
   2. EXTEND
   3. LINE
   4. LENGTH
   5. STRETCH
7. What does an aligned dimension measure?
   1. The delta X or delta Y distance between two points.
   2. The diameter of circle or radius of an arc.
   3. The true length of a line or the true distance between two points.
   4. The horizontal or vertical distance between two points.
   5. The angle between two lines or the angle between the imaginary lines between three points.
8. What best describes the threads created using the THREAD command?
   1. Graphical representations of the actual thread.
   2. A texture
   3. The actual thread.
   4. They are enlarged to look better.
   5. Center
9. What is a parametric construction plane inserted on the model or in model space called?
   1. A Work Plane
   2. A Work Point
   3. A Work Feature
   4. A Work Sketch
   5. A Work Model
10. What is an angular dimension measuring?
    1. The delta X or delta Y distance between two points.
    2. The diameter of circle or radius of an arc.
    3. The true length of a line or the true distance between two points.
    4. The horizontal or vertical distance between two points.
    5. The angle between two lines or the angle between the imaginary lines between three points.

Lab Exercise 21-1

Time allowed: 2 hours.

Step 1

Project the Center Point onto the Base plane.

Step 2

Note the location of X0Y0Z0. Draw the necessary sketches and extrude them to produce the solid model shown below. Apply all of the necessary geometrical and dimensional constraints to maintain the objects shape and size. All sketches must be fully constrained. (Figure Step 2A and 2B)

Figure Step 2A
Suggested Base Sketch –
Right Side (YZ) Plane

Figure Step 2B
Dimensioned Multiview Drawing
Competency [Click to see image full size]

Step 3

Create the fillets and chamfers after the model is totally constructed.

Step 4

Apply the colour shown above. (Figure Step 4)

Figure Step 4
Solid Model
Home View

Step 5

Move the End of Part Icon up above the fillets as shown in the figure. Suppress all of the threaded features. (Figure Step 5)

Figure Step 6

Step 6

Find the following to a precision of 6 decimal points: (Figure Step 6)

Figure Step 7

A The XYZ coordinates of corner D.

____________________________

B The length of the edge from corner A to corner B.

____________________________

C The distance from corner A to corner C.

____________________________

D The distance from corner C to corner D.

____________________________

E The angle between the edges B to C and B

____________________________

Step 8

The area of the shaded area of Figure Step 8. Do NOT include the area of features on the plane.

____________________________

Step 9

The perimeter of the shaded plane in Figure Step 9.

____________________________

Figure Step 9

Step 10

The area of the shaded area of Figure Step 10. The area should include the complete surface without any features.

____________________________

Figure Step 10

Step 11

Using the three figures below, change the colors of the faces shown to: Aluminum – Polished. (Figure Step 11A, 11B, and 11C)

Figure Step 11A

Figure Step 11B

Figure Step 11C

Step 12

• If you are a student completing this course in a classroom setting, your instructor will give you instructions on what to do after you complete this module.
• If you are an online student doing this course by correspondence, send an email to your instructor with the answers from the measurement questions in this module. For example:

The answers in the email can be given as follows:

An Assembly File

An assembly file contains the information required to assemble two or more part files to create an assembled model. See Figure 22-1. As the model is assembled, assembly constraints must be assigned so that each part knows how it aligns or fits with the other parts in the assembled model. A part (.ipt) file that has been placed in the assembly can be edited while in the assembly file and the modifications will be saved back to the original part file. On the other hand, if the original part file is modified after the assembly file has being created, the modifications will automatically display in the assembly. An assembly file does not actually contain any of the part files that are placed in the file, it simply contains a reference to them.

Figure 22-1
An Assembled Model

A reference is a link back to the part files. The part files that have been placed in an assembly file must be available to Inventor to display them when an assembly file is opened. The current project file keeps track of those links and will automatically keep track of the location of all the part files. If an assembly file is sent to a client or an associate, the part files that were placed in the assembly file must also be included.

Creating an Assembly File

To create an assembly file, use the NEW command and select an assembly template rather than a part template. An assembly file has the extension .iam. IAM is an acronym for Inventor Assembly.

Bottom-up vs Top-down

Assembly files can be created using either the bottom-up or the top-down method. A bottom-up assembly is an assembly created from a series of part files that were previously created and saved in their own .ipt file. A top-down assembly is an assembly file where all parts of the assembly are created on the fly. In other word, they are created in the active assembly file, one at a time. They are aligned and constrained in their correct position in relationship to the other parts in the assembled model. Inventor will save each part in its own file with the extension .ipt. In the Inventor book, only the bottom-up method is taught.

The Browser Bar in an Assembly

When an assembly is the active file, the Browser bar will display all of the parts that have been placed in the assembly. If a part in the browser is expanded it will display its children which includes its alignment and constraints to the other parts of the assembled model. See Figure 22-2.

Figure 22-2
An Assemble in
the Browser Bar
Inventor

If the same part is placed more then once into the assembly file, the Browser bar will number them accordingly. For example, this may happen if an assembly required two identical bolts. Only one part file is created and named Bolt.ipt. It is then placed into the assembly file twice. The Browser bar would number the bolts parts as follows:

On the first occurrence: Bolt:1

On the second occurrence: Bolt:2

WORK ALONG: Creating the Parts for an Assembly

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Use the following instructions to complete all parts in this workalong. Create the following parts and ensure that you do the following:

A Each part must be saved in its own .ipt file.

B Project the Center Point onto the Base sketch plane and note the location of X0Y0Z0.

C Draw the necessary sketches and extrude or revolve them to produce the solid model shown. Apply all of the necessary geometrical and dimensional constraints to fully constrain each sketch.
D Apply the colour and material shown.

Step 3

Construct Part A. (Figure Step 3A, 3B, and 3C)

Part: Base

Part Name: Inventor Workalong 22-1A

Template: English-Modules Part (in).ipt

Color: Stainless – Brushed

Material: Stainless Steel

Figure Step 3A
Solid Model – Home View

Figure Step 3B
Solid Model – Orbited View

Figure Step 3C
Dimensioned Multiview Drawing [Click to see image full size]

Step 4

Construct Part B. (Figure Step 4A and 4B)

Note: See Steps 3 to 14 if you require help creating this model.

Part: Post

Part Name: Inventor Workalong 22-1B

Template: English-Modules Part (in).ipt

Color: Chrome – Black Polished

Material: Steel

Figure Step 4A
Solid Model –
Home View

Figure Step 4B
Dimensioned Multiview Drawing

Step 5

Draw the Base model of part 22-1B by extruding circles. Your Base model should appear as shown in the figure. (Figure Step 5)

Figure Step 5

Step 6

Start a new sketch on the top of the model and draw a construction line from the centre to the edge of the top plane along the Y axis as shown in the figure. Hint: Ensure that you draw the line along the Y axis by snapping to the centre of the circle and to the grid on the Y axis. The length of the line is not important. (Figure Step 6)

Figure Step 6

Step 7

Insert a Work Plane in the centre of the model using the Perpendicular to a Line method. Enter the WORK PLANE command and move the cursor to the end of the construction line. The Work Plane icon will display as shown in the figure. Click the end of the line when the icon displays. (Figure Step 7)

Figure Step 7

Step 8

Move the cursor onto the Y axis and it will display as shown in the figure. When the Y axis is displayed, click it and the Work Plane will display as shown. (Figure Step 8A and 8B)

Figure Step 8A

Figure Step 8B

Step 9

Enlarge the Work Plane to extend it past the edges of the model. One way to do this is to use the LOOK AT/VIEW FACE command and change the view so that it is looking perpendicular to the plane as shown in the figure. (Figure Step 9)

Figure Step 9

Step 10

Start a new sketch on the Work Plane. (Figure 10)

Figure Step 10

Step 11

Enter the SLICE GRAPHIC command (F7) and the model will display from the sketching plane back. Disable the grid display. It is easier to draw this sketch without the grid. (Figure Step11)

Figure Step 11

Step 12

Using the PROJECT GEOMETRY command, project the Z axis and the X axis onto the sketching plane. (Figure Step 12A and 12B)

Figure Step 12A

Figure Step 12B

Step 13

Using the OFFSET command, construct offsets to both the Z and X axis to start the construction of the slot. Trim the lines in the sketch and insert the dimensions to fully constrain the sketch. Ensure that you dimension from both sides of the Z axis as shown in the figure. (Figure Step 13A and 13B)

Figure Step 13A

Figure Step 13B

Step 14

Extrude the sketch. Set it to extrude in both directions and to cut. Set the distance to All. Complete the part by adding the hole, the threads, the fillets, the colour, and the material as specified in Figure 14A, 14B, and 14C.

Figure Step 14A [Click to see image full size]

Figure 14B

Figure 14C

Step 15

Create Part C. (Figure Step 15A, 15B, 15C, and 15D):

Part: Wedge Ring

Part Name: Inventor Workalong 22-1C
Template: English-Modules Part (in).ipt
Color: Titanium – Polished
Material: Titanium

Figure Step 15A
Solid Model – Home View

Figure Step 15B
Solid Model
– Orbited View

Figure Step 15C
Dimensioned Multiview Drawing

Figure Step 15D
The Base Sketch

Step 16

Construct Part D. (Figure Step 16A and 16B)
Part: Wedge
Part Name: Inventor Workalong 22-1D
Template: English-Modules Part (in).ipt
Color: Chrome – Polished
Material: Steel

Figure Step 16A
Solid Model – Home View

Figure Step 16B
Dimensioned Multiview Drawing [Click to see image full size]

Step 17

Change the face colour of the top face of the part to: Metal Steel (Knurled) as shown in Figure 16A.

Step 18

Construct Part F as follows: (Figure Step 18A and 18B)
Part: Handle
Part Name: Inventor Workalong 22-1E
Template: English-Modules Part (in).ipt
Color: Metal-AL-6061 – Machined
Material: Steel

Figure Step 18A
Solid Model – Home View

Figure Step 18B
Dimensioned Multiview Drawing

Step 19

Construct Part E as follows: (Figure Step 19A, 19B, and 19C)
Part: Screw
Part Name: Inventor Workalong 22-1F
Template: English-Modules Part (in).ipt
Color: Metal-AL-6061 – Machined
Material: Steel

Figure Step 19A
Dimensioned Multiview Drawing [Click to see image full size]

Figure Step 19B
Solid Model –
Home View

Figure Step
19C
Solid Model –
Orbited View

Step 20

Change the face colour of the cylindrical top of the part to: Metal Steel (Knurled) as shown in the solid model figure.

Grounded Parts

By default, the first part that is placed into an assembly file will be grounded. A grounded part is a part that has all of it degrees of freedom removed and is fully constrained in that file. It is important to ground at least one part of every assembly. If no parts are grounded, the assembly can be moved around in model space. Once one part is grounded, the other parts can be constrained to it making their movement relative to the grounded part. If required, more then one part can be grounded.

In the Browser bar, a grounded part will display a Push Pin icon as shown in Figure 22-3 and 22-4. To enable or disable a part being grounded, right-click the part in the Browser bar. In the Right-click menu, select Grounded. In Figure 22-5, the selected part is currently grounded, enabled and visible.

Figure 22-3 Grounded Part as it Displays in the Browser Bar

Figure 22-4
Grounded Part Icon

Part Visibility

The visibility of parts in an assembly can be enabled or disabled. When the part’s visibility is disabled in the assembly, the part’s icon in the Browser bar will display greyed out.

Enabled Parts

Parts can be enabled or disabled in the assembly file. If a part is enabled, it displays and can be selected in the assembly. If it is disabled, only an outline displays and It cannot be selected. Sometimes it is easier to disable some parts to make it easier to place additional parts.

Assembly Constrains

There are many different constraints used when creating an assembly. In this module, only the mate constraint will be taught. A mate constraint constrains two assembled parts to one another by mating their centerlines and/or by mating a face on one part to a face on the other part. Mating is the most common way to assemble two parts together. It often takes more then one constraint to assemble two parts together. Both parts must have a symmetrical feature to mate them using the centerline method.

Figure 22-5
The Right-click Menu for a Part
in an Assembly File

USER TIP: The Browser bar contains a great deal of information about the active assembly file. The grounded part has a Push Pin icon. If a part is disabled, it will display a green part icon and if its visibility is disabled, the part icon will be grey as you can see in the figure.

WORKALONG: Creating an Assembly

Step 1

Check the default project and if necessary, set it to Inventor Course.

Step 2

Using the NEW command, enable the English tab and select the temple file: Modules Assembly (in).iam. Save and name the assembly: Inventor workalong 22-1. (Figure Step 2)

Figure
Step 2

Step 3

Enter the PLACE COMPONENT command. In the Place Component dialogue box insert part files: Inventor Workalong 22-1A.ipt and Inventor Workalong 22-1B.ipt into the assembly file. (Figure Step 3A and 3B)

Figure Step 3A [Click to see image full size]

Figure Step 3B

Step 4

Disable the grounding of part 22-1A and enable the grounding of part 22-1B. (Figure Step 4A, 4B, and 4C)

Figure Step 4A

Figure Step 4B

Figure Step 4C

Step 5

Enter the PLACE CONSTRAINT command. In the Place Constraint dialogue box set Type to Mate, Selections to 1, Offset to 0.000 and Solution to Mate. (Figure Step 5)

Figure Step 5

Step 6

Move the cursor onto the part 22-1A and move it until the Centerline constraint symbol appears. When it displays as shown in the figure, select it. Move the cursor onto the part 22-1B and do the same. Part 22-1A will move onto Part 22-1B. Click Apply. (Figure Step 6A, 6B, and 6C)

Figure Step 6A

Figure Step 6B

Figure Step 6C

Step 7

Move the cursor onto the top of the base on part 22-1B as shown in the figure. The mate arrow will display pointing up. Press F4 and rotate the model. Select the mate constraint for the bottom of the part 22-1A. (Figure Step 7A, 7B, and 7C)

Figure Step 7A

Figure Step 7B

Figure Step 7C

Step 8

Press F6 to change the Home view. (Figure Step 8)

Figure Step 8

Step 9

Enter the PLACE COMPONENT (P) command and insert part 22-1C, 22-1D, 22-1E, and 22-1F. Ensure that you place each part only once. (Figure Step 9)

Figure Step 9

Step 10

Using what you just learned, assemble and constrain part 22-1C. (Figure Step 10)

Figure Step 10

Step 11

Using the PLACE CONSTRAINT command, constrain the arc in part 22-1D to the arc in part 22-1C. (Figure Step 11)

Figure Step 11

Step 12

In the Offset box, set the offset to 0.015. Enable the Pick Part First box. See the Author’s Comments below. (Figure Step 12)

Figure Step 12