Las Vegas, Nevada, December 3 6, Speaker Name: Alan Kalameja. Course Title: Autodesk Inventor Assembly Modeling.

Las Vegas, Nevada, December 3 6, 2002 Speaker Name: Alan Kalameja Course Title: Autodesk Inventor Assembly Modeling Course ID: MA31-1 Course Outline: This class is designed to take an individual through the basics of assembly modeling using Inventor. Assembly constraints will be the main topic focused on during the discussion. Tips for successful assemblies will also be discussed. Adaptive assemblies will also be taught as a means of controlling the behavior of one part based on how the part was assembled. Design Constraints will also be demonstrated as a means of applying motion to an assembly model. A brief outline of all topics is listed below: Using Project Workspaces with Assembly Models Placing Components into an Assembly Applying Assembly Constraints to Individual Parts Using the Move and Rotate Component Tools Applying Motion and Transitional Constraints Creating New Parts While in an Assembly Using ALT-Drag Constraints Using Design Views in an Assembly Producing Adaptive Assemblies Using Sketch References in an Assembly Producing Adaptive Subassemblies Adaptive Sketches using 2D Layouts Using the Content Library Creating Component Patterns in an Assembly Producing Quarter, Half, and Three-Quarter Sections Replacing a Part in an Assembly Using imates and Composite imates Driving Assembly Constraints Creating Assembly Features Creating Presentation Models from an Assembly Placing a Parts List, Revision Table, and Revision Tag in an Assembly Drawing Assembly Modeling Productivity Tips

How Inventor Handles Assembly Models Autodesk Inventor software employs an innovative-segmented database, custom-built for working effectively with large assemblies. Called the Adaptive Data Engine, it enables users to quickly open and work with huge assembly models, and allows fast and automatic partial opens as well. The result is very high performance and overall greater productivity. The Adaptive Data Engine stores multiple data types in a single file with discrete segments. It optimizes system performance by automatically loading only those segments that are required for the current operation, then loading other segments on demand. Contrast that with traditional mechanical design systems, which load all assembly design data boundary representations (solids), feature data, graphics, and more into main memory, often resulting in page faults and swapping and slower performance, even though users may not require access to every data type for every model. Some Windows-based modelers try to solve this problem with lightweight parts and other technologies that cache a static version of the assembly s graphics. But such lightweight components or subassemblies cause problems when they become outdated without the user s knowledge and must be reloaded. The Adaptive Data Engine is fully associative, ensuring that all engineering deliverables including assemblies, subassemblies, components, notebooks, and drawings are always up to date. Using a Project Workspace with Assembly Models Autodesk Inventor uses projects to logically organize files and to maintain valid links between files. A project consists of a project home directory, a project file that specifies the paths to the locations of the files in the project, and the local and network folders containing Autodesk Inventor files. A project file is a text file with an.ipj extension. The file specifies the paths to the Autodesk Inventor files in the project. To assure that links between files work properly, add the location for all files to the project file before working on a project. You can use any text editor to create or edit the file. The project file for each project must be located in the home folder for the project. 2

You can have as many projects as needed to manage your work. A folder called a Projects folder contains shortcuts to all the project files you use. When you start a work session, Autodesk Inventor checks to find the Projects folder. If a Projects folder is not specified, or the specified folder cannot be found, you will be given the option of specifying one. A project file may simply specify the location of your workspace or can specify a number of paths both on your computer and on the network. A project file can contain the following sections: Included path files: Specifies the path and name of another project file. The information in the two files is merged. Only one project file can be included. Workspace: Specifies the default location for files. If all of the files for the project are located in one place, this may be the only entry in the project file. If you are working on a design team, the Workspace identifies your personal work area. Local search paths: Specifies additional file locations. The locations may be on your computer or on a network. Workgroup search paths: Shows the shared network locations where Autodesk Inventor searches for referenced files. Workgroup locations are used mainly when you are working in design teams. Library search paths: Shows the locations where Autodesk Inventor searches for standard parts or other named libraries. This path is the first searched by Autodesk Inventor. Sample Project Files: [Workspace] Workspace=I:\Temp\Inventor\WorkSpaces\Project1 [Included Path File] PathFile=I:\Program Files\Autodesk\Inventor R2\Samples\Models\Sample1\Sample1.txt [WorkSpace] WorkSpace=I:\Temp\Inventor\WorkSpaces\Sample1 [Local Search Paths] [Workgroup Search Paths] Workgroup=I:\Temp\Inventor\WorkSpaces\Base Assembly [Library Search Paths] SampleLib=I:\Temp\Inventor\WorkSpaces\Fasteners 3

Assembly Modeling Panel Bar Commands Assembly modeling commands can be selected from the Assembly Panel Bar illustrated below. These commands include the following; Place Component, Create Component, Place Constraint, Move Component, Rotate Component, and Quarter Section View. These commands will be discussed in greater detail throughout this document. The Assembly Browser displays a hierarchy of all component occurrences in the assembly. Each occurrence of a component is represented by a unique name. From the Browser, you can select a component for editing, move components between assembly levels, control component status, rename components, edit assembly constraints, and manage design views. Assembly Name Grounded Component Assembly Constraints Component Occurrence Sub-Assembly Name 4

Placing Components into an Assembly The first component in an assembly is automatically positioned with its origin coincident with the assembly coordinate origin. Additional components are positioned with the cursor, attached at the component center of gravity. Start with an assembly file that already contains the grounded first component. Click the Place Component button to choose a component to place. Go to the folder that contains the component, select the component, and click Open. The selected component is placed in the graphics window, attached to the cursor. Select a location and click to place an occurrence of the component. Move the cursor to a different location and click to place a second occurrence, continuing until all occurrences are placed. To quit, right-click and select Done. Note: You can drag and drop a component from Windows Explorer or a Browser window. Drag and drop places a single instance, unlike multiple occurrences as described above. Whether you place components through the dialog box or drag and drop, use assembly constraints to position components and remove degrees of freedom. 5

Applying Assembly Constraints to Individual Parts Activating the Place Constraint dialog box allows you to place the following constraints: Mate or Flush, Angle, Tangent, and Insert. Mate or Flush Constraint A mate constraint positions selected components face-to-face or adjacent to one another with faces flush. The geometry you select is usually a component face, but you can also select a curve, plane, or point. Angle Constraint An angle constraint controls the angle between edges or planar faces. Tangent Constraint A tangent constraint positions faces, planes, cylinders, spheres, and cones tangent to one another. Insert Constraint An insert constraint places a mate constraint between selected faces or mates cylinders along axes. For example, an insert constraint can be used to position a bolt in a hole. Note when applying constraints: If other components obscure selection, do one of the following: Temporarily turn off visibility before you place a constraint. Click to select a component, then rightclick and select Visibility. Select Pick Part First in the dialog box and click the component you want to constrain. Clear the check box to restore selection mode. 6

Using the Move and Rotate Component Tools Use the Move Component button on the Assembly toolbar to drag individual components in any linear direction in the viewing plane. 1. Click the component to drag to the new location. 2. Release the mouse button to drop the component. Moved components follow these guidelines: An unconstrained component remains in the new location until you constrain it to another component. A partially constrained component adjusts location to comply with a constraint. A constrained component snaps back to its constrained position when you update the assembly. A grounded component remains grounded in the new location. Components constrained to the grounded component will also move to the new location. Use the Rotate Component button on the Assembly toolbar to rotate an individual component. Follow the steps below: 1. Click the component to rotate. 2. Drag to the desired view of the component. 3. For free rotation, click inside the 3D rotate symbol and drag in the desired direction. 4. To rotate about the horizontal axis, click the top or bottom handle of the 3D rotate symbol and drag vertically. 5. To rotate about the vertical axis, click the left or right handle of the 3D rotate symbol and drag horizontally. 6. To rotate planar to the screen, hover over the rim until the symbol changes to a circle, click the rim, and drag in a circular direction. 7. To change the center of rotation, click inside or outside the rim to set the new center. 8. Release mouse button to drop component in rotated position. Note when moving or rotating components in an assembly: When you click Update, a constrained component snaps back to its constrained position. An unconstrained or grounded component relocates to the new position. Any components constrained to a grounded component snap into their constrained positions in the new location. 7

Robot Frame Project Create a new metric assembly model of the robot frame illustrated below. Use a combination of mates, flushes, and offsets to assembly the frame. 680Bar.ipt 50mm Offset Robot Base Sub.iam Use the following steps for creating this assembly: 1. Create a new metric assembly. 2. Place a new component called Robot Base Sub.iam. Place two occurrences of this sub assembly. 3. Place five occurrences of the part 680Bar.ipt. 4. Use a series of Mate-Mate and Mate-Flush constraints to assemble the robot frame. 5. Mate-Flush constraints with an offset of 50 mm will need to be applied to two 680Bar locations. 8

Piston Project Open the file Piston Assembly.IAM. Use Mate, Tangent, and Insert constraints to assemble the piston illustrated below. Wrist Pin Connecting Rod Piston Rod Cap Screw Rod Cap Use the following steps for creating this assembly: 1. Open the file Piston Assembly.iam 2. Use a series of Mate-Mate constraints to assemble the rod cap to the connecting rod. 3. Use an Insert constraint to assemble the rod cap screws to the rod cap. 4. Use a Mate-Mate constraint to assemble the wrist pin to the connecting rod. Use a Mate-Flush constraint along with the appropriate offset distance to assemble the face of the wrist pin to the face of the connecting rod. 5. Assemble the piston to the wrist pin using a Mate-Mate constraint and a Tangent constraint. 9

Applying Motion Constraints Motion constraints are used to specify intended motion ratios between assembly components. The first selected component moves relative to the second selected component. Two types of motion constraints are available. The rotation constraint type is used to drive such items as pulleys and gears. The Rotation/Translation constraint type is used to apply motion to rack and pinion components. Motion Constraints Project Use the following steps for applying motion constraints to this assembly: 1. Open the file Rotation_Assembly.IAM 2. Turn off the visibility of the Rotation_Gear Box part. 3. Apply motion constraints to the top face of each gear. 4. Change the solution type from Forward to Reverse. 5. Under Rotation_Plate:1 in the Browser, suppress the angle constraint. 6. Expand Rotation_Gear1 in the Browser and suppress the second flush constraint. 7. Test for motion by dragging one of the gears in a rotary direction. 10

Applying Transitional Constraints A transitional constraint will maintain contact between the two selected faces. A transitional constraint can be used between a cylindrical face and a set of tangent faces on another part. Transitional Constraints Project Open the file 02 Cam Follower.IAM Use the following steps for creating this assembly: 1. Open the file 02 Cam Follower.iam. 2. Activate the Place Constraint dialog box and select the Transitional tab. 3. In the assembly file, choose the red follower along the edge surface as the first selection. 4. For the second selection, select the edge surface of the cam. 5. To test the cam for functionality, suppress the angle constraint found in the Browser under the 02 Cam component. 6. Drag the cam in a rotary direction and observe the results of the follower. 11

Creating New Parts While in an Assembly You can create a new part in the context of an assembly file. Creating an in-place part has the same result as opening a part file, with the additional option of sketching on the face of an assembly component or an assembly work plane. To allow the size of the new part to change with assembly requirements, you can designate the part as adaptive and constrain it to fixed geometry in the assembly. To create an in-place part, use the following steps below: 1. Click the Create Component button. 2. When the Create In-Place Component dialog box appears, enter a name for the part and click OK. 3. Select a component face or work plane on which to sketch. 4. If you want to reorient the view to the sketch, click the Look At button. 5. Use the tools on the Sketch toolbar to create a sketch on a selected plane. 6. Select Extrude, Revolve, Loft, or Sweep to create a feature using the new sketch. 7. Continue to select faces on which to sketch and add new features as needed. When the part is complete, double-click the top-level assembly in the Browser to reactivate the assembly environment. Note: A mate constraint is automatically placed between the new sketch and the face or work plane. To omit this constraint, clear the check box in the Create Part In-Place dialog box when you create the part file. 12

End Plate Project Use the following steps for creating this assembly: 1. Open the file End Plate.IAM. 2. Create a new part called End Cap.IPT. 3. Check and verify that the current units are set to centimeters. 4. Pick the front face of the End Plate as the location for the new sketch plane. 5. Project the edges of the elliptical shape and the two holes. 6. Extrude the inner shape a distance of 10 cm. 7. Create a new sketch plane located between the End Plate and the End Cap. 8. Switch to wireframe mode and project the edge of the large circle. This circle will form a lip where the End Cap will fit into the End Plate. 9. Extrude this circular shape a distance of 3 cm into the part. 10. Create a new sketch plane along the top face of the End Cap. 11. Construct a circle with a diameter of 42 cm. Locate its center near the middle of the part. 12. Use horizontal and vertical constraints to line up the circle center with the center dots of the small holes and arc segments. 13. Extrude this shape a distance of 10 cm. 14. Create a new sketch plane along the top face of the extruded circle just created. 15. Project the edge of the small hole located in the End Plate. 16. Extrude and cut this circle through the plate. 17. Add fillets with a 3 cm radius to the edges of the End Cap. 18. When finished, select Finish Edit from the menu as shown in the following image. Complete this exercise by adding Mate constraints to fully assemble the End Cap to the End Plate. 13

Using ALT-Drag Constraints All assembly constraint types can be easily placed without activating the Place Constraint dialog box through the use of ALT-drag. To begin the ALT-drag process, hold down the ALT key and then click and drag on a surface or edge of an assembly component. This component must be ungrounded. Depending on the surface or edge that is picked, the following default constraints are applied: Mate Constraint - Clicking and dragging on a planar face or a linear edge. Tangent Constraint - Clicking and dragging on a cylindrical face. Insert Constraint - Clicking and dragging on a circular edge. While constraining using ALT-drag, the constraint type can be changed after the first component is dragged. To change to a different constraint type, release the ALT key and press one of the following shortcut keys: M or 1 Mate Constraint A or 2 Angle Constraint T or 3 Tangent Constraint I or 4 Insert Constraint R or 5 Rotation Motion Constraint S or 6 Slide Motion Constraint X or 8 Transitional ConstraintDuring the process of ALT-Drag constraining, different solutions can be cycled through by pressing the spacebar. The following solutions are affected by the spacebar: While in the Mate constraint, pressing the spacebar switches between mate and flush. While in an Angle constraint, the first component flips when pressing the spacebar. While in the Tangent constraint, the inside and outside solutions are switched when pressing the spacebar. While in the Insert constraint, the opposed and aligned solutions are switched when pressing the spacebar. 14

Cover Project Use the following steps for creating this assembly: 1. Open the file MDT Cover.IAM. 2. Use Alt-Constraints to assemble the gasket to the base using an Insert constraint. 3. Continue using Alt-Constraints to assemble the cover to the gasket using another Insert constraint. 4. Drag and drop a 0.25 x 1.00 Hex Head Bolt from the content library into this drawing. 5. Use Alt-Constraints to assemble the bolt to the cover using an Insert constraint. 6. Create a component pattern of six bolts to complete the assembly. 15

Using Design Views in an Assembly A design view preserves an assembly display configuration, which you can recall by name when you next work on the assembly. One advantage of using a design view is that you can turn off visibility of components you do not need to see and then save that view with a design view name. When you reload the design view, only the components you need are displayed. A design view captures the following display characteristics: Component visibility (visible or not visible) Component selection status (enabled or not enabled) Color and style characteristics applied in the assembly Zoom magnification Viewing angle Use design views to simplify the display of an assembly during the design process: Turn the display of components on and off as needed to visualize a problem. Create design views that have different purposes. You can define components as enabled or not enabled to allow selection when relevant to the current task. Open large assemblies quickly by displaying only the components needed for the immediate design session. Recall display configurations for individual designers working on a shared assembly. Save views of an assembly design in progress to preserve working ideas. Use design views to create drawing views to document the assembly. In the assembly, set up the design views, specifying view orientation, visibility, color, and other attributes of the components. Save each design view with a unique name and specify the design view to use when you create drawing views. 16

Producing Adaptive Assemblies An existing part can be useful in more than one assembly, as long as its size and shape can adapt. You can define the features of a part as adaptive when you create them in the part file. When you place such a part, you also define it as adaptive within the assembly, and allow features to resize and change shape when you constrain them to other components. In the early stages of assembly design, some requirements are known while others are subject to change. Adaptive parts can be useful because they adjust to design changes. Parts created in place and parts placed from part files can both be defined as adaptive. When you place a part in an assembly, its size is fixed unless you define the part as adaptive in the assembly. To define a part as adaptive, select the part in the graphics window or the Browser, right-click, and select Adaptive. When you constrain an adaptive part to fixed features on other components, underconstrained features resize when the assembly is updated. In general, use an adaptive part: When an assembly design is not fully defined, and a part is required in a particular position but its final size is not known. When the position or size of a feature will be determined by the position or size of a feature on another part in the assembly. Only one occurrence of a part can define its adaptive features. If you use multiple placements of the same part in an assembly, all occurrences are defined by the one adaptive occurrence, including placements in other assemblies. If you want to define different elements of a part as adaptive for different assemblies, save the part file with a unique name, and save its adaptive definitions, but do not use the original. Follow these guidelines to make sure adaptive features and parts update predictably: Use only one tangency per revolved feature. Avoid offsets when applying constraints between two points, two lines, or a point and a line. Avoid a mate constraint between two points, a point and a plane, a point and a line, and a line and a plane. Avoid tangency between a sphere and a plane, a sphere and a cone, and two spheres. Note: Parts created in external CAD systems cannot be made adaptive because imported parts are considered to be fully dimensioned. 17

Linkage Project Use the following steps for creating this assembly: 1. Open the file Adaptive Pins.IAM. 2. Use English units to create a new link bar as shown in the following image. 3. Extrude this sketch a distance of 0.25. In the Browser, set this feature to Adaptive. 4. Assemble the link bar part to the Adaptive Pins assembly using Mate-Mate constraints. 5. Experiment using Mate-Flush constraints on the part and observe the results as the part adapts to the assembly. 18

Using Sketch References in an Assembly Loops, edges, and complex shapes in an assembly can be easily updated when the underlying geometry is modified through Sketch References. These cross part relationships are managed similarly to other adaptive relationships. A new In-Place Features option, which is part of the Assembly tab of the Options dialog box, controls whether loops and edges that are projected across parts will be associative. By default, projected edges will be associative. To disable the associativity, hold down the CTRL key during the projection process. To create a temporary break between the associative sketch and the reference part, turn Adaptivity off through the Browser. Sketch Block Project Use the following steps for creating this assembly: 1. Open the file Sketch Block.IAM. 2. Double-click on the Sketch Block to edit this part in-place 3. Add a rectangular lug on the front face of the Sketch Block. The dimensions of the rectangle measure 2 by 1. Add a 0.50 diameter circle to this lug. 4. Extrude this sketch 0.25 into the Sketch Block. 5. Create a work plane. Select the top face of the Sketch Block and offset the work plane 2. 6. Mirror the lug to the other side of the Sketch Block using the work plane just created as the mirror plane. 7. When finished making changes to the Sketch Block, right-click and select Finish Edit from the menu 8. Notice how the cover adapts to the changes made to the Sketch Block. 19

Producing Adaptive Subassemblies Subassemblies can be defined as adaptive. You can drive the size of components in the subassembly by applying constraints across all subassembly parts. In the Browser, click on the designated subassembly and make it adaptive. All other instances of the subassembly do not display the adaptive icon; however all of these instances will behave in the same way. Scoop Project Use the following steps for creating this assembly: 1. Open the file Chief Scoop.IAM. 2. Assemble the four Chief Cylinders to the Chief Plates and Scoops. Use a series of Mate-Face and Mate-Center constraints to accomplish this. 3. When all four cylinders have been assembled, right-click on the first cylinder in the Browser and select Adaptive from the menu. 4. Drag one of the scoops and notice the other scoop moves. 20

Adaptive Sketches using 2D Layouts You can use a sketch to represent functional aspects of your design, such as outlines and pivot points, and add work features through key sketch points before features are created. A 2D layout can then be assembled with other layouts to quickly verify a design concept. For example, you can create a mechanism out of 2D sketched parts, constrain the joints together, and drive the constraints so that you can observe the motion. Changing the sizes of parts is as simple as dragging their sketches. Once you have the relationships defined, you can finalize the shapes and create the features. You can create a layout sketch of a part file in an assembly. The 2D geometry in the sketch forms the basis of an assembly layout. Analyze your assembly design to determine if this technique will be useful. Then use the following guidelines: In the part environment: 1. Create a new part file. 2. Add sketch geometry and work features to the first sketch as needed. 3. Add dimensions and constraints to position the sketch geometry. 4. Continue to construct additional work features and sketch geometry on the first sketch, adding dimensions and constraints as needed. 5. Click Update to recalculate the work feature positions. 6. Save the part file. In the assembly environment: 1. Create an assembly file. 2. Place the file containing the sketch geometry and work features as a normal part file. 3. In the assembly, activate the part file for in-place editing. 4. Use work planes as surrogate faces on which to create other work features and sketches. 5. Use sketch constraints and dimensions to position the geometry. 6. Click Update to recalculate the work feature positions. When you place or create new parts in the assembly, use the work features to position them. For example, you can constrain a cylindrical part to a work axis or mate a part face to a work plane. If needed, edit the dimensions to reposition the parts. 2D Sketch 21

Using the Content Library To display the Standard Parts Library, select the Model button from the Browser and then select Library. The Browser changes to display the Standard Parts Library that supports 18 international standards and up to 12 different classes of standard parts in the form of screws, nuts, pins, rivets and even structural shapes. When working with the content library, you can perform searches, view the placement history, and keep a list of your most commonly used standard parts in a favorites section. Since a majority of the parts assembled in a machine consist of standard and purchased items, this comprehensive parts library makes it easier to find and use standard parts quickly and efficiently. 22

Creating Component Patterns in an Assembly Arranging assembly components in a pattern saves time, increases your productivity, and captures design intent. For example, you may need to place multiple bolts to fasten one component to another or place multiple subassemblies into a complex assembly. Below are examples of the Rectangular and Circular tabs of the Pattern Component dialog box You can create a circular pattern by specifying the number of components and the angle between then. You can create a rectangular pattern by specifying column and row spacing. You can create both circular and rectangular patterns by matching features patterned on a part. Usually, you pattern components at several points in the assembly design process. After you place a component in an assembly. When you place a component: You position it using an existing part feature pattern. You select the component and copy it into a pattern. 23

Pipe Project Use the following steps for creating a component pattern in this assembly: 1. Open the file Pipe Assembly.IAM 2. Activate an existing design view called Bolt Assembly. 3. In the Browser, select the Bolt, Nut, and two Washer parts. Right-click on one of these parts and select Demote from the menu. 4. When the Create In-Place Component dialog box appears, enter Cap_Fastener as the new file name. 5. Click OK to the warning message that states that some assembly constraints may be lost. 6. Notice the new listing in the Browser called Cap_Fastener.IAM. 7. Drag the Cap_Fastener assembly away from the hole to show that the constraints were lost. 8. Apply an Insert constraint from the bottom of the washer to the top of the hole. 9. Select the Pattern Component tool and pick the Cap_Fastener assembly. 10. Click the Select button in the Feature Pattern Select area. 11. Pick any hole along the top surface of the plate. 12. When all holes highlight, click OK to place the pattern. 13. The completed exercise is illustrated in the following image. 24

Producing Quarter, Half, and Three-Quarter Sections You create a section view to visualize portions of an assembly within chambers or that are obscured by components. While the assembly is sectioned, you use part and assembly tools to create or modify partsin-place. To begin, open an assembly file containing one or more components. Set visibility for components. Select the component in the graphics window or the Browser, then: 1. To hide components, right-click and clear the check mark beside Visibility. 2. To show components in wireframe for context, right-click and clear the check mark beside Enabled. 3. Click one of the Section View tools on the Assembly toolbar, then select any planar or work plane to define the cutting plane. 4. Right-click and select Flip, if necessary to display the desired view of the section. 5. Click the Create Component tool on the Assembly toolbar. When prompted to select a sketch plane, select the plane used to define the section. 6. If desired, use the Project Cut Edges tool on the Sketch toolbar to project edges of a part cut by the section plane onto the sketch plane. 7. Use sketch and feature tools to create new geometry. Note: From Quarter section and Three-quarter section views, you can right-click and select the opposite view. 25

Replacing a Part in an Assembly You can replace one assembly component with another component, but existing assembly constraints are deleted. 1. Click the Replace Component tool, then click a component to replace. 2. In the Open dialog, go to the folder that contains the component, select the component, and click Open. 3. A warning message notifies you that constraints will be deleted. Click OK to continue or Cancel to discontinue replacing a component. Hinge Project Use the following steps for replacing a part in this assembly: 1. Open the file Hinge Assembly.IAM. 2. Replace the arm with the file New Arm Assembly.IAM. 3. Since the replacement part needs to have constraints added, use the Insert constraint to assemble the edge of the bushing with the edge of the adjacent hole. Also, enter an offset value of -0.0025 which will act as clearance between the bushing and hole. 4. Drag the new arm and check for proper movement. 5. To perform a collision detection on the assembly, add an angle constraint between the face of the hinge and the face of the new arm. 6. In the Browser, locate the angle constraint just created, right-click on this constraint, and select Drive Constraint from the menu. 7. In the Drive Constraint dialog box, make the following changes: Enter -78 in the Start field. Enter -85 in the End field. Expand this dialog box. Enter a value of 0.1 degree in the Increment field. Be sure to place a check in the box next to Collision Detection. 8. Click the Reverse button to drive the constraint. The motion will stop when interference is detected between the arm and hinge. 26

Using imates imates are predefined assembly constraints. One set of imates is attached to a part and another set is attached to the mating part. imates are ideal for defining standard constraints in such components as nuts, bolts, plates, and shafts. Multiple imates are able to be attached to a part. imates are defined as the component is being created. When creating imates, there must be a name match between the primary imate of the placed component and the unconsumed imate half. The imate is indicated by a single imate symbol in the Browser and the graphics window. End Connector Project Use the following steps for creating imates in this assembly: 1. Open the file imate End.IAM. 2. Add an imate to the centerline axis of the threaded hole. 3. Add an imate to the face of the housing. 4. Add an Angle imate to the top face of the housing. 5. Rename imate:1 to Axis1 6. Rename imate:2 to Face1 7. Leave iangle:1 as is. 8. Your model and Browser should appear similar to the following image. 27

IMate Assembly Project Use the following steps for assembling imates: 1. Open the file imate Assembly.IAM and examine the imates already created. 2. Place a single occurrence of the component imate End.iam into this assembly. 3. Match the imate axis at the end of the rod with the threaded hole axis. 4. Match the imate face at the end of the nut with the face of the end connector. 5. Match the Angle imate with the center of the rod and the face of the end connector. 6. Place the component imate Mount.ipt into this assembly and automatically have it assemble to the rod. 7. Your assembly should be similar to the following image. 28

Using Composite imates imates can also be grouped into a single composite imate. In this way, ALT-dragging the composite imate rather than using individual imates can easily assemble a component or subassembly in one easy step. The following steps are used for creating a composite imate: 1. Create the individual imates. 2. Select all imates located in the Browser. 3. Right-click and then select Create Composite from the shortcut menu. In order to make sure that a successful match will occur between any two imates in an assembly, the imate type and values must match. These imate names are used for pairing purposes. Adjustable-End Project Use the following steps for creating composite imates: 1. Open the file Composite imate Assembly.IAM. 2. In the Browser, expand imates and observe the results. 3. Begin the process of combining all imates into one by first selecting the three imates, right-clicking, and selecting Create Composite from the menu. Notice a single imate glyph present on the End Connector. 4. In the Browser, rename icomposite:1 to Adjustable-End 5. Use the Save Copy As command from the File menu and save this assembly as Adjustable-End. 29

Composite imate Assembly Project Use the following steps for creating an assembly using composite imates: 1. Open the file Composite imate Assembly.IAM. 2. Place a new component occurrence called Adjustable-End.IAM 3. Expand the Browser for both assemblies and notice the imates are identical. 4. Use Alt-Drag constraining to assemble the Adjustable-End to the end of the rod. 5. Place another new component occurrence called Composite imate Mount and check the Use imate box. Notice how this component is automatically placed in the assembly and orientates itself based on the imates. 6. Click the Replace Component tool. Choose Adjustable-End as the component to replace. From the file listing, choose Composite imate Clevis.ipt as the replacement component. 7. Notice in the following image that the new replacement component automatically assembles itself based on imates. 30

Driving Assembly Constraints Use the Drive Constraint tool on the context menu to simulate mechanical motion by driving a constraint through a sequence of steps. The Drive Constraint tool is limited to one constraint, but you can drive additional constraints by using the Equations tool to create algebraic relationships between constraints. To begin, constrain two components together. 1. In the Browser, right-click on the constraint and select Drive Constraint. The Drive Constraint dialog box opens. 2. In Start, enter the beginning value. The default value is the angle or offset defined for the constraint. 3. In End, enter the ending value. The default is the Start value plus ten. 4. In Pause Delay, set the time between steps. Adjust the default value to speed up or slow down motion. 5. Click the More button to set options, as follows: 6. Select the Drive Adaptivity check box to adapt components to fit constraint value, if needed. 7. Select the Collision Detection check box to check for interference. 8. Set the Increment between steps by specifying either the value or the total number of steps. Value may be entered, measured, or as dimensioned. 9. Set the Repetition of the sequence: Start/End runs once and returns to the beginning; Start/End/Start runs once forward, then once backward. If desired, enter a value to run the sequence more than once. 10. Click the Forward button to start the sequence or click the Step Forward button to advance the sequence one step at a time. 31

After the sequence begins, you can click the Stop button, click Forward or Reverse, Step Forward or Step Reverse, or Go to Beginning or Go to End. Note: To record the driven constraint sequence, click the More button to set the Avi rate, then click the Start Recording button. To reduce size of the animation file, reduce the graphics window size and use a solid background color. Twist Clamp Project Open the file Twist Clamp.IAM Apply a drive constraint using the information from the dialog box as a guide. Double Slider Coupling Project Open the file Double_Slider_Coupling.IAM Apply a drive constraint using the information from the dialog box as a guide. 32

Creating Assembly Features Assembly features are features that are defined in an assembly. They only affect a part when the part is viewed in the context of the assembly. Assembly features allow you to remove material from various components after they have been assembled. Examples of material removal processes include matchdrilling operations and post-weld machining operations. Typical operations involving assembly features include cutting extrusions, drilling holes, and cutting chamfered edges. A number of assembly practices involve the addition of a set of features (often including parts) following the assembly of the as designed piece parts. A common example, as shown in the following image of the timing cam assembly, would be to drill and pin following assembly. Parts are placed that need to be precision-located following some assembly adjustments, making the prior location of the holes impractical from a cost efficiency perspective. Once the correct timing position is set relative to the key seat and other parts in the drive train, the cam is pinned in position, as shown in the following image. A hole, which does not exist in the hubs or cam plate, is drilled and the pin is pressed in place. 33

Creating Presentation Models from an Assembly You can develop exploded views and other stylized views of an assembly and use them to create drawing views that document your design. The stylized views are saved in a separate file called a presentation file. Each presentation file can contain as many presentation views as needed for a specified assembly. Using Design Views to Create Presentation Views You can develop design views in the assembly and use them to create presentation views. For example, turn off the visibility of some parts in a complex assembly and save a design view that shows only certain components. In the presentation file, you can use that design view to set up an exploded view of those components. Developing Exploded Presentation Views You can automatically explode the view when creating a new presentation view. Assembly constraints will be used to determine the direction that the components will move to create the view. After placing the view, you can manually tweak individual components in the view to create the optimum view of the components. Note: Presentation views do not recognize assembly constraints for any purpose other than creating the first automatic explosion. You can manually tweak a component along any specified vector. 34

Placing a Parts List in an Assembly Drawing Use the Parts List button on the Drawing Annotation toolbar to place a parts list. A parts list uses the formatting set in the active drafting standard. 1. Click the Parts List button. 2. In the graphics window, select the drawing view for the list. 3. In the Create Parts List dialog box, select the level and range of parts for the list and click OK. 4. Note: When First-Level Components is selected, the Range is automatically set to All. 5. Move the indicator in the graphics window and click to place the parts list. The parts list will snap to edges or corners of the sheet or to the title block. Tip: To move a parts list after it is placed, move the cursor over the parts list, then drag the green dot to move it to the desired location. Placing a Revision Table To formally display and keep track of engineering drawing changes, a revision table is inserted. Once a revision table has been placed, double-click on any value in a field. The dialog box that appears will allow you to change its value. To keep track of changes on the actual drawing, the part that has been changed can be flagged with a revision tag. This tag should correspond with the information located in the revision table. 35

Placing Balloons in an Assembly Drawing Use the desired Balloon button on the Drawing Annotation toolbar to add reference balloons to a drawing. Note: If you add balloons to a drawing before creating a parts list, the balloons will show the item numbers of first-level components. You can select a balloon and change it to show the item number of the part to which it is attached. To Add Balloons to Individual Parts: 1. Click the Balloon button. 2. In the graphics window, select the part and then click to set the start point for the leader line. 3. Move the cursor and click to add a vertex. 4. When the symbol indicator is in the desired position, right-click and choose Continue to place the symbol. The symbol style is determined by the active drafting standard. Continue placing balloons. When you finish placing balloons, right-click and select Done from the menu to end the operation. To Add Balloons to All Parts in a Drawing: 1. Click the arrow next to the Balloon button and select Balloon All. 2. In the graphics window, select the view. Note: The balloons are added to either the top-level components or to all parts, depending on the balloon setting in the active drafting standard. 36

Robot Frame Project Use the following steps for inserting a parts list, balloons, and revision table into this drawing: Open the file Robot Frame Drawing.IDW Add a parts list to the lower right corner of the title block. Add a revision table to the upper right corner of the border. Add a revision tag to one of the parts and edit the revision table. 37

Assembly Modeling Productivity Tips Customize Assembly Viewing As you add components, turn off visibility of components, which no longer impact the portion of the design on which you are currently focused. Turn off visibility of non-essential components and save the design view with a unique name. Reload the design view whenever you work on the assembly. Pause over a component in the Browser to highlight it on the graphics screen. Right-click and select Find in Browser or Find in Window to locate components. Save a design view of a complex subassembly and turn on visibility for only the components needed to place the subassembly. Use that design view when you place the subassembly. Turn off enabled status for parts you do not need to select but need to see for frame of reference. Use color to segregate subsystems in an assembly. For example, display all components in the pneumatics system in one color, all components supplied by a certain vendor in another color, and so on. Plan For Efficiency Plan the top-level assembly and subassembly structure before you create parts. Create logical subassemblies and combine them into larger assemblies. Keep all components used in a subassembly in the same directory. Create a shared network directory for components that will be shared by many designers on many projects. Fill-in the Summary and Project properties for individual components. Create a unique template and use it to create components for a specific project or subassembly. Pre-define common properties in the template so all components created from that template inherit the properties. Assign imates to standard parts such as nuts, washers, bolts, and shafts. Manage Assembly Constraints Use only as many constraints as are needed to control component position and movement. Pause the cursor over a constraint in the Browser to highlight it in the graphics window. Avoid constraints between features that might be removed later in the design process. Credits Special thanks to the developers of the Autodesk Official Training Courseware for Inventor Versions 2, 4, and 5 for use of the models and assemblies used for this presentation. 38