Assembly Design Workflows - Mastering Autodesk Inventor 2015 and Autodesk Inventor LT 2015 (2014) 

Mastering Autodesk Inventor 2015 and Autodesk Inventor LT 2015 (2014)

Chapter 8. Assembly Design Workflows

A typical assembly file is composed of links to the included components and assembly relationships. The components are parts or subassemblies that exist as separate files. When components are placed into an assembly file, links to those individual files are created in the assembly file. Initially a component is free-floating and can be moved and rotated in any direction unless it's grounded in place or constrained to other components.

For example, if you were to create an assembly of a simple drilled base plate and a bolt to be inserted in the hole, you would have three files:

·     The assembly file (with a filename extension of .iam)

·     The base plate part file (with a filename extension of .ipt)

·     The bolt part file (with a filename extension of .ipt)

When the part files are placed into the assembly file, links are created to the locations of those files. If the hole in the base plate part is enlarged, the assembly is automatically updated to reflect that change since it is linked to the part file. To assemble the plate and bolt, at least one assembly relationship would be created by selecting the shaft of the bolt and the hole in the plate. Assembly relationships can be created using the Constraint tool or the Joint tool. Assembly relationships have two functions:

·     They define how two or more components relate to one another.

·     They limit the degrees of freedom any one component has in the assembly.

Developing a good assembly design workflow is paramount to achieving performance, flexibility, and stability in your designs. In this chapter, you'll explore several types of workflows to achieve that goal. Included in this chapter is a discussion on how to use subassemblies to enhance performance. Using subassemblies within your design can substantially improve performance. Component count can be in the hundreds of thousands of parts, as long as you have sufficient memory on your system.

In this chapter, you'll learn to

·     Create assembly relationships using the Constraint and Joint tools

·     Organize designs using structured subassemblies

·     Work with adaptive components

·     Create assembly-level features

·     Manage bills of materials

·     Use positional reps and flexible assemblies together

·     Copy assembly designs for reuse and configuration

·     Substitute a single part for entire subassemblies

·     Work with assembly design accelerators and generators

·     Use design calculators

Assembly Relationships

Mastering the use of the Constraint and Joint tools to create functional assembly relationships is an important part of learning to create assemblies in the Autodesk® Inventor® program. Assembly relationships are the glue and nails of construction when it comes to building your assemblies. Properly using assembly relationships will permit the construction of stable assemblies, assist in developing stack-up tolerances, and allow parts to be driven to show the animation of a process.

If you use assembly relationships improperly, you can create a nightmare of broken and/or redundant relationships, preventing assemblies from functioning properly, destroying assembly performance, and causing rework. Understanding how assembly relationships function in an assembly will help assure success in building and editing your design.

Another important concept for assembly relationships is the idea of removing or defining a component's degrees of freedom. When you create relationships between assembly components, you are also changing the way those components are allowed to move in the assembly, just as you do when you assemble parts in the real world.

Degrees of Freedom

Initially each component within an assembly file possesses six degrees of freedom. The degrees of freedom (DOF) are bidirectional and consist of three axial degrees of freedom along the origin x-, y-, and z- axes, as well as full rotational freedom around the same axes. You might think of degrees of freedom like the roll, pitch, and yaw of an aircraft. For a pilot to maintain control of the aircraft, the side-to-side roll, the up-and-down pitch, and the clockwise or counterclockwise yaw of the aircraft must be controlled. Likewise, you will create assembly relationships between your components to prevent them from moving freely or at least to control the way in which they are allowed to move.

For ease of use when learning to create assembly relationships between components, it might help to make the degrees of freedom visible through the View tab by clicking the Degrees Of Freedom button. As constraints are applied to your component, the DOF triad will change to show only the remaining DOF. When the component is fully constrained, the triad will disappear. Figure 8.1 shows the Degrees Of Freedom button and the resulting triad.

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Figure 8.1 Activating the Degrees Of Freedom view

You can also analyze the degrees of freedom for the complete assembly. The Degree Of Freedom Analysis button is located in the Productivity panel drop-down list on the Assemble tab. A dialog box displays each component (part or subassembly) at the active level of the assembly. The number of translation and rotation DOF are listed.

If you select Animate Freedom at the bottom of the dialog box and then select a component in the list, it will move to show the DOF, assuming it is not already fully constrained. Figure 8.2 shows the Degree Of Freedom Analysis dialog box.

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Figure 8.2 Animating an underconstrained component from the Degree Of Freedom Analysis dialog box

Follow these steps to animate the underconstrained component:

1.  Click the Get Started tab and choose Open.

2.  Browse for the file mi_8a_001.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  Click the View tab and then click the Degrees Of Freedom button to turn on the degrees-of-freedom triad for each part.

You'll notice that each part has an icon denoting the axes it is able to translate along or rotate around. There are only three triads shown because the part called 8–001 is grounded and cannot move at all. You can see this by looking at the browser and noting the push pin icon shown on that part.

Enable the Productivity Panel

If you don't see the Productivity panel, you might need to enable it. To do so, first make sure the Assemble tab is active; then right-click anywhere on the Ribbon menu and choose Show Panels. Select Productivity from the list.

4.  Click the Assemble tab, click the drop-down on the Productivity panel, and select Degree Of Freedom Analysis.

5.  Select Animate Freedom at the bottom of the dialog box.

6.  Click 8_002 in the list. Watch it rotate in the free axis, demonstrating its DOF.

7.  Click 8_003 in the list. Watch it rotate and move up and down, demonstrating its DOF.

8.  Click 8_004 in the list. Watch it rotate and slide along the face of the plate in two directions, demonstrating its DOF.

These tools can be helpful when you are trying to determine the assembly relationships applied to components in an existing assembly. In addition to animating DOF, you can also just click and drag a part to see how it can move. In either case, you might find that leaving the DOF triads turned on will help you as you learn how assembly relationships work and are created. You can close the current file without saving changes and continue on to the next section.

Grounded Components

A component can be grounded in place so that it cannot move or rotate unintentionally. A grounded component is fully constrained and has 0 degrees of freedom. Every assembly should have at least one grounded component so that it will be stable. If components are not grounded, the assembly can become misaligned from the x-, y-, and z-axes and will cause problems when you try to detail the assembly in the drawing environment. You can ground or unground any component in an assembly by right-clicking it and selecting Grounded from the context menu.

Placing Components in an Assembly

To place components in an assembly, you can use the Place button on the Assemble tab and then browse to locate the component. To ground a component while you place it, you can right-click during the placement preview and choose Place Grounded At Origin.

Additionally, you can drag part and assembly files from Windows Explorer and drop them into the assembly. To place additional instances of components already in the assembly, you can copy and paste components from the graphic window or simply click and drag them from the browser.

In certain workflows where parts are placed into the assembly in the correct position and orientation to begin with, all components can be grounded. This is done automatically when an assembly is created from a multi-body part using the Make Components tool. If a particular component needs to be adjusted, it can be ungrounded and then constrained using Assembly constraints or assembly connections.

The ground-all strategy can also be used to rebuild assemblies that have a great many errant Assembly constraints resulting from major uncontrolled changes. For instance, if you opened an assembly that has 50 constraints and of those 42 have errors, you might be better off to select all the components and ground them in place. Next, you would expand the Relationships folder in the browser and then select all of the relationships with errors and delete them. You could then leave everything grounded or unground and reconstrain them one at a time in order to fix the assembly.

How the Constrain Tool Works

In Inventor, Assembly constraints are used to attach parts or subassemblies together, creating assembly relationships between the components and therefore defining the way they fit together based on the selection of faces, edges, or vertices and user-defined parameters. In general practice, the function of constraints follows real-world assembly techniques where fasteners, adhesives, and welds attach one component to another.

There are seven basic types of constraints in Inventor. Most of the constraint types have multiple solution types that can be used to achieve the result you are looking for. Here is a list of the constraint types and their solutions:

1.  Mate constraints position components face to face or adjacent to one another.

·     The Mate solution positions selected faces normal to one another, with faces coincident; imagine two plates butted together.

·     The Flush solution aligns components adjacent to one another with faces flush; imagine two plates flushed along an outside corner.

2.  Angle constraints position two components at a specified angle to define a pivot point.

·     The Directed Angle solution always applies the right-hand rule to selected faces or edges.

·     The Undirected Angle solution allows either orientation and is used in situations where component orientation flips.

·     The Explicit Reference Vector solution defines the direction-of-rotation axis.

3.  Tangent constraints position two components to contact at a point of tangency.

·     The Inside solution positions the first selected component inside the second selected component at the tangent point.

·     The Outside solution positions the first selected component outside the second selected component at the tangent point.

4.  Insert constraints are a combination of a face-to-face Mate constraint between planar faces and a Mate constraint between the axes of the two components.

·     The Opposed solution reverses the mate direction of the first selected component.

·     The Aligned solution reverses the mate direction of the second selected component.

5.  Symmetry constraints position two components symmetrically to both sides of a selected plane or planar face. The Symmetry constraint is typically used in conjunction with other assembly relationships.

6.  Rotation constraints allow one component to rotate based on the selection of a second component.

·     The Rotation solution allows the first selected component to rotate in relation to another component using a specified ratio; imagine two gears.

·     The Rotation-Translation solution allows the first selected component to rotate as it translates the face of another component; imagine a rack and pinion.

7.  Transitional constraints specify the relationship between a cylindrical component and a contiguous set of faces on another component, such as a cam in a slot.

When using constraints, a minimum of two constraints are required to fully constrain two components together so that their relationship is fully defined. Underconstrained components allow motion in the unconstrained axis or plane. Components that are fully contained within a subassembly will not figure into the constraint analysis when the top-level assembly is opened or modified, so it is typically best for the performance of your assembly files to fully constrain all components that are not meant to be moveable. See “Working with Constraints” later in the chapter for more information.

How the Joint Tool Works

The Joint tool allows you to define the working relationship between a pair of components with a single joint relationship. With the Constraint tool you might create multiple constraint relationships to remove degrees of freedom; by contrast, you might achieve the same results with just one joint relationship, by defining the degrees of freedom you intended to remain. Although you can achieve the same result using the Constraint tool that you can with the Joint tool, the Joint tool results in fewer assembly relationships, which can be much easier to manage later.

Inventor offers six basic types of joints, as well as an Automatic option that will choose a type based on the selected inputs. Here are the joint types and options:

1.  Automatic joints create either a Rigid, Rotational, Cylindrical, or Ball joint, depending on the geometry of the selections.

2.  Rigid joints position a component in place and remove all degrees of freedom. This joint type is used for glued, welded, or bolted joints that do not move.

3.  Rotational joints position a component in place and create one rotational degree of freedom. This joint type is used for hinged joints and levers, and it can be created with a specified limit value.

4.  Cylindrical joints position a component in place and create one translational and one rotational degree of freedom. This joint type is used for creating a joint between a shaft and a hole, for example, and can be created with a specified limit value.

5.  Ball joints position a component in place and create three rotational degrees of freedom. This joint type is used for socket and ball joint type joints and can be created with a specified limit value.

6.  Slider joints position a component in place and create one translational degree of freedom. This joint type is used for hinged joints, levers, and so on, and it can be created with a specified limit value.

7.  Planar joints position a component in place and create two translational and one rotational degree of freedom perpendicular to the planar face. This joint type is used when one object will move along a planar surface such as a conveyor, and it can be created with a specified limit value.

See “Working with Joint Relationships” later in the chapter for more information.

Working with Constraints

As mentioned, several types of constraints are available for use in an assembly. To know which one to use and when, you should be familiar with each. Keep in mind, however, that certain constraint types are used more often than others. In the following pages, you will explore the creation of the various constraint types.

The Mate Constraint

The Mate constraint type consists of two solutions: Mate and Flush. Figure 8.3 compares the two solutions. On the far left the selections are shown, in the middle the Mate solution is shown, and on the right the Flush solution is shown.

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Figure 8.3 Mate and Flush solutions

To explore the Mate constraint options, you will open a simple fixture assembly and assemble two plates to match the completed assembly next to it:

1.  Click the Get Started tab and choose Open.

2.  Browse for the file mi_8a_002.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  Select the View tab and click the Degrees Of Freedom button to turn on the DOF triad for each underconstrained part.

4.  From the Assemble tab, click the Constrain button (or press C on the keyboard).

5.  In the Place Constraint dialog box, ensure that the Assembly tab is active and the Mate button is selected for the type. Make sure the Preview check box is selected and the Predict Offset And Orientation check box is cleared.

Within the Place Constraint dialog box, you have three check boxes:

Pick Part First This check box, indicated by the small red cube, is useful when parts are partially obscured or are positioned in such a way that clicking a face or edge is difficult. This option requires you to first select the component and then filters the selectable geometry to that single component.

Predict Offset And Orientation This button measures the distance between the selected faces, allowing you to eyeball a part placement and then retrieve the distance. If the check box is not selected, a default of 0 is entered for the offset.

Show Preview This check box, denoted by the eyeglasses icon, controls whether the selected components will adjust position or orientation so you can review the constraint before clicking the Apply button or the OK button to actually create it.

6.  For Selection 1, click the orange face on the part with the triangular feature. Watch the on-screen highlights to be sure you select the face and not an edge. It may be helpful to zoom in.

7.  For Selection 2, click the circular face on the base part.

You should see the part “snap” into place based on your selection points. This is just a preview of the constraint and is controlled by the Preview check box. Notice that the first and second geometry-selection buttons are color-coded in the Place Constraint dialog box. Also notice that as you select faces, they are shaded to match the first and second geometry selections.

8.  To adjust the constraint selection, click the Selection 2 button in the Place Constraint dialog box. This removes the previous selection (the circular face) and allows you to reselect the mating face.

9.  For the reselection, click the orange face on the base plate.

10.Click Apply to place the Mate constraint on the two parts.

11.Select the yellow face of the base plate and the yellow face of the side plate for Selection 1 and Selection 2 (again, ensure that you are selecting faces and not edges).

12.You should see the two yellow faces mate together in a way that is not what you want. Click the Flush button in the Solutions area of the dialog box, and you should see the preview update to give a more desirable result.

13.Click the OK button to place the Flush constraint and close the dialog box.

At this point, the DOF triad should have only one remaining arrow, indicating that all of the other DOF triads have been removed as the constraints were added.

14.Click and drag the part with the triangular feature and note that it will slide in the direction indicated by the DOF symbol, and only in that direction.

You can click and drag the part and see that it slides back and forth in the unconstrained direction indicated by the arrow. Leave this file open and continue to the next section, which discusses the Free Rotate and Free Move tools.

Using Free Rotate and Free Move

Next, you will place the final constraint required to fully assemble the two parts. But before placing the remaining constraint, it may be helpful to rotate the part so that you can easily select the required faces. To do so, you will use the Free Rotate tool. The Free Rotate tool allows you to rotate a selected component and rotate just it in the assembly. The Free Rotate tool suspends any assembly relationships currently involving the selected component to allow it to be rotated. The assembly relationships are reactivated when the Update button is clicked or when some other action, such as placing another constraint, forces an update. The Free Move tool works the same as the Free Rotate tool regarding assembly relationships. Continue from the previous step to see how this works:

1.  From the Assemble tab, click the Free Rotate button.

2.  Select the part with the triangular feature, and you will see the rotate “globe” appear.

·     For free rotation, click inside the rotate globe and drag in short strokes.

·     To rotate about the horizontal axis, click the top or bottom handle of the rotate globe and drag vertically.

·     To rotate about the vertical axis, click the left or right handle of the 3D rotate symbol and drag horizontally.

·     To rotate flat to the screen, place your cursor over the edge of the globe until the symbol changes to a circle and then click and drag around the globe.

3.  Spin the part so you can see the purple face.

4.  Right-click and choose Done to exit the Free Rotate tool.

5.  From the Assemble tab, click the Constrain button.

6.  Select the purple face on each part and then click the OK button.

This will fully constrain the part and remove the final DOF arrow from the display. You can continue to experiment with Assembly constraints on your own by copying and pasting multiple instances of the parts and then constraining them together, or you can close this file without saving changes and continue to the next section to explore more constraint options.

Editing and Deleting Constraints

Each of the constraints you placed in the previous steps was added to the browser under the parts involved. You can access these constraints to make changes or delete them by expanding the browser node for one of the components. In the following steps, you will edit and delete a constraint:

1.  Click the Get Started tab and choose Open.

2.  Browse for the file mi_8a_003.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  Expand the plus icon next to both of the parts in the browser to reveal the constraints listed below them. There are two Mates and one Flush constraining these two parts.

4.  Right-click the Flush constraint and select Edit.

You'll notice that the options are much like those used to create the constraint. You can reselect selection inputs 1 and 2, modify the solution from Flush to Mate, or even change the type. In this case you will add an offset value.

5.  Enter –10 mm in the Offset input box. If the preview button is selected, you should see the part adjust to preview the flush offset.

6.  Click the OK button to accept the edit.

7.  Click the Flush constraint in the browser again. Notice that it now displays the offset value.

8.  At the bottom of the browser is an input box where you can adjust the offset without needing to bring up the edit dialog box. Type 12 mm and press the Enter key on the keyboard. The part will adjust to the new offset.

9.  Double-click the icon next to the Flush constraint in the browser.

10.An Edit Dimension box appears, offering another way to edit the offset parameter for this Flush constraint.

The Show and Hide Relationships Tools

In addition to locating constraints in the browser, you can use the Show Relationships tool to select a component and locate all of the assembly relationships that involve it. Once the relationship glyphs are shown, you can right-click any of them and choose from a number of options, such as Edit, Delete, Suppress, and so on. You can then use the Hide Relationships tool to turn off the display of the relationship glyphs in the graphics area.

If any assembly relationships contain errors, you can use the Show Sick Relationships tool to find them quickly.

11.It is often helpful to name constraint offset parameters for use later. Type Block_Offset = 40 mm into the box and then click the green check mark button (or press the Enter key).

12.On the Manage tab, click the Parameters button.

13.In the resulting dialog box, you'll see the Block_Offset parameter in the list. Note that the other two parameters are for the Mate constraints. Click the Done button to exit the Parameters dialog box.

14.Select the View tab and click the Degrees Of Freedom button to turn on the DOF triad for each underconstrained part. In this case, no triads appear, because the assembly is currently fully constrained.

15.Right-click the Flush constraint in the browser and choose Delete. You'll now see a DOF arrow showing you that the part is free to slide along one axis.

16.Click and drag the part to see it move in its free axis.

17.From the Assemble tab, click the Constrain button.

18.In the Place Constraint dialog box, click the Predict Offset And Orientation check box (find it next to the Preview check box).

19.Set the solution to Flush and then select the yellow faces of the two parts.

20.Note the offset value reports the current distance between the two yellow faces. Enter Block_Offset = 20 mm and then click the OK button.

Mate and Flush constraints will likely make up a majority of the constraint types you edit and create. Take the time to master these constraints, and you will find the other constraint types much easier to learn. You can close this file without saving changes. If you'd like more practice with Mate and Flush constraints, you can open the files mi_8a_104.iam, mi_8a_105.iam, mi_8a_106.iam, and mi_8a_107.iam (located in the Chapter 8 directory of your Mastering Inventor 2015 folder) and assemble them using the concepts you just learned. Use the assembled parts as an example to put together the unassembled parts in each of these files.

Mate to Edges, Centerlines, and Vertices

In addition to selecting faces for creating Mate constraints, you can use edges, centerlines, and vertices as selections. When using edges or centerlines, keep in mind that you are defining a different number of degrees of freedom than when using faces; therefore, the results can be quite different. It is also important to understand that edges and centerlines have no negative or positive value, and therefore edge-to-edge type constraints are not a good choice for creating mate offsets. Instead, use a face-to-edge mate in those cases.

Depending on the available geometry, you will often need to use the Select Other drop-down menu tool to cycle through the available selections to select an edge or vertex. To use the Select Other tool, hover over a selection and wait for the Select Other drop-down menu to appear. Then select the available geometry from the list. Figure 8.4 shows the Select Other tool being used to select a center point on the left, an axis in the center, and a cylindrical face on the right.

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Figure 8.4 Using the Select Other tool

The Angle Constraint

The Angle constraint permits three solutions within this constraint type. The solutions are Directed Angle, Undirected Angle, and Explicit Reference Vector. The Directed Angle solution always applies the right-hand rule, meaning the angle rotation will function in a counterclockwise direction.

The Undirected Angle allows either counterclockwise or clockwise direction, resolving situations where a component orientation will flip during a constraint drive or drag operation.

The Explicit Reference Vector solution allows for the definition of a z-axis vector by adding a third click to the selection. This option will reduce the tendency of an Angle constraint to flip to an alternate solution during a constraint drive or drag. Figure 8.5 illustrates the selections required for this solution.

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Figure 8.5 Explicit reference vector

Follow these steps to explore the Angle constraint:

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_007.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

4.  In the Type area of the Place Constraint dialog box, select the Angle button.

5.  In the Solution area, click the Directed Angle button.

6.  For Selection 1, click the large face of the painted board that the hinges are mounted on.

7.  For Selection 2, click the large face of the unpainted board that the hinges are mounted on.

8.  Enter 90 into the Angle input box, and note that the preview displays as expected.

9.  Click the Selection 1 and Selection 2 buttons to clear them and then select the unpainted board for Selection 1 and the painted board for Selection 2. Pay attention to which selection button is pushed in as you select to ensure that you get this right.

Place Assembly Constraints Using Alt+Drag

Rather than using the Place Constraint dialog box, you can press and hold the Alt key and then drag a component into position. Constraints are inferred based on the type of geometry selected. The constraint is previewed in the graphics area as you drag over the components involved. To set a specific constraint, release the Alt key and enter one of the following shortcut keys. You can press the spacebar to flip the constraint solution, from Mate to Flush, for example.

·     M or 1 changes to a Mate constraint.

·     A or 2 changes to an Angle constraint.

·     T or 3 changes to a Tangent constraint.

·     I or 4 changes to an Insert constraint.

·     R or 5 changes to a Rotation motion constraint.

·     S or 6 changes to a Translation motion (slide) constraint.

·     X or 8 changes to a Transitional constraint.

To see the Alt+drag method in action, select the Get Started tab and click the Show Me Animations button. Click the Assemblies – Constraints link in the list and then choose Alt-Drag Shortcut Animation from the next list.

You will see from the result that the 90-degree angle is dependent on the selection order. In this case, you could enter –90 to flip the angles also, but had you selected edges rather than faces, entering –90 would not work. Next, you will explore the Undirected Angle solution.

10.To clear your selections and input before continuing, click the Cancel button to exit the Place Constraint dialog and then click the Constrain button to bring it back up.

11.In the Type area of the Place Constraint dialog box, click the Angle button; then in the Solution area, click the Undirected Angle button.

12.Select the two faces and enter 90 (for 90 degrees) again. You'll note the preview updates as expected.

13.Click the Selection 1 and Selection 2 buttons to clear them and then select the unpainted board for Selection 1 and the painted board for Selection 2. Pay attention to which selection button is pushed in as you select to ensure that you get this right.

You will notice that the angle is not dependent on the selection order. And if you try entering –90 for the angle input, you'll see that the negative value does not change the angle. This option can be more stable for use in setting up angles that will be changed in configurations, animations, and so on, but it is still largely dependent on the other constraints in the assembly. If the constraints holding the hinge to the boards were modified, the Undirected Angle constraint may need to be adjusted. Next, you will explore the Explicit Reference Vector solution to see that it allows you to more fully define the angle.

14.Click the Cancel button to exit the Place Constraint dialog and then click the Constrain button to bring it back up.

15.In the Type area of the Place Constraint dialog box, click the Angle button; then in the Solution area, ensure that the Explicit Reference Vector button is selected.

16.For Selection 1, click the large face of the painted board that the hinges are mounted on.

17.For Selection 2, click the large face of the unpainted board that the hinges are mounted on.

18.Run your cursor over the cylindrical faces in the center of either hinge. You should see the direction arrow flip back and forth depending on which face is highlighted.

19.When you find a face that points the arrow out away from the center of the assembly, click it. This selects the center axis of the hinge pivot and therefore defines the entire Angle constraint without relying on other existing constraints to establish the vector reference.

20.Enter 90 degrees.

You'll note that the preview updates incorrectly, flipping the assembly down and causing an interference situation. To correct this, you can enter a negative angle, or you can simply reselect Selection 3 so that it points the other way.

21.Click the Selection 3 button again to clear it and then find a face that makes the arrow point in toward the center of the assembly and select it. You'll notice that the preview updates to flip the assembly up, as desired.

You may be wondering why there are so many angle options. Originally Inventor did not include all three of these angle solutions, and options were added to improve the predictability of Angle constraint updates. At this point, though, if you use the default Explicit Reference Vector solution, your Angle constraints will update predictably.

As a final note on Angle constraints, you will probably find that using edges rather than faces for Angle constraints will provide more predictable results, particularly when setting up constraints to be used in creating positional variations for animation or documentation purposes. You can close this file without saving changes and continue to the next section.

Using the Right-Hand Rule

A good way to visualize the Explicit Reference Vector command is to use the right-hand rule. Take your right hand and make a “gun” shape with your index finger pointing out and your thumb pointing up. Now point your middle finger to the left, 90 degrees to the index finger. Your hand will then be making the three major axes. You can then use your thumb to determine the positive axes of the cross product of the x- and y-axes (the index and middle fingers).

The Tangent Constraint

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A Tangent constraint results in faces, planes, cylinders, spheres, and cones coming in contact at a point of tangency. Tangency can exist inside or outside a curve, depending on the direction of the selected surface normal. The number of degrees of freedom a Tangent constraint removes depends on the geometry. When a Tangent constraint is applied between a cylinder and a planar face, the constraint will remove one degree of linear freedom as well as one degree of rotational freedom from the set.

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_008.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

4.  In the Type area of the Place Constraint dialog box, click the Tangent button.

5.  For Selection 1, click the face of one of the sphere-shaped ball bearings.

6.  For Selection 2, click the face of one of the half-sphere cutouts in the block.

7.  Note that the preview sets the bearing to the outside. To fix this, click the Inside button in the Solution area of the Place Constraint dialog box.

8.  Click the Apply button and then create an identical Tangent constraint for the second ball bearing.

9.  Create another Tangent constraint, but this time use the Outside solution and select the cylinder of the shaft and the spherical face of one of the ball bearings. Click the OK button to create the constraint and exit the Place Constraint dialog box.

10.Before creating the last Tangent constraint, click the shaft and pull it up toward the top of the ball bearing it is tangential with. This is just so that the next Tangent constraint will not solve to the lower hemisphere and run the shaft into the block.

11.Create another Tangent constraint, again using the Outside solution, and select the cylinder of the shaft and the spherical face of one of the ball bearings.

Tangent constraints are fairly straightforward, and although they are not the most common constraint type to use, they are often the only one that will allow you to get the result you need when working with cylinders, spheres, and curved faces. You can test the function of the shaft and bearing constraint set by clicking and dragging the shaft to see it rotate, and then you can close the file without saving changes. Figure 8.6 shows the placement of a Tangent constraint.

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Figure 8.6 Tangent constraints

The Insert Constraint

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The Insert constraint is probably the best choice for inserting fasteners and other cylindrical objects into holes or for constraining any parts where circular or cylindrical geometries are to be constrained to one another. A single Insert constraint will replace two Mate constraints (one along the edge and one through the centerline), retaining one rotational degree of freedom. Options for the Insert constraint are Opposed and Aligned. The Insert constraint also allows for specifying offset values between components. Figure 8.7shows common uses of Insert constraints.

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Figure 8.7 Insert constraints

Follow these steps to explore the Insert constraint:

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_009.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

4.  In the Type area of the Place Constraint dialog box, select the Insert button.

5.  Select the bottom edge of one of the screw heads for Selection 1. Notice that the highlight shows that the edge and the centerline are selected.

6.  Select the top edge of one of the eight holes on the plate for Selection 2.

7.  Toggle the solution button to see the difference in the two solutions and then set the solution to Opposed.

8.  Enter 2 mm in the Offset input box and then click the Apply button.

9.  Select the edge of one of the washers and then the bottom edge of the screw head you just inserted to place and apply another Insert constraint.

10.Set another Insert constraint using the edge of the yellow face of one of the boss features on the end flange and one of the nuts. Use the Aligned solution to flip the nut so it is set down inside the boss feature.

11.Use Insert constraints to place the blue cover on the base part by selecting the rounded corners.

You can continue to practice with the remaining hardware. Use Copy and Paste to add more instances if you'd like. When you've finished, you can close the file without saving changes. For further practice with Insert constraints, take a look at mi_8a_109.iam andmi_8a_110.iam. You can investigate the constraints used in the assembled versions of these models to help if needed.

Minimum Distance Using the Measure Tool

You can find the minimum distance between two assembly components by using the Measure tool. To access the Measure tool, select the Inspect tab and select Measure Distance from the Measure panel. Click the Priority drop-down box in the Measure Distance tool and set it to Part Priority. Next, select the first part and then select the second part. The returned value is the minimum distance between the two parts.

The Symmetry Constraint

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The Symmetry constraint, shown in Figure 8.8, positions two components symmetrically to each side of a plane or planar face. When one of the components is moved or its orientation is changed, the other component maintains its symmetrical relationship based on the existing degrees of freedom of each component.

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Figure 8.8 Symmetry constraint

Follow these steps to explore the Symmetry constraint:

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_130.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

The goal for this assembly is to create a symmetry relationship in order to maintain the same distance for the number 1 and number 2 bolts as they are threaded into the yellow receiver part. Currently the assembly has a number of constraints in place to help define the mechanism; however, there is still something missing. If you click and drag on the number 1 screw, you'll see that the behavior is not quite correct. If you click and drag on the yellow receiver part, you'll see something closer to the correct behavior, but the bolts do not maintain a symmetrical distance. You'll add the missing constraint to resolve this.

3.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

4.  In the Type area of the Place Constraint dialog box, select the Symmetry button.

5.  Select the blue face of one of the bolt heads for the first selection.

6.  Select the blue face of the other bolt head for the second selection.

7.  For the third selection, choose the visible work plane in the center of the yellow receiver part.

8.  Click the OK button to create the constraint.

9.  Now you can click and drag bolt number one to see that the two bolts maintain a symmetrical relationship on each side of the selected work plane.

Symmetry constraints are a quick and easy way to set up your assembly to hold components equidistant to a planar face or work plane or maintain a symmetric orientation. In this particular assembly there are two motion constraints in place that allow the assembly to perform the threading action. In the next sections you'll explore these constraints. You can close this file without saving changes in order to continue.

Within the Place Constraint dialog box are the Motion tab and the Translational tab. From the Motion tab, you can add Rotation constraints and Rotation-Translation constraints. A Rotation constraint is typically placed between two components, such as gears, simulating a ratio-based rotation. Rotation-Translation constraints allow a linear distance and revolution ratio to be applied for component pairs such as rack and pinion sets. From the Translational tab, you create constraints between a rotating and nonlinear translating face, such as cams and followers.

The Rotation Constraint

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To create a simple Rotation constraint, first place two components constrained around their axes. Neither component should be grounded; instead, they should be constrained to allow rotation around the axes. The Rotation constraint applies a Forward or Reverse solution to the two components, along with a ratio that will determine rotation speeds, as shown in Figure 8.9.

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Figure 8.9 Rotation constraint options

In the following steps you will create a reverse Rotation constraint on a small cog set:

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_010.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

4.  Click the Motion tab in the Place Constraint dialog box.

5.  In the Type area of the Place Constraint dialog box, select the Rotation button.

6.  For Selection 1 click the yellow face on the large cog, and for Selection 2 click the yellow face on the small cog.

7.  In the Solution area, click the Reverse button.

8.  Note that the ratio is automatically set to 3 ul (ul means unitless). You could enter any value you want, but in this case you'll leave it at 3 based on the selected geometry. You should be aware had you selected the cogs in the opposite order, the ratio would be 0.333, the reciprocal of its current value. Click the OK button to create the Rotation constraint.

Currently, the assembly is fully constrained and will not rotate. This is because of the Mate constraint named Alignment Mate, which has been placed on the XZ origin planes of each cog. The purpose of this Mate constraint is simply to line up the cogs in their start position. To let the Rotation constraint work, the mate must be suppressed or deleted.

9.  Locate the Alignment Mate constraint in the browser. You can do so by expanding either of the cogs in the browser.

10.Right-click the Alignment Mate constraint and choose Suppress. The constraint will now be grayed out and will not calculate against the assembly.

11.Click and drag either of the cogs to rotate them.

If you start the rotation with both yellow faces showing and count the number of times the small cog rotates before the yellow face on the large cog comes back around, you will see it make three revolutions for every one of the large cogs, as specified by the ratio in the constraint input. You can close the file without saving changes and continue to the next set of steps, where you will create a Rotation-Translation constraint.

The Rotation-Translation Constraint

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In the following steps you will create a Rotation-Translation constraint as would be used to constrain a rack and pinion gear set:

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_011.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

4.  Click the Motion tab in the Place Constraint dialog box.

5.  In the Type area of the Place Constraint dialog box, select the Rotation-Translation button.

6.  Hover over any of the component geometry and notice that the selection glyph displays a rotation arrow, indicating it is looking for the rotational selection. Selection order is important in this case. For Selection 1, click the yellow face on the cog.

7.  For Selection 2, in the Solution area click along the bottom edge of the rack. Be certain to select the edge, not the face. Although there is nothing preventing you from selecting the face or anything indicating that it is not the correct selection, the constraint will simply not work if the face is selected.

8.  Note the value added to the Distance input box. This is the total travel of the rack for one revolution of the cog. This value is initially calculated from the selections, but you can enter your own value as required. In this case, the number is not a whole number because of the mix of Imperial and metric dimensions used in this model. Click the OK button to create the constraint.

Figure 8.10 shows the constraint selections.

Currently, the assembly is fully constrained and will not rotate. This is because of the Mate constraint named Start Point Mate, which has been placed on the rack and cog. To let the Rotation-Translation constraint work, the mate must be suppressed or deleted.

9.  Locate the Start Point Mate constraint in the browser. You can do so by expanding the rack in the browser.

10.Right-click the Start Point Mate and choose Suppress. The constraint will now be grayed out and will not calculate against the assembly.

11.Click and drag the rack to see the rotation and translation take place.

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Figure 8.10 Rotation-Translation constraint options

Although motion constraints are easy to place, be aware that often the real work is in the calculations to create components with the correct geometry beforehand. If you have a need to create a lot of gears, you'll want to explore the gear generator found in the design accelerator tools. For now, you can close the file without saving changes and continue to the next section.

Transitional Constraints

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Transitional constraints allow the movement of an underconstrained component along a path in a separate part. To create a Transitional constraint, you first select a moving face on the underconstrained component. Then you select a transitional face or edge on a fully constrained or grounded part. Figure 8.11 illustrates a cam and follower with a Transitional constraint applied.

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Figure 8.11 A Transitional constraint

Follow these steps to explore the Transitional constraint:

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_012.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

4.  Click the Transitional tab in the Place Constraint dialog box.

5.  For Selection 1, click the yellow face on the follower wheel. Note that the first selection must be the moving face.

6.  For Selection 2, click the orange face on the cam. Note that this selection must be the translational face.

7.  Click the OK button to create the constraint.

8.  Click and drag the cam and rotate it around the axis to see the assembly in action.

Components used in Transitional constraints must always be in contact for them to work; therefore, no offsets are permitted. The translational face (in this case the cam) can be any combination of flat, arced, or spline-defined faces, but it is generally best to avoid sharp corners. When finished examining the Translational constraint functionality, you can close the file without saving changes.

Additional Constrain Tools and Options

In addition to the basic constraint types and options, there are a number of other tools and options to be aware of. These tools and options are covered in the following pages.

Using the Assemble Tool to Place Constraints

The Assemble tool allows you to move a component into place and place a constraint based on the selected geometry. This tool is designed to select a component and then fully constrain it. When using the Assemble tool, you select the component you want to move into place first, and then you select the component you want to constrain to. Because of this, you can constrain only one component at a time with this tool. To constrain a second component, you must click the OK button to exit the Assemble tool and then select the Assemble button again, or right-click and select Repeat Assemble.

As constraints are placed, the geometry involved is left highlighted on-screen. These new constraints are not created until you exit the Assemble tool by clicking the OK button. If any conflicts with existing constraints are created, you are presented with the Assemble Constraint Management dialog box. You can find options in this dialog box to resolve the conflicts.

You can open the file mi_8a_013.iam to explore the Assemble tool, following these general steps:

1.  From the Assemble tab, click the Assemble button, using the Relationships panel drop-down.

2.  Select some geometry on the component to be moved into place.

3.  Select some geometry on the component that is intended to stay in place.

4.  Enter values such as offsets or angle values if needed.

5.  If necessary, change the solution type (from Mate to Flush, for example).

6.  From this point you can do any of the following:

·     Click the Apply button and continue to define other constraints for the selected component.

·     Click the OK button to create the constraints based on the previous selections and exit the Assemble tool.

·     Click the Undo button to delete the current selections and then continue defining constraints.

Relationship Audio Notification

When you place a relationship in an assembly, Inventor makes a sound at the time of the preview or at the time of the constraint creation, depending on the preview option at the time. You can disable this sound by selecting the Tools tab, clicking Application Options, and then selecting the Assembly tab. Uncheck the Relationship Audio Notification check box to disable the sound.

You can change the sound by replacing the default sound file with one of your choice. The sound file is Connect.wav and can be found in the C:\Program Files\Autodesk\Inventor 2015\Bin folder (assuming that is the install path).

Constraint Sets

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Constraint sets allow you to constrain two components together using their user coordinate systems (UCSs). You define the UCS in the part or subassembly file first and then place constraints on the coordinate system planes and axes rather than the component geometry.

You can open the file mi_8a_014.iam to explore constraint sets, following these general steps:

1.  From the Assemble tab, click the Constrain button.

2.  In the Place Constraint dialog box, click the Constraint Set tab.

3.  Expand the browser nodes for both components so you can see the UCS features listed.

4.  Select UCS1 in each part for Selections 1 and 2.

5.  Click the OK button to create a set of constraints between the two UCS triads.

Constraint sets can often be helpful when components are modeled referencing a common datum set in each component. When finished creating the constraints, you can close the file without saving changes.

Constraint Limits

Constraint limits allow you to define minimum and maximum constraint values so components can move freely within the limits but not beyond them. You can imagine a model of a door hinge. You might want the hinge to swing from 0 to 270 degrees, but not outside of that range or the hinge might interfere with itself.

You can open the file mi_8a_015.iam to explore constraint limits. In this assembly there are four parts. These would be four subassemblies in reality, but for the sake of simplicity, they have been condensed into part files. The router base is grounded in place, and the y- and z-axis assemblies have been fully constrained with constraint limits, so they are free to slide within the bounds of the bearing rods and gantry uprights. You can click and drag the z-axis assembly to see how it behaves in a realistic manner thanks to the existing constraint limits. But if you click the x-axis assembly, you will see that it does travel along the bearing rods realistically, but it can continue sliding through the router base and beyond. To fix this, you will add a constraint set to the x-axis assembly, limiting its travel to a more realistic result:

1.  From the Assemble tab, click the Constrain button (or type C on the keyboard).

2.  Leave the constraint Type set to Mate and set the solution to Flush.

3.  Select the two yellow faces for Selection 1 and Selection 2, making sure to select the large yellow face on the router base for Selection 1 and the smaller yellow face on the x-axis assembly for Selection 2.

4.  Click the button to expand the dialog box.

5.  Click the Maximum and Minimum check boxes.

6.  Enter -10 mm for the maximum value.

7.  Enter -395 mm for the minimum value.

8.  Click the Use Offset As Resting Position check box.

9.  Enter -150 for the offset value (located back toward the top of the dialog box).

10.Enter X Travel in the Name input box and then click the OK button to create the constraint.

11.Click the x-axis assembly, and you will see that it now stops before running through the other components.

Figure 8.12 shows the constraint limit being created.

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Figure 8.12 Placing constraint limits

You can drag the x-axis assembly to its minimum and maximum limits, but when you let go, it returns to the resting value you set in the dialog box. Keep in mind you are not required to use the resting position option. If no resting value is used, the assembly will stay where it was last placed, which is the behavior exhibited by the z-axis assembly.

Constraint limits are a great tool to use in the setup of free-moving components to get them to behave predictably. However, you should be aware that there may be a small performance hit when using too many of these at once. So, keep that in mind as you use them. You can close the assembly without saving changes.

Driving Relationships

It is often desirable to simulate motion by driving a relationship through a beginning position and an ending position to confirm the intent of the design. In general, Offset and Angle constraints may be selected to drive components within an assembly. To accomplish this, simply right-click the desired constraint and select Drive (as shown in Figure 8.13).

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Figure 8.13 Driving a constraint

You can open the file mi_8a_016.iam to explore the drive constraint options. If you expand the Z-Axis Assembly node, you will find two constraints labeled Drive Me. When you right-click a constraint and choose Drive, the Drive (Angle Constraint) dialog box appears, allowing you to alter the constraint by specifying steps between the start position and the end position. When a constraint is driven, any components constrained to the driven component will move in accordance to their particular shared constraints. The motion may be set to forward or reverse, stopped at any time, and even recorded (click the Record button prior to activating the move). If any of the affected components are constrained to a grounded component or if the movement will violate any existing constraint, then the drive constraint will fail.

Expanding the dialog box as shown in Figure 8.14 by clicking the button will reveal additional controls over the drive constraint.

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Figure 8.14 Drive constraint dialog box options

The increment of movement can be controlled by a value or by a total number of steps from beginning to end. The length of a particular driven constraint can be controlled by the number of allowable repetitions from Start to End or can be reversed by using the Start/End/Start option. The constraints in mi_8a_016.iam are set up in this manner.

For a continuous revolution by degrees, you may exceed 360 degrees by specifying the total number of degrees of revolution or by including an equation such as 360 deg * 3. Another approach is to set the End rotation to 360 degrees and then simply increment the Repetitions value for the number of revolutions. You can open the file mi_8a_108.iam to further explore constraint limits.

Other adaptive parts properly constrained within the driven assembly will adjust to changes if the Drive Adaptivity option is selected. This particular option allows determination of a maximum or minimum condition for the adaptive part.

Checking the Collision Detection option allows for determination of an exact collision distance or angle between the driven parts. Using the Collision Detection option will help you determine interferences between moving parts so that those parts can be modified before manufacturing. In mi_8a_108.iam there is a small red link that can be swiveled out of the way to avoid a collision of parts. If you leave it sticking out and drive the Drive Me constraint and enable the Collision Detection option, you can determine where the parts come into contact with one another. Inventor reports the angle of collision in the Drive Constraint dialog box. You can change the Increment value to a fraction of a degree to see a more exact value.

Contact Solver

Another method for driving components within an assembly involves the Contact Solver option. With this option, only minimal constraints are required to drive a number of components. Components are not required to be constrained to one another for the Contact Solver to work.

The Contact Solver works in much the same way as parts interact in the real world. Without the Contact Solver applied, moving parts can be run through one another, creating interference. With the Contact Solver applied, parts will stop when they contact one another. A simple example of this is the slide arm pictured in Figure 8.15. On the left, you can see that the arm segments have been extended past the point that they could be in reality, allowing the slide stops to run through the slide slot. On the right, the parts have been added to a contact set and the Contact Solver has been turned on, preventing the slide stops from running through the slots.

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Figure 8.15 With and without Contact Solver

To add parts to a contact set, right-click the part and choose Contact Set from the context menu. An icon appears before each component showing when it has been added to the contact set. In addition to adding parts to a contact set, you must ensure that the Contact Solver is turned on; do this by choosing Activate Contact Solver from the Inspect menu. Once all active participants within the contact set are selected and the Contact Solver is activated, then a single driven constraint can provide a real-life simulation. Note that it is best practice to turn the Contact Solver off when performance is a consideration.

To explore the contact sets, open the file mi_8a_017.iam and follow these basic steps:

1.  Select any components you want to be added to the contact analysis.

2.  Right-click the selected components and choose Contact Set from the context menu.

3.  Select the Inspect tab and click the Activate Contact Solver button.

4.  Drag the part with the black end cap in and out to see the assembly extend and contract based on the contact points.

Using the Contact Solver for Collision Detection

If you have parts that interfere (such as a dowel pin in a hole) and have the Collision Detection option selected, the Drive Constraint command will stop immediately because it will have detected this interference. If you need to test the collision of parts, look into using the Contact Solver.

Redundant Relationship and Constraint Failures

Excessive relationships are considered redundant when you have overconstrained components. Redundant relationships will interfere with the proper operation of your assemblies and can cause relationship errors and performance issues.

Two toggles will assist in flagging bad constraints; you can find them by selecting Tools  Application Options and selecting the Assembly tab. Enabling Relationship Redundancy Analysis allows Inventor to perform a secondary analysis of Assembly constraints and notifies you when redundant constraints exist.

Enabling Related Relationship Failure Analysis allows Inventor to perform an analysis to identify all affected constraints and components if a particular constraint fails. Once analysis is performed, you will be able to isolate the components that use the broken constraint (or constraints) and select a form of treatment for individual components.

Because analysis requires a separate process, performance can be affected if these two check boxes are active. Because of this, it is advisable to activate the analysis only when problems exist.

Working with Joint Relationships

The Joint tool allows you to define the working relationship between a pair of components with a single joint relationship. This is done by pairing joint points found on faces and edges of components. Several types of joints are available for use in an assembly, so in order to know which joint type to use and when, you should be familiar with each. Although you can achieve the same result using the Constraint tool that you can with the Joint tool, the Joint tool results in fewer assembly relationships, which can make managing them later much easier. You can also use the Joint and Constraint tools together to fully define the assembly relationship of your design as you see fit.

Joint Selection Inputs

All of the joint types are created by defining two origin selections and two alignment selections. Keep in mind that the alignment selections are created automatically based on your origin set selections. However, the inferred selections are often not the correct solution for particular joint, resulting in a preview that is incorrect. In these cases, you can simply click the Alignment selection buttons again to reselect edges or faces for alignment.

Constraints or Joints: Which Should You Use?

Because the Constraint and Joint tools provide two methods of doing the same thing, creating assembly relationships, you might wonder which you should use. The answer will likely depend on your experience and familiarity with both tools. If you are comfortable with the Constraint tool, you might find that it fits your approach to creating assembly relationships best, in which case you might find that you seldom end up using the Joint tool. Conversely, if the Constraint tool seems less intuitive to you, you might find that you prefer the Joint tool.

The preference for one or the other of these tools might depend on the type of designs you create. For instance, if you create frame structures or weldments with mostly static components, you might find that you lean toward creating Rigid joints, rather than Mate and Flush constraints. Of course, you might also use a mix of constraints and joints, choosing the relationship type that works best for you.

Rigid Joints

The Rigid joint type creates a joint between points on a pair of faces, a pair of edges, or an edge and a face. Rigid joints remove all degrees of freedom creating a “fixed” joint. You can use the Flip Component and Invert Alignment buttons to adjust the orientation of the component if the preview shows the component incorrectly. Figure 8.16 shows connection points being selected for a Rigid joint.

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Figure 8.16 Connection points

To explore the Rigid joint options, you will open a simple fixture assembly and assemble two components using a Rigid joint.

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_120.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Joint button.

4.  Use the Type menu to select Rigid from the list.

5.  For the first origin selection, hover over the yellow face of the component named Side_302.

6.  Move your cursor down to select the center-bottom connection point, as shown in Figure 8.16.

7.  For the second origin selection, hover over the yellow face of the base component and choose the center-top connection point, as shown in Figure 8.16.

8.  Use the Flip Component and Invert Alignment buttons to correct the alignment of the Side_302 component.

9.  Enter -5 mm in the Gap input box in order to set the far faces flush.

10.Click the OK button to create the Rigid joint. Figure 8.17 shows the result.

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Figure 8.17 The Rigid joint results

Next, you'll edit the Rigid joint you just created and adjust the selections. You can continue with the file you have open or close it and open the file mi_8a_121.iam.

1.  Locate and expand the Relationships folder in the Model browser and then right-click the Rigid joint and choose Edit.

2.  Click the second origin button in the Connect area of the dialog box in order to clear the selection.

3.  Click the first origin button in the Connect area of the dialog box in order to clear that selection as well.

4.  Next, with the first origin button active still, select the center connect point of the bottom edge of the Side_302 component, as shown in Figure 8.18.

5.  For the second origin selection, select the center connect point of the top edge of the base component, as shown in Figure 8.19.

6.  Note that the -5 mm gap distance results in a different offset when the two edges are selected compared to when the two faces were selected.

7.  Set the Gap value to 0 mm.

8.  Enter Yellow Faces in the Name input box; then click the OK button to apply the changes.

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Figure 8.18 Selecting an edge connection point

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Figure 8.19 Selecting the other edge connection point

You'll note that the name in the browser is now changed to read Yellow Faces. Naming joints in this manner allows you to organize and quickly locate joints for editing. You can close this file when finished and continue to the next section to explore Rotational joints.

Rotational Joints

The Rotational joint type creates a joint between points on a pair of faces, a pair of edges, or an edge and a face. Rotational joints specify one degree of freedom, creating a rotating joint based on the connection points you select. You can use the Flip Component and Invert Alignment buttons to adjust the orientation of the component if the preview shows the component incorrectly. Additionally, you can create a rotational limit so that the rotational joint will only rotate through a specified set of angles.

To explore the Rotational joint options, you will open a simple assembly and create one Rotational and one Rigid joint in order to define the rotation of a handle crank.

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_122.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

Take a moment to examine the parts listed in the model tree. If you drag your cursor over each part name, you will see that part highlight in the browser. You'll refer to these part names in the following steps.

3.  From the Assemble tab, click the Joint button.

4.  Use the Type menu to select Rotational from the list.

5.  For the first origin selection, hover over the yellow face of the component named 8_105.

6.  Move your cursor down to select the connection point at the center of the hole.

7.  For the second origin selection, choose the connection point at the center of the yellow face of the component named 8_104 (the gray base component).

8.  Click the Limits tab in the Place Joint dialog box.

9.  Click the check box for the Angular Start option and enter 360 deg in the input box.

10.Enter 180 deg in the End input box.

11.Click the OK button to create the rotational joint. Figure 8.20 shows the result.

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Figure 8.20 The Rotational joint results

You can click and drag the 8_105 component to see it rotate through the range of motion specified in the Limits tab. This allows the joint to work realistically so that it stops without running through the other component. Next, you'll add a Rigid joint to complete the assembly. You can continue with the file you have open or close it and open the file mi_8a_123.iam.

1.  From the Assemble tab, click the Joint button.

2.  Use the Type menu to select Rigid from the list.

3.  For the first origin selection, hover over the red face of the component named 8_106 and then click to select the center connection point of the hole.

4.  For the second origin selection, hover over the red face of the component named 8_105 and then click to select the center connection point.

5.  Click the first alignment button and choose the blue face on the inside of the keyway; you might need to zoom in closely to select it.

6.  Then click the blue face on the key feature on the 8_105 component and click the Invert Alignment button to set the proper alignment.

7.  Click the OK button to create the rigid joint and then click and drag the components to see the behavior you've achieved. Figure 8.21 shows the completed assembly.

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Figure 8.21 The completed assembly

Here you've used a rigid joint in combination with a rotational joint to define the rotational limits and assembly alignment of a simple mechanism. Keep in mind that you could have achieved the same results using the Constraint tool instead of the Joint tool, or you could have used the two in combination. You can close this file and continue to the next section to explore the Slider joint type.

Joint Selection Options

You can find three right-click context menu options to help you when creating joints:

·     Infer Origin: This is the default option, where the Origin is inferred based on the selections.

·     Offset Origin: You can drag the manipulator arrows or input an offset value to change the location of the Origin.

·     Between Faces: You can specify a virtual midpoint between two selected faces by selecting the two faces and a point.

To use these options, click the Joint tool and then right-click and choose one of the options from the context menu.

Slider Joints

Much like the Rigid and Rotational joints, the Slider joint type creates a joint between points on a pair of faces, a pair of edges, or an edge and a face. Slider joints specify one translational degree of freedom, defining a sliding action. As with other joint types, you can use the Flip Component and Invert Alignment buttons to adjust the orientation of the component if the preview shows the component incorrectly. Additionally, you can create a linear travel limit so that the joint will only slide through a specified linear distance.

To explore the Slider joint options, you will open a simple assembly and create a couple of Slider joints.

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_124.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

In this file there are three bearing pads. One of the bearing pads has been set up to slide in the first rail channel already. This was done using the Constraint tool. If you expand the Relationships folder in the browser, you'll find two Mate constraints and one flush constraint. The three of these together create the relationship that allows the bearing pad to slide through a specific linear distance in the first rail channel. You'll use the Joint tool to create the same relationship for the remaining two bearing pads with just a single slider joint for each pad.

3.  From the Assemble tab, click the Joint button.

4.  Use the Type menu to select Slider from the list.

5.  For the first origin selection, hover over the yellow face on either of the unconstrained bearing pads.

6.  Move your cursor to select the connection point at the center of the edge near the red face, as shown in Figure 8.22.

7.  For the second origin selection, hover over the yellow face of the center channel on the rail.

8.  Move your cursor to select the connection point at the center of the edge near the red face, as shown in Figure 8.23.

9.  Click the Align buttons to see which faces are being used as the alignment selections. If the red faces on each part are not selected, select them so that both red faces are aligned, as shown in Figure 8.24.

10.Click the Limits tab in the Place Joint dialog box.

11.Select the Linear Start check box and then enter 0 mm in the input box.

12.Select the Linear End check box and then enter -250 mm in the input box. The rail is 300 mm long and the bearing pad is 50 mm long, so the linear limit is 300 – 50, or 250, and you use a negative value to control the direction.

13.Click the OK button to create the slider joint.

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Figure 8.22 Connection point on the bearing pad

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Figure 8.23 Connection point on the channel

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Figure 8.24 The correct alignment of the bearing pad

You can click and drag the bearing pad to see it slide through the range of linear motion specified in the Limits tab. This allows the pad to work as if the rail had end stops in place. And note that you've created this relationship with just a single joint, whereas the existing relationship required three constraints.

Next, you'll add another slider joint to the remaining bearing pad. You can continue with the file you have open or close it and open the file mi_8a_125.iam.

1.  From the Assemble tab, click the Joint button.

2.  Use the Type menu to select Slider from the list.

3.  For the first origin selection, hover over the yellow face on the unconstrained bearing pad.

4.  Move your cursor to select the connection point at the center of the yellow face, as shown in Figure 8.25.

5.  For the second origin selection, hover over the yellow face of the remaining free rail slot and then click to select the center connection point, as shown in Figure 8.26.

6.  Click the Align buttons to see which faces are being used as the alignment selections. If the red faces on each part are not selected, select them so that both red faces are aligned.

7.  Click the Limits tab in the Place Joint dialog box.

8.  Select the Linear Start check box and then enter 125 mm in the input box.

9.  Select the Linear End check box and then enter -125 mm in the input box. The rail is 300 mm long, and the bearing pad is 50 mm long. But since the connection points are in the center of each, you'll use half of these values to come up with the offsets: 150 – 25 = 125. You use the negative of this number to specify the other direction.

10.Click the OK button to create the slider joint.

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Figure 8.25 The center connection point of the bearing pad

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Figure 8.26 The center connection point of the rail slot

You can click and drag the bearing pad to see it slide through the range of linear motion specified in the Limits tab. If the bearing pad does not stop at the ends of the rail slot, edit the Slider joint and check your inputs and alignment selections.

Creating a slider joint is a straightforward process; however, some thought is required to select the correct connection points and specify the correct limit values in order to achieve the correct relationship for each situation. Once you're satisfied with the slider joints you've created, you can close this file without saving changes and continue to the next section.

Cylindrical Joints

The Cylindrical joint type creates a joint between points on a pair of faces, a pair of edges, or an edge and a face. Cylindrical joints specify one rotational degree of freedom and one translational degree of freedom, defining a sliding and rotating action. As with other joint types, you can use the Flip Component and Invert Alignment buttons to adjust the orientation of the component if the preview shows the component incorrectly. For Cylindrical joints you can create both angular and linear limits.

To explore the Cylindrical joint options, you will open a simple slip latch assembly and create a Cylindrical joint.

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_126.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Joint button.

4.  In the Type menu select Cylindrical from the list.

5.  For the first origin selection, select the circular yellow face of the tan-colored part.

6.  For the second origin selection, select the yellow face of the small latch catch part.

7.  Click the Align buttons to see which faces are being used as the alignment selections. If the red faces on each part are not selected, then select them so that both red faces are aligned.

8.  Click the Limits tab in the Place Joint dialog box.

9.  Select the Angular Start check box and then enter -80 deg in the input box.

10.Select the Angular End check box and then enter -20 deg in the input box.

11.Select the Linear Start check box and leave the input box value at 0 mm.

12.Select the Linear End check box and then enter 200 mm in the input box.

13.Click the OK button to create the cylindrical joint. Figure 8.27 shows the result.

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Figure 8.27 A slip latch with a cylindrical joint

You can click and drag the slide bolt to see it slip through the range of angular and linear motion specified in the Limits tab. You'll note that the catch on the slide bolt can pass through the rise in the latch body that defines the slot. To prevent this, you could create a contact set and turn on the Contact Solver as mentioned earlier in this chapter. When you've finished exploring the results of the cylindrical joint, you can close the file without saving changes and continue to the next section.

Planar Joints

The Planar joint type is pretty basic and creates a joint between points on a pair of faces, a pair of edges, or an edge and a face. Planar joints specify two translational degrees of freedom and one rotational. As with other joint types, you can use the Flip Component and Invert Alignment buttons to adjust the orientation of the component if the preview shows the component incorrectly. However, unlike many other joint types, Planar joints have no Limit options.

To explore the Planar joint options, you will open a simple assembly and create a Planar joint between game pieces and a game board.

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_127.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Joint button.

4.  Use the Type menu to select Planar from the list.

5.  For the first origin selection, select the circular yellow face on the bottom of either of the tipped-over game pieces.

6.  For the second origin selection, select the center connection point of any of the squares on the game board.

7.  You can click the Align buttons to see which faces are being used as the alignment selections, although in this case the alignment is not important.

8.  Click the Limits tab in the Place Joint dialog box.

9.  Notice that both the Angular and Linear limits options are grayed out and cannot be selected, indicating that they are not available for planar joints.

10.Click the OK button to create the planar joint.

11.Click and drag on the game piece you placed, and you'll note that it can slide along in any direction but will stay fixed to the top plane of the game board. Figure 8.28 shows the game pieces in place.

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Figure 8.28 Planar joints placing game pieces

Although the planar joint might seem too basic to be of much use, it is often used in combination with one of the other joint or constraint types to further define a mechanism or movement that translates in any direction along a planar surface. When finished, you can close the file without saving changes and continue to the next section.

Ball Joints

The Ball joint type is most often used to create a joint between center points of a pair of spherical faces; however, it can use a connection point found on any pair of faces, pair of edges, or an edge and a face. Ball joints specify three rotational degrees of freedom. As with other joint types, you can use the Flip Component and Invert Alignment buttons to adjust the orientation of the component if the preview shows the component incorrectly. However, there are no Limit options for Ball joints.

To explore the Ball joint options, you will open a simple assembly and create a joint between two parts.

1.  Click the Get Started tab and choose the Open button.

2.  Browse for the file mi_8a_128.iam located in the Chapter 8 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  From the Assemble tab, click the Joint button.

4.  Use the Type menu to select Ball from the list.

5.  For the first origin selection, select the center connection point on the spherical yellow face on the blue arm part.

6.  For the second origin selection, select the center connection point of the yellow face on the gray socket part.

7.  Click the Limits tab in the Place Joint dialog box.

8.  Notice that both the Angular and Linear limits options are grayed out and cannot be selected, indicating that they are not available for planar joints.

9.  Click the OK button to create the planar joint.

10.Click and drag the blue arm part to see that it rotates in the socket. You'll notice that it can currently pass though the other part.

11.Select both parts and then right-click and choose Contact Set.

12.Go to the Inspect tab and click the Activate Contact Solver button to turn the solver on.

13.Now you can click and drag the blue arm part and see that it will not pass through the socket part. Figure 8.29 shows the resulting assembly.

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Figure 8.29 A Ball joint

Although the Ball joint has a fairly specific use, it can often be the only choice for creating certain types of relationships between parts. When you've finished exploring the Ball joint tools, you can close the file without saving changes and continue to the next section.

Understanding Subassemblies

You create assemblies by placing assembly relationships between parts to position and hold those parts together. When working with small assemblies, you can often assemble all the parts together at one level. Working with larger assemblies, however, often requires the use of multiple levels of assemblies for the sake of organization and performance. Lower-level assemblies are referred to as subassemblies.

Imagine a common caster-wheel assembly. Although it may seem like a simple component, it is, of course, made up of many small parts. If you needed to use this caster in an assembly multiple times, you wouldn't place all the small parts into an assembly individually over and over. Instead, you would package them as a subassembly and place multiple instances of the subassembly throughout the top-level assembly. Figure 8.30 shows a caster-wheel assembly ready to be placed as a subassembly.

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Figure 8.30 A caster-wheel assembly

Most things you design and build are typically made from subassemblies of some sort. In manufacturing it makes sense to create subassemblies of common parts to make the assembly process easier. It makes sense to design in the same fashion. In the caster example, it saves you from having to duplicate the work of assembling the caster parts repeatedly for each instance of the caster that exists in the top-level assembly.

A second benefit to using subassemblies is the flexibility they add to the bill of materials. Using the caster as a subassembly rather than as loose parts provides the ability to count the caster as a single item, to count the total of all the caster parts, or to do both.

Knowing When to Use Assemblies

Although it is often necessary to create parts as assemblies (to have a correct bill of materials or to provide the correct motion), it is not always the best choice. For example, in the caster example, unless you need the casters to swivel in your assembly, consider modeling the caster as a single part or deriving the assembly into a single part. This will lower the overhead of your models as well as reduce the number of parts to track throughout your design.

There is a third and important concept to consider when working with subassemblies: model performance. Imagine that you decided to place four instances of the caster into an assembly as loose parts rather than as a subassembly. For the sake of simplicity, say it takes 28 relationships among the caster parts and two relationships between the caster and the top-level assembly, for a total of 30 relationships. You do this for all four casters, for a total of 120 relationships in the top-level assembly. Had you assembled the caster as a subassembly and then placed that subassembly into the top-level assembly, you would have used just 28 in the caster subassembly and two per caster, as shown in Figure 8.31, for a total of only 36 relationships.

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Figure 8.31 Reduced assembly relationships

If you consider assembly relationships to be nothing more than calculations that Inventor must make to hold the assemblies together, then by using subassemblies, you have required Inventor to create and maintain 86 fewer calculations overall. This reduction in constraints can have a significant impact on the assembly's performance and make the task of editing the assembly much easier.

Top-Down Design

Inventor allows you to approach the creation of parts and assemblies in three basic ways. Figure 8.32 shows these three distinctive workflows for assembly design.

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Figure 8.32 Design workflows

The first of these methods is called top-down design. In the purest sense, top-down design is performed completely within the top-level assembly of a machine or device. Parts and subassemblies are created from within the uppermost assembly, as opposed to creating components outside the top-level assembly and then placing these components later. Using this approach, you can reference and project geometry from other parts within the assembly into new parts, thereby ensuring the fit of the new parts. Another benefit to top-down design is that the designer can better visualize how each part relates to others within the assembly. When it's properly utilized, you minimize the number of overall Assembly constraints required and allow for a stable design.

The second method works by creating parts independently and then placing and constraining them into the assembly. This method is called bottom-up design. Bottom-up design is common when creating parts from existing drawings and new pencil sketches. This workflow is ideal for repairing imported geometry, creating standard parts for your library, and converting standard parts into iParts and iFeatures. Working in the single-part environment does not easily allow you to create or reference other parts that will be utilized within your assembly design. As a result, this is probably the least efficient workflow for 3D design but is often the one employed by new users.

The third method is some combination of top-down and bottom-up design and is the most common. This approach might be called middle-out. This is top-down design with the ability to add existing subassemblies and parts as needed. Utilizing various functions such as parts libraries, Frame Generator, Bolted Connections, and Content Center components within an assembly file is an example of middle-out design.

Developing an Efficient Assembly Workflow

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Consider an example of a top-down workflow to better understand the benefits and efficiency of this type of design. Within this workflow, you will first create the top-level assembly file and then create the part files:

1.  On the Get Started tab, click the New button and select the Standard.iam template.

2.  Click Create on the Assemble tab, or right-click in the browser or graphics area and select Create Component. The default option in the Create In-Place Component dialog box is to create a new component as a standard single-part file. Instead, click the drop-down arrow in the Template area and select Standard.iam.

Available Templates

The choices available in the drop-down are the templates from the default tab. If you want to use a template from a different tab, click the Browse Templates button instead. Once you click the Browse Templates button, you will be presented with the Open Template dialog box, which gives you a choice of standards and templates.

3.  Name this assembly 2nd Level Assembly and then set New File Location to the Chapter 8 folder.

If it is known at the time of creating the subassembly file, determine the BOM structure for this subassembly. Note that you can change this later using the BOM Editor as needed. Figure 8.33 illustrates the selection choices for the BOM structure.

The choices for BOM structure are listed here with a brief description. You'll take a more in-depth look at BOM structure settings later in this chapter in the “BOM Structure Designations” section.

1.  Virtual Components These components require no geometry, such as paint, grease, and so on.

2.  Normal This is the default structure for all parts that are intended to be fabricated.

3.  Purchased These are parts or assemblies that are not fabricated in-house.

4.  Inseparable Generally, these are assemblies that cannot be disassembled without damage, such as weldments, riveted assemblies, and so on.

5.  Phantom Typically, this is a subassembly created to simplify the design process by reducing Assembly constraints and to roll parts up into the next-highest assembly level.

6.  Reference This is used for construction geometry or to add detail and references to the top-level assembly.

4.  In this top-down design example, you will be using Normal components. Confirm that Default BOM Structure is set to Normal and click the OK button.

5.  You will then be prompted to select a sketch plane for the base component of this assembly. In the Model browser, expand the assembly origin folder and select the XY Plane option.

This will place and anchor the new assembly to the top-level assembly origin. The origin planes of the new assembly will be anchored to the selected top-level assembly origin plane upon creation and will be grounded to the top-level origin plane. This new, second-level assembly will be activated within the Model browser, ready for editing, as shown in Figure 8.34.

6.  With the second-level assembly active, select Create Component once again, and this time use the Standard.ipt template to create a new part. Name this component Rotary Hub and set it to be saved in a subdirectory called Parts within your workspace, as shown in Figure 8.35. If the subdirectory does not exist, you will be prompted to create it. Leave the BOM structure setting as Normal and then click the OK button.

7.  To place the part, select the XZ plane from the Origin folder in 2nd Level Assembly.iam.

8.  Now you are in the Rotary Hub part file. Use the Start 2D Sketch button and select the XZ plane. You might need to expand the Origin folder to determine which plane is the XZ plane.

9.  Create and dimension the sketch, as shown in Figure 8.36.

10.Press E to display the Extrude dialog box and extrude the outer ring to a length of 1 inch.

11.Create a sketch on the top face of the ring. Sketch a concentric circle offset 0.5 inch to the inside of the overall diameter. Place a center point on the offset circle.

12.Start the Hole tool. The center point will be automatically selected. Set the diameter to 0.375 inch, and set Termination to Through All.

13.Create a circular pattern of the hole feature with six instances, as shown in Figure 8.37.

14.Click the Save icon. Since the part is active, it is saved, but the top- and second-level assemblies are not. Click the Return button twice to return to the top-level assembly.

15.Click Save again, and you will be prompted to name the top-level assembly file. Name the file Top Level Assembly and click the OK button.

16.The Save dialog displays the state of all the assembly files. Both of the assembly files are marked Initial Save. This means they exist only in memory and haven't been saved to hard drive (or network drive) yet. If you were to click in the Save column to change it to No, the files would be closed without saving, and you would just have the part file on the disc drive. Confirm that the both files are marked Yes, and click the OK button.

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Figure 8.33 BOM structure options

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Figure 8.34 Second-level assembly active

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Figure 8.35 Creating Rotary Hub.ipt in the Parts subdirectory

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Figure 8.36 Rotary Hub sketch

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Figure 8.37 A circular pattern of the hole feature

These steps illustrate the method of creating a true top-down design, starting with the assembly, then defining the subassembly, and finally creating a part to reside in the assembly structure. If this seems like a purely academic exercise because it is not the way you typically work, you might find that the concepts can still be useful to you every now and again. Often, the top-down, middle-out, or bottom-up approach is dictated by the need to assign part numbers and create assembly structure to match. Keep these things in mind as you work with Inventor assemblies, and you will more than likely find an opportunity to use them somewhere along the way.

Layout Sketches

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Another top-down (and/or middle-out) design workflow is the use of layout sketches or sketch blocks. Layout sketches are created in a part file, using sketch blocks to represent individual parts as basic 2D symbols. The 2D blocks are “assembled” in the part sketch and can be dimensioned and constrained to simulate simple assembly mechanisms to test function and to some extent fit. The first step in creating a layout sketch is to create a part file and a sketch. Next, 2D sketch geometry is created and turned into sketch blocks, with a single block representing each component within the mechanism. Nested blocks (blocks made of other blocks) can be used to represent subassemblies and can even be set as flexible to allow them to pivot around or translate motion along an axis. Once the basic 2D layout design is complete, you can use the Make Part and Make Component tools to write out the blocks as individual part models from the sketch blocks. From there, a 3D assembly can be created based on, and linked to, the sketch blocks. In this way, if you update the sketch layout, the parts and assemblies will automatically update.

The following example will introduce layout and sketch-block functionality:

1.  Click the Get Started tab and click Open.

2.  Browse for the file mi_8a_019.ipt located in the Chapter 8 directory of the Mastering Inventor 2015 folder and click Open.

3.  Locate the sketch called Layout Assembly in the browser and click the plus sign to expand it.

4.  Notice that the sketch contains a block called Base Mount. Right-click the sketch and choose Edit Sketch.

5.  Select the Create Block button from the Create panel (note that you might need to use the small black arrow to expose the flyout menu).

6.  Select all of the geometry on the left of the sketch with the visible dimensions.

7.  Click the Insert Point button in the Create Block dialog box and then select the lower-left corner of the rectangle as the insert point.

8.  Enter Base Plate for the block name and then click the OK button to create the block.

9.  Expand the Blocks folder in the browser and notice that the Base Plate block has been added to the block definitions. The geometry you selected has been converted to a block as well and now behaves as a single entity.

10.Place a Concentric constraint on each of the half-circle shapes on the base plate and the corresponding half-circle shape on the base mount. Exit the Constraint tool by right-clicking and clicking the OK or Cancel button.

11.Select the Arm Assembly block from the Blocks folder and drag it into the graphics area to place an instance of it.

12.Place a Concentric constraint on the right circle of the Base Mount block and the large dashed circle on the bottom link of the Arm Assembly block. Exit the Constraint tool by right-clicking and clicking the OK or Cancel button.

13.Select the Cylinder Assembly block from the Blocks folder and drag it into the graphics area to place an instance of it.

14.Place a Concentric constraint on the left circle of the Base Mount block and the larger circle on the Cylinder Assembly block. Exit the Constraint tool by right-clicking and clicking the OK or Cancel button.

15.Right-click the Cylinder Assembly block and choose Flexible. This allows the underconstrained geometry to solve independently at the top-level block.

16.Click and drag the free end of the Cylinder Assembly block to see the plunger slide in the cylinder.

17.Place a Concentric constraint on the free end of the Arm Assembly block and the free end of the Cylinder Assembly block.

18.Click Finish Sketch to return to the feature level. Figure 8.38 shows the layout sketch.

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Figure 8.38 Blocks folder and blocks in the sketch

Notice that you can continue to drag the sketch assembly to see the adjustment of the cylinder and the angle for the arm assembly. As you can see, creating layout sketches in this fashion allows you to solve linear and pivot motion layouts in 2D. Once the sketch layout has been completed, you can use the Make Components tool to write each block out to an individual part and/or assembly file. You can close the current file without saving changes or use it to explore the Make Components workflow using these general steps:

1.  Click the Make Components button on the Manage tab and then select the sketch blocks you want to create components for.

2.  Select additional blocks to add to the list, or select from the list and click Remove From Selection to exclude any blocks you decide you do not want to create components for.

3.  Select Insert Components In Target Assembly and then set the assembly name, the template from which to create it, and the save path (or clear this option to create the parts only). If the assembly already exists, use the target assembly location's Browse button to select it.

4.  Click Next to accept your selections.

5.  The next dialog box allows you to name and set paths for the files to be created. Click the cells in the table to make changes for the components as required:

·     Click or right-click a cell to choose from the options for that cell type, if any.

·     You can Shift+click multiple components and use the buttons above the Template and File Location columns to set those values for multiple components at once.

6.  Click Include Parameters to choose which layout model parameters to have present in the created parts.

7.  Click the Apply or OK button to make the components. If the component files are created in an assembly, the assembly file is created with the parts (and subassemblies) placed and left open in Inventor, but the assembly and parts are not saved until you choose to do so. If you choose to create the components without an assembly, you are prompted to save the new files as they are created.

8.  You can then open each part file and create 3D geometry based on the sketch block. Changes to the original layout sketch push through to the 3D part and assembly.

Layout sketches can boost your productivity. During the initial stage of design, there are frequent changes as you nail down the details. When you initially create the layout sketch, you can easily investigate “what if?” scenarios. You can add as much or as little detail as you need to define the function and form. If you do need to make a change in the relationship of components, you can do that in the layout sketch, and then the update will get pushed to all the components. Once components are generated from the blocks, you can edit them and build the model parts based on the basic blocks. You can open the assembly called mi_8a_020.iam to examine a simple assembly created from the layout sketch used in the completed version of the previous exercise.

Flexibility

When multiple instances of the same subassembly are used within a design, each instance can be made flexible, allowing underconstrained components in the subassembly to be solved at the top-level assembly. The caster assemblies in Figure 8.39 have been made flexible so they can be swiveled and positioned independently as they would in the real world.

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Figure 8.39 Flexible subassemblies

A subassembly instance is made flexible by right-clicking the instance within the browser and selecting Flexible. Flexible subassemblies are displayed with an icon next to the instance name in the browser so that you can easily determine which instances are flexible.

Flexible assemblies can be nested into flexible subassemblies and will still update whenever the original assembly is changed. One common use of flexible assemblies would be in the creation of hydraulic cylinders that require extensions of different lengths when used in multiple locations within a top-level assembly. When each instance of the assembly is made flexible, each cylinder can move accordingly within the top-level assembly.

If a subassembly with nested flexible subassemblies is to be placed into a top-level assembly, you simply right-click that subassembly to bring forward the flexibility of the nested flexible assemblies. Consider the example of the hydraulic cylinder. Multiple instances of the cylinder might be placed into an extension arm assembly, and each instance made flexible so that they can be allowed to adjust as they are constrained to the extension-arm parts.

If two instances of the extension arm are then placed into a top-level assembly, those instances need to be made flexible as well in order to allow the cylinders to demonstrate flexibility. You can use the file mi_08a_030.iam to explore flexible subassemblies.

Adaptivity

Cross-part adaptivity is a powerful feature of Autodesk Inventor, and it can be turned on or off at will. Adaptively is an option that allows a sketch or feature in one part to update based on a sketch or feature found in another part. Although adaptivity is a powerful tool when properly used, it can also cause performance problems when used indiscriminately in large assemblies or when an adaptive part is utilized in another assembly without its related part. But you can fix both situations with simple methods.

Because active adaptive parts can cause performance issues in large assemblies, you should turn off adaptivity after use. If a related part is edited, adaptivity on the associated part should be turned on, and the assembly should be updated to reflect the changes on the related part. Once this is done, that adaptivity should be turned off once again.

Tracking Adaptivity

It is a good idea to turn off adaptivity when it's not in use; however, Inventor does not have a good method to tell you what parts were adaptive. One way is to rename the browser nodes so that you can tell what parts were adaptive. A simple way to do this is to append -A on the browser node. Now you'll know which parts were adaptive even where they are not currently adaptive.

If an adaptive part is to be used in other designs, save the part with a different filename and remove the adaptivity from the new part. Otherwise, the adaptive relationships will carry over into the other design, and you won't be able to edit shared parts.

Creating Adaptivity

This example creates an adaptive relationship between two parts and demonstrates how they are linked together:

1.  On the Get Started tab, click Open.

2.  Browse to Chapter 8 in the Mastering Inventor 2015 directory and open mi_08a_021.iam.

3.  Click the Create button on the Assemble tab, or right-click in the browser or graphics area and select Create Component.

4.  Name the new part file Gasket. For New File Location, browse to the Chapter 8 folder, confirm that Constrain Sketch Plane To Selected Face Or Plane is selected, and click the OK button.

5.  Select the top face of the rotary hub part for the new part sketch. Depending on the Application Options Sketch settings, Inventor might create Sketch1 for you or you might need to do this manually. If no sketch is created, use the Start 2D Sketch button and select the top face of the rotary hub part again.

6.  Click Project Geometry on the Sketch tab and select the top face of the existing part. The geometry is projected into the sketch. Note that adaptive glyphs have been added to the browser to indicate that the part and sketch are adaptive. Also, there is a Reference1 node nested under the sketch. This node contains the information linking the two parts, as shown in Figure 8.40.

The adaptive glyph is displayed when adaptivity is turned on. You can turn adaptivity on and off by right-clicking the node in the browser. You can toggle the feature or sketch adaptivity while editing the part, but you have to return to the assembly level to toggle adaptivity on the part. Additionally, you can disable the creation of adaptive loops when projecting geometry altogether; to do so, select the Tools tab, click Application Options, select the Assembly tab, and then uncheck the Cross Part Geometry Projection option.

7.  Finish the sketch by right-clicking and selecting Finish 2D Sketch from the context menu, as shown in Figure 8.41. Do not click Finish Edit or Inventor will not only finish the sketch but will also exit the part and return you to the assembly.

8.  Extrude the Gasket part to a thickness of 2 mm, click the Return button to return to the assembly, and then click Save.

9.  To see how adaptivity works, double-click the rotary hub component to activate that part for editing. You can double-click the part in the graphics area or the icon next to the part name in the Model browser to activate any part for editing.

10.In the Model browser, right-click Extrusion1 and select Edit Sketch. Change the overall diameter from 130 mm to 160 mm and click the OK button.

You will notice that the overall diameter and the diameter of the hole pattern of the rotary hub component have changed, but the corresponding gasket part remains unchanged.

11.Click Return to move up to the second-level assembly design state once again. Both parts are active at the subassembly level, so the gasket part updates to match the rotary hub component.

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Figure 8.40 Part marked with the adaptive icon in the browser

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Figure 8.41 Selecting Finish 2D Sketch, not Finish Edit

As you can see, the ability to adapt one part to another can make updates across parts easy. You can close this assembly without saving the changes and continue.

Removing Adaptivity from Parts

Once a design has been approved and released for production, you should completely remove adaptivity from all parts within your assembly. Removing the adaptivity ensures that the part can be reused within other designs without conflict and will not be updated accidentally.

If you decide to retain adaptivity within your original assembly but plan on using the adaptive part in other assemblies, the adaptive icon will not display on those instances of the part. This is because only one occurrence of a part can define its adaptive features. However, all occurrences reflect changes and adaptive updates, including occurrence in other assemblies. It is for this reason that you must use adaptivity carefully.

To completely remove adaptivity from a part, either activate or open the adaptive part and activate the adaptive sketch. Expand the sketch and right-click Reference to select Break Link, as shown in Figure 8.42.

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Figure 8.42 Breaking the adaptive link

When the adaptive link is broken, the reference geometry is converted to normal sketch geometry. This geometry will need to be fully dimensioned and constrained. Once the geometry has been converted to normal sketch geometry, the part will no longer be able to be adaptive.

Making Temporary Use of Adaptivity

Use adaptivity to find mounting holes for positioning hardware components on a base part. For example, consider a mounting clip and a base plate.

Constrain the clip to the base plate; then make the base plate active for editing and create a sketch on the plate surface. With the sketch active, project the mounting holes, locating holes, and other needed geometry from the mounting clip to the base plate. This creates adaptive relationships in the base plate to the mounting clip.

Once the design is finalized and all the mounting clips are properly located, simply turn adaptivity off on the base plate. When the design is released for production, or at any other desired time, convert the reference geometry created when you projected the geometry to normal sketch geometry. Then dimension and constrain the mounting holes as you would any other feature.

Assembly Features

An assembly feature is a feature created and utilized purely within the active assembly file and environment. Because this feature was created within the assembly file, it does not exist at the single part or subassembly level. A good example of an assembly feature in use is the technique of creating drilled holes through a standard tabletop within an assembly. Common practice is to place brackets on the tabletop to find the mounting-hole locations. This allows the holes to be drilled at the same time, ensuring an exact match and placement. Assembly features in Inventor mimic this approach.

Examining the individual tabletop file reveals that the part file does not contain the drilled holes, simply because the drill operation was performed at the assembly level rather than the part level. To understand the reasoning behind this, you might consider that the tabletop is a common part stocked in the shop and then machined as required for each assembly in which it is used. Although the stock part might exist as a cataloged item with no holes, it may exist in many different assemblies with holes of various sizes and locations. Using assembly features allows you to work in this manner.

Other examples of assembly features are contained within the weldment environment, where preparations used to facilitate welding components together are at the assembly level. Preparation features allow trimming of soon-to-be-welded components to eliminate interferences between welds and other parts of the weldment.

Care must be taken when creating geometry within the context of the assembly because it is easy to create an assembly feature when intending to create a part feature. Although this is a common mistake that new users will make, it is one that anyone can experience. In a multilevel top-down design, always make sure you are working in the proper assembly or component by double-clicking the assembly or component in the Model browser for the purpose of opening that component for editing.

To explore the creation of assembly features, follow these steps:

1.  On the Get Started tab, click Open.

2.  Browse to Chapter 8 in the Mastering Inventor 2015 directory and open mi_08a_022.iam.

This assembly consists of three parts, two of which are instances of the same part, Part_100_8. The other component, Part_200_8, currently interferes with the other two parts. Your goal is to cut a keyhole in both instances of Part_100_8 so that the keyed bar will fit into them. Part_100_8 is a stock bracket used in many assemblies; therefore, you must take care not to create a feature in it that will have a negative impact on its use in all of the assemblies that consume it. To start, you will explore a keyway created by another user at the part level.

3.  Double-click the front instance of Part_100_8 to set it active for edits.

4.  Locate the feature called Keyway Cut in the browser, right-click it, and choose Unsuppress Features.

5.  Right-click and choose Finish Edit to return to the assembly level.

Notice how the keyway cuts the part in the same location on each instance of the part, missing the location on the second instance because of the orientation of the two instances of Part_100_8. Another important aspect of the keyway is that it impacts every instance of the part, in every assembly it was used in. To fix this, continue.

6.  Double-click the front instance of Part_100_8 to set it active for edits again.

7.  Locate the feature called Keyway Cut in the browser, right-click it, and choose Delete. Click the OK button in the delete confirmation dialog box.

8.  Right-click and choose Finish Edit to return to the assembly level.

9.  From the 3D Model tab, click the Start 2D Sketch button and choose the large front face of the front instance of Part_100_8 to create the sketch on.

10.From the Sketch tab, click the Project Geometry button.

11.Select the circular edge and the three flat edges of the keyed bar's end profile, projecting the complete key profile into the sketch.

12.Click the Finish Sketch button. Notice the sketch location in the browser.

13.From the 3D Model tab, click the Extrude button. Notice that the only operation available in the Extrude dialog box is Cut. You cannot add material at the assembly level.

14.Set the Extents drop-down box to All, ensure that the cut is going in the right direction, and then click the OK button.

15.You should see the keyhole cut through both instances of Part_100_8 and the keyed bar (Part_200_8) disappear.

16.Expand the Extrusion1 feature in the browser and you will see the listing of all components involved in the extrusion cut.

17.Right-click Part_200_8 and choose Remove Participant so the keyway cut does not cut the keyed bar.

18.Finally, right-click either instance of Part_100_8 and choose Open. Notice that the keyhole is not present in the part file because it exists only as an assembly-level feature.

You can close this file without saving changes. You should know that in addition to removing participating components from an assembly-level feature, you can add components to an assembly feature by right-clicking the feature, choosing Add Participant from the menu, and then choosing the component from the browser. On the right of Figure 8.43, a component named Top-103:2 is being removed from the feature named Extrusion 1 so that the extrusion cut does not go through that part. On the left, another component is being added to the extrusion feature.

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Figure 8.43 Adding/removing participants from assembly features

Assembly features can be made with the Extrude, Revolve, Hole, Sweep, Fillet, Chamfer, and Move Face tools. Keep in mind that all assembly features are allowed only to cut or remove material and cannot add material to a part. Other commonly used assembly feature commands within the Assembly panel environment are the Mirror and Patterns commands.

Isolate Components Before Creating Assembly Features

If you select the components to be involved in an assembly feature first and then create the feature, you will not need to remove participants that you didn't intend to cut in the first place.

Managing the Bill of Materials

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In Inventor, the Bill of Materials (BOM) is the internal, real-time database that exists within every assembly. Real-time means that as components are added to the assembly, they are automatically added and counted in the BOM. Although you might be accustomed to referring to the tabled list of parts on the 2D drawing as a bill of materials, in Inventor such a table is called a parts list. Parts lists pull directly from the assembly BOM.

The BOM is controlled at two levels: the part level and the assembly level. Both levels factor in certain aspects of how the bill of materials is generated, how components are represented, and ultimately how the parts list is generated within the drawing environment.

Parts-Level BOM Control

In the part environment, the designer has the ability to define the BOM structure of just a part. At this level, the structure can be defined as Normal, Inseparable, Purchased, Phantom, or Reference. Determining the default setting at the part level allows control of how the component is identified within the overall BOM for any assembly the component is used in. By setting the structure at the part level, you can control the assembly BOM display according to the part settings. Any structure settings at the part level can be overridden and changed to Reference at the assembly level.

Another important structure setting at the part level is the Base Quantity property. This setting controls how the part is listed in the BOM. If Base Quantity is set to Each, the part is tallied by count. This is the default for most standard parts. The Base Quantity can also be set to reflect the value of any given model parameter. This is most often set to a length parameter so that the Base Quantity property will tally the total length of a part used in an assembly. Parts pulled from Content Center and Frame Generator have their Base Quantity property set to pull a length parameter by default. The Base Quantity property is set by choosing Tools  Document Settings and selecting the Bill Of Materials tab.

Assembly-Level BOM Control

BOM control accelerates at the assembly level. You can access the Bill Of Materials dialog box by clicking the Bill Of Materials icon on the Manage panel of the Assemble tab. In the drawing environment, the BOM Editor dialog box is accessible by right-clicking the parts list and selecting Bill Of Materials.

The Bill Of Materials dialog box allows you to edit iProperties, BOM properties, and the BOM structure; override quantities for components; and sort and create a consistent item order for generating parts lists. Figure 8.44 shows the Bill Of Materials dialog box.

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Figure 8.44 Bill Of Materials dialog box

Exporting a bill of materials is a straightforward process, with icons across the top of the dialog box allowing the export of the BOM data in a structured or parts-only view in formats such as MDB, dBase, or various Excel formats. The Engineer's Notebook icon permits the export of database information as a note.

Adding and Removing Columns

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You can add columns to the model in any of the three tabs in the Bill Of Materials dialog box by clicking the Choose Columns icon, which will display a dialog box list in which you can drag a desired column to a specified location, as shown in Figure 8.45. To remove a desired column, simply drag the column to be removed back to the dialog box list.

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Figure 8.45 Choose Column dialog box

The next icon at the top of the Bill Of Materials dialog box allows you to add custom iProperty columns. The drop-down list shown in Figure 8.46 within the Add Custom iProperty Columns dialog box will display a combined list of all the available custom iProperties contained within the assembly.

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Figure 8.46 Custom iProperty list

If a desired custom iProperty does not exist within the list of components, you can add it manually by selecting the <Click To Add iProperty Column> option displayed in the list box. Be sure to set the data type to the correct format when manually adding a custom iProperty to the assembly file. Manually added iProperties will be stored in the assembly file. Figure 8.47 shows the addition of a custom iProperty column called Assembly Station.

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Figure 8.47 Creating a new custom iProperty

Once custom iProperty columns have been added to the assembly bill of materials, individual parts can be populated with custom iProperties as needed. Individual parts that already contain those iProperties will show the values within the respective row and column. iProperties that are edited or added to a respective part row will be pushed down to the part level; therefore, filling out iProperties at the assembly level is often the most efficient way to populate part iProperties.

The Create Expression icon located at the beginning of the Formula toolbar launches the Property Expression dialog box so you can create an iProperty expression. The newly created expression can contain a combination of custom text and iProperty names in brackets. The iProperty expression will be substituted for the field in which the expression was created once the expression is evaluated. In Figure 8.48, the expression is created in the Description field.

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Figure 8.48 Creating property expressions

Looking across the top of the Bill Of Materials dialog box, the two icons to the far right are Part Number Merge Settings and Update Mass Properties Of All Rows. Clicking the Update Mass Properties Of All Rows icon recalculates the total mass for all components within the assembly.

Clicking the Part Number Merge Settings icon allows different components possessing the same part number to be treated as the same component. For instance, say six base plates of the same size are used in an assembly. Four of these plates have holes drilled upon installation, and two have holes placed during fabrication. As far as the shop is concerned, all six are the same part, but in the design both plate types exist as separate part files.

To have the BOM count the total number of plates, you set the Part Number property to match on both items and then use Part Number Merge Settings to have these files counted as a single item.

BOM Structure Designations

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You can choose from five designations when assigning BOM structure to components: Normal, Inseparable, Purchased, Phantom, and Reference. Any part or assembly file can be assigned one of these designations within the BOM. The designation is then stored in the file, meaning that if a part is marked as Purchased in one assembly, it will be designated as Purchased in all assemblies. The structure designations are as follows:

1.  Normal This is the default structure for most components. The placement and participation in the assembly bill of materials are determined by the parent assembly. In the previous example, you created an assembly file rather than a single part. As a result, you will be determining the characteristics of how this assembly file will behave in the top-level assembly bill of materials. With a Normal BOM structure, this assembly will be numbered and included in quantity calculations within the top-level assembly.

2.  Inseparable These are generally assemblies that cannot be disassembled without damage. Examples of Inseparable assemblies might include weldments, glued constructions, and riveted assemblies. In a parts-only parts list, these assemblies will be treated as a single part. Another example is a Purchased part such as a motor.

3.  Purchased This designation is typically for parts or assemblies that are not fabricated in-house. Examples of Purchased components are motors, brake calipers, programmable controllers, hinges, and the like. A Purchased component is considered as a single BOM item regardless of whether it is a part or a subassembly. Within a Purchased assembly, all child parts are excluded from the BOM and quantity calculations.

4.  Phantom Use Phantom components to simplify the design process. A Phantom component exists within the design but is not shown as a line item in the BOM. A common use for a Phantom component would be a subassembly of parts that are grouped for ease of design. Setting the subassembly to be a Phantom component allows the parts to be listed in the BOM individually. Other examples of Phantom components could include hardware sets, screws, nuts, bolts, washers, pins, and various fastener-type components. A good example of a Phantom assembly would be a collection of parts that are normally assembled onto the machine one at a time. However, in the interest of reducing the overall number of Assembly constraints within the design, the engineer might choose to preassemble the various components within a Phantom assembly. That assembly could then be constrained as one component instead of multiple parts.

5.  Reference Mark components as Reference when they are used for construction geometry or to add detail and references to the top-level assembly. A good example of a Reference component is a car body and frame that represents the outer shell for placement of a power train. In the 2D documentation, the car body and frame would be shown as hidden lines illustrating the overall design while highlighting the power train as the principal component within a view. Reference geometry is excluded from quantity, mass, or volume calculations regardless of their own internal BOM structure. As a result, they are not included within the parts list. They are placed only within the overall assembly to show design intent and position.

In addition to using these five BOM structure designations for component files, you have the ability to create a virtual component, which has no geometry and does not exist as an external file. A virtual component can have a complete set of properties that are similar to real components but are primarily used to represent bulk items such as fasteners, assembly kits, paint, grease, adhesive, plating, or other items that do not require creating an actual model. A virtual component can be designated as any of the previous BOM structure types and can contain custom properties, descriptions, and other aspects of the BOM data like any other component.

A virtual component will be shown in the Model browser as if it were a real part. Virtual components can be created by selecting the check box next to the Default BOM Structure drop-down in the Create In-Place Component dialog box, as shown in Figure 8.49.

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Figure 8.49 Creating a virtual component

Virtual Components in Templates

If you use the same virtual components in most of your assemblies, you might want to create them in a blank assembly, fill out their BOM properties using the BOM Editor, and then save the assembly as a template file. Then when you create a new assembly, the virtual components will already be present. Any of them not required can simply be deleted.

BOM View Tabs

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Each tab in the Bill Of Materials dialog box represents a different BOM view. All tabs permit ascending or descending sorting of the rows in the BOM by clicking the respective column header. You can also reorder rows by simply clicking and dragging a component's icon.

With the Model Data tab active, you see the components listed just as they exist in the Model browser. You can add or remove columns to populate the Model Data tab independently of the other BOM view tabs. On this tab all components are listed in the BOM regardless of BOM structure designation. Item numbers are not assigned on the Model Data tab. The model data is not exportable or available for placement as a parts list. Instead, this tab is typically used for organizing the BOM and assigning the BOM structure designation.

Figure 8.50 shows a bill of materials on the Model Data tab. Notice that there are no item numbers listed and that all component structure types are displayed, including Reference and Phantom components. Notice too that the last two parts listed are virtual parts and have been given different BOM structure designations.

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Figure 8.50 BOM Model Data tab

In addition to the Model Data tab are the Structured and Parts Only tabs. These tabs are disabled by default. To enable them, right-click the tab and choose Enable BOM View; alternatively, click the View Options button along the top of the Bill Of Materials dialog box.

The Structured tab can display all components of the assembly, including subassemblies and the parts of the subassemblies. In Structured view, additional icons will be active on the toolbar, allowing you to sort by item and renumber items within the assembly BOM. The order of the BOM item numbers is stored in the assembly file.

The View Options icon allows you to enable or disable the BOM view and set the view properties from the drop-down. Choose View Properties to modify the Structured view. The resulting Structured Properties dialog box contains two drop-down lists defining the level, the minimum number of digits, and the assembly part delimiter value. If the level is set to First Level, subassemblies are listed without the components contained within. If set to All Levels, each part is listed in an indented manner under the subassembly, as shown in Figure 8.51.

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Figure 8.51 Structured Properties dialog box

The Parts Only tab lists all components in a flat list. In this BOM view, subassemblies designated as Normal are not listed as an item, but all their child components are displayed. By contrast, Inseparable and Purchased subassemblies are displayed as items, but their child components are not displayed.

Bill of materials settings that are modified by the Bill Of Materials dialog box will carry forward into the drawing parts lists contained in the assembly. Note that if both the Structured and Parts Only views of the BOM are enabled, the same part may have a different item number in each view.

Figure 8.52 shows a bill of materials in the Structured view compared to the same assembly in the Model Data view. The first thing to note is that all the components have been assigned item numbers in the Structured view. You might also notice that the Reference and Phantom components that are listed in the Model Data view are filtered out of the Structured view. Closer inspection reveals that although the Phantom subassembly named TK-035-001 is not included in the Structured view, its child parts are listed, each with an arrow next to the icon to denote that they are part of a subassembly. Recall that Phantom subassemblies are used to group parts for design organization and to reduce Assembly constraints while allowing the parts to be listed individually.

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Figure 8.52 BOM structured view

Figure 8.53 shows a bill of materials in the Parts Only view. This Parts Only view filters out Reference and Phantom components just like the Structured view does. Notice too that although the subassemblies are not listed as items, their child parts are. The exceptions to this are Purchased and Inseparable assemblies. In the figure, the Purchased subassembly lists as a single item, since it is a Purchased component comprising two Purchased parts and is assumed to be purchased as one item. Note that if you had the need to list the parts as items rather than the subassembly, you would designate the subassembly as Phantom rather than Purchased.

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Figure 8.53 BOM Parts Only tab

Take a look also at the Inseparable subassembly named TK-035-004. It lists as an item along with one of its child parts named K-035-01. This child part lists because it is a Purchased item and needs to be ordered. Had both children of the Inseparable subassembly been Normal parts, neither would be listed in the Parts Only view.

Adding Two Parts with the Same Part Number

You may occasionally need to add two separate part files to an assembly but have them listed as the same part number. For instance, when you're using Frame Generator, each member is created as a separate part even though those parts might be identical in profile and length. This is done so you can modify each part individually as needed. However, if the parts remain identical once the design is complete, you can use the BOM Editor and set each identical part file to use the same part number even though the part files have different names. This allows the BOM to count the parts as a single item.

Assembly Reuse and Configurations

Frequently existing assemblies are used in other designs or are used in multiple locations within the top-level assembly. There are three basic workflows for reusing and configuring assemblies in a design:

·     Copying designs

·     Using view, positional, and level-of-detail representations

·     Using iAssemblies (table-driven assemblies)

Copying Designs

Often you'll need to copy a previous design to create a similar design based on the original. Part of the challenge of doing this with Inventor is creating copies of only the parts that will be modified in the new design while reusing parts that do not incur changes, all while maintaining healthy file links. To do this effectively, you can employ the Copy Components tool from within the assembly to be copied.

ICopy

Depending on the design, you might be called on to create subassemblies containing similar geometry but having different sizes and/or positions in the top-level assembly. Rather than manually creating each of these subassemblies, you can use the iCopy tool. iCopy combines skeletal modeling (using a part file as the “skeleton” on which to arrange other components) and adaptivity. If you design curtain walls, trusses, bridge-type frames, or any design where subassemblies are basically the same but vary in size and position, you may want to explore the iCopy tool. There are four general steps to using iCopy:

1.  Create a target assembly using the skeletal target layout part.

2.  Create the subassembly to be patterned using the template layout part.

3.  Use the iCopy Author tool in the subassembly to make it usable as an iCopy template.

4.  Use the iCopy tool to copy/pattern the subassembly.

To begin this process, first select the top-level assembly from the browser tree and then click the Copy button from the Pattern panel (note that you might need to click the small black arrow to find the Copy button). You will be presented with the Copy Components: Status dialog box, which lists the top-level assembly and the components within, as shown in Figure 8.54. Use the Status buttons next to each component to set the component to be copied, reused, or excluded from the copy operation.

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Figure 8.54 Copy Components: Status dialog box

In the example in Figure 8.54, the component named mi_08_309_PCB is the only part that needs to be redesigned for the new assembly; therefore, it is the only part set to be copied. In the original design, there are two that have been excluded in this copy operation because they will be swapped out for other parts that are already created, after the copy has been made. You will notice that the other components except the top-level assembly are set to be reused. Once the copy status of each part is set, click the Next button to move to the Copy Components: File Names dialog box, shown in Figure 8.55.

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Figure 8.55 Copy Components: File Names dialog box

In the Copy Components: File Names dialog box, you want to set the destination button to Open In New Window in order to create a new, separate assembly file. You can then use the Prefix and/or Suffix controls to modify the existing filenames, or you can type in new names as required. By default, File Location is set to Source Path, meaning that the new files will land right next to the existing ones. If that is not desirable, you can right-click each File Location cell and choose User Path or Workspace. Care should be taken to ensure that file location paths are not set outside the project search path. When the filename and paths are set, click the OK button.

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Rolling Revisions

A large part of any engineering department's time and energy is focused on revision control. You can think of a revision roll as just a copy of an existing design with improvements. Here is a general procedure for rolling the revision of an approved design, where Rev1 is complete and Rev2 is being created:

1.  Open the Rev1 assembly and start the Copy Components tool.

2.  Configure the Copy Components list to include, exclude, and reuse components as required for Rev2.

3.  Set the destination button to Open In New Window and click the OK button to create the Rev2 assembly.

4.  Rename and set the file location for all copied components as well as for the Rev2 assembly file.

5.  Add additional components to the Rev2 assembly as needed and make any other modifications required.

6.  Open the Rev1 drawing file and use Save As to create a Rev2 copy.

7.  In the Rev2 drawing, click the Manage tab and use the Replace Model Reference button to exchange all of the Rev1 views, parts lists, and other references with Rev2.

The new assembly file will open in a separate window. Interrogation of the Model browser should reveal that the components set to be reused are listed just as they were in the original assembly, the components set to be copied are listed as specified, and the components set to be excluded are not present at all.

Using Representations

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Inventor provides the ability to create and store three basic types of representations within an assembly file. Representations allow you to manage assemblies by setting up varying views, positions, and levels of detail for your models. Each of these allows for the creation of user-defined representations, and each has a master representation. Note that although user-defined representations can be renamed and deleted as required, master representations cannot. Using representations enhances productivity and improves performance in large assembly design.

Once representations are created in an assembly, you can open that assembly file in any combination of those representation states by clicking the Options button in the Open dialog box, as shown in Figure 8.56. Keep in mind that although you can open or place a file by typing the filename rather than scrolling and clicking the icon, you cannot access the Options button without explicitly scrolling and selecting the file in the dialog box.

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Figure 8.56 Opening a file in a representation

View Representations

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View representations, also known as design views and ViewReps, are used to configure the display of an assembly and save that display for later use. View representations control the following settings:

·     The visibility state of components, sketch features, and work features

·     Component color and styles applied at the assembly level

·     The enabled/not enabled status of components

·     The “camera view,” meaning the on-screen zoom magnification and orientation

·     The browser tree state

In effect, view representations allow “snapshot views” of portions of an assembly file. Each view representation is saved within the assembly file and has no effect on individual parts or subassemblies. View representations are relatively simple to create and use. To create a view representation, follow these general steps:

1.  While in the assembly, simply zoom and rotate your model until you have the desired view showing in the current graphics window.

2.  Expand the Representations folder and right-click View to select New, as shown in Figure 8.57.

3.  Turn off the visibility of a few parts; these visibility changes will take place only within this view representation.

4.  After creating the new view representation, click Save to preserve the newly created representation.

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Figure 8.57 Creating a new view representation

You can protect the view representation you create from accidental edits by right-clicking it and choosing Lock. View representations can be accessed either by double-clicking the desired representation or by right-clicking the desired representation and selecting Activate. Private view representations are views created in early releases of Inventor and are not associative.

Activating a New View Representation to Prevent Errors

Probably one of the most misunderstood “errors” in Inventor is the “The current Design View Representation is locked” message. This tells you that changes will not be saved, and it alarms a lot of new users. What this means is that you have turned off the visibility (or enabled status or any number of other things) while in the master view representation. Since the master is locked, these changes will not be saved, and the next time you open the file, the model will be at the previous state. To circumvent this issue, be sure to activate a new ViewRep or use the one called Default, make your changes, and then save. This way, your visibility, color overrides, and other settings will be saved in the ViewRep.

Positional Representations

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Positional representations, often referred to as PosReps for short, can be employed to set up and store components in various arrangements and are used to help test and analyze assembly motion. Positional representations work by overriding Assembly constraints, assembly patterns, or component properties.

To create a new positional representation, expand the Representations heading in the browser, right-click the Positional Representations heading, and then choose New. Continue by right-clicking the component, pattern, or constraint in the Model browser that you want to change. Choose Override from the context menu. The Object Override dialog box will open to the Relationship, Pattern, or Component tab, depending on the entity type that you right-clicked. You can rename the new representation from the default name to something more meaningful; however, you cannot rename the master representation.

In the following exercise, you will create positional representations to control the movement for the components of a hobby-type CNC router. Note that there are four components in this assembly. In the real world, these four components would be modeled as subassemblies; however, they have been created as simple part files in order to simplify the model. Follow these steps to explore the options involved in creating simple positional representations:

1.  On the Get Started tab, click Open and then select the file mi_08a_023.iam from the Chapter 8 folder of the Mastering Inventor 2015 folder.

2.  Click and drag the component named Z-Axis Assembly_08, and notice how it can be dragged to cause interference and into an unrealistic location.

Currently this assembly has two sets of constraints defined. One set defines the X, Y, and Z travel limits, and the other set defines the home position for each of the assembly components. In the current state, all of these constraints have been suppressed. In the next steps you will create a positional representation and unsuppress the home position constraints.

3.  Click the plus sign to expand each component in the browser and notice the suppressed constraints.

4.  Locate the Representations folder in the browser and then click the plus sign next to the icon to expand it.

5.  Right-click Position and choose New to create a new positional representation, as shown in Figure 8.58.

6.  Expand the Position node, if needed, and notice that a positional representation called Position1 has been created and is currently active, as denoted by the check mark.

7.  Select Position1; then click it and rename it Home Position.

8.  Right-click the Z Home constraint listed under the Z-Axis Assembly component and choose Override, as shown on the left of Figure 8.59.

9.  In the Override Object dialog box, click the Suppression check box and set the drop-down box to Enable.

10.Click the Value check box and set the value to -580 mm; then click the OK button. This sets the z-axis assembly to a static up and down position. You can click and drag the component to see this.

11.Right-click the Y Home constraint and choose Override.

12.In the Override Object dialog box, click the Suppression check box and set the drop-down box to Enable.

13.Click the Value check box and set the value to -28 mm; then click the OK button. This sets the y-axis assembly to a static left and right position. If you click and drag the z-axis assembly, you will see that it is now locked in place.

14.Right-click the X Home constraint listed under the X-Axis Assembly component and choose Override.

15.In the Override Object dialog box, click the Suppression check box and set the drop-down box to Enable.

16.Click the Value check box and set the value to 395 mm; then click the OK button. This sets the x-axis assembly to a static forward and backward position.

17.Right-click the Master positional representation and choose Activate. Click and drag the z-axis assembly and notice that it is free to drag again.

18.Right-click the Home Position representation and choose Activate to set the assembly back to its defined home position; notice that it is constrained in place.

In the next set of steps you will create another positional representation and unsuppress the set of constraints that will control the X, Y, and Z travel limits.

19.Right-click Position at the top level of the Positional representation node and choose New to create a new positional representation.

20.Expand the Position node, if needed, and notice that a new positional representation has been created and is currently active, as denoted by the check mark.

21.Rename the new positional representation to Set to Range.

22.Right-click the Z Travel constraint and choose Suppress (Override), as shown in Figure 8.60.

This toggles the suppression value of the Z Travel constraint and enables it so the travel is limited in the z-axis to hold it to a realistic range of motion. Next, you will do the same for the Y and X Travel constraints.

23.Right-click the Y Travel constraint and choose Suppress (Override).

24.Right-click the X Travel constraint and choose Suppress (Override). Note that you may need to expand the x-axis assembly component in the browser to find this constraint.

25.Right-click the Home Position representation and choose Activate. Click and drag the z-axis assembly to set the assembly back to its home position.

26.Right-click the Set to Range representation and choose Activate to set the assembly so it can be dragged within its defined range of travel.

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Figure 8.58 Creating a new positional representation

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Figure 8.59 Overriding a constraint value

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Figure 8.60 Enabling a suppressed constraint

As you can see from the previous steps, positional representations are a powerful way to show components in multiple positions as required during the operation of a mechanism. You can close the current file without saving changes and continue to explore the use of positional representations in subassemblies. Follow these steps to discover the tools used for handling positional representations in subassemblies:

1.  On the Get Started tab, click Open and then select the file mi_08a_024.iam from the Chapter 8 folder of the Mastering Inventor 2015 directory.

2.  Expand the Representations folder for the top-level assembly (located at the top of the browser tree).

3.  Right-click Position and choose New to create a new positional representation.

4.  Expand the Position node, if needed, and notice that a positional representation called Position1 has been created and is currently active, as denoted by the check mark.

5.  Select Position1; then click it and rename it Range of Travel.

6.  Expand the component called CNC Hobby Router and then expand the Representations folder for this subassembly.

7.  Expand the Position node to reveal the positional representations already created in this subassembly.

8.  Right-click the Set To Range positional representation and choose Activate.

At this point, you have created a positional representation for the top-level assembly and then set that positional representation to use the Set To Range positional representation in the subassembly.

9.  Click and drag the router assembly and notice that the parts will not move. To fix this, you need to set the subassembly to be flexible within the positional representation.

10.Right-click the CNC Hobby Router (either in the browser or in the graphics area) and choose Override from the context menu. In the Override Object dialog box, you will notice that Set To Range is the active positional representation as defined previously.

11.Click the Flexible Status check box and set the drop-down box to Flexible; then click the OK button.

12.Click and drag the router assembly and notice that the parts will now move according to the Set To Range positional representation that is defined in the subassembly.

Once you've explored the nested positional representations, you can close this file without saving changes. Positional representations also allow the reuse of identical subassemblies within a top-level assembly file. By using positional representations in conjunction with flexible assemblies, you can demonstrate a subassembly in different positions. Figure 8.61 shows an assembly containing multiple instances of a cylinder subassembly, each at a different extension length. This model could be created by setting up positional representations in the cylinder subassembly defining each extension value or by leaving the cylinder subassembly underconstrained and then setting each subassembly to be flexible.

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Figure 8.61 Multiple instances of a cylinder subassembly

To help manage positional representations, you can set up the browser to display only the overrides present in each positional representation, as shown in Figure 8.62. The buttons along the top of the Representations browser allow you to create a new positional representation, validate the overrides to ensure that no errors are created in the representations, and manage the overrides via Microsoft Excel.

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Figure 8.62 The Representations browser

Because the positional representation properties of an assembly are stored separately, multiple views can be created in the drawing environment, representing different positions of the same assembly. Figure 8.63 shows an example of an overlay view showing both available positions of a bucket assembly on a front loader.

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Figure 8.63 Overlay view of a positional representation

Level of Detail Representations

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Proper use of level of detail (LOD) improves speed and reduces the memory required to load and navigate large assemblies. When working with a large assembly, you suppress components that are not required for a certain aspect of working with the design and then save that suppression state as a level-of-detail representation. For instance, if you are designing a large material-handling unit, you might open the unit in the LOD representation with everything suppressed except the frame while you work on the frame skins, thereby significantly reducing the number of parts loaded into memory.

Suppression vs. Visibility

It is a common misconception that making components invisible reduces the overhead of your assemblies. When a component's visibility is toggled off, it is still loaded into memory. To unload it from memory, you must utilize LOD reps. If you work with large assemblies, you can set All Components Suppressed as the default LOD. The assembly will open more quickly, and then you can select a previously defined LOD or unsuppress just the parts you want to work with. This method consumes less RAM than opening the complete assembly and then suppressing components.

Another common example of LOD representations might be to suppress external components while working on internal components simply for convenience. In addition to this standard method of suppressing components to create LOD, you can employ substitute LOD representations to trade out a large multipart assembly with a single part derived from that assembly.

Just as view and positional representations have master representations, so does the LOD. However, there are three additional default LOD representations: All Components Suppressed, All Parts Suppressed, and All Content Center Suppressed. These system-defined LODs cannot be removed or modified.

1.  All Components Suppressed Suppresses everything within the assembly, allowing you to quickly open the assembly and then unsuppress components as required.

2.  All Parts Suppressed Suppresses all parts at all levels of the assembly; however, subassemblies are loaded, allowing you to examine the assembly structure without loading all the part files.

3.  All Content Center Suppressed Suppresses any component in the assembly that is stored in the Content Center Files directory as designated by the IPJ (project) file.

Although Chapter 9, “Large Assembly Strategies,” covers the specific steps to create LODs, here are the general procedures.

To create a user-defined LOD, follow these steps:

1.  Expand the Representations heading in the browser, right-click the Level Of Detail heading, and then choose New Level Of Detail.

2.  Continue by right-clicking the component or components you want to suppress and choosing Suppress from the menu.

3.  Once this is done, you must save the assembly while still in the LOD.

4.  After saving the assembly, you can create more LOD representations or flip from one to another to compare the results.

To create a substitute LOD, you start by expanding the Representations heading in the browser, right-click the Level Of Detail heading, and then choose New Substitute. There are two methods for creating substitutes. The first method simply prompts you to select any existing part file to swap out for the assembly file in the LOD, and the second creates a derived part from the source assembly. When using the Derive Assembly method, you are asked to specify a part template to use and then are brought right into the derive assembly process. The derived part is automatically marked as a substitute during the derive process and placed into the LOD.

On the left, Figure 8.64 shows an assembly in its master LOD with 302 component occurrences in the assembly and 77 unique files open in the Inventor session, denoted by the numbers at the bottom of the image. On the right, the same assembly is set to a substitute LOD and reduced to a single component in the assembly, and only two unique files open in the Inventor session. As you can imagine, you can achieve a significant savings in memory by placing an assembly with a substitute LOD active into a top-level assembly.

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Figure 8.64 Substitute LOD representation

It is important to understand that substitute LODs are intended to be used either by excluding components during the derive process or in combination with user-defined LODs to exclude components. Simply making a substitute LOD of an assembly with all components included may not give you the performance gain you anticipated unless you have made the substitute from another LOD that has parts suppressed or you have excluded parts while creating the substitute LOD.

LOD states are created automatically when you suppress components while in the master LOD. To save suppressions to a new LOD representation, click Save, and you will be prompted to click Yes or No to save the LOD. If you choose Yes, you can specify a name for the LOD. If you choose No, the suppression states of the component are discarded, and the assembly is saved in the master LOD.

Temporary LOD representations are created in subassemblies when a subassembly component is suppressed from a top-level assembly. A tilde and index number are listed after the subassembly name to denote a temporary LOD state. Note that the subassembly is not modified. You can open the subassembly on its own and save the suppression states as a named LOD if desired.

It is important to understand the difference between LOD representations and iAssembly configurations with respect to how they affect the bill of materials. Although you can suppress features at will and substitute part files for assemblies with the use of LOD representations, Inventor still understands that all the parts in the master LOD will be included in the bill of materials. When you suppress a component in an LOD representation used in a drawing view, the view updates and any balloons attached to that component are deleted. However, the parts list will still list the component because it always refers to the master bill of materials.

If your intent is to create an assembly configuration where some parts are to be listed in the bill of materials and others excluded, an iAssembly is the correct tool.

LODs and Parts Lists

New Inventor users often attempt to use LODs to create a parts list in the drawing environment that shows only the unsuppressed components. However, this is not allowed outright. To use an existing LOD for parts-list purposes, you should right-click it in the browser and choose Copy To View Rep. Once the View Rep is created, it can be used in the parts list by editing the parts list, clicking the Filter Settings button in the Parts List edit dialog box, and then selecting Assembly View Representation from the list.

Using iAssemblies

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An iAssembly is a table-driven assembly file that allows the use of component part configurations to build variations of a design. Some of the strengths of assembly configurations of this type are the abilities to swap out one component for another, to include or exclude components altogether, and to adjust assembly constraint offset values to create various configurations of the original assembly.

It is important to understand that when you create an iAssembly, you create what is called an iAssembly factory. The configurations that will be output from this factory are called the iAssembly members. It may help to think of the factory as the parent file and the members as children.

To create an iAssembly, most often you start with an assembly composed of iParts. First, the iParts are created for all parts that will vary in size or configuration of features. Next, create the assembly using iPart members where required. Once the basic assembly is created, you add the configuration table, turning the assembly into an iAssembly.

The assembly used in the next exercise represents a simplified push-button panel. Your goal is to create an assembly configuration with variations in the number and type of buttons used, as shown in Figure 8.65.

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Figure 8.65 Configurations of a push-button panel

Follow these steps:

1.  On the Get Started tab, click Open.

2.  Browse to Chapter 8 in the Mastering Inventor 2015 directory and open mi_08a_025.iam.

3.  Switch to the Manage tab and click Create iAssembly on the Author panel. This will open the iAssembly Author dialog box, shown in Figure 8.66.

4.  The first thing you should do is consider the naming conventions for the iAssembly members. Click the Options button at the bottom of the dialog box to bring up the naming options. Here, you would typically configure the name for the member part number and the member names so that as you add rows to the iAssembly table, the naming drops out automatically. In this case, you will simply click the OK button to choose the defaults.

Either column can be set to be the filename column from which member part numbers are generated. You can do so by right-clicking the Member or Part Number column headers and choosing File Name Column from the menu. The filename column is indicated by the save or disk symbol.

5.  Examine the Components tab and expand the tree next to the part called cover_plate_08:1. In the tree of each part are four different nodes that you can use to add a column to the table. Select Table Replace from the tree and use the button to add it as a column in the table.

6.  Now that you have added a column to the table, you will add a row. Right-click anywhere on row 1 in the lower pane of the dialog box and choose Insert Row. Your table should now resemble Figure 8.67.

The Table Replace column allows you to replace an iPart member for another iPart member within the assembly. In this case, the part named CP_001-03 is the sheet-metal cover plate. This plate is an iPart that has four different sizes within the iPart table.

7.  Click the cell in row 2 in the cover_plate_08:1 Table Replace column to activate a drop-down menu.

8.  Click the arrow for the drop-down menu, as shown in Figure 8.67. Then select CP_001-04 and click the OK button to exit the dialog box.

9.  Examine the Model browser, and you will notice that a table has been added to the browser. Expand the table, and you will find a listing of the iAssembly members, mi_08a_025-01 and mi_08a_025-02.

10.mi_08a_025-01 will have a check mark next to it, informing you that this is the active member of the iAssembly. To set mi_08a_025-02 as active, right-click it and choose Activate, or simply double-click it.

Working with iAssemblies

Many iAssemblies require only a few size variables and a few components that can be interchanged. Although in the exercise using iAssemblies both the plate and buttons are iParts, often an iAssembly requires only a few components to be iParts for configuration.

It is typically best to tackle iAssemblies in a structured manner, configuring only one part of the table at a time and then returning to the model to test that change. Making many changes in the table at once may make it difficult to determine how changes affect the model.

Once a couple of rows are added using the iAssembly Author interface, you can edit the table with Microsoft Excel to add many rows at once and quickly make changes to the column entries. Also in Excel, you can create formulas to concatenate column entries, calculate entries, or use if/thens to determine entries.

11.Now that you have used a different-sized plate, you will need to add another button to the assembly. To do so, select the existing black button and use Copy and Paste to add a new instance to the assembly.

12.Place an Insert constraint between the new instance of the button and the empty hole on the plate, as shown in Figure 8.68.

13.Once the new button is constrained, set mi_08a_025-01 to be active again in the table tree, and notice that you are presented with an error message warning you that the new constraint is looking at geometry that is no longer present. Click Accept in the error dialog box.

Notice that the new button remains even though the hole it was constrained to is gone. To address this, you need to edit the table further and configure the iAssembly to suppress the extra button when not needed.

14.Right-click the Table icon in the Model browser and choose Edit Table.

15.Locate part push_button_08:4 in the tree and use the button to place Include/Exclude in the table as a column.

16.Set the value for this column to be Exclude for row 1, as shown in Figure 8.69. Click the OK button to return to the model, and activate both members to see that no constraint errors occur.

17.Next, you will change out the black buttons in member mi_08a_025-02 to use a second green and a second red button. Edit the table, and choose the last two instances of part push_button_08 from the tree in the top-left pane. Locate the Table Replace parameter for each and use the button to include them in the table.

18.Set the Table Replace values in row 2 to Red and Green, as shown in Figure 8.70.

You do not need to change the values in row 1 because one of the buttons is already set to Black as required and the other, as you recall, you excluded so that it does not show in the row 1 configuration.

19.Click the OK button to exit the table-authoring dialog box and then activate mi_08a_025-02 from the table. Note the changes to the four-button configuration. You should now have two red and two green buttons in an alternating pattern.

20.Last, you will set one of the buttons to be in a different position. Edit the table to return to the iAssembly Author dialog box again and activate the Parameters tab.

21.Expand the Constraints folder, select Insert:1, and use the button to add it as a column in the table.

22.Set the value of this column to 7 mm for row 2 of the configurations.

23.Click the OK button to exit the dialog box, and notice that one of the buttons is now pushed in because you have modified the constraint offset value.

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Figure 8.66 The iAssembly Author dialog box

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Figure 8.67 Configuring an iAssembly table

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Figure 8.68 Adding an Insert constraint

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Figure 8.69 Exclude/include components in an iAssembly

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Figure 8.70 Table Replace in the iAssembly Author dialog box

You can close this assembly file without saving changes. iAssemblies allow you to create configurations of your assemblies by including and excluding components, configuring constraints values, setting iProperties, and much more. When creating drawing files for iAssemblies, you often need a drawing for each member. The members have the same annotations and tables, with only some values differing.

Use Assembly Design Accelerators

The functional-design tools enable you to create complex geometry by entering size data. Before any geometry is created, you can verify whether the design meets the requirements by performing calculations. The formulas used for the calculations are based on international standards, and they are fully documented in the Engineer's Handbook. This allows you to override or ignore certain calculations when experience dictates.

Functional Design vs. Geometric Modeling

Rather than modeling geometry first and then hoping that the form satisfies all the design criteria, in the functional-design method, you use the tools to make sure the design operates correctly given the design criteria prior to finalizing the product's shape. If functional design is done well, the geometry will be the result of the design process rather than the input to it.

Functional Design in the Real World

You might already use functional design every day but might not identify it by that name. Consider the following scenario: You're called on to specify a V-belt for a current pulley system design. You could space the pulleys and then hope to find a belt that fits well, but that wouldn't be typical. Instead, you'd most likely narrow down the general size of the belt needed and determine the load and speed required and then use this information to look up a proper belt size from a supplier catalog, thereby letting the function drive the design and assist you in specifying the belt. You can use design accelerators in Inventor to do the same thing.

Working with Design Accelerators

Design accelerators can be overwhelming at first because of the sheer number of accelerators and because the user interface is slightly different from the rest of Inventor. Therefore, you'll look at the dialog boxes, the browser structure, and the user interface for these tools.

Design Accelerators Input

Design accelerators are available only in the assembly environment. Design accelerator dialog boxes are tabbed dialog boxes, as shown in Figure 8.71. The Design and Calculation tabs appear in most of the dialog boxes. Two particular areas in these dialog boxes are worth pointing out.

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Figure 8.71 A typical design accelerator : dialog box

The Results pane displays the calculated values for a particular design. The Summary pane indicates whether a design is acceptable with the given parameters. These panes are hidden by default and can be displayed by double-clicking the double line on the right and bottom edges of the dialog box or by clicking the button along the borders. The border of the design accelerator window turns red to indicate a design failure or to flag a more general error.

The calculation is not an automatic operation; for example, if a calculation fails and the values turn red, you typically change the parameters to correct the problem. You will not see the result of your change unless you click the Calculate button. Many calculators offer different types of calculations. Choosing a particular calculation method will disable certain fields (driven values) and enable some other fields (input values).

Remember to Calculate (or Not to Calculate)

One common mistake is not clicking the Calculate button. The design accelerators will not update when you simply change values. You must click the Calculate button.

Also keep in mind that you can deselect the Calculate button in order to not calculate the design and just place design accelerator components that might not comply with design inputs. This can often be helpful in the early stages of a design when you just need a form to start with.

Design Accelerators Output

There are two sorts of functional design tools: generators and calculators. It is important to understand the difference between these two categories. The output generated by design generators consists of subassemblies with actual geometry in them. For example, the V-belt generator will generate a belt part. But it can create pulleys as well.

Design calculators don't generate any geometry, but the result of the calculation places a subassembly node in the browser and can be edited and repeated with different values. The dialog box for calculators is also restricted to one tab: the Calculation tab.

Most (but not all) design generators use parts generated from Content Center. Table 8.1 lists the various design accelerators and their dependency on the Content Center library databases.

Table 8.1 Design accelerators' use of Content Center database

Generator/accelerator

Needs Content Center

Bolted Connections

Yes

Weld Calc

No

Tolerance Stack Up Calc

No

Limits and Fits Calc

No

Beam Calc

No (but recognizes section properties of Content Center and Frame Generator parts; see Chapter 15, “Frame Generator”)

Column Calc

No (but recognizes section properties of Content Center and Frame Generator parts; see Chapter 15)

Plate Calc

No

Shaft Generator

No

Cam Generator

No

Gear Generator

No

Bearing Generator

Yes

Key Connection Generator

Yes

Spline Generator

No

Belt Generator

No

Sprocket and Chain Generator

Yes

Spring Generator

Yes (but only for Belleville springs)

Pins Generator

Yes

Seals and O-rings Generator

Yes

Engineer's Handbook

No

Design Accelerator Solve States

Many design accelerators use solve states to control when and how they solve for and update the geometry contained within them. The solve state of the generator subassemblies is indicated by an icon in the browser. Manual Solve is the default mode, but you can change it to Automatic Solve by right-clicking the design accelerator component, selecting Component, and then selecting the solve mode you want to use. Figure 8.72 shows the Automatic Solve icon next to the synchronous belt component.

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Figure 8.72 Synchronous belt in Automatic Solve mode

There are three solve states that can be changed in the Component context menu, as described in Table 8.2.

Table 8.2 Solve states of design accelerator components

State

Explanation

Solve Off

Changes to design accelerator input conditions have no effect on the design accelerator component.

Manual Solve

Changes to design accelerator input conditions have an effect only after editing the design accelerator component.

Automatic Solve

Changes to design accelerator input conditions immediately affect the design accelerator component.

The Solve Off, Manual Solve, and Automatic Solve options are mutually exclusive, meaning that when you select one option, it turns the current one off. The Solve Off menu does exactly what its name suggests: It turns off the solver completely so that the design accelerator component is frozen until the next edit.

The difference between Manual Solve and Automatic Solve is simple. Using the example of a V-belt, when the distance between the axes changes, a V-belt will automatically readjust the pulley positions if Automatic Solve is on. If Manual Solve is on, the user will have to update the pulley positions by clicking the Manual Solve menu. A red lightning bolt will appear in the browser. Manual Solve is used as the default for performance reasons and to prevent interactions with the assembly solver.

The Calculate option on the context menu is a toggle between two states; clicking it once turns it on, and clicking it again turns it off. You can toggle this option by using the Calculate button at the top right of each design accelerator dialog box as well. When calculation is turned off, the performance of the generator is faster.

Because design accelerator assemblies typically consist of multiple parts that are constrained together, Inventor offers specific edit, delete, promote, and demote tools for design accelerator entities.

Using Default Values

The values used in the last calculation of a design accelerator component will be reused when you create a new design accelerator component with the same generator. If you want to use the default values of a design accelerator, hold down the Ctrl key when starting the design accelerator tool.

Bolted Connection Generator

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This generator is the most popular design accelerator tool because it is able to make an entire set of bolts, washers, nuts, and the necessary holes in the supporting geometry as an all-in-one operation. Figure 8.73 shows placement options for the Bolted Connections tool; you might notice the similarity between these options and the Hole tool placement options.

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Figure 8.73 Placement options in a bolted connection

There are four placement options:

1.  Linear Allows the creation of a bolted connection without any preexisting sketch by selecting a distance to two different linear edges

2.  Concentric Uses any circular edge (the edge does not have to be part of a hole feature; the edge can be part of a cylindrical extrusion) to make a bolted connection with a larger or smaller hole size

3.  On Point Requires an existing work point or vertex as input

4.  By Hole Requires an existing hole, and the bolted connection will incorporate the existing hole

Although the Bolted Connections tool will create holes for you, it is often best to create the holes first with the regular Hole tool and then use the By Hole option rather than using the Linear or Concentric option. The disadvantage of the latter two options is that they create only a point in a sketch, but the point is not dimensioned and could easily move. When the sketch point moves, the bolted connection will not follow the new position of the hole.

When you use By Hole, the bolted connection will automatically follow any positional change of the preexisting holes but will not follow diameter changes automatically. Keeping the diameter of the holes generated by the bolted connection in sync with the diameter changes in the preexisting hole requires manually selecting a different diameter in the Diameter field of the bolted connection. The reason this was done is to give you a choice because you don't necessarily want all your bolts to increase in diameter when the underlying hole diameter increases.

Placing a Bolted Connection Pattern

In the following example, you will connect the cap with the plate using bolted connections. The cap has three holes drilled in it, and they form a circular pattern.

1.  On the Get Started tab, click Open and browse to mi_08a_027.iam in the Chapter 8 folder of the Mastering Inventor 2015 folder.

2.  Select the Design tab and then click the Bolted Connection button.

3.  In the Placement area, confirm that By Hole is selected in the drop-down list.

4.  Select the top face of the cap as the start plane.

5.  Select one of the holes. Since there is a hole pattern, the preview will display at the original instance of the hole no matter which hole you select. Note too that the Follow Pattern option is displayed in the Bolted Connection dialog box. Check the box so that all the holes will get fasteners.

6.  Click the Termination button and select the back side of the plate. The Bolted Connections generator is smart enough to know which side of the plate is valid for termination. When you hover over the plate, the back side highlights and you can click to accept.

7.  In the Thread area, set the diameter to 8 mm to match the holes in the cap. In Figure 8.74, you can see that holes have been added to the dialog browser pane.

Note that there are three drilled holes automatically added to the plate. You could click the Drilled Hole bar in the right pane and then click the down arrow to select a different hole type (for example, counterbore). The Bolted Connections generator is clever enough to filter out countersink hole types for holes on faces that are not exposed.

At this point, you can add all necessary hardware to finish the connection. It is important to note that the order of the icons in the pane on the right represents the stacking order of the bolted connection beginning from the start plane and moving down. If you want to place a bolt on the start plane, you just click the area marked with Click To Add A Fastener.

8.  Click the area marked Click To Add A Fastener above the holes.

9.  In the resulting selection window, set Standard to DIN and Category to Socket Head Bolts.

10.Select DIN 404 (or something comparable).

The bolt is automatically sized to be long enough to go through the selected components, if the bolt type library selected has a length that is long enough. If you want to change the bolt length, you can drag the preview arrow at the end. Only valid lengths from Content Center can be selected.

11.To finish the bolted connection by adding a nut and washer, click the area marked Click To Add A Fastener below the holes and select a washer.

12.Click the lower Click To Add A Fastener bar again and select a nut.

At this point, you might realize that you want to add a washer between the bolt head and the top face of the cap part.

13.Click the Click To Add A Fastener bar below the bolt and choose a washer.

14.Click Apply to create the patterned bolted connection.

image

Figure 8.74 Following the holes of an existing pattern

You can continue experimenting with the bolted connection tool or close the file and continue to the next section.

Creating a Threaded Hole in the Plate

If you wanted to thread the plate to avoid adding a nut and washer, you could do so by clicking ISO Drilled Hole section of the pane and then clicking the button with the three small dots. Doing so would bring up the Hole options, allowing you to change the hole type to threaded.

Calculating the Bolt Strength

Next, you'll edit a bolted connection and calculate its strength. The design problem you are trying to solve is as follows: Considering an axial force of 750 N and a tangential force of 300 N, will three bolts be sufficient to hold the cap on the plate?

1.  On the Get Started tab, click Open and browse to mi_08a_028.iam in the Chapter 8 folder of the Mastering Inventor 2015 folder.

2.  Locate the existing Bolted Connection in the Model browser and then right-click it and choose Edit Using Design Accelerator. Note you may need to expand Component Pattern 2 and then expand Element:1 to find the Bolted Connection node.

3.  In the Bolted Connection Component Generator dialog box, click the Calculation tab.

The Calculation tab provides four strength calculation options:

·     Bolt Diameter Design

·     Number Of Bolts Design

·     Bolt Material Design

·     Check Calculation

Do you meet the design criteria with just three bolts? It all depends on the material you choose for the bolts.

4.  Set the Type Of Strength Calculation drop-down to Number Of Bolts Design.

5.  In the Loads area, enter 750 N for Maximal Axial Force and 300 N for Maximal Tangent Force.

6.  Assume that this application requires fasteners with high thermal conductivity. In the Bolt Material area, check the box next to the material field and select Copper-Nickel C96200. To narrow down the material choices, type Copper in the text field below the Material column header. Note that the text filter name is case-sensitive.

7.  Click Calculate to analyze the fasteners.

In the Bolts section, you will see that the Number Of Bolts (z) is now calculated at 4 (recall that ul means unitless in Inventor).

8.  Click the OK button to close the Bolted Connection Component Generator dialog box.

To comply with the calculation, you need to edit the cap and update the hole pattern from three to four. Once you've done so, the bolted connection pattern will follow accordingly if the Automatic Solve option is enabled.

9.  Right-click the existing Bolted Connection in the Model browser and then select Automatic Solve from the list.

10.Right-click the component named mi_08a_028_Cap in the browser and choose Edit. This will set the cap active for edits.

11.Locate the feature called Circular Pattern 1 in the browser; right-click it and choose Edit Feature. This pattern controls the number of holes.

12.Change the Placement value from 3 to 4; then click the OK button.

13.To return to the assembly, click the Return button on the Ribbon menu or right-click and choose Finish Edit.

As a result of the changes you've made to the number of bolt holes, the bolted connection pattern has updated as well. Although all of the design accelerators are slightly different, they all share a common way of solving problems and creating components. Autodesk provides tutorials covering each of the design accelerators on the Autodesk Inventor wiki:

http://wikihelp.autodesk.com/Inventor

The Bottom Line

1.  Create assembly relationships using the Constraint and Joint tools. Assembly relationships are an important part of working with Inventor assembly files. Assembly constraints determine how assembly components fit together. As relationships are applied between components, degrees of freedom are removed.

1.  Master It You are new to 3D and find the concept of assembly relationships a bit challenging. Where can you find a simple overview of constraints?

2.  Organize designs using structured subassemblies. Subassemblies add organization, facilitate the bill of materials, and reduce assembly relationships; all this results in better performance and easier edits. One of the habits of all Inventor experts is their effective use and understanding of subassemblies.

1.  Master It You need to hand off an accurate BOM for finished designs to the purchasing department at the end of each design project. How can the BOM be extracted from Inventor?

3.  Work with adaptive components. Geometry can be set to be adaptive so that it can be sized and positioned in the context of where it is used in the assembly. You can set underconstrained geometry to be adaptive by specifying the elements allowed to adapt.

1.  Master It You want to set a feature of a part to be adaptive so that it can adapt to another part in an assembly. However, the feature is based on a fully constrained sketch. How would this be done?

4.  Create assembly-level features. An assembly feature is a feature created and utilized within the active assembly file. Because the feature is created within the assembly file, it does not exist at the single-part or subassembly level.

1.  Master It You want to make a notch in a standard part that will not affect its use in every other assembly it is used in. Can this be done?

5.  Manage bills of materials. Managing a bill of materials can be a large part of any assembly design task. Understanding the BOM structure goes a long way toward successfully configuring your bill of materials.

1.  Master It You need to mark a component as a reference component in just one assembly file. However, when you attempt to do so using the BOM Editor, it is designated as a reference in every assembly. How can you set just a single instance of a component to be a reference component?

6.  Use positional reps and flexible assemblies together. Often, you may need to show a design in various stages of motion to test interference and/or proof of concept. Copying assemblies so that you can change the assembly relationships to show different assembly positions can become a file management nightmare. Instead, use flexible subassemblies and positional representations.

1.  Master It You need to show your assembly in variations dependent on the position of the moving parts and the task the machine is accomplishing at given stages of its operation. How do you do this?

7.  Copy assembly designs for reuse and configuration. Because of the live linked data that exists in Inventor assemblies, using Windows Explorer to copy designs and rename parts is difficult and often delivers poor results. Using the tool provided in Inventor will allow you to copy designs and maintain the links between files.

1.  Master It How do you duplicate an existing design to create a similar design?

8.  Substitute a single part for entire subassemblies. Working with large assemblies, particularly where large, complex assemblies are used over and over as subassemblies within a top-level design, can tax almost any workstation if not approached in the correct manner.

1.  Master It You would like to swap out a complex assembly for a simplified version for use in layout designs or to use in large assemblies in an attempt to improve performance. What is the best way to do that?

9.  Work with assembly design accelerators and generators. Design accelerators and generators allow you to rapidly create complex geometry and the associated calculations that verify the viability of your design.

1.  Master It Your design needs a bolted connection, but you are not certain about the number of bolts to use to ensure a proper connection. How do you determine this?

10.Use design calculators. Design calculators do not create any geometry, but they permit you to store the calculations in the assembly and repeat the calculation with different input values at a later time.

1.  Master It You need to calculate the size of a weld between two plates to withstand a certain lateral force. What tool do you use?