Advanced Modeling Techniques - Mastering Autodesk Inventor 2015 and Autodesk Inventor LT 2015 (2014)

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

Chapter 5. Advanced Modeling Techniques

Chapter 4, “Basic Modeling Techniques,” introduced some of the primary modeling tools you need when creating a 3D parametric part. Modern parametric modeling utilizes numerous tools to create stable, editable parts. The basic workflow of creating a part is to create a base feature and then build upon that base. The tools used to build the additional features can vary depending on your need and may range from simple extruded features to complex combinations of different feature types.

In this chapter, you will explore some of the more complex and curvy modeling techniques used to create models with the Autodesk® Inventor® and Autodesk® Inventor LT programs. Some of these features involve creating a base profile sketch along with support sketches used for defining paths and shape contours. Such features are based on the same rules used to create simpler features, such as extrudes and revolves, but they take it to the next level by using multiple sketches to define the feature. Other advanced features covered in this chapter depart from these concepts and move into the new territory of feature creation. In either case, having a strong understanding of sketch-creation and editing principles is assumed and recommended.

All the skills in this chapter are primarily based on creating a single part, whether in a part file or in the context of an assembly file.

In this chapter, you'll learn to

· Create complex sweeps and lofts

· Work with multi-body and derived parts

· Utilize part tolerances

· Understand and use parameters and iProperties

· Troubleshoot modeling failures

Creating Complex Sweeps and Lofts

Now that you have moved on from creating simple features, you can explore the use of sweeps and lofts to create features with a bit more complexity. Both sweeps and lofts require one or more profiles to create a flowing shape. Sweeps require one sketch profile and a second sketched sweep path to create 3D geometry. Lofts typically require two or more sketch profiles and optional rails and/or points that assist in controlling the final geometry.

Creating and Using Sweeps

You can think of a sweep feature as an extrusion that follows a path defined by another sketch. 2D or 3D sketch paths can be used to create the sweep feature. Like most Inventor geometry, a sweep can be created as either a solid or a surface. Sweeps can add or remove material from a part, or you can use the Intersect option like you can with the Extrusion tool. If your intent is to create multi-body parts, you can choose the New Solids option also.

Creating 2D Paths

When creating a sweep feature, you will typically want to first create the path sketch and then create a profile sketch that will contain the geometry to be swept along the path. To create the profile sketch, you will need to create a work plane at the end of your path. This plane will be referenced to create a new sketch. It's not mandatory that you create the path and then the profile, but it is easier to define the profile sketch plane (that is, a work plane) by doing it this way. Normally, this geometry will be perpendicular to one end of the sweep path.

A basic rule of sweep features is that the volume occupied by the sweep profile may not intersect itself within the feature. Some self-intersecting features are currently supported, but many will fail. An example of a self-intersecting feature is a sweep path composed of straight-line segments with tight radius arcs between the segments. Assuming that the sweep profile is circular with a radius value larger than the smallest arc within the sweep path, the feature will self-intersect and the operation will fail. For a sweep to work, the minimum path radius must be larger than the profile radius. In the 2D sketch path example shown in Figure 5.1, the path radius is set at 12 mm. Knowing that the minimum path radius value is 12 mm, you can determine that the sketch profile radius must be less than or equal to this value.


Figure 5.1 2D sketch path

Creating the Sweep Profile

Once a sketch path has been created, you can create a work plane on the path and then sketch the profile on that plane. To see this process in action, follow these steps, starting with the creation of the path:

1. On the Get Started tab, click the New button.

2. On the Metric node of the New File dialog box, select the Standard(mm).ipt template.

3. Create a 2D sketch as shown in Figure 5.1.

4. Once you've created the sketch path, right-click and choose Finish 2D Sketch; then click the Plane button on the 3D Model tab to create a work plane.

5. Select the endpoint of the 2D sketch path and then the path itself to create the plane. This creates a plane on the point normal to the selected line. Figure 5.2 shows the created work plane.

6. Once you've created the work plane, right-click the edge of it and select New Sketch.

7. In the new sketch, use the Project Geometry tool to project the 230 mm line into this new sketch. It should come in as a projected point.

8. Create a circle anchored to the projected point, give it a value of 20 mm in diameter, and then click the Finish Sketch button.

9. Select the Sweep tool. If you have a single sweep profile, it should automatically select the profile and pause for you to select a path.

10.Select a line in the path sketch to set it as the path.

Note that you can select either Solid or Surface for the feature. The sweep type will default to Path, and the orientation will default to Path as well. The Sweep tool also has an option to taper the sweep feature, as shown in Figure 5.3.

A number less than zero for the taper will diminish the cross section as the profile follows the path. A positive number will increase the cross section. If the taper increases the cross section at the radius of the path to a value that exceeds the radius value, the feature will fail because this will create a self-intersecting path.

11.Adjust the taper to a negative value to see the preview update. Note that if you enter a positive value that's 0.5 or more, the preview will fail, indicating a self-intersecting path. Set the taper back to 0, and click the OK button to create the sweep.


Figure 5.2 Creating a work plane on which to sketch


Figure 5.3 Sweep dialog box options

You'll notice that this sweep feature consumes both sketches in the browser, just as an extruded feature consumes the sketch it is created from. To edit the sweep, you can expand the browser node by clicking the plus sign and access both the profile and path sketches to make edits. You can also right-click the sweep feature node and choose Edit Feature to change the options in the Sweep dialog. Explore the ways to edit the sweep you just created, and then you can close the file without saving changes. In the next section you will look at more sweep options.

Exploring Sweep Options

Although sweeping along a path is the default option, you can also utilize the Path & Guide Rail or Path & Guide Surface option to control the output of the Sweep tool. These options provide additional control for more complex results. Often these options are utilized on sweeps based on a 3D sketch path, but this is not required. You can create a 3D sketch path by using the Include Geometry tool, or you can just use the existing geometry edges where valid selections exist.

Path & Guide Rail Option

The Path & Guide Rail option provides a means to control the orientation of a profile as it is swept along a path. In Figure 5.4, the rectangular sweep profile will be swept along the straight path but controlled by the 3D helical rail. This approach is useful for creating twisted or helical parts.


Figure 5.4 Sweep profile, Path & Guide Rail option

The 3D helical rail is guiding the rotation of the profile even though the sweep profile is fully constrained with horizontal and vertical constraints. Creating this part starts with creating the sweep path as the first sketch followed by creating a second sketch perpendicular to the start point of the sweep path. The 3D helical rail is created using the Helical Curve tool in a 3D sketch. Follow these steps:

1. Open the file mi_5a_004.ipt from the Chapter 5 directory of your Mastering Inventor 2015 folder. If you have not already downloaded the Chapter 5 files from www, please refer to the “What You Will Need” section of the introduction for the download and setup instructions.

2. Click the Sweep button on the 3D Model tab.

3. Change the Type drop-down to Path & Guide Rail, choose the straight line as the path and the helix as the guide rail, and then click the OK button. Your result should resemble Figure 5.5.


Figure 5.5 Sweep feature with Path & Guide Rail option

Using guide rails to control the path and further define the shape of the sweep greatly expands the range of shapes you can create with the Sweep tool. You can close the current file without saving changes and take a look at the use of the Twist option in the next section.

Path & Twist Option

In this exercise, you'll use the Twist option to provide the helical twisting of the sweep feature:

1. Open the file mi_5a_005.ipt from the Chapter 5 directory of your Mastering Inventor 2015 folder.

2. Click the Sweep button on the 3D Model tab. Note that because there is only one profile and one path, the Sweep tool automatically selects them for the Profile and Path selections.

3. Enter 90 in the Twist input box and note the preview.

4. Change the Twist input to 360 in the Twist input box and note the new preview.

5. Next, change the Twist input to -360 and again note how the preview changes.

6. Lastly, change the Twist input to -360*3 and again take note of the change to the preview.

7. Click the OK button to create the twisted sweep.

Using the twist option, you're able to quickly create twisted, swept features without the use of a guide rail sketch. Feel free to experiment with the twist option using this file, and then you can close it without saving changes and take a look at the use of a guide surface in the next section.

Path & Guide Surface Option

At times you will need to sweep a profile that will conform to a specific shape and contour. This is often necessary when working with complex surfaces, particularly when cutting a path along such a surface. In the following exercise, you will use some surface tools to manipulate a solid shape while exploring the sweep guide's Surface option:

1. On the Get Started tab, click Open; open the file mi_5a_006.ipt from your Chapter 5 folder.

2. Click the small arrow on the Surface panel of the 3D Model tab to see the Replace Face tool. Figure 5.6 shows the Surface panel expanded.

3. Click the Replace Face tool, select the red face as the existing face, select the wavy surface for the new face, and click the OK button.

4. Right-click ExtrusionSrf1 in the browser and select Visibility to turn it off.

5. Click the Plane button on the 3D Model tab, click and hold down on the yellow surface, and then drag up to create an offset work plane at 85 mm.

6. Right-click the edge of the work plane and choose New Sketch.

7. Using the Project Geometry tool, select the wavy face. This will result in a projected rectangle in your sketch.

8. Create a circle with the center point at the midpoint of the projected rectangle and the tangent point on the corner of the rectangle so that your results look like the image onthe left of Figure 5.7. Click the Finish Sketch button to exit the sketch.

9. Click the Start 3D Sketch button on the Sketch panel, or right-click in the empty space of the graphics window and choose New 3D Sketch from the context menu.

10.Click the Intersection Curve tool from the 3D Sketch tab and choose the circle and the wavy face. Finish the 3D sketch and turn off the visibility of the 2D sketch and the work plane. The result will be a curve, as shown on the right of Figure 5.7.

11.Create a 2D sketch on the front face, as shown in Figure 5.8. Be sure to select the projected edges and make them construction lines so that Inventor won't pick up the entire front face as a sweep profile. The top two corners will be coincident to the curved construction line along the top. When the sketch is fully constrained and completed, as shown in Figure 5.8, click Finish Sketch.

12.Select the Sweep tool and choose the profile you just sketched for the profile input.

13.Select the 3D intersection curve for the path.

14.Click the Cut button to ensure that this sweep removes material from the part and click the OK button.

15.The resulting cut sweep will be too shallow in some places, as shown on the left of Figure 5.9.

16.Edit the sweep, and set the Type drop-down to Path & Guide Surface. Select the wavy surface as the guide surface and then click the OK button. The result will look like the image on the right of Figure 5.9.


Figure 5.6 Surface tools


Figure 5.7 Creating a sweep path


Figure 5.8 Creating a sweep profile


Figure 5.9 Path vs. Path & Guide Surface

Using a guide surface to match the exact curvature of a complex shape is often the only way to achieve the type of features found on plastic parts and other consumer products of stylized form. You can close this file without saving changes and move on to the next section to explore lofted features.

Sweep along an Edge

It's often useful to sweep a profile along an existing edge or edges in order to create a complex sweep shape. In the past you might have been required to create a 3D sketch beforehand and use the Include Geometry option. But you can now just use the edges for the sweep path, and Inventor will create the 3D sketch and included geometry for you, as demonstrated in the following steps:

1. On the Get Started tab, click Open; open the file mi_5a_007.ipt from your Chapter 5 folder.

2. Click the Sweep button on the 3D Model tab.

3. The profile should be selected automatically since there is just one sketch to use. Select the outer edge of the part for the sweep path.

4. Click the OK button to create the sketch.

5. Expand the sweep feature in the browser and notice the presence of the automatically created 3D sketch.

As you can see, setting up a part file to use the edges for a sweep path can provide a quick and powerful way to create otherwise difficult features. You can close this file without saving changes and continue on to explore loft features.

Creating Loft Features

Whereas a sweep allows the creation of single profile extruded along a path, loft features allow the creation of multiple cross-sectional profiles that are used to create a lofted shape. The Loft tool requires two or more profile sections to function. Rails and control points are additional options that help control the shape of a loft feature. A good example of a lofted shape is a boat hull.

Loft with Rails

You could create a boat hull by defining just the section profiles, but you can gain more control over the end result by creating a loft with rails. Figure 5.10 shows the completed wireframe geometry to create a section of a boat hull. The geometry includes four section sketches, each composed of a 2D spline sketched onto a work plane. There are two rails: the top and bottom composed of 3D sketch splines.


Figure 5.10 Loft with rails geometry

Follow these steps to explore the creation of a loft feature with the use of rails:

1. On the Get Started tab, click Open; open the file mi_5a_008.ipt found in your Chapter 5 folder.

2. Select the Loft tool from the 3D Model tab (note that you might need to click the flyout arrow under the Sweep button to find the Loft button).

3. Since the four section sketches are open profiles, the Loft tool will automatically set the output to Surface. Select the four cross-section sketches in consecutive order, front to back or back to front.

4. Click the Click To Add button in the Rails section of the dialog box and select 3D sketches named Rail1 and Rail2.

5. If you have the Preview option selected at the bottom of the dialog box, you should see a preview of the surface indicating the general shape, as shown in Figure 5.11. Click the OK button, and the surface will be created.


Figure 5.11 A surface loft with rails

Patch and Stitch Surfaces

That concludes the lofting part of the boat hull, but if you'd like, you can continue with the following steps to learn a bit more about working with surfaces:

1. To finish the hull, select the Mirror tool on the Pattern panel of the 3D Model tab.

2. Select the hull surface for the Features selection and then click the Mirror Plane button.

3. Expand the Origin folder in the browser, click YZ to use it as the mirror plane, and click the OK button.

4. Next, you will create a 3D sketch to create a line for the top edge of the transom (back of the boat); right-click in the graphics window and choose New 3D Sketch.

5. On the 3D Sketch tab, click the Line tool and draw a line across the back of the boat to form the top of the transom. Draw another line across the bottom of the transom where the two sides do not quite meet. Figure 5.12 shows the back of the boat with the 3D sketch lines.

6. Click Finish Sketch when the lines are drawn.

Turning Off the Translucency of Surfaces and Shadows to See Better

If you have difficulty seeing the endpoints when attempting to draw the 3D Sketch line, you can expand the mirror feature in the browser, locate the loft surfaces, and then right-click and deselect Translucent.

It might also help to go to the View tab and deselect all of the shadows options.

7. Select the Patch button on the Surface panel of the 3D Model tab to bring up the Boundary Patch tool and ensure the Automatic Edge Chain option is not selected. Then select your 3D sketch lines and the back curved edges to create a surface for the transom. When creating boundaries, you need to select the lines in the order in which they occur in the boundary. Click the Apply button and then create another boundary patch across the top by selecting the two edges of the sides and the top edge of the transom. Figure 5.13 shows the selections.

8. You'll notice the gap in the base of the hull. Use the Boundary Patch tool to create a surface by clicking both edges of the gap and the small edge at the bottom of the transom.

9. Select the Stitch tool on the Surface panel and select all five of the surfaces you created. It's easiest to window-select them all at once.

10.Click the Apply button and then the Done button.


Figure 5.12 3D sketch lines for the transom


Figure 5.13 Boundary patch selections

Using the Shell Tool

You should now have a solid boat. If you didn't complete the previous exercise, you can open the file mi_5a_009.ipt to explore the Shell tool. If you're continuing with the boat you created from the loft exercise, be sure to save your file. This is just good practice before running calculation-intensive operations like the Shell tool, particularly on free-form shapes like this boat hull. Once you've saved your file or opened the one provided, follow these steps to explore the Shell tool:

1. Once your file has been saved, select the Shell tool on the Modify panel of the 3D Model tab.

2. Click the top face for the Remove Faces selection and set Thickness to 10 mm.

If your system is a bit undersized, you might want to skip the next two steps and click the OK button now to let the shell solve for just one thickness. Otherwise, you'll specify a unique thickness for the transom.

3. Click the button to reveal the Unique Face Thickness settings, click the Click To Add row, and then click the transom face.

4. Set the unique face thickness value to 30 mm and click the OK button to build the shell. Figure 5.14 shows the completed boat.


Figure 5.14 The completed boat

Although at this point you have gone far past the initial lofted surface to finish the boat model, you started by creating a loft from the 2D sketch profiles and then used the 3D sketches as rails to further define the shape. Of course, if you are a boat designer, you might see a few areas of the design that need improvement. But, for now, you can close the file without saving changes and move on to explore the area loft options in the next section.

Area Loft

Area loft is used in the design of components where the flow of a gas or liquid must be precisely controlled. Area loft is a different way of controlling the finer points of creating a loft shape. Figure 5.15 illustrates what might be considered a fairly typical loft setup, consisting of three section profiles and a centerline. The goal here is to create a loft from these profiles and to create a fourth profile to control the airflow through the resulting part cavity so that it can be choked down or opened up as needed.


Figure 5.15 Area loft profiles

Follow these steps to explore the creation of an area loft:

1. On the Get Started tab, click Open; open the file mi_5a_010.ipt from your Chapter 5 folder.

2. Start the Loft tool and select the three sections in order, starting with the small rectangular shape.

3. Right-click, choose Select Center Line, and then click the centerline sketch line running down the middle of the profile sketches.

4. Right-click again, and choose Placed Sections; notice as you choose an option from the context menu that the dialog box updates to reflect your selections. You could have just as easily used the dialog box controls to do this, but oftentimes it is easier not to create the extra mouse travel.

5. Slide your mouse pointer over the centerline and then click roughly halfway between the circular section and the middle section.

Once you click a location, the Section Dimensions dialog box appears, as shown in Figure 5.16, giving you control over the position and section area of the placed section. You can switch the position input from Proportional Distance, where you enter a percentage of the centerline length, to Absolute, which allows you to enter an actual distance if you know it.

In the Section Size area, you specify the actual area or set a scale factor based on the area of the loft as calculated from the sections before and after the one you are creating. On the far left, you can switch the section from driving to driven, letting the area be calculated from the position. Any number of placed sections can be used to create precise control of the feature.

6. Leave Section Position set to Proportional Distance, change the position to 0.75, set the area to 800 (as shown in Figure 5.16), and click the OK button. You can access the section again by double-clicking the leader information.

7. Double-click the End section leader text and change it from Driven to Driving using the radio buttons on the left. Notice that you can set the area but not the position.

8. Change the area to 800 and then click the OK button in the Section Dimensions dialog box. Then click the OK button in the Loft dialog box to create the lofted solid.


Figure 5.16 Section Dimensions dialog box

Figure 5.17 illustrates the placed loft section and the modified end section.


Figure 5.17 Creating an area loft

You may have noticed that by changing the end section to an area of 800 square millimeters, you altered the size of the end profile from the original shape, in this case slightly reducing the diameter of the circle. Keep this in mind as you create area lofts, and you can use the original sketch to just rough in the shape and not worry as much about getting the size exactly right until you refine the area loft profile. Of course, as always, you should still fully constrain the sketch profile. You can close this file without saving changes and take a look at the centerline loft options in the next section.

Centerline Loft Feature

The centerline loft feature allows you to determine a centerline for the loft profile to follow, just as you did with the area loft. In the following steps, you'll create a wing feature using the centerline loft and look at some of the condition options available in lofted features as well:

1. On the Get Started tab, click Open; open the file mi_5a_012.ipt from your Chapter 5 folder.

2. Click the Loft button and select the yellow face of the wing stub feature and the sketch point at the end of the arc as sections.

3. Right-click, choose Select Center Line, and then click the arc. Notice how the lofted shape now holds the centerline, as shown in Figure 5.18.

4. Click the Conditions tab in the Loft dialog box so you can control the curve weight and transition type at the work point and wing stub profile.

5. Click the drop-down next to the Edges1 (Section) and set it to Tangent. Change the weight to 0.5 to adjust the blend from the wing stub feature.

6. Click the small drop-down to set Point Sketch2 to Tangent and then set the weight to 1.5.

7. Currently, the loft is extending out past the work plane. Often, this can be a problem because the work plane may have been established for the overall length of the part. To resolve this, set the drop-down to Tangent To Plane, and select the work plane on the screen. Notice the adjustment. Figure 5.19 shows the preview of the adjustments before and after the tangent plane is selected.

8. Click the OK button and examine your lofted shape.

9. You can use the Mirror tool to mirror the loft you just created and the wing stub feature using the work plane in the tail area.


Figure 5.18 A loft with and without centerline


Figure 5.19 Adjusting the curve weight and condition of : the loft

Feel free to edit the loft to adjust the shape of the wing to something a bit more to your liking. Here is the full list of conditions available, depending on the geometry type:

1. Free Condition No boundary conditions exist for the object.

2. Tangent Condition This condition is available when the section or rail is selected and is adjacent to a lateral surface, body, or face loop.

3. Smooth (G2) Condition This option is available when the section or rail is adjacent to a lateral surface or body or when a face loop is selected. G2 continuity allows for curve continuity with an adjacent previously created surface.

4. Direction Condition This option is available only when the curve is a 2D sketch. The angle direction is relative to the selected section plane.

5. Sharp Point This option is available when the beginning or end section is a work point.

6. Tangent This option is available when the beginning or end section is a work point. Tangency is applied to create a rounded or dome-shaped end on the loft.

7. Tangent To Plane This option is available on a point object, allowing the transition to a rounded dome shape. The planar face must be selected. This option is not available on centerline lofts.

The angle and weight options on the Conditions tab allow for changes to the angle of lofting and the weight value for an end condition transition. In this example, if the endpoint condition is changed to Tangent on the work point, the weight is automatically set to 1 and can be adjusted. Click the weight, and change it to 3 to see how the end condition will change in the preview. Experiment with the weight to see the changed conditions. If a value is grayed out, the condition at that point will not allow a change. Keep in mind that adding more intermediate profiles to the loft is often the best way to control and define a specific loft shape.

Creating a Part Using Loft and Sculpt

It is often useful to create lofted surfaces when curved corners of differing radii are present. In the next exercise you'll use the Loft tool to create the gently sloping edges of a tablet device housing. Then you'll use the Mirror tool to duplicate the surface, and finally you'll use the Sculpt tool to convert the enclosed surface into a solid.

1. On the Get Started tab, click Open and open the file mi_5a_015.ipt from your Chapter 5 folder.

2. Click the Loft button and set the output to be a surface using the Output button.

3. Select sections End Profile1 and End Profile2 from the browser.

4. Right-click and choose Select Rails; then select the 3D sketches named Top Rail and Bottom Rail from the browser.

Figure 5.20 shows the Loft dialog box and model preview with the selections made.

Selecting the sketches from the browser isn't required, but it does eliminate the chance you might accidentally select an edge rather than the sketch if you try to select them on-screen.

5. Click the OK button to create the lofted surface.

6. Use the Stitch tool (on the Surface panel of the 3D Model tab) to stitch the lofted surface you just created and Boundary Patch1 together.

7. Use the Mirror tool (on the Pattern panel of the 3D Model tab) to mirror the stitched surface, Extrusion1, Split1, and Fillet1. Use the YZ plane found in the Origin folder as the mirror plane selection.

8. Use the Mirror tool again, and this time select the mirror feature you just created as the feature to mirror and use the XZ plane found in the Origin folder as the mirror plane selection.

9. On the Surface panel, click the flyout arrow next to the Patch button to find the Sculpt button and then use the Sculpt tool and select all four quadrants of the surfaces as the surfaces selection. Your result should look like Figure 5.21.


Figure 5.20 Creating a surface loft


Figure 5.21 A solid model created from surface lofts and the Sculpt tool

Creating Multi-body Parts

It is possible to create a multi-body part file with separate solids representing each part of an assembly and then save the solids as individual parts, even having them automatically placed into an assembly. Creating multiple solid bodies in a single-part file offers some unique advantages compared to the traditional methods of creating parts in the context of an assembly file. For starters, you have one file location where all your design data is located. Second, it is often easier to fit parts together using this method by simply sketching one part right on top of the other, and so on.

These two advantages are also the main two disadvantages. Placing large amounts of data (and time and effort) into a single file can be risky should that file be lost. And creating a part with an overabundance of interrelated sketches, features, and solid bodies can create a “house of cards” situation that makes changing an early sketch, feature, or solid a risky endeavor. Used wisely, though, multi-body parts are a powerful way to create tooling sets, molds, dies, and other interrelated parts.

If you do large-machine design, you would be wise to create many smaller, multi-body part files rather than attempting to build one large one. Or you might find that using multi-body parts will work well for certain interrelated components whereas using traditional part/assembly techniques works for the rest of the design.

Creating Multiple Solids

In the following steps, you'll explore the creation of multi-body parts by building a simple trigger mechanism. The challenge here is to define the pawl feature on the trigger lever as it relates to the hammer bar. Figure 5.22 shows the trigger mechanism in its set position on the left and at rest on the right.


Figure 5.22 A simple trigger assembly

As the trigger lever is engaged, the hammer bar overcomes the pawl (lip), and the spring is allowed to force the hammer bar to swing. In the following steps, you'll explore the multi-body solid options as you use one solid to determine the precise fit with the other:

1. On the Get Started tab, click Open; open the part named mi_5a_016.ipt from your Chapter 5 folder.

2. Create a sketch on the front face of the plate.

3. Create a rectangle, as shown in Figure 5.23, using the top hole as a reference to anchor the rectangle.

4. Extrude the rectangle 3 mm away from the plate and use the New Solid option in the Extrude dialog box (leave the circle unselected from your extrude profile so that you end up with a hole).

5. When you click the OK button, you'll see that the Solid Bodies folder in the model tree now shows two bodies present, one representing the base plate and another representing the hammer bar.

6. Create another sketch on the front of the plate and create another rectangle toward the bottom, referencing the end of the hammer bar as shown in Figure 5.24.

7. Extrude the rectangle 3 mm away from the plate, use the New Solid option in the Extrude dialog box, and then click the OK button. This completes the base feature for the trigger lever.

8. Expand the Solid Bodies folder in the browser and notice that there are three solids listed (if you see fewer than three, edit your extrusions and make sure you used the New Solid option).

9. Double-click the text that is your hammer bar and rename it Hammer Bar, for reference later.

10.Right-click the solid that is your trigger lever and choose Properties. In the resulting dialog box, set the name to Trigger Lever and change the color to blue; then click the OK button.


Figure 5.23 The hammer-bar sketch


Figure 5.24 The trigger-lever sketch

Here are several things to note at this point:

· If you expand the browser node for each solid listed in the Solid Bodies folder, you can see the features involved in each.

· You can right-click a solid or solids, choose Hide Others to isolate just the selected ones, and then use Show All to bring back any hidden solids.

· You can select the solid and then choose a color style from the Color Override drop-down on the Quick Access bar (at the very top of your screen).

· You can right-click each solid and choose Properties to set the name and color, view the mass properties, and strip previously overridden values. For instance, if you set just the front face of one of the solids to be red and then decided you wanted the entire solid to be blue, you could use the Strip Overrides option to remove the red face and set the solid to blue. If you did not use the Strip Overrides option, the red face would remain red, and the other faces would become blue.

Using One Solid to Shape Another

Next, you'll create the pawl notch in the trigger lever. To do so, however, you will first make a copy of the hammer bar and then turn that solid into a combined solid that represents the hammer bar in both the set and resting positions. After that, you'll cut that solid away from the trigger lever. You can continue with the file from the previous steps or open the part named mi_5a_017.ipt from your Chapter 5 folder. Then follow these steps:

1. Use the ViewCube® to change the view so that you can see the cylindrical face of the hole in the hammer bar and then choose the Circular Pattern tool on the Patterns panel.

2. Select the Pattern A Solid button and click the hammer bar for the Solid selection.

3. Click the edge or face of the top hole for the rotation axis and set the placement count and angle to 2 and 15 degrees, respectively.

4. Use the button at the top-right corner of the dialog box to set the output to Create New Solid Bodies (the rightmost button), as shown in Figure 5.25.

5. Ensure that the rotation direction is counterclockwise; use the Flip button if it is not and then click the OK button.

If you expand the Solid Bodies folder in the browser, you will see that there are now four solids, the last being the patterned copy of the hammer bar. You will now turn the visibility of the original hammer bar off and use the copy to cut a pawl notch in the trigger plate.

6. Right-click the solid named Hammer Bar in the Solid Bodies folder and choose Visibility to hide that solid.

7. Select the Circular Pattern tool again and choose the Pattern A Solid option, as you did previously.

8. Click the edge or face of the top hole for the rotation axis and set the placement count and angle to 2 and 15 degrees, respectively.

9. Set the rotation direction to go clockwise using the flip button. This should place the patterned copy in place of the original hammer bar.

10.This time use the buttons at the top-right corner of the dialog box to set the output to Join and then click the OK button. This will merge the selected solid with the new patterned one. Figure 5.26 shows the selections.

11.Select the Combine tool on the Modify panel and select the blue trigger lever for the Base selection.

12.Select the fused, rotated body for the Toolbody selection and then set the operation type to Cut so that you are subtracting it from the trigger lever. Then click the OK button.

13.Select any solid in the Solid Bodies folder and choose Show All to turn the visibility of all solids back on.


Figure 5.25 A circular pattern to create a new solid


Figure 5.26 Using a circular pattern to join a copy to another solid

Now that you've solved the trigger-pawl shape and size by using a multi-body part, you could finish the parts by adding features to each body. You'll note that if you create an extrusion, for instance, you can select which solid to add that extrusion to. If it is a cut extrusion, you can select multiple bodies and cut them all at once. The same is true of fillets, holes, and so on.

Move and Rotate Solid Bodies

You can also use the Move Bodies tool to reposition solids once they are created. Try it on your trigger-mechanism parts. Note that to free-drag a solid you have to click the edges or outlines of the preview object rather than on the original object as you might suppose. You can also create a rotation using the Move Bodies tools, or you can move and rotate a body at the same time by creating a two-line action in the Move Bodies dialog box. To locate the Move Bodies tool click the Modify panel flyout arrow. Figure 5.27 shows the Move Bodies options.


Figure 5.27 Moving a solid body within a part file

The options are as follows:

1. Free Drag Move via X, Y, or Z Offsets or, better yet, just click the preview and drag it.

2. Move Along Ray Select an edge or axis to define the move direction and then specify an offset value or just click and drag it in that direction.

3. Rotate Select an edge or axis to define the rotational pivot and then specify an angle or click and drag it.

4. Click To Add Create as many move actions as you want and do them all at once.

Split Solids

Another tool that you may find useful when working with multi-body parts is the Split tool. For instance, if you create a simple solid block by sketching a rectangle on the XY plane and then extruding it 40 mm in both directions, you could then use the XY plane as a parting line to split the solid into two separate solids. You could also create a sketched curve, extrude it as a surface, and use it to split the solid.

Make Part and Make Components

Once you have created your multi-body part, you can write out each solid as an individual part file. The resulting part files are known as derived parts. You can think of these derived parts as just linked copies of the solid bodies. If you make a change in the multi-body part, it will update the derived part. You can break the link or suppress the link in the derived part as well. Using the Make Part and Make Components tools allows you to detail each solid body individually in separate drawings. If you attempt to detail the multi-body part in the drawing, you will see all the solids at once. There is no control to turn off individual solid bodies in a drawing view.

Additionally, you can choose to take your multi-body part and write the whole thing to an assembly. The assembly will consist of all the derived parts placed just as they exist in the multi-body part. These files will be grounded in place automatically so that no Assembly constraints are required to hold them in place. If you decide you would like to apply constraints to all or some of the parts, you can unground them and do so, as well as organize them into subassemblies, and so on.

You should be aware, too, that any additional modeling that you do in the derived part or assembly will not push back to the multi-body part file. Although this may seem like a limitation, it can also be viewed as a good thing, allowing for the separation of design tasks that some design departments require. Here are the general steps for creating components from a multi-body part file:

1. Click the Make Components button on the Manage tab and then select the solid bodies from which you want to create parts.

2. Select additional solids to add to the list or select from the list and click Remove From Selection to exclude any solids that you decide you do not want to create parts from.

3. Select Insert Components In Target Assembly; 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 exits, use the Target Assembly Location's Browse button to select it.

4. Click Next to accept your selections, shown in Figure 5.28.

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

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

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

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

7. Click the Apply button or the OK button to make the components (Figure 5.29). If the component files are created in an assembly, the assembly file is created with the parts 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 parts without an assembly, you are prompted to save the new files.


Figure 5.28 The Make Components: Selection dialog box


Figure 5.29 The Make Components: Bodies dialog box

You can set default behaviors of the Make Components dialog box in a multi-body part file (or a template file) by selecting the Tools tab, clicking Document Settings, selecting the Modeling tab in the dialog box that opens, and clicking the Options button. Figure 5.30shows these options.


Figure 5.30 Setting the Make Components Options defaults

Creating Derived Parts and Assemblies

You can create parts derived from other components using the Derive tool. Common uses of the Derive tool are to create scaled and mirrored versions of existing parts, to cut one part from another part, and to consolidate an assembly into a single-part file. Nonlinear scaling is accomplished using an add-in available in the Inventor installation directory.

Creating Derived Parts

Derived parts are base solids that are linked to the original feature-based part. Modifications to the derived part in the form of additional features are allowed. Original features are modified in the parent part, and changes to the parent part are moved to the derived part upon save and update. There is no reasonable limit to the number of times the parent part or succeeding derived parts can be derived again into more variations.

Deriving a Part File

To derive a single-part file, follow these steps:

1. From a new part file, select the Manage tab and then click the Derive button.

2. In the Open dialog box, browse to the part file and then click the Open button.

3. Select from one of these derived styles:

· A single solid body with no seams between faces that exist in the same plane

· A single solid body with seams

· One or more solid bodies (if the source part contains multiple bodies)

· A single surface body

4. Use the status buttons at the top to change the status of all the selected objects at once or click the status icon next to each individual object to set the include/exclude status.

5. Optionally, click the Select From Base button to open the base component in a window to select the components.

6. Specify the scale factor and mirror plane if desired.

7. Click the OK button.

If the part being derived contains just one body, it is displayed on-screen. If the part being derived is a multi-body part with only a single body set as visible in the part, it is displayed on-screen. If the part being derived is a multi-body part with more than one visible body, no bodies are displayed on-screen. Select the bodies to include by expanding the Solid Bodies folder and toggling the status. To include all bodies, select the Solid Bodies folder and then click the Include Status button. Figure 5.31 shows the Derived Part dialog box.


Figure 5.31 Derived Part options

Deriving an Assembly File

To derive an assembly file, follow these steps:

1. From a new part file, select the Manage tab and then click the Derive button.

2. In the Open dialog box, browse to the assembly file and then click the Open button.

3. Select from one of these derived styles:

· A single solid body with no seams between faces that exist in the same plane

· A single solid body with seams

· One or more solid bodies (if the source part contains multiple bodies)

· A single surface body

4. Use the status buttons at the top to change the status of all the selected objects at once, or click the status icon next to each individual object to set the include/exclude status.

5. Optionally, click the Select From Base button to open the base component in a window to select the components.

6. Click the Other tab to select which component sketches, work features, parameters, iMates, and part surfaces to include in the derived assembly.

7. Click the Representations tab to use a design-view representation, positional representation, and/or level-of-detail representation as the base for your derived part.

8. Click the Options tab to remove geometry, remove parts, fill holes, scale, and/or mirror the assembly.

9. Click the OK button. Figure 5.32 shows the Derived Assembly dialog box.


Figure 5.32 Derived Assembly dialog box options

Modifying Derived Parts

Often, you will need to modify a derived part source file after having derived it into a new part. To do so, you can access the source part or assembly from the Model browser of the derived part by double-clicking it in the browser or by right-clicking it in the browser and choosing Open Base Component. The original file is opened in a new window where you can make changes as needed. To update the derived part to reflect changes to the source file, use the Update button on the Quick Access bar (the top of the screen).

You can edit a derived part or assembly by right-clicking it in the browser and choosing Edit Derived Part or Edit Derived Assembly. This will open the same dialog box used to create the derived part so that you can change the options and selections you set when the derived part was created. Updates will be reflected in the file when you click the OK button. The Edit Derived Part or Edit Derived Assembly options are unavailable if the derived part needs to be updated.

You can also break or suppress the link with the source file by right-clicking the derived component in the browser and choosing the appropriate option. Updates made to the source file will not be made to the derived part when the link is suppressed or broken. Suppressed links can be unsuppressed by right-clicking and choosing Unsuppressed Link From Base Component. Breaking the link is permanent; it cannot be restored.

Using the Component Derive Tool

Another way to derive components is to use the Derive Component tool on the Assembly Tools tab while in an assembly file. This tool allows you to select a part on-screen (or select a subassembly from the browser) and then specify a name for the new derived part file. You'll then be taken into the new derived part file. The resulting derived part or assembly uses the default derive options and the active assembly representations as they are saved in the source file. You can use the edit option in the derived part to change the settings if needed.

Working with Patterns

Inventor includes two tools to create patterns:

· Circular Pattern tool

· Rectangular Pattern tool

The Circular Pattern tool does just what you'd expect it to; it patterns a feature or set of features around an axis. The Rectangular Pattern tool also does what you'd expect, plus more. Using the Rectangular Pattern tool, you can create a pattern along any curve. If you select two perpendicular straight lines, edges, or axes, the result will be a rectangular pattern. However, if you select an entity that is not straight, the pattern will follow the curvature of the selected entity.

Rectangular Patterns

Rectangular patterns use straight edges to establish the pattern directions. You can select a single feature or several features for use in the pattern. Be sure to check the Model browser to see that you have only the features that you intend to pattern-select because it is easy to accidentally select base features when attempting select negative cut features. Start your exploration of patterns by creating a simple rectangular pattern, as shown here:

1. On the Get Started tab, click Open.

2. Open the file mi_5a_018.ipt from your Chapter 5 directory.

3. Click the Rectangular Pattern button on the Pattern panel of the 3D Model tab.

4. With the Features button enabled, select the three features whose names start with the word switch in the browser.

5. Right-click, choose Continue to set the selection focus from Features to Direction 1, and then click the straight edge, indicated in Figure 5.33. Use the Flip Direction button to ensure that the direction arrow is pointing toward the round end of the part.

6. Set the count to 4 and the spacing length to 10 mm.

7. Click the red arrow button under Direction 2 to set it active and then click the straight edge along the bottom, indicated in Figure 5.33.

8. Set the count to 5 and the spacing length to 10 mm.

9. Click the Midplane check box in the Direction 2 settings to ensure that you get two instances of the pattern to each side of the original.

10.Click the OK button, and you will see the resulting pattern.


Figure 5.33 Creating a rectangular pattern

Circular Patterns

You can pattern features around an axis using the Circular Pattern tool. Angular spacing between patterned features can be set in two ways:

1. Incremental Positioning specifies the angular spacing between occurrences. Example: four holes at 90-degree increments.

2. Fitted Positioning specifies the total area the pattern occupies. Example: four holes fit into 90 degrees.

You can enter a negative value to create a pattern in the opposite direction, and you can use the Midplane check box to pattern in both directions from the original.

Continue from the previous exercise with the open file, or open mi_5a_020.ipt to start where that exercise ended:

1. In the Model browser, select the end-of-part marker, and drag it down below the feature named Indicator Cut. Or right-click the feature named Indicator Cut and choose Move EOP Marker.

2. Click the Circular Pattern button on the Pattern panel of the 3D Model tab.

3. With the Features button enabled, select the feature named Indicator Cut.

4. Right-click and choose Continue to set the selection focus from features to axis.

5. Select the center face of the feature named Indicator Stud Hole.

6. Set the count to 4 and the angle to 90; then click the button.

7. In the Positioning Method area, click the Incremental option so that the four occurrences of the pattern are set 90 degrees apart rather than being fit into a 90-degree span. Alternatively, you could set the angle to 360 and leave the positioning method to Fitted and get the same result.

8. Click the OK button. Figure 5.34 shows the resulting circular pattern.

You'll note that your patterned objects require some adjustments. One of the occurrences of the Indicator Cut interferes with the switch feature, and the one opposite of that does not cut through the part correctly (use the ViewCube to look underneath the part to see this clearly). To resolve this, you will first edit the circular pattern and change the way the occurrences solve, and then you'll suppress the occurrence of the switch feature in the rectangular pattern.

9. Right-click the circular pattern in the browser and choose Edit Feature, or double-click it in the browser.

10.Click the button to reveal the Creation Method area and then select the Adjust option. This allows each instance of the pattern to solve uniquely based on the geometry of the model when the feature is using a Through or Through All termination solution.

11.Click the OK button and examine the pattern again, and you'll notice that the top instance of the indicator cut that was not cutting all the way through the part now is.

12.Expand the rectangular pattern in the browser to reveal the listing of each pattern occurrence.

13.Roll your mouse pointer over each occurrence node in the browser until you highlight the one that interferes with the circular pattern.

14.Right-click that occurrence and choose Suppress.


Figure 5.34 Creating a circular pattern

Any occurrence other than the first can be suppressed to allow for pattern exceptions or to create unequal pattern spacing. Figure 5.35 shows the adjusted patterns.


Figure 5.35 The adjusted patterns

Patterns along Curves

Although the Circular Pattern tool allows you to pattern objects around a center axis, it does not provide a way to keep the patterned objects in the same orientation as the original. To do so, you can use the rectangular pattern. Keep in mind that the term rectangular pattern is a bit of a misnomer; this tool might more accurately be described as a Curve Pattern tool because it allows you to select any curve, straight or not, and use it to determine the pattern directions. Continue from the previous exercise with the open file, or openmi_5a_022.ipt to start where that exercise ended; then follow these steps:

1. In the Model browser, select the end-of-part marker and drag it down below the feature named Pin Insert Path Sketch. Or right-click the sketch named Pin Insert Path Sketch and choose Move EOP Marker.

2. Click the Rectangular Pattern button on the Pattern panel of the 3D Model tab.

3. With the Features button enabled, select the feature named Pin Insert Cut.

4. Right-click and choose Continue to set the selection focus from Features to Direction 1.

5. Click the sketched curve (line or arc).

6. Set the count to 10, and notice that the preview extends out into space.

7. Click the button to reveal more options.

8. Click the Start button in the Direction 1 area and then click the center of the Pin Insert Cut feature on-screen to set that center point as the start point of the pattern.

9. Change the solution drop-down from Spacing to Curve Length, and note that the length of the sketch curve is reported in the length box.

10.Change the solution drop-down from Curve Length to Distance and then type 14 at the end of the length value to compensate for the start point and endpoint adjustments.

11.Toggle the Orientation option from Identical to Direction 1 to see the difference in the two and then set it back to Identical.

12.Click the OK button to set the pattern. Figure 5.36 shows the resulting pattern and the dialog box settings.


Figure 5.36 A pattern along a curve

The Coil Tool and Spiral Patterns

In addition to creating patterns based on edges and sketches, you can use surfaces to define the pattern direction. In this exercise, you'll use the Coil tool to create a surface coil to use as a pattern direction. You can continue on from the previous exercise with the open file, or you can open mi_5a_024.ipt to start where that exercise ended. Then follow these steps:

1. In the Model browser, select the end-of-part marker and drag it down below the feature named Coil Pattern Sketch. Or right-click the sketch named Coil Pattern Sketch and choose Move EOP Marker.

2. Click the Coil button on the 3D Model tab (note that the Coil button is found in the flyout menu along with the Sweep and Loft buttons).

3. In the Coil dialog box, set the output to Surface.

4. In the graphics area on-screen, choose the line segment in the Coil Pattern Sketch feature at the base of the part for the Profile selection.

5. Select the visible work axis in the center of the part for the Axis selection.

6. Click the Coil Size tab and set the type to Revolution and Height.

7. Set Height to 25 mm and Revolutions to 4.

8. Click the OK button to create the coiled surface.

You'll now create two work points based on the coil location for use in placing holes. Once the holes are placed, you can pattern them using the surface coil.

9. Click the Point button on the Work Features panel of the 3D Model tab and select the vertical tangent edge and the surface coil to create work points at the intersections, as shown in Figure 5.37.

Turn On Edges to See Tangent Lines

If you cannot see the tangent edges on your model, you can go to the View tab and set the Visual Style tool to Shaded With Edges.

10.Click the Hole tool on the 3D Model tab and set the Placement drop-down to On Point.

11.Select one of the work points for the Point selection and then select the flat side face of the part to establish the direction.

12.Set the Termination drop-down to To and then select the inside circular face of the part.

13.Set the diameter to 3 mm and then click the Apply button.

14.Repeat the previous three steps to place the second hole and then click the OK button.

15.Click the Rectangular Pattern button on the 3D Model tab.

16.Click the two holes for the features (it might be easiest to select them from the browser) and then right-click and choose Continue.

17.Select the surface coil for Direction 1 and use the Flip button to change the direction so that you see the previewed pattern.

18.Set the count to 10 and the length to 10 mm.

19.Click the button and choose Direction 1 for the orientation.

20.Set the Compute option to Adjust and then click the OK button to create the pattern.

21.Right-click the coil and work points and turn off the visibility of these features to see the finished part clearly. Figure 5.38 shows the pattern.


Figure 5.37 Work points at the coils and tangent edge intersections


Figure 5.38 A spiral pattern

Pattern Solids

Oftentimes a part can be modeled as a base feature and then patterned as a whole to create the completed part. Once the part is patterned, nonsymmetrical features can be added and/or patterned occurrences can be suppressed. You can also use the Pattern Entire Solid option to create separate solid bodies when creating multi-body part files is the goal. To take a look at patterning these options, open the part named mi_5a_028.ipt and follow these steps:

1. Select the Rectangular Pattern tool on the Pattern panel of the 3D Model tab.

2. Click the Pattern A Solid button so that the entire part is selected to be patterned. Notice the two buttons that appear in the top-right corner of the dialog box:

Join This option is used to pattern the solid as a single solid body.

Create New Bodies This option is used to pattern the solid as separate solid bodies for multi-body part creation.

3. Leave this option set to Join and set Direction 1 to pattern the solid in the direction of the part width four times at a spacing of 10 mm.

4. Set Direction 2 to pattern the solid in the direction of the part thickness two times at a spacing of 3 mm, as shown in Figure 5.39.

5. Expand the pattern in the Model browser and right-click to suppress the two middle occurrences on the top level. Roll your mouse pointer over each occurrence to see it highlight on-screen to identify which occurrences are the correct ones. Figure 5.40 shows the results of suppressing the correct occurrences.

6. Now you'll pattern the entire solid again. Select the Rectangular Pattern tool again and click the Pattern A Solid button.

7. Set Direction 1 to pattern the solid in the direction of the part length two times at a spacing of 50 mm.

8. Set Direction 2 to pattern the solid in the direction of the part width two times at a spacing of 40 mm, as shown in Figure 5.41.

9. Create a new 2D sketch on one of the long narrow faces and project the tangent edge of the slot cuts or sketch a rectangle on the face. Do this for both ends of the face. Then use the Extrude tool, set the extents to To, and select the vertex, as shown in Figure 5.42. The result will be the removal of all the partial slot features.

10.Create another sketch on the same face, sketch an arc from corner to corner, and set the radius to 400 mm. Then use the Extrude tool to extrude just the arc as a surface (click the Surface Output button in the Extrude dialog box). Set the extents to To again and select the same vertex you previously selected.

11.Select the Replace Face tool from the Surface panel of the 3D Model tab. You may have to expand the arrow on the Surface panel to expand the drop-down to find the Replace Face tool.

12.Select the two recessed faces for the Existing Faces selection and then select the extruded surface for the New Faces selection, as shown in Figure 5.43.

13.Create a sketch on the top face and create two rectangular profiles to use for creating an extrude cut, as shown in Figure 5.44. This cut removes the middle slots and holes, resulting in two long slots down the middle.

14.Select the Shell tool from the Modify panel. Choose the bottom face as the Remove Faces selection and set the Thickness to 1 mm. Figure 5.45 shows the finished part from the top and bottom views.


Figure 5.39 Patterning a solid


Figure 5.40 Suppressed occurrences


Figure 5.41 Patterning the solid again


Figure 5.42 Filling the end slots


Figure 5.43 Replacing faces


Figure 5.44 Cutting the slots


Figure 5.45 The finished part

Dynamic Patterns

It is often desirable to have features such as holes set up in a standard spacing that will dynamically update based on changes to the overall length. You can do this by setting up your patterns with parameter formulas to calculate the spacing from the length parameter. Parts set up in this way can then be saved as template parts, allowing you to select them for new part creation and simply edit the length parameter. To set up a dynamic pattern, open the file mi_5a_032.ipt and follow these steps:

1. Click the Manage tab and select the Parameters tool.

2. Notice that many of the dimensions in this part have been named. This is good practice when creating formulas. To create a formula to determine the spacing, click the Add Numeric button in the lower-left corner of the dialog box. This will create a new user-defined parameter. Enter Adjust_Len for the parameter name (recall that spaces are not allowed in parameter names).

3. Click the unit cell and set the Units to ul, meaning unitless.

4. Type isolate(Length - End_Offset;ul;mm) into the Equation column. There are two parts to this equation:

Length - End_Offset Subtracts the distance from the end of the part from the overall length of the part

Isolate (expression; unit; unit) Neutralizes the distance unit mm so that the Adjust_Len parameter can read it as unitless

5. Click the cell for the Count equation and enter isolate(ceil(Adjust_Len / Spacing);ul;mm) in the cell. There are three parts to this equation:

Adjust_Len / Spacing Divides the adjusted length distance by the value specified in the pattern spacing

Ceil (expression) Bumps the value up to the next highest whole number

Isolate (expression; unit; unit) Neutralizes the distance unit mm so that the Count parameter can read it as unitless

6. Click the Done button and then use the Update button to update the part (you can find the Update button on the Quick Access bar at the top of the screen). Figure 5.46 shows the Parameters dialog box.


Figure 5.46 Formulas to adjust the hole spacing

You might notice that because the length value is currently set to 111 mm, the last hole is running off the part. Because the equation used the Ceil function to bump the calculated value to the next whole number, the count will always be on the high end. Depending on the part length, this may leave you with an extra hole. You can suppress the occurrence of this hole in the Model browser quite easily. Another approach is to remove the Ceil function and allow Inventor to round the calculated value up or down automatically. Depending on the length and spacing values, this might leave you with a missing hole at the end of the pattern where a value gets rounded down. Both are valid options, and you can decide which works best for your situation.

Edit Extrusion1 to adjust the part length, and try different values to see how the hole count drops out. You can also open the files mi_5a_033.ipt and mi_5a_034.ipt to examine similar hole patterns. In mi_5a_033.ipt, the Distance option is used in the pattern feature to evaluate the length of the part. It holds an end offset value and then spaces the holes evenly along that distance. In mi_5a_034.ipt, the pattern is calculated from the center of the part rather than coming off one end. These are just a few examples of how to use user parameters to create dynamic patterns. There are other variations as well. In the next sections, you'll take a more in-depth look at parameters.

Setting iProperties and Parameters

Parameters in part and assembly files can provide powerful control over individual parts and assemblies while also improving efficiency within designs. Part parameters enable the use of iParts, which are a form of table-driven parts. Assembly parameters enable the use of table-driven assemblies and configurations. Parameters are accessed through the Tools menu and within the Part Features and Assembly tool panels. In addition to parameters, you can use iProperties to add information to your files.


iProperties, generically known as file properties, allow the input of information specific to the active file. The iProperties dialog box is accessed through the File drop-down in Inventor. iProperties are a powerful way to pass information from the model files to the drawing file, allowing you to fill out information in title blocks, standard notes, and parts list automatically. The dialog box contains several tabs for input of information:

1. General Contains information on the file type, size, and location. The creation date, last modified date, and last accessed date are preserved on this tab.

2. Summary Includes part information such as title, subject, author, manager, and company. Included on this tab are fields for information that will allow searching for similar files within Windows.

3. Project Stores file-specific information that, along with information from the Summary, Status, Custom, and Physical tabs, can be exported to other files and used in link information within the 2D drawing file.

4. Status Allows the input of information and the control of the design state and dates of each design step.

5. Custom Allows the creation of custom parameters for use within the design. Parameters exported from the Parameters dialog box will also appear in the list. Formulas can be used within a custom parameter to populate values in preexisting fields within the Project and Status tabs.

6. Save Determines the behavior of the current file upon save.

7. Physical Allows for changing the material type used in the current file and displays the calculated physical properties of the current part, such as mass and moment of inertia, as determined by the material type.

Active use of iProperties will help the designer in improving overall productivity as well as provide the ability to link part and assembly information into 2D drawings. Adding search properties in the Summary tab will assist the user in locating similar files.

Custom iProperties are either created manually in the Custom tab of iProperties or created automatically by exporting individual parameters from the Parameter dialog. Custom iProperties may be linked to drawings and assemblies for additional functionality.

Accessing iProperties Through Windows Explorer

When you right-click an Inventor file in Windows Explorer and choose Properties, you can select the iProperties tab from the file properties dialog box. Clicking the iProperties button on the iProperties tab opens the Inventor iProperties dialog box just as you would see it in Inventor.

This can offer people in the office who do not have access to Inventor the ability to view and change iProperties when needed. For instance, someone in the manufacturing department can use this to set the Mfg. Approved Date iProperty once a part has been successfully built on the shop floor based on a given drawing and/or part file. To change iProperties without having Inventor installed, you can install Inventor View. Inventor View can be downloaded for free from the Autodesk website.

You can also use the Details tab in this way to quickly confirm the Inventor version the file was created in and last saved under.

Part Parameters

Part parameters are composed of model parameters, user parameters, reference parameters, and custom parameters. Model parameters are automatically embedded as a part is dimensioned and features are created. Most are a mirror image of the sketch-creation process. As each dimension is created on a sketch, a corresponding model parameter is created, starting with a parameter called d0 and incrementing each time a new parameter is created. When you name a dimension, you are changing the automatically assigned parameter name. To access the list of parameters, select the Manage tab and click the Parameters button. Figure 5.47 represents a typical parameter list.


Figure 5.47 Part parameter list

Looking across the top of the dialog box, you will see columns for the parameter name, unit type, equation, nominal value, tolerance type, model value, parameter export, and descriptive comments. Take a look at each of these columns:

1. Parameter Name The values in this column correspond to the name of the parameters assigned as the part is built. Each parameter name starts with a lowercase d followed by a numeric value. The parameters can be renamed to something that is more familiar, such as Length, Height, Base_Dia, or any other descriptive single word. Spaces are not allowed in the parameter name. Hovering your mouse pointer over a name will initiate a tool tip that will tell you where that variable is used or consumed. Parameters can be of three types:

· Model parameters are created from dimensions or dialog box inputs that drive the geometry.

· Reference parameters are created from dimensions that are driven by other geometry entities.

· User parameters are created by you, the user, and are used in formulas and iLogic rules or referenced by model parameters.

2. Unit/Type The unit type defines the unit used in the calculation. Normally, the unit type will be set by the process that created it. When a user parameter is created, you will be presented with a Unit Type dialog box when you click in the Unit column. This will allow you to select a particular unit type for the user parameter.

3. Equation This column either specifies a static value or allows you to create algebraic-style equations using other variables or constants to modify numeric values.

4. Nominal Value This column displays the result of the equation.

5. Tolerance This column shows the current evaluated size setting for the parameter. Click the cell to select Upper, Lower, or Nominal tolerance values. This will change the size of tolerance features in the model.

6. Model Value This column shows the actual calculated value of the parameter.

7. Key A parameter can be made a key by selecting the key check box for the parameter row.

8. Export Parameter These check boxes are activated to add specific parameters to the custom properties for the model. Downstream, custom properties can be added to parts lists and bills of materials by adding columns. Clearing the check box will remove that parameter as a custom property. After a parameter is added, other files will be able to link to or derive the exported parameter. Text and True/False parameters cannot be exported.

9. Comment This column is used to help describe the use of a parameter. Linked parameters will include the description within the link.

User Parameters

User parameters are simply parameters that a user creates by clicking the Add button in the lower-left portion of the Parameters dialog box. You can add numeric, text, and True/False parameters; however, only numeric parameters may be exported or contain expressions. Text and True/False parameters can be created for use in iLogic rules. User parameters can be used to store equations that drive features and dimensions in the model. The user-created parameter can utilize algebraic operators written in the proper syntax that will create an expression in a numerical value.

Reference Parameters

Reference parameters are driven parameters that are created through the use of reference dimensions in sketches and the use of derived parts, attached via a linked spreadsheet, created by table-driven iFeatures, or created through the use of the application programming interface (API). For instance, Inventor sheet-metal parts create flat pattern extents, which are stored as reference parameters.

Formatting Parameters

If needed, you can format the parameter to display differently than the default display. To do so, you must first select the Export Parameter check box in the Parameters dialog box for the parameter you intend to customize. Once the parameter is selected for export, you can right-click that parameter and choose Custom Property Format to access the Custom Property Format settings. In the Custom Property Format dialog box you can change property type, units, format, and precision as well as control the display of unit strings, leading zeros, and trailing zeros. When you've configured the parameter formatting, it is reflected in the custom iProperty for that parameter.

For instance, if you have a part dimension length of 100.00 mm and you want to call that length into the part description but do not want to see the units string (mm) or the zeros after the decimal point, you would go to the Manage tab, click the Parameters button, and then select the Export Parameter check box for the length parameter. Then you'd right-click the length parameter and choose the Custom Property Format option. And then finally you'd uncheck the Unit String and Leading Zeros options. To see the results, you'd exit the Parameters dialog box and then right-click the top-level node in the browser (typically the filename), choose iProperties, and then click the Custom tab to find the custom iProperty that corresponds to the exported parameter.

Parameter Functions

One of the most important aspects of working with parameters is the ability to create expressions using the available parameter functions. The functions in Table 5.1 can be used in user parameters or placed directly into edit boxes when you are creating dimensions and features.

Table 5.1 Functions and their syntax for edit boxes


Unit type


cos (expression)


Calculates the cosine of an angle.

sin (expression)


Calculates the sine of an angle.

tan (expression)


Calculates the tangent of an angle.

acos (expression)


Calculates the inverse cosine of a value.

asin (expression)


Calculates the inverse sine of a value.

atan (expression)


Calculates the inverse tangent of a value.

cosh (expression)


Calculates the hyperbolic cosine of an angle.

sinh (expression)


Calculates the hyperbolic sine of an angle.

tanh (expression)


Calculates the hyperbolic tangent of an angle.

acosh (expression)


Calculates the inverse hyperbolic cosine of a value.

asinh (expression)


Calculates the inverse hyperbolic sine of a value.

atanh (expression)


Calculates the inverse hyperbolic tangent of a value.

sqrt (expression)


Calculates the square root of a value. The units within the sqrt function have to be square mm in order to return mm. For example, sqrt(144 mm^2) returns 12.

sign (expression)


Returns 0 for a negative value, 1 if positive.



Returns an exponential power of a value.
For example, exp(100) returns 2.688E43.

floor (expression)


Returns the next-lowest whole number.
For example, floor(3.33) returns 3.

ceil (expression)


Returns the next-highest whole number.
For example, ceil(3.33) returns 4.

round (expression)


Returns the closest whole number.
For example, round(3.33) returns 3.

abs (expression)


Returns the absolute value of an expression.
For example, abs(3*-4) returns 12.

max (expression1; expression2)


Returns the larger of two expressions.
For example, max(3;4) returns 4.

min (expression1; expression2)


Returns the smaller of two expressions.
For example, min(3;4) returns 3.

ln (expression)


Returns the natural logarithm of an expression.

log (expression)


Returns the logarithm of an expression.

pow (expression1; expression2)


Raises the power of expression1 by expression2.
For example, pow(3 ul;2 ul) returns 9.

random ()


Returns a random number.

isolate (expression; unit;unit)


Used to convert the units of an expression.
For example, isolate(Length;mm;ul), where Length=100mm, returns 100 ul.


Internal Parameter

Returns the constant equal to a circle's circumference divided by its diameter, 3.14159265359 (depending on precision).
For example, PI*50 mm returns 157.079633.


Internal Parameter

Returns the base of the natural logarithm 2.718281828459 (depending on precision).

* 1 unit or / 1 unit


Used to convert unit types of an expression, much like isolate.
For example, 100 mm *10 ul returns an errant value for a unitless parameter.
100 mm / 1 mm * 10 ul returns 1000 ul.
100 mm * 10 ul / 1 mm also works.

Setting Up User Parameters in Your Templates

Although many times parameters are used to control design input on a per-design basis, you can often use preestablished parameters in template files, so only a couple of key parameters need to be changed in the part file to create a new variant of a standard part. User parameters are especially powerful when these types of template parts are created.

Consider, for example, a standard-type mounting bracket. The general shape is carried through in all iterations, but you can identify several key dimensions that are driven by the particulars of each new design situation. Dimensions such as length, width, height, and thickness are good examples of parameters that can be identified and set up in a template part.

Other things to consider for use as parameters would be critical dimensions such as the locations of holes from the edge of the part, hole sizes, hole counts, and hole spacing. If the hole offset is determined by the material thickness and hole size, then a formula can be established in the part template to calculate the minimum offset value.

Once the part parameters are created and tested for accuracy, the part can be turned into a template by using the Save Copy As Template option in the Save As menu. This will save the part file in the Template directory. Template parts can be as simple or complex as you need, but generally this works best for simple parts. For more complex parts, consider creating iParts, covered in Chapter 7, “Reusing Parts and Features.”

When creating parameter-based template parts, you might want to consider creating user parameters with descriptive names for all the key parameters so they are all grouped together. This way, you (or another user) can quickly identify key parameters used to drive the design later when creating parts in your real-world designs.

Assembly Parameters

Assembly parameters function in much the same way as part parameters except they will generally control constraint values such as offset and angle. When you're authoring an iAssembly, other parameters will be exposed for usage, such as assembly features, work features, iMates, and component patterns, as well as other parameters that may exist within an assembly.

Adding Part Tolerances

Inventor allows you to analyze parts in a manner that ensures valid fit and function at dimensional extremes. When parts are assembled within an Inventor assembly file, you can check to ensure that the parts can be assembled without interference, by setting each part to evaluate at the upper or lower tolerance value. By specifying dimensional tolerances within parts, you are capturing valuable design data that will assist in manufacturing and assembly. In addition to creating the parts separately and then assembling them, you can use multi-body parts to create mated parts in one file, making it easy to design tolerances across multiple parts.

Less Is Often More with Tolerances

When considering part designs for manufacturing, be careful not to apply precise tolerance values where they are not necessary for the design and assembly. Excessive and unneeded tolerances during the design phase can substantially increase the cost to manufacture each part. The secret to good design is to know where to place tolerances and where to allow shop tolerances to occur.

Tolerances are an important tool for communicating design intent to manufacturing. Large tolerances indicate that the dimensions aren't critical to the part's function, whereas tight tolerances indicate that manufacturing needs to pay extra attention to that machining operation. Loosening up tolerances can help manufacturing reduce the reject rate, while tightening up certain tolerances can reduce rework during the assembly process or in the field.

Tolerances in Sketches

You can add tolerances to any individual sketch dimension by right-clicking and choosing Dimension Properties to set precision and tolerance values. You can also access the tolerance setting from within the dimension edit box to set the tolerance as you set the value. Altering the dimension to adjust for tolerance and precision using either method will not affect any other dimension within the part. However, a global file tolerance can be specified within a part using the Document Settings dialog box and will affect every dimension within the model.

In addition to the Dimension Properties menu option and the dimension edit box option, you can access and modify tolerances in the Parameters dialog box. Using the Parameters controls, you can set parameter values for multiple dimensions to include the tolerance as needed. No matter how you access the tolerance setting, there are four options you can use to evaluate the dimension/parameter:

1. + Upper The upper tolerance value in a stacked display. This value should be Maximum Material Condition (MMC). For a hole, the smallest diameter is MMC, whereas for a shaft the largest diameter is MMC.

2. Median The midway point between the upper and lower tolerances. This is commonly used when Computer Numerical Control (CNC) machines are programmed from the solid model.

3. – Lower The lower tolerance in a stacked display. This value should be Least Material Condition (LMC). For a hole, the largest diameter is LMC, while for a shaft the smallest diameter is LMC.

4. • Nominal This is the actual value of the dimension.

Figure 5.48 shows the access to the tolerance settings through the sketch dimension edit box as well as the settings in the Tolerance dialog box. In this case a deviation tolerance is placed on the 36 mm diameter, and the model is set to evaluate at the upper value (note that the plus sign is selected). Since this document's settings are defaulted to three places, all sketch dimensions are in three places to start. In the illustration, the precision has been set to just two decimal places, for just this dimension.


Figure 5.48 Sketch showing tolerances

Tolerance vs. Allowance

Tolerance is the acceptable (but undesired) deviation from the intended (nominal) dimension.

Allowance is the intended (desired) difference of dimensions between two mating parts, depending on the type of fit specified.

Setting Global File Tolerances

Adding tolerances during the design phase pays dividends down the road. There will be fewer errors creating drawings, and tolerances provide clues to design decisions that are useful when updating an existing part. You might find using standard tolerances makes the design process more efficient because the designer needs to focus only on the general tolerance for a dimension (two-place vs. three-place tolerance) and apply special tolerances where needed. You can create custom templates to store tolerance types and other settings for each standard. When the part is created using such a template, standard tolerance values can be overridden for specific dimensional values, or you can override all tolerances within a file or just a specific dimension.

An example of this type of tolerance would be a tolerance rule that states that all decimal dimensions held to two places shall be +/−0.05 and all decimal dimensions held to three places shall be +/−0.001, meaning a dimension of 0.50 would be held to an upper limit of 0.55 and a lower limit of 0.45, whereas a dimension of 0.500 would be held to an upper limit of 0.501 and a lower limit of 0.499.

You can create and modify global tolerance values within a single part by selecting the Tools tab, clicking Document Settings, and then clicking the Default Tolerance tab within an active part file or template. By default, a file will not be using any tolerance standards. In Figure 5.49, the Use Standard Tolerancing Values box has been selected to enable the addition of new standards for the file. To export the tolerance values to the drawing files, the Export Standard Tolerance Values would need to be selected as well.


Figure 5.49 Document settings for tolerance

Once the tolerance values are set, the dimension in the part will evaluate at the nominal value, meaning that if you entered a value of 36 for a part length, that is what the length would be. To evaluate the model at its upper limit at +/−0.001, you would edit the dimension for the length and set the precision to three places and the evaluated size to Upper (using the + button). The length would then change to 36.05, if you are using the earlier example. The default tolerances are set to +/– tolerances. To select another tolerance standard, simply override the existing tolerance values in the tolerance setting and choose another tolerance type, such as deviation. You can see all of this in action in the following steps:

1. On the Get Started tab, click Open; then open the part named mi_5a_035.ipt in the Chapter 5 folder.

2. Select the Tools tab and then click the Document Settings tab.

3. Select the Default Tolerance tab and notice that there are two linear tolerance standards and one angular tolerance standard already set up. Note that there is a linear precision for one decimal and another for two decimals, but there is not one for three decimals. Keep this in mind as you proceed.

4. Click the check box to use the standard tolerancing values, click the Apply button, and then click the Close button.

Now that the part is set to use a global part tolerance, you will edit a dimension and change the precision setting to two decimals so it will use one of the global linear tolerance settings. It is important to note that the dimension precision for all of the dimensions in the part is currently set to three decimal places (the default setting).

5. Edit the 15 mm dimension by double-clicking the text of the dimension.

6. Click the flyout arrow in the dimension input box and select Tolerance.

7. Set the precision to just one decimal place and then click the blue plus sign to evaluate the dimension at its upper value.

8. Click the OK button to exit the Tolerance dialog box and then click the green check mark in the dimension edit box.

9. Although the sketch automatically updates to evaluate the dimension at its upper value, you'll need to update the model to see the solid update. Click the Update button on the Quick Access bar (at the top of the screen; it looks like a lightning bolt).

10.To evaluate the entire part at the lower value, select the Manage tab and click the Parameters button.

11.In the Parameters dialog box, click the red minus sign in the Reset Tolerance area and then ensure the Immediate Update check box is selected to see the Model Values column update.

Compare the nominal and model values in the parameter table to see that some of the dimensions are now reevaluated. Since the dimension default precision for the part is set to three places, the 25 mm and 3 mm dimensions are using that precision (for which no tolerance was set) and therefore have no lower value. Don't be confused by the precision being displayed in the Parameters table because that precision is display only. You can click the Equation cell for each dimension and then right-click and choose Tolerance to access the tolerance and precision settings for each dimension to see or change them.

12.Click Done to exit the Parameters dialog.

13.To change the global dimension precision, select the Tools tab and click the Document Settings button.

14.Select the Units tab and set Modeling Dimension Display for Linear Dim Display Precision to two places; then click the OK button.

Now the 25 mm dimension is using the file default precision of two places, and since it is still set to evaluate at the lower value, it changes to 24.99. You can begin to see the power of using tolerances in your models to evaluate tolerance ranges as you design. You can close this file without saving changes. In the next section you'll look at using limits and fits tolerances.

Part Tolerances in Drawings

Keep in mind that when a part is used in the drawing environment, it will reflect the current evaluated model dimensions and will show the tolerance callout only for retrieved dimensions.

Typically, it is best to create multiple dimension styles with various precision and/or tolerance options in the drawing environment and handle tolerance dimensioning for the print using those tools. You must keep in mind that the tolerance settings in the part are designed to function with the assembly environment and allow calculating tolerances and stack-ups within the assembly. They are not meant to provide tolerancing in the drawing environment.

Working with Limits and Fits

A fit tolerance defines the way two components mate together. There are three basic categories of fits:

1. Clearance This allows the mating components to slide together freely so they can be assembled and disassembled easily.

2. Transition This provides a fit close enough to securely hold the two components together but still allow them to be disassembled.

3. Interference Often called a press fit or friction fit, Interference provides a means to hold two components together by slightly oversizing one component that fits into the other. Some force is required to achieve the fitting of the two components together, and disassembly is not intended.

You can create parts according to fits by adding tolerance values to sketch dimensions and setting the tolerance type to one of the Limits/Fits options. Using a fits table as a reference, you can then set the tolerance according to the desired fit type.

In the following exercise, you will edit a part and set tolerances for the two mating solid bodies, using Table 5.2 as guide for the fits. To start, you will set the inside and outside diameters to use tolerances based on a common diameter of 36 mm. The goal is have a loose fit that allows the insert to slip freely into the sleeve. Follow these steps:

1. On the Get Started tab, click Open; then open the part named mi_5a_036.ipt from your Chapter 5 folder.

2. Select the dimension called Sleeve_ID and double-click to bring up the dimensionedit box.

3. Click the flyout arrow and choose Tolerance from the list.

4. Set the Type drop-down to Limit/Fits-Show Size Limits.

5. Set the Hole drop-down to H11 to create a loose running fit, as listed in Table 5.2.

6. Click the red minus sign to evaluate the inside diameter at its lower limit.

7. Click the OK button to exit the Tolerance dialog box and then click the green check mark in the dimension edit box.

8. Select the dimension called Insert_OD and double-click it to bring up the dimension edit box.

9. Click the flyout arrow and choose Tolerance from the list.

10.Set the Type drop-down to Limit/Fits-Show Size Limits.

11.Set the Shaft drop-down to c11 to create the other half of the loose running fit.

12.Click the blue plus sign to evaluate the outside diameter at its upper limit.

13.Click the OK button to exit the Tolerance dialog box and then click the green check mark in the dimension edit box.

14.Zoom in on the cutout in the sleeve, and you'll see a green arrow on one corner. Zoom in closer on the green arrow, and you will see the gap between the diameter sketches of the sleeve and the insert reflecting your tolerance edits. However, the model itself currently displays no tolerance and needs to be updated to match the sketch.

15.Click the Update button on the Quick Access bar (it looks like a lightning bolt at the top of the screen).

You should see a gap between the solids, providing a loose running fit. Because the current model is being evaluated at the extremes (the upper tolerance for the inside diameter and the lower for the outside diameter), you can determine whether the current design will provide the correct fit. In the real world, you might determine that the outside diameter of the insert needs to be less than 36 mm for the nominal value so that you can ensure a better fit.

Continue with the following steps to explore more options when working with part tolerances.

16.Zoom back out and then click once on any blank area of the graphics screen (to clear any currently selected entities). Then right-click, choose Dimension Display, and choose Tolerance from the flyout menu. This will show you the evaluated dimension values, as shown in Figure 5.50.

17.Right-click either of the dimensions and choose Dimension Properties.

Table 5.2 Example of limits and fits using a hole basis system







Loose running

General fits with smaller clearances.





Very small clearances for accurate guiding of shafts, with no noticeable clearance once assembled.





Snug fit with small clearance. Parts can be assembled and disassembled manually.





Small clearances or slight interferences. Parts can be assembled with little force, such as with a rubber mallet.





Guaranteed interference, using cold pressing.





Medium interference, using hot pressing or large-force cold pressing.




Figure 5.50 Dimensions showing limit/fits

You'll notice that you can set and adjust the tolerance options in this menu as well. You can use the Document Settings tab to set up standard tolerances for the entire file and change the precision and dimension display. These are the same settings you accessed by editing the dimensions and parameters in the previous steps.

This concludes the formal steps of this exercise, but you can continue experimenting with the tolerances using Table 5.2 as a reference. For instance, you might set up a press fit and evaluate the inside diameter at the upper value and the outside at the lower to check to see whether there is indeed enough interference to provide a solid press fit when both dimensions are evaluated at their extremes. (Note that Table 5.2 is not a complete fits list and is provided as reference for this exercise only.)

Working with Free-Form Modeling and Direct Editing Tools

Traditionally 3D parametric modelers such as Inventor have operated on the concepts of sketch and feature dependencies and a model history tree; this approach allows you to step back into the design and change parameters in order to edit the model. With the free-form modeling tools, you create features by moving, rotating, and scaling surface model points, edges, and faces. The Direct Editing tool allows you to add edits to the model tree without stepping back into the model design tree.

Free-Form Modeling

The typical free-form workflow starts with creating a free-form shape such as a box, sphere, cylinder, torus, or quad-ball. Once the shape is created, you use the free-form edit tools to refine and define the shape by selecting points, faces, or edges of the shape and then moving, rotating, or scaling those selections.

Once the shape has been created and edited to the desired shape, you exit the free-form editing mode and are returned to the standard modeling mode where you can sketch and add features to further refine the model as needed.

Creating a Free-Form Shape

To explore the free-form modeling tools, you'll open a file that has been derived from another file. This file contains a motorcycle frame, upon which you will create a fuel tank using the free-form tools.

1. On the Get Started tab, click Open; then open the part named mi_5a_037.ipt in the Chapter 5 folder.

2. On the 3D Model tab, locate the Freeform panel and click the Box button.

3. Choose the XY Plane for the first selection.

4. Choose visible work point in the graphics area (or select Work Point1 from the browser) for the second selection.

5. Set the Length input to 560 mm, set the Width input to 210 mm, and set the Height input to 260 mm.

6. Set the Faces input for the Length to 4 and leave the others at the default.

7. Click the Both Direction button in the Direction control to have the box form created equally on each side of the XY work plane.

8. Click the OK button to create the box form.

Figure 5.51 shows the box form inputs.


Figure 5.51 Creating a : box form

Once your box is created, you'll notice the form feature node created in the model browser as Form1 or something similar. Notice, too, that once you create a form, you are still in the free-form editing mode, as indicated by the available selections in the Ribbon menu. You can close this file without saving changes.

Adding Symmetry to a Free-Form Shape

When you create a free-form shape, it is often helpful to allow the edits to the form to be made symmetrically in one or more planar directions. In Figure 5.51 you can see three check box controls that allow you to specify that the form you create will automatically edit symmetrically in the selected directions. This can be useful if you know that the form will be symmetric in advance, but you can also turn symmetry on or off at any point in the free-form editing process, as illustrated in the following steps:

1. On the Get Started tab, click Open; then open the part named mi_5a_038.ipt in the Chapter 5 folder.

2. In the browser, locate the feature named Form1 and double-click it (or right-click and choose Edit Freeform).

3. Next, click the drop-down arrow below the Edit Form button to expose the list of form editing tools and then click the Symmetry button in the list.

4. Click two opposing faces in order to establish symmetry down the center of the motorcycle, as shown in Figure 5.52.

5. Next click the OK button to set the symmetry.

6. Observe the gray line running through the center of the form that signifies a symmetry condition exists on the form.

7. Click the Edit Form button on the Freeform panel of the 3D Model tab to bring up the Edit Form dialog box.

8. Click any face on the form shape and notice that the opposing, symmetric face is automatically selected also.

9. Click and drag one of the arrow controls in the graphics area to see the symmetric edit in action.

10.Click and drag a different arrow control to see the symmetric edit in action again.

11.Experiment with the controls as you like (these will be explained in more detail in the steps to come) and then click the Done button to create the edits.

12.Click the drop-down arrow below the Edit Form button to expose the list of form editing tools. Then click the Clear Symmetry button in the list and notice that the gray symmetry line running through the center of the form has been removed.


Figure 5.52 Adding symmetry to a form

Adding symmetry to a free-form shape allows you to more quickly and accurately create shape modifications when a symmetric relationship is desired. You can close this file and continue to the next section to further explore the free-form editing tools.

Editing a Free-Form Shape

The Edit Freeform tool contains several controls that can be used in combination or individually to manipulate a free-form shape precisely or visually. For instance, if you wanted to select a face and move it up based on your current view, you could change the Selection button from All to Face, change the Transform Mode button from All to Translation, and change the Transform Space button to View. Figure 5.53 shows the Edit Form dialog box controls followed by a short description of most of the buttons.


Figure 5.53 Edit Form tool controls

Selection Buttons

The Selection buttons set a filter status allowing you to select only points, edges, faces, or bodies, or to select any of them. The controls provided are as follows:

1. Point Filters the selection for only vertex points.

2. Edge Filters the selection for only the edges between faces.

3. Face Filters the selection for only faces.

4. All Allows the selection of any entity. This is the default.

5. Body Filters the selection for entire solid bodies.

Transform Buttons

The Transform buttons can be used to isolate the edit actions. The controls provided are as follows:

1. All (Mode) Allows translation, scaling, and rotation edits. This is the default.image

2. Translation (Mode) Allows selections to be moved in one of the three selected axis directions.image

3. Rotation (Mode) Allows selections to be rotated around one of the three selected axis directions.image

4. Scale (Mode) Allows selections to be scaled in one of the three selected axis directions.image

5. World (Space) Sets the x-, y-, and z-axes based on the world coordinate.

6. View (Space) Isolates two axes based on the current view.

7. Local (Space) Sets the x-, y-, and z-axes based on the local coordinate.

In the following steps, you will use the free-form editing tools to change the free-form box shape into a fuel tank for the motorcycle.

1. On the Get Started tab, click Open; then open the part named mi_5a_039.ipt in the Chapter 5 folder.

2. In the browser, locate the feature named Form1 and double-click it (or right-click and choose Edit Freeform).

3. Click the Edit Form button on the Freeform panel of the 3D Model tab to bring up the Edit Form dialog box.

4. In the Selection area of the Edit Form dialog box, click the Body button.

5. In the Transform area of the Edit Form dialog box, click the Rotation button.

6. Click the box form shape in the graphics area to select it for the rotation.

7. Click the front view of the View Cube; then click (but do not drag) the rotation control and enter -20 for the rotation input.

Figure 5.54 shows the rotated box form.

8. Click the Home button on the View Cube (looks like a house).

9. In the Selection area of the Edit Form dialog box, click the Face button.

10.In the Transform area of the Edit Form dialog box, click the Translation button.

11.Click once in empty space of the graphic area to clear your selection; then hold the Ctrl key on the keyboard and click the two faces, as indicated in Figure 5.55.

12.Click the control arrow pointing to the left of the motorcycle (in the Z direction) and then enter 50 into the input box.


Figure 5.54 Rotating the box form


Figure 5.55 Editing the Free-form shape

Figure 5.56 shows the finished fuel tank created with the freeform tools.


Figure 5.56 Finished : fuel tank

Here are a few tips to know about when working with the free-form editing tools:

· Select points in order to add more roundness or less roundness to an area of the free-form shape.

· You can use the ViewCube in combination with the View (Transform Space) button to set custom directions quickly.

· You can click and drag a control in order to visually edit, or you can click the control and then enter an input.

· You can click, drag, and hold a control and then enter an input.

· By default the controls center on the selections you've made; however, you can use the Locate button to select an edge or point to change the center of the controls in order to get a different result.

· You can use the Display button to toggle the Smooth model display.

· You can use the Edit Form drop-down arrow to find more editing tools, such as Insert Edge, Subdivide, Bridge, Match Edge, and so on. If you pause your cursor over each button, Inventor will display a description of the functionality for each tool.

When you're finished experimenting with this file, you can close it without saving changes. You can refer to the file named mi_5a_039_done.ipt for a reference if you'd like.

Using the Direct Edit Tool

The Direct Edit tool lets you make quick edits to existing features. You can make adjustments to the location, shape, and size of features by directly editing the geometry, rather than editing the sketch or feature that originally created the feature. Specifically, you can use the Direct Edit tool to do the following:

· Quickly explore “what if” design alternatives

· Modify imported parts

· Limit modifications to only the feature you choose, without risking the accidental modification of dependent features

· Quickly update a complex model created by another user without needing to diagnose the feature structure

Figure 5.57 shows the Direct Edit tools.


Figure 5.57 The Direct Edit controls

Using the Direct Edit Tool

In some ways the Direct Edit tool allows you “break the rules” in terms of best practices for editing and updating your 3D models. Generally it is better to locate the original feature or sketch and make the edit there. However, there are times when the Direct Edit tool might be the better choice.

For example, imagine you are tasked with implementing a quick engineering change order (ECO) to an existing part model created in the past by another user. When you look at the design, you see a complex hierarchy of dependent part features. Locating the sketch that was used to create the feature you want to change is difficult, and it introduces the risk of modifying dependent features. Using the Direct Edit tool, however, allows you to change only the geometry you intend to, and it allows you to do so quickly without spending more time that you've been allowed to implement the change.

As a matter of best practice, the Direct Edit tool should be reserved for these types of situations and not used as a general modeling tool.

Troubleshooting Failures with the End-of-Part Marker

Once in a while, even the most skilled design engineer experiences a modeling or design failure. The part may be supplied by a customer or co-worker who has not practiced sound modeling techniques, or you may have to drastically modify a base feature in a part you designed. These kinds of edits change a base feature to the point that dependent features cannot solve, and a cascade of errors can occur. Knowing how to fix these errors can save you hours of work.

One of the best ways to troubleshoot a part and determine exactly how the part was originally modeled is to use the end-of-part (EOP) marker to step through the creation process. In the Model browser, drag the end-of-part marker to a location immediately below the first feature. This will effectively eliminate all other features below the marker from the part calculation.

Often when making modifications to a part, you might change a feature that causes errors to cascade down through the part. Moving the end-of-part marker up to isolate the first troubled feature allows you to resolve errors one at a time. Many times, resolving the topmost error will fix those that exist after it. Figure 5.58 shows a model tree with a series of errors. On the right, the end-of-part marker has been moved up.


Figure 5.58 Using the end-of-part marker to troubleshoot feature errors

Step 1: Editing the First Feature

Normally, the first feature will start with a sketch. Right-click the first feature and select Edit Sketch. Examine the sketch for a location relative to the part origin point. Generally, the first sketch should be located and anchored at the origin and fully dimensioned and constrained. If the sketch is not fully constrained, then add dimensions and constraints to correct it.

If you see sketch entities highlighted in magenta, you probably have projected geometry that has lost its parent feature. To resolve errors of this type, it is often required to break the link between the missing geometry and allow the projected entities to stand on their own. To do so, right-click the objects in the graphics area or expand the sketch in the browser, and right-click any projected or reference geometry that is showing errors; then choose Break Link. This frees up the geometry so that it can be constrained and dimensioned on its own or simply deleted. Figure 5.59 shows the Break Link option listed in the context menu for a projected loop.


Figure 5.59 Breaking : projected object links

Once the sketch is free of errors, you can return to the feature level. Often, you'll be greeted by an error message informing you that the feature is not healthy. Click Edit or Accept. Then edit the feature. Most often you will simply be required to reselect the profile or reference geometry. Once the feature is fixed, drag the end-of-part marker below the next feature and repeat the step. Continue through the part until all sketches are properly constrained.

Occasionally, a base sketch may become “lost” and may need to be reassociated to a sketch plane. To do so, you can right-click and choose Redefine, as shown in Figure 5.60. Depending on how drastic the change in the sketch plane is, this may be all that is required. Often, though, you will need to edit the sketch, clean up some stray geometry using the Break Link option, and then dimension and constrain it so that it is stable.


Figure 5.60 Redefining a sketch

Step 2: Moving the EOP Marker Down One Feature at a Time

Step 2 might be called “learn from your mistakes” (or other people's mistakes). When you have part/feature failures, you should take advantage of them and analyze how the part was created to determine why the sketch or features became unstable. It's always good practice to create the major features first and then add secondary features such as holes, fillets, and chamfers at the end of the part. On occasion, loft and sweep features may fail or produce incorrect results because fillets and chamfers were created before the failed feature. To determine whether this is the case in your model, suppress any holes, fillets, chamfers, or any other feature that you think might be causing the failure.

Once the failed feature is corrected, introduce one suppressed feature at a time until you encounter a failure. This will identify the cause. You may then attempt to move the offending feature below the failed feature and examine the result. If you are unable to move the offending feature, instead reproduce the same feature below the failed feature and leave the original suppressed. When the problems are corrected in a part, you can go back and delete the suppressed offending features.

Although it's not always a silver bullet, you might want to try the Rebuild All tool right after fixing the first broken sketch or feature. Often if the fix was fairly minor, Rebuild All will save you from having to manually edit dependent features one at a time. You can access this tool by selecting the Manage tab and selecting Rebuild All.

Using the End-of-Part Marker to Time-Travel

The end-of-part marker is a powerful yet often-neglected tool. With this tool, you can go “back to the future” and edit or add features to your model. A good example of using the EOP marker is to preserve design intent. Let's say you created a base feature, placed some holes down the center of the part (based on dimensions), and then altered the side faces of the part. The holes are linked to the unaltered edges of this part. You now want to tie the holes to the midplane of this part regardless of the feature size.

You could do this by placing a centered work plane down the part. However, you cannot do this now because when you go back to edit the hole sketch, the work plane would not be available for projection onto the sketch plane. You also cannot drag the work plane above the holes because it was created on the new, altered base feature faces. In this case, you'll want to drag the EOP marker above the hole feature. Now you can place the work plane centered on the two faces. Drag the EOP marker back down to the bottom of the tree. Now edit the hole feature and project the work plane so that the hole centers can be constrained to it.

You can also use the EOP marker to reduce file size when you email a model. If you drag the EOP marker to the top of the browser, only the feature tree (commonly called the part DNA or part recipe) is saved to disk. When the EOP marker is dragged down to the bottom again, all the feature data is recalculated.

The Bottom Line

1. Create complex sweeps and lofts. Complex geometry is created by using multiple work planes, sketches, and 3D sketch geometry. Honing your experience in creating work planes and 3D sketches is paramount to success in creating complex models.

1. Master It How would you create a piece of twisted, flat bar in Inventor?

2. Work with multi-body and derived parts. Multi-body parts can be used to create part files with features that require precise matching between two or more parts. Once the solid bodies are created, you can create a separate part file for each component.

1. Master It What would be the best way to create an assembly of four parts that require features to mate together in different positions?

3. Utilize part tolerances. Dimensional tolerancing of sketches allows you to check stack-up variations within assemblies. When you add tolerances to critical dimensions within sketches, you can adjust parts to maximum, minimum, and nominal conditions.

1. Master It You want to create a model feature with a deviation so you can test the assembly fit at the extreme ends of the tolerances. How would this be done?

4. Understand and use parameters and iProperties. Using parameters within files assists in the creation of title blocks, parts lists, and annotation within 2D drawings. Using parameters in an assembly file allows the control of constraints and objects within the assembly. Exporting parameters allows the creation of custom properties. Proper use of iProperties facilitates the creation of accurate 2D drawings that always reflect the current state of included parts and assemblies.

1. Master It You want to create a formula to determine the spacing of a hole pattern based on the length of the part. What tools would you use?

5. Troubleshoot modeling failures. Modeling failures are often caused by poor design practices. Poor sketching techniques, bad design workflow, and other factors can lead to the elimination of design intent within a model.

1. Master It You want to modify a rather complex existing part file, but when you change the feature, errors cascade down through the entire part. How can you change the feature without this happening?