A Hands-on Test-Drive of the Workflow - Mastering Autodesk Inventor 2015 and Autodesk Inventor LT 2015 (2014) 

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

Chapter 2. A Hands-on Test-Drive of the Workflow

In this chapter you will explore the basic steps involved in creating part models, creating drawings of those parts, putting those parts together into an assembly model, and then creating a drawing of that assembly. At this point it is assumed that you have taken the time to read Chapter 1, “Getting Started,” and are familiar with the Autodesk® Inventor® software interface and navigation tools. If you have not done so, you might want to take the time to read that chapter before continuing.

Although Inventor includes a number of tools that go far beyond the simple tasks of creating parts, drawings, and assemblies, the workflow involved in creating and detailing your designs is the foundation upon which you will build as you learn Inventor. The goal of this chapter is to get you familiar with the overall workflow. In the chapters to follow, you will explore the tools and environments in more depth.

In this chapter, you'll learn to

·     Create a part model

·     Create and detail drawings of part models

·     Put part models together in assembly files

·     Create and detail drawings of assembly models

Creating a Part Model

Throughout this chapter you will be working toward creating the simple mechanism shown assembled in Figure 2.1.

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Figure 2.1 An assembly created with Inventor parts

To become familiar with this assembly, you can open the files mi_2a_180_Complete.jpg, mi_2a_180_Video.mov, or mi_2a_180_Video.mp4; all are located in the Chapter 2 directory of your Mastering Inventor 2015 folder once you've downloaded this book's companion files and created the folder structure Inventor expects for them, as described in the “Before You Start…” sidebar.

To create a model of a part, you will use an Inventor *.ipt file template. Once your new file is created, you will create basic profiles using sketching tools such as lines, arcs, and circles to define the shape of the features that make up the part. You'll also add dimensions and geometric constraints to the sketch. You'll then use the sketched profiles to create the 3D features that will define the parts. Figure 2.2 shows the basic workflow involved in creating a part from sketches and features.

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Figure 2.2 Creating a part model

Before You Start…

Before you begin, make sure you have downloaded the tutorial files from www.sybex.com/go/masteringinventor2015. Place the files in a folder on your computer (such as \My Documents\Mastering Inventor 2015).

If you are using the Autodesk® Inventor LT™ program, the use of project files does not apply, so you can skip the steps listed here. If you are using the full version of Inventor, follow these steps to set the Mastering Inventor 2015 project to be the active project:

1.  From within Inventor, close any open files.

2.  From the Get Started tab, click the Projects button.

3.  From the Projects dialog, click the Browse button.

4.  From the Choose Project File dialog, browse to your Mastering Inventor 2015 folder, select the Mastering Inventor 2015.ipj file, and click Open.

5.  Note that the Mastering Inventor 2015 project is denoted as being the active project with a check mark.

6.  Click Done to close the Projects dialog box.

Now you are ready to get started with this book's exercises.

Starting with a Part Template

Inventor installs with several part templates that you can use to create your part files. In thefollowing steps, you'll use a millimeter-based part template to start your model.

1.  From the Get Started tab, choose New (or press Ctrl+N on the keyboard). Alternately, you can use the New button on the Home screen.

2.  From the Create New File dialog box, expand the Templates folder (if required) and select the Metric folder from the list on the left.

3.  Click Standard (mm).ipt from the list of part templates on the right side of the dialog box. Figure 2.3 shows the metric templates displayed in the Create New File dialog box.

4.  Click the Create button at the bottom of the dialog box to create a new file from the selected template.

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Figure 2.3 Creating a file from a metric part template

Leave the file open and continue to the next section to create a base sketch in this new part file.

Understanding Origin Geometry

When you start a new file from a part template, the file contains some basic origin geometry located in the Origin folder. The Origin folder is found in the browser. Figure 2.4 shows a model of a screw with the Origin folder expanded and the origin geometry set to be visible. You can see the geometry browser nodes in the list on the left and the origin planes and axes displayed on the right as they run through the screw geometry.

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Figure 2.4 Origin geometry in a part model

To create a base sketch for your part, you will use an origin plane to sketch on. Because origin geometry cannot be changed, using an origin plane to sketch on allows you to anchor your base sketch in space and provides a stable foundation upon which to create your part.

For a new file, the origin geometry is typically set to be invisible, but you can right-click any origin geometry and choose Visibility to make it appear. Right-clicking again and deselecting Visibility will toggle the origin feature's visibility back off.

Creating a Base 2D Sketch

When you create a new part, Inventor will prompt you to select an origin plane on which to sketch, or it will create a new sketch for you on a designated origin plane. You can control this behavior by selecting the Tools tab and clicking the Application Options button. On the Part tab, you will find the Sketch On New Part Creation option.

If this option is set to No New Sketch, Inventor will prompt you to select an origin plane to create your base sketch; otherwise, the base sketch will be created on the plane designated by this option automatically. Figure 2.5 shows the option for controlling the sketch behavior for new parts.

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Figure 2.5 Setting the Sketch On New Part Creation option

In the following steps you will create a simple sketch to use as the base for your part. If the option for controlling the sketch behavior for new parts was set to use one of the origin planes automatically, then you can skip these steps.

1.  From the 3D Model tab, select the Start 2D Sketch button.

Inventor will temporarily turn on the origin geometry and pause for you to select one of the planes to sketch on, as shown in Figure 2.6.

2.  Expand the Origin folder in the browser and watch the selection highlight to select the XY origin plane to place your sketch on. Note that you can select an origin plane by clicking it in the browser or by selecting the edge of the plane in the graphics area.

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Figure 2.6 Selecting a plane to sketch on

Once you've selected a plane to sketch on, you will see a Sketch node created in the browser. The Sketch tab is now active and displays the sketch tools, as shown in Figure 2.7.

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Figure 2.7 A new, active sketch

Creating a Profile in the Sketch

Now that you have a sketch created and active for editing in your new part file, you will create a profile to form the base feature of your part.

1.  From the Create panel on the Sketch tab, click the Center Point Circle button.

You should see a dot in the center of your sketch; this is the projected origin center point of your part.

2.  Click the dot to place your cursor on the origin center point so that the circle is centered and anchored to the origin of the part.

3.  Enter Dia = 200 for the diameter of the circle, as shown in Figure 2.8.

Entering Dia = 200 does two things at once. Entering 200 defines the value of this dimension parameter. Preceding it with Dia = defines the name of the parameter, making it easier to recall later.

4.  Press the Enter key to create the circle.

5.  Right-click and choose OK or Cancel to exit the Circle tool.

6.  From the Sketch tab, click the Finish Sketch button to exit the sketch environment.

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Figure 2.8 Creating a sketched circle

Creating a Base 3D Feature

Next, you'll use the circle in your sketch as the base profile for the base 3D feature for this part.

1.  From the 3D Model tab, click the Extrude button.

2.  Enter 25 for the extrude distance.

Note that you can enter the value in the dialog box or in the mini-toolbar controls, and each will have the same result. You might need to click the black arrow to expand the Extrude dialog box in order to see the buttons within it.

3.  Click the OK button (or the green check mark button) to create the extrude feature.

Notice that an extrusion feature has been created in the browser, and if you expand it, you'll find Sketch1, as shown in Figure 2.9.

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Figure 2.9 The base extrusion

If you had the need to change or add something to Sketch1, you could do so by right-clicking Extrusion1 or Sketch1 in the browser and choosing Edit Sketch. Likewise, if you wanted to modify Extrusion1, you could right-click Extrusion1 and choose Edit Feature.

Creating a Secondary 2D Sketch

Next, you'll create a new sketch on the top face of the extrusion you just created.

1.  From the 3D Model tab, select the Start 2D Sketch button.

2.  Click the top face of the extrusion to place the sketch.

3.  From the Draw panel on the Sketch tab, click the flyout arrow and then select the Two Point Center Rectangle tool, as shown in Figure 2.10.

4.  Select the projected center point to place the rectangle.

5.  Enter Dia for the first input and then press the Tab key on the keyboard. This will recall the value of the diameter dimension you created previously.

By reusing the diameter parameter when creating the rectangle, you are linking the diameter and the width of the rectangle. This means that if you were to change the diameter value at some point, the rectangle width will automatically adjust as well.

6.  Enter 25 for the second input and then press the Enter key.

7.  Right-click and choose OK or Cancel to exit the Rectangle tool.

8.  Select the outer projected edge of the base feature (the circle) and then use the Construction button to toggle the line type to a dashed construction line.

This allows Inventor to ignore the circle as a profile boundary in the steps to come.

Figure 2.11 shows the circle being set to a construction line.

9.  When your sketch looks like Figure 2.12, click the Finish Sketch button to exit the sketch environment.

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Figure 2.10 Creating a sketched rectangle

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Figure 2.11 Creating a construction boundary

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Figure 2.12 The finished sketch

Creating a Secondary 3D Feature

Next, you'll cut a dovetailed slot from the part using the sketch created in the previous steps. If you did not complete the steps up to this point, you can open the file mi_2a_001.ipt, located in the Chapter 2 directory of your Mastering Inventor 2015 folder.

1.  From the 3D Model tab, click the Extrude button.

2.  If needed, click the black arrow to expand the Extrude dialog box in order to see the buttons within it. Enter 10 for the extrude distance.

Recall that you can enter the value in the dialog box or in the mini-toolbar controls, and each will have the same result.

3.  In the Extrude dialog box, click the Cut button to ensure that the rectangle is cut from the base feature (or set the Solution drop-down to Cut in the mini-toolbar controls).

4.  Click the More tab in the dialog box and enter 12 for the taper distance.

5.  Click the OK button (or the green check mark button) to create the extrude feature.

Notice that another extrusion feature for this dovetailed cut has been created in the browser; if you expand it, you'll find Sketch2, as shown in Figure 2.13.

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Figure 2.13 The dovetail cut extrusion

Patterning a 3D Feature

Next, you'll pattern the dovetailed slot to create a second, cross slot. If you did not complete the steps up to this point, you can open the file mi_2a_002.ipt located in the Chapter 2 directory of your Mastering Inventor 2015 folder.

1.  From the 3D Model tab, find the Pattern panel and click the Circular Pattern button.

2.  For the Features selection, click Extrusion2 in the browser list.

3.  Right-click and choose Continue to switch from the Features selection mode to the Rotations Axis selection mode (or you can click the red arrow in the dialog box).

4.  Click the outer face of the part to use the cylindrical surface as the rotation axis.

5.  Enter 2 for the count.

6.  Enter 90 for the angle.

Figure 2.14 shows the Circular Pattern dialog box at this point.

7.  Click the OK button to create the pattern feature.

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Figure 2.14 The patterned dovetail slot

This concludes the creation of this basic part model. Although this model is somewhat simple, it demonstrates the workflow used to create much more complex part models. Keep in mind that for the majority of the part models you will use this workflow:

1.  Create a new file using an Inventor *.ipt file template.

2.  Create basic profiles using sketch tools to define the shape of the features that make up the part.

3.  Use the sketched profiles to create the 3D features that will define the parts.

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Explore Design Iterations Using Save Copy As

Often when you are designing a part file, you might come to a point in your design at which you want to explore a design idea, without altering your current design. You can do this in Inventor by using the Save Copy As option to save a reserved copy of your current work while still continuing to work on the current file.

The steps to use the Save Copy As option are described here:

1.  Click the Inventor button located at the top left of the screen.

2.  From the drop-down menu, select Save As.

3.  From the Save As flyout menu, select Save Copy As.

4.  Name the file with a name that represents the stage of the design, such as mi_2a_002_without holes.ipt.

Creating and Detailing Drawings of Part Models

In this section you'll open an existing drawing and create views of a part model and then add dimensions and annotations. In the real world, often you'll use a drawing template to create a new drawing, much as you did with the part model template. Other times, you will be editing existing drawings just as you will be doing in these steps.

Creating a Base View on a Drawing

In Inventor, drawing views are created by referencing model files. In the following steps, you'll open a part model and then create a view of it on an existing drawing:

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

2.  Browse for the part file mi_2a_004.ipt in the Chapter 2 directory of your Mastering Inventor 2015 folder and click Open.

If you'd like, spin the part around and take a look at it using the ViewCube® or the Orbit tool. Note that this is basically the same part created earlier in this chapter, with a couple of modifications. Do not close the part; you will want to have it open in the upcoming steps.

3.  On the Get Started tab, click the Open button, browse for the drawing file mi_2a_004.idw in the Chapter 2 directory of your Mastering Inventor 2015 folder, and click Open.

This is a drawing file that has been created using rather poor techniques. In the following steps, you'll clean up this file and create views of the same part file but with much better results.

4.  Hover your cursor over the part on the drawing sheet, and you will see a dotted outline of the view.

5.  Right-click the dotted view border and choose Delete; then click the OK button to confirm that you want to delete the view.

6.  On the Place Views tab, click the Base button to create a base view.

7.  With the Drawing View dialog box open, move your mouse pointer around on the drawing, and you will see a dynamic preview of the part file that you opened earlier. Do not click the screen just yet or you will inadvertently place the drawing view.

Note that all open model files are listed in the File drop-down list. You can select any open model file from the list or click the Browse button to select another file.

8.  In the Scale field, enter 0.5, as shown in Figure 2.15, or use the drop-down list to select 1/2.

9.  In the Orientation pane on the right, click through the available options and watch the preview at your mouse pointer change. Select Top when you've finished.

10.In the Style area, click just the middle button to create an unshaded view with no hidden lines.

11.Uncheck the Create Projected Views Immediately After Base View Creation check box, found in the lower-left corner.

12.Click anywhere on the page to create the view (or click the OK button).

13.Hover your cursor over the view until you see a dotted outline of the view; then click and drag it to move the view to the lower left of the page so that it fits well.

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Figure 2.15 Base View options

Figure 2.16 shows the drawing with the base view.

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Figure 2.16 A well-placed base view

Creating Projected Views on a Drawing

Next, you'll use the base view you created to project other views onto the page. If you did not complete the previous steps, you can open the file mi_2a_005.idw located in the Chapter 2 directory of your Mastering Inventor 2015 folder.

1.  On the Place Views tab, click the Projected button to create views projected from the base view.

2.  Click the base view on the drawing sheet.

3.  As you drag your mouse pointer around the base view, notice the view previews that are being generated.

4.  Drag straight to the right and click. You will see a rectangular bounding box, indicating that a view will be placed there.

5.  Drag diagonally up and to the right from the base view (toward the top-right corner of the page) and click.

6.  Right-click and choose Create to generate the projected views.

7.  Select the view border (dashed bounding box) of the top-right view; then right-click and choose Edit View.

8.  In the Style area at the bottom right of the dialog box, click just the blue button on the right to shade the view and then click the OK button.

Figure 2.17 shows the drawing with the additional projected views.

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Figure 2.17 Projected views

Creating Dimensions on a Drawing

Next, you'll add dimensions to the views. If you did not complete the previous steps, you can open the file mi_2a_006.idw located in the Chapter 2 directory of your Mastering Inventor 2015 folder.

1.  Switch from the Place Views tab to the Annotate tab and then click the Dimension button.

2.  Click any of the circular edges around the perimeter of the base view.

3.  Move your cursor to the outside of the part.

Note that Inventor will give you a radius dimension if you select an arc edge, and it will default to a diameter dimension if you happen to select an edge that is a circle. Often, edges in views overlap, making it difficult to predict whether the selection will return a radius or a diameter. To deal with this, you can right-click and switch the result.

4.  With the dimension still previewing at your cursor, right-click and choose Dimension Type; notice the various dimension types you can place with the current selection.

5.  Choose Diameter as the type and then click on-screen to place the dimension (if the Edit Dimension dialog box appears, you can just click OK without making any edits).

6.  Note that the Dimension tool is still active. Click the line on the left side of the dovetailed slot (make sure you're not clicking the green midpoint dot), and notice that the results display the length of the selected line.

7.  Click the line on the right side of the dovetailed slot, and notice that the results display the distance between the two selected lines, as shown in Figure 2.18. You can click the drawing sheet to place the dimension.

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Figure 2.18 Placing dimensions

You can continue experimenting with the Dimension tool if you'd like, or you can move on to the next section and take a look at assemblies. Keep in mind that there is an entire chapter of this book devoted to the topic of creating and dimensioning drawing views, but this section ideally gave you an idea of the workflow used in Inventor to create drawings from models.

Putting Part Models Together in Assembly Files

In this section, you will explore the workflow used to create assembly models. Assembly files start out as empty container files, into which you place your part models. Once the parts are placed, you can begin to assemble them using what are known as Assembly constraints. Assembly constraints are simply relationships between the geometry of different parts.

In the next set of steps, you will assemble a simple mechanism composed of just a handful of parts. You can open the files mi_2a_180_Complete.jpg, mi_2a_180_Video.mov, or mi_2a_180_Video.mp4 in the Chapter 2 directory of your Mastering Inventor 2015 folder to have another look at the final assembly in action.

Inventor LT and Assembly Files

If you are using Inventor LT, you will not have the ability to create assembly files with your version. If you find that you need to assemble part files, you might look into upgrading to the full version of Inventor.

Placing, Rotating, and Moving Parts in an Assembly File

In the next set of steps, you will open an assembly file and place a part in it. Then you will rotate and move the free-floating or unconstrained parts around in the assembly. As you'll see, when parts are placed into an assembly, they are initially free to move and rotate in all directions.

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

2.  Browse for the assembly file mi_2a_190.iam in the Chapter 2 directory of your Mastering Inventor 2015 folder and click Open.

This assembly file was created from an assembly template much like the part template you used at the beginning of this chapter. Most of the parts have been placed into the assembly. However, there is one more part that needs to be placed, and you will do this next. Once the part is added, you will take a few moments to rotate and move parts around the assembly.

3.  From the Assemble tab, click the Place button (or right-click in the graphics area and choose Place Component).

4.  Browse for the part file mi_2a_183.ipt in the Chapter 2 directory of your Mastering Inventor 2015 folder, and click Open.

5.  Click in the graphics area to place the part into the assembly.

6.  Note that you have the opportunity to place another instance of the same part. In this case, though, you will right-click and choose Cancel to exit the Place Component tool.

7.  Notice that the components are listed in the browser. Take a moment to click the various components, and notice that when selected in the graphics area, the component is highlighted in the browser. When selected in the browser, it is highlighted in the graphics area. To deselect components, you can just click an empty space.

Turning On a Missing Model Browser

Although it isn't common to need to turn the Model browser off, you can do so. More commonly, you may accidentally turn it off by clicking the X button on the right side of the browser title bar. To display it again, from the View tab click the User Interface button on the Windows panel. You'll most likely want to have all the items in this list selected except for possibly the iLogic Browser and the Eco Materials Adviser.

8.  Click the Free Rotate button found on the Position panel of the Assemble tab (or press G on the keyboard).

9.  Click any of the parts other than the large, round base part to select a part for rotating.

10.Click and drag in the center of the rotate “target” to orbit the part around.

11.Click and drag the outside of the rotate “target” to rotate the part around.

12.Click and drag one of the horizontal or vertical lines on the rotate “target” to rotate the part on that axis.

13.Click another part to set it active for rotating.

14.Click anywhere in the graphics area that is not on a part to exit the Free Rotate tool.

15.Next, click and drag any of the parts, other than the large round base part, to move the part.

Note that the large, round base part cannot be rotated or moved because it is grounded in place. If you right-click it and deselect Grounded, it will be available to rotate and move. However, it's always best to have one base part that is grounded in place to provide a stable foundation on which to build your assembly.

Editing a Component by Accident

If you happen to accidentally double-click a component from within an assembly file, Inventor will switch from the assembly environment to the part-editing environment. You'll be able to see that you've done this when the browser shows the other components grayed out, and the 3D Model tools are displayed in the Ribbon menu. To exit the part-editing environment and return to the assembly environment, you can right-click and choose Finish Edit, or you can use the Return button on the far right of the 3D Model tab.

As you've seen, when parts are placed into an assembly, they are initially free to move and rotate in all directions. This ability to move is referred to as the parts' degrees of freedom. Your goal when creating assemblies is to remove these degrees of freedom until your assembly behaves as designed. You can close this file without saving changes and continue to the next section, where you will put the parts together.

Working with Degrees of Freedom in an Assembly

As you saw in the previous section, parts are initially free to move and rotate when placed into an assembly. Next, you'll open another version of the assembly file and examine the behavior of a partially constrained part.

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

2.  Browse for the assembly file mi_2a_191.iam in the Chapter 2 directory of your Mastering Inventor 2015 folder and click Open.

3.  Click and drag the screw, and notice that it can move freely.

However, you'll notice that the round base part cannot move. This is because it is grounded in place. To help better visualize how underconstrained parts can move, you can turn on the degrees of freedom (DOF) icons.

4.  From the View tab, click the Degrees Of Freedom button.

You'll notice that arrows and other icons are overlaid on the screw. These are the DOF indicators and are displayed to show you the remaining degrees of freedom present. Figure 2.19 shows the screw with all of its DOF icons displayed. This part can move in the x-, y-, or z-axis and can rotate around all those axes as well.

In Figure 2.20 the part has only two remaining degrees of freedom because it has been constrained to a hole. It has the ability to move in one axis and rotate around that same axis. This is because the centerline of the part and the centerline of the hole have been constrained together.

Next, you'll place an Assembly constraint to insert the unconstrained screw into the hole on the large base part.

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

6.  In the Type area of the Place Constraint dialog box, select the Mate button (hover your cursor over the buttons to see their names).

7.  Select the cylindrical face of the screw shaft for Selection 1. Notice that the highlight shows that the centerline is selected.

8.  Select the cylindrical face of the hole on the large round base part for Selection 2.

9.  Click the OK button in the Place Constraint dialog box to create the Mate constraint.

10.In the browser, expand the browser nodes for either of the parts, and you will see the Mate constraint you just placed listed under it.

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Figure 2.19 Six degrees of freedom

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Figure 2.20 Two degrees of freedom

Notice that all but two of the DOF arrow icons have been removed from the screw part in the graphics area, and the remaining icons indicate that the screw is free to rotate in the hole and slide in and out of the hole. You can click and drag the screw to confirm this.

Constraining parts to remove degrees of freedom is the way you assemble parts in an assembly file. If the goal is to create a mechanism that moves in a predictable manner, you will leave some degrees of freedom unconstrained so that those parts can still move. You can close this file and continue to explore this idea further.

Placing Assembly Constraints to Define Mechanical Movement

In this section you will place Assembly constraints between parts within an assembly file. Your goal is to constrain the parts in a way that allows the assembled mechanism to operate as it does in the video file (see mi_2a_180_Video.mov or mi_2a_180_Video.mp4).

Using Mate Constraints to Create Sliding Bearings

In the following steps you place Mate constraints on square bearings and the base part to create a sliding motion for the bearings:

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

2.  Browse for the assembly file mi_2a_192.iam in the Chapter 2 directory of your Mastering Inventor 2015 folder and click Open.

3.  Select the View tab; then click the Degrees Of Freedom button to turn on the degrees of freedom triad for each part that is not grounded or fully constrained.

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

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

Here is an explanation of these two options:

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

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

6.  For Selection 1, click the blue face on one of the square bearings. Watch the on-screen highlights to be sure you select the face and not an edge. It may be helpful to zoom in.

7.  For Selection 2, click anywhere on the blue x-shaped face of the base part, as shown in Figure 2.21.

You should see the part “snap” into place based on your selection points. This is just a preview of the constraint and is controlled by the Preview check box. To place the constraint, you need to click the Apply or OK button. Clicking the Apply button places the constraint and then leaves the dialog box open so you can place another constraint, whereas clicking the OK button places the constraint and then closes the dialog box.

8.  Click Apply to place the Mate constraint between the two parts.

9.  Place another Mate constraint using the tapered side face of the x-shaped slot feature and the tapered side face of the same bearing part.

The selection order is not important, but be sure you are selecting faces and not edges, because edges will give you a different result. It might help to zoom in to select the faces. Recall that you can use the wheel button on your mouse to zoom in and out. Figure 2.22 shows the faces to be selected.

10.Once your selections are made, click the OK button to place the constraint and close the dialog box.

11.Click and drag on the bearing part to see it slide in the groove.

Notice too that the DOF icons for the bearing have changed to indicate that it can move in only one axis now.

12.Apply two more Mate constraints to the other bearing part so that it will slide in the other cross groove.

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Figure 2.21 Mate constraint selections

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Figure 2.22 Tapered face selections for the second Mate constraint

You can open the file mi_2a_193.iam to see the assembly completed at this stage and compare it to yours.

Using Insert Constraints to Fasten Parts Together

Next, you'll constrain the remainder of the assembly using the Insert constraint. An Insert constraint places a mate between a center axis and a circular edge all at once, and it's ideal when you are constraining fasteners and other cylinder-shaped parts to holes.

You can continue using mi_2a_192.iam from the previous steps or close it and open mi_2a_193.iam in the Chapter 2 directory of your Mastering Inventor 2015 folder.

1.  Select the View tab; then click the Degrees Of Freedom button to turn on the degrees of freedom triad for each part that is not grounded or fully constrained.

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

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

4.  For Selection 1, click the circular edge of one of the bearings, as shown in Figure 2.23.

5.  For Selection 2, click the circular edge of one end of the oblong link, as shown in Figure 2.24.

6.  Click Apply to place the Insert constraint between the two parts.

7.  Place another Insert constraint using the circular edge on the other bearing and the bottom edge of the oblong link.

Note that because the hole is concentric to the round end of the link, this selection is the same as the circular edge of the hole. Figure 2.25 shows the edges to be selected.

8.  Once the second insert is placed, exit the Place Constraint dialog box, and test the motions of the assembly by clicking and dragging the green dot in the center of the oblong link and “tracing” the outer circular edge of the large, round base part.

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Figure 2.23 Selection 1 for the Insert constraint

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Figure 2.24 Selection 2 for the Insert constraint

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Figure 2.25 Edge selections for the second Insert constraint

To complete the assembly, place an Insert constraint between the flat washers and the holes on the top of the oblong link and then place Insert constraints between the bottom edge of the screw heads and the top of the flat washers. When you've finished, you can open the file mi_2a_194.iam in the Chapter 2 directory of your Mastering Inventor 2015 folder to compare it to your results. Then you can close all the files you have open and continue to the next section to explore the tools used to document assemblies in the 2D drawing environment.

Creating and Detailing Drawings of Assembly Models

In this section, you'll open an existing drawing and add a detail view to the sheet. Then you'll use the annotation tools to place a parts list and part number balloons in the drawing. Finally, you'll export the finished drawing as a PDF file so that it can be shared with people who do not have Inventor.

Inventor LT and Assembly Files

If you are using Inventor LT, you will not have the ability to create drawings of assembly files with your version. If you find that you need to create and detail assembly models, you might look into upgrading to the full version of Inventor.

Creating an Assembly Detail View

In the following steps, you'll open a drawing that contains a single base view of an assembly model. You'll create a detail view by referencing the existing base view.

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

2.  Browse for the drawing file mi_2a_195.idw in the Chapter 2 directory of the Mastering Inventor 2015 folder and click Open.

3.  On the Place Views tab, click the Detail button.

4.  Click anywhere on the existing base view to use it as the basis of the new detail view. This will open the Detail View dialog box.

In the Detail View dialog box, the View/Scale Label And Style settings can be adjusted as needed.

5.  Set the Scale to 1:1.

6.  Next, you'll create the detail boundary by clicking the existing base view. To do so, click the base view approximately in the center of the screw on the right, as shown in Figure 2.26.

7.  Drag the boundary out to a size close to that shown in Figure 2.26 as well. The goal is to encircle the screw, the washer, and the yellow bearing.

8.  Click the screen to set the boundary size.

9.  Move your cursor to the top left of the drawing and click the screen where you would like to place the detail view.

10.Click the detail boundary on the base view, and note the six green grips. Click and drag any of the outer grips to resize the boundary, and use the center one to control the location. Make adjustments as needed to center the boundary on the area of detail.

11.Hover your cursor over the detail view on the page, and you will see a dotted outline of the view. Click and drag this border to adjust the placement of the detail view.

12.Click and drag the label text for the detail view (it will likely read “Detail A”) to move it up.

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Figure 2.26 Placing a detail view

Figure 2.27 shows the detail view placed on the sheet.

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Figure 2.27 The well-placed detail view

You can experiment with moving and resizing the detail boundary on the base view, and notice that it will automatically update the detail view. In the next section, you'll add a parts list to the drawing.

Placing a Parts List and Balloons

Next, you'll create a parts list table in the upper-right corner of the drawing and then add callout balloons. You can continue using the drawing you have open or open the file mi_2a_196.idw located in the Chapter 2 directory of your Mastering Inventor 2015 folder.

1.  Switch from the Place Views tab to the Annotate tab and click the Parts List button (it's toward the right, on the Table panel).

2.  Click either the base view or the detail on the sheet to point the parts list to the assembly file.

3.  Click the OK button and then snap the parts list to the top-right corner of the drawing border.

4.  On the Annotate tab, click the Balloon button.

5.  In the base view, select the edge of the large, round base part and drag out; click once to place the balloon on the sheet, right-click, and choose Continue.

6.  Repeat step 5 for each part in the detail view and then right-click again and choose Cancel to exit the Balloon tool.

You can click the balloons to adjust the placement of the balloon end or the arrowhead end if needed. Figure 2.28 shows the balloon placement.

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Figure 2.28 Assembly part callout balloons

You can open the file mi_2a_197.idw in the Chapter 2 directory of your Mastering Inventor 2015 folder to compare your results. When you're satisfied with your balloon placement, you can continue to the next section to explore the steps used to export the drawing as a PDF file so that it can be emailed and viewed by others who do not have Inventor.

Exporting a Drawing to a PDF File

In the following steps, you can use the drawing file you have been working on, or you can open the file mi_2a_197.idw in the Chapter 2 directory of your Mastering Inventor 2015 folder.

1.  Click the Inventor button located at the top left of the screen.

2.  From the drop-down menu, select Export.

3.  From the Export flyout menu, select PDF.

4.  Name the file as you like and then click the Options button.

5.  Select the Remove Object Line Weights option and set the Vector Resolution to 600 DPI.

Note that if the drawing happened to have multiple sheets, this is where you'd choose to include all of the sheets in one PDF file.

6.  Click the OK button in the PDF Drawing dialog box and then click the Save button to create the PDF in the Chapter 2 directory of your Mastering Inventor 2015 folder.

Review the PDF file, or open the file mi_2a_199.pdf located in the Chapter 2 directory of your Mastering Inventor 2015 folder to see the result of the PDF export.

The Bottom Line

1.  Create a part model. The process of creating a part model starts with an *.ipt template file. Once you've started a part model from a template, you create sketches to define feature profiles, and then you make those profiles into 3D features using one of the 3D modeling feature tools.

1.  Master It You created a base 3D feature for your parts by extruding a sketch profile at a distance of 15 mm. Then you created other sketches on the top face of the base feature. However, you now realize that the base feature should have been 25 mm thick. Can the base feature be changed after you've created other features on it?

1.  Create and detail drawings of part models. The process of creating a drawing file starts with an *.idw template file. Once you've started a drawing from a template, you create views of a referenced part model file. After the views are created, you can add dimensions and other annotations to the view.

1.  Master It You've created a drawing of a part model and then realize that you need to make a change to that model. How will the change to the part model be handled by the drawing file?

1.  Put part models together in assembly files. The process of creating an assembly model starts with an *.iam template file. Once you've started an assembly model from a template, you place part model files into the assembly and then use Assembly constraints to arrange and assemble the part models.

1.  Master It You've assembled your part models in an assembly file and then need to make a change to a part-model file. How will the change to the part model be handled by the assembly file?

1.  Create and detail drawings of assembly models. The process of creating an assembly drawing starts with an *.idw template file, just as it did with creating part drawings. Once you've started a drawing from a template, you can create views of a referenced assembly model file. After the views are created, you can add annotations such as parts lists and callout balloons, as well as dimensions, text notes, and so on.

1.  Master It You've created a drawing of an assembly model and then realize that you need to make a change to one of the part files within that the assembly model. How will the change to the part model be handled by the drawing of the assembly?