On the Get Started tab, click the Open button.

Browse for the file named mi_11a_005.iam located in the Chapter 11 directory of the Mastering Inventor 2010 folder, and click Open.

Activate the View Representation called Mastering Inventor.

On the Design tab, click the Spur Gear button found on the Power Transmission panel. Note that if you've used the Worm or Bevel Gear tools last you may need to use the drop-down to locate the Spur Gear button.

Expand the More options by clicking the >> button and set Input Type to Gear Ratio.

In the Common section, change Design Guide to Module. Enter 3.6 in the Desired Gear Ratio field. Enter 8 degrees in the Helix Angle field.

For Gear 1, select the cylindrical face of the bearing (or any of the green faces) and the Red face of Gear 4. Set the number of teeth to 19.

For Gear 2, select the cylindrical face of the bearing (or any of the yellow faces). Confirm that Facewidth for both gears is 20mm.

When you click Calculate, the preview will update as shown in Figure 11.25. If an error is displayed, check all of the inputs.

Figure 11.25. Smaller Gear 1 on the left, larger Gear 2 on the right

By choosing the Module Design Guide, you also determined the module value (this value is read-only in this method, which is indicated by its field being grayed out).

After satisfying the space and position requirements, you'll now concentrate on selecting the right material for the gears to satisfy the power and speed requirements.

Activate the Calculation tab, and set Method Of Strength Calculation to ISO 6336:1996.

Expand the More options by clicking the >> button and confirm Type Of Load Calculation is set to Power, Speed → Torque because power and speed are known inputs.

In the Material Values area, check the boxes to enable material selection for Gear 1 and Gear 2. Choose 37Cr4 with a face-hardened heat treatment for Gear 1 and 30CrMoV6 4 for Gear 2.

In the Loads area, enter 7.5kW for the power and 260rpm for the speed.

Set Required Life to 15000hr.

Click the Factors button to change load and lubrication parameters. The only modification you will make in this dialog box is to the Kinematic diagram of your gear. Use the slider to select the diagram as shown in Figure 11.26. This diagram corresponds best with the gearbox situation.

Click OK in the Kinematic Diagram dialog box and again in the Factors dialog box to return to the Spur Gears Component Generator dialog box. Then click Calculate.

You will notice that you exceed the safety factors for pitting and tooth breakage, as shown in Figure 11.27. To avoid breakage, you can make your gears stronger by making them wider.

Figure 11.26. Kinematic diagram of the gear set

Figure 11.27. The gear calculator indicates there's a risk of pitting or breakage for this design.

On the Design tab, change the face width of Gear 1 to 60mm and the face width of Gear 2 to 58mm.

In the Advanced Options of the Calculation tab (click the >> button to access these options), change the Contact Safety Factor value of 1.2 to a less cautious factor of 1.0 and click the Calculation button to see if this design complies as indicated in Figure 11.28. You can then click OK to build the gears.

On the Get Started tab, click the Open button.

Browse for the file named mi_11a_007.iam located in the Chapter 11 directory of the Mastering Inventor 2010 folder, and click Open.

Activate the view representation called Gears. Make Gear Set:2 and Spur Gear:1 flexible by right-clicking on them in the browser and selecting Flexible. Verify that you can freely rotate Gear 1 around the axis of the bore hole in Gear 4. Figure 11.30 shows Gear 1 and Gear 4.

Figure 11.30. Gear 4 on the left and Gear 1 on the right

Start the Key Connection Generator from the Power Transmission panel on the Design tab. In the Key area, confirm that the default key type is ISO 2491A. If another key type is selected, click in the field to display the list of keys from Content Center. Change No: Of Keys from 1 to 3.

In the Shaft Groove area, confirm that the Groove With Rounded Ends type is selected. Select the Red cylindrical face of Gear 1 as Reference 1 and the Green end face of Gear 1 as Reference 2. A preview of the keys display on the model.

In the Hub Groove area, select the Blue face of Gear 4 as Reference 1 and any circular edge of Gear 4 as Reference 2.

Based on these selections, the Key Connection Generator updates with an 18mm × 7mm × 50mm key. We need a 63mm long key, which can be selected from the drop-down list in the Key area. Only valid lengths from Content Center are displayed.

In the Select Objects To Generate area, confirm that the Key, Shaft Groove, and Hub Groove buttons are selected. Depending on your parts, the shaft or the gear may already have a groove.

The Key Connection Generator selects an orientation based on the shaft. If you want a specific orientation, select a work plane on the shaft or gear. You can only select planes in the components or in their parent assemblies. No other planes can be selected.

On the Get Started tab, click the Open button.

Browse for the file named mi_11a_009.iam located in the Chapter 11 directory of the Mastering Inventor 2010 folder, and click Open.

Start the Shaft Generator from the Power Transmission panel of the Design tab, and click in the graphics window to temporarily place the shaft.

The four buttons in the Placement section specify the exact location of the shaft. If the shaft is the first component, you can skip the precise placement. For this example, click the first button and select a cylindrical surface (such as one of the yellow ones) to define the axis. The next button is automatically enabled, and you select an inside surface to define the start of the shaft (such as the Green face).

Next, select the work plane to define the orientation. If the shaft preview extends outside the housing, click the Flip Side button.

The default shaft consists of four sections. Delete the first three sections by clicking on the section, either in the list or in the graphics window, and clicking the X icon on the right side of the segment. Your assembly should look like Figure 11.35.

Figure 11.35. Default shaft with first segment active

Two sets of arrows are now visible on the shaft. The thin RGB arrows on the shaft depict the X, Y, and Z directions as usual and cannot be dragged. The thicker arrows, however, can be dragged.

Dragging the thick double-sided red arrow changes the length of the active shaft segment, and dragging the red dots allows you to change the diameter (in Figure 11.35, above, the first segment is active). You can also enter the diameter and length values manually by clicking the...icon (or double-clicking the segment row in the dialog box), and collect the dimensions by measuring the surrounding geometry.

Dragging the thick blue arrow allows you to change the orientation of the shaft. Dragging the thick green arrow offsets the end of the shaft from the housing. Note that by default the Mate icon is checked, indicating that the shaft will be constrained to the housing.

Every segment has four sets of drop-down icons. The second set defines the overall shape of the segment, and the other icons add detail such as chamfers, fillets, grooves, reliefs, wrench flats, threads, and keyways. Figure 11.36 shows the fourth drop-down set.

In these steps, we will create the shaft segments:

Double-click the green arrow at the end of the shaft and set the offset to 0.5mm.

Change the size of the first segment to 60mm × 78.5mm, as shown in Figure 11.37. You can double-click the segment field to display a dialog box or you can use the controls in the graphics window. Add a 0.5mm chamfer to the segment by using the first set of drop-down icons.

Figure 11.36. The four icon sets that define the geometry of a segment

Figure 11.37. Changing the size of the first segment

Add four more cylindrical segments to the shaft to accommodate the future bearings and the output gear. Right-click below the section and select Sections

You have now created the geometry of the shaft so that it fits nicely within the confines of the gearbox, but does it also satisfy the load requirements?

To find out the forces and moments that are at play on the output gear, click OK in the Shaft Generator and create the shaft.

Figure 11.38. Geometry of shaft with five segments

Right-click on the Spur Gears subassembly and choose Edit Using Design Accelerator. Click the Enables/Disables Calculation button (in the top-right corner of the dialog box) to enable the Calculation tab on the Spur Gears component.

Click the Calculate button and consult the calculation results by clicking the Results button on the Calculation tab. From the results (shown in Figure 11.39), you learn that the radial force on the shaft on the output gear location is 3064N, the tangential force is 7007N, and the axial force is 984N.

Right click on the shaft in the browser or graphics window and select Edit Using Design Accelerator. Click the Calculation tab and select the green dot in the middle of section 2 in the 2D preview or in the graphics window.

Select Loads from the Loads/Support drop-down list. The available load types are shown in Figure 11.40; they are radial force, axial force, continuous load, bending moment, torque, and common load. Select the down arrow, which is the first load icon.

Figure 11.40. The six different load types

The radial force on the gear translates into a force in the X direction on the shaft. Likewise, the tangential force on the gear will result in a force in the Y direction on the shaft situated in the center of segment 2, which is the segment on which the output gear will sit. By clicking the ...button on the force in the dialog box or by double-clicking the force arrow in the graphics window, you can change the Forces option to Forces in X and Y Axes.

Enter the Force in X axis = 3064N and the Force in Y axis = 7007N. See also Figure 11.41. You can now delete the default radial force on segment 1.

Here are a couple of tips for navigating around the shaft preview. The force arrow can be dragged along the shaft so that it snaps to one of the green hotspots. The green hotspots depict the center and the extremities of the segments and are associative to any shaft geometry change. The blue hotspot depicts the active hotspot (any load or support that is added will be added to the active hotspot). So, it is extremely important to position your blue dot in the right location prior to adding loads or supports!

Figure 11.41. Entering the radial and tangential forces and positioning supports for the shaft

The force arrows can be reconnected to the green hotspots by double-clicking the arrow and entering a zero distance. When you hold down the Ctrl key, you can rotate the force vector to change its angle.

Next, we add the rest of the forces.

Add a −94 8N axial force to the center of section 2.

Add a torque of 966Nm to section 2 and a torque of −966Nm to section 5. The torques must be equal and opposite, so the torque value for section 5 is preset to −966Nm. Torque is shown with two circular arrow glyphs that are pointing in opposite directions as illustrated in Figure 11.42.

Figure 11.42. Adding torque and axial force to the shaft

The shaft will also undergo some bending because of the axial force on the output gear. Determining the value of the bending moment is relatively simple:

The value of the pitch diameter can be found once again in the gear calculation results table (274.673mm) of Figure 11.40.

Enter a bending moment value along the x-axis of 948N*274.673mm/2 on segment 2, as shown in Figure 11.43.

Figure 11.43. Adding a bending moment to the shaft

Finally, you add to segment 5 the actual load that the shaft will have to provide (20kN). The load is shown as the arrow on the left pointing down in Figure 11.44.

Select Supports from the Loads/Support drop-down list. Double-click the Free support and change the offset to 10mm. Select the hotspot in the middle of section 4 and add a Fixed support. Delete the default Fixed support.

On the Get Started tab, click Open.

Browse for the file named mi_11a_011.iam in the Chapter 11 folder.

Start the Disc Cam Generator from the Power Transmission panel of the Design tab.

Click the Cylindrical Face button and select the (red) camshaft.

Click the Start Plane button and select the side of the first raised section on the shaft. Note that because the assembly is sectioned you need to select the face on the un-sectioned side. In this case you can also select the Yellow face of the engine case, as both are in the same plane.

In the Cam area, enter 2.15mm for Basic Radius and 2mm for Cam Width.

In the Follower area, enter 0.5mm for Roller Radius and 0.4mm for Roller Width.

The cam angle vs. lift data is entered in the Actual Segment area. You select the particular segment from the drop-down list at the top of the area, and enter the data.

Confirm that the Actual Segment drop-down is set to segment 1. This segment is part of the base radius, so we are going to set Lift At End to 0.00mm.

Change the drop-down list to segment 2. This segment continues the base radius, so we are going to leave the end height at 0.00mm.

Click Add After to create a new segment 3. This segment will transition from zero to maximum lift. Instead of using the linear transition shown in Figure 11.48, we are going to set Motion Function to Harmonic (sinusoidal). Set Motion End Position to 225 degrees, and Lift At End to 0.7mm.

Click Add After to create a new segment 4. This segment will transition from maximum to zero lift. Confirm Motion Function is set to Harmonic Sinusoidal. Set Motion End Position to 270 degrees, and Lift At End to 0.00mm.

Change the drop-down to segment 5. Confirm that Motion End is 360 degrees and Lift At End is 0.00mm.

You can also overlay other graphs like acceleration and torque over the inlet cam shape graph, as shown in Figure 11.49.

Figure 11.48. Inlet cam shape

Figure 11.49. Inlet cam shape with acceleration and speed overlays

A full overview of all calculations and all graphs can be obtained by exporting the results into an HTML-formatted report by clicking the Results icon in the top-right corner.

Click the Calculation tab.

The camshaft rotates at half the crankshaft speed, so 1000/2 = 500rpm. In the Cycle Data area, confirm that Speed is selected and enter 500rpm.

In the Follower Loads area, enter 1N as the Force On Roller. Confirm that the Accelerated Weight is 0.01kg. Enter 0.544N/mm for Spring Rating, or spring constant k. Both the spring force and spring constant will be calculated in the next section of the chapter.

Set Cam Material and Follower Material to Steel SAE 5130. This material has an allowable pressure of 900MPa, which is 50% higher than the calculated maximum pressure.

Click Open on the Get Started tab.

Browse to the file called mi_11a_012.iam in the Chapter 11 folder.

The browser is set to Modeling view, so all of the constraints are in a folder at the top of the browser instead of being nested under the components. Find the Drive Me constraint and confirm that the value is 0.0 degrees.

Measure the distance between the Red face on the valve bushing and the Blue face on the crankcase. The result, shown in Figure 11.53, is the minimum working load length of the spring.

Figure 11.53. Determining the minimum load spring length

Start the Compression Spring Generator from the Spring panel on the Design tab.

In the Placement area, click the Axis button and select the valve stem. The Start Plane button is automatically enabled, so select the Red face of the valve bushing. A preview is displayed, but the default spring values are much too large for this application.

Confirm that Installed Length is set to Min. Load.

In the Spring Wire area, set Wire Diameter to 0.15mm.

In the Spring Start and Spring End areas, set Closed End Coils to 1, Transition Coils to 1, and Ground Coils to 0.5.

In the Spring Length area, confirm that Length Inputs is set to L0, n → t. Enter 3.5mm for Loose Spring Length, which is considerably larger than the Minimum Working Load Length value of 2.392mm, so the spring preload will keep the valve seated. Enter 6 for the number of active coils.

In the Spring Diameter area, set Diameter to Inner and enter 1mm. The geometric inputs are shown in Figure 11.54.

If you clicked Calculate, you would get impossible values for the minimum load length or pitch. This is because you did not define all load conditions yet, and so far, you have no idea if the spring you are designing meets the requirements for forces and stresses. To determine this, you will enter the working conditions for the spring on the Calculation tab.

Click the Calculation tab. In the Spring Strength Calculation area, select Work Forces Calculation from the drop-down list.

The spring dimensions are carried over from the Design tab, so you just need to enter the working dimensions for the spring. In the Assembly Dimensions area, select H, L₁ → L₈ from the drop-down list. The Min. Load Length is carried over from the Design tab. Enter 0.7mm, the cam lift, for the Working Stroke value. Enter a nominal value of 2.39mm for the Working Load Length value.

In the Spring Material area, select Heat Treated Wire Carbon Steel.

Figure 11.54. Working load state of the compression string

Click Calculate. If you look at the calculation results in Figure 11.55, you will see that the Max. Load is .984N, which is satisfactory for this design, and the maximum torsional stress, τ₈, of 854MPa is less than the material limit of 972 MPa.

Click OK to create the spring.