Lesson 1_formula One Car Design

Lesson 1 – Basic Part Design I This lesson consists of creating three relatively simple parts that are commonly found in race car suspensions:  Bellcranks  Suspension mounts  Rod ends Creating these parts provides a good exercise in the basics of part modeling in Autodesk Inventor. Objectives After completing this lesson, you will be able to:  Describe the essential characteristics and purposes of bellcranks, suspension mounts, and rod ends.  Set Snap Spacing.  Use construction geometry.  Apply the Mirror feature.  Use the Shell and Hole tools.  Use sketch constraints.  Apply the Fillet feature.

About Bellcranks

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The purpose of the bellcrank is to transfer wheel loads to the spring-damper unit. The bellcrank pivots about a fixed axis on the car’s frame. It is connected to the suspension pushrod at one end and the spring-damper unit at the other end.

The relative distances between the pivot point and the pushrod and damper connections help determine the motion ratio, which is the amount of damper/spring movement for each unit of wheel movement. To facilitate changes to the design, those distances and the angle between the connections are dimensioned directly on the sketch.

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Exercise: Create a Bellcrank In this exercise, you do the following:  Create the base sketch.  Create the relief.  Create the counterbore.  Create the counterslots.  Mirror the relief.

Completed exercise

Create the Base Sketch 1. Open a new metric part file. 2. Set sketch grid density.  Click Tools > Document Settings, and activate the Sketch Tab.  Set Snap Spacing to 100 mm for both X and Y.  Set Grid Display to 1.

 Click OK to close the dialog box. 3. Create a new sketch on the XY plane. 4. Create two construction lines coincident with the origin, and constrain and dimension circles to them.

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Note: The 15 mm hole is the pivot axis and the two 10 mm holes will be the connections to the pushrod and damper body. 5. Add the perimeter lines and arcs around the circles.  Constrain the arcs to be concentric with the circles.  All three of the outer arcs have a 15 mm radius. Dimension one and apply an equal constraint to the other two.  Apply tangent constraints between the arcs and adjacent lines. Some of these constraints may have been applied automatically when you created the sketch.

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6. Extrude the sketch using the Midplane option. Set the Distance to 30 mm.

Create the Relief 1. Define a new sketch on the top of the bellcrank. 2. Create the following sketch geometry.

Note: The 15 mm and 25 mm arcs are concentric with the existing holes, and each of the lines is parallel to the existing edges. 3. Extrude the sketch 10 mm into the part using the Cut option.

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4. Apply a 3 mm fillet to the bottom loop and corners of the relief.

Note: The fillet radius depends on the radius of the ball end mill that is used to create the relief.

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Create the Counterbore  Create a 22 mm diameter x 6 mm deep counterbore at the pivot hole.

Create the Clearance Slots 1. Create a new sketch on the world XY plane. 2. Press F7 to activate Slice Graphics. 3. Use Project Cut Edges on the sketch. This enables you to constrain new sketch elements to existing geometry which is intersected by the active sketch plane. 4. Create two construction circles of 28 mm diameter concentric with the 10 mm holes.

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5. Create two closed loops consisting of lines tangent to the construction circles and collinear with projected edges, and arcs concentric with and equal to the existing curved edges.

6. Extrude the sketch 20 mm using both the Midplane and Cut options.

7. Apply a 3 mm fillet to the edges of the both slots.

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Mirror the Relief  Use the Mirror tool to replicate the filleted relief on the bottom side of the bellcrank.

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About Suspension Mounts

The suspension mount provides a location to mount the upper and lower control arms to the frame. The design illustrated secures a spherical bearing or rod end in double shear. It can be fabricated from sheet material and formed to the required shape. It is secured to the frame by welding.

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Exercise: Create a Suspension Mount In this exercise, you do the following:  Create a sketch.  Extrude the sketch and apply fillets.  Use the Shell and Hole tools.

Completed exercise

1. 2. 3. 4.

Open a new metric part file. Create a new sketch on the world XY plane. Set the Snap Spacing to 100 mm. Create the sketch as shown.

Note: The “fx:” preceding the 17.5 dimension indicates there is an equation associated with the parameter. In this case, it is equal to ½ of the parameter currently set at 35.

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Extrude the Sketch and Apply Fillets 1. Extrude the sketch 25 mm using the Midplane option.

2. Apply 4 mm fillets to the back edges.

Use the Shell and Hole Tools 1. Use the Shell tool with a thickness of 2.5 mm and remove the inner material.

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2. Use the Hole tool with the Concentric Placement option to create an 8 mm hole through the mount. Make the hole concentric with the leading curved surface.

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About Rod Ends

Spherical rod ends provide a spherical joint between components. They prevent translation but enable rotation around all three principal axes. Rod ends are frequently used in race car suspensions to provide a low friction connection that transmits pure axial loads. Since they are free to rotate in all directions, they cannot transmit moment or bending loads. The part modeled in this exercise is the housing only. A complete rod end includes the spherical center section.

Exercise: Create a Rod End In this exercise, you do the following:  Create and extrude circles and apply a fillet radius.  Create a work axis and revolve a sketch around the work axis.

Completed exercise

Create and Extrude Circles and Apply a Fillet Radius 1. 2. 3. 4.

Open a new metric part file. Set the Snap Spacing to 100 mm. Create a new sketch on the XY plane. Create a 10 mm circle centered on the origin and extrude it 30 mm.

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5. Create a new sketch on the XZ plane. 6. Create a 27 mm diameter circle 11 mm above the top of the cylinder. Use the Project Geometry tool to include the top of the cylinder in the sketch.

7. Extrude the circle 10.5 mm using the Midplane option.

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8. Apply a 1mm fillet radius to the cylinders.

Create a Work Axis and Rotate a Sketch Around the Work Axis 1. Create a work axis centered on the larger cylinder.

2. Create a hemisphere centered on the larger circle.

3. Revolve the sketch around the work axis using the Cut option.

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