Lesson 2_formular One Car Design

Lesson 2 – Basic Part Design II This lesson consists of creating three moderately challenging race car components:   

Wheel Sprocket Front roll hoop

Objectives After completing this lesson, you will be able to:       

Revolve a sketch around an axis. Create an offset work plane. Base a new sketch on a work plane. Use the Project Cut Edges tool. Apply the Circular Pattern tool. Create and apply User Parameters. Use Extrude with the Intersect option.

Exercise: Create a Wheel In this exercise, you do the following:  Create the base sketch.  Make the rim cutout.  Create the wheel spokes.  Apply fillets and chamfers.

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Create the Base Sketch In this sequence, you define a half cross section of the wheel and revolve it around its center axis. It is recommended that you keep sketch geometry simple to reduce the number of constraints to manage. For that reason, several fillets and chamfers are omitted from this base sketch. They can be added as features later in the exercise. 1. 2. 3. 4. 5. 6. 7.

Open a new metric part file. Set the Grid spacing to 100 mm. Start a new sketch on the YZ plane. Project the center point onto the sketch plane. Create a horizontal line and constrain it to the center point. Convert the line to a center line. Create and dimension the following sketch.

Note: An ordinate dimensioning scheme is used here for clarity. Sketches in parts use linear dimensions. 8. Revolve the sketch around the center line through a full 360 degrees.

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Make the Rim Cutout The rim cutout is not strictly required for appearance sake since a tire will be placed over the rim. However, modeling it enables you to determine the inertial properties of the wheel. The cutout is created by revolving a sketch around the wheel axis using the Cut option. 1. Create a new sketch on the YZ plane. 2. Press F7 to activate Slice Graphics. 3. Use the Project Cut Edges tool.

4. Use the Project Geometry tool on the XY plane. 5. Create the cutout sketch.

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6. Revolve the sketch using the Cut option.

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Create the Wheel Spokes The wheel spokes are defined by cutting out a single opening and copying it with the Circular Pattern tool. 1. Create a work plane 65 mm offset from the XZ plane toward the outside of the wheel.

2. On a New Sketch, create the following on the work plane:     

Draw two construction circles constrained to the origin, with diameters of 134 mm and 274 mm. Constrain the outer arc concentric and equal to the 274 mm circle. Constrain the 16 mm inner arc tangent to the 134 mm circle. Constrain the center of the 16 mm circle to be vertical with the center point. Constrain the left and right edges to be equal to one another.

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3. Extrude the sketch through all existing geometry with the Cut option using a -3 degree taper. This taper reduces the size of the extrusion along its length.

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4. Turn off the visibility of the work plane. 5. Apply a 1 mm fillet to the inner and outer loop of the spoke cutout.

6. Use the Circular Pattern tool to create six copies of the spoke.

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Apply Fillets and Chamfers In this sequence, you apply the fillets and chamfers to the wheel. Applying these features at the end of the modeling process helps retain sketch simplicity during the early modeling steps. 1. Apply a 3 mm fillet to the seven edges shown (three outer and four inner edges).

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2. Apply a 1 mm fillet to the three edges of the center nut opening.

3. Apply a 4 mm chamfer to the two edges of the centerbore.

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4. Apply fillets to the outer rim; a 3 mm fillet to the seven edges indicated below and a 6 mm fillet to one edge.

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About Sprockets

The sprocket shown is the driven sprocket in the system. The required output speed determines the number of teeth required on the sprocket. In this case, the number of teeth = N  52 The sprocket must be matched to the roller chain it is used with. Sprocket profiles are defined by one of several standards. In the following exercise, an ANSI (American National Standards Institute) standard tooth form is applied within a metric part file, illustrating that units can be easily mixed within Inventor. The ANSI tooth form is defined with a set of equations. These equations are entered in Inventor as parameters and applied to the geometry.

Exercise: Create a Sprocket In this exercise, you do the following:  Create the base sketch.  Examine the tooth profile.  Enter the equations.  Model the tooth.  Complete the teeth.  Add the mounting holes.

Create the Base Sketch 1. Open a new Standard (mm).ipt part file and set the grid spacing to 100 mm. 2. Start a sketch on the XZ plane. 3. Create two circles constrained to the origin, one with a 95 mm diameter and the other with a 180 mm diameter. Autodesk® Formula Car Design

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4. Extrude the sketch 3.5 mm using the Midplane option.

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Examine the Tooth Profile One half of the tooth profile is illustrated in bold as shown. It consists of the following segments:    

An arc of radius R from the midpoint of the tooth root to point v. Arc of radius E from v to x. This arc is centered at q. Line from x to y. Arc of radius F from y to z.

The input values required for calculating the parameters are:   

Chain Pitch = 0.5 inch Chain Roller Diameter = Dr  0.306 inch Number of teeth = N  52

The parameters are provided by the following equations, where the values are in inches.

Ds  1.005Dr  0.003 E  1.3025 * Dr  0.0015 F  Dr (0.8 cos(18  (56 / N ))  1.4 cos(17  (64 / N ))  1.3025 M  0.8Dr cos(25  (60 / N )) T  0.8Dr sin(35  (60 / N )) W  1.4 Dr cos(180 / N ) H  F 2  (1.4 Dr  0.5 * Pitch) 2 S  0.5( Pitch) cos(180 / N )  H sin(180 / N ) Autodesk® Formula Car Design

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OD 

P  cos((180 / N )( Ds  Dr )  2 H tan(180 / N )

Enter the Equations The equations are entered in the Parameters dialog box. Several of the variable names have to be modified because they conflict with the internal names for units. For example, the variable S was changed to Sv. 1. 2. 3. 4. 5.

Click Tools > Parameters. Click Add. Enter Pitch as the Variable Name. Set the Unit to inch. Enter 0.306 in the Equation field.

6. Continue entering the other equations. The equations can be entered in any order.

Model the Tooth 1. Start a new sketch on the XZ plane. 2. Create a sketch of a half tooth using the parameters shown. Autodesk® Formula Car Design

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3. Extrude the half tooth profile using the Midplane option.

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Complete the Teeth In this sequence, you replicate the teeth and shape their tip. 1. Mirror the half tooth about its right face.

2. Use the Circular Pattern tool to replicate the tooth 52 times around the sprocket.

3. Create a new User Parameter named OD2 using the equation:   1 . OD 2  Pitch 0.6  tan(180 / N )   Note: Remember the parameter names were slightly modified so as not to conflict with unit names. In this case, N corresponds to Nt. 4. Create a new sketch on the XZ plane. Autodesk® Formula Car Design

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5. Create a circle constrained to the origin. 6. Dimension the circle to a diameter of OD2.

7. Extrude the circle using both the Midplane and Intersect options.

8. Create a new sketch on the YZ plane. 9. Press F7 to activate Slice Graphics. 10. Project the top line of the tooth and create a sketch to trim the sides.

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11. Revolve the sketch around the sprocket’s center axis using the Cut option.

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Add the Mounting Holes 1. Create a new sketch on the side of the sprocket. 2. Create a construction circle 110 mm in diameter.

3. Create a center point and constrain it horizontal to the origin and coincident with the construction circle. 4. Use the Hole tool to create a 10 mm diameter hole located on the center point.

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5. Use the Circular Pattern tool to make eight holes centered on the sprocket axis.

6. Use the same method to create a circular pattern of four 11 mm diameter holes located on a 149 mm construction circle.

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About Roll Hoops Race cars typically require a roll structure behind and in front of the driver; with these in place, if a rollover occurs, the driver is protected from the road surface.

Exercise: Create a Front Roll Hoop In this exercise, you do the following:  Define a cross section.  Create a sweep path.  Perform a sweep.

Define Cross Section 1. Open Frame.ipt. 2. Create a new sketch plane on the upper surface of the square tubing.

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3. Create a 25 mm circle and add tangent constraints to the rear and side edges.

4. Finish the sketch.

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Create the Sweep Path 1. Click the Work Plane tool. The work plane is defined as parallel to the XZ plane and passing through the center point of the cross section circle. 2. Click on the XZ Plane within the Origin folder, and then click the center of the circle.

3. 4. 5. 6.

Define a new sketch on the work plane. Project the center point of the circle onto the sketch plane. Create a line, arc, and a second line starting from the circle center point. Constrain the end of the horizontal line coincident with the edge of the horizontal tube.

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7. Finish the sketch.

Perform Sweep 1. Click the Sweep tool. 2. Click the path which was just created.

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Completed Roll Hoop

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