American Chopper Tutorial

AMERICAN CHOPPER

In this project we had created various Parts in Solidworks. After the creation of those parts assembled in Solidworks for the Final Product. The various steps involved in the creation of Parts & Assembly are given below.

The various parts which are used in this Project.

1. Transmission Belt.
2. Kick Stand.
3. Front Fender.
4. Rear Fender.
5. Oil Tank.
6. Chain
7. Pedal
8. Front Wheel.
9. Rear Wheel.
10. Front Fork.
11. Chassis.
12. Engine
13. Gas Tank.

Various Commands used in Solidworks during this Project are as follows:

• Extrude: To add the Material along the Z-Direction.
• Cut-Extrude: To remove the material.
• Thin Extrude: To Extrude as a Thin Feature.
• Fillet/Chamfer: To add/remove material around the corners or edges.
• Projected Curve: The two sketches project onto each other to form the 3D curve.
• Linear Pattern: To Create Linear Sketch/Features Pattern along required axis with no of instances.
• Circular Pattern: To Create Circular Sketch/Features Pattern along required axis in terms of angle
• Mirror: To copy the features/sketch over the Plane
• Dome: To Create dome over surfaces
• Sweep: A Sketch Profile creates a base, boss, or cut sweep by moving a 2D profile along a 2D or 3D sketch path.
• Shell: The shell tool hollows out a part, leaves open the faces you select, and creates thin-walled features on the remaining faces.
• Revolve: To Create extrude around the axis.
• Surface Sweep: A Sketch Profile creates a surface sweep by moving a 2D profile along a 2D or 3D sketch path.
• Extend: To extend the existing surface
• Split: To Split the Single Surface into two
• Revolve Cut: To Remove the material around the axis
• Blocks: To group the sketch entities and make it as a block
• Appearances: To Change the appearances of features, bodies, surfaces
• Trim Lines: To remove the unnecessary entities.
• Loft: You can create a guide curve loft by using two or more profiles and one or more guide curves to connect the profiles.
• Revolved Surfaces: To add Revolved surfaces around the axis
• Thicken: To Thicken Surfaces into Solids or to create solids from enclosed volumes
• Surface Trim: To remove the unwanted surfaces
• Surface Knit: To Knit two surfaces as single surface
• Merge: To merge two entities or surfaces
• Apply Constraints/Relations in the sketch.
• Spline: To draw smooth curves
• 3D Sketch: Create entities in 3D
• Offset Entities: To Offset the entities in the sketch.
• Convert Entities: To convert the edges/surfaces to form as entity
• Creating Decals
• Insert Image to the sketch.

Steps followed to create Transmission Belt:

1. Click on the new part and then selected the template which I had created earlier.(you can use default template as well if you don’t have any template created but make sure you are using MMGS format).
2. Select the Front plane ---> Sketch. (you can also choose other options like Sketch --> Front plane or Extrude Boss/Base ---> Front Plane).
3. In the sketch window following steps need to be performed to get required shape

3.1. Select Line command and create a line (horizontal relation and 350mm).

3.2. Create a arc from the end point of line (Tangent relation and R70 mm).

3.3. Create a line from the end point of arc (Tangent relation).

3.4. Create a arc from end point of line to base line (Tangent relation and R60 mm).

3.5. offset the sketch to 3.5 mm (offset to outside) (not required if you are using step 4)

You can create arc in two ways by using arc command or you can use same line command as well.

Once the relation and dimensions the sketch will have proper constraints and it will turn to black.

4. Now you can go to Extruded Boss/Base and extrude (Blind) the sketch with a depth of 88 mm in direction 1 and select thin feature option in the Extruded Boss/base give a depth of 3.5 mm in direction 1.
5. Now you can go to Extrude Boss/Base and extrude (Blind) the sketch with a depth of 88 mm in direction 1. (required if you are using 3.5).
6. Create fillets to the corners. you can select the corners in multiple ways. corner radius is 1mm.
7. Now Change the appearances of the model by clicking on the appearance in task pin. Select the rubber --> Matte.

8.Save the part as Name_Transimmison_Belt.

9. Upload part to the google drive, Copy the sharable link to the Answer box in the challenge and describe the steps followed.

Steps followed to create Kickstand:

1. Click on the new part and then selected the template which I had created earlier. (you can use default template as well if you don’t have any template created but make sure you are using MMGS format).
2. Rename the Right Plane to Midplane. This is for better understanding it is up to you to rename it or not.
3. Select the Front plane ---> Sketch ---> Ellipse command (horizontal & Coincidence constraints with origin, 40 mm Major axis, 18 mm Minor axis.
4. Exit Sketch.
5. Select the Mid plane ---> Sketch --> Spline command. Draw a spline above origin with starting from centre of ellipse dimensional constraints to the end point of spline (horizontal distance 220 mm, Vertical distance 110 mm). Make sure spline has only one point Select the diamond symbol in the spline and give horizontal constraint, distance from origin to end point of handle 225 mm.
6. Now Create a plane at the end point of spline (features ---> Reference Geometry ---> Plane (First Reference --Spline & Second Reference - End point of spline).
7. Select the New Plane ---> Sketch---> Ellipse command (horizontal & Pierce constraints with end point of spline, 30 mm Major axis, 12 mm Minor axis.
8. Exit Sketch.
9. Select the Loft Boss/Base ---> Ellipse 1 ----> Ellipse 2 (make sure to adjust the snap points for proper loft) ---> Centreline (spline).
10. Goto Tools ---> Features ---> Dome ---> select the outer surface of Ellipse 1 (Elliptical dome & 13 mm) Repeat the similar actions for Ellipse 2 with dimension 5 mm.
11. Select the Midplane --> Rectangular (centre point Rectangle) on the Ellipse 1 (length 28mm, breadth 8mm) at the centre of origin.
12. Exit Sketch.
13. Select the Extrude Cut --> Trough all - both sides.
14. Select the Top Plane --> Sketch ---> Circle command (draw a circle on the origin of Día 9 mm).
15. Exit the sketch.
16. Select the Extrude Boss/Base. In Direction1 give the option up to Next (it will extrude to next available surface). In Direction 2 given the option up to Next.
17. Select the midplane ---> Sketch ---> Line (tick the box Midpoint line). Draw a line from the centre of origin of length 50 mm at 2.5 mm from origin. Make sure the line as Horizontal and vertical to origin.
18. Exit the Sketch.
19. Goto Tools ---> Feature ---> Split. In Split select the sketch (in which we have created line) and then click on cut surface. you need to select the body which you want to remove and make sure you have turn on the consume bodies. Hide the sketch for better viewing purpose
20. Select the Fillet Command and give fillets to internal edges which are generated after the rectangular cut of 2mm.
21. Select the Fillet Command and give Fillets by selecting both inner surfaces of 0.5 mm.
22. Now Change the appearances of the model by clicking on the appearance in task pin. Select the Metal ---> Chrome.

23.Save the part as Name_Kick_Stand.

24. Upload part to the google drive, Copy the sharable link to the Answer box in the challenge and describe the steps followed.

Steps to create Front Fender:

1. Click on the new part and then selected the template which I had created earlier.(you can use default template as well if you dont have any template created but make sure you are using MMGS format).
2. Rename all the three plane to front plane LSW as Vertical Plane Front Fender, Top Plane as Center Plane Front Fender & Right Plane as Mid Plane Front Fender.
3. Select the Vertical Plane Front Fender --> Sketch --> Arc command. Draw a Arc above the origin (horizontal constraint between two end points of arc, vertical constraint between center of arc to origin, distance betwen orign and center of arc 280 mm, distance between two end points of arc 160 mm & Radius of arc R125).
4. Offest the arc to the side of origin with a distance of 6mm. Draw a vertical line from end points main arc (no dimensional value is required but make sure it crosses the offest arc).
5. Now use the extend lines command and join the offest arc with the vertical lines drawn before.
6. Now use Trim command to remove the extra vertical lines.
7. Draw a construction from the origin of any length but make sure it is horizontal.
8. Exit from the sketch.
9. Now Select the sketch and use Revolve Boss/Base command. In direction 1 give 5 degree & in direction 2 give 130 degree. EXit the revolve boss/base.
10. Now select the Center plane Front Fender --> Skecth --> Line command (select construction line). Draw a line of 34 mm from origin in direction above to origin.
11. Now select the line and choose Dyanamic Mirror in Tools --> Sketch Tools --> Dynamic Mirror.
12. Now Select spline Command. Draw a spline from the end point of line towards the edge of the part with one point in between the end point of line to edge of the part.
13. The distance from center of origin to point on the spline (vertical distnace 45 mm & 50 mm horizontal distance). the distance from origin to the end point of spline is 200. Now apply vertical constraint to the handle in the end point of spline and radius of curvature as R160. You can check the curvature to have smooth spline without any concave or convex by enabling Curvature view. Please disable the curvature view after you have got desired curvature.
14. Exit the sketch.
15. Goto Tools ---> Feature ---> Split. In Split select the sketch(in which we have created line) and then click on cut surface. you need to select the body which you want to remove and make sure you have turn on the consume bodies. Hide the sketch for better viewing purpose
16. Now Select the Vertical Plane Front Fender --> Skectch (make sure that you can see the inner side of the part. if the view is not correct make necessary change with the help of shift and arrow keys.).
17. Draw a construction line from origin to the end of the part(make sure the construction coincide with the inner edge of part with vertical constraint).
18. Now Select spline Command. Draw a spline from the end point of line towards the edge of the part with one point in between the end point of line to edge of the part.
19. The distance from center of origin to point on the spline (vertical distnace 182 mm & 47 mm horizontal distance). Add horizontal constraint to the end point of spline with origin. Now apply vertical constraint to the handle in the end point of spline and radius of curvature as R180. You can check the curvature to have smooth spline without any concave or convex by enabling Curvature view. Please disable the curvature view after you have got desired curvature.
20. Exit sketch.
21. Goto Tools ---> Feature ---> Split. In Split select the sketch(in which we have created line) and then click on cut surface. you need to select the body which you want to remove and make sure you have turn on the consume bodies. Hide the sketch for better viewing purpose
22. Select the Fillet Commands --> 2mm select the top surface of the part and make sure fillet are created.Exit from fillet command.
23. Now Change the appearences of the model by clicking on the appearence in task pin. Select the Painted ---> Car ---> Siena.

24.Save the part as Name_Front_Fender.

25. Upload part to the google drive, Copy the sharable link to the Answer box in the challenge and describe the steps followed.

Steps to create Rear Fender:

1. Click on the new part and then selected the template which I had created earlier.(you can use default template as well if you dont have any template created but make sure you are using MMGS format).
2. Rename all the three plane to front plane LSW as Vertical Plane Rear Fender, Top Plane as Center Plane Rear Fender & Right Plane as Mid Plane Rear Fender.
3. Select the Vertical Plane Front Fender --> Sketch --> Arc command. Draw a Arc above the origin (horizontal constraint between two end points of arc, vertical constraint between center of arc to origin, distance betwen orign and center of arc 90 mm, distance between two end points of arc 364 mm & Radius of arc R290).
4. Offest the arc to the side of origin with a distance of 6mm. Draw a vertical line from end points main arc (no dimensional value is required but make sure it crosses the offest arc).
5. Now use the extend lines command and join the offest arc with the vertical lines drawn before.
6. Now use Trim command to remove the extra vertical lines.
7. Draw a construction from the origin of any length but make sure it is horizontal.
8. Exit from the sketch.
9. Now Select the sketch and use Revolve Boss/Base command. In direction 1 give 10 degree & in direction 2 give 140 degree. EXit the revolve boss/base.
10. Now Select the Center Plane Front Fender --> Skectch (make sure that you can see the inner side of the part. if the view is not correct make necessary change with the help of shift and arrow keys.).
11. Draw a arc above the origin with distance between two ends as 160 mm, horizontal constraints between two endpoints & vertical constraint between center of arc to origin. make sure the center of arc is below the origin at a distance of 227 mm.
12. Goto Tools ---> Feature ---> Split. In Split select the sketch(in which we have created line) and then click on cut surface. you need to select the body which you want to remove and make sure you have turn on the consume bodies. Hide the sketch for better viewing purpose.
13. Apply Fillet command to the four corners of part. The radius of fillet be 45 mm.
14. Apply Filler Command by selecting the top surface of the part.The radius of filler be 4 mm.
15. Now choose the sheel command and select the inner surface of the part and give the thickness as 4 mm.
16. Now Change the appearences of the model by clicking on the appearence in task pin. Select the Painted ---> Car ---> Siena.
17. Save the part as Name_Rear_Fender.
18. Upload part to the google drive, Copy the sharable link to the Answer box in the challenge and describe the steps followed.

Steps to be followed to Create Oil Tank:

1. Click on the new part and then selected the template which I had created earlier.(you can use default template as well if you dont have any template created but make sure you are using MMGS format).
2. Rename the Front Plane LSW to Midplane Oil Tank.
3. Select the Top plane ---> Sketch. Select the line Command and make it as construction line. Draw a construction line of 230 mm to the left side of the origin.
4. Select the point command and draw a point vertical to origin at a distance of 146 mm above the origin.
5. Select the Construction and choose Dynamic mirror entity (tools --> Sketch tools --> Dynamic mirror entity).
6. Draw a vertical line of 50 mm above the origin, continue the line towards the point at a certain angle & then draw a arc (by moving away from line and coming back to start point) make sure the endpoint coincide with origin.
7. Now apply a coincedence relation between center of the arc and the Construction line, Apply a coincedence relation between slanted line and point.
8. Exit from the sketch.
9. Select the Extrude Boss/Base. In direction 1 give a depth of 170 mm and direction 2 give a depth of 10 mm.
10. Select the Mid Plane Oil Tank ---> Sketch. Select the line command and draw a vertical line of 166 mm above the origin.
11. Draw a line from the origin at an angle of 92.5 degree to the left side of origin and make sure you are not applying any relation. The horizontal length of line from origin be 215 mm.
12. Draw a line from end point of slanted line above origin of length 42 mm and coincide with edge of the part. make sure you are not applying any perpendicular relation between slanted line and new draw line.
13. Draw a spline from the shorter line towards the vertical line with one point in between. The horizontal and vertical of point in spline from origin are 107.5 & 113 respectively.
14. Exit from the sketch.
15. Select the Extrude Boss/Base and make sure you have untick the merge results. in direction 1 through all and in direction 2 through all.
16. now Select the command Combine (insert --> Features ---> Combine). Select the two bodies and make sure sub type is in common in Combine option.
17. Now Change the appearances of the model by clicking on the appearance in task pin. Select the Painted ---> Car ---> Siena.
18. Create Fillet a 10 mm on all edges of the part.
19. Now Change the appearances of the fillets in model by clicking on the appearance in task pin. Select the Painted ---> Car ---> white.
20. Now select the shell command and gives thickness of 3mm. Make sure you didn’t select any surfaces.
21. now save the part with name YUVARAJ_OIL_TANK.

Steps to be followed to Create Chain:

1. Click on the new part and then selected the template which I had created earlier. (you can use default template as well if you dont have any template created but make sure you are using MMGS format).
2. Rename the Front Plane --> Midplane Chain, Top Plane --> Centerplane Chain, Right Plan --> FrontPlane Chain.
3. Select the Midplane Chain ---> Sketch. Select the line Command and make it as construction line. Draw a horizontal construction line of 650 mm to the right side of the origin and from end point of horizontal line draw a vertical construction line of 147 mm below the origin.
4. Draw a circle of diameter 289 mm on the start point of horizontal construction line. Draw a circle of diameter 99 mm on end point of vertical construction line.
5. Draw a arc from the larger circle to the lower circle without touching the quadrants with a radius of 1500 mm (draw above and below the origin). Give proper constraints tangent realtion with the arcs and circles
6. Trim the lines which are not required and then exit the sketch.
7. Select the Midplane chain and then sketch. Draw a horizontal construction line of length 15.13 mm.
8. Draw circle\'s on the end points of the construction line of equal length of diameter 8mm.
9. Draw circle\'s on the end points of the construction line of equal length of diameter 12mm.
10. Draw a arc from the one circle to another circle without touching the quadrants. Give constraints tangent between arc and circle and then radius of 28 mm.
11. Trim the lines which are not required and convert the sketch to blocks and save the block as chainlink1.
12. Draw a construction line of length 15.13 mm and then draw circles on the end point of the construction line of diameter 8mm.
13. select the slot command and then draw a slot between the end points of the centre line with a radius of 5.5 mm.
14. convert to sketch to block and then save as chainlink2.
15. Exit from the sketch without saving.
16. Select the midplane chain and then sketch.
17. Select the tools --> blocks --> Insert blocks. Insert both blocks chainlink1 and chainlink2.
18. select the chainlink1 and make coincidence with starting point of the arc and then coincidence with the sketch.
19. No make chianlink2 concentric with chainlink1 and also coincidence with sketch.
20. extrude the sketch and then select the pins and then extrude to a depth of 25mm with midplane option. Fillet the pins both surfaces with 0.5 mm.
21. Extrude the sketch and then remove the sketch in the selected contours, Select the surface(which looks similar to chainlink1) and extrude to a depth of 2mm with a offest of 9.5mm.
22. Extrude the sketch and then remove the sketch in the selected contours, Select the surfaces which appears similar to chainlink2 and extrude to a depth of 2mm from the vertex of chainlink1.
23. Now select the curve driven pattern and select the larger arc above the origin, with spacing 30.25 mm.
24. make sure the pattern will not cross the arc
25. Repeat the steps 20,21, 22, 23 & 24 till you complete closed loop.
26. When the loop is completed there will not be proper connection between last one and first one we need to remove the last body.
27. choose the Midplane chain and then sketch with the help of offset, and then draw last link to complete the chain.
28. Move the pin bodies to one folder and surface bodies to another folder.
29. Mirror the surafce bodies with the help of mirror command and midplane chain.
30. Save the Part as YUVARAJ_CHAIN.

Steps to be followed to Create the Pedal:

1. Select the Front Plane and draw a vertical construction line with midpoint option enabled of length 35mm.
2. Draw a horizontal constrcution line from both endpoints of the vertical lines and then draw a horizontal line from the end point of the horizontal construction line. make sure the length from the end point of vertical line to end point of horizontal line of 72 mm.
3. Draw a arc from the start poins of the line and tangent relation with horizontal lines and vertical lines.
4. Draw a slanted line from the end point of the both horizontal lines. Makes sure the both slanted lines are parallel to each other.
5. The end point dimnsions of the slanted line below the origin are 23 mm below the horizontal line (below the origin) and 112 mm far from the vertical construction line.
6. The end point dimensions of the slanted line above the origin, 159 mm far from the vertical construction line.
7. Draw a circle on the center point of origin of diameter 16 mm and a draw one more circle of equal length at a vertical distance of 47 mm. horizontal construction between two circles center points.
8. Draw a circle in between slanted lines of diameter 18 mm, 13 mm distance from horizontal line below the origin and 125 mm from the vertical construction line.
9. Draw a horizontal construction line, The starting point of line from vertical construction line be 255 mm & 84 mm from the lower horizontal line.
10. Draw a circle of diameter 15 mm. Distance from vertical construction line be 218.40 mm & distance from the horizontal line below the origin be 42mm.
11. Draw a spline from the end point of the slanted lines to the start point of the horizontal line created.
12. Apply tangency relation between end point of slanted lines and splines, angle constraints and length constriants for splines above the origin are 15 degrees, 250 mm for the handle near the horizontal construction line. The 200mm for handle near the end point of the slanted line.
13. The angle constraints and length constraints for splines below the orign are 35 degress and distance of 245 mm near the horizontal construction line. The 545 mm for handle near the end point of the slanted line.
14. Draw a fillet of 60mm on the intersection points horizontal and start point of slanted line.
15. Extrude the sketch and holes with a depth of 8mm.
16. Extrude the holes and reverse the extrude with a depth of 20mm.
17. Give fillet to surfaces extruded of 20 mm with the value of 1 mm.
18. Select the top plane and sketch on the top plane. Draw a vertical construction line from front face of the part to the outer most surface of the part.
19. Draw a vertical line from the outer most surafce of the part, draw a horizontal line from the end point of vertical line and then draw a vertical line from the end point of the horizontal line and then draw a vertical line from the end point of the horizontal line and close the loop.
20. Revolve the sketch and then exit the sketch.
21. Insert features and then Create a dome of 3mm on the front side of the revolved surface.
22. Select the sketch and then extrude of depth 100 mm from the front surface of the part.
23. Select the chamfer option and then choose distance -distance sub option with values 16 & 9mm.
24. Select the chamfer option and then choose distance - distance sub option with values 16 & 7.5 mm.
25. Select the sketch ---> Front plane. offset entites 2.5 mm from all the extruded surfaces.
26. Then extrude the sketch of depth 2.5 mm and then select the offset option with offset 20mm.
27. Create fillets on the extruded surfaces of length 1 mm
28. Select the liner pattern choose any tangent edge, Select the entities as 4 and then select features and fillets.
29. Create fillets on foot peg of the shifters and then apply.
30. Save the part as YUVARAJ_PEDAL.

Steps to be followed to create Front Wheel:

1. Click on the new part and then selected the template which I had created earlier.(you can use default template as well if you dont have any template created but make sure you are using MMGS format).
2. Click on the sketch and select front plane.
3. Click on line command and choose mid point line option in the line command from the origin, make a closed figure as rectnagle with dimension horizontal dimension 110mm vertical dimension 40 mm.
4. Draw a horizontal line 140 mm wide at a vertical distance of 330 mm from origin.
5. Draw a vertical construction from the horizontal line (140 mm) of length 28 mm. make sure the vertical line starts from the mid point of horizontal line. give concident relation between vertical line and origin.
6. Draw two slanted equal length lines towards origin from the end points of the vertical line. add relation between two slanted lines equal length and end points are horizontal. Dimensions 75 degree between slanted lines and horizontal line.
7. Draw a arc from the end points of the slanted lines with radius of 230 mm. Select the mid point of the arc and end point of the vertical construction line and then make coincident.
8. Apply fillets to the intersection corners.
9. Exit from the sketch
10. Revolve the sketch over the midpoint line which was created at the origin.
11. Sketch on the right plane. Draw a construction line from origin with length of 320 mm.
12. Draw one more construction line with a angle of 31 degree and add constraints of equal length between two construction line.
13. Draw a horizontal line of length 22.5 mm from origin to the left of the origin
14. Draw a arc between two construction line . select the origin and center point of arc and apply constraints merge.
15. Draw a spline from end point of horizontal line (22.5) to the left point of the arc. apply vertical constraint on lower handle and length of 340 mm.
16. Mirror the arc, spline and horizontal line over the the vertical construction line.
17. Exit from the sketch.
18. Extrude the sketch with the help of midplane option of depth 122mm. Deselect the merge results.
19. Sketch on the right Plane. Draw a vertical construction line from the origin to the end point of the before extrude, Select the outermost edge of the extrude and click on convert entites. Apply coincident relation between vertical construction line and conver entity.
20. offest the left, right and bottom edges to inner direction of value 9mm.
21. Trim the extra lines or curves.
22. Draw a two vertical construction line from bottom edge of the spoke to the offest line. The distance between two vertical construction line is 9mm, the right most line is 2.5 mm from the origin.
23. Draw a construction line from the origin to the upper curve with the angle of 9 degree.
24. Draw a spline from end point of 9 degree reference line to the end point of 2.5 mm offest line.
25. apply verical constraint to the lower handle and dimension of 300 mm.
26. Draw a spline from 9 mm offest line to the arc and apply verical constraint to lower handle and dimension of 300 mm.
27. Length between two splines be 9mm.
28. Mirror the two splines about the vertical construction line.
29. Exit From the sketch.
30. Select the Extrude cut, In selected contour options select the three areas which are created with the splines created, Give depth as through all Deselect the auto select option in future scope and select the spokes.
31. Sketch on the right plane. Draw 3 construction circles from the origin of dia 215, 350 & 485 mm.
32. offset edge of each spoke inwards, the offset value be 4.5 mm and convert these edges to construction.
33. click on power trim and remove the construction circles such a way that point are created on the intersection of construction circles & construction offset entities.
34. Draw arc (joining from one spoke to other spoke) on the interesection points with radius 200 mm(points created by 485 mm circle), 75mm(points created by 350 mm circle), 15mm (Arc created with the help of outer point created by 215 mm)& 20mm (arc created with the help of inner point created by 215 mm circle).
35. Now offset all the arc with the value of 8mm. make sure the offset is towards the origin.
36. Now remove the excess lines which are crossed the offset lines created by spoke edges.
37. now join the the arc and offset curves and make it closed sketch.
38. Extrude the sketch and use the option upto the vertex in both sides. deselect the Auto-select option and select the spokes.
39. Sketch on front plane. create intersection curve on the inner surface of rim. Make sure to remove the extra intersection created in the bottom. Convert the top intersection curve to construction line.
40. Draw a vertical construction line from origin to mirror.
41. Draw a horizontal construction line from the origin towards the left of the origin of length 20 mm, Draw a line from the end point of the construction line to the edge of the rim.
42. Draw a vertical line from the end point of the horizontal line above the end of the arc and join to the arc with the help of line. make sure apply a tangent relation between line joining the arc.
43. Draw a spline from the end point of tangent reference line to the end point of the horizontal construction line.
44. Apply vertical constraints to lower handle and dimension of 525 mm. Apply tangent constraint and dimension of 150 mm.
45. mirror the spline and three straight line about the vertical construction line.
46. Exit the sketch and select the revolve cut. revolve about the horizontal and remove the material only from spoke and Hub.
47. Now Select circular pattern and choose the bodies and make sure you had selected equal spacing and select the circular reference and give instances as 3.
48. Now select the combine and choose the 3 spokes, Rim and Hub.
49. Apply 4mm fillets to front and back face.
50. Sketch on the right plane and draw circle of 340mm.
51. Exit the skecth and select the extrude option with offset value of 45mm and 7mm thickness (deselect the merge results).
52. Select the front face of rotor and sketch a cirlce of dia 8mm vertical with origin at a distance of 160mm.
53. Select the linear pattern and select the circle with 20 mm spacing in x direction, 4 instances and 320 degrees.
54. Extrude cut and select the sketch and choose the option upto next and then deselect the auto select and choose the rotor.
55. Circular pattern and select the extrude cut and choose the circular refernce and instance as 14.
56. Sketch on the front face of the rotor. Draw 2 circle of dia 100 & dia 240 Draw two lines which cross the two circles.
57. Add relation to the lines with origin as coincident and dimensional value between lines of angle 25 degree.
58. use power trim and remove the circle and make a closed sketch.
59. Extrude cut and select the sketch and choose the option upto next and then deselect the auto select and choose the rotor.
60. Apply fillets on inside four corner of 4mm.
61. Circular pattern and select the extrude cut & fillets and choose the circular refernce and instance as 10.
62. Skecth on the right plane, draw a circle at the origin of dia 40 mm.
63. Extrude cut trough all the bodies.
64. Select the front surface of the caliper and 2 draw circle at the origin of dia 200mm & 380mm.
65. draw the lines on the circle and make sure the lines are coincidence with the origin.
66. Angle between the lines be 54 deg, Draw a vertical construction line from origin & add angle of 63 degree with upper line.
67. power trim and remove the extra lines and make a closed sketch.
68. Extrude the skecth, Depth away from rotor 19.5 mm & direction 10.5 mm (deselect the merge results).
69. Add chamfer the both sides with distance - distance option 6mm and 20 mm.
70. Add fillets to the outside upper edge and lowe edge of value 8mm.
71. Add fillets to outside edges all round the part on both sides of value 4mm.
72. Sketch on front plane. create intersection curve on the outside surface of rim. Make sure to remove the extra intersection created in the bottom. Convert the top intersection curve to construction line.
73. Draw a slanted line from the intersection curve away from the origin, and draw a three point of arc from these slanted edges.
74. Select the center point of arc and origin apply relation of vertical, make slanted lines of equal length, make end point of slanted lines horizontal. the distance between upper edge 154 mm, The radius of the arc be 113 mm the distance of center of arc from the origin be 280.7 mm.
75. apply fillets to both corners, exit the sketch.
76. Revolve the sketch and choose the temporary axis and deselect the merge results.
77. Skecth on the front plane and choose the edge of the rim and convert entities. Change the convert entities line to construction.
78. Draw four rectangle (three point center rectangle) on either side of origin (two above the origin, two below the origin).
79. The width of all rectangle be 8mm, Upper edge of the rectangles above the origin be 138 mm, The upper edge below the origin be 90 mm long, apply relations like equal length (between the rectangles above the origin) and parallel(between the recatngles left and right side of the origin).
80. Distance from bottom edge of the rectangle above the origin and left of the origin horizontal distance 20mm and vertical distance from above origin 50mm . Angle dimension of 130 between top rectangle and construction line.
81. Distance from top edge of the rectangle below the origin and left of the origin horizontal distance 25 mm and vertical distance from below the origin 29 mm.
82. Distance from bottom edge of the rectangle above the origin and right of the origin horizontal distance 54 mm and vertical distance from above origin 63 mm . Angle dimension of 50 between top rectangle and construction line.
83. Distance from top edge of the rectangle below the origin and right of the origin horizontal distance 96 mm and vertical distance from below the origin 46 mm.
84. Exit the skecth and select the Extrude cut with offset option 450mm, offset from the surface and select the surface of tyre 4mm. Feature scope just select the tyre.
85. Apply full round fillets to the all rectangles created with the extude cut.
86. Circular patter and select the extude cut and fillets, instance 14, Circular reference in the model
87. Rename the solid bodies as Rim, Rotor, Caliper & Tyre.
88. Apply materails to all the solid bodies Tyre - Matt Rubber, Caliper - siena, Rotor - Carbon steel, Rim- Chrom plate.
89. Save the model as YUVARAJ_FRONT_TYRE.

Steps to be followed to create Rear Wheel:

1. Click on the new part and then selected the template which I had created earlier. (you can use default template as well if you don’t have any template created but make sure you are using MMGS format).
2. Go to: Insert > Reference Geometry > Axis. Select the FRONTPLANE REAR WHEEL and the Top Plane and select the “Two Planes” option.
3. Select the FRONTPLANE REAR WHEEL and create a sketch by clicking on the 2D Sketch icon. Create a vertical Construction line of length 273 from origin. Draw a horizontal line of length 320mm from the end point of vertical construction line. Draw one more horizontal line of length 310 mm at a distance of 20 mm from 320mm horizontal line.
4. Create a Revolve with the sketch created and select the axis created.
5. Create a New plane with offset distance 160 mm from Right Plane. Rename the new plane to MIDPLANE REAR WHEEL.
6. Create a Fillet of 5mm by selecting the inner surface of the revolve.
7. Create a new sketch on the MIDPLANE REAR WHEEL. Draw two construction circle of diameter 530 & 384.50. Draw a diagonal construction line with an angle of 30 Degree to Front Plane.
8. Draw a Spline with one midpoint from the end point of diagonal construction line to origin at a distance of 18 mm from origin towards the diagonal construction line. Midpoint of spline need to be on the 384.50 construction circle at a horizontal distance of 64.50 from starting point of spline. Close the sketch
9. Create a thin extrude with the help of above sketch. Direction 1 à Midplane à300 mm. Thickness à Midplane à 9 mm. Feature Scope all bodies and click ok.
10. Create a New Sketch on MIDPLANE REAR WHEEL. Draw a construction circle of diameter 530 mm. Draw a diagonal construction line with an angle of 10 Degree to Front Plane. Draw a Spline with one Midpoint from the end point of diagonal construction line to the origin. Close the Sketch.
11. Create a thin extrude with the help of above sketch. Direction 1 à Midplane à300 mm. Thickness à Midplane à 9 mm. Feature Scope all bodies and click ok.
12. Create a New Sketch on MIDPLANE REAR WHEEL. Draw 2 construction circle of diameter 403 & 389.50 mm. Draw a Centreline between the construction circle of 403 mm and Sketch3 of ExtrudeThin1. Connect the other side of the spline with Sketch4 of Extrude-Thin2. Draw another Centreline perpendicular at the midpoint of the first centreline of length 5 mm.
13. Create two 3 points Splines at the endpoints of the diagonal centreline. Connect the midpoint of the spline with the lower point of the perpendicular centreline.
14. Create a thin extrude with the help of above sketch. Direction 1 à Midplane à300 mm. Thickness à Midplane à 9 mm. Feature Scope all bodies and click ok.
15. Repeat 12, 13 & 14 steps with some variation in dimensions 298 & 286 mm.
16. Repeat 12, 13 & 14 steps with some variations in dimensions 194 & 183 mm.
17. Mirror the 3 Thin Features Created & Cut revolve over Front Plane.
18. Create a Circular Pattern of Mirrored Feature. Select the axis and Total angle is 360 and instances as 3. Check the Equal spacing option as well
19. Create a 2D Sketch on MIDPLANE REAR WHEEL. Draw a circle of diameter 90 mm. Close the sketch.
20. Extrude the sketch with a length of 300mm.
21. Create a 2D sketch on FRONTPLANE REAR WHEEL. Draw a vertical line from Top Plane above the origin and then two horizontal straight line from the start and end point of vertical line. The horizontal line near the origin end point be 25 mm away from the origin, the horizontal line above the origin end point be 150 mm away from the origin. Connect these two end points with a spline which has one midpoint.
22. Mirror the above sketch over the Midplane.
23. Create a Cut-Revolve over the axis and angle be 360 degree.
24. Create a Radius of 3 mm on web created.
25. Create a Sketch on MIDPLANE REAR WHEEL. Draw a circle of 60 mm.
26. Create a Extrude Cut of length 100 mm.
27. Create a New Sketch on Front Plane Rear Wheel. Draw a closed sketch at 253 mm away from origin from the end point of cut revolve with mid plane as centre and draw a spline from the end point of line to make it closed sketch.
28. Create a revolve about the axis select the angle as 360 degree.
29. Create a new sketch on the front plane. Draw a closed as shown in the below image.
30. Create a Revolve for the above sketch around the axis and select the angle as 360 degree.
31. Create a New plane at an offset distance of 105 mm from MIDPLANE REAR WHEEL.
32. Select the New plane and create a 2D Sketch and draw two circle of diameter 60 & 320
33. Create a extrude for the sketch created above of length 7mm.
34. Create a new sketch on new surface created, draw vertical construction line from the origin, Draw a circle of diameter 8 mm at 145 mm above the origin on the vertical construction line.
35. Create a Linear Pattern for the circle. Direction 1: X-Axis, Distance between the hole be 15 mm, Number of instances: 4 & Angle: 230 deg. Close the sketch
36. Select the Extrude Cut and sub option as UP TO NEXT.

37.Create a circular pattern for above Extrude CUT, Select the Axis 1, Angle: 360, Number of Instances: 14 and select the Equal spacing option.

38. Create a 2D Sketch on Front Surface of Extrude 8. Draw two Construction circle of radius 105 & 45 respectively. Draw a diagonal Construction line at a angle of 25 degree to the Front plane. Draw a line from smaller circle to bigger circle on the diagonal construction line and one more line which coincide with front plane. Join the two lines with the help of arc and make it closed sketch. Close the sketch.
39. Select the Extrude Cut and Sub option as UP TO NEXT.
40. Create a Fillet of 5 mm to the Corner Edges of the above Extrude Cut.
41. Create a Circular Pattern for the Extrude Cut & Fillet select the axis, no of instances be 9, Select the Equal spacing option.
42. Create a Fillet of 1 mm by selecting the front and back surfaces of Extrude 8.
43. Create a New Plane at a Offset of 3.5 mm from the midplane.
44. Create a new sketch on the plane created. Draw 2 construction circle of radius 90 & 180 respectively, Draw 2 diagonal construction lines from origin at an angle of 63 & 117 respectively. Make a Closed sketch on the intersection all construction elements.
45. Extrude the sketch with Sub option as Mid Plane and length as 30mm.
46. Create a Chamfer on the top and bottom surfaces of Extrude created. Select the Sub-option as Distance – Distance and dimension values be 6 mm & 20 mm.
47. Create a Fillet of 8mm on the corners.
48. Create a Fillet of 4mm on the edges.
49. Create a New Sketch for the creation of sprocket. Draw 2 circles of diameter 60 & 300 respectively.
50. Create an Extrude of thickness 15 mm.
51. Create a chamfer with sub option as angle distance and select the outer edge. The angle be 45 degrees and length be 4mm.
52. Create a sketch on the Front Surface of the above extrude. The sketch and dimensions as per the screen shot attached below.
53. Create an Extrude cut for the above sketch of thickness 15 mm.
54. Create a Fillet of 2.2 mm on the edges created Extrude cut.
55. Create a circular pattern for the Extrude Cut & Fillet. Instances 60, Total Angle 360 & Select the axis
56. Create a new sketch on front surface of extrude 7 and create a closed sketch as shown below
57. Create an Extrude Cut with sub option as up to next and click ok.
58. Create a Sketch on Front Face of the Extrude 7 and draw the below sketch.
59. Create a Extrude Cut for the above sketch and select the sub option as up to next.
60. Create a Fillet on the inner edges of value 1 mm.
61. Create a Circular pattern and select above two extrude cuts & Fillets, axis, angle be 360-degree, Number of instances as 7 and select the Equal distance option.
62. Create a 2d Sketch on the Front Plane. The sketch dimensions are details are in the below screen shot.
63. Create a Extrude Revolve about the axis 1.
64. Create a Fillet of 7mm to the edges of the Revolve feature.
65. Create a New Plane at an Offset of 400 mm to the Front Plane.
66. Create a 2D sketch on the New Plane Created and draw the below sketch.
67. Create Extrude Cut of depth 6 mm for the above sketch.
68. Create a new sketch on the New plane created refer below screen shot for more details.
69. Create Extrude Cut of depth 6 mm for the above sketch and click ok.
70. Create sketch on the new plane created. Refer the below screen shot for more reference about the sketch.
71. Create a Extrude cut of depth 6mm for the above sketch and click ok.
72. Create Fillet of radius 4 mm and click ok.
73. Create a Circular Pattern Select three extrude cuts and fillets and select the axis as axis1, Number of instances: 9 and angle: 360 and select Equal Spacing.
74. Change the appearances of the part. Select the body and change to light grey, Change the colour of tyre as dark grey, Change the brake calliper colour as brown.
75. Save the Part as Rear_Wheel_Name.

Steps to be followed to create Front Fork:

1. Create a 2d Sketch on the Front Plane. The sketch details are shown in the below image.
2. Create Revolve for the above sketch.
3. Create a New Plane at Offset distance of 60 mm to the Right Plane.

4. Create a 2d Sketch on the New Plane Created. The sketch details are shown below
5. Create Extrude for above sketch of thickness 40 mm and sub option as Blind.
6. Create New Plane on the Flat side of the above extrude created.
7. Create a Fillet of 5mm on the edges.
8. Create a Linear Pattern of the extrude & fillets. Number of instances: 2, Distance: 240mm.
9. Create a New sketch on the Mid Plane. The sketch details are shown below
10. Create a Extrude of the above sketch and select the sub option as up to next.

11. Create a 2D Sketch on the Flat surface of the mirror feature. Sketch details are shown below.
12. Create Extrude for the above sketch and select the Sub option as up to next.
13. Create New plane at a Offset distance of 48 mm to the front plane.
14. Create New Sketch on the New plane created the details of the sketch as shown below.
15. Create revolve for the above sketch by selecting the axis of rotation as straight line in the above image.
16. Create a Shell for the above revolve by selecting the circular surface.

17. Select the Plane 2 and create 2d Sketch. Refer the below screen shot for more details of the sketch.
18. Create a Revolve for the above sketch.
19. Create a Fillet of 3 mm on the edge of revolve.
20. Create a Dome on the revolve created surface and change the dimension as 7mm.
21. Create a Fillet of 1mm on the outer edge of the revolve.
22. Create a 2d Sketch on the surface of the first extrude created. Please refer to below Screen shot for more details of the sketch.

23. Create a new sketch on the Top plane. Refer to the below screen shot for more details about the sketch.
24. Create a 2d Sketch on the Front Plane. For more details about the sketch please refer below screen shot.
25. Create a Projected curve with the help of above sketch.
26. Create a New Plane. Reference 1: Projected curve. Reference 2: End point of the Projected Curve.
27. Create Swept Boss/Base with the help of Projected curve & Sketch created.
28. Create a 2d Sketch on the End surface of the Swept Boss/Base. The sketch is shown below.
29. Create new plane Reference 1: End surface of the Swept Boss/Base & change the angle to 90 degree. Reference 2: Sketch created above.
30. Create a sketch on the plane 3. The details of the sketch are shown below.
31. Create Revolve of the above sketch.
32. Create one more sketch on the Plane 3. The details of the sketch are shown below.
33. Create Revolve for the above sketch.
34. Create New Plane Reference 1: Plane 3 & 126 angle Reference 2: Axis created by above revolve.
35. Create sketch on the new plane created. Sketch details are shown in the below Screen shot.
36. Extrude the above sketch and depth be 15 mm. Sub option as Mid Plane.
37. Create a Fillet 5mm & 4mm on the new extrude created.
38. Create a 2D sketch on the extrude surface created. The details of the sketch as shown below.

39. Create Sketch on the top plane. The details of the sketch are shown below.
40. Create Sketch on the Right plane. The details of the sketch are shown below.
41. Create a Projected Curve with above sketches.
42. Create a Swept Boss/Base with the help of projected curve and sketch 14.
43. Mirror the Bodies (Sweep 2 & Dome) over the Midplane.
44. Create new plane Reference 1: Top Plane & Angle 59 Degree. Reference 2: Axis 3
45. Change the appearance to light grey of the part.
46. Change the appearance of brake line & Left and Right Handle to dark grey.
47. Save the File as Front_Fork_Name.

Steps to be followed to create Chassis:

1. Create a New part in Solidworks and change the name of Top plane as Bottom Plane Chassis, Front Plane as Mid Plane Chassis.
2. Select the Mid Plane Chassis and create a new sketch.
3. Add Picture to the Sketch. The location of sketch X: -930 mm; Y: -805 mm. Length of the Pic X: 3508 mm Y: 2480 mm.
4. Change the transparency of the image to 0.40 and select the Full Image.
5. Create a Sketch on the Mid Plane. The Details of the sketch shown below
6. Create a sketch on the Midplane. The Details of the sketch are shown below,
7. Create a Sketch on the Bottom plane. Draw a line and Spline as shown below.
8. Create a Projected Curve for sketch 2 & Sketch 3.
9. Create a Swept Boss/Base with the help of projected curve & Sketch 1
10. Mirror the sweep about the Mid plane.
11. Create a Sketch on the Right Plane. The details of the sketch as shown below
12. Create Extrude with the help of above sketch of thickness 22 mm and sub option as Blind.
13. Create a 2D sketch on the surface created. The details of the sketch as shown below.
14. Create Cut-Extrude with the help of above sketch and Select the sub-option as Up to Next.
15. Create a Chamfer on the bottom sharp edge created by Extrude. Sub option as distance distance D1: 90mm & D2; 44mm.
16. Create a Fillet for the sharp edges of the dimensions 25 mm. For more details refer to above image.
17. Create another fillet of dimension 50 mm. For more details refer to above image.
18. Create New Plane with reference as Mid Plane & vertex point of Fillet 1.
19. Create a 2d Sketch on the new plane created. More details of the sketch are given below.
20. Create the Flat extruded surface created and create a new sketch. Details of the sketch are shown below.
21. Create a Sweep Boss/Base with Sketch 6 & Sketch 7.
22. Create a 2D sketch on Plane 1. The details of the sketch are shown below.
23. Create a new sketch on the Flat surface of the extruded Boss. More details of the sketch are shown below.

24. Create a Sweep Boss/Base with the help of Sketch 9 & Sketch 8.
25. Create a sketch on the Plane 1. The details are shown below
26. Create Extrude for the above sketch. Select the sub-option as Midplane and length as 44mm.
27. Select the Flat surface of the above Extrude and create a new sketch. The Details of the sketch are shown below.
28. Create a Extrude of depth 223, Sub Option as Bind.
29. Create a Dome on the outside flat surface of extrude 3. Let the distance be 10 mm.
30. Create a sketch on the Mid plane. The details of the sketch are shown below.

31. Create a new plane. Reference 1: Right Plane, Reference 2: Vertex point of Sketch 12.
32. Create Sketch on the new plane created. The details of the sketch are shown below.
33. Create a Sweep Boss/Base with Sketch 12 & Sketch 13.

34. Create a New sketch on the Midplane. The sketch details are shown below
35. Create a extrude cut. Select the sub option as mid plane and distance be 60 mm.
36. Create a new Plane at a offset distance of 185 mm to the Bottom Plane.
37. Create a sketch on the new plane created. The details of the sketch are shown below.
38. Create a New sketch on the Mid Plane. The details of the sketch are given below
39. Create a Sweep Boss/Base with the help of sketch 15 & sketch 16.
40. Create a Sketch on the Mid plane. The details of the sketch are given below.
41. Create a Revolve Cut for the above sketch.
42. Create a New sketch on the mid plane. The details of the sketch are given below.
43. Create a revolve Boss/Base to the above sketch and select the construction line as axis of rotation.
44. Create a new sketch on the mid plane. The details of the sketch are shown below.
45. Create a Extrude with sub option as mid plane and length as 340 mm
46. Create a Fillet of radius 2mm to above extrude and revolve.
47. Create a New Plane at an offset distance of 165 mm to the mid plane.
48. Create a sketch on the new plane. The sketch details are shown below.
49. Create Extrude for the above sketch with sub option as mid plane and length as 10 mm.
50. Create a Fillet of 20 mm to over come sharp edge on the right top of the above sketch.
51. Create a Fillet of 1 mm to surface and created by above extrude.
52. Mirror the above Extrude and fillets created over the Midplane.
53. Create a Sketch as below and Create a Extrude of depth 40 mm with sub option as blind and enable the thin feature of thickness 8 mm.
54. Create a Fillet of 20 mm to the edges of the above extrude.
55. Create a Fillet of 3mm to sharp edges of the part.
56. Create a new sketch on the top surface of the thin extrude. The details of the sketch are shown below.
57. Create a Extrude Cut for the above sketch.
58. Create a New Plane at a Offset distance of 308 mm to the Bottom Plane.
59. Change the appearance of the part as Gloss Blue and save the part as Chassi_Yuvaraj

Steps to be followed to create Engine:

1. Create a New part and select the Front Plane to Create New Sketch. The details of the sketch as shown below.
2. Extrude the above Sketch and select the sub option as Blind and depth as 200 mm.
3. Create a New Plane with two reference. Reference 1: Front Plane, Reference 2: Mid-Point of the edge. Change the plane name as Mid Plane Engine
4. Select the Mid Plane Chassis and Create a 2D sketch and add Chopper image (Tools à Sketch Tools àSketch Picture). X position: -1493 mm; Y position: -965 mm; Distance in X direction: 3508 mm; Distance in Y direction: 2480 mm. Change the Transparency of the image as 0.40.
5. Create a 2D Sketch on the above created Extrude surface. The details of the sketch are shown below.
6. Create a Extrude of above Sketch with sub option as Blind and depth as 50 mm.
7. Create a 2D sketch on the surface of new Created Extrude. Create a Sketch as shown below.
8. Create Extrude with the help of above sketch. Sub option as Blind and thickness as 40 mm.
9. Create a 2D sketch on the midplane. The sketch Details are shown below
10. Create Extrude with the help of above sketch. Sub option as Mid plane and depth as 150 mm.
11. Create a Fillet of 50 mm to the above Created surface.
12. Select the Right plane and create 2D sketch as shown below.
13. Create a Revolve to the above sketch.
14. Create a new plane Parallel to the Right Plane, select a vertex point of the Extrude 1.
15. Create a New Sketch on the New Plane created. The sketch details are shown below.
16. Create a revolve with the help of above sketch.
17. Create a 2D sketch on the above created surface. The sketch details are shown below.
18. Create a circular pattern of the above sketch. Distance between instances be 40.
19. Repeat above two steps on other revolve.
20. Create a Cut-Extrude with sub option as blind. Change the distance to 88 mm.
21. Create a Dome on the outer surface and change the distance to 10 mm.
22. Create a new plane at a offset distance of 250 mm to the Mid plane.
23. Create new sketch on the new plane created. The Sketch details are shown below.
24. Create a circular pattern. No of instances be 12. For more details refer to below screen shot.
25. Create a Cut-Extrude. Direction: offset from surface, Distance: 3 mm; please select the surface offset option.
26. Repeat the above steps on other Revolve as well.
27. Create a Cut -Extrude. Direction: offset from surface, Distance: 3 mm; please select the surface offset option.
28. Create a Chamfer with Angle Distance option (3mm , 45 degree).
29. Create a surface fillet of radius 1 mm.
30. Create a Sketch on the Mid Plane. The details of the sketch are shown below.
31. Create Extrude for the above sketch, Sub Option as Midplane and distance as 150 mm.
32. Create a new sketch on the mid plane as shown below. Please refer to below screen shot for more information.
33. Create a Extrude with sub option as mid plane and length be 110 mm.
34. Create a new sketch on the Mid Plane. The Details of the sketch are shown below.
35. Create Extrude with sub option as Mid Plane and length as 100 mm.
36. Create a new sketch on the top surface of the above extrude. The details of the sketch are shown below.
37. Create Extrude with sub option as Blind with a length of 8 mm.
38. Create a Chamfer with sub option as distance distance. D1=30 mm; D2= 240 mm.
39. Create a new sketch on the top surface of above extrude and use convert entities option. Please refer to below screen shot for more information.

40. Create Extrude for the above sketch with the sub option as Blind. Depth as 125 mm.
41. Create Chamfer with sub option as distance distance D1: 90 mm; D2: 15 mm.
42. Create Fillets of radius 15 mm to the edges created by the extrude
43. Create a New plane parallel to top surface of the above extrude at a offset distance of 315 mm towards origin.
44. Create Sketch on the new plane. The details of the sketch are shown below.
45. Create Cut Extrude with the help of above sketch with sub option as Blind and thickness be 8mm.
46. Create Fillets of radius 10 mm to the edges created by extrude cut.
47. Create Linear pattern of Extude Cut and fillets features. No of Instances: 14; Distance 16 mm. select the edge which is parallel to the direction of extrude.
48. Create a Fillet of 2mm by selecting the surfaces created by Extrude Cut.
49. Create 2D sketch on the mid plane. Create a arc as shown in the below screen shot.
50. Create Extrude Cut with the help of above sketch. Direction 1 as mid plane and select through all option for direction 1 & direction 2. Enable the Thin Feature direction: One-Direction and be the thickness as 0.5 mm.
51. Create a Fillet of radius 10, 8 & 5mm.
52. Create a 2D sketch on the surface and sketch details are shown below.
53. Create a Extrude with the help of above sketch with sub option as Blind and distance be 2 mm.
54. Create fillets of radius 10 mm to the edges of the extrude created above.
55. Create a Dome to the open surface of the above extrude.
56. Mirror the above features Extrude, Fillets & Dome over mid plane.
57. Create a 2D sketch on the Mid Plane. The sketch details are shown below.
58. Create Extrude with help of above sketch. Sub option as Mid Plane and distance be 20 mm.
59. Create Fillet to the edges created by above extrude. The fillet radius be 10 mm.
60. Mirror the above body over the Right Plane.
61. Create a Fillet of radius 25 & 4 mm.
62. Create new sketch on the bottom of the part. The details of the sketch are shown below.
63. Create a Extrude Boss/Base with sub option as blind and distance be 50 mm.
64. Create a New Sketch as shown below.
65. Create a Extrude with sub option as blind and distance be 12 mm.
66. Create fillet of radius 5 mm to the edges.
67. Create a New sketch as shown below.
68. Create Extrude with sub option as blind and distance be 85 mm.

69. Create New Sketch as shown below.
70. Create Extrude with sub option as blind and distance be 15 mm.
71. Create two chamfers with sub option as Angle distance. Distance: 4mm; Angle: 45 degree.
72. Create New Sketch as shown below.
73. Create Extrude with sub option as up to next.
74. Create fillet of radius 2.20 mm to the edges created
75. Create Circular pattern with extrude & Fillet No of instances: 21; Total angle: 360 Degree.
76. Create Chamfer with sub option as distance - distance on the spindle D1: 24 mm; D2: 75 mm.
77. Create Chamfer with sub option as Angle – distance Angle: 45 Degree D1: 5 mm.
78. Create New Sketch as shown below.
79. Create New Sketch as shown below.
80. Create Sweep Boss/Base with the help of above two sketches.
81. Create New Sketch on the Mid Plane as Shown below.
82. Create New Plane at a Offset Distance of 350 mm to the top plane.
83. Create New sketch on the New Plane Created as shown below.
84. Create Sweep Boss/Base with the help of above two sketches.
85. Create New Sketch on the Plane 6. Details of the sketch are shown below.
86. Create Revolve with the help of above sketch.
87. Create Fillet of radius 2mm to the edges.
88. Create new sketch on top plane as shown below,
89. Create Cut-Extrude with sub option as Offset from surface and change the distance as 1mm.
90. Create Circular Pattern with No.of instance as 30 Degree, Angle: 360 Degree.
91. Create New Sketch as shown below.
92. Create New Plane as shown below.