Design of rear wheel and front fork

REAR WHEEL

RIM

• Open Part model>Select Unit system as MMGS
• Rename the pales as follows:

1. Front Plane > MidPlane RWheel (Referred as midplane)
2. Top Plane > Centre RWheel (Referred as centre plane)
3. Right Plane > Front RWheel (Referred as a front plane)

• Outer Rim and Hub: Select Front RWheel and sketch as follows: Draw a horizontal midpoint line of 300mm with the midpoint at the origin. Complete a rectangle of breadth 45mm with the midpoint line as one of its sides. Draw another horizontal midpoint line of 320mm with its midpoint at 273mm vertically above the origin. Draw two lines of equal length from the ends of the midpoint line inclined towards the midpoint, downwards at an angle of 75 deg with the midpoint line. Draw a three-point arc from the ends of inclined lines of radius 600mm. Centre of the arc is vertical with the origin and vertical distance between the midpoint line and the midpoint of the arc is 40mm. Apply a fillet of radius 5mm at the ends of the arc.
• Revolve extrude the above sketch and use line at the origin as the axis of revolution.
• Spoke: Start a sketch on MidPlane RWheel. Draw an arc of radius 265mm concentric with the hub. Draw a vertical construction line between the origin and the midpoint of the arc. Draw another construction line between the origin and end of the arc and at an angle of 31 deg with the vertical construction line. Draw a horizontal line of length 22.5mm at the origin. Draw a spline between the ends of the horizontal line and the arc. The spline is made vertical at the lower end and given a dimension of 300mm. Mirror the spline about the vertical construction line.
• Extrude the above sketch about the midplane for a depth of 300mm and don’t merge yet.
• Start a sketch on the midplane. Convert the outer edge of the spoke and offset the remaining edges for an offset of 9mm. Trim out the unwanted extra lines. Draw two vertical construction lines, between the offset entities and the actual edges of the spoke, with 9mm apart from each other and the nearest line is at horizontally 2.5mm from the origin. Draw a vertical construction line between the origin and the midpoint of the arc (outer edge of a spoke). Draw another construction line between the arc and the origin at an angle of 9 deg with the vertical construction line. Draw a spline between the upper end of the nearest construction line (small lines between the offset entities and the edges) and the upper end of the 9 deg construction line, another spline from the other upper end of the construction line to a point on the arc. Upper ends of spline are at 9mm apart. Splines are made vertical and given weight as 300mm at the lower end. Mirror these splines about the vertical construction line.
• Make an extrude cut from the above sketch only on the spoke (not on the hub) up to the vertices of spoke on both sides of the sketch plane.
• Start a sketch on the midplane. Draw three construction circles of diameter 194mm, 298mm and 403mm. Offset the edges of spokes (Formed from the extruded cut) to their respective centres, use offset distance as 4.5mm. Trim the offset curves and the circles accordingly to obtain three sets of reference intersection points (i.e. set1 as intersection points of the outer circle, set2 from the circle of 298mm dia and set3 from the circle of 194mm dia). Each set has 4 reference points. Three continuous arcs of radius 75mm are drawn between the reference points of set1, three continuous arcs of radius 25mm are drawn at set2. Another three continuous arcs of 15mm, 20mm and 15mm radii are drawn at set3 reference points. Offset these 3 sets of arcs (Includes 9 arcs) to a distance of 8mm towards the origin. Trim out the unwanted protrusions and form three closed profiles using line command.
• Make extrude from the above sketch on the spoke up to the vertices of spoke on both sides of the sketch plane.
• Start a sketch on Front Plane. Draw a construction intersection curve from the inner face of the rim (Arc). Draw a line tangent to the arc to the edge of the rim, continue with a vertical line till the origin, a horizontal line up to a point 25mm horizontal to the origin. Draw a spline and close the profile, make spline vertical at lower end and tangent to the line at the upper end. Give the line weight of spline as 200mm at both ends of the spline. Mirror the closed profile about the y-axis. Remove the unwanted and extra line and curves.
• Make a revolve cut of the above sketch with use of temporary axis.
• Circularly pattern the spoke accordingly for 3 instances and combine the spokes, hub and outer rim bodies to form a rim with the hub.
• Apply a fillet of radius 3mm to the faces of the spoke and the hub on both sides.
• Make a cut-out of dia 60mm at the centre of the hub and make a slot for an axle.
• Axle: Start a sketch on the front plane as follows: a horizontal construction line of 25mm at the origin, a vertical line of 30mm, a line of 225mm along +ve X-axis, a13mm vertical line, a line of 225mm along –ve X-axis. Draw a line of 90mm collinear with the construction line along –ve X-axis. Close the sketch with a spline between the ends of both horizontal lines accordingly. The spline is made tangent to the line at the top end, weight is 50mm and at the lower end, 45deg with horizontal, 125mm line weight is given.
• Revolve extrude the above sketch about the horizontal construction line.
• Combine the axle with rim body, Check for rebuild errors and apply Chromium plate as material.

BRAKE ROTOR

• An offset extrude of a contour between a converted entity of outer cylinder of the axle and 320mm dia circle, made on Midplane, and is extruded with 7mm thickness at an offset distance of 105mm from MidPlane and don’t merge.
• Holes: Sketch on the face of the rotor as follows: draw a circle of dia 8mm at 145mm vertically above the origin. Linear pattern the circle for four instances with 15mm spacing and are aligned at 230 deg anti-clockwise with +ve X-axis. This sketch is used to make a cut-out from the rotor.
• Circularly pattern this cut-out for 14 instances around the rotor with equal spacing.
• Cut-outs: Draw two circles C1, C2 of dia 90mm, 210mm on the face of the rotor. Draw 2 lines collinear with the origin, one line vertical and another line at 25 deg with the vertical line. Trim the extra portions of the circle and the lines. Apply sketch fillet of radius 5mm to all the corners and keep these corners constrained. Make a cut-out of this sketch through the entire rotor only, not through the whole body.
• Circularly pattern this for 9 instances with equal spacing on the rotor.
• Check for rebuild errors and apply Carbon Steel as material.

BRAKE CALLIPER

• Start a sketch on the face of the brake rotor as follows: Draw two circles C3, C4, centre at the origin, and are of dia 180mm, 360mm. Draw two lines, collinear with the origin, which are at 54 deg with each other. One line is kept at 63 deg with the vertical axis so that both lines will be symmetric with the horizontal axis. Trim out the unwanted portions of the circles and the lines.
• Extrude the above sketch at an offset of 3.5mm back into the brake rotor, with midplane option and depth of 30mm and don’t merge to obtain separate bodies.
• Chamfer: Apply asymmetric chamfer with D-D option and distances are 6mm, 20mm to the faces of the extrude of the calliper as desired.
• Fillet: Apply a fillet of 8mm radius to the two outer corners of the calliper. Apply another fillet of 4mm radius to the calliper at the edges of the chamfer.
• Check for rebuild errors and apply Siena painted car as the material.

SPROCKET

• An offset extrude of a contour between a converted entity of outer cylinder of the axle and 300mm dia circle, made on the face at the end of the axle, and is extruded with 15mm thickness towards the midplane and don’t merge.
• Sprocket teeth: make an angle- distance (A-D) chamfer with 4mm distance and 45 deg angle at the end of the plate on both sides.
• A cut-out is made at the chamfered edges to form the slots as teeth of the sprocket. A cut-out is made only to the sprocket and the following sketch is used to make this.
• A horizontal midpoint line of 17mm with its midpoint vertical to the origin, A downward arc of radius 4.5mm centred at 144.5mm vertical to the origin, 15mm vertically below the midpoint of the line and the ends of the arc are horizontal. Two lines of equal length are drawn in between the ends of the midpoint line and the ends of the arc. These two lines are made tangent to the arc. This sketch is used for cut-out as mentioned above. Apply a fillet of 2.2mm radius to the upper edges of the cot-out just made.
• Circularly pattern the cut-out and the fillet around the sprocket for 60 instances.
• Cut-out: Using circles two cut-outs are made from the sprocket. Sketch for 1^st cut-out is as follows: two circles are drawn of dia 90mm, 255mm centred at the origin. Another circle of dia 203mm is drawn at (x, y) = (50, 35), Trim the portions of 203mm dia circle accordingly and offset for 12mm distance downward. Extend and trim the required portions of all these arcs accordingly. Sketch for 2^nd cut-out is as follows: two circles are drawn of dia 172mm, 255mm centred at the origin. Another circle of dia 135mm is drawn at (x, y) = (50, 35), Trim the portions of 135mm dia circle accordingly and offset for 12mm distance upward. Extend and trim the required portions of all these arcs accordingly.

• Fillet the edges of inner faces of the cut-outs for 1mm radius. Circularly pattern these cut-outs and fillets around the sprocket for 7 instances.
• Check for rebuild errors and apply Carbon steel as the material.

TYRE

• Select the front plane and sketch as follows: Convert the intersection curve of the outer face of the rim as an entity. Draw two equal lines inclining outward from the ends of the converted entity (Line). Outer ends of these lines are 354mm apart from each other and are in horizontal relation at 303mm vertical distance. A three-point arc of radius 366mm is drawn from the ends of these lines. Sketch fillet of radius 7mm is applied to the corners at the ends of the arc and corners are kept constrained.
• Revolve the above sketch accordingly around the rim and don’t merge, to obtain a separate solid body.
• Threads: To produce threads a sketch is made on the front plane. This sketch has four 3- point centre rectangles and the details are as follows. Say the rectangles as R1, R2, R3 and R4. R1, R3 rectangles are equal with length 97mm and breadth 8mm. R2, R4 rectangles are equal with length 280 mm and breadth 8mm i.e. breadth of all four rectangles is equal.
• A horizontal construction line is drawn along –ve X-axis from the origin. R1, R2 are inclined at 40 deg with the horizontal construction line, whereas R3, R4 are inclined at 140 deg. Say P1, P2, P3 and P4 are the top-most points of these rectangles and their position concerning the origin is given as follows:
  • (X₁, Y₁) = (-110, -10), (X₂, Y₂) = (30, 0), (X₃, Y₃) = (111, 110), (X₄, Y₄) = (-30, 121).
• One more set of two rectangles are drawn on the front plane, say R5, R6. Length and breadth of R5 rectangle are 170mm, 8mm. Similarly, the length and breadth of the R6 rectangle are 158mm, 8mm. The lower short side of R5, R6 are collinear with the upper long sides of R2, R4 rectangles at a distance of 30mm from P2, P4 points.
• A cut-out is made from the above sketch at an offset distance of 400mm and options at direction1, offset from the surface with 6mm offset distance and outer face of the tyre is selected as surface, under feature scope the only tyre is selected as the body to cut. Full round fillet feature is applied on ends of the inner faces of the threads formed from R1, R2, R3 and R4 rectangles.
• Circularly pattern the threads along with the fillets for 9 instances with equal spacing around the tyre and select tyre as the body under feature scope option.
• Check for rebuild errors and apply Matte rubber as the material. Save the file.

FRONT FORK

• Open Part model>Select Unit system as MMGS
• Rename the pales as follows:

1. Front Plane > MidPlane FFork (Referred as midplane)
2. Top Plane > Front FFork (Referred to as a top plane)
3. Right Plane > Right FFork (Referred as a right plane)

• Create a new plane from midplane at an offset distance of 105mm named as Side plane FFork (Referred as Side plane).
• Start a sketch on the side plane and start a horizontal line of 1330mm from the origin, continue with a vertical line of 30mm, continue a horizontal line to a point (-505, 30) w. r. t the origin, continue a line to a point (-485, 25) w. r. t the origin, continue a horizontal line till (-50, 25) w. r. t the origin and close the sketch at the origin.
• Revolve the sketch about 1330mm line.
• Start a sketch on the flat face of the fork tube. Convert the face to a circle and draw another circle of dia 75mm concentric with the first circle. Draw another circle of dia 80mm centred at (105, 100). Draw a vertical line from the top quadrant point of 3^rd circle up to 24mm below the origin and continue with a horizontal line up to the 2^nd Draw another line between the top quadrant point of 2^nd circle and the right quadrant point of 3^rd circle. Trim the unwanted sketch.
• Select the appropriate contour and make an extrusion of handle clamp onto the fork tube at an offset distance of 20mm with 40mm depth and don’t merge. Fillet the edges of clamp accordingly with 5mm radius and make sure not to fillet the mirror face (face on the midplane). Don’t merge with fork tube.
• Linearly pattern the clamp along with fillet for 2 instances with 240mm spacing in the direction of fork tube.
• Start a sketch on the side plane and draw a circle of dia 40mm. Centre of this circle is at 70mm along –ve X-axis from the origin. Extrude the circle up to the midplane and merge with the fork tube only.
• Select the upper face of the second clamp and start a sketch of a circle with 50mm dia concentric with the edges formed from 80mm dia arc of the clamp, draw a line along the edge of the clamp at the midplane and trim out the portions of the sketch to create a semi-circle. Make an extrusion of this sketch between the adjacent faces of both clamp plates and merge them with the clamp.
• Create a sketch on the side plane as shown in the following image using 2 lines, a three-point arc.

• Revolve the sketch about the long line as the axis of revolution to form a headlight bucket. Create a sketch on the flat face of the light bucket i.e. offset the flat face of the light bucket inwards to 4mm distance and make an inward draft cut-out for a depth of 10mm with draft angle as 5 deg. Apply dome feature with dome radius as 7mm on the bucket at the flat face formed from the cut-out.
• Using convert intersection entities feature, a sketch as shown below is drawn on the side plane and a revolve cut is made in the light bucket with help of temporary axis of the light bucket as its axis of revolution. Apply a fillet of 3mm, 1mm radius to the edges of light bucket accordingly. Move the whole light bucket body for a distance of 48mm along the –ve Z direction.

• Start a sketch on the top face of the 1^st clamp and draw a circle (Say handle circle) of 35mm dia centred at 50mm horizontal to the midplane and 24mm vertical to the horizontal face of the clamp. On the side plane, draw a line and the ends of this line are at (-302,-273) and (-226,-96) w. r. t the centre of the handle circle. Draw a spline between the upper point of the line and the centre of handle circle. The spline is made tangent to the line at the lower end with 200mm line weight, at upper-end spline is made horizontal and line weight is given as 425mm. Start a sketch on the front plane and make a construction line by converting the line from the previous sketch. Draw a spline between the centre of handle circle (Snap point of the centre on the front plane) and to a point that is 119mm vertically above the far end of the construction line. The spline is made horizontal at the lower end and line weight is given as 300mm.
• Using project curve, with the sketch on sketch option, a curve is formed from both of the previous two sketches. This curve is used as a guide path. Create a sweep of the handle circle with the curve (created using project curve) as the guide curve and merge with clamps.
• Create a new plane, say plane1, at end face and midsection of the handlebar. On this plane, a sketch is made as follows: A vertical line of 154mm from the centre of handlebar, continue with an arc of radius of 100mm and its end at (24, 118) from the start point, draw three continuous arcs of radius 35mm from the end of the 100mm arc and the ends of these three arcs are in vertical relation and the vertical distance between these ends of arcs is of equal length, draw another line from the end of the 3^rd arc up to the edge of the handle with its vertical dimension as 10mm and close the sketch with a horizontal line.
• Make a revolved extrusion of the above sketch about the line of 154mm as its axis of revolution to create the handle grip and merge this only with the handlebar.
• Draw a rectangle of 55mm length and 25mm breadth on the plane1 and one end of its length is 15mm vertically below the centre of the handlebar. Make a revolved boss from the rectangle around the handlebar accordingly and merge with a handlebar to form the lever ring.
• Create a new plane say plane2, with plane1 as first reference and the temporary axis of lever ring as a second reference, the angle at first reference is given as 160 deg and its normal is flipped.
• Sketch on plane2 for the lever is as follows: A horizontal construction line of 15mm is drawn at centre lever ring from its right end. From the other end of the construction line, a horizontal line is drawn to the left edge of the lever ring’s midpoint. Continue with a line of 84mm at 60 deg angle, a 175mm horizontal line, a small line at 70 deg with –ve X-axis. Draw a line of 54mm from the endpoint of the construction line which is at 105 deg with –ve X-axis and continue with a line which is at 109 deg with the above line. Trim out the extra portions of the line and make sure the profile thus formed is a closed one.
• Extrude the above sketch with midplane depth of 15mm and merge with the handlebar. Apply fillets of radii 25mm, 5mm and 4mm as required to obtain a clean finish.
• To draw cable, a sketch of 9mm dia circle (Say cable circle) is made on a face of the cable as shown in the figure.

• Two curves are drawn from the centre of the cable circle and up to a point on the upper clamp such that cable is in between the handlebar and the fork end. One curve is on the front plane and the other is on the right plane and their dimensions and relations are given as below figures.

• From these two curves, another curve is obtained through projecting the curve with the sketch on sketch option and the thus formed sketch is used as a guide curve for sweep to produce the cable.
• Apply material as follows to the bodies: Apply Chromium plate to all bodies as most of them will be using it. Modify material of handgrip and cable to glossy rubber material. Then modify dome and cut-out faces (Chamfer look-a-like) to area light of luminous density of 1 w/srm².
• Check for rebuild errors and mirror all bodies about midplane and don’t merge bodies.
• Combine both fork tubes, axle to a single body, Combine Clamps, handgrips, levers, rings and cables to a single body.
• Create a suitable view for the body and check for rebuild errors and then save the file.