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Rear Wheel
Open a new part with model units set to millimeters.
Go to: File > New > Part
Select the three planes in the feature tree and make them visible by clicking on the glasses.
Change the name of the Front Plane Double click on the Front Plane in the feature tree. Change the name into: FRONTPLANE REAR WHEEL
Create an axis Go to: Insert > Reference Geometry > Axis Select the FRONTPLANE REAR WHEEL and the Top Plane and select the “Two Planes” option. Click OK
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Create a sketch on the FRONTPLANE REAR WHEEL by clicking on the 2D Sketch icon Draw the sketch as shown in the picture. Ensure that the construction line
starts at the Origin.
Create a revolve Go to: Insert > Boss/Base > Revolve Axis of revolution
: Select the new Axis1
Click OK
Create a new plane parallel at the Right Plane Go to: Insert > Reference Geometry > Plane Select the Right Plane. Change the Offset Distance
into 160 mm.
Ensure that the offset is directed to the middle of Revolve1. If not, click “Reverse direction” Click OK Double click on the new Plane1 in the feature tree and change the name into “MIDPLANE REAR WHEEL”. Create a sketch on the MIDPLANE REAR WHEEL Draw the circle as shown in the picture. Create an extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into 150 mm
Click OK | Page
Create fillets on the edges of the green surface Select the green surface as shown in the picture. Go to: Insert > Features > Fillet/Round
> 5 mm
Click OK
Select the “MIDPLANE REAR WHEEL” and create a new sketch Draw the spline
as shown in the picture.
Use the SolidWorksModel part as reference file if the 2D sketch is unclear to you (Extrude-Thin1, Sketch 3).
Create a thin extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into: 300 mm
Select the Thin Feature option. Direction: Midplane Change
into: 9 mm
Feature Scope: All bodies Click OK
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Select the “MIDPLANE REAR WHEEL” and create a new sketch Draw the spline
as shown in the picture.
Make sure that the spline is constructed out of three points. The midpoint is just below the upper point of the spline as shown in the detail.
Detail Use the SolidWorksModel part as reference file if the 2D sketch is unclear to you (Extrude-Thin2, Sketch 4).
Create a thin extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into: 300 mm
Select the Thin Feature option. Direction: Midplane Change
into: 9 mm
Feature Scope: All bodies Click OK | Page
Make the sketches of Extrude-Thin1 and Extrude-Thin2 visible Click on the
before Extrude-Thin1 in the feature tree.
Select: Sketch3 > Right mouse click > Show Repeat this action for Sketch4 The sketches are visible now. Select the “MIDPLANE REAR WHEEL” and create a new sketch. Draw a construction
circle with a diameter of 403 mm.
Start a spline at the intersection point between the construction circle and Sketch3 of Extrude-Thin1. Connect the other side of the spline with Sketch4 of Extrude-Thin2 as shown in the orange circles in the picture.
Draw the sketch and add the dimensions. Create a thin extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into: 300 mm
Select the Thin Feature option. Direction: Midplane Change
into: 9 mm
Feature Scope: All bodies Click OK | Page
Select the “MIDPLANE REAR WHEEL” and create a new sketch Draw a construction
circle with a diameter of 298 mm.
Start a spline at the intersection point between the construction circle and Sketch3 of the Extrude-Thin1. Connect the other side of the spline with Sketch4 of Extrude-Thin2 as shown in the orange circles in the picture.
Draw the sketch and add the dimensions. Create a thin extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into: 200 mm
Select the Thin Feature option. Direction: Midplane Change
into: 9 mm
Feature Scope: All bodies Click OK | Page
Select the “MIDPLANE REAR WHEEL” and create a new sketch Draw a construction
circle with a diameter of 194 mm.
Start a spline at the intersection point between the construction circle and Sketch3 of Extrude-Thin1. Connect the other side of the spline with Sketch4 of Extrude-Thin2 as shown in the picture.
Draw the sketch and add the dimensions. Create a thin extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into: 200 mm
Select the Thin Feature option. Direction: Midplane Change
into: 9 mm
Feature Scope: All bodies Click OK | Page
Create a new sketch on the FRONTPLANE REAR WHEEL Draw the sketch as shown in the picture. Make sure that the spline is constructed out of three points. The midpoint is just below the upper point of the spline as shown in the detail. Mirror the spline around the vertical construction line in the middle of the sketch. Use the SolidWorksModel part as reference file if the 2D sketch is unclear to you (Cut-Revolve1, Sketch 8). You could change the shape of the spline by dragging at the tangency arrows. Design a curve you like.
Detail Create a revolved cut Go to: Insert > Cut > Revolve Axis of revolution
: Select Axis1
Click OK | Page
Mirror the spoke of the rim
Go to: Insert > Pattern/Mirror > Mirror Mirror Face/Plane
: FRONTPLANE REAR WHEEL
Features to Mirror
: Extrude-Thin1, Extrude-Thin2, Extrude-Thin3, Extrude-Thin4, Extrude-Thin5, Cut-Revolve1
Click OK
Create fillets at the edges of the green surfaces Select the two green surfaces at the front and back of the rim as shown in the picture. Go to: Insert > Features > Fillet/Round > 3 mm
Click OK | Page
Create a circular pattern
Go to: Insert > Pattern/Mirror > Circular Pattern Pattern Axis
: Axis1
Total Angle
: 360 deg.
Number of instances
:3
Select the “Equal Spacing” option. Features to Pattern
: Extrude-Thin1, Extrude-Thin2, Extrude-Thin3, Extrude-Thin4, Extrude-Thin5, Cut-Revolve1, Mirror1
Click OK
Select the “MIDPLANE REAR WHEEL” and create a new sketch Draw the sketch as shown in the picture.
Create an extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into 100 mm
Click OK
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Select the “FRONTPLANE REAR WHEEL”
and create a new sketch
Draw the sketch as shown in the picture.
Create a revolve Go to: Insert > Boss/Base > Revolve Axis of revolution
: Select Axis1.
Click OK Select the “FRONTPLANE REAR WHEEL”
and create a new sketch
Draw the sketch in the center of the rim as shown in the picture.
Create another revolve Go to: Insert > Boss/Base > Revolve Axis of revolution
: Select Axis1
Click OK
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Create a new plane parallel at the MIDPLANE REAR WHEEL Go to: Insert > Reference Geometry > Plane Select the “MIDPLANE REAR WHEEL”. Change the Offset Distance
into 105 mm.
Ensure that the offset is directed outwards. If not, click “Reverse direction” Click OK
Create a sketch on the new Plane2 Draw the sketch as shown in the picture.
Create an extrude Go to: Insert > Boss/Base > Extrude Change
into: 7 mm
Ensure that the extrusion is directed outwards. If not, click “Reverse direction” Click OK
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Create a new sketch at the front surface of the new Extrude8 Draw the sketch as shown in the picture. Start with a vertical construction line and a circle with a diameter of 8 mm as shown in the detail.
Detail Create a linear pattern sketch Go to: Tools > Sketch Tools > Linear Pattern Direction 1
: X-axis
Change
into: 15 mm
Number
:4
Angle
: 230 deg
Entities to Pattern
: Select the circle.
Click OK
Create an extruded cut Go to: Insert > Cut > Extrude Direction 1
: Up To Next
Click OK
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Create a circular pattern Go to: Insert > Pattern/Mirror > Circular Pattern Pattern Axis
: Axis1
Total Angle
: 360 deg.
Number of instances
: 14
Select the “Equal Spacing” option. Features to Pattern
: Extrude9
Click OK
Create a new sketch at the fr ont surface of Extrude3 Draw the sketch as shown in the picture.
Create an extruded cut Go to: Insert > Cut > Extrude Direction 1
: Up To Next
Click OK
Create fillets at the edges of Extrude10 Select the four green edges as shown in the picture. Go to: Insert > Features > Fillet/Round > 5 mm Click OK
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Create a circular pattern Go to: Insert > Pattern/Mirror > Circular Pattern Pattern Axis
: Axis1
Total Angle
: 360 deg
Number of instances
:9
Select the “Equal Spacing” option. Features to Pattern
: Extrude10, Fillet3
Click OK
Create fillets at the edges of the green surfaces Select the two green surfaces at the front and back of the brake disk as shown in the picture. Go to: Insert > Features > Fillet/Round > 1 mm Click OK
Create a new plane parallel at Plane2 Go to: Insert > Reference Geometry > Plane Select “Plane2”. Change the Offset Distance
into 3,5 mm.
Ensure that the offset is directed to the “MIDPLANE REAR WHEEL”. If not, click “Reverse direction” Click OK | Page
Create a new sketch at Plane3 Draw the sketch as shown in the picture.
Create an extrude Go to: Insert > Boss/Base > Extrude Direction 1 Change
: Midplane into: 30 mm
Click OK
Create chamfers on the edges of the green surface Select the surface as shown in the picture. Go to: Insert > Features > Chamfer Select the Distance - distance option. Change
into: 6 mm
Change
into: 20 mm
Select the “Select trough faces” option. Select the “Tangent propagation” option. Click OK Repeat this action at the other side of Extrude6 | Page
Create two fillets Select the edges as shown in the picture. Go to: Insert > Features > Fillet/Round
> 8 mm
Click OK
Create fillets on the green edges Select the edges as shown in the picture. Go to: Insert > Features > Fillet/Round
> 4 mm
Click OK
Change the color of the brake caliper: Select the features of the brake caliper (Extrude11, Chamfer1, Chamfer2, Fillet5, Fillet6) > Right click > Feature Properties > Color > Change color > Select the color you like Create a new sketch
on the green surface of Revolve3
Draw the sketch as shown in the picture.
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Create an extrude Go to: Insert > Boss/Base > Extrude Direction 1
Change
: Blind (Ensure that the offset is directed outwards) into: 15 mm
Click OK
Create chamfers on the edges of Extrude12 Select the two green edges as shown in the picture. Go to: Insert > Features > Chamfer Select the Angle - distance option. Change
into: 4 mm
Change
into: 45 deg
Select the “Select trough faces” option. Select the “Tangent propagation” option. Click OK
Create a new sketch at the front of Extrude7 Draw the sketch as shown in the picture and detail.
Detail
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Create an extruded cut Go to: Insert > Cut > Extrude Direction 1 Change
: Blind : 15 mm
Click OK
Create two fillets at the green edges Select the two edges as shown in the picture. Go to: Insert > Features > Fillet/Round
> 2,2 mm
Click OK
Create a circular pattern Go to: Insert > Pattern/Mirror > Circular Pattern Pattern Axis
: Axis1
Total Angle
: 360 deg.
Number of instances
: 60
Select the “Equal Spacing” option. Features to Pattern
: Extrude13, Fillet7
Click OK | Page
Create a new sketch
on the front of Extrude12
Draw the sketch as shown in the picture.
Use the SolidWorksModel part as reference file if the 2D sketch is unclear to you (Extrude14, Sketch 18).
Create an extruded cut Go to: Insert > Cut > Extrude Direction 1
: Up to next
Click OK | Page
Create another sketch
on the front of Extrude12
Draw the sketch as shown in the picture.
Use the SolidWorksModel part as reference file if the 2D sketch is unclear to you (Extrude15, Sketch 19). Create an extruded cut Go to: Insert > Cut > Extrude Direction 1
: Up to next
Click OK | Page
Create fillets at the green surfaces and edges Select the green edges and surfaces as shown in the picture. Go to: Insert > Features > Fillet/Round
> 1 mm
Click OK
Create a circular pattern Go to: Insert > Pattern/Mirror > Circular Pattern Pattern Axis
: Axis1
Total Angle
: 360 deg.
Number of instances
:7
Select the “Equal Spacing” option. Features to Pattern
: Extrude14, Extrude15, Fillet8
Click OK Select the “FRONTPLANE REAR WHEEL” a new sketch
and create
Draw the sketch as shown in the picture.
Create a revolve Go to: Insert > Boss/Base > Revolve Axis of revolution
: Select Axis1.
Click OK | Page
Create fillets at the green edges Select the edges as shown in the picture. Go to: Insert > Features > Fillet/Round
> 7 mm
Click OK
Create a new plane parallel at the FRONTPLANE REAR W HEEL Go to: Insert > Reference Geometry > Plane Select the “FRONTPLANE REAR WHEEL”. Change the Offset Distance
into 400 mm.
Click OK Create a sketch at the new Plane4 Draw the sketch as shown in the picture. Connect all the dimensions with the origin.
Create an extruded cut on surface Go to: Insert > Cut > Extrude Direction 1
: Offset from Surface
Face/Plane
: Select the pink face as shown in the picture.
Change
into: 6 mm
Click OK
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Create a new sketch on Plane4 Draw the sketch as shown in the picture. Connect all the dimensions with the origin. Create an extruded cut on surface Go to: Insert > Cut > Extrude Direction 1
: Offset from Surface
Face/Plane
: Select the pink surface as shown in the picture.
Change
into: 6 mm
Click OK
Create another sketch on Plane4 Draw the sketch as shown in the picture. Connect all the dimensions with the origin.
Create an extruded cut on surface Go to: Insert > Cut > Extrude Direction 1 Face/Plane
Change
: Offset from Surface : Select the pink surface as shown in the picture. into: 6 mm
Click OK
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Create fillets on the green edges
Select the eight green corner edges as shown in the picture. Go to: Insert > Features > Fillet/Round
> 4 mm
Click OK
Create a circular pattern
Go to: Insert > Pattern/Mirror > Circular Pattern Pattern Axis
: Axis1 or face1 (the green surface in the picture)
Total Angle
: 360 deg
Number of instances
:9
Select the “Equal Spacing” option. Features to Pattern
: Extrude16, Extrude17, Extrude18, Fillet10
Click OK
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Change the color of the tire: Select the features of the tire (Revolve4, Fillet9, Extrude16, Extrude17, Extrude18, Fillet10, CirPattern6) > Right click > Feature Properties > Color > Change color > Select the color you like Hide -
all planes and sketches except: FRONTPLANE REAR WHEEL MIDPLANE REAR WHEEL
Save the file with the following name: Rear Wheel
Congratulations, you just finished the Rear Wheel! | Page
