Handle

Brake Handle

Create a base sketch at the front plane, and then use Smart Dimension to define the length of the lines and the angles. Please see the base sketch below.

Extrude the base sketch to 2 in, and its end condition is Mid-Plane.

Create another sketch (Sketch 2) on the right side of the object. Doing so by first drawing a circle with diameter 0.9 in and draw a counterpoint arc with the same origin as the circle. Set the distance of the origin of the circle to the left edge to be 0.6in. Then, make the arc to be tangent to the left edge through “add relation”

Draw two vertical lines from the top of the object to the bottom. (Length 2.12in, distance between two lines: 0.73 in). Use smart dimension to define the distance between left vertical line and the left edge to 0.1in.

Use “3 Point Arc” to connect the bottom end point of left vertical line to the left end point of the arc. Set the 3 point arc to be tangent to both vertical lines and the center point curve.

Create a line connect the bottom end point of right vertical line to the circle.

At the right side of the center point arc, create a vertical and tangent line with respect to the arc. The bottom end point of right vertical line is horizontal to the end point of the line created before. Then, create a horizontal line having a length 0.19 in.

Connect the horizontal line to the circle. Then use Trim Entities to delete the lines between them. Please see the below image.

Use extrude cut to cut through the sketch created above , with depth 2in.(Direction 1: Blind , Direction2: Blind) [Cut-Extrude 1]

Use VarFillet to round the edges with different radius. (From 0.3 in—> 0.15in—>0.1in) Please the see the figure below AND Repeat the same precedes for the other left edges of the object. [VarFillet 1 to VarFillet 4]

Use Fillet to round the top edges,setting the fillet radius to be 0.2in and to round the rest of the edges with radius 0.1 in. [Fillet 1 to Fillet12]

Create a reference mid plane, with face 1 and face 2 as specific by below figure. [Plane1]

Create another sketch on the plane 1. Draw a vertical line with length 1.29 in and horizontal line with length 0.97 in. Then use 3 point arc and center point arc to connect the lines with radius 1.08 and 0.84 respectably. [Sketch 6]

Use extrude cut to cut the sketch 3, with depth 0.4 in [Cut-Extrude 2]

Draw a center rectangle, centering at the mid plane. (length 0.15 in & width 0.59 in). Then, use extrude cut to cut from the sketch plane in two directions, one direction cutting 1.84 in and another outward direction 3.26 in.[Cut-Extrude 3]

Creating a new sketch, draw a circle centering at the same as the rectangle created above, diameter 0.25 in. Then, use extrude cut to cut through the circle. [Cut-Extrude 4]

Extrude out the sketch inward direction to 0.05 in. [Boss-Extrude 2]

Create a concentric circle with radius 0.45 in and extrude out to 0.15 in a outward direction.[Boss-Extrude 3]

Use fillet to round the edge of the circle created above, radius with 0.02 in.[Fillet 13]

Create a sketch on the front plane, and draw two vertical lines with equal length 0.04 and a horizontal line 0.15 in. Please see the figure below.

Extrude cut the sketch plane to 0.15 in. [Cut-Extrude 5]

Use circular pattern to create the same appearance. Set the spacing to be 60 deg, and the instances to be 6. [circular pattern]

Create a circe at the front plane of the object , diameter with 0.15 in and use extrude cut to cut through the circle. [Cut-Extrude 6]

Create another circle sharing the same center point. (Diameter 0.3) Then use extrude cut from that sketch plane, depth 0.03 in. [Cut-Extrude 7]

Repeat the step 24 for another side of the object.

Create a circle at the back of the object , diameter 0.15 in. Then, use extrude cut the circle to 0.43 in. [Cut-Extrude 9]

Draw a concentric circle with diameter 0.3 in and extrude cut to 0.02 in. [Cut-Extrude 10]

Create a new sketch at the front side of the object , and draw a circle with diameter 0.2 in. Extrude out to 0.05 in. [Boss-Extrude 4]

Crate the sketch on the plane in step 28. Please see the picture below.After creating the skeptic, use revolve 1. [Revolve 1]

Use fillet to round the edges at the top of the handle, radius 0.02 in. [Fillet 14]

Use covert entities to create the shape of half circle by clicking the curve in the middle, and use extrude cut to cut 0.2 in. [Cut-Extrude 11]

Use circular pattern to replicate the pattern, setting the degree to 60 deg, and instances 6 . [CirPattern 2]

At the top of the plane, create a circle with diameter 0.15 in and extrude cut to 1.64 in. [Cut-Extrude 2]

Use fillet round the top surface, radius 0.01 in. [Fillet 15]

Use convert entities to covert the inner face to the plane one, and use trim entities to delete the lines. Please see the figure below.

Use extrude out to 0.1 in. [Boss-Extrude 5]

Finally, use mirror to replicate that feature, by choosing the mirror plane as plane 1 and feature to mirror Boss-Extrude 5.

Resulting image for handle body

Create a sketch on the front plane, and draw a vertical from the origin(length 1.01in), and draw a 3 point arc has the radius 0.23 in. Then draw a circle with diameter 0.15mm at the constructing line . Please see the figure for more details. After finishing the sketch, extrude out to 0.2 in. [Boss-Extrude1]

Create a new sketch on the front plane, use convert entities, converting the lines from the bottom into this plane. Then, draw a line in the middle. (Length 0.51in)

Extrude the sketch to 0.05 in. [Boss-Extrude2]

On the back of the object, use convert entity to covert the edges from the top to the bottom plane, and draw a line connect the right edge and the left edge.

Extrude the sketch region to 0.1 in. [Boss-Extrude3]

On the back of the object, draw three construction lines, and use 3 point arc , and two curves to create the image. After that, extrude out the sketch, setting the end condition to be through all. Please look at the image shown on the left. [Boss-Extrude3]

On the top plane, crate two horizontal lines, each with 3.87in, and a vertical line.(Length 0.98). Since it is very hard to describe by words, please look the figure on the left.

Extrude cut the sketch to 0.61 in. [Cut-Extrude2]

Use fillet to round the edges highlighted on the image, radius with 0.1 in. [Fillet2-Fillet 6]

The resulting parts of the Handle Bar

Create a base sketch on the front plane. Draw two vertical lines. ( one is 0.4 in, and another is 0.35 in). The distance between them is 0.08 in.

Draw a horizontal line at the top of the 0.35 in.( Length is 0.06 in)

Use 3 point arc by connecting the end point of the horizontal line and the end point of the vertical 0.4 in line. Please see the following base sketch.

Use Revolve, Axis of revolution is 0.4 in vertical line.

Then, we will get the resulting parts for Handle screw.

Insert the parts: Handle body(Handle_Fangyi ), Handle2FromZihan, and two screws in a new assembly.

Create a Concentric mate between the face of the Handle 2 and the hole of the handle body by clicking the the face of handle —>mate —> choose the hole of the handle body—>select the Concentric mate. Please see the highlighted part of the figure. [Concentric 1]

Create a Width mate between the handle body and the handle2 . Set the Width reference as the inner face of the body handle, and set the Tap selections as the left and the right faces of handle 2 between the inner faces.[Width1]

Create concentric mates between the screws and the handle body of the holes. [Concentric 2 & Concentric 3]

Create coincident mates between the screws and the handle body. Click the contacted faces of screws and select coincident mate. [ Coincident 1 &Coincident 2]

Then, we will get the resulting assembly.