Week 5. 3D Scanning and Printing

For my 3d printing I Created a Ball Bearing using OnShape

my approach to modeling a ball bearing in OnShape. This document outlines the step-by-step process I used to create all components including the outer race, balls, cage, and inner race.

Starting the Sketch

Here's exactly how I set up my initial sketch:

Initial setup:
- Started in an empty Parts Studio
- Pressed 'S' as a shortcut to begin sketching
- Selected the front plane
- Used 'N' key for normal view
- Used 'E' to hide all planes for a cleaner workspace
Creating the base geometry:
- Used 'L' and 'Q' to make a construction line from the origin
- Set construction line length to exactly 22mm
- Drew a circle with a precise 12mm diameter
- Added a vertical line for reference
- Used 'Shift+M' to create a midpoint relationship between the line and origin

Building the profile:
- Created a centerpoint rectangle
- Set dimensions to 4.8mm width and 12mm height
- Used 'i' key to make it coincident with the circle
- Applied mirror command to reflect the four lines using my reference line

Creating the 3D Components

Here's how I transformed the sketch into 3D components:

Setting up for revolution:
- Defined a mate connector at the origin with Z axis pointing up
- Made the sketch visible again
- Used the revolve command on both regions around the mate connector

Results of the revolution:
- Created three distinct parts in my Part Studio:
- Outer race (ring)
- Center/inner race
- Ball component

Adding Visual Style

Enhancing the appearance of the components:

Color and transparency:
- Applied light gray appearance to races
- Adjusted transparency of two parts using the slider
- Made the ball orange for better visibility

Creating the Ball Pattern

Duplicating the ball in a circular pattern:

Setting up the pattern:
- Defined a mate connector at the origin
- Created an assembly circular pattern
- Selected the ball as the component to pattern
- Specified 8 instances around the axis

Building the Cage

Creating the component that holds the balls in position:

Starting the cage design:
- Used "Create Part Studio in Context" feature
- Selected the mate connector as origin
- Started a sketch on the top plane
- Used 'P' to hide planes for cleaner view

Creating the cage geometry:
- Used 'U' to project one ball silhouette to sketch
- Selected the circle and pressed 'Q' to convert to construction line
- Used 'B' to create circles connected to the center
- Extruded the circular edge with mid-plane option
- Set thickness to 3mm with 25mm extrusion
Finalizing the cage:
- Performed boolean operation to subtract balls from cage (kept tools)
- Applied shell command with 1mm thickness
- Removed three faces for proper structure
- Mirrored upper cage over the top plane
- Renamed part to "cage" and customized appearance

Note: In real bearings, there are two sides of the cage held by pins - might try implementing that approach later.

Final Assembly and Animation

Completing the assembly and making it move:

Inserting the cage:
- Inserted cage into the main assembly
- Created a group relation between cage and balls

Setting up motion:
- Hid the mate connector at the origin
- Selected the face of the cage
- Picked the mate connector from the origin
- Suppressed the tangent relationship (no longer needed)
- Used Revolute tool to animate the assembly