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Scripted Parts: Ball Bearing - Part 1

From FreeCAD Documentation
Tutorial
Topic
Part Scripting - Ball Bearing #1
Level
Beginner
Time to complete
30 min
Authors
r-frank
FreeCAD version
0.16.6706
Example files
See also
None


Introduction[edit | edit source]

This tutorial is meant as a beginner's introduction to creating parts with python scripts within FreeCAD.
This tutorial will cover how to build a ball bearing with a CSG-workflow.
The code will produce a new FreeCAD document with 12 shapes (Inner Ring, Outer Ring and 10 balls/spheres).
It will look like this:


Workflow[edit | edit source]

The workflow is more or less identical how you would create the part in part workbench.
Just some small differences.

  • Create a new empty document and make it the active document
  • Insert Cylinder
  • Insert Cylinder
  • Do boolean cut to get basic shape of inner ring
  • Select all edges and apply a fillet
  • Insert torus
  • Move torus into position and do a boolean cut to create the groove for the balls
  • Repeat all steps for getting the shape for the outer ring
  • Insert first ball
  • Insert other balls using math to calculate the position of the balls
  • Set view to axometric
  • Zoom to fit all


Filleting edges[edit | edit source]

In part workbench using the GUI, you would select chamfers in the 3D view or in the menu for fillets and then apply the fillets.
Here we select all edges of a shape and apply fillets.
Therefore we need to select the edges BEFORE creating the groove.


Notes[edit | edit source]

This tutorial is using part primitives and boolean operations, which can be performance consuming.
For doing a scripted part with revolved sketches have a look at the tutorial Scripted Parts: Ball Bearing - Part 2.


Links[edit | edit source]

Scripted objects: The wiki page explaing the basics of scripting
Topological data scripting: A tutorial for covering basics of scripting
Scripted Parts: Ball Bearing - Part 2: Doing it with sketches
Bearing Script 1: Base for this tutorial, thanks to JMG ...


Code[edit | edit source]

## Ball-bearing script
## 11.08.2016 by r-frank (BPLRFE/LearnFreeCAD on Youtube)
## based on ball bearing script by JMG
## (http://linuxforanengineer.blogspot.de/2013/08/free-cad-bearing-script.html)
#
#needed for inserting primitives
import Part
#needed for calculating the positions of the balls
import math
#needed for translation of torus
from FreeCAD import Base
#
#VALUES#
#(radius of shaft/inner radius of inner ring)
R1=15.0
#(outer radius of inner ring)
R2=25.0
#(inner radius of outer ring)
R3=30.0
#(outer radius of outer ring)
R4=40.0
#(thickness of bearing)
TH=15.0
#(number of balls)
NBall=10
#(radius of ball)
RBall=5.0
#(rounding radius for fillets)
RR=1
#first coordinate of center of ball
CBall=((R3-R2)/2)+R2
#second coordinate of center of ball
PBall=TH/2
#
#Create new document
App.newDocument("Unnamed")
App.setActiveDocument("Unnamed")
App.ActiveDocument=App.getDocument("Unnamed")
Gui.ActiveDocument=Gui.getDocument("Unnamed")
#
#Inner Ring#
B1=Part.makeCylinder(R1,TH)
B2=Part.makeCylinder(R2,TH)
IR=B2.cut(B1)
#get edges and apply fillets
Bedges=IR.Edges
IRF=IR.makeFillet(RR,Bedges)
#create groove and show shape
T1=Part.makeTorus(CBall,RBall)
T1.translate(Base.Vector(0,0,TH/2))
InnerRing=IRF.cut(T1)
Part.show(InnerRing)
#
#Outer Ring#
B3=Part.makeCylinder(R3,TH)
B4=Part.makeCylinder(R4,TH)
OR=B4.cut(B3)
#get edges and apply fillets
Bedges=OR.Edges
ORF=OR.makeFillet(RR,Bedges)
#create groove and show shape
T2=Part.makeTorus(CBall,RBall)
T2.translate(Base.Vector(0,0,TH/2))
OuterRing=ORF.cut(T2)
Part.show(OuterRing)
#
#Balls#
for i in range(NBall):
  Ball=Part.makeSphere(RBall)
  Alpha=(i*2*math.pi)/NBall
  BV=(CBall*math.cos(Alpha),CBall*math.sin(Alpha),TH/2)
  Ball.translate(BV)
  Part.show(Ball)
#
#Make it pretty#
App.activeDocument().recompute()
Gui.activeDocument().activeView().viewAxometric()
Gui.SendMsgToActiveView("ViewFit")