diff --git a/examples/cylindrical_gear.py b/examples/cylindrical_gear.py
new file mode 100644
index 0000000..a8266a2
--- /dev/null
+++ b/examples/cylindrical_gear.py
@@ -0,0 +1,132 @@
+import cadquery as cq 
+from math import *
+
+class HollowCylinderSelector(cq.Selector):
+    """
+    Selects any shape present in the infinite hollow cylinder.   
+    """
+    #It works for the use I have in this code, it's not tested for any other configuration hence it might not be super robust
+    def __init__(self, inner_radius, outer_radius, along_axis = "Z"):
+        self.r1 = inner_radius
+        self.r2 = outer_radius
+        if along_axis == "X":
+            self.axis = 0
+        elif along_axis == "Y":
+            self.axis = 1
+        elif along_axis == "Z":
+            self.axis = 2
+        
+    def filter(self, objectList):
+        result =[]
+        for o in objectList:
+            p = o.Center()
+            p_coords = [p.x, p.y, p.z]
+            del p_coords[self.axis]
+            p_radius = sqrt(p_coords[0]**2 + p_coords[1]**2)
+
+            if p_radius> self.r1 and p_radius < self.r2 :   
+                result.append(o)
+
+        return result
+
+def involute(r):
+    #callback for paramCurve() function
+    def curve(t):
+        """
+        The involute curve is the curve that describe the flank of a tooth of a gear
+        """
+        x = r*(cos(t) + t*sin(t))
+        y = r*(sin(t) - t*cos(t))
+        return x,y
+    return curve
+
+def cylindrical_gear(m, z, alpha, b, helix_angle = None):
+    """
+    Create a cylindrical gear (either straight or helix)
+    Note that the helix one is pretty slow to be generated and the filling of the root edge of the gear don't work for helix_angle > 3°
+
+    params :
+    m : module of the gear (gear meshes only if they have the same module)
+    z : number of teeths
+    b : thickness of the gear 
+    """
+    r_p = m*z/2 #primitif radius (radius at which contact with other gear is made)
+    r_a = r_p + m   #radius of the top of the tooth
+    r_f = r_p - 1.25*m #radius of the root of the tooth
+    r_b = r_p*cos(radians(alpha)) #radius of the base circle from where the involute curve starts
+
+    def create_tooth_profile(m, z, alpha):
+        #Callback for eachpoint() function
+        def tooth_profile(loc):
+
+
+            STOP = sqrt((r_a/r_b)**2 - 1) # the STOP value is calculated by solving the following equation for t : ||involute(t)|| = r_a , ||involute(t)|| being the norm of the vector 
+            #below I start my 2D shape by sketching the 2 flanks of the tooth define by the 2 involutes
+            right = cq.Workplane("XY").parametricCurve(involute(r_b), stop = STOP, makeWire=False)
+            wire = cq.Workplane("XY").tag("base").transformed(rotate=(0,0,180/z)).parametricCurve(involute(r_b), stop = -STOP, makeWire=False)        
+
+            end_point_a = wire.val().endPoint().toTuple() #storing the global coord of the point for later use
+            if r_b < r_f:                
+                raise ValueError("r_b is smaller than r_f, your gear is undercut, try changing yours input parameter (use smaller alpah angle")
+                # A gear could work even if it's undercut, I was just lazy to take care of it
+                  
+            else:
+                wire = (wire.vertices("<X").workplane(centerOption="CenterOfMass").hLine(r_f-r_b)) # drawsing the rest of the profile starting from the bottom of the left involute
+                start_arc_root_pt = wire.val().endPoint().toTuple() #storing coord of the point again
+                #below building the final closed wire of the 2D tooth shape
+                wire = (wire.workplaneFromTagged("base")
+                    .moveTo(start_arc_root_pt[0], start_arc_root_pt[1] )
+                    .radiusArc((r_f,0),r_f)
+                    .hLine(r_b-r_f)
+                    .parametricCurve(involute(r_b), stop = STOP, makeWire=False)
+                    .radiusArc(end_point_a,r_a)
+                    .combine()
+                    .wire().clean()
+                )    
+            return wire.val().moved(loc)  #took the trick from slot2D function, eachpoint feeds via the previously created polararray
+            # the Location objects of the points, so this return create a 2D tooth profile and then rotate it to the right coord
+        return tooth_profile
+
+    #creating all the 2D profiles of the gear
+    teeths = (cq.Workplane("XY")    
+    .polarArray(0, 0, 360, z) #since my involute curve starts at the origin, I just need rotate workplane, which actually works when specifing 0 radius to polararray
+    .eachpoint(create_tooth_profile(m,z,alpha), useLocalCoordinates=True)
+    )
+
+    #extruding the 2D teeths in 3D
+    if helix_angle is None:
+        teeths = teeths.extrude(b)
+    else:
+        teeths = teeths.twistExtrude(b, helix_angle)
+
+    # creating the final gear by extruding the middle portion and unioning it with alls the teeths previously created
+    gear = (cq.Workplane("XY").circle(r_f).extrude(b).union(teeths)
+    .edges( #Selecting only the edges parallel to Z axis at the root of the teeths
+        HollowCylinderSelector(0, 1.01*r_f) -
+        cq.DirectionMinMaxSelector(cq.Vector(0,0,1)) -
+        cq.DirectionMinMaxSelector(cq.Vector(0,0,1),directionMax=False)
+        )
+    .fillet(0.4*m) 
+    .faces(">Z")
+    .circle(0.5*r_f)
+    .cutThruAll()
+    )
+    return gear
+
+############################################################
+############################################################
+############################################################
+
+#Creation of 2 gears that meshes
+
+alpha = 20
+m = 1
+z1 = 20
+z2 = 12
+b = m*5
+
+
+gear = cylindrical_gear(m,z1,alpha,b)
+gear2 = cylindrical_gear(m,z2,alpha,b).val().move(cq.Location(cq.Vector(m*z1/2+m*z2/2,0,0)))
+show_object(gear)
+show_object(gear2)
diff --git a/examples/gear_cadquery.PNG b/examples/gear_cadquery.PNG
new file mode 100644
index 0000000..6e02005
Binary files /dev/null and b/examples/gear_cadquery.PNG differ