Created the knob from Solidworks Modelmania 2006

[raydeleu]

As an exercise to use Replicad, I modelled the knob that was used in Solidworks Model Mania 2006. If you want to know more about these types of exercises, have a look at https://blogs.solidworks.com/tech/2023/02/24-years-of-model-mania.html.

I encountered several issues while creating this model, but after comparing the results with other CAD programs the result with Replicad is still quite good.

The main issues I encountered were:

• I had a lot of trouble defining the shape that is used to create a profile with a radius of 32 mm on the "finger" of the knob. Other than suggested in generic sweeps must start at origin? #97 it seemed possible to define the sweep without starting the sweep at the origin. But the orientation of the profile curve seems very odd. I have to investigate this further, but it seems that when using a rail curve defined on the YZ plane, the profile curve has to be defined with x,y coordinates where the x-coordinate points to the inside of the curve. You can think of it like the profile defined in x,y coordinates flows along the rails in the direction of the z-axis. Perhaps the following image clarifies this. The profile is shown in red, the rail for the sweep has the curve used to define the side view of the "finger".

• The knob is a hollow shape (thin solid) with a wall thickness of 4 mm. As the outer edge of this shape has a fillet of 4 mm, the radius at the inside becomes 0 mm. OpenCascade has issues in creating this, so I used a reduced wall thickness of 3.9 mm. Strangely enough I encountered the same issue in OnShape which is based on the Parasolid kernel, the same kernel used in Solidworks.

• The structure at the inside of the knob should be filleted with a radius of 1 mm. This seemed to be possible only for a limited number of edges. Again the same issue occured in OnShape.

As always, the code is shown below:

// Knob that was used in SolidWorks Model Mania 2006

const main = (
{draw,
makeSphere,
EdgeFinder,
makeBaseBox,
makeCylinder,
Sketcher},
{},    
) => {

// create sketch of sideview of finger of the knob  
let sideView = draw()
.movePointerTo([-60,0])
.ellipse(20*Math.sin(Math.PI/6),20*Math.cos(Math.PI/6),20,20,0,0,false)
.smoothSplineTo([0,32])
.ellipse(32,-32,32,32,Math.PI/2,0,false)
.close()

// identical to side view but only top edge
// to be used as a rail to sweep the 32mm radius profile  
let sweepRail = draw()
.movePointerTo([-60,0])
.ellipse(20*Math.sin(Math.PI/6),20*Math.cos(Math.PI/6),20,20,0,0,false)
.smoothSplineTo([0,32])
.ellipse(32,-32,32,32,Math.PI/2,0,false)
.done()
.sketchOnPlane("YZ")

// variable used to define the rounded profile of r=32mm on top of knob  
// the knob to cut is 2*16 mm wide, so cutter to 18mm
// r=32, so height is SQRT(SQR(32)-SQR(16))	
let segmentHeight = 32 - Math.sqrt((32*32)-(16*16))

// create a rounded profile to shape finger of knob  
function sweepProfile(plane,origin)
{
let section = new Sketcher(plane,origin)
.movePointerTo([segmentHeight,-20])
.lineTo([segmentHeight,-16])
.threePointsArcTo([segmentHeight,16],[0,0])
.lineTo([segmentHeight,20])
.lineTo([-1,20])
.lineTo([-1,-20])
.close()
return section}

// create sweep of profile  
let profileCut = sweepRail.clone()
.sweepSketch((plane,origin) => sweepProfile(plane,origin))		

// create finger of knob by extruding sideview
sideView = sideView.sketchOnPlane("YZ").extrude(32).translate([-16,0,0])

// cut the profile out of finger  
sideView = sideView.cut(profileCut)

// fillet the sides of the finger  
sideView = sideView.fillet(4,(e)=>e.containsPoint([16,0,32-segmentHeight]))
sideView = sideView.fillet(4,(e)=>e.containsPoint([-16,0,32-segmentHeight]))

// create a half dome   
let ball = makeSphere(30);
let cutBall = makeBaseBox(80,80,40).translate(0,0,-40)
ball = ball.cut(cutBall);

// fuse the half dome with the finger and fillet the edges  
sideView  = sideView.fuse(ball)
sideView = sideView.fillet(4,(e)=>e.inBox([18,40,1],[-18,-40,50]))

// store the shape to be used later on to create inside structure of the knob  
let intersectBall = sideView;

// make a hollow shape, removing the bottom face  
// thickness should be 4, but this yields kernel error
// probably because outer fillet is 4 mm results in inner fillet problem
sideView = sideView.shell(-3.9,(f)=>f.containsPoint([0,0,0]))

// create 3 ribs and a stem   
let rib =  makeBaseBox(4,40,40).translate(0,20,4);
let rib1 = makeBaseBox(4,40,40).translate(0,20,4).rotate(120,[0,0,0],[0,0,1]);
let rib2 = makeBaseBox(4,40,40).translate(0,20,4).rotate(240,[0,0,0],[0,0,1]);
let stem = makeCylinder(10,30,[0,0,0],[0,0,1]).translate(0,0,4);

rib = rib.fuse(rib1)
rib = rib.fuse(rib2)
stem = rib.fuse(stem)

// make the stem hollow, note that ribs had to be created first  
let stemHole = makeCylinder(6,40,[0,0,0],[0,0,1]);
stem = stem.cut(stemHole);

// intersect the ribs and stem with the contour of the knob   
stem = stem.intersect(intersectBall)

// fuse inner parts with the hollow knob  
sideView  = sideView.fuse(stem)
sideView  = sideView.fillet(2,(e)=>e.inDirection("Z"));
// EXPERIMENTS: inner structure should be filleted with 1mm radius
// seems impossible, also in OnShape!   
// sideView  = sideView.fillet(0.3,(e)=>e.inBox([-32,-32,3],[32,32,32]));
// sideView  = sideView.fillet(0.5,(e)=>e.atAngleWith("YZ",0));
// sideView  = sideView.fillet(1);

// display the resulting shapes
let shapeArray = [
{shape: sideView, name: "sideView"},
{shape: profileCut, name:"profileCut"}
]; 

return shapeArray

}

[raydeleu]

I finally managed to create most of the fillets in OnShape as well.

This made me rethink my approach towards filleting. Instead of "filleting late" I tried the approach of "filleting early": I filleted the inner ribs and the stem (cylinder) before fusing this to the rest of the shape. Here is the result in Replicad.

The changed code is:

// create 3 ribs and a stem   
let rib =  makeBaseBox(4,40,40).translate(0,20,4).fillet(1);
let rib1 = makeBaseBox(4,40,40).translate(0,20,4).fillet(1).rotate(120,[0,0,0],[0,0,1]);
let rib2 = makeBaseBox(4,40,40).translate(0,20,4).fillet(1).rotate(240,[0,0,0],[0,0,1]);
let stem = makeCylinder(10,30,[0,0,0],[0,0,1]).fillet(1).translate(0,0,4);

rib = rib.fuse(rib1)
rib = rib.fuse(rib2)
stem = rib.fuse(stem)

// make the stem hollow, note that ribs had to be created first  
let stemHole = makeCylinder(6,40,[0,0,0],[0,0,1]);
stem = stem.cut(stemHole);
stem = stem.fillet(1.0,(e)=>e.inPlane("XY",4))

I then again tried the methods contained in the code shared above to find the missing edges, but these all resulted in either kernel errors or errors as no edges were selected.

[raydeleu]

After tweaking some of the dimensions I was a able to achieve this result in Replicad:

The outer fillets were increased to 5 mm, the wall thickness was decreased to 3 mm. These changes yield a larger rounding on the inside of the knob before filleting. The inner fillets were decreased to 0.7 mm. I used the inBox selection mechanism:

sideView  = sideView.fillet(0.7,(e)=>e.inBox([-29,-29,3],[29,29,20]));

The complete code can be found here https://github.com/raydeleu/ReplicadManual/blob/main/models/knob10.js