Inventor 101

[JD Mather]

 

Next add Face Draft to the sides of the rib.

Select the bottom of the Rib to set the Pull Direction and then select the sides of the rib near these planar "hinge" edges.

[JD Mather]

 

I don't recall if we have done Full Round Fillet yet. For this feature we select three faces in order. Side face 1, Center face, and Side face 2. This ensures that if we change the thickness of the rib, the fillet always spans the 3 faces. And because of the draft angle on the rib - the fillet is not R4 as we might expect.

[JD Mather]

 

Add R10 edge fillets to the 4 edges shown.

[JD Mather]

 

Add R2 fillets to the edges shown.

[JD Mather]

 

Start a new sketch as shown on the bottom of the part.

 

Sketch a rectangle and change the corners to center points.

[JD Mather]

 

By now you should be an anticipating some of our next moves.

 

Constrain and dimension the sketch as shown.

[JD Mather]

 

Now add Clearance holes for M8 Hex Head Cap Screws (I incorrectly show Socket Head Cap Screws selected in the image).

[JD Mather]

 

Place a counter bored hole on the top of the part, concentric to the cylindrical feature as shown.

[JD Mather]

 

Start an new sketch on the "right side" of the part as shown.

Sketch vertical line from the projected origin.

Convert the endpoint of the line to a sketch center point.

Dimension the height from the bottom of the part.

Note that this line will keep the hole centered.

[JD Mather]

 

Create an 8mm Hole through the part.

[JD Mather]

 

"Paint" the part to whatever color you want.

Remove the "paint" from the machined faces.

Save the file.

[JD Mather]

Start a new metric part file.

 

Start a new sketch on the right side plane (YZ) and create the sketch shown.

 

 

Add the ellipse and horizontal object line shown.

 

 

Trim the ellipse below the horizontal line and Finish the sketch.

Save the file with the name Knob.

 

[JD Mather]

Right click on the YZ plane and make it Visible.

Create a new offset Workplane, click and drag entering a distance of 41.

 

Start a New Sketch on this new Workplane.

 

Create a vertical construction line going down from the projected origin center point a distance of 41mm.

Add a 20mm circle.

Finish Sketch2.

 

 

Oops - I made a mistake. No problem.

Double click on the Workplane1 in the browser and change the offset distance from 41 to 30.

(it was the construction line length that is 41mn, not the workplane offset distance)

[JD Mather]

Create a new Workplane2 offset a distance of 45mm from the YZ workplane.

 

 

Create a New Sketch on Workplane2 and Project Geometry the vertical construction line from Sketch2.

Create a circle at the end of the projected construction line as shown.

 

 

Finish Sketch and save the file.

[JD Mather]

Mirror Workplane 1 and 2 about the YZ plane.

 

Start Sketch 4 and Project Geometry the 20mm circle.

Start Sketch 5 and Project Geometry the 16mm circle.

 

Finish sketch and save the file.

[JD Mather]

Start the Loft command and select the sketches from left to right.

Click OK.

 

 

Right click on the Workplanes and turn off the Visibility.

[JD Mather]

Start Sketch6 on the XZ Plane and create a 20mm circle as shown.

Finish sketch.

 

 

Extrude the circle To Next.

 

[JD Mather]

Add 6mm Fillets as shown.

 

Note: You must pick two edges on the ends for the fillets to go all the way around.

 

[JD Mather]

Add a threaded hole as shown.

 

 

That completes this part.

Set the material to Steel and Chrome texture.

Save the file.

 

Holes should not have sharp edges - add a 1mm Chamfer to the edge of the hole.