Mars Rover Wheel

This build explores the sweep operation and the circular pattern tool.

Sketch - Wheel Profile

Start by creating the circles that form the wheel profile using the dimensions shown. Use an offset for the outer circle

Starting with a single vertical construction line, create a single spoke, 2mm wide and trim the intersections if the circles.

Select the two vertical lines of the spoke and open the circular Pattern tool from the Create menu. Set the centre point to the centre of the circle and the quantity to 7

Trim the intersection of the spokes and rim to finish the sketch

Sweep - Twisted Spokes

The sweep tool is a bit like extrude but you can specify a path for the extrusion to follow. It also allows you to add guide rails that influence the shape of the extrusions at the edges.

As a path for the sweep to follow we will first create a straight line out from the wheel centre. Start by creating a new sketch on a plane perpendicular to the wheel and draw a 30mm line out from the centre. Finish the sketch.

We will use a coil spring placed at the centre of the wheel as a guide rail to force a rotation of the hub during the sweep.

Select the coil tool from the 3D create menu. It will ask you to first select a plane and then draw a circle to form the base of the coil. Choose the same plane as the wheel and draw a circle at the centre, about the same size as the hub. Set the height to 30mm

We only want a slight twist on our spokes so set the number of revolution to 0.1. It won't look like a spring any more.

We're now ready to sweep the wheel into a 3D object. Select the wheel profile and then the sweep tool.

We want to set the type of sweep to Path + Guide Rail. Do this and select the straight line as the path and the coil as the guide rail. Don't forget to set the operation to Join.

Our wheel is starting to take shape:

Sketch - The Tooth

We are now going to add some grip to the wheel. We will make one using a simple path sweep before duplicating it with the mirror too.

From the timeline edit your first sketch and create a tooth shape along the edge using a Fit Point Spline.

Press return to finish the spline and finish the sketch.

The sketch probably wont be visible so turn it on from the browser panel

Get yourself well zoomed into the tooth

We now want to create a new plane to work on that is tangent to the wheel at the point inline with the point of the tooth.

From the construction menu select Plan Tangent to a Face at Point

S

Click the wheel rim and then the point of the tooth

Click ok and create a new sketch on this plane.

We want to be able to work with the edges of the wheel so we need to project them onto the sketch. Press P to activate the project tool and select the wheel edges.

We are going to use the mirror tool to make our tread symmetrical so a straight line across the circle and project another 5mm from the centre.

Finish one side of the tread using lines and the trim tool

And then fillet the join. Be careful not to fillet too much or you will break the continuity of your line.

Using the mirror tool, select the curved section as your objects and the centre line as the mirror line. Then delete the mirror line.

Sweep - Single Thread

Using the single path sweep tool, sweep the profile of your tooth along the path.

If it doesn't work, go back and check that your line has not lost continuity as the mirror operation can sometimes do that.

Circular Pattern - Remaining Treads

Select Circular Pattern from the Create > Patterns Menu

And using the shift key highlight the objects making up the tread.

Set the axis as the centre of the circle and create treads around the entire circumference.