# Impossible Object 2 – Non regular Reuleaux Wheels

In a previous post we’ve seen how to build Reuleaux polygons from regular polygons. While already intriguing they were still regular. Now we will see that in fact we can start from the same base and build non regular constant width 5 sided polygons (There is no degree of liberty with 3, and I’m not doing with 7+ but it would work the same). Here is how to build them with inventor.

The files for this tutorial are [here for the inventor file] and [here for the STL]

1. The first step is from an empty part drawing, create a new 2D sketch and draw a 5 points star. Make sure you are not creating any constraints on the segments (like alignment with axis, relation with other points…). To check if any were created, press F8 (show all constraints), then remove any constraints using the small cross near each icon:
2. Set the length of one segment with a name (I’ve used length = 40mm to get wheels compatible with the previous article). Then use equal constraint to fix all segment to the same length (You can hid the constraints back with F9).
3. Pass all the segments to construction and draw thee points arcs from each vertices to get the outline of the Reuleaux polygon. Remark that, because of the constraints you can pull any vertex and deform the final shape.  You can copy multiple time the initial shape and deform it to have strange wheels. Before finishing the sketch, make sure to run a “sketch doctor” to close any open loops, otherwise you won’t be able to extrude the wheels.
4. Now extrude the wheels. Now we will add on one face of the wheel a embossed version of the start. To do that (repeat for each wheel), create a new a 2D sketch on one face. If the face outline was not projected in the sketch, use project geometry to do it. Change all the line (and origin if available to construction then draw the 5 point star with the construction switch ON.
5. Remove the construction switch and select the offset tool. Now select all 5 star lines and press enter to validate. You can now draw an offset version of the star “inside”. Repeat a second time and then fix the distance to 1mm and 2mm from original star. (after some try 0.5mm and 1.5mm work great to get the star closer to the border)
6. The current profile are intersecting so to be able to extrude/emboss them you have to add “points” to all the intersections. Once done exit the sketch.
7. Extrude or emboss 0.5mm deep the star, then add a 0.5mm filet on the star and a 1mm fillet on the outside edges of the wheel. (if you select the ‘all fillets’ option, you can capture all the star filet at the same time so no need to select one after the other).

Here it is, you have a set of non regular wheels compatible with the previous ones.
The files for this tutorial are [here for the inventor file] and [here for the STL]