pic: Enigma Wheel 2

[kgzak]

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[JesseK]

This one is alot better for its strength!

Be sure to add fillets where the 'spokes' meet the inside of the outer rim. The radius should be at least the same as the radius of the intended CNC bit.

[JamesCH95]

I can tell you from my wheel design experience that it's better to have your spokes taper towards the outside, that is to say that your spokes should be thicker near the hub and narrower near the rim.

Think about making the question marks grooves instead of slots. It would reduce machining time and improve strength, two wins in my book.

Looks good otherwise! Do you have a material picked out or a calculated weight?

[Brandon Holley]

Originally Posted by JesseK

This one is alot better for its strength!

Be sure to add fillets where the 'spokes' meet the inside of the outer rim. The radius should be at least the same as the radius of the intended CNC bit.

You will also need to add the radius for the cutting bit into the bottom part of the question mark. That is, if you are planning on milling these wheels.

I like the iteration, keep it going.

-Brando

[Chris is me]

Next steps:
1. Can you lighten the hub? That's a lot of solid material there, I bet you could figure out a pattern to make that lighter.
2. Fillets on your wheel's spokes are cool for reducing stress. You have them on the hub side but not the wheel side.
3. Tread grooves apparently make putting on treads easier and more secure. Plus it's an interesting CAD exercise for your first time.

[kgzak]

Originally Posted by Chris is me

Next steps:
1. Can you lighten the hub? That's a lot of solid material there, I bet you could figure out a pattern to make that lighter.
2. Fillets on your wheel's spokes are cool for reducing stress. You have them on the hub side but not the wheel side.
3. Tread grooves apparently make putting on treads easier and more secure. Plus it's an interesting CAD exercise for your first time.

1. Working on that
2. Just added that
3. How would I go about doing that?

[R.C.]

Originally Posted by kgzak

3. How would I go about doing that?

I take it your using inventor.

Currently 1323 is hosting CAD Tutorials that our ROP Arch class paid for.

http://team1323.com/tutorials/Solidw...xample%202.mov

Here's one that shows how to use the revolve cut feature. Something similar should exist in Inventor. Basically you want to draw a square the thickness of your groove and revolve cut it into your piece.

-RC

[kgzak]

Originally Posted by R.C.

I take it your using inventor.

Currently 1323 is hosting CAD Tutorials that our ROP Arch class paid for.

http://team1323.com/tutorials/Solidw...xample%202.mov

Here's one that shows how to use the revolve cut feature. Something similar should exist in Inventor. Basically you want to draw a square the thickness of your groove and revolve cut it into your piece.

-RC

I am still unsure how to go about this. It won't let me create a new sketch on the outside of my circle. Did I do something wrong? As I said I am new at this so I am not completely sure what to do. Could someone who uses inventor help me out? Not that it didn't help but I am not sure how to go about this in inventor.

[EricH]

Not totally sure on how to do this myself, especially in Inventor, but:

Create a workplane parallel with the axis of rotation of the wheel and running through the center of the wheel. Make your rectangle/square/groove shape on the workplane and do a revolve feature around the axis of rotation of the wheel.

[Brandon Holley]

Originally Posted by EricH

Not totally sure on how to do this myself, especially in Inventor, but:

Create a workplane parallel with the axis of rotation of the wheel and running through the center of the wheel. Make your rectangle/square/groove shape on the workplane and do a revolve feature around the axis of rotation of the wheel.

A quicker/alternative method for the groove may be to use an extruded cut from the mid plane.

Make a sketch at the midplane of your wheel (the plane that would divide your wheel in half along the circumference).

Make a sketch with 2 concentric circles. Constrain one of those circles to be the outer edge of your wheel. Add a distance constraint between the two circles (this will be the depth of your groove; be sure the 2nd circle is smaller than the outer before adding the distance dimension).

Now extrude cut, and use the "midplane" feature as opposed to the standard "blind". Set your distance to be however wide you want your groove to be and build your feature. Voila, a tread groove.

Let me know if you have any questions.

-Brando

[JamesCH95]

From my experience designing wheels I've found that the most efficient way to make a wheel goes like this:

-Make a sketch with two enclosed sections: the "spider" (a spider is the hub and spokes) and rim cross sections
-Revolve the spider
-Extrude-cut the spider to create 1 spoke
-Make a circular pattern to create all the spokes
-Revolve the rim from the original sketch (use the "share sketch," or similar, option)
-Do any finishing fillets you may need

I've made a couple dozen wheel designs using this method and I've found it to be very robust. There are some flourishes that make it run even smoother, see what you can work out!