how to design a tread pattern on a wheel or tire

kuifje_tintin

Hi there,

can anyone tell me how I would go about desiging a tread pattern. I want to design a plastic wheel to be 3d printed, but i want to have some say V-shaped grooves in the surface, and i ha no idea how to extrude or sketch on a cruved surface.

Thanks for any tips!

konstantin_shiriazdanov

check this doc https://cad.onshape.com/documents/4f5516d659b5a2193924e3c1/w/2c69cf8ac53be008704bbffa/e/ea5348d67dbdb7afc52fe951
i think it uses the most of requared features to create some simple profile on the double curved tire surface with minimal distorsions

Jake_Rosenfeld

Hi @kuifje_tintin

If you are looking for a simple way to get started with this (using only internal features) you could try an extrude up-to-face with offset.  This will push a projection of your sketch into the face at a standard distance:



You can then use a series of patterns to apply your groove:


https://cad.onshape.com/documents/13ef57b4f19208a00f95434f/w/aed63231ace7db04cbeded6d/e/d945937defdaabe66dfb1270

kristoffer_falk

Hi

I am trying the same thing, but I keep get an error, when I try to make the circular pattern.

Jake_Rosenfeld

@kristoffer_falk

It's hard to diagnose without actually going into your document, but it looks like you've only selected the bottom faces of your pocket.  You need to select all the faces of your pocket (the side faces and the bottom face).  This is made relatively easier by using the create selection button (the mouse with the + next to it) and using the "Pocket" selection type.
https://cad.onshape.com/help/Content/createselection.htm

You can also just manually select all the faces since there aren't too many to select.

kristoffer_falk

@Jake_Rosenfeld

Thanks for the answer. 

It makes very much sence, but no matter what I try, the circular pattern cannot regenerate properly.

Here is a link to my document:

https://cad.onshape.com/documents/a1ec71c942c235a8a585444f/w/d09780828fd5d7e4f9b9f4cd/e/5d30a43d82428622781b4373

Jake_Rosenfeld

@kristoffer_falk

Your tire was not a cylinder.  Because of the way you created it, it had a flat portion along the top.  When a pattern instance tried to land there, it failed due to the difference in geometry at the seed and at the destination:


I suggest that instead of extruding and then revolving, you just revolve the sketch face directly.  Then you will have true cylindrical geometry that is happy with patterns:

https://cad.onshape.com/documents/fbaaa9481eed593c7f3b7eaf/w/b527374e58bc49590bfdd658/e/8c69a4aa47ddbe03ea9beaaf

kristoffer_falk

@Jake_Rosenfeld

Great - now I got it. 

I have made a nice thread now, but I cannot make the circular pattern of the thread to fully intersect, which leaves these 0.03 mm thick dividers in the threadpattern.
When ordering a 3d print of the tyre, they cause a conflict. I have tried to mark the side of the divider, and then remove them with a 0.03 extrude, but it doesn't remove it all. No matter what I do there is a small part left in the top.
Is there a way to remove them or even better - avoid them when I make the circular pattern of the thread?

Jake_Rosenfeld

Hi @kristoffer_falk

I did some tinkering and got the treads to overlap for you:

https://cad.onshape.com/documents/99cb578aeb80777db838f1f7/w/4785e367aa8bf01e84f1dfeb/e/4115e3274ae353e2cb721d4d

The first thing I did was change the extrude.  I changed it from "blind" to "up to next" with an "offset distance" of 0.5mm.  This means that the bottom of the pocket will be rounded rather than flat.  Since this offset is a translational offset rather than a true offset, the rounding of each pattern instance still won't line up perfectly, but it's a little better.

I also changed the extrude to a "new" rather than a subtract.

Doing his "new" allowed me to do the circular pattern as a "part pattern", which are typically faster than feature pattern and more stable than face pattern.  I used the "remove" option on this part pattern to cut the treads out of the tire.



You'll notice another tab at the bottom called "Thicken".  In this tab I did a little more tinkering such that the bottom (inside?) lined up correctly.  In this doc, I first create a 0-distance offset surface off of the outside of the wheel.  I then split the face of the surface using sketch 2.  I am not splitting the face of the tire directly because I don't want to mess with that geometry (as of now there is no way to "heal" a split face).  I then create 3 new parts by thickening the faces created by the split (and delete the offset surface; it is no longer needed).  I then do the same thing as the other part studio (Subtractive part pattern of the 3 tool parts).

Using thicken rather than extrude will do a true offset rather than a translational offset; the top of the thicken will match the radius of the outside of the wheel and the bottom of the thicken will be offset into the part by the specified value. 



The thicken part studio creates even better geometry, but could also be improved by changing the underlying sketch such that some integer number of pattern instances lines up perfectly.