Tire Tread - But a Connected Tread Pattern!

[cggzilla]

Hi all, this is my first time posting here but I have learned so much from these forums through Google searches and old posts. 

I am trying to create the tire tread of a certain racing tire. The body of the tire is revolved from the profile. I have created tires in the past without issue, but this new pattern involves a continuous tire tread pattern! My workflow is this:

1. Create the tire itself (easy)

2. Create a tread pattern sketch
3. Project the tread to the tire so it is curved

4. Turn the projected tread into a patch surface

5. Thicken the patch so I have a solid
6. Create a circular pattern and Cut the tire with the solids (using combine -> cut)

This works great for tread patterns that don't intersect. However, this tread pattern is continuous so the pattern solids need to overlap. I am getting a "Failed to Boolean bodies together" error. 

Is there a better way to go about this? I know the overlapping tread pattern is quite janky, but I don't need it to be perfect. I feel like I am doing this in a very backwards way... Thanks in advance!

[cggzilla]

Alright, so I just figured out I could have just used split face on my flat tread pattern sketch and then offset it... but I am still having the same issue trying to overlap the tread pattern

[TheCADWhisperer]

Can you File>Export your *.f3d file to your local drive and then Attach it here to a Reply?

[HughesTooling]

How about this using Emboss? See attached file. I used a parameter  to calculate the width of a rectangle from the diameter and number of repeats around the circumference.

Mark

[cggzilla]

Thank you for the help everyone, so far I have actually gotten the connecting pattern to work, but now am having issues with one of the outer patterns. Unfortunately I do not think I can use emboss as it is a revolved profile (it is a cambered/slanted tire).

The missing pattern is the outside facing portion of the tire and I would like the tread to cut a bit into the sidewall (like at the backside). For some weird reason the back side offset without issue, while the front gives an error.

Fusion 360 is also working excruciatingly slow for some reason, even when I suppress the circular patterns!

[TheCADWhisperer · Accepted solution]

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@cggzilla wrote:

Fusion 360 is also working excruciatingly slow for some reason, even when I suppress the circular patterns!

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Do you need the mesh body in the file?

Can you simplify the profile sketch(es)?

This image shows a curve that is about half the thickness of a sheet of paper.

The fewer faces you have generally the better the performance.

It might be more computationally efficient to do a portion of the body and then Pattern Bodies and Combine rather than Pattern Feature.  (I didn't try with this file as the first thing I would do is simplify sketch geometry that cannot be (easily) measured or manufactured (see 0.052 curve - I saw many other locations, especially is this is more for visual rather than real world manufacturing/functional need).

[HughesTooling · Accepted solution]

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@cggzilla wrote:

. Unfortunately I do not think I can use emboss as it is a revolved profile (it is a cambered/slanted tire).

How about creating the pattern on the inside of a ring that's slightly bigger than the tyer then cut from the tyer?

Something like this.