AnsweredAssumed Answered

How to add deformation to imported tyres

Question asked by Sebastian Mulford on Dec 17, 2020
Latest reply on Dec 19, 2020 by Paul Salvador

Like • Show 0 Likes0
Comment • 17

Hi,

I am struggling to edit an imported tyre (DrivAer) to have a realistic contact patch. I have split the tyre at the correct height to give the contact patch (picture below).

However, along the contact patch, I want the tyre grooves to be parallel to the floor (or contact patch) and at a constant height with the same geometry (ie curved at the edges) as it was before. So, essentially I can't work out how to make (or replicate) the tyre grooves from being a circular feature to a linear feature along the contact patch. This concept of uninterrupted grooves should be more obvious from the following picture, which has rectangular grooves, as for my case I currently have (a) and want the grooves to be uninterrupted like in (b).

The grooves for this tyre can be more clearly seen in the following picture.

Is there a way to accomplish this?

Heiko Sohnholz Dec 19, 2020 3:31 AM

Correct Answer

Here is one using "Deform".

See the reply in context

Attachments

05_Wheels_Front.SLDPRT.zip4.2 MB

No one else had this question

Outcomes

17 Replies

Glenn Schroeder Dec 17, 2020 8:35 AM
Mark Correct
Correct Answer
I typed a bunch of instructions, but then wasn't sure if that idea would work, so I tried it. It needed some tweaking, so I'm glad I attempted it before posting. In any case, instead of explaining I decided to post the example. Please review it and let me know if you have any questions. (To save time I didn't bother fully defining all the sketches, but I would never skip that for anything in my work.)

I'm using SW2021, so if you're using an earlier version you won't be able to view it and I'll have to explain it with text and screenshots.
Attachments
- flat tire.SLDPRT.zip104.6 KB
Like • Show 1 Like1
Actions
- Matt Peneguy @ Glenn Schroeder on Dec 17, 2020 9:12 AM
  Mark Correct
  Correct Answer
  We're on Windows 7, so I can't install 2021, here. Can you give a short synopsis of what you did? I'm thinking that you used a plane and ellipsis in a different configuration...Beyond that, I'd be guessing.
  Like • Show 0 Likes0
  Actions
  - Glenn Schroeder @ Matt Peneguy on Dec 17, 2020 11:03 AM
    Mark Correct
    Correct Answer
    Matt Peneguy wrote:
    
    We're on Windows 7, so I can't install 2021, here. Can you give a short synopsis of what you did? I'm thinking that you used a plane and ellipsis in a different configuration...Beyond that, I'd be guessing.
    
    Nothing that complicated (I'm not an engineer, remember?).
    
    I started off with a simple boss extrude to create the cylinder and then a revolved cut for the first groove. I know I could have done all this in one Revolve, but this seemed simpler.
    
    Next I made the flat part with an Extruded Cut.
    
    Then is where it got a little more interesting. I had initially thought I could start a sketch on a plane perpendicular to the flat surface and use Convert Entities on the edges of the groove to create lines for an extruded cut. That didn't work quite like I'd planned, so I placed a vertical construction line, then another one horizontal off it's center point. Then I used the Convert Entities tool on the edges of the groove on the opposite side from the flat place.
    
    After doing that I used the horizontal construction line (at the top of the screenshot above) to mirror those lines to the opposite side, where the flat part is, and added a short horizontal line to close it.
    
    Finally, I went back to the other lines from the Convert Entities feature and made them construction, and then used this sketch for an extruded cut . . .
    
    . . . and add fillets to smooth off the rough edges.
    
    Of course I didn't take the time to make multiple grooves, but this should illustrate what I did. I think this is what the OP wanted, or did something get past me (it wouldn't be the first time)?
    Like • Show 2 Likes2
    Actions
    - Matt Peneguy @ Glenn Schroeder on Dec 17, 2020 11:59 AM
      Mark Correct
      Correct Answer
      Glenn Schroeder wrote:
      
      Matt Peneguy wrote:
      
      We're on Windows 7, so I can't install 2021, here. Can you give a short synopsis of what you did? I'm thinking that you used a plane and ellipsis in a different configuration...Beyond that, I'd be guessing.
      
      Nothing that complicated (I'm not an engineer, remember?).
      
      I started off with a simple boss extrude to create the cylinder and then a revolved cut for the first groove. I know I could have done all this in one Revolve, but this seemed simpler.
      
      Next I made the flat part with an Extruded Cut.
      
      Then is where it got a little more interesting. I had initially thought I could start a sketch on a plane perpendicular to the flat surface and use Convert Entities on the edges of the groove to create lines for an extruded cut. That didn't work quite like I'd planned, so I placed a vertical construction line, then another one horizontal off it's center point. Then I used the Convert Entities tool on the edges of the groove on the opposite side from the flat place.
      
      After doing that I used the horizontal construction line (at the top of the screenshot above) to mirror those lines to the opposite side, where the flat part is, and added a short horizontal line to close it.
      
      Finally, I went back to the other lines from the Convert Entities feature and made them construction, and then used this sketch for an extruded cut . . .
      
      . . . and add fillets to smooth off the rough edges.
      
      Of course I didn't take the time to make multiple grooves, but this should illustrate what I did. I think this is what the OP wanted, or did something get past me (it wouldn't be the first time)?
      I see. Makes sense. I was wondering if he needed a "realistic" version where the grooves would actually deform. But what you've posted should give a reasonable visual approximation...Which without more information, is a very good assumption.
      Makes me wonder if another good method would be to use convert entities on the tyre profile with the flat spot and then do a swept cut with the groove profile...As with everything in SW, there's always many ways to do anything.
      Like • Show 2 Likes2
      Actions
Scott Perman Dec 17, 2020 2:47 PM
Mark Correct
Correct Answer
Would Flex work for something like this?

I hope he is just looking for a visual representation because that is in no way representative of what the tire does under load.
Like • Show 3 Likes3
Actions
- Sebastian Mulford @ Scott Perman on Dec 18, 2020 10:14 AM
  Mark Correct
  Correct Answer
  Sorry, yes, all I require is a visual representation as I will be conducting a CFD investigation with this tyre with a more realistic contact patch. I have now also attached the unedited tyre to the post.
  Like • Show 1 Like1
  Actions
  - Heiko Sohnholz @ Sebastian Mulford on Dec 18, 2020 2:44 PM
    Mark Correct
    Correct Answer
    Hello Sebastian, hello Matt,
    the result auf my short experiment was made during a meeting - so I don't have saved the file (only the screenshot I've posted).
    But now I must admit, that I'm not able to get the proper result as I expected.
    So I'm very sorry but I have no file to upload for you. Don't know why but, deforming the part outside will work, but inside I've never seen any result.
    I apologize.
    Like • Show 1 Like1
    Actions
    - Matt Peneguy @ Heiko Sohnholz on Dec 18, 2020 3:40 PM
      Mark Correct
      Correct Answer
      Heiko Sohnholz wrote:
      
      Hello Sebastian, hello Matt,
      the result auf my short experiment was made during a meeting - so I don't have saved the file (only the screenshot I've posted).
      But now I must admit, that I'm not able to get the proper result as I expected.
      So I'm very sorry but I have no file to upload for you. Don't know why but, deforming the part outside will work, but inside I've never seen any result.
      I apologize.
      Thanks for clarifying, I thought I was doing something wrong. I downloaded his file and it's imported geometry, which makes things even more difficult. SW does not like this file.
      My plan was to cut his tyre in half, get the profile from that, then use a path with the flat spot and sweep the profile along that path...But, I can't get the profile. SW won't even let me Section View it. Here's what Featureworks has to say:
      Glad we got an AE on this...No way am I going to figure this out.
      Like • Show 0 Likes0
      Actions
- Paul Salvador @ Scott Perman on Dec 19, 2020 10:08 AM
  Mark Correct
  Correct Answer
  ..(flex)... yeah... it seems to work ok? (this is a test edit - let's see if this clears the moderation?)
  Attachments
  - 05_Wheels_Frt.zip5.7 MB
  Like • Show 3 Likes3
  Actions
  - Paul Salvador @ Paul Salvador on Dec 19, 2020 9:05 AM
    Mark Correct
    Correct Answer
    ..wow.. posted this yesterday... and moderated again????
    Like • Show 0 Likes0
    Actions
    - Heiko Sohnholz @ Paul Salvador on Dec 19, 2020 9:59 AM
      Mark Correct
      Correct Answer
      Paul Salvador
      Would you please post your file (again)? I would like to take a look at your solution.
      Thx.
      btw: almost every post of mine is moderated. Last weekend I've posted a solution on Sunday, it was released on Monday. Yeah...
      Like • Show 1 Like1
      Actions
      - Paul Salvador @ Heiko Sohnholz on Dec 19, 2020 10:10 AM
        Mark Correct
        Correct Answer
        Hello Heiko,.. I just did a "test edit" and it looks like the moderation bot cleared it?
        Like • Show 1 Like1
        Actions
Heiko Sohnholz Dec 18, 2020 8:51 AM
Mark Correct
Correct Answer
Hi,
please create an additional body, than use the "Deform" Feature and the option "Surface push".
You can even drag out you profile using this:
Like • Show 4 Likes4
Actions
- Matt Peneguy @ Heiko Sohnholz on Dec 18, 2020 9:15 AM
  Mark Correct
  Correct Answer
  Heiko Sohnholz wrote:
  
  Hi,
  please create an additional body, than use the "Deform" Feature and the option "Surface push".
  You can even drag out you profile using this:
  Heiko's answer is the correct answer to this thread because you can have 2 configurations, one in the deformed state and one that's not. But, I was asked to post my solution, which I believe may be the simplest.
  
  Heiko,
  I've never used Deform. Can you post your part? I want to see how you got it to work, I tried and failed.
  Attachments
  - Tyre.SLDPRT.zip251.3 KB
  Like • Show 0 Likes0
  Actions
Paul Salvador Dec 18, 2020 3:04 PM
Mark Correct
Correct Answer
..why not release some of the virtual air pressure? (sorry, someone had to do it)
Like • Show 2 Likes2
Actions
ömür tokman Dec 18, 2020 4:46 PM
Mark Correct
Correct Answer
Maybe this gives an idea.
You can change this size to make a full round or curve.
Attachments
- SW2018.SLDPRT.zip119.4 KB
Like • Show 1 Like1
Actions
Heiko Sohnholz Dec 19, 2020 3:31 AM
Unmark Correct
Correct Answer
Here is one using "Deform".
Attachments
- 05_Wheels_Front-HS-Deform.SLDPRT.zip5.5 MB
Like • Show 3 Likes3
Actions

How to add deformation to imported tyres

Attachments

Outcomes

Attachments

Attachments

Attachments

Attachments

Attachments

Related Content

Recommended Content