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Rubber Track Design

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Message 1 of 17
mklassen78
2659 Views, 16 Replies

Rubber Track Design

Trying to model a track but i have it in more of a triangular orientation then an ovel like this sample picture. Any advice on how to pattern the tread and inner lug around any shape i desire? I have tried making an extrusion on one of the flat faces and then patterning it around but it keeps the lug in the same orientation and does not follow the contour nicely. Any advice for me

?Engineering-Rubber-Track.jpg

16 REPLIES 16
Message 2 of 17
streharg
in reply to: mklassen78

You can do rectangular pattern in part enviroment along choosen curve, and set orientation to direction1. This should work.

 

I hope that's what you're looking for.

 

Greg

PDSU 2016
4790K, 32 Gb ram, GTX 960 ...
Fancy HP LCD
🙂
Message 3 of 17
JDMather
in reply to: mklassen78


@mklassen78 wrote:

Trying to model a track but i have it in more of a triangular orientation . Any advice for me?



See this document pg 16

http://home.pct.edu/~jmather/SkillsUSA%20University.pdf


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Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


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Message 4 of 17
mklassen78
in reply to: JDMather

Thank you for your replies! JDMather that does work to pattern around and i can get it to follow the contour i want but it leaves a gap between the "treads" as it is patterned around a curve. It does not keep tangent. Any solution to that?

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Message 5 of 17
JDMather
in reply to: mklassen78

Attach your ipt file here.


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Message 6 of 17
mklassen78
in reply to: mklassen78

Hope this helps more

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Message 7 of 17
JDMather
in reply to: mklassen78

I don't see a pattern in the file you attached?

 

When I attach my solution the sketch for the tread will be on the XY plane.

The extrusion for the belt will initially be a surface body and then Thicken after the Pattern of the treads.


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Message 8 of 17
mklassen78
in reply to: mklassen78

That is why im on this forum, It will not allow me to pattern and keep tangency, It just gives an error. The lugs i want to pattern are in the file though.

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Message 9 of 17
JDMather
in reply to: mklassen78


@mklassen78 wrote:

.... It just gives an error.


 

Post screen shot of error.

 


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Message 10 of 17
JDMather
in reply to: JDMather

I experimented with this one a bit more.

It is going to be a bit more work than I originally thought.

Because the tread cleats bend around the curves - my attempt would be with patterned-trimmed surfaces, thicken and trim again.


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Message 11 of 17
stevec781
in reply to: JDMather

In theory oit should be easy with the pattern feature but from the simple example I tried it looks like Inv has a problem with following the tangency of the path when it goes around the ends.

 

 

pattern.JPG

Message 12 of 17
VdVeek
in reply to: stevec781

You can also try an Emboss function. Make a sketch with your profile and Emboss this on your track.

Have also a look at the standard Inventor Belt Design tool. In a Synchronous Belt inventor uses a pattern similar to your track.

 

Rob.

Autodesk Inventor 2015 Certified Professional & Autodesk Inventor 2012 Certified Professional.
Message 13 of 17
streharg
in reply to: stevec781

Even if you want to pattern it around, it will not fit curved surface. So maybe you should pattern only sketch, and then project sketch on surved surface, then extrude it. If i'll have time, i'll try to do it later today.

 

Greg

PDSU 2016
4790K, 32 Gb ram, GTX 960 ...
Fancy HP LCD
🙂
Message 14 of 17
stevec781
in reply to: stevec781

It doesnt need to fit the curved surface, just model them over sizes and then use a surface to trim down to the height needed.

 

I dont think you can use a sketch pattern as sketch pattern wont follow a curve, just a straight line - I think.

Message 15 of 17
nannerdw
in reply to: mklassen78

You might be able to model the belt profile in the sheet metal environment as a contour flange.  Then use the Rip and Unfold commands to flatten it, sketch the tread patern, extrude it with the Face command, and Refold.  The extruded face will stretch itself to follow the contour of the sheet metal part.

Message 16 of 17
VdVeek
in reply to: stevec781

I made this simple track with the emboss feature. First created a sketch with a pattern of the profile, dimensions linked to the geometry of the basic track to match the right size. Then emboss the sketch first on the straight part, then reused the sketch and emboss this on the curved part of the track with wrap to face option on. Last step, circular pattern the 2 embosses to the other sides. Check the attached ipt (2012) to see how i did it.

 

Inventor Rups.jpg

Rob.

Autodesk Inventor 2015 Certified Professional & Autodesk Inventor 2012 Certified Professional.
Message 17 of 17
VdVeek
in reply to: VdVeek

An other option is to use the "Bend Part"option hidden under the Model Tab, section Modify. Create the Track as a flat with profile. Then place a sketch where you define the bend distances, and then 'Bend Part'. Make sure that you don't get interference by adjusting the sketch and pattern. See my ipt for more info.

Rob.

Autodesk Inventor 2015 Certified Professional & Autodesk Inventor 2012 Certified Professional.

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