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Folding a linear sketch pattern round a curve

stephen_allenstephen_allen Member Posts: 16
edited July 17 in Community Support
Hi everyone,

I'm out of my comfort / knowledge zone with a project. 

I'm trying to model a toothed belt profile for a replacement RC tank tread for 3d printing. 

I want the replacement tread to be one continuous surface, with 46 curved "teeth" which fit into the existing trapezoid shaped holes in the drive wheels (pictured here http://imgur.com/a/Pcc6j6S).

I've modelled one section in this document:


There are two design constraints:

(1) I'd like to avoid joining, so one continuous circle is required.

(2) the circle would have to be folded in on itself to fit on a 180mm x 180mm print bed (like this picture http://imgur.com/a/TscEQ39)

I don't think face or part patterns will do the job, so any help would be appreciated 

Best Answer

  • MichaelPascoeMichaelPascoe Member Posts: 463 PRO
    edited July 19 Accepted Answer
    When you pattern a part along a curve, the part rotates with the curve. The tooth profile was drawn tangent to a flat line which would be fine if you are making a flat belt. However, when the tooth was patterned along the curve, the tangent portion of the tooth was cutting into the belt creating the "artifacts" which were also the source of the shell failure. If you extend where the tooth meets the belt, it will give the curve pattern tolerance to rotate the tooth along the curve without cutting into the belt. Remember, if you want more mathematically correct teeth, it would be best to use equations to drive a sketch. This method should be fine for what you are using it for.

    https://cad.onshape.com/documents/5824eab54cd33d78e2efc340/w/6780e46751ef4421f90ee54f/e/f4d3c652bb34a481c8fd6e30

Answers

  • MichaelPascoeMichaelPascoe Member Posts: 463 PRO
    edited July 17
    Hi Stephen,

    There are several ways you could do this. Here is an approach that is not equation intensive:
    • Create variables of the dimensions that you want to easily change.
    • Sketch the main shape of the belt. Note: this needs to be properly constrained in order to easily adjust the size.
    • Sketch one tooth and one tread, placed in a symmetrical location for patterning.
    • Extrude the main belt, a single tooth, and a single tread.
    • Composite a curve for the curve pattern path. This is not necessary but saves clicks.
    • Curve Pattern the tooth then the tread or vice versa. (Note: the path I have chosen is in the center of the flexible portion of the belt to ensure the teeth and treads flex back to the right position when unfolded.)
    • Measure the length of the belt with custom feature: Measure Value by @konstantin_shiriazdanov
    • Adjust "sketch - Main" until you get the belt length you desire. 
    (Note: For a more exact length, you will need to set up equations to drive the main sketch.)

    https://cad.onshape.com/documents/5824eab54cd33d78e2efc340/w/6780e46751ef4421f90ee54f/e/376e9f3d866048f4d4c9c364




  • stephen_allenstephen_allen Member Posts: 16
    Thanks, I'll try that once I get back to my desktop PC.

    One question is whether that will work with the wavy belt design I'm after. The continuous belt tread above will be more like a construction line, and the teeth will be hollow.

    As an example of what I'm trying to achieve something like this existing belt on thingiverse https://www.thingiverse.com/thing:15528

    The reason for that is to take advantage of the flexibility of curves in non-flexible plastics like PLA and ABS
  • MichaelPascoeMichaelPascoe Member Posts: 463 PRO
    edited July 17
    Ah, in that case:

    Instead of drawing the treads and teeth the way I did, draw the shape you would like to be removed. Then when you curve pattern the treads and teeth, click the remove tab instead of add.

    https://cad.onshape.com/documents/5824eab54cd33d78e2efc340/w/6780e46751ef4421f90ee54f/e/376e9f3d866048f4d4c9c364


  • stephen_allenstephen_allen Member Posts: 16
    That's fantastic- thanks very much.

    The real elegance in that solution in the shell to get the continuous thickness.

    I notice there are two artifacts (I think of the Extrude of the belt centre) opposite each other on the inner curve. I'll have a play with the actual tooth profile this morning and see if they persist. If they do, I guess I can either trim them post-print, or could boolean subtract something to trim them?
  • MichaelPascoeMichaelPascoe Member Posts: 463 PRO
    The artifacts are probably due to the radius of the bend in the belt being too sharp for the parameters you have given it. If you play around with those bends, that may fix your problem.
  • stephen_allenstephen_allen Member Posts: 16
    Thanks for all your help.

    Unfortunately I'm still struggling here a bit. Hopefully your advice will work for the artefacts, however I'm having a more fundamental problem.

    I've added my "production" tooth profile and removed it as you kindly suggested above - but the shell is now broken, with no clear error.

    Here's where I have got to:

  • MichaelPascoeMichaelPascoe Member Posts: 463 PRO
    edited July 19 Accepted Answer
    When you pattern a part along a curve, the part rotates with the curve. The tooth profile was drawn tangent to a flat line which would be fine if you are making a flat belt. However, when the tooth was patterned along the curve, the tangent portion of the tooth was cutting into the belt creating the "artifacts" which were also the source of the shell failure. If you extend where the tooth meets the belt, it will give the curve pattern tolerance to rotate the tooth along the curve without cutting into the belt. Remember, if you want more mathematically correct teeth, it would be best to use equations to drive a sketch. This method should be fine for what you are using it for.

    https://cad.onshape.com/documents/5824eab54cd33d78e2efc340/w/6780e46751ef4421f90ee54f/e/f4d3c652bb34a481c8fd6e30

  • stephen_allenstephen_allen Member Posts: 16
    Thanks, I understand now.

    Yes, for my purposes of a "community" repair for a low-powered toy, an approximate tooth profile is enough. The design decisions favour curved profiles over precision so as to ease the strain on points of the printed part.

    Ironically I did have something like that flared design as the original tooth profile. I'll re-check that design and see if I can recreate it.

    Thanks again for your help. It's wonderful to have such a great community of pros like yourself willing to assist us more casual makers when we are stuck.
  • MichaelPascoeMichaelPascoe Member Posts: 463 PRO
    Happy to help  B)  

    Let me know how it goes, if you have the time. Sounds like a neat project.
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