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How to model a hose using Onshape?

3dexter3dexter Member Posts: 89 ✭✭✭
How to model a simple hose using Onshape?


Attached example.
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Comments

  • onshaperonshaper Member, Mentor Posts: 98 ✭✭✭
    edited May 2015
    It is preferred to 3D sketch this part which Onshape cannot do right now.

    Looking at it, it seems you could fully define the centerline with three workplanes and three sketches. Finally you would perform a sweep with a sketch that defines the cross section.

    Good luck!
  • 3dexter3dexter Member Posts: 89 ✭✭✭
    Onshaper said:
    It is preferred to 3D sketch this part which Onshape cannot do right now.

    Looking at it, it seems you could fully define the centerline with three workplanes and three sketches. Finally you would perform a sweep with a sketch that defines the cross section.

    Good luck!

    One problem is the 3D sketch and another is escription (MOTORE) in the hose!
  • sergio_p_sergio_p_ Member Posts: 37 ✭✭
    Hi 3Dexter! Looks like we are in the same bussines :-) I design rubber hoses, engine mounts and door sealings as well for the automotive market.

    One ugly way to model a hose would be extruding the straight portion, then revolutioning the radius and follow then with the next straigth, radius... notch marks are common extrusions, the same for the timming marks. The only problem by now would be the texts.

    Regards!



    Sergio PLUCHINSKY
    CAD, FEA and Engineering Consultor
    +54 9 11 2250 0564
  • 3dexter3dexter Member Posts: 89 ✭✭✭
    Hi 3Dexter! Looks like we are in the same bussines :-) I design rubber hoses, engine mounts and door sealings as well for the automotive market.

    One ugly way to model a hose would be extruding the straight portion, then revolutioning the radius and follow then with the next straigth, radius... notch marks are common extrusions, the same for the timming marks. The only problem by now would be the texts.

    Regards!



    We are complicating something that is very simple in other CAD software.

    But it is an alternative to 3D sketch sergio_pluchinsky.
  • brucebartlettbrucebartlett Member, OS Professional, Mentor Posts: 1,816 PRO
    +1 for 3d sketcher
    +1 for text in the 2d sketcher
    +1 for import of vectors to sketcher (could also get your text in this way)

    I know these are all on the Onshape radar. Hopefully we see these tools soon.
    Engineer ı Product Designer ı Onshape Consulting Partner
    Twitter: @onshapetricks  & @babart1977   
  • r_paulr_paul Member Posts: 22 ✭✭
    edited May 2015
  • Ben_Ben_ OS Professional, Mentor, Developers Posts: 274 PRO
    edited May 2015
    Take a top down look at the profile you want to use for the path and draw it on the top plane. Extrude.



    next look at another main plane and draw out the profile and extrude cut it out of the block



    Make a plane using the curve-point option at the end of the curve/path



    Draw the profile on the newly made plane at the end point of the path



    Next sweep the profile on the path as a new solid



    Delete the first body defining the path and voila! This took about the same time it would have to define the 3D sketch...



    All done with 3 Sketches, 2 extrudes, one plane and one sweep feature

    Here is the model
    https://cad.onshape.com/documents/a4cba537bda44adf8f377bd3/w/eb41423d8c0949569ae03b3d/e/K17Ex85HZWzDs393swcpRV3j

    Second tab is another one done more angular like. Things to note on the second one are:
    1. Use of 'Intersect' on the second extrude to reduce features
    2. When defining the path you are not stuck to one line you can select multiple sections like the initial lead out, then the following fillet, the next lead out and the next compound fillet.... etc...

    Have a look at how I did it and right click on a feature and 'rollback' to see the steps. Pro-tip, the roll back feature and dragging the roll back line up and down are a handy thing to play with in figuring out how others model and diagnostics on what may have gone wrong in models.

    All of this done on a cheapie Chromebook, on crappy wifi. So to be up and running in the CAD world is now cheap like borscht! Love it!
  • andrew_troupandrew_troup Member, Mentor Posts: 1,629 ✭✭✭✭
    sweet!
  • 3dexter3dexter Member Posts: 89 ✭✭✭
    edited May 2015
    R.Paul said:
    Thanks @R.Paul & @Ben!

    The review tool is only enabled when you select the option "Make a private copy", would not it interesting that the same was already enabled so you accessed the link?

    So anyone with the link can view and comment without the need to make a private copy!
  • Ben_Ben_ OS Professional, Mentor, Developers Posts: 274 PRO
    @3Dexter ;
    If I have your email I can share the file so we can markup and see each others edits as well FYI
  • sergio_p_sergio_p_ Member Posts: 37 ✭✭
    Realy lateraly thinked :-)

    Regards


    Sergio PLUCHINSKY
    CAD, FEA and Engineering Consultor
    +54 9 11 2250 0564
  • brent_jackson992brent_jackson992 Member Posts: 1
    Many thanks to BenE. That example really helped me a ton.
    I have found, however, that I cannot sweep a closed 3d path. Once I add the last leg, OnShape seems to get confused on how to mate the beginning and end. Closed paths work great with 2D path sweeps.

    In my case there are 2 equal curves that meet with a twist... Although my swept surface is perfectly perpendicular to one of the curves, it doesn't seem well to mate well to the other, although all end points are concurrent.
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