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Troubles with Loft

hansrudolfhansrudolf Member Posts: 40 ✭✭
Hi, Hansrudolf here again...

I was trying to generate a loft between a circular tube and a rectangular tube, but failed miserably. So just for testing I tried a loft between two circular tubes, to create something like a funnel, but that didn't work also.  What I can do in that latter case is doing two surface lofts, from the inner and from the outer circles. But I think the result is not a solid, and not suitable for 3D printing.
When I select the faces (*) of the tubes, then one shows two yellow circles, but the other a yellow and a red one. The loft then does not show, and the error says: "cannot use faces or regions with inner loops as profiles." Now I don't know where there is an inner loop...

(*) should I try to better specify which faces I mean? Unfortunately I know not a better word for these. The faces you see when you cut a tube with a saw.

I hope someone can tell me what I'm doing wrong.
Many thanks,
Hansrudolf

Comments

  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,312 PRO
    The hard one first, loft will match vertices, split the circle up to match the corners of the rectangle. 

    More complex, create bridge curves from corners to circle, then use them as guides in the loft.

    Circle to circle, you need to pick more carefully. Pick the circle also defines the start of the loft. If the points aren't projected, then you get an hour glass.

    The best way think of a loft section is by percentage. If I pick 4 things, the path is from 0 to 1 traversing 4 things. Each loft section is going from 0 to 1 and the loft is trying match things up.

    You can stop this behavior by breaking things up or adding guide curves.

    And of course, why work with solids when you're creating surfaces. At the end you can enclosure your surface patches. This is actually the best way.

    Post an image when you're done.



     

  • romeograhamromeograham Member Posts: 256 PRO
    edited July 23
    Solid lofts cannot use profiles like the end of a tube: the inside wall of the tube is the "inner loop" that the error is referring to.

    One workflow is to loft two Solid profiles (like the end of a cylinder to the end of a solid box), then using the Shell command to create the hollow tube shapes.

    Here's an example: https://cad.onshape.com/documents/9129bd3e586ee8b1d71c6661/w/1a6076cddbda554bf42d47fa/e/5a28262c7299d2fe34173a12



  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,312 PRO
    @romeograham

    Nice example!

    Notice the transition is composed of 4 surface patches. The circle is automatically being divided into 4 segments. You gotta love parasolids. Many systems will force you to match vertices. Pro/e in the early days made you have an equal number of vertices in the from/to direction. What we have here is much easier.

    You can over ride this blend and create anything you want by breaking up the circle yourself. I don't know why you'd want to though.

    I like Romeo's geometry.


  • romeograhamromeograham Member Posts: 256 PRO
    Thanks @billy2

    I was trying to show the minimum viable example for this feature. The "inner loops" error that Onshape has is confusing, especially if coming from another system that would have handled @hansrudolf 's example without trouble (SolidWorks, for instance). Onshape is fantastic, and requires minor rewiring of our old brain pathways at times.

    Once this feature is working, one can start to play with continuity at the Start / End, more complex profiles, guides etc to capture design intent better.


  • larry_haweslarry_hawes Member Posts: 427 PRO
    Thanks @billy2

    I was trying to show the minimum viable example for this feature. The "inner loops" error that Onshape has is confusing, especially if coming from another system that would have handled @hansrudolf 's example without trouble (SolidWorks, for instance). Onshape is fantastic, and requires minor rewiring of our old brain pathways at times.

    Once this feature is working, one can start to play with continuity at the Start / End, more complex profiles, guides etc to capture design intent better.


    VERY nice explanation/example Romeo, I've wrestled with the hidden logic within lofting for a long time.
  • hansrudolfhansrudolf Member Posts: 40 ✭✭
    OK, no success up to now. Spent the whole afternoon, first with what Billy2 wrote. Split the tubes in 4 parts, then I could loft one of the quarters, but the loft had a very strange form. The second and following quarters never worked.
    Then over to romeograham's method. This worked, kind of, except that my shell commands only shelled the circular and the rectangular tubes. The Loft stayed solid. I tried then to boolean add the 3 parts, but that didn't work also.
    Perhaps I should try to construct 3 separate parts and then doing an assembly?

    Kind regards,
    Hansrudolf
  • larry_haweslarry_hawes Member Posts: 427 PRO
    Can you post the link to the doc, or an example?
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 2,518
    @hansrudolf @romeograham ‘s method is the only one that will work. Make sure that “add” is selected in the loft command. 
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • larry_haweslarry_hawes Member Posts: 427 PRO
    edited July 23
    NeilCooke said:
    @hansrudolf @romeograham ‘s method is the only one that will work. Make sure that “add” is selected in the loft command. 
    THIS.... and 'merge with all'
  • larry_haweslarry_hawes Member Posts: 427 PRO
    Here's what I discovered...


  • hansrudolfhansrudolf Member Posts: 40 ✭✭
    Interesting thing, larry_hawes, but a bit difficult to follow. It looks a bit like my 'strange' loft, though.
    As I still have no success with the tips by Neil Cooke, (and I'm sure he knows what he says), I try to add a link to my part. Hopefully that works...
    https://cad.onshape.com/documents/f052bc4b56864a4770f884f3/w/eb7fb482984570f9bf0384af/e/0dba7f23c154fec5d82c8597

    Many thanks for the help,
    Hansrudolf
  • larry_haweslarry_hawes Member Posts: 427 PRO
    edited July 23
    Hope this helps...and it works with filets at the sketch level. I think it was Sketch 2 that was messing up the loft/shell

    https://cad.onshape.com/documents/826b23ea3dab4799e4eabec0/w/f2da2224d8ad385fd3eac66d/e/c14b6913bd7f9edd4d35cec5


  • billy2billy2 Member, OS Professional, Mentor, Developers Posts: 1,312 PRO
    edited July 24
    @hansrudolf
    Make sure your loft is being added to the other parts. I think you might have 3 parts.

    great job Larry with video.


  • larry_haweslarry_hawes Member Posts: 427 PRO
    billy2 said:
    great job Larry with video.
    THX Always learning...
  • hansrudolfhansrudolf Member Posts: 40 ✭✭
    Although I did my best to copy the examples, they didn't work for me. I even tried another browser, and still have the same problem. Could it be because I use the free Onshape and not the professional version? On the examples I see a horizontal menu band at the lower edge of the window, which I never see in my drawings.
    Nonetheless, I could solve my problem by drawing 3 different parts and then assembling them. Little trick was to first shelling the parts from one side only, so I had solid material for placing the mates. After assembling I could shell the parts from two sides, and hooray! Now starting the 3D Printer!

    Many thanks for all the help, really a great community. (How) can I remove the examples from my documents list?
    Kind regards,
    Hansrudolf
  • romeograhamromeograham Member Posts: 256 PRO
    @hansrudolf
    The menu bar at the bottom on the example files shows up because you have "View Only" access to those files.
    You can make a copy of your own to use. I think the menu item is here:


    You need to make sure you have "Add" selected in the Loft command to join all the parts together as you go. Then you should be able to shell the part all at once.

    This work is being done in a Part Studio (not an Assembly), so you shouldn't need Mates at all to make the Loft.

    For a View Only document, you can always see how features were made by Right-Clicking on each feature and selecting "View":


    This way you can step through someone's workflow without having your own copy of the part.

    Good luck!

  • hansrudolfhansrudolf Member Posts: 40 ✭✭
    Many thanks, that is good to know in the future. As I wrote, although I did not forget the 'add', the shell did not work. But as an assembly all worked fine, and the part is already printed successfully.

    Kind regards,
    Hansrudolf
  • steve_shubinsteve_shubin Member Posts: 95 ✭✭✭

    If I read @hansrudolf posts above correctly, while in the Part Studio, Hans never got the single part with a loft in the middle to shell all the way through.

    I’m perplexed why, as there is a lot of very helpful information above

    I’ll take a stab at it.

    In Hans second post above, Hans said that the loft had a very strange form. 

    The PART 1 GIF below shows a sketch on the face of the cylinder made with the USE tool and the SPLIT tool

    The reason for using the Split tool was because sometimes the loft TWISTS. In fact it was twisting for me when the circle was taller than the cuboid. Splitting the sketch of the circle into 4 segments, prevented the loft from twisting

    Hans, the GIFs below were made with the free version of Onshape.


  • romeograhamromeograham Member Posts: 256 PRO
    edited July 26
    @steve_shubin
    Nice reminder on the Split step. I did not realize that even with the split sketch, you can still select the faces (or did you end up selecting the sketches?) for the loft.
    That would have removed much of the weirdness that @larry_hawes was seeing with the various relative positions of the two profiles.

    Thanks!
  • NeilCookeNeilCooke Moderator, Onshape Employees Posts: 2,518
    @steve_shubin bossing it again - excellent work!
    Neil Cooke, Director of Technical Marketing, Onshape Inc.
  • steve_shubinsteve_shubin Member Posts: 95 ✭✭✭
    edited July 26
    @romeograham

    When selecting the profile of the circle to do the loft, I clicked directly on the sketch WITHIN THE SKETCH / MODELING WINDOW. I was NOT ABLE to select the circle profile to do the loft by selecting the sketch from the Features list. Be aware that I am using Onshape on an iPhone.

    Part of what helps in keeping this loft from being problematic, is that both profiles — the circle and the rectangle —have the same number of segments. The circle has 4, and the rectangle has 4


    @NeilCooke

    Thanks

  • romeograhamromeograham Member Posts: 256 PRO
    edited July 26
    @steve_shubin
    Got it. Because the sketch is showing, it gets selected automatically, and you have the 4 segments to work with. (If you were to hide the sketch OR "Select other" to select the face instead, we'd be back to the beginning with the loss of twist control). 

    I think you could (alternatively) split the face of the cylinder with your dotted lines, and work with faces rather than sketches - since the boundary of the circular face would have 4 segments, you'd have similar control to your sketch method.
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