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Trouble combing two thickened lofts

going_alonggoing_along Member Posts: 13

I have lofted two surfaces and thickened them to create two parts but however I choose to combine the two they will not join and I get red warning lines crossing both parts. The first image below shows the two parts seperate, the second shows what comes up during a boolean union.

One of the parts is generated from sketches 1-3, the other from sketches 3a-4. Sketch 3a Uses parts of sketch3 but is formed on it's own plane that is on the face of plane 3. In fact I have tried various combination of using faces or planes on which to base sketch3a but always with the same result. Since the problem is on only one side the cause should be obvious, but I just cannot see it :'(

Help in pointing out what is probably blindingly obvious would be appreciated.
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Comments

  • S1monS1mon Member Posts: 49 PRO
    Onshape (and the Parasolid kernel, and many other CAD systems) has a hard time doing the boolean operation when the adjacent surfaces are wavering across one another. You started with two surfaces which share edges, but when you thicken them, the resultant end surfaces are not the same (the thickened edges are based on the surface normals). If you zoom in you can see there are little slivers that overlap but not in a super consistent way.

    You have a few options:
    1. Join the two lofted surfaces first, and then thicken.
    2. Clean up the almost adjoining ends of the two parts using replace face first, and then boolean.
    3. Create the main area first with one loft/thicken and then add the inside flanges separately, possibly with a sweep.
    4. Create cross-sections which have the thickness built in, and use a solid loft. It would be challenging to make the second lofted area the same wall thickness as the first, given how they join.
  • going_alonggoing_along Member Posts: 13
    S1mon, thank you for your clear explanation. I have quickly tried your option 2 without any success so far (but I have not used Replace Face before). Option 3 I tried using Sweep to extrude the flanges but this has not so far produced an exact match with the profile of the main section. Option 1 was where I started over a week (elapsed) ago but it was very difficult to get the profile structures to align which is why I recently simplified down to having 2 separate parts as you see now.

    However now that I know what was going wrong I can work at it.
  • alnis_smidchensalnis_smidchens Member Posts: 166 EDU
    Whenever there's a cranky boolean with two close-but-not-quite faces, I often just toss in a move face for 0.1 mm (or another small number, in this case 0.2 mm) to get the parts to intersect and join properly. It's not the cleanest solution in the world, but it's "good enough" most of the time, 95% of the time. Often, with complex lofts, move faces of even 0.5 mm won't work, so just dial it back until it does. If the face(s) on one part don't work, try moving the ones from the other face. All of @S1mon's tips are also good for sure! There's always a dozen ways to approach a problem in CAD, and 99.8% of the time, at least one will work (or more if you're lucky).

    My solution:
    https://cad.onshape.com/documents/0cc3fe4007791d7bdcd16361/w/1f356037844b053a00633685/e/0a5e2b6143d12ad315558b9b


    Hope this helps!
    Get in touch: [email protected] | My personal site: https://alnis.dev | My YouTube channel (I make tutorial videos for Onshape & Inventor): https://www.youtube.com/c/AlnisSmidchens
  • Evan_ReeseEvan_Reese Member Posts: 538 PRO
    @alnis_smidchens
    I see that NX download! don't deny it!  :D

    Evan Reese / Principal and Industrial Designer with Fractal
    Website: fractalmade.com
    Instagram: @evan.reese.designs
  • alnis_smidchensalnis_smidchens Member Posts: 166 EDU
    @Evan_Reese guilty as charged! I'm currently working on modeling a fancy part in every CAD program that has an education version for practice (and for fun!). So far I have:
    Done it:
    - Onshape - went pretty smoothly
    - Inventor - barely scraped by, I had to use some workarounds to get a loft to work that involved lots of manual clicking
    - Solidworks - also went pretty smoothly especially considering how I've only recently really gotten into SW
    Attempted but failed:
    - Fusion 360 - I couldn't get it to cooperate even after trying a bunch of different methods, threw errors for valid loft setups
    Remaining to try:
    - NX
    - Creo
    - BricsCAD
    - Solid Edge
    - IronCAD
    - FreeCAD
    Ones I probably won't do:
    - CATIA - no free student version (I did actually pay for the SolidWorks student license so that I can be prepared for any SW stuff in university)
    - Microstation - It looks like quite the process to get a student version, including having my school contact them. I will probably spend more time trying to get a license than I will modeling this part.

    If anyone has suggestions for other CAD software I should check out, please let me know! Also, here is the part I'm modeling:


    Get in touch: [email protected] | My personal site: https://alnis.dev | My YouTube channel (I make tutorial videos for Onshape & Inventor): https://www.youtube.com/c/AlnisSmidchens
  • Evan_ReeseEvan_Reese Member Posts: 538 PRO
    @alnis_smidchens
    Cool project! I hope you're making it into a video.
    @going_along
    I didn't mean to hi-jack your thread. Were you able to get your question answered? I'm glad to take a look if not.
    Evan Reese / Principal and Industrial Designer with Fractal
    Website: fractalmade.com
    Instagram: @evan.reese.designs
  • michael3424michael3424 Member Posts: 527 ✭✭✭
    @alnis_smidchens - You might try Alibre.  They should have a 30-day trial version but I don't think that they have a free educational version.  Their basic (hobby) version is $199, I think, but that is pretty limited compared to Onshape.

  • matthew_stacymatthew_stacy Member Posts: 111 PRO
    @alnis_smidchens , what's the current Microstation product for mechanical design?  I started off with Microstation Modeler, but that was ... ugh in the 1990's.  I thought they ditched the mechanical engineering audience decades ago.

    Unfortunately I wasn't prescient enough to purchase SolidWorks when I was starting out.  But with Onshape I get a second chance to follow Jon Hirschtik's vision!

    Cheers,

    -Matt

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