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Lofted Surface problem--what am I missing?

Question asked by Jim Steinmeyer on Jun 4, 2020
Latest reply on Jun 10, 2020 by Jim Sculley

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In designing a new mixer shell We are attempting to use a Skeleton sketch while in the idea phase. As our sheet metal abilities do not include being able to roll a large sheet with different radisus on each end yet we bump break the sheet with a different spread between the breaks top and bottom. To make the end model and drawing easier I am currently attempting to place a sketch in the SSP and create the lofted surface to verify it works. and currently it doesn't. I have counted the number of segments a couple of times to verify (I think) that they are the same number. When I select the sketches to create the loft it will only select part of the top sketch, and then twists the surface. Can someone please suggest where my error is? Is this even the correct method? is there a better one? Thank you

Jim Sculley Jun 4, 2020 11:11 AM

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You have selected your sketches from opposite ends. Drag either green dot to the other end:

And there appears to be a gap between segments in the top sketch.

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Jim Sculley Jun 4, 2020 11:11 AM
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You have selected your sketches from opposite ends. Drag either green dot to the other end:

And there appears to be a gap between segments in the top sketch.
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- Dan Pihlaja @ Jim Sculley on Jun 4, 2020 11:09 AM
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  Or just RMB on it in the Profiles selection area (the blue area) and select flip endpoints connectors.
  And now that I look it up, Flip connectors is only available in Boundary, and not Loft.
  
  As for why it isn't selecting the entire length....I don't know.
  
  Edit: Corrected text.
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- Jim Steinmeyer @ Jim Sculley on Jun 4, 2020 11:11 AM
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  Thank you Jim.
  Another thing that was giving me problems was that some how at the 12th segment from the middle there were somehow 2 line segments one over the other. I think that is why the lost only went just so far.
  The two together have everything working as they should.
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Jim Steinmeyer Jun 4, 2020 12:41 PM
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Ok, the next question in my continuing education in surfacing.
I needed to add a flat wing to the loft so I created a sketch and did a surface fill. My goal is to turn this into a 1/4" sheetmetal part. I understand that I will need to knit the surfaces So I select the surface fill and the loft and knit. It only did a knit with the flat next to the fill. When I thickened it then only the fill and the first segment of the loft were thickened. Do I need to progressively knit all 37 of the flats around the loft? Or is there a better way?
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- Dan Pihlaja @ Jim Steinmeyer on Jun 4, 2020 1:03 PM
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  All the faces that were created with the loft should be 1 surface body. If you added anything else, you would have to knit that.
  
  Expand your surface body folder in your tree and see how many surface bodies you have.
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- Jim Sculley @ Jim Steinmeyer on Jun 4, 2020 1:04 PM
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  Jim Steinmeyer wrote:
  
  Do I need to progressively knit all 37 of the flats around the loft? Or is there a better way?
  No, something is not right. It should work.
  
  Can you you upload the latest file?
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  - Jim Steinmeyer @ Jim Sculley on Jun 5, 2020 9:24 AM
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    Sorry for the delay, I was at lunch.
    The updated file is attached.
    
    Thank you
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    - Jim Sculley @ Jim Steinmeyer on Jun 5, 2020 10:39 AM
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      After thinking about this for a bit, I think you may be making this much harder than it needs to be. Is there a reason you aren't using a lofted bend here? You only need to define the theoretical arcs (no segments, no surfaces), and SOLIDWORKS will handle the faceting for you. It even allows you to have your tangent flat on the end, all in one feature. You use two planar sketches, like this:
      
      Set up your lofted bend as you require:
      And voila!
      
      Flattened:
      More information here:
      2020 SOLIDWORKS Help - Creating Lofted Bends
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      - Jim Steinmeyer @ Jim Sculley on Jun 5, 2020 2:56 PM
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        Jim,
        That is actually how I originally did this part. I am using a driving sketch that gives me the first two sketches. Then after I had it done and showed to the shop I was informed that they do not have the ability to roll it and need to bump break it with a shoe with varying distances between the top and bottom curves. So I thought using the radiused sketches as a guide and breaking it into segments and making a surface might be the slick way to accomplish this. That and I had just watched a presentation from our VAR about surfacing and thought I would try something new.
        I suppose I could accomplish the same thing with a lofted bend and a thin feature. I will give that a try.
        
        Thank you
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      - Jim Steinmeyer @ Jim Sculley on Jun 10, 2020 11:47 AM
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        Well we were put on a different project for a few days and finally just got back to this and something seems missing. I unsuppressed my lofted bend, deleted it so I had the sketches available and attempted to recreate it using the help page you referenced. For some reason I do not appear to have all of the options listed in the help page. Steps 6, 7 and 8 seem to be unavailable in my property manager. Is this a new feature in 2020? I am still on 2019 but I think the network manager for 2020 was loaded last night so I may be able to upgrade if needed.
        
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        Jim Steinmeyer @ Jim Steinmeyer on Jun 10, 2020 12:13 PM
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        And then I figured it out by selecting the bent option.
        Thank you again Jim.
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        Jim Sculley @ Jim Steinmeyer on Jun 10, 2020 12:22 PM
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        In order to see the 'Bend Line Control' options in the property manager for 'Formed' lofted bends, the profiles have to have the same number of segments. Since only one of your sketches included the straight tangent portion, the controls were not shown. As you've discovered, the 'Bent' option doesn't have that requirement.
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Lofted Surface problem--what am I missing?

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