15 Replies Latest reply on Oct 24, 2012 6:49 AM by Peter Edmonds

    Won't Allow for Continuous Loft

    Elinor Mileti

      I'm attempting to remodel a handle (file attached). The file was gigantic and a mess, so I exported and then re-imported as a parasolid file and ended up with an imported surface. From there I used split lines to create a series of profiles from which to loft. Using more split lines I created splines to help define the lofts.


      Need: I need to create one continuous surface loft across all the profile sketches.


      Problem: I can loft sections, but continuously get errors when trying to loft across all the profiles together.


      Please help me make this lofted surface!! I feel like I've gotten so close, but no cigar.

        • Re: Won't Allow for Continuous Loft
          Bjorn Hulman

          Elinor, I open your file, rolled back to the original surface, deleted the round flat recessed face, did a fill surface on the edge that was created, checked the merge box and the create solid box and got a solid body.


          I'd also recommend using far less profiles when attempting to loft and controlling it with guide curves. Also, have a go at some surfacing tutorials and have a look on youtube, there are some really helpful videos out there that will show you some handy techniques.

            • Re: Won't Allow for Continuous Loft
              Elinor Mileti

              I realize that I can utilize fewer profiles, and have attempted lofting without selecting all of them to no avail anyway. That's not my concern though.


              I altered the surface since I do not need the recessed face at all, and ended up with a single (knit) surface which mirrors itself across the front plane.


              From there, I do not need a solid body. What I'm looking for is a way to take the geometry from this given surface, create profiles across it to loft from and end with a new (albeit identical) surface with editable features. I need it done this way because I work in R&D and future alterations are a possibility.


              Given the file above, and this file, can you explain what it is that is going wrong?

            • Re: Won't Allow for Continuous Loft
              Peter Edmonds

              Elinor, Bjorn, Mark


              I've just been referred (through I Get It) to this thread in an effort to solve another issue.


              I haven't looked at your model. I've been trying to generate a boat hull surface that is developable, and get a rollout flat part. As part of this I have exploited generating a surface between two profiles with multple guide lines - fairly standard SW stuff. Im my case the profiles were open 3D spline curves, representing the centre keel profile and an outer pseudo chine line. I set up the guide curves as a series of straight lines, skewed in 3D boat space, These lines represented a continuum of press/roll lines that could be used to curve up the eventual flat plate. I intend them to ensure that the SW surface is developable.


              It may well be worth exploring one or more guide curves in your model. This technique is introduced in the Lofts and Splines lesson 3 in the Advanced Part Modelling Training Manual 2009 (when I did the course), and I expect elsewhere. Mark refers to the guid curve in his post of Jun 21.


              Any guidance on where to go for solution to my rollout issue?

                • Re: Won't Allow for Continuous Loft
                  Kevin Quigley

                  Creating developable 3D surfaces is a complex task requiring add ons or other software. Rhino has a developable surface tool that enables this, but most marine designers use specialist tools (add ons for Rhino) for this.


                  The only way to get a flattenable surface in SolidWorks is to make sure the surface bends in one axis only - think sheet metal. As soon as you go double curvature you are into the realms of specialist add ons / othert software.


                  Of course you can fake it, but this takes years of experience of working with the materials and geometry, and even then it is often trial and error. We used to do this for getting the sheet flat forms for pressed steel parts - but it was never that accurate.

                    • Re: Won't Allow for Continuous Loft
                      Peter Edmonds



                      A reply to your earlier e-mail, after I had sent the other reply.


                      I tried Rhino a few years ago, but it didn't do much for me. The ruling lines went the wrong way, and I couldn't see how to conbtrol them. Much better to generate shapes in "real" marine hull software.


                      I agree with second paragraph. I;ve achieved tins in SW by using the straight lines as guide curves between the 2 profiles. This keeps me out of double curvature.


                      what I am doning I don't regard as faking it - it is just an understanding of the geometry. Think the series of cones, which is how we did it before computers were availoable. I regard an understanding of the geometry as a valid alternative to trial and error. Think the straight generator lines, which represent the roll/press lines on the plate as you bend it to shape. try this on your next pressed steel parts - it isn;t hard. Think the traditional ductwork transition round to rectangular (with radius corners) - documented in SW. It appears in I Get It Sheet Metal Lesson 65.


                      Ask me again in a few months when I have some more procuction expereince.I should be able to send examples if/whebn required.



                  • Re: Won't Allow for Continuous Loft
                    Kevin Quigley

                    I've not got time to look at this in detail but if I was doing this I'd avoid lofting and use boundary surface tool. Using this tool you have a lot of control over edge conditions. I would also tend to work on one half, and create a helper surface aloing the centreline to build the boundary surface from.


                    The general rules I work to are:


                    1. Lay down the wire frame first (sketches - try to keep to 2D planar sketches and use as few as possible, and keep sketches as simple as possible).

                    2. Create a helper surface on centre line as dictated by your sketch network.

                    3. Get the big surfaces in first to define the shape.

                    4.Mirror, knit into solid then apply smaller fillets etc as a solid

                    5. Tidy up awkward areas using delete face/fill surface/knit into solid


                    Unfortunately there are no shortcuts with this when you are copying existing data.


                    However if you are creating from scratch you can look at supplementary tools such as Modo/T Splines for a more freeform approach.


                    Also in SolidWorks 2013 consider using the new Intersect tool to rought out the main surfaces and then create a solid from the enclosed shapes.

                      • Re: Won't Allow for Continuous Loft
                        Peter Edmonds



                        Thanks for the suggestions. I'm already into 3rd party software for shaping. I used HULLFORM (a Perth development by Peter Rye), which supports development using Kingore's algortithm with ruling lines between longitudinal lines. I am now in the process of starting up in DELFTship; initially in the free (earlier) version.


                        In the current project I have been back to the conic sections as we used pre-computers, with some support from HULLFORM. .I entered 3D point offsets ex HULLFORM direct into SW. I copied 2 longitudinal lines as splines, then used Lofted Bend between them, and achieved rollout. The generator lines (straight on the surface) are skewed in 3D space, but only small conical cunvergence. The rollout looks all right on the screen. 


                        I achieved the rollout after posting this morning.


                        In the future I want to generate my hull shape in DELFTship and transfer as an IGES file.


                        I look forward to exploring the boundary surface; found on the Surfaces toolbar. However I can't find it in the Glossary or under Help.


                        Regards from Perth, W.A.


                        Peter Ednibds

                        Naval Architect