9 Replies Latest reply on Aug 19, 2009 11:34 AM by Matt Lombard

    Lofting issue

    Jason Aspinall

      Attached in a 2009SP3 file of a small envelope I'm trying to produce with a 5 plane loft.  It should be readiy apparent looking at the three profile sketches and two guide curves what the shape is supposed to look like.  However, for some reason I cannot get Swx to follow the guides properly.  Instead of getting a uniform section through the model following the guides, it appears to be ingoring some control points and creating a model much larger.

       

      Any ideas how I control this?

        • Re: Lofting issue
          Matt McKendrick
          I would place more guides curves connecting point-to-point of each sketch, even on the corner radii start and stop points.  This should force the connectors into position.  Also, how you select each sketch will determine where the connectors end up.  Try and select each sketch on the center-top line, and the connectors should line up properly.  On the attached part, I merely selected the sketch entities like I described above.
          • Re: Lofting issue
            Matt Lombard

            You can't do something like this all in one feature. You should do this in 3 features. One would be the main 4 sided shape, and then one feature each for each end cap. And use surfaces (boundary and fill). And you'll need to know how to use the SelectionManager. You could actually do this completely without the guide curves.

             

            Once you get into the groove of working this way, it will change how you look at modeling.

              • Re: Lofting issue
                Jason Aspinall

                Mmm, to be fair, I don't do a tremendous amount of lofting, never needed to in the job I do (and I've been a user of swx since 1997!), and now I do :/

                 

                Since posting the question, I've been fiddlind around with the job, and see that the aspects giving me most grief are the points on the top & bottom sketches.  Creating the loft minus those two points produces exactly the shape I'm after, less of course the rounded ends...then I set about simply "doming" the two flat ends, which would result in someting along the lines as to what I was after, but not quite.  Seems producing the "domes" do not follow the same radius as the sides, creating a reverse rad from the edge off the long rad, around to the "point" on the top/bottom sketches.

                 

                I'm now disecting your model to see how you create the same with boundary surfaces (which I've *never* used before).

                 

                Cheers!

                • Re: Lofting issue
                  Jason Aspinall

                  One further question Matt, this surfacing boundary modelling appears to be doing the job quite nicely, except for the fact it's producing just surfaces.  I need this part to be a solid, so I can then split it half, shell it out and carry on with the design...

                   

                  How does one go about solidifying it?

                    • Re: Lofting issue
                      Matt McKendrick

                      You need to completely close the surfaces, no open gaps.  Use the Knit Surface feature, select all of the boundary surfaces that define the outside of the desired solid and check "try to form solid".  That should do it.

                      • Re: Lofting issue
                        Christopher Thompson

                        Are are the surfaces joined together? If not use the knit function. There can be no open surfaces or gaps.

                         

                        If all the surfaces are joined together (knitted), than use the thicken feature and select the make solid option.

                        • Re: Lofting issue
                          Matt Lombard

                          wow, the surfaces don't knit. (in 2009)

                           

                          wassupwiddat?

                           

                          Interestingly, I can neither confirm nor deny that you can or can't make the knit happen in a certain beta version of a certain CAD package. See the solid and surface bodies folders counts? Something to look forward to anyway. Long way to go to get a good example file.

                          loftmatt.jpg

                            • Re: Lofting issue
                              Jason Aspinall

                              Got the part solid now, it was the "minimal adjustment" causing problems...with it off it doesn't appear to have changed the model.

                               

                              As for shell it out etc... I'll almost certainly go down the road of using the Split feature to create the new new bodies, derived from this part, just in case I need to tweak the basic shape so I can then filter those changes into the new bodies.

                               

                              Thanks for your help