27 Replies Latest reply on Jun 11, 2012 4:41 AM by Kevin Quigley

    Issues working with imported NURBS surface models

    George Maddever

      Hi everyone,

       

      I'm trying to integrate SolidWorks with a NURBS surface design front-end and having some issues. The designer at the front-end can manipulate the outer shape within a set of constraints, after which the NURBS surfaces are passed to SolidWorks as an IGES model.

       

      The model imports fine into SolidWorks and forms a solid with no errors.

       

      When in SolidWorks, I need to be able to use this external geometry to create some internal geometry, However there are faults on these NURBS surfaces (points of small radius) that prevents me using SolidWorks features like "offset surface", or "shell".

       

      I've tried unsuccessfully for ages to get the guys generating the NURBS surfaces to sort their geometry out, but with the shapes they're modelling, for some reason we get these beautiful, lightly curved, continuous surfaces that have these tiny, tiny points of tight radius, where NURBS edges meet.

       

      Beyond trying further to get these guys to eliminate these issues, is there anything in SolidWorks or a third-party plug-in that I can use to fix these errors? I'm tearing my hair out trying to get a usable NURBS model that behaves in SolidWorks. If I could just get SolidWorks to "ignore" areas of the surface where radius goes tighter than a certain amount, and just paint over it, that'd be bliss!

       

      Thanks in advance,

       

      George.

        • Re: Issues working with imported NURBS surface models
          James Pare

          Try igs in & out (round tripping)

          this can fix some surface errors that are usually difficult to get rid of

          • Re: Issues working with imported NURBS surface models
            Jerry Steiger

            George,

             

            I hate to say it, but you might need to build the surfaces in SolidWorks. Even then, you may still have the same types of problems and need to try different methods for making some of the problem faces.

             

            Jerry Steiger

              • Re: Issues working with imported NURBS surface models
                George Maddever

                Jerry,

                 

                Sadly I don't think that's viable. We're trying to build a system here that I can automate a SolidWorks process based on models coming through from a NURBS modeller and some parameters from a database. Each model will be different and the process needs to have a high degree of automation. Re-modelling each shape in SolidWorks would take, say, an hour per time, and with the volumes we're looking at getting through the system we'd need several seats of solidworks and full-time operators to make it work.

              • Re: Issues working with imported NURBS surface models
                Alin Vargatu

                George, can you post such an example?

                • Re: Issues working with imported NURBS surface models
                  Jeff Mowry

                  I wonder if you can trim off the areas of tight radii, extend the new edges to meet again (or fill with something other than tight-radii), and reform the solid.  It's not a very good method if the guys upstream keep modifying things, but if not, it will probably work fine.

                  • Re: Issues working with imported NURBS surface models
                    Kevin Quigley

                    I did a quick 2 minute edit of your IGEs file using above method. Literally 2 mins. The top surface is OK, the bottom has a slight indent in the centre, but this could be solved by adding curves to act as guides. Probably another few mins. Looking at the IGES in Rhino it has been created very lazily - all they need to do is create some centre line helper surfaces and rebuild the surfaces from these. This will sort out the tangency issues no problem.

                    • Re: Issues working with imported NURBS surface models
                      Michael Kasten

                      George,

                       

                      I have opened the IGES file in Maxsurf to check out the tangency issue.  The model seems generally well done, but could be simpler.  The issue you are having is definitely the result of the NURBS modeling not having been done to actual completion.  By this, I mean in order to have tangency across the centerline, the center control points must be perfectly aligned with the matching control points on either side. 

                       

                      Maxsurf has a good tool for this called "Align to Vector" whereby you select two control points to establish the vector, then select others that you want aligned with the vector, in this case the matching centerline controls (there are two control points on center, one for each side). 

                       

                      The attached image shows the non-alignment across the CL (where the control net is stepped).  The controls simply need to have exactly the same height and longitudinal position.  It is easy to fix, but this should definitely be done by the NURBS modeling guys rather than trying some crazy workaround in SW...

                       

                      (I don't use SolidWorks but often need to exchange data with SW, which is problematic on my end, especially with surfaces that SW has "lofted" automatically, which are inordinately complex.)

                       

                       

                      QUESTION... Does not SolidWorks have the ability to expose the underlying NURBS control net, and thus gain control of the NURBS geometry...?? See attached perspective image...

                       

                       

                      Michael Kasten

                        • Re: Issues working with imported NURBS surface models
                          Kevin Quigley

                          In answer to your question, no SolidWorks cannot expose the underlying control points for the surface. I personally see this as a big flaw. Only by opening a SolidWorks file in Rhino (or another system that can access the CVs) do you really see the quality of a surface. In general SW surfaces are a bit on the heavy side - especially those made using Boundary or Fill.

                           

                          If there is one thaing that would allow better surfacing inside SW it is the ability to expose the CVs and allow direct editing of the CVs. But you cannot do that and retain a full history/associative system execpt if you embed it inside a feature (as Autodesk do with Alias Design for Inventor), or indeed SW do with Freeform (but that only applies to a surface face not the edges or multiple faces).

                            • Re: Issues working with imported NURBS surface models
                              Michael Kasten

                              Kevin,

                               

                              Thank you for this reply and for explaining the "history" rationale.  Understood now why.   And you are entirely correct to say that the SW auto generates surfaces are on the "heavy" side - quite an understatement...

                               

                              Does anyone use T-Splines (tsElements) to actually initiate NURBS models inside SW...?  Or is it only for manipulating imported NURBS from Rhino...?

                               

                               

                              Michael Kasten

                                • Re: Issues working with imported NURBS surface models
                                  Kevin Quigley

                                  We use tsElements and Rhino/TSplines and Modo. TsElements can only be used to import meshes as obj files or TSplines surfaces. Once in SolidWorks you can edit the resultant surface by editing faces edges or points on the TSplines surface. There are a few hidden commands including extrude face where you can add faces but on the whole tsElements is mainly an editing tool.

                                   

                                  The great thing about TSplines or tsElements is that you can import meshes and let then do the conversion to Nurbs. And they do a great job as well. Autodesk made a smart move buying TSplines!

                              • Re: Issues working with imported NURBS surface models
                                George Maddever

                                Thanks for all the advice so far guys and girls!

                                 

                                SO far this is proving a tough nut to crack.

                                 

                                We've done a bit more work on the front-end surface model  and it behaves a lot better in Rhino. However, we're still having singularity issues with SolidWorks in terms of offsetting surfaces. It's still giving us low radius artefacts despite the model showing up as fine natively in rhino.Pinch.JPG

                                 

                                It seems to be a real issue with SolidWorks and clumsiness with working with NURBS surfaces. If we produce holed surfaces with clearance around the singularities and patch them in SW, we get something we can work with. The strange thing is it behaves inconsistently. You can offset it 10mm (say), it offsets fine. Offset it 20mm it fails. Offset it 30mm and it succeeds. Offset it 50mm and then offset that back 30mm to get the 20mm that fails and it works!

                                 

                                It's this kind of inconsistency which is doing my head in. I can generate models I can work with, but getting them behaving themselves in such a way that I can start to write an API to deal with customised shapes in a consistent and efficient manner is, as yet, eluding me!

                                  • Re: Issues working with imported NURBS surface models
                                    John Layne

                                    George,

                                     

                                    Can you post the Rhino Model?

                                    • Re: Issues working with imported NURBS surface models
                                      Kevin Quigley

                                      George, this is not a SolidWorks issue. It is still down to the way the surface has been created inside Rhino.

                                       

                                      I attach a screenshot of the area inside Rhino, with surfaces offset by 10 and 20mm.

                                       

                                      Note how the surface is created with a singularity point at the area identified in your screenshot? I imagine the end cap surface was created using a revolve or loft around an axis in Rhino. This type of modelling allows for quick surface generation but is inherently poor quality. Incidentally Rhino offsets the surfaces but flips the other side - so you cannot create a complete offset surface in one operation. The Rhino kernel allows quite a lot of flexibility for this sort of stuff, whereas parasolid is a bit more rigid. Exactly the same issue would happen in most solid kernels in other modelling apps. I tried it in SharkFX as well (ACIS) - also fails.

                                       

                                      So, it comes back to the issue - the quality of the modelling inside Rhino. The problem is that a lot of designers create surfaces that might look OK in Rhino but they allow for no downstream quality. Contrary to popular opinion (and not helped by CAD vendors) creating quality manufacturable surfaces is a time consuming affair that requires skill and understanding of the underlying technologies. There are no shortcuts - even using things like TSplines needs some care.

                                       

                                      I would suggest, as a back up option you consider doing all the modelling inside SolidWorks, or you must be prepared to do some editing inside SolidWorks.

                                       

                                      If your Rhino guys don't understand the issue tell them to check out Autodesk Alias tutorials online - or better yet take a look at the CadJunkie's Rhino video on the infamous 3 sided corner. It is not exactly the same issue as you have, but it shows the principles involved.

                                       

                                      http://cadjunkie.com/1515/the-dreaded-3-way-corner

                                       

                                       

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