20 Replies Latest reply on Oct 13, 2016 9:55 PM by Paul Salvador

    Solidworks and "faulty faces"

    Mikael Martinsson

      Why does SW struggle so much in handling "faulty faces"?

      We use SW for mold design, but we don't use the mold tool function and one reason is because of this problem.

       

      The parts for the tools (engine block, flywheel housing, gearbox housings e.tc.) comes mainly from Catia, Creo and Siemens NX.

      Regardless if it's a step file or a native file, we will always get a solid after import, sometimes with the addition of a quick diagnostic->heal gaps.

       

      But in 99% of the cases, we are left with "faulty faces", some that won't repair automatically but instead needs to be replaced one by one.

      The "faulty faces" looks ok, even if you turn on zebra stripes or similar, but SW considers them faulty and we can't spend a day to repair each time a customer sends a new revision.

       

      So today we use the cavity function, creating a "base part" with the mold block and its cavity together with all parting surfaces to split the different components (core, cavity, slide e.tc.)

      This always work if you can get a solid body after import. No matter if there still are faulty faces.

      But sometimes I would prefer going with the surface approach instead of base part approach.

       

      So i tried another idea:

      - I made my mold base part, and splitted the solid with my parting surfaces to a core and a cavity solid.

      - Then i removed all outer surfaces from the solids and was left with 2 surface bodies, representing core and cavity.

      - Finally i tried to use the offset/copy surface to copy one of these surfaces to a new part, but SW refuses since it is "faulty".

       

      So the surface is complete, no need to knit anything, only to make a copy, but Solidworks says "NO".

      This is really frustrating.

       

      I know that one solution here would be to export the surfaces to parasolid and import them in a new part, but that mean losing the link to the original part.

      Why is it so hard? I can still use these "faulty" surfaces to cut a solid, but I can't copy them into a new part.

        • Re: Solidworks and "faulty faces"
          Steve Calvert

          because it is hard to convert 100% of the stuff...

           

          Steve C

          • Re: Solidworks and "faulty faces"
            Mikael Martinsson

            Of course it is hard to do it 100%, especially on large mold parts with draft and radius.

            But that is the reality that all cad systems has to manage.

             

            When I use an imported file to make a cavity in a solid block, I can work with it and copy it to new parts even though the surfaces in the cavity are faulty.

            If I convert this solid block into a surface, by removíng a random surface, I will no longer be able to copy it to a new part.

             

            So as long as the faulty face are in a solid body, SW handles it ok. But if the faulty face are in a surface body, it wont

            • Re: Solidworks and "faulty faces"
              Tony Lancaster

              It seems that lately every step file that I open has every single face show as a faulty face. I used to be able to open step files with no issues but 2015 seems to struggle. Attempting to fix even one faulty face locks up my SolidWorks indefinitely. Does not matter the complexity of the part. it takes so long that sometimes it is easier to remodel the part entirely than to try and import a stp file and make use of it.

              • Re: Solidworks and "faulty faces"
                Mikael Martinsson

                Yeah, I have had similar experience with step files. Remodeling would be almost impossible in our case since it's really complex parts. And we will probably not be able to convince our customers to abandon Catia, Creo and Siemens for SW either.

                 

                But the question remain.

                Why can't we copy (offset/copy) an already knitted surface to a new part if there are faulty faces inside the knitted surface? I mean it is already knitted!

                Why can I get 2 knitted surfaces (core and cavity) when using Mold tool function, but then it is impossible to knit the parting surface, or any other surface, to these knitted surfaces even if they contain only one single faulty face? How was mold tool function able to knit them in the first place?

                 

                This is a big limitation on surfaces in SW. And today my only options is to have the faulty faces inside a solid body, because then, for some reason, you don't have these limitations.

                • Re: Solidworks and "faulty faces"
                  Scott Harvey

                  Can you upload a part with faulty faces you are having trouble with.  If your part is proprietary and you know what area causes the problems then butcher the part by cutting all around the defective area for us to see.  Don't just say you can't.  If you want to drive past this challenge we need to see what you are dealing with.

                   

                  You are preforming one of the most challenging procedures SolidWorks has to offer in my opinion.  Even though I feel I am very good at handling faulty faces sometimes I reach back to my client and tell them to remove the faulty fillets (fillets in my experience are typically the culprit for bad imports).  I then proceed to import the corrected model and add the fillets back in after the imported feature.  Sometimes that means 100 fillets, but adding 100 fillets takes me a hell of a lot less time than patching 100 fillets.

                  • Re: Solidworks and "faulty faces"
                    Tom dunn


                    My surfacing book says to use a Parasolid .x_t format if possible. The Parasolid is the native modeling kernel for solidworks. A Parasolid file is not a translation but a direct read into solidworks.Therfore, if the Parasolid format is available, it would be the first choice of any 3d format to bring into SolidWorks.  Not sure if this is an option or will help out with missing faces. Tom

                    • Re: Solidworks and "faulty faces"
                      Mikael Martinsson

                      Scott:

                      I'll have to come back to this later on, with an example, when the work load is a litter lower. Proprietary issues as you mention. Anyway, my question is still not how to repair all surfaces in an imported file. I can do that, but not within reasonable time if the solid body built from say 20 000 surfaces has 150 "faulty" ones.

                       

                      Tom:

                      Absolutely, but unfortunately with large customer you don't have this option. It is more like "handle what you get".

                       

                      And again, my question is more "why Solidworks can't do some things when the model is a surface, containing faulty faces, but if it is a solid, still containing faulty faces, it will". Perhaps this is a limitation in the Parasolid kernel? I don't know.

                       

                      One example:

                      I import a step file, resulting in a solid body with faulty faces according to diagnostic.

                      - I can run the mold tool function using parting line and shut off command to create a core and cavity surface (knitted surfaces).

                      - However, I can't then knit another surface to either the core and cavity surface.

                       

                      Why? SW was able to knit the core and cavity

                       

                      Second example:

                      I open the imported file in an assembly. Then create a new, empty part.

                      - If the imported file is a solid I can use “Join” to make a copy of the imported part in the new part.

                      - If I instead remove one surface from the imported solid, converting it to a surface model, it is not possible to use the similar surface command “offset/copy” to make a copy of the surface in the new part.

                       

                      Why? Both models contains the same faulty surfaces.

                        • Re: Solidworks and "faulty faces"
                          Scott Harvey

                          You are basically saying the model imported wrong and has bad geometry.  Why is SolidWorks not able to work off a model with bad geometry?  Answer, you have bad geometry.  Can only speculate the why.  You are too far down the rabbit hole saying well this works and this does not work.  Come back up and realize you have faulty faces.  You are compounding your problem and applying the steam roller approach.

                           

                          Like I said before.  If I get a lot of errors I ask the client to remove the fillets (fillets are typically 99% of my problems) and send me back another x_t, step, or iges.  It literally takes less than a minute to apply dozens of fillets.

                          • Re: Solidworks and "faulty faces"
                            Richard Gergely

                            I am amazed you use the shut off or parting surface features. Other than split line most of that stuff is decoration.

                             

                            I do quite a few automotive tools a year with free form faces, the parts come in pants and I fix them.

                            Anyway forget parasolid it's usually the worst from Catia stick with step or iges.

                             

                            My personal favourite problem is when you can't delete faces to fix them because the bad surface is invisible, I have a trick or two for that.

                             

                            There is something you should consider quite often a lot of these bad surfaces come from the original Catia file and p*** poor modelling.

                            • Re: Solidworks and "faulty faces"
                              Mikael Martinsson

                              Thanks for your answers!

                               

                              Scott:

                              I understand your point of view, and I agree with you, having a 3d model without faulty faces will always be the best solution, no question about that. But if you can't get that, Solidworks is still able to "work off" the bad geometry as long as the geometry is a solid, but not if it is a surface. And this was still my original question, even though I am quite far down the rabbit hole.

                               

                              Richard:

                              Don't be so amazed , I don't normally use the parting surface/mold tools.

                               

                              I design a lot of tools, having a "solid" approach using the "cavity" function to create a base part with all split surfaces in it. Together with a skeleton driven assembly of all non-forming parts, it works 100% as long as you're able to get a solid body after import. With this approach I can also replace the customer part very easy when they send a new revision, and that happens a lot.

                               

                              However, I would be able to build my model more efficient if SW could copy a surface to a new part (offset/copy) in a similar way as I copy a solid (join), but it won't work due to "faulty faces". I guess I just have to accept this and continue refining my current approach.

                               

                              We share favorites regarding those surfaces that you can't click on and delete since they are invisible!

                                • Re: Solidworks and "faulty faces"
                                  Leroy Bauer

                                  I know this is an old thread, but it deals with the problems that I am dealing with right now.  I have a solid model (.igs) that has many faulty faces and gaps when imported into SW.  I have been able to get rid of a lot of them just with the auto fix SW tools.  However, I am at a point where I can't fix the rest of the problem areas.  Any help or input would be appreciated.  Thanks.

                                    • Re: Solidworks and "faulty faces"
                                      Ken Maren

                                      Good Luck.  You'd get this fixed faster remodeling it rather than trying to repair it.   All those small faces makes it nearly impossible.  

                                        • Re: Solidworks and "faulty faces"
                                          Leroy Bauer

                                          Thanks Ken.  I kind of came to the same conclusion.  However, I haven't had much experience repairing models in SW so I thought I'd throw it out there to you experts and see if there was something simple that I was missing.  I actually started remodeling it but I don't have much experience modeling with draft angles so I was getting pretty frustrated with that.  Appreciate the input.

                                        • Re: Solidworks and "faulty faces"
                                          Paul Salvador

                                          awh... guns.. ya know.. this was done many years ago.. and I actually have a model in a DAT tape from 1997?.. but someone using Pro/e posted in back in 1999, which is pretty good if you do a search.. (fun image for you, sorry, I'm not a gun person).. but your model can be translated with a few tricks... BUT still it has issues.. the MAIN issue is the tolerance which was used in the original model and the export carried that over... this model will most likely ALWAYS have issues.. starting over is the best way to clean up up.. anyhow. here is resolved (with issues) solid x_t ...fix but it is solid so you can play....   precious....

                                          precious.png

                                    • Re: Solidworks and "faulty faces"
                                      Mark Biasotti

                                      Hi Mikael,

                                       

                                      There is certainly an art to getting imported geometry 100% healed. I believe that part of the issue is the tolerances imposed by the CAD system that you're importing from and also the type of Modeling kernel employed in the building of the original model. Two examples.

                                       

                                      PTC Granite Kernel used in CREO translates quite well to SW, but if in some instances when the user changes the default tolerance in ProE to something other than it's default, it might allow them to build a water-tight model in ProE but when exported thru IGES or STEP can become a nightmare. And the reason that the tolerance was change in the first place, usually stems from an ignorance in bad modeling practice - with the tolerance change being a way to get around the bad modeling practice. 

                                       

                                      Second, different modeling kernels produce different geometric results, that are initially identical but are topologically different. One of the best examples of this is the difference between CGM and Parasolid - a.k.a. CATIA and SolidWorks. A lot of conspiracy theory has been given to Dassault holding back on interoperability between CATIA and SW as a pure political move to not have one brand encroach on the sales of the other. But that is not the entire story. I'm not saying that this partially might be true but honestly I don't know if this is true?  I can say that having worked in-depth with both, that problems arise (and I even see it now having just got a CATIA model from a current client) that the way geometry is created in CATIA is different from the way is created in SW. For instance a sphere in CATIA is quite different than a SW sphere in that the CATIA sphere has 8 faces where as the SW sphere has two with the seam between the two faces being completely hidden from the user in SW. A sweep in CATIA has, what I call two arbitrary seams visible to the user where the SW sweep as one or none - either invisible to the user.  I am not sure about the nuances of these, and my former colleagues will probably be quick to correct me on the nuances, but they would definitely agree with the main point; - CGM CATIA definitely employs a different solution for making there bodies manifold than does Parasolid.

                                       

                                      With all that said, I know it doesn't help your immediate problem. So, I'm wondering if you've looked at some of the more advanced tools of Import Diagnostics?  Most of the time I first perform an automatic ID on the import but some times I have to "get involved" by using some of the more advanced tools like Gap Closer.  If you're not aware of this tool it can be accessed by RMB on one or more of the faulty gaps that are displayed in the PM dialog list.  A thorough read of the Import Diagnostics help item might save you time the next time you come upon a imported model that can't be fixed.

                                       

                                      Now I'm not saying the Gap Closer is the be-all to end-all, but I have healed bad imports using it. It is a manual intervention to the ID tool that does help.  I also will admit that I do plenty of delete, replace, faces as will as Boundaries and fills to replace bad patches.

                                       

                                      Mark