16 Replies Latest reply on Jul 22, 2008 5:34 PM by Kevin Raley

    Surface triming and solid body problems

    Kevin Raley
      Hello all,

      New poster but not new to solidworks, however I am new to the surfacing features and have come looking for some advice or assistance with a particular part that is driving me crazy.

      I am recreating an existing object that I dont have access to the original files so think reverse engineered.

      If there is a better way to get to the end of having a solid body with the basic shape I am ok doing that just not sure how else to recreate a compound curved part like this though.

      2 main problems here that I am pulling my hair out over (and I dont have any to spare). Basically the shape is generally correct and here are my problems:

      1.) Surface triming with feature "Surface-Extrude2" (blue-green) I am trying to cut a curve into the outer surface on the bottom, and when I select the bodies to keep as being "Surface-trim1" (orange&gray) the upper section it won't remove the curved surface that performs the cut. I have tried various combinations of standard and mutual cuts as well as trying to select the parts to remove. None of these seems to be working correctly

      2.) So after struggling with problem #1 for some time I decided to attack it a different way in that my plan was to create a solid body of the entire part then do an extruded cut feature. In heading down that road I was unable to knit everything into a solid body. Even though I had already created a closed volume and wasnt able to create a solid body. I have removed those boundary surfaces in this pic for clarity. I have even tried thickening the "Surface-Trim1" to the inside by very small amounts and it wont let me do that either.

      So any ideas from you surface experts out there???

      Regards,
      Kevin
        • Surface triming and solid body problems
          Kelvin Lamport
          I'm definitely not a surface expert, and don't know if it will help, but try cutting with the surface before the mirror feature.

          Does the cutting surface create a knife edge or zero thickness feature?

          Are you being given any error messages?
            • Surface triming and solid body problems
              Kevin Raley

              Kelvin Lamport wrote:

               

              I'm definitely not a surface expert, and don't know if it will help, but try cutting with the surface before the mirror feature.



              Does the cutting surface create a knife edge or zero thickness feature?



              Are you being given any error messages?

              I get no errors when performing the cut but I get strange results. I will try cutting before mirroring that sounds like an easy test.

              I do get an error when trying to form the solid bodies that is something like "unable to knit surfaces"... so that is basically not much help in diagnosing what is wrong.

            • Surface triming and solid body problems
              Tom Nicholson
              I'm guessing your wanting the blue-green surface to not be there after using it to cut? whats wrong with just hiding it?
                • Surface triming and solid body problems
                  Kevin Raley

                  Tom Nicholson wrote:

                   

                  I'm guessing your wanting the blue-green surface to not be there after using it to cut? whats wrong with just hiding it?

                  Yes I can hide and have hidden it to continue working on it. I think but cannot confirm that I believe that in some way it is causing my problem to create a solid body part as the final desired part. Just beacuse its hidden doesnt SW still try to include it as a part of the solid body?


                  Now I have just tried performing the cut before the mirror and same results see the picture. I did try trimming it several ways too.

                  Thanks in advance for everyones help.


                    • Surface triming and solid body problems
                      Mark Kaiser
                      I'm probably missing something here, because this solution sounds too easy. If you want to get rid of a surface body, just delete it, you don't have to trim it away. RMB on the surface body and select delete.
                        • Surface triming and solid body problems
                          Matt McKendrick
                          I may not fully understand the problem, so this may not be the answer you are looking for.

                          Attack this issue as 2 surface trims. First, make sure the orange/gray surface feature is knitted together and is a signle surface body. Then trim this surface using the blue/green surface. Then create another trim using the orange/gray surface to cut away the outer "flange" of the blue green surface. Assuming that there are no other gaps in any of the faces, knit both of these remaining surfaces together using the "try to form solid" option.

                          I hope this helps, but again, I am probably not understanding the full issue here. If this is the case, I apologize.
                    • Surface triming and solid body problems
                      Charles Culp
                      Kevin,

                      My first approach would be trim surface, as you tried. Another direction would be to use the Insert>Curve>Split Line, with the "intersection" method. Then you can do "delete face" as Mark suggests.

                      This looks fairly straight forward... could you .zip and upload your model?
                      • Surface triming and solid body problems
                        Jerry Steiger
                        Kevin,

                        As others already pointed out, if the blue-green surface is just used for cutting, you can just delete it after you make the cut. It shouldn't be causing you any trouble when you try to form a solid unless you pick it as part of your selection process, but it could get shipped out along with your solid model if you export your part, so it is often a good idea to delete those tool surfaces. If you decide later that you really need the surface for something, you can just delete the deletion and you've got your surface back.

                        Did you check your closed surfaces after SW failed to make a solid out of it? Are you quite sure it was closed? The Thicken command will not give you the option "Create solid from enclosed volume" if the part isn't closed. SW can also fail to make a solid if your geometry is corrupt, yet another reason to check the part.

                        Check the curvature on your surfaces. You may have some very small radii that are stopping them from thickening. This won't necessarily stop it from making a solid from an enclosed volume though.
                          • Surface triming and solid body problems
                            Kevin Raley
                            Hello all,

                            Thanks for all the suggestions, I have tried to delete it after making the cut but then the feature "curved bottom edge gets elimnated and the orange/surface returns returns to its orginal shape.

                            I will give the other ideas a you have presented here a try and then zip up the part and upload it.

                            Regards
                              • Surface triming and solid body problems
                                Kevin Raley
                                Ok.....

                                Trying the other ideas here but thought I would upload the zip file.


                                Thanks
                                • Surface triming and solid body problems
                                  Mark Kaiser

                                  Kevin Raley wrote:

                                   

                                  Thanks for all the suggestions, I have tried to delete it after making the cut but then the feature "curved bottom edge gets elimnated and the orange/surface returns returns to its orginal shape.

                                  It sounds like you are deleting a feature in the feature manager tree, not a surface body. If you delete a feature, it will delete its 'child' related features further down in the FMT. If you delete a surface or solid body, it will not delete any features in the FMT, as long as you perform this operation after all of the features (at the bottom of the FMT). You can delete bodies (surface or solid) without affecting other features.

                                  I did look at your model, but couldn't tell what it is supposed to end up like. Is the 'curved bottom edge' a feature? I didn't see it.
                                    • Surface triming and solid body problems
                                      Charles Culp
                                      Kevin,

                                      I cannot interpret your model. In order for surface trims to work, the surfaces must extend past each other. You will have to make your surfaces larger so they extend past each other, and then you can trim them. You must have a fully enclosed volume, with all the edges coincident for the knit tool to create a solid body.
                                        • Surface triming and solid body problems
                                          Kevin Raley
                                          Hello all,

                                          Ok posting the updated model here, I had simplified the first one I posted. This one is complete with all the surfaces intact.

                                          I guess an old dog can learn a new trick.... Mark you were correct I was deleting it in the FMT, I have never used the delete body tool before. Thanks I was able to delete the offending surface.

                                          Now I am down to creating the solid body from this part, this is still giving me fits. I have knitted all the surfaces together that I can but cant get the last one to knit, it gives an error as "unable to knit surface". I have in the past gotten the flat section to form a solid body, so perhaps forming it first then rest of them.

                                          It may help you to view a sectioned view of the model using plane 1.

                                          I am going to work on the order of the knitted surfaces and see if that makes any difference too.

                                          Thanks for everyones input....

                                          Regards,
                                          Kevin



                                            • Surface triming and solid body problems
                                              Charles Culp
                                              All I did was delete the two faces that were not part of the exterior geometry, then knit again. They are the last two items in the feature tree.
                                              • Surface triming and solid body problems
                                                Mark Kaiser
                                                Kevin,

                                                I got your part to a solid, although I hacked on it a little. See if it's what you need.

                                                I deleted your yellow surface as it went into the interior of the part and was not needed in the interior. I did a surface loft to replace it where it went around the exterior of the part. I then tried to knit and form a solid, it formed one surface body but no solid. I did a tools>check, and it gave me an open surface, with the edges bounded in blue. I did a surface fill with the open edges, then another knit and form solid. This time it worked.

                                                If you rollback to before 'surface fill1', you can find the open surface. After I formed the solid, I colored the faces of it red around where the open surface used to be.

                                                Charle's method is cleaner than mine.
                                                  • Surface triming and solid body problems
                                                    Kevin Raley
                                                    Hello guys,

                                                    Wow..... I love this place thanks for all the help.

                                                    I think we were all heading down the same path as I was logging in to post my soloution to the problem, I got both of your messages.

                                                    Mark I think we did the same thing. I have not opened your file yet so I cant be exactly sure.

                                                    I have attached my solution.

                                                    Thanks everyone.... sometimes just a fresh idea can make all the difference.

                                                    on me guys!!

                                                    Regards,
                                                    Kevin