16 Replies Latest reply on May 11, 2009 3:54 PM by Jon Balduf

    Cut assembly part with a surface part?

    Tim Le
      Problem: I'm modeling a centrifugal fan housing that goes on a helicopter. The outlet of the housing pokes through the aircraft skin. I have to match the fan outlet exactly to this skin. The customer has provided an assembly where the fan mates to and the matching aircraft skin (which is a surface part).

      My plan was to model the fan housing so that it extends beyond the aircraft skin, mate it to the assembly so that it is positioned correctly and then cut it with the aircraft skin surface. Is this possible?

      I know it is possible to do a surface cut within a part, but is it possible to do an "in-context" surface cut using an existing surface part within the assembly?

      If this is not possible, the alternative is to somehow insert the skin surface part into the fan housing part and do a normal surface cut. But the challenge here is how do you locate the two in the exact same same position as they were in the assembly?
        • Cut assembly part with a surface part?
          Deepak Gupta
          Did you tried to use the Cavity option in the Assembly.

          or

          Edit you part in the assembly, and create the in-context surface and do the surface cut.
          • Cut assembly part with a surface part?
            Tim Le
            Thanks Deepak, creating an in-context surface by copying it (offset surface, zero distance) and then doing the surface cut seems to work.
            • Cut assembly part with a surface part?
              Charles Culp
              Jon,

              To cut a hole in a surface model, use the "trim" tool (in the surfacing menu). "Extruded cut" only works on solid bodies.
                • Cut assembly part with a surface part?
                  Jon Balduf

                  Charles,
                  Thanks for replying. I tried the trim command but was unsuccessful with it. It would cut everything on the outer side but couldn't get it to flip the cut?

                  Jon
                    • Cut assembly part with a surface part?
                      Jerry Steiger
                      Jon,

                      It's not clear from the image what you are trying to do. The user interface for Trim is different from Cut. For a simple trim, you pick the surface that you want to use as a tool and the surface or surfaces that you want to trim. Then you select either the parts of the surface you want to keep or the parts that you want to remove. For a mutual trim, you pick the surfaces that you want to mutually trim one another and then pick the parts that you want to keep or remove.
                        • Cut assembly part with a surface part?
                          Jon Balduf

                          Thanks for the replies. I'm sorry for the confusion. What I'm trying to do is cut holes in a surface imported part. I believe this is not a solid part but imported surfaces if I understand it correctly. We have imported a part from a vender that we need to put holes in. Right now the work around is to sketch the holes on the drawing for the shop to put them in. I also realize I could probably download a solid but too far into the project to turn around. I hope this clears things up.

                          Thanks,

                          Jon
                            • Cut assembly part with a surface part?
                              Anna Wood
                              John,

                              Can you Knit the surfaces together and form a solid as you are doing the knit feature? Look up Knit in SolidWorks Help

                              Please post your part, I suspect there is a very easy solution for you that we can give you for future use for this type of part.

                              Zip the file into an archive and post the zip file.

                              Cheers,
                          • Cut assembly part with a surface part?
                            Deepak Gupta

                            Jon Balduf wrote:

                             

                            Charles,

                            Thanks for replying. I tried the trim command but was unsuccessful with it. It would cut everything on the outer side but couldn't get it to flip the cut?



                            Jon

                            Draw you sketch of the hole and use Trim (Insert > Surface > Trim). Use the sketch as the trim tool and choose whether you to keep the selection or remove the section. This will give you a choice keeping or removing the outside or inside area.
                              • Cut assembly part with a surface part?
                                Jon Balduf
                                Hi - Take a look at this part. I have tried to trim a hole in this but it tells me the trimmed pieces selected can't be sewn together? I also tried knitting the part together but tells me that cannot knit a surface to itself? If you notice in the tree it's a surface-import so there is just one surface to select. I hope this helps.

                                Thanks everybody,
                                Jon
                                  • Cut assembly part with a surface part?
                                    Jerry Steiger
                                    Jon,

                                    I was able to trim a hole in the part, so your problem may have to do with the type of hole you are trying to make. Even if you can trim holes, you will need to build side walls, unless you are just trying to get something good enough for a drawing.

                                    The imported geometry is bad and it looks like you tried to fix it by adding a couple of missing surfaces, but it is going to take quite a bit more work to make it right. Select the imported surface part in the feature manager and then Tools/Check and then pick Selected items and Check. You will see one Open surface and six Face-face inconsistent errors. If you look at the errors you will begin to see what you will need to fix to make it a solid. Most of the problems around the two latch features probably won't be very hard to fix. Getting the dome features to work could be pretty tricky. It will probably be easier to break it into two bodies, as it gets tricky where the two parts just touch one another.

                                    You could also try reimporting from the original file without knitting all of the surfaces together, then knit them yourself. This might actually be easier. Another option is to select faces from the existing body and knit them together. This looks fairly promising. The basic bodies can be made by knitting together just the inside surfaces and then thickening them to the outside. (You will have to do the smaller part with two knit surfaces, deleting the hole in one and extending it to the other and then knitting them together before the thicken.) That gets you the major bits and you can probably generate the dimples and part of the latches in a similar fashion.