18 Replies Latest reply on Oct 12, 2016 1:04 PM by Rob Edwards

    surface cut doesn't cut

    Chris Lamb

      Hello all,

       

      I'm trying to use surface cut to cut a thread. I have made a thread and offset from the surface which I want to cut into another part. Everything looks good... I think, but when I go to surface cut and select the cut and part it's fine - then when I try to cut it blinks, doesn't give me any message, sits back and smiles at me but doesn't cut.

       

      The surface is open which I thought perhaps was the issue so I closed the base end with surface fill but it still wouldn't cut. I'm pulling my hair out with this!

       

      image_1.png

      image_2.png

      image_3.png

        • Re: surface cut doesn't cut
          Tom dunn

          your thread surface is open here

          also the bottom has a small face

           

          this might work better if you close off your surface make it a solid then use the combine feature.

            • Re: surface cut doesn't cut
              Chris Lamb

              Ah... I feel stupid that I missed that!

               

              I did also notice that with the bottom surface. Could you suggest how I'd close the surface, because it's a helix thread it means that the bottom isn't a complete circle - because the helix runs off from the base. I'd like it if I could close the surface to make a complete surface... without extending the walls below the thread?

            • Re: surface cut doesn't cut
              Jason Edelman

              Yes, you need to enclose the bottom of the surface that intersect the solid body. A 'Surface Fill' feature should do it.

               

              May I ask why you just did not use the Cut-Sweep as your feature?

               

              Solids do everything surfaces do with less steps/features...

               

              Best, Jason

                • Re: surface cut doesn't cut
                  Chris Lamb

                  Yes, I have tried that previously, but to close the bottom surface I had to extend the walls below the thread (which begins in the middle of the sketch that is revolved). I am unsure if there's a way to close the bottom surface, which when I attempt to do so I have to click separate circular sections currently making up the bottom surface.

                   

                  I used cut-sweep for the other part (image 1) which is the male of the thread. I then extended the surface using surface offset by 0.3mm which is the area I want to remove from the revolved base at the bottom (images 2 & 3).

                   

                  I want the surface offset to be used to surface cut on the revolve, leaving the revolved base with a female thread which will be 0.3mm from the wall which has the helix thread.

                • Re: surface cut doesn't cut
                  Christian Chu

                  I'm confusing of what you tried to do

                  the part has a thread cut (solid)

                  then you offset the thread profile to create a new surface

                  Then you expect using the new surface to cut the solid?

                  Am I guessing correct here?

                    • Re: surface cut doesn't cut
                      Chris Lamb

                      Almost. That is exactly what I did, however, I don't want to cut the same solid with the new surface (offset 0.3mm), I want to cut the other feature and save that as another part - which will be threaded (female) to the male which the offset is of. The solid I am trying to cut with the surface that I have offset is the revolved base below it (revolve2).

                    • Re: surface cut doesn't cut
                      Tom dunn

                      I think I see what you are trying to do. Make an opposite mating part that would screw on to the first surfacecut1?

                      • Re: surface cut doesn't cut
                        Tom dunn

                        I created the inside threaded part by using your offset surface shown as red. If you do a cross section view, you can see the internal threaded part. I am not sure how you want the rest of the part to look.

                          • Re: surface cut doesn't cut
                            Chris Lamb

                            Thank you very much! You have understood exactly what I'm trying to do.

                             

                            I have the part open now and it is very close to what I want. I am struggling to edit it though because I can't see what you've done. There are multiple surface-knits and surface-planes which I'm confused by.

                             

                            It looks great when I put it in sectional view. The only thing being that I want it to mate with the bottom surface not have a 0.3mm surface-offset on all faces, but on the threaded (sides) only. So it would then mate up against the base perfectly. I think the thread looks as though it may be slightly more than 0.3mm so am unsure if you have offset from the surface-offset I created, where I'd like the surface-offset I created to be the outer surface which would be the outer of the new part when I surface-cut the base below.

                            • Re: surface cut doesn't cut
                              Chris Lamb

                              I have tried backward-engineering from the part you edited. Took my time and can follow (most of) what you did. I have attempted to copy it, but slightly different. Just to attempt to get the thread to the bottom rather than with the small gap as I explained before. I'm having an issue when it comes to surface-trim, I believe it goes back to your first reply where the surface isn't complete at the bottom.

                               

                              I have remade the surface offset and it includes the hole I had previous but I can't seem to get the other hole in the bottom, where you referred to a small face. I think if I can get this to merge then I can close the surface fill the base and it'll cut from the revolved part no problem! Any help on how to get the area you highlighted to close would be very appreciated!

                               

                              I tried 2 ways - with the enclosed surface-fill top and without, neither worked as it's the bottom which is causing issues!

                               

                              image_4.png

                               

                              image_5.png

                            • Re: surface cut doesn't cut
                              Mark Kaiser

                              You made a thread once from a sketch, right?  Maybe it would be easier to offset the thread profile sketch, and make you new thread from this?

                                • Re: surface cut doesn't cut
                                  Chris Lamb

                                  I tried this first, however, it needs to revolve which creates a "step" on the bottom outside of the thread and doesn't allow the bottom surface from the first part to mate (with a cylindrical extrusion, to which the thread is created on the inside) with the upper outside of the base.

                                • Re: surface cut doesn't cut
                                  Rob Edwards

                                  Instead of an offset surface Body Copy (with zero), Delete Face and cut thicken worked.  I had to alter your revolve sketch to just the threaded part, and lift it up a touch

                                  edit: maybe its possible to do both cuts at same time, it asked me which bodies I want keep

                                  • Re: surface cut doesn't cut
                                    Tateos Tvapanyan

                                    You can use "Indent" to achieve the same result.

                                     

                                    Capture1.JPG

                                     

                                    Capture2.JPG

                                      • Re: surface cut doesn't cut
                                        Chris Lamb

                                        This worked beautiful. Thank you so much! I am so very grateful to you.

                                         

                                        Now, the reason for this: I am making 3 parts which will have different diameter holes in the base (revolve2) which will thread onto 1 part (extrude1 - glass feature). The diameters will allow 1 part with 3 different outside diameter pipes to protrude.

                                         

                                        1.png

                                        2.png

                                        3.png

                                         

                                        Now, with surfacecut1 (made for trial 3d prints, so as not to waste plastic) off:

                                         

                                        4.png

                                        5.png

                                         

                                        Thank you so much to everyone for your help!

                                         

                                        Chris.

                                      • Re: surface cut doesn't cut
                                        Tom dunn

                                        Hi Chris, how are you doing with this?

                                          • Re: surface cut doesn't cut
                                            Chris Lamb

                                            Hey, I'm still trying to find how to close the small section and make a complete part on the bottom base to then use to cut the base part. I have tried the other methods suggested as all of you guys have written them but still pulling my hair out!

                                             

                                            My most recent reply, with the images where I can't surface trim are the best I've got so far. The face which wasn't included is now included but it's just the small face on the bottom I'm trying to enclose with the rest of the body.