8 Replies Latest reply on Aug 1, 2018 6:59 PM by Solid Air

    Revolve Design Library Feature with Only Two References

    Tanner Johnson

      Im trying to create a library feature that only needs a point and a plane/surface for reference. The issue is I am trying to do this with a revolve feature similar to how the hole wizard works; however, I can either not get the plane to generate off of the just those two references or I have more references that need to be added when applying the feature to a part. Is there a way to create a revolve feature for the design library that will only need a surface/plane and a point?

       

      Update 7/25/2018: Figured out a way to do a revolve while still keeping only two references. The key is in how you place your initial sketch and those after. If you do not reference (as long as you do not need orientation i.e. a circle) then you can just use a line in the sketch at an undesignated angle/length and then use a first cut extrude to convert your initial point. You can then create a plane using those references and when you use those of the revolve, as long as you do not add any references in the revolve besides dimensions and these previously defined references, you can do a revolve with only a plane/face and a point.

       

      Update 7/26/2018: Figured out you don't even need an extrude cut. Just use the first surface/face/plane that you start with and offset another plane. Make your first sketch with a point and then convert that point from that sketch onto the other plane. You can then either place a random, non-referenced line or a dot without references to create your plane that can revolve. The dot doesn't have to be in either of the sketches, just make sure it isn't in a line with the other two or that it doesn't add an external reference. It may help to have an axis made from the first two dots so that you can remove any horizontal/vertical relations and have them as perpendicular or parallel.

       

      Update 7/26/2018 (continued): Sorry about so many rapid fire updates, learning a lot of different stuff from using this application. If you do the second method with only sketches and planes, you can't directly import those sketches and the features. It will mess up the Library feature. You will need to collect the group in a file (as in highlight what you want in the file, right click, and choose add to new folder) and then click the folder and whatever features (probably a revolve or something similar) and add as a library feature. You will then need to open that library feature and under the file, add each sketch, plane, and axis (or whatever you have in the file) to the library feature using the "add to library" option. This will add the drawings without causing your library feature to become something else.

       

      If you find a better way, please let me know.

        • Re: Revolve Design Library Feature with Only Two References
          Sumit Rana

          Hi Tanner,

          Thanks for the update, good to know that you found out the solution by yourself and shared with us. Mark this question as "self assumed answer" it's just below the title of your question.

           

          Sumit

          • Re: Revolve Design Library Feature with Only Two References
            Solid Air

            My question is why just not use Hole Wizard?

              • Re: Revolve Design Library Feature with Only Two References
                Tanner Johnson

                Hey Solid Air, Thanks for the question.

                 

                The reason I can't use a the hole wizard is the cavities I'm working with are extremely complex, with not just non-standard hole callouts, but curved "chamfers" for lack of a better term and dimensions for tolerancing on depth and diameters that can't be done inside of a Hole Wizard. Although it would have made my life ten times easier. you can do some of this in hole wizard, but not with as much complexity. At least as far as I know.

                  • Re: Revolve Design Library Feature with Only Two References
                    Solid Air

                    Post a picture of what you are trying to create and I will tell you if I think this can be done with hole wizard (although you will still need to create a library feature).

                      • Re: Revolve Design Library Feature with Only Two References
                        Tanner Johnson

                        Here are two of the simpler examples. they aren't exactly what I'm working with, because I'm not allowed to show those, but these have the same idea as the others.

                        example1.JPG

                        Example2.JPG

                        Sorry about it making the reply so long. Looking forward to what you think.

                          • Re: Revolve Design Library Feature with Only Two References
                            Solid Air

                            Easily done using Hole Wizard (although you will not be able to edit them in HW and under most circumstances hole callout will not work).  The example below was done using legacy hole although I could have done them with hole from a standard.  I have also included the model for your review.  Since I did not know which version of SW you are using, I created them in SW2012 (cannot be too many of us that use that version anymore) so you should not have any problems opening it.

                              • Re: Revolve Design Library Feature with Only Two References
                                Tanner Johnson

                                Oh, I had no idea you could do this with hole Wizard. I figured you wouldn't be able to change the drawing after you made the hole. Thanks for this. I was able to modify the drawing to get some of the shapes to work, but some of them aren't diameters or angles and this causes an error when I have a radius. I get something that says "need diametric dimension" when I add this in a new drawing that isn't yours. I noticed that with hole wizard there are some things I would need to learn before I could begin using it properly. By not a diameter or angle, I mean it isn't a chamfer, but a curved line with a radius that starts at one diameter and ends at the next. Just imagine the chamfer in hole2 being curved rather than straight.

                                 

                                I tried adding the features you sent (without my modifications) as a library feature. It does the same thing as a revolve cut was doing before I did the fancy footwork. It adds edges for references on orientation that I don't want. I also tried going in and modifying your drawing for hole wizard's relations so that it didn't have any of the typical relations that cause this from drawings, but it still comes through. I'm going to need to play around a little bit to see if I can get this to work with library features, but otherwise, this is awesome.

                                  • Re: Revolve Design Library Feature with Only Two References
                                    Solid Air

                                    With a true hole wizard hole, you need to avoid deleting existing geometry or dimensions and you have to be careful on the what you do to the line on the surface the hole starts on.  Experiment is my best advice.  I do not use it too much because I have confused other users but I like it because you can put a hole without creating a lot of supporting geometry (I like to use the least amount of features I can and still show design intent and the ability to easily alter).