15 Replies Latest reply on Oct 27, 2010 5:03 PM by Chris Dolejska

    Circular Pattern

    Martin Stone

      I'm trying to create a circular pattern of the chamfer I have just made (the one on the tooth at 12 o' clock). But I keep getting an error message saying "Some chamfered items are no longer in the model. Edit the feature to reselect the items." I'm not sure what that means so can anyone enlighten me please?

       

      No. of instances = 40

      Feature to Pattern = Chamfer2

        • Re: Circular Pattern
          Martin Stone

          I've just found the solution. I ticked the "Geometry pattern" box in the options menu & it worked fine.

          • Re: Circular Pattern
            Peter Gumprecht

            Personally, I'd do it as a revolved cut rather than a chamfer pattern.

            Hope this helps.

             

            revolved cut.png

              • Re: Circular Pattern
                Glenn Schroeder

                I thought of that too, but then wouldn't the bottom of the chamfer be rounded instead of straight?

                  • Re: Circular Pattern
                    Peter Gumprecht

                    Rounded?

                    It would be whatever you sketched the revolve profile to be.

                    revolved cut sketch.png

                      • Re: Circular Pattern
                        Glenn Schroeder

                        I didn't explain properly.  Since it's a revolve the bottom edge of the cut (the edge closest to the center of the gear) would be an arc instead of a straight edge.  Maybe that wouldn't matter.

                          • Re: Circular Pattern
                            Peter Gumprecht

                            Glenn,

                            After re-reading your post I now understand what you mean by round instead of flat. You are totally correct. The revolve would create a radial edge on each tooth while the chamfer would create a flat edge. I guess it depends on how the gear is manufactured so as to model it correctly.

                             

                            Regards,

                             

                            -Pete

                          • Re: Circular Pattern
                            Martin Stone

                            I just tried to do it that way & it was giving a "zero thickness" error.

                              • Re: Circular Pattern
                                Peter Gumprecht

                                Martin,

                                Just an observation but your initial sketch is not fully defined. A bad practice/habbit you should avoid.

                                I would say that as a general rule of thumb never leave any portionof a sketch undefined (blue), with the exception of centerline endpoints.

                                Can anyone back me up on this.

                                 

                                In terms of the revolve not working(zero thickness error), that is because the edgepoints of the gear are further away from the point of revolve

                                than the sketch plane centerpoint. As indicated in my marked up picture below. Does this make sense? I can try to elaborate further if needed.

                                If the outside of the gear was a diameter instead of the 1mm flats the sketch would work fine.

                                 

                                revolved cut mark-up.png

                                  • Re: Circular Pattern
                                    Martin Stone

                                    Yep, fully understand about the zero thickness thing & thanks for the tip on fully defining my sketches. Question though, why do sketches need to be fully defined?

                                      • Re: Circular Pattern
                                        Peter Gumprecht

                                        Fully defined sketches protect against accidental dragging or movement of sketch elements.

                                        Also, how can you design/draw something without knowing the dimensions?

                                        It just seems like common sense to me but I have been doing this a long time so it's my default way.

                                        Not a dig on how anyone else does things. I fully realize that there are 100's of ways to do the same things.

                                         

                                        Regards

                                        -Pete

                                        • Re: Circular Pattern
                                          Scott Essner

                                          Martin,

                                           

                                          I'm going to guess that you're new to SolidWorks and that you have experience with AutoCAD or a similar 2D tool.

                                           

                                          One of the key differences between these packages is the relationship between sketch entities and dimensions.

                                           

                                          In AutoCAD, you draw sketch entities and define their key dimensions as you draw them.  When you dimension these entities, the sizes of the entities drive the dimension value.

                                           

                                          In SolidWorks, the opposite is true.  The dimensions (and other sketch relations) actually drive the sizes of the entities.  Without fully defining your sketch with dimensions and relations, the entities can be dragged or changed, which is obviously not desirable.

                                           

                                          The advantage of dimensions driving features is the control it gives the user.  The user can define the key dimensions for a part, and change those dimensions such that other features change size accordingly to achieve design intent.

                                           

                                          Regards,

                                          Scott

                                            • Re: Circular Pattern
                                              Martin Stone

                                              Scott, you are correct, I am new to Solidworks but have over 20 years experience with AutoCAD. I am unemployed at the moment and I've noticed more jobs advertising for Solidworks experience,  I'm trying to teach myself so I go into my garage & find an engine part that I can reverse engineer. I have used Inventor (self taught) in the past but find Solidworks much easier to use, especially in the sketch department.

                                               

                                              I understand about the dims. driving the entities but what I meant was that, more often than not, I complete a sketch and it's not fully defined. I could go to each entity that is still blue and "Make Fixed" but why would I need to do that?

                                                • Re: Circular Pattern
                                                  Scott Essner

                                                  Martin,

                                                   

                                                  Kudos for taking the initiative to build new skills. 

                                                   

                                                  You're right, using the make fixed tool is not the way to fully define a sketch.  Typically you would use a combination of sketch relations and dimensions to define feature sizes as well as feature locations. 

                                                   

                                                  If you have a specific example of a sketch that's not fully defining for you, post either a picture of it or a zip file containing the model and we'll try to help you get to the bottom of it.

                                                   

                                                  Scott

                                                  • Re: Circular Pattern
                                                    Chris Dolejska

                                                    ""I understand about the dims. driving the entities but what I meant was  that, more often than not, I complete a sketch and it's not fully  defined.""

                                                     

                                                     

                                                    Then that means it can move on you. Go ahead and click and drag it and watch it distort. When it's fully defined it's locked in place. It also means that there is some dimension that you are not calling out. IOW you have designed something without a dimension therefore you don't know if it's thick enough or long enough etc.

                                                     

                                                     

                                                    ""I could go to each entity that is still blue and "Make Fixed"  but why would I need to do that?""

                                                     

                                                    "make fixed" works in some instances, when you are not sure what dim to add to make it fully defined.