16 Replies Latest reply on Aug 26, 2013 6:38 PM by Jeremy Feist

    Sketch is unsolvable, but why?

    Mason Morton

      I've attached the part. The problem comes when I place a dimension between the two shapes (the DIM with a value of .305"). I can't think of any reason why adding this dimension would cause the sketch to become unsolvable. I created this same sketch in Solid Edge and it did it no problem. Also, you should be able to add an equal relation to the two lowest, right-hand lines of the two different patterns, but this makes it go unsolvable too. Once again, I was able to do this in Solid Edge (see image) no problem.

       

      Any ideas, am I missing something? I've used Solid Edge for a lot longer than SW, but I feel this isn't something I'm doing wrong, just SW's solver.

       

      Solid_Edge_Sketch.JPG

        • Re: Sketch is unsolvable, but why?
          Kelvin Lamport

          First of all, it is often better/easier/quicker to pattern a feature (or body) rather than pattern in a sketch.

           

          I don't have time to figure out exactly why that sketch doesn't work ... other than it has too many constraints.

           

          An alternate method if you have to create multiple copies within a sketch, is to fully constrain the seed (yours isn't) and then simply copy the seed (complete with dimensions) along a vector.

           

          Sketch Pattern.png

            • Re: Sketch is unsolvable, but why?
              Mason Morton

              Thanks for your reply, Kelvin. But the reason for creating two instances within the sketch is to determine the correct lengths of the sides of the shapes (there will be only two different lengths that are used on all of the line segments). This is necessary to make sure the pattern correctly nests once the pattern contains many instances. For this reason, the two instances need to be linked dimensionally so the length of the shorter segment (for example) can be determined parametrically by the solver when the longer segment is set to a specific length.

               

              The second reason is to determine pattern spacing since the pattern is staggered and the x and y spacing will be different from one another.

               

              Sorry, that's a mouthful.

            • Re: Sketch is unsolvable, but why?
              Bernie Daraz

              I noticed that you have the same dimension on two different lines with an equal constraint, I believe that is the cause of your error.

              • Re: Sketch is unsolvable, but why?
                John Burrill

                It could be that SolidEdge is more tolerant of redundant mates than SolidWorks.

                However, you can still produce this part pretty easily and with fewer sketch relations

                I uploaded a part that creates the sketch using sketch patterns.

                I had to add one dimension in order to make the part fully-defined.

                • Re: Sketch is unsolvable, but why?
                  Mason Morton

                  Thanks for your replies, I'll take a look next week. Starting the weekend a little early!

                  • Re: Sketch is unsolvable, but why?
                    Bernie Daraz

                    I was curious so I tried, it can also be done with one sketch and Fill Patterned.

                     

                    fill.png

                      • Re: Sketch is unsolvable, but why?
                        Mason Morton

                        You're correct (as Kelvin also pointed out), but the point of having two of the shapes in a single sketch is to determine the perfect spacing. What you're doing is guesswork: the edge lines don't point at intersections like I'd like ( as they are in the 2nd pic). This creates the nesting that is necessary to have an interesting geometric pattern.

                         

                        I still don't have a good answer for this, but I started the sketch from scratch and got a result I was happy with. I appreciate all of you for taking time out of your day to help answer this.

                         

                        Pattern_1.jpgPattern_2.jpg

                          • Re: Sketch is unsolvable, but why?
                            Bernie Daraz

                            I agree that there is a benefit to the 2nd sketch, as shown by my earlier response to the extra and error causing dimension. It may as well have been construction lines though. Once the spacing is determined I thought it could be easily replicated with the Pattern Fill command, that was the reason for my additional post. One of the good things about SW and the forums in general is the availability of help AND alternatives. I frequently look at other posts in a few categories and learn from the questions as much as the answers.

                            • Re: Sketch is unsolvable, but why?
                              John Sutherland

                              Now I see what you are aiming for.

                               

                              The method is to create one component, constrained so that it cannot be morphed, and fix or otherwise fully define it so that it will not translate or rotate.

                               

                              Then copy that component, and the copy will be able to translate and rotate until you relate it to the first component by verticies coincident with lines.  Then the sketch will be fully defined.

                          • Re: Sketch is unsolvable, but why?
                            Mason Morton

                            If anyone is still interested, Solver3.sldprt has the final working sketch.

                             

                            The sketch is overdefined with a few too many parallel relationships. I was able to get the sketch to work with the redundant relationships in place through trial and error of some different methods, but I think that's what was giving me problems. Parallel 44, 49, 61, and 65 can all be deleted and the sketch will remain fully defined. With them in place, the sketch is a little unstable: delete the .300" dimension, and the sketch becomes unsolvable. If you delete the mentioned paralled relationships, this behavior disappears. It wasn't apparent that these relationships were redundant and overdefining to me until I was again remaking the sketch. I would think SW should've been calling these relationships overdefined the entire time, but for some reason was allowing them under some circumstances.