18 Replies Latest reply on Oct 20, 2010 2:36 PM by Steve Calvert

    Dimension to intersection?

    Bonnie Caruthers

      I am using 2010 SP4.0

       

      I have been unable to find a way to dimension to an intersection.  For those of you who have used Pro/E (Scott?) will know the option I mean.  I see you can right click and get "midpoint" but no intersection. Do not see a filter for it either.

       

      thanks,

      bjc

        • Re: Dimension to intersection?
          Alin Vargatu

          CTRL+Select the 2 entities. With them selected click on the Point command in the sketch toolbar. You get the intersection (even the virtual sharp).

          • Re: Dimension to intersection?
            Scott McFadden

            Hi Bonnie,

            Yes I know exactly what you are talking about.  Also was prevalent in Autocad as well.

             

            The mid-point is in the Solidworks 2D editor as well, FYI.

             

            If you are trying to create an intersection with 2 intersecting sketched lines in the drawing

            the closest you can come to having an intersection snap is if you hit F3 the snap toolbar

            will come up and there is an interstion of a line to a sline snap.  Closest thing.

             

            snap.jpg

            • Re: Dimension to intersection?
              Michael Maestas

              Try this link, It should lead you in the right direction.  Alin is correct in the discription on how this is done.

               

              Hope we all helped you.

                • Re: Dimension to intersection?
                  Bonnie Caruthers

                  Hey everyone,

                   

                  Thanks so much for all your help!  Sorry I have been MIA.  I know how frustrating that is on a forum when you have made an effort to help someone new and they seem to simply evaporate!  I just got so tied up with work, learning SW, still using Pro/E, caring for a sick animal, etc...  I have tried to get back here but something always came up.  I have other questions but have not even had a chance to post them either.  I hope my disappearing will not keep any of you from helping me out in the future.

                   

                  As for the issue at hand...I never even had a chance to try it out as a project became critical then I was swept back to Pro/E.  So the next time I post a question I do promise to be more visible!

                   

                  Cheers,

                  Bonnie

                • Re: Dimension to intersection?
                  Steve Calvert

                  Bonnie, I know how you feel.  I used Pro/E for a little while after Unigraphics for a long while and I miss the intersection dimenesion tool.  I can tell you that I have become a better designer/modeler because of it though.  I really like using my sketch dimensions from the model in the drawing so if I need an interesction somewhere it usually shows up in the sketch somewhere.  But even in the sketch you have to create the interesection by adding a 'virtual sharp'.  Try looking at the "Help" pages for 'Virtual Sharp' to see the several different kinds of sharps at your fingertips.  I try to teach my Engineers and Designers here about "Design Intent".  If it's your intent to have an intersection dimension - show that in your skecth.

                   

                  Now, onto other more important things:  With Solidworks World coming up at the end of January and the hope that we will see somekind of Top Ten Enhancement lost, let's make this our number one suggestion.

                   

                            "Give the ablility to dimension to an intersection without creating a virtual sharp first."

                   

                  Any takers?

                   

                  Steve

                  • Re: Dimension to intersection?
                    John Ehrhardt

                    These "tricks" are extremely bad.  My six year old Inventor CAD had an intersection option.

                    After another 20 min of experimenting with the above knowledge revealed that invisible int points can be created.

                     

                    This workflow must be improved-

                    In drawing environment,

                    pick first line, pick second line, pick point tool icon to create an invisible point only recognized later when hovering over the invisible location.

                    start dimension, hunt for the unseen first point, watch for a point symbol to appear where no visible point exists, pick to attach a dmension, repeat for the other invisible point.

                     

                    Eschew Obfuscation

                    Time for an ER.

                      • Re: Dimension to intersection?
                        Steve Calvert

                        When you say invisible you really mean hidden, right?  Your workflow for creating the sketch point is correct but you know that you can show the sketch in the drawing view and then select that point for dimensioning.  If I need an intersection to show up in my drawing I make sure to add it in my sketch.  I try and show sketch dimensions in the drawing as uch as possible.  OR you can select two lines in a drawing view and then select the point tool to place that point in the view BUT it isn't hidden unless you don't show points.

                         

                        My 10+ year old Unigraphics has the same intersection tool, I love it and wish SW could find a way to incorporate it.

                         

                        Steve

                          • Re: Dimension to intersection?
                            John Ehrhardt

                            Thanks for your comment, Steve.  SolidWorks does things in its special way.  This forum is very helpful.

                             

                            I had no knowledge that the point was hidden and classified as a unique virtual sharp entity.  For me, it was invisible.  Enabling Show virtual sharps does reveal the created points.

                             

                            You mention showing the sketch in the drawing.  Which sketch is this (part feature sketch or drawing sketch element)?  The dimension I was creating was for a chamfer with no sketch, that had edge fillets applied.