7 Replies Latest reply on Nov 26, 2016 9:59 AM by John Willett

    How to Verify "Merged" Sketch Relations

    John Willett

      Ignorant questions:  I have occasionally seen the explicit option to "Merge" two or more points when adding relations (though I can't seem to replicate this now).  This apparently happens automatically with points (or ends of lines) that are automatically "merged," e.g., when drawing a broken line or a rectangle, and perhaps in other situations where relations are added.  Such "merged" points apparently are not so indicated in "Display/Delete Relations," perhaps because there are no longer separate points.  I like to be able to see all the relations in a sketch, so my questions are:

       

      1) How can one unambiguously see whether points (or ends of lines) have been merged, or whether more relations (e.g., coincidences) are needed?

       

      2) Is it better, from the point of view of future editing, to create explicit relations (e.g., coincident) between separate points (or ends of lines) or to allow them to be automatically "merged?"

       

      I told you they are ignorant questions, but I would surely like to get some clarity. -- John Willett

        • Re: How to Verify "Merged" Sketch Relations
          John Stoltzfus

          You can use        to evaluate your relations

           

           

           

          I would let the points be automatically related as much as possible..

          • Re: How to Verify "Merged" Sketch Relations
            Bjorn Hulman

            Hi John,

            further to John Stoltzfus suggestion. If you have not already done so, you can turn on 'display entity points in part/assembly sketches'. This will put little ends on your lines. a blue end means it's unrestrained in at least one axis. A black point means it is fully defined. If you have two lines coming together and there is what appears to be one black point, they are likely merged and defined. If there are 2 bluepoints, thay are not.

              • Re: How to Verify "Merged" Sketch Relations
                John Willett

                John & Bjorn -- Thanks to both of you for taking the trouble to reply.

                 

                >>If you have two lines coming together and there is what appears to be one black point, they are likely merged and defined. If there are 2 bluepoints, thay are not.<<

                 

                Bjorn -- I think what you are saying above is:  If the lines are under-defined and dragging one moves the other without separating the ends, these end points must be merged.  If the lines are fully defined and only one point is showing between them without any relation symbol, then they must be merged.  In any case the "merge" relation is never shown symbolically nor in "Display/Delete Relations."  Is that about right?

                 

                >>I would let the points be automatically related as much as possible.<<

                 

                John -- I'll take your recommendation to heart even though it bothers me not to see the relations explicitly.  In any case, sometimes adding a relation between two points offers to merge them (as between endpoints in simple sketches), whereas other times it offers coincidence (as between an isolated point and a line end point).  I'm not sure what controls which choice you get, but I don't want to beat the issue to death... -- John Willett

              • Re: How to Verify "Merged" Sketch Relations
                Solid Air

                John Willett,

                 

                While you will not be able to see the merged relation between endpoints (that was what I was taught to call them) of lines or, lines and arcs, you will also not be able to add a coincident relation between endpoints; SolidWorks will not give you that option.  Do not confuse sketch points with endpoints; they are not the same.

                 

                In response to your last post, my first paragraph answers that, since a merged relation is not displayed, it will not be present in the Display/Delete Relations property manager (whether the endpoints are automatically merged during sketching or you merge the endpoints manually).  This is something you must just accept.

                 

                As for determining if endpoints are merged, turning on entity points (guess that's what SolidWorks calls them) is a good suggestion but these points will not turn black unless the sketch is fully defined (a fully defined sketch does not indicate merged endpoints).  Probably the best way is to select the endpoint and drag it in four directions.  If the endpoints of the lines and/or arcs are merged, they will move together.

                 

                I hope this helps.

                  • Re: How to Verify "Merged" Sketch Relations
                    John Willett

                    >>Do not confuse sketch points with endpoints; they are not the same.

                    ...since a merged relation is not displayed, it will not be present in the Display/Delete Relations property manager...  This is something you must just accept.<<

                     

                    Good point about sketch points.  I think that about sums it up.  Thanks! -- John Willett