11 Replies Latest reply on Jul 10, 2014 8:51 AM by John Harder

    How to Break a Part's Link to Assembly Origin (Top Down Design)

    John Harder

      Hi, I am working on my first "Top Down" design.  I started with a sketch in my assembly of 3 mating parts.  Starting here in the assembly instead of with individual parts has worked beatifully for working on the intricate connections between the parts in one place as my design evolves.  However, my middle part will have 3 different configurations, each a different width. The only way I have found to accomplish this is by changing my layout sketch in 3 different configurations (at the assembly level - cannot do it at the part level).  This worked great until I started to make drawings of my parts and realized that since all of the parts' orgins are linked to the assembly origin, when I change configuration to a wider middle part and it pushes the third part over It changes the origin of the third part (since its now further from the assembly origin).  This then moves the drawing view in my drawing file.

       

      Am I going about this correctly?  Is there an easier way to have these parts share sketches at the connections?  If not, is there a way to break the link of the part's origin to the assembly origin and still have it linked to the original layout sketch?

       

      Thanks in advance for everyone's help!

       

      John

        • Re: How to Break a Part's Link to Assembly Origin (Top Down Design)
          John Harder

          Maybe another way to ask the question is, what is the best way to set up my relationships to this layout sketch?  I've read else where that using the correct relationships is the key.  The assembly is fairly simple.  Just 4 parts total that all connect.  I'd like to be able to adjust these connections in geometry and tolerances later in the design.  I previously converted entities in my part sketches, but it seems that may not be the way to go because it locks the part to the exact location?  Remember my middle part has three different widths.  The only way I currently know to drive that is by changing this layout sketch which moves the hinge and far right part (thus changing the origin of the parts and messing up the drawing views).  Thanks!

           

           

          layout sketch.JPG

            • Re: How to Break a Part's Link to Assembly Origin (Top Down Design)
              Jerry Steiger

              John,

               

              I think the best way to do this type of design is to use your sketch in the assembly to drive the location of the origin of the parts. Then the changing length of the middle part doesn't move the origin of your outer parts. This is likely to involve using master sketches in the assembly and then converting entities from them into sketches in the parts. You might want to set up planes in your assembly that you can use to orient the parts as well.

               

              Jerry S.

                • Re: How to Break a Part's Link to Assembly Origin (Top Down Design)
                  John Harder

                  Thanks Jerry.  That's actually what I have done.  The problem is when I widen the center part, it moves the two parts to the right, thus changing their origin.  I have actually just found a work around that seems to work really well, but I'm new to Top Down design, so we'll see if I'm missing something.  I created all center parts off of the sketch only referencing the left side ball/socket in the original boss/extrude.  I think used a derived sketch to copy the right side connection to the rubber living hinge.  This keeps both connections linked up to the original sketch, and doesnt' require the original sketch to be widened for the subsequent variations in middle part width.

                   

                  Thanks for your help!

              • Re: How to Break a Part's Link to Assembly Origin (Top Down Design)
                John Harder

                Or a third way to ask/solve my problem: is there a way to lock a drawing view so that if the origin of the part changes, the view doesn't get dragged around on(or off) the sheet?  This may be the easiest fix, but I can't find a way to do this.

                • Re: How to Break a Part's Link to Assembly Origin (Top Down Design)
                  Jamil Snead

                  I found a method that I think would work but might not be worth the trouble. When you are finished sketching the part in the context of the assembly open the part by itself and edit the sketch again. Suppress any dimensions that go to other parts in the assembly and delete relations that locate the sketch to other parts in the assembly (coincident, concentric etc.). You don't need to delete dimensions or relations that are only between entities in this sketch. You also don't need to delete non-locating relations like equal length or radius. After you have suppressed the dimensions and deleted relations you can move the entire sketch over to the origin and put some relation to tie it there (midpoint, coincident, concentric). Now go back to the assembly and your part will be in the wrong place. Delete the in-place mate (but don't let it delete all of your relations) and then manually add mates to locate the part back in place. Now you can edit the part sketch from within the assembly and unsuppress dimensions and add back any relations to other parts.

                   

                  I hope that is clear and I am pretty sure it works. I tried it with a very simple assembly.

                  • Re: How to Break a Part's Link to Assembly Origin (Top Down Design)
                    Jamil Snead

                    Another method is to just start the part by itself as a new part (not from within the assembly) and sketch it as best you can. Then bring that part into the assembly and mate stuff up. Once it is located you can edit the original sketch from within the assembly and add in-context relations as needed.