8 Replies Latest reply on Apr 29, 2010 5:02 PM by Alan Stoldt

    Centerlines and centerline Labels in a Config rich environment

    Alan Stoldt

      CENTERLINES AND CL TEXT.JPG

      Above is a picture taken from 2 different sheets, showing different configuarions of an Assembly. The cylinder diameter and length change from one to the next. I have perhaps 20 configs that I am making drawings for.

       

      When I copy a master sheet or template and change to a specific config, the Centerline doesn't keep any corresponding relationship to the geometery. Is there a way (short of drawing the CL in the Assembly as a sketch) to acocmoplish this so that the Cl will extend past the physical end of the assembly by such and such on each end?

       

      Additionally, I've added a CL note on the verticle line, the note "Anchor" button doesn't attach it to anything specific, it is part of the drawing view, but requires adjustment for each drawing. Is there a way to attach a note to an "insertion point" R, C or L type to a coincident mate with the line? Anything along those lines?

       

      Thank you in advance for your time and suggestions.

        • Re: Centerlines and centerline Labels in a Config rich environment
          Mark Kaiser

          I can get the centerlines to update in a part with mulitple configs, if I use the center line command from the annotations menu, and don't modify the length of it any manually.  For the note, short of attaching it with a leader, I don't have any suggestions.

          • Re: Centerlines and centerline Labels in a Config rich environment
            Alan Stoldt

            All right, revisiting this as I have yet to find a simple, on the fly, solution.

             

            I have a cylindrical base part with several (or hundreds) of configs, each part needs to be detailed. To maintain consistancy, I create a master template to begin with, then change configs as required. Some tweaking of notes is expected.

             

            In some instances as the cylinder gets longer, a section arrow may not increase causing the section to fail.

            Pipe Example.JPG

            I drew a generic pipe as an example. In differing configuartions the overall length may change. The O.D. will change. The Pocket geometry on each end will change.

             

            In the top example, at Part Level I sketched a CL extending 1/4" from each end. I bring the view into a drawing and create a section using the endpoints of that line, then I hide that line. My section arrow keep relationships during configuartion changes. Mission accomplished. Sort of.

             

            Is there no way at the drawing level to achieve this "simple" request without resorting to an added feature at the part (or assembly) level?

             

            I cannot relate the section Arrow line to an existing Midpoint or to the origin. I can eyeball it in, but this may foreshorten some critical dimensions at some point in time.

             

            The bottom view is a Broken Out section, but as the OD of the cylinder changes the depth changes as well.

             

            I could create additonal configuartions (or derived configuartions) at part level and have a feature cuttng the section, but again, this seems like an unnecessary added step.

             

            I very well may be over looking something basic, but I tried several "intuitive" solutions that didn't work.

             

            Any help is appreciated.

             

            Thank you.

              • Re: Centerlines and centerline Labels in a Config rich environment
                Wayne Tiffany

                Correct me where I have missed something.

                 

                Having the top view section line tied to a sketch line in the part seems to me to be a good solution.  That way the part config handles the length of the line and the drawing section line stays with it.  Seems simple and practical.

                 

                The line in the third view I think is what you are saying you eyeball into position.  How about making it coincident to the plane that you certainly have in the middle of the part.  That way it would always be through the center.

                 

                WT

                  • Re: Centerlines and centerline Labels in a Config rich environment
                    Alan Stoldt

                    Having the top view section line tied to a sketch line in the part seems to me to be a good solution.  That way the part config handles the length of the line and the drawing section line stays with it.  Seems simple and practical.

                    Wayne,

                     

                    Yes, this functions as I want. My question is more how to accomplish thisat the drawing level, where it seems it should be possible as well.

                    The line in the third view I think is what you are saying you eyeball into position.  How about making it coincident to the plane that you certainly have in the middle of the part.  That way it would always be through the center.

                    No, the third view is a section line at the Part Level. It is on axis of the cylinder without fail.

                     

                    I realize I have two different things going on here, but they are similar problems so I added on to this post.

                     

                    At the Drawing Level can you make a Section Arrow coincident to a Plane or Line or anything?

                     

                    I have tried pre-selecting sketches until I am blue in the face (perhaps red...) and I cannot make an existing line the line used for a complete section.

                     

                    I can make a section with the line from Mid to Mid, but the section arrows should pass outside of the part, no?

                     

                    pipe 002.JPG

                  • Re: Centerlines and centerline Labels in a Config rich environment
                    Jeremy Feist

                    if you go with the broken out section, you can set the depth to be to the center of a circle. when defining the depth, select a circular egde in an end view that will always be there and always be centered. (OD perhaps?)

                     

                    for the regular section, RMB on the section line and edit sketch. you should be able to add dimensione from the endpoints to the ends of your tube. you may need to hide these dims, but it should work.

                     

                    Jeremy