5 Replies Latest reply on Apr 20, 2009 5:54 AM by Lorenzo Gaudino

    Connect a dimension value in a text note.

    Lorenzo Gaudino
      I need to put the value of a dimension into a text note, inside a drawing. The only way that seems to work is "Dim@Sketch1@@Config@Filename.SLDPRT". Aside the useless length of this form ("Dim@Sketch1" SHOULD work), the worst is if I make more configurations I need to correct every single note for every configuration, that is exactly what I want to avoid...

      I tried to do a Configuration specific Property called "MyDim", and for that "Dim@Sketch1" works. Too bad that the property assumes the value of the last config I loaded, for all the configurations.
      i.e. I made two configs: the first with Dim=1, then one with Dim=2.
      Then I save, put a view for each configuration and put the note $PRPVIEW:"MyDim" into each view.
      As a result, both notes show a "2".

      Someone can help?
        • Connect a dimension value in a text note.
          Sandip Darveshi
          Hi Lorenzo,

          Please do make use of this for the attached note

          $PRPMODEL:"MyDim"

          and for note without arrow

          $PRPSHEET:"MyDim"

          to each view you want to attach annoation (note).

          It will give you the required result.

          Thanks and Regards,
          • Connect a dimension value in a text note.
            John Lhuillier
            When typing out the annotation note on the drawing you can pick on the actual dimension in the drawing view that it shows up in. This will put that dimension in your note.
            • Connect a dimension value in a text note.
              Lorenzo Gaudino
              Thanks for reply. The only way that works is to define MyDim="Dim@Sketch1@@Config@Part1.SLDPRT" for the first configuration. When you add new configs MyDim assumes the new config value.
              In the note I put $PRPVIEW:"MyDim", as I could put more than one part in the same drawing, so $PRPSHEET is not correct and $PRPMODEL need to be attached to the model. I know I could do as John suggest, but I don't want to put a quote just to link a note. Well, I put the note just to NOT add a view with the quote. I'm doing some sheetmetal cutting dxf, so I want to write down the tickness beside the profile.

              This is another workaround, but if I would add a new Dimension AFTER I've made the configurations, then I should add MANUALLY all the definitions... It's ridiculous. As SW knows the value of all the variables, you should be able to recall them from anywhere. Why I can't simply write in the note something like $Dim@Sketch1, or $PRP:"Dim@Sketch1" and see the correct value appear? This should also happen in the config name and tables. I wonder if they will do it anytime in the future.
                • Connect a dimension value in a text note.
                  Eddie Cyganik

                  Lorenzo,

                  If the dimension is a constant in all of the parts, then a custom property will work and it does not need to be attached to a view, just associated to it.

                  In my attached image, I have 3 configrations all related via a common dimension referred to using a configuration specific file property called "Length".

                  Each of the views has a note that independently updates with the correct value.
                    • Connect a dimension value in a text note.
                      Lorenzo Gaudino
                      @Eddie
                      Thanks for reply. I think $PRPSHEET is to be used just for drawings with one part, i.e. if you put the Mass in the sheet format, that is not associated with a view, it will update related to the view specificated in the sheet properties. It seems that, if the view specificated is left to "Default", it behaves like $PRPVIEW if you associate the note to a view. But if you select another view then all the notes will change according to that.
                      In the image you can see the differences, with the first view selected in the sheet properties.

                      I always believe this should not be necessary. You should be able to write "Dim@Sketch1" and automatically see the dimension for that view, that configuration. And for the model in the sheet properties if not associated to a view. This should be automatic.