9 Replies Latest reply on Apr 17, 2014 11:59 AM by Matthew Lorono

    Dangling dimensions

    Mary Cimino

      I would like to know if there is quick way to fix the dangling dimensions after making model changes. I always delet them and insert new dims. I have be wasting alot of time doing this. Can you help me.

        • Re: Dangling dimensions
          Mark Kaiser

          Are you inserting the dimensions from the part file, or creating dimensions in the drawing file?  I'm assuming choice #2, and this is why they are dangling after you change the part file. 

           

          Sometimes you can grab the endpoints of the dimensions extension lines and reattach them, but most of the time you have to recreate them.  This is with the case of creating your own dimensions in the drawings.

          • Re: Dangling dimensions
            Mary Cimino

            Yes the second one. So if I create the dim in the part file it should change and stay attached. I will try this. Thanks.

              • Re: Dangling dimensions
                Mark Kaiser

                Maybe we should back up.  Are you talking about dangling dimensions in part files, that would be in sketches?  Or are you talking about dangling dimensions in drawing files?  We are all assuming drawing files so far.

                 

                If you are talking sketches in part files, it depends on what the dimensions are related to.  If you're changing faces, deleting sketch lines, that dimensions are related to, they are going to dangle, is what it is in SW.  I think the 'best practice' in part files, is to dimension to other sketch entities, even in different sketches, as opposed to dimensioning to faces, which change internal id's often.

                • Re: Dangling dimensions
                  Scott McFadden

                  Mary,

                  I always insert my dimensions from my model into the drawing.  This is how I build design intent into the model.

                  The only time I create dimensions in the model are the ones I cannot create in the model.  Either because the sketch is fully constrained without these dimensions or maybe because I need a reference dimension.

                   

                  Then if I end up with a dangling dimension it is because I changed my sketch with a dimension being deleted.

                • Re: Dangling dimensions
                  Bernie Daraz

                  This is not intended as a wisecrack but why not dimension your drawing after you've completed the modeling. I always get asked by my bosses why isn't the drawing dimensioned if there is a drawing at the time.

                    • Re: Dangling dimensions
                      Raul Bueno

                      You can have revisions where drawings can already be made then you have to go back and modify, or in many cases you have drafted out completly and the engineers/designers decided to do it differently due to a change else where so you must change everything again.

                    • Re: Dangling dimensions
                      Raul Bueno

                      Honestly to get the best results from your dimensions in a drawing is to do as Scott does. Model your parts and dimension them as you would want in your drawings. When you import these dimensions they will update as your sketch changes (if they are just moved around) if you delete a dimension you will have to re import the dimensions for the new ones to show up and delete the old ones. Also keep in mind what plane you have your part on. This will make a big difference on where the end of the dimension lines end up on the part i.e.- if you dimension a modeled part on the right plane and you show it on the front in your drawing it might show up with the dimensions coming from the center of the part (instead of from the edges). Play with it and i think you will like the time it will save when done correctly.

                       

                      EDIT- also if you have part with alot of diameters in it modeling and drafting it on the same plane can be very important also or they will not always show up on the imported dimensions. ALSO as a helper note, if you use imported dimensions and your are trying to drag and drop them to another view if the dimension is on the left side make sure the view you are trying to drag it to is on the same side of the part (you can move the view wherever after the dimensions are dropped into the view) or sometimes it will not work, and also make sure the starting point of the dimension is dropped in the same spot(ish) as the view you are pulling it from.

                      • Re: Dangling dimensions
                        Daniel Hamilton

                        I have dealt with the same issues when the "replace model" option is used in a drawing, I have had "some" success with deleting the dimension then un-deleting it, kinda hit and miss, but it does work.

                          • Re: Dangling dimensions
                            Matthew Lorono

                            Daniel, if you are encountering dangling dimensions with Replace Model command, this is because face and edge IDs have changed, or they are not tracking.  If face/edge IDs have changed, you may wish to file an enhancement request to do a better job of understanding how the face/edge IDs of the new model are the same as the model being replaced (please include example models of these in your submission).  However, if the IDs are the same, then you may wish to contact your VAR to have then check out if there might be a bug.  Thanks!