10 Replies Latest reply on Jul 27, 2011 12:53 AM by Ben Druce

    Changing what a smart dimension is attached to

    Carrie Ives
      I am going to ask this question in two ways.

      First way (for former Pro/E users)- in Pro/E, in your sketch, if you find that you created a dimension between two items and it should have been between two others, you select the dimension, hit edit, replace, and recreate the dimension. The drawing will have the dimension in the new location (assuming it was shown previously). Can I do this in Solidworks? How?

      Second way (for those who haven't used Pro/E)- I have a sketch that is fully dimensioned. These dimensions may be shown on a drawing. (I do not know because I am editing a part.) In this case, the sketch is of a hole pattern. It is currently dimensioned from hole to hole, and the bottom left hole is dimensioned back to the part. I am assuming that if I delete a dimension and create another one (to dimension to the top right hole) that the drawing will no longer have the hole pattern dimensioned. Is that correct? Is there a way to get a smart dimension to be between two different things than what it was originally created to dimension? I know that sometimes when I fix failed sketches, I can get the dimensions to reattach to other geometry if the original geometry is gone.
        • Changing what a smart dimension is attached to
          Mahir Abrahim
          You can try clicking on the dimension and then dragging the endpoint of the extension line to the new desired sketch entity. This doesn't always work. If it does, the dimension will remain shown in the dwg (if you've shown it in the first place). However, unlike ProE, more people use reference dims in dwgs instead of model dimensions. Using reference dims you can make whatever changes to a sketch that you like, but the drawing dimensions will still be firmly attached to your model edges.
            • Changing what a smart dimension is attached to
              William Sanders

               

              You can try clicking on the dimension and then dragging the endpoint of the extension line to the new desired sketch entity. This doesn't always work

              It will work consistently if you attach it to the same entity type.

              Where it won't work, for instance, is if you try to re-attach a dimension to a line, when it was originally dimensioned to a point - or vice-versa.

            • Changing what a smart dimension is attached to
              Carrie Ives
              I just did the drag thing and changed a dimension in my sketch that was shown on my drawing. The dimension on the drawing turned green and I can't reattach it, so I guess I will have to delete it and show it again.

              Carrie
              • Changing what a smart dimension is attached to
                Carrie Ives
                For the dimension that I am currently working on, a cut was dimensioned from the top of the part and should have been dimensioned from the bottom.
                I changed the dimension in the sketch by dragging what it was attached to so that it showed up the way that I wanted. This turned the drawing dimension green. (The green dimension has the same name as the one in the sketch.) I tried the display/delete relations for the green dimension on the drawing, but it did not have anything. I then tried to undo my changes and managed to crash out of Solidworks. I tried to change the dimension in the sketch using the display/delete relations and replace, but that moved my sketch off the part, and I don't know how change the direction of a dimension in the sketch. (and now, it won't let me select anything in the sketch...someone forgot to tell my computer it was Friday not Monday)
                At this point, I'm just going to delete the green dimension and see if I can get it to show again.
                  • Changing what a smart dimension is attached to
                    Eddie Cyganik

                    Carrie,

                    The only way I can get this to work is to modify the "sketch" dimension by draging the dimension to a new location...

                    ...then open the drawing & delete the "Army Drab Green" dimension and finally, insert model items again and the dimension will appear as changed in the sketch, with the same ID. Actually to show that they remain one in the same dimension, do not delete the green dimension, leave it alone, then insert model items. You can then look at the properties of both to see they are the same.

                    Now why SW doesn't automatically delete the old and replace it with the new one, only heaven knows.

                    As far as changing direction of dimensions;
                    You can drag the end of an extension line to any location, this includes crossing over the other extension line. You can even move or relocated both. So, using this method should work for you to reverse directions.

                    One last thing, I'm a former Pro/E User and I recall a command that I often used in drawings when the manufacturing guys asked for a change, it was called: "Modify Dimension Scheme". When selected a drawing dimension and activated this command, the system would automatically open the part and place you in sketch mode where you could alter the dimensioning scheme of the feature related to the originally selected drawing dimension. Once complete, you would exit from sketch mode and once again, the system would automatically rebuild the part, close the part and place you back in the drawing and you'd be looking at the modified dimensioning scheme. Slick as Snot, ...well, that's not a very good analogy but that was/is one powerful command.

                    SolidWorks: Can you investigate the Pro/E Command: "Modify Dimension Scheme"
                  • Changing what a smart dimension is attached to
                    Carrie Ives
                    Pro/E doesn't have the "modify dimension scheme" as a separate command anymore, but you can go into your sketch, pick a dimension, hit "edit, replace" create your new dimension. If it was shown on your drawing before you replaced it, it will be updated to the new dimension. Also, the replace command will let you replace one line (or other entities) with another. Really useful if you have a lot of things referencing something you want to delete and replace with something else. (Sometimes it makes sense to change the sketch, other times it makes more sense to either "edit references" or "reroute" (same command just different names for it)at the feature level. This is one of the things I have not found anything truly equivelent to in SolidWorks. Hopefully, I have just been looking in the wrong places.) While SolidWorks will let me change my dimensioning scheme by dragging the end of my dimensions, I never really feel like I know what it is dimensioning to and just don't trust it as much.
                    • Re: Changing what a smart dimension is attached to
                      Rob Taylor

                      Reattaching linear smart dimensions at the drawing level in 2009 seems to function better than previous releases except for dangling dimensions.

                      Highlight dim, move dim if necessary to ensure extension lines are visible, select extension line end – (red if dangling), drag each end to a point, line or edge. If this fails, first drag to other geometry and then back to desired location.