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.
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.
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.
Carrie
This is also how to repair dangling dimensions in sketches.
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.
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"
Yeah totally agree with Carrie.
Why doestn't SW have the replace and re-route comands? Maybe it does but nobody has been able to point it out.
If you're used to building really robust models that reference and update constantly then this feaure is essential.
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.