Changing what a smart dimension is attached to

 

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.

I think I have a solution for you. Right click on the dimension you want to re-attach to a new entity. Click on 'display/delete relations' in the RMB menu. This will pop up the relations manager in the feature tree. In the entities box, click on the entity you wish to replace (it will be listed line line2, arc3...) then select the new entity in the graphics window. The new entity will then show up in a box with the word 'replace' to the left of it. Hit the replace button. This should re-associate your dimension to the new entity.

This is also how to repair dangling dimensions in sketches.

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"