When clicking on one line then the other to identify the dimension within, if the mouse is dragged outside of the boundaries, the dimension is doubled. How do I stop this from happening?
In the example, the .05 is the issue and the in-between dimension is the actual (driven) result.
Solidworks thinks all construction lines are centerlines. One of the most frustrating parts of the software, IMO.
Josh Brady wrote:
This is by design and is quite helpful when you're designing revolves so that you can easily dimension diameters.
I'm pretty sure you can't turn it off. Just don't drag your dimensions across centerlines/construction lines during creation. You can drag them to the other side of a regular line without doubling. Once the dimension is created, you can drag it around and it won't change.
Take note of the cursor as you are placing the dimension.
It's a mouse with a padlock in the mouse body.
Also, the RMB on the cursor is blue. This means that when you right click during creation, the dimension's "form" becomes locked and you can then freely drag for placement (in your case) without worries of making the dim double.
Kevin
If you don't want that to happen, you can of course just not drag your cursor past the one construction line as the others mentioned, but another option is to select the end points of the lines instead of the lines themselves.
Glenn Schroeder wrote:
If you don't want that to happen, you can of course just not drag your cursor past the one construction line as the others mentioned, but another option is to select the end points of the lines instead of the lines themselves.
But then you'll still have to choose dimension orientation (unless the selected points are aligned to the dim):
Kevin
If you select Horizontal (or Vertical) dimension instead of Smart dimension, then the centerline doubling doesn't occur.
You lose some of the intelligence of a Smart dimension, but Horizontal (and Vertical) dimension are stupid dimensions.
If you select Horizontal on a vertical situation, then a vertical dimension is created (& vice versa) instead of SW just complaining.
Also, either the Horizontal or Vertical dimension can be used on an inclined situation. Below is a Vertical dimension:
Kevin
This is by design and is quite helpful when you're designing revolves so that you can easily dimension diameters.
I'm pretty sure you can't turn it off. Just don't drag your dimensions across centerlines/construction lines during creation. You can drag them to the other side of a regular line without doubling. Once the dimension is created, you can drag it around and it won't change.