sketched entity

I am using SW 2004. In drawing mode, I sketched a few entities. I
later tried to delete them. I was able to delete all the entities
except one (a vertical line). I tried unsuccessfully to put this
entity on a layer and blank it. I did notice that the entity was
related to a view (when I moved the view, the entity moved with it).
Out of desperation, I gave the entity a dimension to an edge in the
view, by giving it a very large dimension, this entity was no longer
in my drawing boundary. But of course if you do a "fit all" it will
show up on the screen. Outside of deleting the drawing and starting
again, what could I have done?
TIA
Paul
Reply to
dbq
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Paul, You have to activate the view that the line is "attached" to to delete it.
Richard
Reply to
Richard Doyle
To finish Richard's statement, do a RMB on the view and choose Lock View. This will then let you select objects that are tied to that view, but far enough away that the view loses the focus. Don't forget to Unlock it when done with that task.
WT
Reply to
Wayne Tiffany
Paul,
While working in drawing mode (when the System Option "Dynamic drawing view activation" is ON), SolidWorks responds to the placements of your mouse cursor by automatically activating one of the drawing views. The view closest to the cursor is likely to be the one with which the sketched entities will be associated. This association will automatically shift to another view when the cursor reaches it, although the sketch entity will "belong" to the view which was activated with the beginning point of a line, for example.
The user can manually "lock" one "view focus" or, alternately, the "sheet focus" to assure that entities sketched (or annotations added) are purposely associated with one or the other. The options can be found via use of the right mouse button pull-down menus (with the cursor over the view or sheet background).
You will likely need to unlock a view (or lock the sheet) in order to delete the sketch entity you said can't be accessed. If one view is locked and the sketch entity is associated with another view (or the sheet), you won't be able to select the line, for example, without shifting the lock status.
Per O. Hoel ________________________________________
Reply to
Per O. Hoel
Thanks Wayne, but I was finished (in my mind at least). And now after seeing Per's reply, I have to say:
Why do you guys make it so bloody hard????
I have always wondered who uses "Lock View Focus" and Lock Sheet Focus" and why. It's very simple to double-click a view to activate it, and to double-click the drawing border area to un-activate views. I have never set Dynamic View Activation to ON, nor do I intend to - I've seen notes fly around too many times on other peoples drawings.
Seriously though, could someone explain the virtues or reasons behind using lock view and lock sheet?
Richard
Reply to
Richard Doyle
Hmmm, interesting, obviously I answered from the "dynamic" side - always keep it on for ease of object placement. However, it appears this may be somewhat of a moot point as it appears that the Dynamic *option* is gone for 2005. Go look up "view boundaries" and read.
It appears that dynamic is always on and the color & style of the boundary indicates the status of the view. Double-clicking will lock/unlock the view, but I don't see any way to actually turn off the dynamic feature. The boundaries are not visible except when activated by passing by or locking.
Now, on the good side, it also appears that if you have a note, etc. attached to a view, and that note ends up over another view, if you don't have some view locked, you can still pick up the note. Used to be that you had to find its owner view, lock it, and then go pick up the note. Now it appears to recognize that it needs to shift the focus to the note's parent view. Cool.
WT
Reply to
Wayne Tiffany
I hadn't noticed the "auto dynamic" thing. I like the new behavior of attaching notes to the view automatically if you place it inside the borders. You can even add multiple notes to multiple views, and as long as you place them inside the borders they will attach to that view. And it still works the old way for notes outside the view border - double-click to activate and the notes stay with the view.
Man, this stuff just keeps getting better and better.
Richard Don't forget to sign up for SolidWorks World
Reply to
Richard Doyle

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