In a part or an assy, open a sketch on one of the system planes, put a line in it, put a note in, then close the sketch and suppress it. The note is still accessible and appears to be outside the sketch. I tried it with 2006 & 2007 with the same results.
How long has it been this way? Always? So then, how do you put notes on the lines, as in to label them like, Bottom of truss, Floor, Air duct, etc. such that they disappear when you don't have the sketch open or visible?
Hopefully this is something obvious that I have overlooked and I will feel like a complete fool. :-)
I can duplicate that in 2006, Wayne, but the note will hide if you disable "Display Annotations" What's more, you can delete the note with the sketch closed or suppressed without any effect on the remainder of the sketch.
It seems the sketch note really exists outside the sketch, at the part level.
Yup, always (as far as I know). I agree that it would make sense to be able to have an annotation that only shows in the sketch that the annotation applies to but stays hidden when that sketch is closed. Kind of like the sketch dims (see below)
The workaround that I have used for years is to put dimensions on the lines, make them driven dims, then over-wrtie the in the text box in the PM for that driven dimension with my description - Floor, trebuchet_arm_travel, treb sling, etc.
Odd timing for your question - I jsut mentioned this in a presentation at the midwest user group yesterday. I asked if anyone else in the room did the same, and I saw a few hands raise so it must not be totally whacked. And i will tell you, it works great (but not as great as if SWx just put in a sketch annotation feature).
Note: a warning box will show up when you start typing over the because in general you don't want to eliminate the dim value, and rightly so. So I just got in the habit of typing Y as my second letter (the Yes that the warning is looking for). So 'floor' becomes 'fYloor'. I don't even look up from my fingers anymore (as my speelling errors confirms, touch typing continues to evade me - though I am making inroads on it).
Ed 'OK, I'm outed - I actually use lines in my designs :)' Eaton
BTW, expanding on the topic - sometimes I have to add dims to the part just to keep a line or endpoint confidently outside of the part for a cut, split line, or whatever. The position of the line doesn't matter so much as long as it is always to the outside. In those cases, to make it clear to the next person that it is not a functional dimension, I will blow away the value and overwrite it with the word ARBITRARY, then mark it NOT for drawing. This is sort of a 'golden rule' thing - when getting parts from others I try to analyze their intent so I don't mess with the stuff that matters, and its nice when its obvious what is not important. Doing this makes it clear to the next guy that the value doesn't matter - it might even be better if I overwrote it with 'KEEP OUTSIDE OF PART' but thats a lot of typing - I have to think about that now. The Neat thing is if you double click the ARBITRARY dim you can still change the value when required. I have heard no complaints or questions from those recieveing my parts after years of doing it.
I have modified dimensions in the past just as you describe, but this particular time I wanted a note with a leader on it and found the missing functionality.
I like your suggestion of the ARBITRARY since it does make it clear that the value is not necessarily important. Thanks - learned one today.
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