Sketch & notes

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.

WT

 

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.


AW

 

Wayne,

I am working on 2003, and it behaves like that also. We are upgrading
to 2006 by the end of the year. woohoo!

Reaper.

 

Hmmm, guess I've just never noticed it before - thanks.

WT

 

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 <DIM> 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 <DIM>
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
<DIM> 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.

 

So, you do use lines!?! I stand corrected....

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.

WT