SW2008- Scan Equal in sketches-trivia question

I seem to remember this working in sketches. It doesn't seem to do so
now. Does anybody remember when this went away?

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I want to say that I first noticed it gone with the introduction of
2006.
I asked my VAR about it at the time, and what happened is they
consolidated it with something else and moved it to an entirely
different menu, away from sketches, making it really, really hard to
find.
I poked around just now and see it was consolidated with
Tool>Dims>Fully define sketch. You jsut have to turn ff the other
stuff (like the dimesnions).

 

Thanks Ed.

I called my VAR on this and rather out of their character the AE did
not know this. Now that you mention it I do remember finding this out
some time ago, but habits are hard to break. I kept asking the VAR why
you would only want this in a drawing (which is where the help says it
still works.)

I was able to constrain all the sketch stuff while on the phone with
the VAR so I didn't lose too much time.

I had a bunch of crescent shaped features to create so I just CTRL
dragged them around till I had enough and then was going to let Scan
Equal constrain them for size. That technique can work quite fast if
one knows where scan equal resides.

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Glad to help.

For those monitoring this thread, the new Tools>Dims>Fully define
sketch is a step up from the old 'add relations' or 'scan equal' in
that it will find relations even on sketches with existing relations
(I know that at least one of the two couldn't be applied to a sketch
with even one existing relation - I don't remember which one, or if it
was both). Kudos and Huzzahs to the development team!

Just like Paul (it's always interesting to find that old time users
that have never worked together adopted similar modeling strategies!)
I would use it to constrain stuff that I Ctrl+Dragged to make copies.

The bummer used to be that it wouldn't work with sketches with ANY
sketch relations at all. After the change, the new function was so
hard to find that, just like Paul, I have developed the habit of
window selecting sketch entities and adding the relations manually

So, inspired by Paul’s question, I took a minute to test it out in
2007, and is my way, the first thing I tried didn't work. Let me
reiterate - "the first thing". This is something mystic I must have
inherited from my Dad. When I worked for him, I could make 50 parts,
49 perfect, with1 flawed in a minor way. When he picked one from the
pile it would be the one that wasn't perfect. And as a chip off the
old block, I piss off my guys regularly because I have somehow
inherited that same knack for picking out the one thing that is wrong
out of an overwhelming pile of perfect when I review their work.

In this case, "the first thing" I did was draw an oddly angled line,
Ctrl+Drag a bunch of copies, and try to Tool>Dims>Fully define
sketch. Though it found the equal relations, it did not find the
parallel (though tools>measure does confirm the parallelism)

Sure enough, as I further tested it, every other relation type
worked.

You should be warned that on collinears it works to the point of
adding too many relations (not overdefining, but if you want some
flexibility in editing later on you would have to weed out some of the
automatic relations after using Tool>Dims>Fully define sketch since
every collinear comes with four additional coincident relations, one
for each endpoint of the two lines to their respective opposite line)

The net is:
-it's a good time saver on imported and Ctrl+drag sketch geometry.
-It doesn't find parallel relationships (bug in 2007 and 2008 through
at least SP0)
-It adds too many relations on collinear (kind of a bug through at
least 2008 SP0)

But 'Tools>Dims>Fully define sketch' can be a huge time saver, so it's
worth looking into, now that we all know the obscure place to find it
Ed.

 

Somehow I associate the name "Fully Define Sketch" with people who
select everything in a sketch and then FIX it. To further disguise it
they use the identical icon as the sketch tool. Pretty uninformative.
I've seen that icon a million times and never thought to use it.

Now I tried a trick that should work and could work but didn't work.
Create a rectangle. CTRL drag it a few times. Delete all relations.
Then use FDS but turn off Horizontal and Vertical. In my small mind
this should result in perpendicular and parallel keeping the
rectangles square instead of Horizontal and Vertical. So far so good.
So why can't I now pivot my rectangles about a corner? There is no
relation that I can see that limits angular movement.

But wait, on further inspection SW double dimensioned between two of
the rectangles. Remove the double dimension and it will allow angular
movement. The reason seems to be that SW FDS dimensions to vertices
not edges in this mode. Lesson learned: it is possible to create a
horizontal or vertical relation using dimensions.


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One thing I have noticed about this feature is that the
autodimensioning always works from the vertices. This results in
double dimensioning frequently. It also results in sketches that can't
take rotation about a vertex. The solution is to delete one of the
dims and then reattach the dim to a line instead of the vertex. This
becomes noticeable when horizontal and vertical constraints are turned
off which happens when converting in-context sketches to regular
sketches.

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