Sketch rotate

I have run into a dilemma and may have to use ACAD (oh no!) to get out of
it.

I have a part that was sketched in the context of a car body on a carrier
and is quite weird as it has to miss several things. So I edit the part in
the assy, put in a bunch of lines & arcs, and then get out of it. Now I
open the part on its own and open the sketch. What I want to do first is
rotate everything to square it up to the system so it has at least some
straight lines & dimensions.

So, how do I rotate all the sketch entities, that are all totally undefined,
so that a particular line goes vertical, or whatever? I could ask for an
angle measurement and then type in a value, but that's only close. I tried
several varieties of autodimension, but it never would let me pull it around
properly. I tried to find a way to snap the end of a line to a reference
line, but couldn't come up with one.

In ACAD it's so simple, but I really don't want to resort to that......
Thoughts?

WT

 

dimension & constrain as needed to define the "geometric shape" of the
sketch so that it will not "distort" when moving or rotating. you should be
able to do this and not have the sketch fully defined/constrained.

next, select a linear line (that's not fully constrained) which is close to
vertical or horizontal, and add said constraint. this in effect should
"snap" the sketch into the desired position/orientation.

an example of this would be a sketch that has it's geometric shape fully
defined, but is not associated with the origin. in this scenario, you would
be able to drag the sketch by one of its end points and the entire sketch
would follow and hold its shape.

hopefully this makes some sense.

cheers,
kb

 

It's easy:

First make sure that there are no relations or dimensions relative to
external geometry.
Pick Tools:Relationsisplay/Delete Relations in the drop down box pick
External, delete any that appear in the list.

Next either add relations and/or dimensions to "hold the sketch together" to
itself.
You can add relations manually or if there are no relations in a sketch you
can use the Constrain All function.
It's under Tools:Relations:Constrain All.
You can add dimensions manually or you can use the Auto Dimension function.
It's under Toolsimensions:Auto Dimension.
This could be use as a way to temporally hold the sketch together while
moving it.

Then you could use the Modify Sketch function. (as long as there are NO
external relations.)
It's under Tools:Sketch Tools:Modify... while in the modify sketch mode you
can move, rotate, mirror, and scale sketch objects.

Hope that helps

 

Wayne,
This just worked for me in a simple test, not sure if this will work in your
case, but...

Window select everything, and Fix, then rotate the sketch using Move or Copy
Entities as required, and then you can again window select to Un-Fix
everything then add constraints and dimensions.

HTH,
Muggs

 

Wayne in 2004 you can rotate everything and drag and drop when it is
completely un constrained.
Tools>Sketch Tools>Rotate or Copy it is a new tool and it will do exactly
what you are asking and is extremely easy to use, check it out

Corey

 

Ok, this response will cover all the suggestions prior to this.

Basically - no go. Now, before you jump all over me for being so stupid,
please understand that I CAN get there, I'm just not willing to manually
define everything to hold it together in order to do it. There are lots &
lots of weird dimensions that would have to be created in order to lock in
the shape, and I don't want to go through the time & trouble to do it at its
seemingly arbitrary rotational position, then blow them away after the
rotation, and do them right.

The move/rotate/copy function is great for moving as you can grab everything
as is and move it as a blob, and 2005 works much better than before. Yes,
you can also rotate that way, but you can't snap the rotation to anything -
it moves in predefined increments. Since the existing angle is not some
even number, I can't EXACTLY align it as desired. Close - sure, but I want
it right.

The Constrain all function added only 7 relations - not nearly enough to
hold its shape. Remember, this is a shape not unlike the Blob, and will
require much thought as to the proper dimensioning method for proper
production.

The Fix all function did just that - fixed everything to where I couldn't
even rotate it.

AutoDimension locks in the dimensions as horizontal & vertical regardless of
the method chosen. I thought maybe I could use a pair of perpendicular ref
lines, autodim to those, then make sure they were not horizontal & vertical
and rotate. Nope - overdefined.

Next?

WT

 

Next?

ok, if i had a need to do what you're attempting, acad (precision rotating)
is what i would use.


cheers,
kb

 

Couldn't you dimension the angle of the surface you want bring it out to 8
places write the number down and use it for your rotation. I think this
should be as accurate as AutoCRUD. Should make everything right.

Corey

 

iirc, i think rotating by reference angle in acad is "dead on"

 

The problem with that is that you now have some number that is used to
establish a rotation value. If your intention is to make a face horizontal,
then it's close. But then when you go back later and try to mate to that
face, you find that in fact, it isn't exactly horizontal and the mate
doesn't work. Simplified explanation, but I think you get the picture.

WT

 

I used a similar method to create that dodecohedron or whatever it is called
I used an 8 place angle to create mirror planes and everything was close
enough to knit not sure what the tol is on knitting though, but I was quite
surpried the method worked. If you don't trust it then I have to say
"GO....run to AutoCad see if we care!!!" =^)

Corey

 

So, is this sparring match considered a draw?? Wah, wah, wah.

WT

 

Wayne

Another way to do it which works well for imported sketches, frankly a
kludge but quite effective, and doesn't require dimensions or relations.
Use "Fix" (hiss, boo....) on the parent sketch
Use the parent to make a Derived sketch.
The derived sketch will be totally robust and totally repositionable
(translate + rotate), using simple relations.
I personally prefer to avoid the rather flaky, cryptic Modify Sketch
toolset.
And as for "Align", I've had that jerk the part origin off the intersection
of the construction planes, for keeps!

 

Interesting concept - hadn't thought of that one, but I can see how it would
work. What's even more interesting is that I was very limited on what I
could do with it. I could manually rotate it, move it around, move it to a
position, but I couldn't add any lines to it, or add a restraint like make a
line horizontal, which was the original goal. But, I did discover that I
could take that same line and make it collinear to a system plane. Got it!

WT

 

Sorry, I should have thought to mention that any relations to rotate or
translate derived sketches have to be external, but you worked it out.
Sometimes it pays to add a datum line to the parent sketch with one end at,
say, the desired origin for the derived sketch, and the line trailing off at
a useful angle, which will end up along one or other construction plane.

If you do need to add geometry to the repositioned sketch, converting the
derived sketch to a new sketch on the same plane does the trick. OK, you end
up with three sketches, but it does have advantages in certain situations.