Sketch rotation

I've seen some posts to this effect in the archives but I don't think any
addressed this particular case.

I'm building a part with four configurations. The configurations consist of
rotation of the part (to simplify mating) as well as
suppressing/unsupressing features.

The part looks like the hub and spokes of a wheel, no rim. It all starts
with a revolved profile to form the disk.

I then created a sketch to cut out material and make the spokes. We'll call
this the base configuration.

I then copied that sketch, broke the relations and rotated the entities by
90 degrees to make the new extrude-cut tool for the "90 deg rotated"
configuration.

As suitable design table supresses/unsupresses the appropriate features.


Here's the question:

Is there a way to make a sketch that is a rotated version of a "parent"
sketch? And, can this rotation be parameterized via a design table?


This would improve both robustness and maintainability of the part and any
assembly it is in. In the case of my part, any modifications would only
have to be made to one sketch and not two.

Thanks,

-Martin

 

mating dosen't require a part to be modeled/oriented in any particular
fashion. that's the beauty of mating. it can rotate, flip or whatever to
get part in correct location/position.

check out derived sketch.

 

OK UM...

Make a new sketch.
Convert entities.
Tools>Sketch Tools>Circular step and repeat.
Select the converted entities.
specify the angle and the centerpoint of rotation
Change the converted entities to construction lines
now the new entities should be under defined.
add an angle reference and you should be able to control the angle reference
in the design table

Is this what you wanted?

Corey

 

OK UM...

i did the same ... although i can't quite tell for sure, it appears i may
have read something in between lines that wans't there.

 

Hi again martin,

STOP! Bad logic!!!

I cannot think of a good reason to make the model so complex when
mating is easier! The logic should be to:
1
make the part as the part must be in reality. no fudging....
2
if you have some features that change on the base part, make
configurations and hide / suppress as needed
3
make the required mates in the assembly. then make assembly
configurations that have different mates (suppress the ones that do not
apply in each configuration). Works great!

One of the things that I remember being frustrated with was the concept
of configurations and how they relate to assemblies. Always remeber
that if you have a part it a subassembly in an main assembly, that you
will need configurations in the part (A, B), then in the subassembly
(partA,B) and in the main assembly (subAssem A, B).

Hope that helps.

 

Well, I've been wondering about this too.

My reasoning is that it is less work. The assembly in question will have
some sixty of these parts. I am designing the part with smart mates. And
so, when placing the part, you choose the configuration (primarily a
rotation change) and click away. The part aligns itself and the rotation
comes in for free.

The alternative would be to make a part without configurations. Then you'd
have to place some sixty of these on the assembly...and then go through each
of them, one-by-one and rotate it to various angles. The good news is that
it is a z-axis rotation only, not a muliple axis rotation.

I suppose that another idea may be to place one part for each rotation
angle, mate and rotate as required, and then copy-drag each part to where
specific rotation instances are required. The trouble with this approach
(haven't tried it) is that you still have to go in and re-mate the parts you
are pasting. Lots of work.

And so I reasoned, that, if I could create a part with multiple rotated
configurations, and, that, if these rotated configurations are all driven by
a single sketch ... then, it's not as much of a kludge because it's still
like having a single part. There's only one defining element and every
rotated configuration changes if you edit the parent sketch. The circular
step-and-repeat approach suggested by Corey seems to be the way to go
(thanks Corey). I have to test it further to be sure that it won't break
with manipulation/changes.

Still bad logic?

-Martin

 

Offhand I would say, use a derived sketch. It will remained tied to the
original sketches dimensions and relations.

On the other hand why not drive the original sketch from a design table
or configuration specific dimension?

 

There is a component array feature. Check it out. If the 60 parts are
inline you can array them in a single step. You can remove instances if
there is a gap somewhere. If there are 2 levels of spokes put in each level
and array them together.

Corey

 

curious logic... but logical!

Actually, I do follow, and I understand how you got where you got. As
Corey says, component arrays are wonderful things.

Again, I do not recommend it, but... if you want to do the sketch
routine, here is what I suggest:

Since the part apparently has a center and spokes, create the first, or
layout sketch with (for example), a vertical construction line from the
origin, and one at whatever angle (but not constrained) from the origin
(not constrained to verical or horizontal, just the rotation end
point). Give these two lines an angle dimension. Construct other
aspects of you basic part, but be sure that the sketch is constrained
to these original 2 lines and center point such that a dimension
defining the angle rotates the rest of the sketch. You can easily test
this by changing the angle dimension. extrude your base feature. Then
in each configuration, you only have to change the one angle dimension.
That way there is no duplication of sketches or features.

Cheers,
Daniel

 

Hey, curious-logical I'll take. There's enough curious to battle with SW,
it seems, that if you have something that works you should go with it.

The prior suggestion to go with step-and-repeat worked like a charm. Now
three configurations of a part are entirely controlled from the first
sketch --as if it were a single config part. Thanks again.

-Martin