maintaining Chirality of sketches

I use inventor and am having all sorts of problems maintaining chirality of sketches using the skeletal modelling technique. http://discussion.autodesk.com/thread.jspa?threadID=531402


My question is, are there the same sort of problems using solidworks?and can you overconstrain a sketch?


many thanks

NOT SURE ABOUT YOUR "CHIRALITY" AND HOW IT APPLIES TO MODELING,....YES, YOU CAN OVERDEFINE A SKETCH.

This is from a thread on the inventor forum. It is a mojor pain that you connot overconstrain a sketch in inventor to completely, mathematically define the geometry


Re: does anybody know how to correctly constrain a drilled slot
The basic issue here is the mathematical concept of chirality, or
handedness. A centerpoint arc is a classic example of chirality, since there
are two possible solutions to an arc defined by a center and two end points.
I remember using 2D CAD packages that always drew arcs in the
counter-clockwise direction because they could only track the order in which
points were placed and they wanted to avoid chirality changes during update.

The Dimensional Constraint Manager (DCM) that Inventor uses tries to
maintain the chirality of sketch geometry. However, there are situations
where it will flip chirality. When I experimented with Josh's slot, the arcs
stayed on the outside, but the horizontal construction line updated to be
tangent to the virtual side of the arcs. This is the way DCM tried to
maintain chirality with conflicting inputs- the arcs maintained chirality
but the tangent constraints between the arcs and the construction line
flipped chirality.

For those of you who are interested in the inner workings of sketchers, here
is an excerpt from the DCM manual:
"Note that a model with N geometries may theoretically have up to 2^N
solutions with different chiralities. An application cannot tell in advance
which of the 2^N chiralities the DCM will need to know in order to solve the
model. Thus, the only practical way to specify which solution is required is
to use the initial geometry locations provided by the application. In some
circumstances it is possible for the DCM to "remember" the chirality of a
model from one evaluation to the next.

Only a single solution will be found by the DCM. Which solution is found
depends upon the initial configuration of the geometries, dimensions and
equations, any pending requests to change the chirality, and a number of
options which are passed to the DCM. Many of the options are provided to
affect which solution is found for underdefined geometry. The solved
position of well defined geometry is unaffected by these options."

Basically, the more information you add to a model, the more likely that it
will be stable. If you don't have a completely defined sketch from a
mathematical perspective (which is different than from a dimensional
perspective), then Inventor needs to guess what your intent was, and you
might not be happy with the results after making changes. Taking Josh's
sketch as an example, if you were to dimension the slot width, and then use
an expression to define the length (Center_To Center_Length =
Overall_Length - Width), the arcs should stay on the outside.

Loren Jahraus
Autodesk Inventor QA

stee, I'm having a little problem here figuring out just what you're after. Solidworks uses both Dimensional and Geometric constraints to define its sketches. You can over constrain a sketch or you can give it no constraints and I mean none what so ever not even horizontal or vertical.


I'm looking at my copy of ASME Y14.5 - 1994 Dimensioning and Tolerancing book and I see three ways to define a slot.


1. Center to center width, height and 2X Radius


2. Overall height x overall witdh and 2X Radius


3. Outside to outside width, hieght and 2X Raduis


All that I would need now is the position of the sketch to some edge, plane, feature, etc. to make it fully constrained.


Does this help?