Constraints in Assembly causing crashes

[mdare]

I've only been using Fusion a few days so I suck at it but I had made some parts and tried to put them together in an assembly and it would crash and when I restarted Fusion and tried to open that part it would crash again. I think the problem was some sides of my rectangular parts were not square and Fusion couldn't handle the conflict. I redrew my parts and made sure they were square and things are going better. But I happened upon an old post of similar problems in older versions of inventor where someone asked if Inventor was a "House of Cards". Walt Jaquith posted the answer below to the question. I think the real answer is on users part to make good parts and on autodesks part to fix the program to be able to handle the problem and give a better error statement saying what the problem is. Hpoe this saves someone a lot of the time I wasted trying to figure it out!

Inventor is not a house of cards, but it's surely possible to build an
assembly that is. On the other hand, it's also possible to build assemblies
that are nearly bulletproof. As you gain experience, you'll learn how.
Dealing efficiently with assembly constraints is one of the primary skills
that an Inventor user needs to learn. Here's my most valuable tip to get
you on your way:

Good assemblies start with good parts. Each Invrntor part is a heirarchy of
fearures, each built on the ones before them. Now look at the browser tree
of a part. You started with a blank part, and added a base feature, then
other features. As you go down the browser, the dependancies between the
features get more complex, and therefore the features themselves get
inherantly less stable. It's easier to get the features at the bottom of
the tree to go sick than it is to get the first few at the top to act up.
Assemblies are the same way. The more parts you add, the more complex your
dependencies get, and the more potential you have for instability. What's
the solution? To work whenever possible from the top of the browser.

Each part, no matter what it looks like, has one set of perfectly stable
features--it's origin geometry. If you constrain two parts together in an
assembly by thier origin geometry instead of their features, your
constraints will never get sick, no matter how you change the parts, and
you'll have created a truly bulletproof assembly. Obviously, for this to
work, the origin geometry has to be positioned in some logical place in
relation to the part itself. This is done when the part is first created,
and involves the first vital decisions that are made about how a part is
going to be laid out. Where the origin geometry is going to end up is an
important consideration.

The next best feature of the part is the first one. It depends only on the
origin geometry, and so is very hard to destabilize. Choosing the right
orientation and attitude for that first feature is another big decision. If
the base feature is done right, subsequent features can be built on it
directly rather than on each other in a series of dependancies. What you're
trying to avoid here is a constraint in an assembly that's based on a
feature in a part that's based, in a tenuous line of dependancies, through
six other features before it finally gets to the stable, foundational base
feature of the part. In a situation like that, almost any little change you
make to the part is going to adversly effect the assembly constraint. If,
on the other hand, the constraint is made to a surface of the base feature
or (better yet) to the part's origin geometry, few (if any) changes to the
features of the part will cause that constraint to go sick. Can the base feature be made in such a way that all other features are placed directly on
it rather than being built up on each other like a...card house? If not,
can the chain of dependancies be kept to only a few links? Assemblies and
parts work exactly the same way in this.

Here's an example: I'm building an assembly that's a shaft with gears,
pulleys, seals and bearings mounted on it. Obviously, I want an origin axis
running right down the middle of the shaft. So create my shaft so that the
part's X axis is the centerline of the shaft. Now I make my gears, etc. the
same way, and when I insert them into the assembly, I constrain their X axis
to the X axis of the shaft rather than picking features on the parts. The
result as far as putting the parts together is exactly the same, but the
configuration is much more stable. I can change the features on the shaft
all I want, but the parts that are mounted to it are going to stay lined up.
Notice also that in this senario, all the subsequent parts are constrained
directly to the first part in the assembly, not to each other. As I said,
when you can manage this, it's the best way to work. Any dependant part can
be modified or deleted altogether without effecting the rest of the
assembly. The moral of the story is to keep your matrix of dependencies as
shallow as possible. The result will be more stable parts and assemblies.

It's not often practical to get a assembly that simply can't implode under
any circumstances. You will get the occasional sick constraint. But you
can make an assembly thats really hard to hurt by planning your dependancies
carefully and logically. This is what makes Inventor fundamentally
different from AutoCad (for instance). It's really just a relational
database. This means that Inventor attempts to define the relationships
(I've called them 'dependencies') between parts, features and so on, in
addition to defining the parameters of the parts themselves. In its guts,
Inventor probably has as much in common with MS Access as it does with
AutoCAD; it just happens to represent things graphically. Once you get a
good handle on those relationships, your assemblies will quit giving you
fits.

Cheers,
Walt

[mdare]

Down loading the sp3 has helped. Trying to constrain everything to the origins was not fun.