Inventor General Discussion

Inventor General Discussion

Reply
Valued Contributor
carnac
Posts: 65
Registered: ‎03-28-2004
Message 1 of 82 (1,155 Views)

IS INVENTOR REALLY USEFUL??

1155 Views, 81 Replies
05-21-2005 01:42 AM
Is it just me or is Inventor a house of cards? The system works well for me until I make an assembly, then when I want to change or replace a part I lose the constraints and the house of cards crumbles and all is to do again. I've taken a class, I have three big fat books on Inventor and still I cannot see how this system is useful to make assemblies. Is this a common problem?
*Derek Burns
Message 2 of 82 (1,153 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 02:19 AM in reply to: carnac
I guess it depends on what you are changing or replacing your part to, as
well as your workflow.
If you are referring to changing or replacing fasteners, then using iParts
will generally resolve your constraint issues. Forward planning is required
if you are making an assembly which you will copy or use to create many
permutations. If you have many variable sized parts , consider creating
iParts of those, also create similar parts from a common base part template.
Breaking down your assembly into smaller subasseblies will reduce the amount
of constraint dependencies.
I find Inventor to be an extremely useful tool.

Derek Burns

wrote in message news:4852684@discussion.autodesk.com...
Is it just me or is Inventor a house of cards? The system works well for me
until I make an assembly, then when I want to change or replace a part I
lose the constraints and the house of cards crumbles and all is to do again.
I've taken a class, I have three big fat books on Inventor and still I
cannot see how this system is useful to make assemblies. Is this a common
problem?
*Richard Hinterhoeller
Message 3 of 82 (1,153 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 04:45 AM in reply to: carnac
For me, it's useful.

The situation you describe was certainly a HUGE frustration at first but
with experience, it's no longer an issue.

Richard

Carnac wrote:
> Is it just me or is Inventor a house of cards? The system works well for me until I make an assembly, then when I want to change or replace a part I lose the constraints and the house of cards crumbles and all is to do again. I've taken a class, I have three big fat books on Inventor and still I cannot see how this system is useful to make assemblies. Is this a common problem?
*Larry Caldwell
Message 4 of 82 (1,153 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 06:16 AM in reply to: carnac
If you bolt a different part on a real-world assembly you have to
re-constrain it as well. Doing it in Inventor, at least, that's not always
the case; dependent on changes in geometry. Hard to see how to expect
Inventor to know how you want to constrain a different part to existing
geometry and further, don't see, even if it made that dubious assumption,
how it would be possible without using a considerable amount of resources to
calculate the differences in the two parts, the existing constraints and
whether or not constraining in the same manner is possible ... not to
mention desirable; for that the program would need to be clairvoyant.
~Larry

wrote in message news:4852684@discussion.autodesk.com...
Is it just me or is Inventor a house of cards? The system works well for me
until I make an assembly, then when I want to change or replace a part I
lose the constraints and the house of cards crumbles and all is to do again.
I've taken a class, I have three big fat books on Inventor and still I
cannot see how this system is useful to make assemblies. Is this a common
problem?
*Jon B. Jacob
Message 5 of 82 (1,153 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 07:27 AM in reply to: carnac
How do you handle the following situation? Say you have two
parts that are cylinders. They are then inserted into an
assembly and constrained with an insert. Then you do a
fillet on one of the parts on the edge that was used for the
constraint. The dreaded red cross then appears. Can one use
another approach to prevent this from happening?

Larry Caldwell wrote:
> If you bolt a different part on a real-world assembly you have to
> re-constrain it as well. Doing it in Inventor, at least, that's not always
> the case; dependent on changes in geometry. Hard to see how to expect
> Inventor to know how you want to constrain a different part to existing
> geometry and further, don't see, even if it made that dubious assumption,
> how it would be possible without using a considerable amount of resources to
> calculate the differences in the two parts, the existing constraints and
> whether or not constraining in the same manner is possible ... not to
> mention desirable; for that the program would need to be clairvoyant.
> ~Larry
>
*Byron Newton
Message 6 of 82 (1,153 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 08:54 AM in reply to: carnac
Constrain with a workplane, axis and workpoint that is constructed in the
part model.

"Jon B. Jacob >" <"Jon B. Jacob" <"jjacob AT acm-nevada DOT com"> wrote in
message news:4852738@discussion.autodesk.com...
How do you handle the following situation? Say you have two
parts that are cylinders. They are then inserted into an
assembly and constrained with an insert. Then you do a
fillet on one of the parts on the edge that was used for the
constraint. The dreaded red cross then appears. Can one use
another approach to prevent this from happening?

Larry Caldwell wrote:
> If you bolt a different part on a real-world assembly you have to
> re-constrain it as well. Doing it in Inventor, at least, that's not always
> the case; dependent on changes in geometry. Hard to see how to expect
> Inventor to know how you want to constrain a different part to existing
> geometry and further, don't see, even if it made that dubious assumption,
> how it would be possible without using a considerable amount of resources
> to
> calculate the differences in the two parts, the existing constraints and
> whether or not constraining in the same manner is possible ... not to
> mention desirable; for that the program would need to be clairvoyant.
> ~Larry
>
*Larry Caldwell
Message 7 of 82 (1,153 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 08:55 AM in reply to: carnac
Well ... in the unlikely event that I concluded an insert constraint was
imperative and it turned out to be on the end I needed a chamfer/fillet on,
I would reapply the insert constraint after it failed. Alternatively, in a
more likely situation where an insert constraint wasn't imperative and I
wanted to be able to add/remove fillets/chamfers at will without losing the
constraints I would use mate axis/mate face on the sketch geometry as
opposed to the part geometry. If you understand that changing part geometry
renders the constraints untenable, there are a lot of ways to approach
modeling practices in order to cause oneself ... what ... the least amount
of grief possibly.
~Larry

"Jon B. Jacob >" <"Jon B. Jacob" <"jjacob AT acm-nevada DOT com"> wrote in
message news:4852738@discussion.autodesk.com...
How do you handle the following situation? Say you have two
parts that are cylinders. They are then inserted into an
assembly and constrained with an insert. Then you do a
fillet on one of the parts on the edge that was used for the
constraint. The dreaded red cross then appears. Can one use
another approach to prevent this from happening?

Larry Caldwell wrote:
> If you bolt a different part on a real-world assembly you have to
> re-constrain it as well. Doing it in Inventor, at least, that's not always
> the case; dependent on changes in geometry. Hard to see how to expect
> Inventor to know how you want to constrain a different part to existing
> geometry and further, don't see, even if it made that dubious assumption,
> how it would be possible without using a considerable amount of resources
> to
> calculate the differences in the two parts, the existing constraints and
> whether or not constraining in the same manner is possible ... not to
> mention desirable; for that the program would need to be clairvoyant.
> ~Larry
>
*Walt Jaquith
Message 8 of 82 (1,153 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 10:24 AM in reply to: carnac
Inventor is not a house of cards, but it's surly 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
*Larry Caldwell
Message 9 of 82 (1,152 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 10:39 AM in reply to: carnac
Well said.
~Larry

"Walt Jaquith" wrote in message
news:4852772@discussion.autodesk.com...
Inventor is not a house of cards, but it's surly 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
Distinguished Contributor
SemiCatS
Posts: 239
Registered: ‎07-28-2004
Message 10 of 82 (1,152 Views)

Re: IS INVENTOR REALLY USEFUL??

05-21-2005 11:12 AM in reply to: carnac
You should really write a book on the subject! Quite a few good points to put one one's mind when creating both parts and assemblies. Very well explained.

Stig M. Thu
Post to the Community

Have questions about Autodesk products? Ask the community.

New Post
Announcements
Do you have 60 seconds to spare? The Autodesk Community Team is revamping our site ranking system and we want your feedback! Please click here to launch the 5 question survey. As always your input is greatly appreciated.