topic Re: IS INVENTOR REALLY USEFUL?? in Inventor Forum

IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 08:42:29 GMT

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?

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 09:19:37 GMT

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?

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 11:45:57 GMT

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?

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 13:16:32 GMT

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?

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 14:27:57 GMT

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
>

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 15:54:58 GMT

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
>

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 15:55:19 GMT

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
>

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 17:24:15 GMT

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

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 17:39:20 GMT

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

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 18:12:13 GMT

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

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sat, 21 May 2005 20:28:15 GMT

Good explaination Walt.

I was going to discuss the usage of origin features (axis, planes and center point) but you did a better job than I could have. I usually try to constrain the first sketch to the origins to keep the first feature properly located.

The only thing I will add that works well for me. When you want to change a part significantly, but want (or need) to keep the original. First open the part you want to use as the basis for the new part. "save copy as" and close the part, you back the assembly and replace the part you want to work with the new part you just created. Since it is a copy, MOST times all the constraints will stay happy. Then go into the new part and start doing your editing. You will still make constraints sick by adding stuff to the model, but it should be less severe. Also.....you will soon learn to add hardware last.
Although the design accelerator SHOULD make less work of this.
Kent also has a GREAT addin called Kwiksert which makes inserting multiple parts much easier.

A little more experience and you will develop a good workflow.

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Sun, 22 May 2005 01:07:07 GMT

Now if only the developers would return us to the good old days when
constraints to the origin axes and planes were honoured even if you
replaced the part with one that was completely unrelated.

There was a time when you could substitute an assembly for a part and if
the part was constrained by the origin, the assembly would too.

This was great for layout work. Start with a block to reserve space,
then replace it with the assembly once it was available.

Richard

Designer_Mike wrote:
> Good explaination Walt.
>
> I was going to discuss the usage of origin features (axis, planes and center point) but you did a better job than I could have. I usually try to constrain the first sketch to the origins to keep the first feature properly located.
>
> The only thing I will add that works well for me. When you want to change a part significantly, but want (or need) to keep the original. First open the part you want to use as the basis for the new part. "save copy as" and close the part, you back the assembly and replace the part you want to work with the new part you just created. Since it is a copy, MOST times all the constraints will stay happy. Then go into the new part and start doing your editing. You will still make constraints sick by adding stuff to the model, but it should be less severe. Also.....you will soon learn to add hardware last.
> Although the design accelerator SHOULD make less work of this.
> Kent also has a GREAT addin called Kwiksert which makes inserting multiple parts much easier.
>
> A little more experience and you will develop a good workflow.

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 10:05:26 GMT

Yes, a long time request...

"Richard Hinterhoeller" wrote in message
news:4852818@discussion.autodesk.com...
Now if only the developers would return us to the good old days when
constraints to the origin axes and planes were honoured even if you
replaced the part with one that was completely unrelated.

There was a time when you could substitute an assembly for a part and if
the part was constrained by the origin, the assembly would too.

This was great for layout work. Start with a block to reserve space,
then replace it with the assembly once it was available.

Richard

Designer_Mike wrote:
> Good explaination Walt.
>
> I was going to discuss the usage of origin features (axis, planes and
center point) but you did a better job than I could have. I usually try to
constrain the first sketch to the origins to keep the first feature properly
located.
>
> The only thing I will add that works well for me. When you want to change
a part significantly, but want (or need) to keep the original. First open
the part you want to use as the basis for the new part. "save copy as" and
close the part, you back the assembly and replace the part you want to work
with the new part you just created. Since it is a copy, MOST times all the
constraints will stay happy. Then go into the new part and start doing your
editing. You will still make constraints sick by adding stuff to the model,
but it should be less severe. Also.....you will soon learn to add hardware
last.
> Although the design accelerator SHOULD make less work of this.
> Kent also has a GREAT addin called Kwiksert which makes inserting multiple
parts much easier.
>
> A little more experience and you will develop a good workflow.

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 16:02:36 GMT

Great post Walt!

I forwarded it to the documentation team as an example.

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 16:24:53 GMT

I will make an observation here that usually a post that is made by a new
moniker and when they make no further response even with great posts like
Walt's then it was probably just a troll anyway.

It has taken me from using IV R1 till now to get a fairly stable large
assembly and sometimes they still blow up and for the most part when they do
I can trace it back to a stupid move on my part.

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 16:28:35 GMT

Now version 10 that's a different story and since it is still sitting on the
shelf because of my lack of intestinal fortitude I can't make a comment on
how useful it is

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 16:40:07 GMT

Good job Walt, I am going to route this to all of our users here.
Doug

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 17:05:29 GMT

>Now if only the developers would return us to the good old days when
constraints to the origin axes and planes were honoured even if you
replaced the part with one that was completely unrelated.

here here!!

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 18:42:08 GMT

Walt Jaquith writes:

> 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. ...

Additional considerations have to be made when using adaptive parts.

First, try to avoid adaptivity where possible to keep dependencies
down. When a part needs to be adaptive I almost never make part
features adaptive. Instead, I only create adaptive work features.
Then I use those adaptive work features in part sketches. This way
these dependencies become constraints in the assembly and are much
easier to change.

When a feature in the assembly disappears the constraint will become
sick and can be fixed easily by editing it. When external geometry
has been projected into a sketch one has to edit the sketch, delete
the sick references, create new ones and constrain the sketch to the
new references. This is a lot more work.

I only wish one could use external work features to create adaptive
work features in an adaptive part. When I want to use a work feature
I have to create the new work feature using some geometry and then
edit the constraint to use the work feature I want.

Matthias

Re: IS INVENTOR REALLY USEFUL??

Anonymous — Mon, 23 May 2005 19:03:14 GMT

A troll you say. A troll? I resemble that remark. Obviously I started this post in a fit of frustration but I appreciate the input from all. I have some work to do and it reassuring to know it'll get better with experience.

Another technique I'm playing with is to ground all parts of my assembly. Of course this will only work for stuff that's not supposed to move. And I find that once everything is grounded they surely do not move.