Constrain to origin?

[Anonymous]

Per my above post with my assembly going askew, is it good practice to
constrain the first grounded part in an assembly to the origin?

It makes sense to me and I would like this not to happen again.

Thanks

Russ Tanner

[JDMather]

>Per my above post

You should reply in the original thread. Above is all relative as the day goes by.
It is considered good practice to apply flush constraints between the workplanes of the logical grounded part workplanes and the assembly workplanes.

http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf
Tip 87

[Anonymous]

Oh gosh nevermind 😜


wrote in message news:5462680@discussion.autodesk.com...
>Per my above post

You should reply in the original thread. Above is all relative as the day
goes by.
It is considered good practice to apply flush constraints between the
workplanes of the logical grounded part workplanes and the assembly
workplanes.

[JDMather]

http://www.sdotson.com/freetut/tipsforassemblies.pdf

[Anonymous]

This information was originally provided by someone in Autodesk. I can't
attach it because it seems IT now has limited my ability to do this.





INVENTOR BEST PRACTICES



Sketches



1. Project the part origin or some other RELIABLE and LOGICAL geometry into
each new sketch and reference new sketch geometry to it.



2. Sketches should be fully constrained and related to the sketch origin.
Avoid using the fix constraint, it makes the sketch difficult to edit by
another user.



3. Apply sketch constraints and dimensions carefully and logically so that
the sketch geometry will change in a predictable manner when a dimension is
edited.



4. Avoid placing fillets and chamfers in sketches. If possible, make them
the last thing added to the part. Only add them earlier if there is a
functional necessity.



5. Use construction lines to make sketch relationships easier to analyze.



6. Use cross part sketches only for strategic relationships. These are
powerful in creating associativity across parts but can add complexity to
making changes in your design.



7. Use silhouettes only when absolutely necessary. These are highly depended
on the sketch plane and its orientation to the source geometry. Large
changes can have unexpected results.



8. Turn off "show constraints" when done. The visibility setting of
constraints is remembered and you might surprise someone when they go edit a
model of yours, activate a sketch and all the constraints appear needlessly.



9. When importing DXF and DWG (remember you can copy and paste in R11) data
use the Auto dimension command. Uncheck the dimension optional and then
press the apply button until the number of constraints needed stops
changing. You might need to click apply three times for this to happen. Now
you should have a much better constrained sketch to start with and need
fewer dimensions to finish fully constraining you sketch.



10. Less is more. Don't overload a sketch too much. Think 20 sketch lines
and 3 to 10 dimensions per sketch. This helps break the model up into
manageable pieces and makes editing the design easier.



Features



11. Rename key features in the feature tree. This makes it easier for
another user to find and edit features.



12. Use user defined parameters for common dimensions in a part where
applicable. For example, if a typical wall thickness is to be used in a
casting design, define a parameter called "wall" and assign that value to
applicable dimensions. If during the design process a universal change in
wall thickness is required it becomes a simple change of one parameter and
hitting the update button. This can also make it easier for downstream users
to quickly identify the key design parameters.



13. If the parameter has a value restriction (only + or - 1 or 0, 90, 180,
or 270), make sure to describe the proper use of the parameter in the
comment field. If you use an external source, such as a spreadsheet, to feed
parameters to your model, make sure to note both the spreadsheet and model
so that they reference one another. Add tolerances to model parameter if you
know them.



14. Use equations. For example, rib thickness is generally a percentage of
wall thickness. Instead of applying a discrete value to a rib's thickness,
make it a function of the wall thickness dimension. Better yet, create a
parametric value to do this (see tip above) and use it for the rib
thickness. By doing so, if the wall thickness is changed, the rib thickness
will change accordingly.



15. If the design is quite complex, use the Engineer's Notebook to document
what/how/why you've designed the way you have.



16. Avoid parent/child relationships between features. Unless necessary,
avoid starting sketches on part faces or projecting feature geometry.
Instead, use the origin geometry or work geometry based off the origin
geometry. Critical relationships between features should be obvious and
logical so that changes to other parts behave in a predictable manner.
Objects to avoid creating relationships to:



. Faces and edges of chamfers and fillets

. Features in a pattern or mirror, unless it's the parent feature(s)

. Edges or seams of non-analytic surfaces (like swoopy curvy surfaces from
loft)

. Non associative cross part projected sketch geometry that is fixed or
grounded

. Grounded work geometry



17. Name your features if they are critical or commonly edited. Naming
construction geometry will make working with the model significantly easier
and should be done as often as possible.



18. Add cosmetic features like decals and embossed text at the end of the
feature tree.



19. If a group of features are all relative to a point other than the
origin, or at an odd angle to the origin planes, create a common set of work
geometry (referenced from the origin) to act as a pseudo-origin point. Build
the features relative to this pseudo-origin



20. Avoid unnecessary features and work geometry. They increase file size,
clutter the feature tree and slow down the program. This is important when
working with complex parts. Strive to have a clean, efficient, stable and
logically ordered part as your finished product. Downstream users
(sometimes, that's even yourself) should be able to understand and edit it
as easily as possible. A minimal investment of time and effort during model
creation will pay off greatly downstream.



21. Don't take shortcuts. Edit features to make changes, use grips to help
speed up finding the feature and dimension to change. Common examples to
avoid:



. Do not fill in holes to remove them. Delete the hole and repair if needed.

. Do not stack extrudes on top of one another to make a part longer. Edit
the dimension.



22. When possible pattern features rather than sketches. these are easier to
edit and understand



23. When making large sweeping design changes to a feature, drag the EOP to
right below the feature you are about to hack. Then progressively roll the
EOP down and repair as needed. This approach is faster and easier than
letting the model fail massively. If the model does have massive failures
re-read these tips and try to create a more solid model and as you repair
it.



24. When filleting difficult models, turn of chain edges to reduce the
number of edges that you are trying to round. Fillet corners with mixed
radii and convex/concave solutions first then finish the other edges after.



25. When e-mail a native Inventor part. Roll the end of part marker to the
top of the browser and save the part. This will decrease your model's size.



Assemblies



26. When possible keep the assembly aligned to the origin and as near as
possible. Assemblies that are far away from the origin or at odd angles can
be difficult to work with.



27. Think about what the first part should be in an assembly before
inserting parts - better yet go ahead and mate the logical grounded part to
the assembly planes.



28. Group parts in the browser to organize them and make for a logical
structure. Rename components when needed. Be aware that names will not carry
if you do component replace. Some users are confused with browser names that
don't match part number or file name. Decide what you will use in your
company and standardize on it.



29. Use assembly construction geometry only when necessary. If you find that
you need a large number of assembly construction geometry than consider
learning master modeling techniques.



30. Use assembly features only when necessary. If you find you are creating
a large number of assembly features reevaluate you design approach or confer
with an Inventor expert to see if there is an alternate approach.



31. Minimize the use of tangent constraints. While useful, they can be
geometrically difficult to maintain and can add to unstable constraint
solutions.



32. Use the select and find tools to your advantage. Save frequently used
views a design views. If working in a workgroup consider saving you views as
a private design view.



33. Use the Degree of freedom tools to help identify under constrained parts
that might make a mechanism not work as intended. The find tools allow you
to search for components with more than x number of degrees of freedom. A
good search to have saved is "Find all components with two or more degrees
of freedom."



34. Turn off adaptivity as soon as you no longer need it.



35.For speedier interference checks use the all content center suppressed
LOD Rep before running an interference analysis. It will ignore any tapped
interferences and speed up the simulation. If you only need to check two
parts use measure to find the minimum distance between parts, if the
interfere the measure too, will alert you.



36. If a face or axis is a key mating surface Create a workplane or workaxis
to assemble to rather than using the faces. Make these in the part not the
assembly. This will allow you to make more changes later and not worry about
assembly constraint problems. It also will allow you more flexibility when
working with advanced techniques like LOD or derive part base master
modeling approaches.



37. If a component is frequently reused and constrained in the same way(s)
consider using iMates or composite iMates to capture these mating
conditions. This will save time latter.



38. Turn off contact solver after analyzing contact motion.



39. When mating things that are symmetrical, mate to your center planes, go
back to the assembly plane when practical.



40. Standardize on component properties and be disciplined in keeping them
accurate and filled out. This will make sorting, searching and finding
components easier. It will also make filling out BOM columns more automatic.



41. Create design views and LODs for use when making drawings and
presentations. A little up front work will save a lot of headaches later.
Use these reps associatively in your drawings and presentations.



42. Use the global visibility overrides for quick visibility changes only.
Leaving these on can cause planes, sketches, welds and other critical design
features to not display causing confusion. A better alternative is to use
public or private design views.



Drawings



43. Align views to one another to make moving views easy



44. Whenever possible use associative design views. When creating views.



45. Recover work geometry and dimensions to save you time annotating. The
work you put into the model and tolerances is most valuable on the drawing
and saves you time.



46. If you need to create construction views, place them on a non printing
sheet rather than off the border, or on a hidden layer. It makes working
with the drawing easier.



47. Spend the time to make and keep up to date your style library. Ensure
you have styles for your most frequent types of annotations.



48. Unless you have a company standard that requires otherwise, try to keep
one part or assembly to one sheet in one IDW. This simplifies the
relationships between drawing and part and protects you should a drawing get
lost or damaged. You will have significantly better performance too.



49. Create a library of symbols and add these to your template. Saves you
time having to redraw them every time.



50. Fully constrain your section and breakout view sketches. This will
ensure that they update correctly.



51. Always anchor your detail views. This will ensure that they update
correctly and move with the important geometry. (Thanks Quinn)



51. If you are making many changes to a part design, open the drawing and
leave it in the background. You will find that the drawing may update faster
and more reliably then having the drawing go through one massive update when
you open it later.



53. When creating leaderless annotation or notes on a view, make sure that
you first create it inside the view border. This will associate the
annotation with the view and it will move with the view.



54. Use property values in Title blocks rather than prompted text. It makes
the drawing title block much smarter in the long run.



55. For drawings that you are archiving, set defer updates to on to be sure
that the drawing does not update.

"Russ" wrote in message
news:5462627@discussion.autodesk.com...
Per my above post with my assembly going askew, is it good practice to
constrain the first grounded part in an assembly to the origin?

It makes sense to me and I would like this not to happen again.

Thanks

Russ Tanner

[Anonymous]

This is the contents of a reply by Walt Jaquith. Walt was responding to a
frustrated user's experience with Inventor. I give it to ever noob that
starts work with me. It's just that good.


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





"Russ" wrote in message
news:5462627@discussion.autodesk.com...
Per my above post with my assembly going askew, is it good practice to
constrain the first grounded part in an assembly to the origin?

It makes sense to me and I would like this not to happen again.

Thanks

Russ Tanner

[mcgyvr]

I always do now because I typically render alot of top level assemblies in Studio and use the reflective ground plane options.

Is it necessary=No
Is it good practice=Yes

[Anonymous]

>logical grounded part workplanes and the assembly workplanes.

hehe, I"ll have to ponder on that one later after work.

Basiclly I have been building assemblies off a grounded part instead of
constraining that part to planes. I got away with it till today.
I do build parts per the BORN method and think xyz in how those parts are
made to keep things lined up.

Thanks for the input

Russ Tanner

wrote in message news:5462680@discussion.autodesk.com...
>Per my above post

You should reply in the original thread. Above is all relative as the day
goes by.
It is considered good practice to apply flush constraints between the
workplanes of the logical grounded part workplanes and the assembly
workplanes.

http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf
Tip 87

[Anonymous]

Some good words of wisdom.

"John-IV1.000E +001 SP0.3.000E +001" wrote in message
news:5462706@discussion.autodesk.com...
This is the contents of a reply by Walt Jaquith. Walt was responding to a
frustrated user's experience with Inventor. I give it to ever noob that
starts work with me. It's just that good.


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





"Russ" wrote in message
news:5462627@discussion.autodesk.com...
Per my above post with my assembly going askew, is it good practice to
constrain the first grounded part in an assembly to the origin?

It makes sense to me and I would like this not to happen again.

Thanks

Russ Tanner

[shaney]

(When I started Inventor) if I would have read this and continuously tried to apply it along with working through the tutorials provided by J.D. Mather and sDotson (or maybe just took some training course), there's no doubt it would have saved us thousands of dollars. It might have saved a few years of my life also not stressing to learn it the hard way. But, I've found my boss loves setting people up for failure and watching them struggle. I guess it makes him feel adequate.

[Anonymous]

All the comments here are appreciated. I can see the mistake of starting an
assembly and relying on just "grounding" the base part.

This is a somewhat complex subject for the guy with just over a year in
Inventor, but as time goes along much is learned.

I would be very interested in looking at some assemblies to see how some of
you with more experience do things in regard to constraints, browser use, so
on. Its one thing to type up a tutorial but examples are very powerful to
analyze and learn from.

If you have something I can look at please email to cad@tannersacre.com

Thanks to all (This is a very informative news group!)
Russ Tanner

wrote in message news:5462681@discussion.autodesk.com...
http://www.sdotson.com/freetut/tipsforassemblies.pdf

[Anonymous]

More likely your boss just didn't understand what is required to properly
apply the tool and assumes it's just another type of AutoCAD, incorrectly,
like most other managers. It is a common flaw of most organizations to
oversimplify implementations of new technology in general and wind up
learning the hard way, doing things more than once, and winding up going
over budget and behind schedule.


wrote in message news:5462969@discussion.autodesk.com...
(When I started Inventor) if I would have read this and continuously tried
to apply it along with working through the tutorials provided by J.D. Mather
and sDotson (or maybe just took some training course), there's no doubt it
would have saved us thousands of dollars. It might have saved a few years
of my life also not stressing to learn it the hard way. But, I've found my
boss loves setting people up for failure and watching them struggle. I
guess it makes him feel adequate.

[shaney]

That part you were replying to applies to everything here, not just inventor. But I appreciate your good faith.

[Josh_Petitt]

>On the other hand, it's also possible to build assemblies
that are nearly bulletproof.

Does this require the Kevlar add-in? 🙂

[mikevick]

Hi This may seem like a stupid question but im moving over from solidworks back to inventor for the first time in four years and im just trying to get my head around some things. On a sketch if i draw a rectangle and stick a construction line from corner to corner i can't constrain the midpoint of that construction line to the origin. why is this? is there a setting i need to turn on in application settings?

[mikevick]

Its ok i found out you project geometry of the origin/center point when you start a drawing and then constrain to that. If there is a way to set this before hand please feel free to add

[JDMather]

---

@mikevick wrote:

Its ok i found out you project geometry of the origin/center point when you start a drawing and then constrain to that. If there is a way to set this before hand please feel free to add

---

Uhhmm, what version of Inventor are you using. (that has been the default behavior for years)  You might want to read these documents

newer

http://home.pct.edu/~jmather/skillsusa%20university.pdf

older

http://home.pct.edu/~jmather/AU2006/MA13-3%20Mather.pdf