Inventor assembly constraints - show constraints only for the part being assembled

[Anonymous]

Hello

I'm new here, trying to learn Inventor. 

One thing I noticed in the assemblies and I don't understand why Inventor does this is to show all constraints from all parts under one part.

It shows the assembly constraints for the part itself and then it shows all the constraints from all the other parts that are assembled onto that part.

For example in the picture I attached three of the mates are used to assemble the spacer onto a plate. The rest of constraints that show up are from other parts assembled onto the spacer.

Why does inventor work like that?

Why not show only the three constraints that are used to assemble the part?

And OK let's say it's a functionality of Inventor, but who uses this "feature". If you have like 10 parts assembled onto the spacer all constraints from all 10 parts will show under the spacer. And if you want to modify the way the spacer is assembled you have to go thru all those constraints to see which ones are just for the spacer and not for all the children's.

I don't understand why its a good thing to go thru like 30 constraints to find the ones you want to modify.

Or is there a setting to see just the constraints for each part ?

Thanks

[swalton]

Unlike PTC Creo, Inventor does not care about assembly order when solving the constraints in an assembly.  The first three constraints on a component have the same solve priority as the next 60.  

It is possible to have the location of the first component placed in an assembly be driven by all the other component locations. The user needs to be able to see and evaluate all the constraints on a component.

It is easy to create complex logic chains with the assembly constraints.  I try not to do that. I try to tie location to origin planes, key components, feature patterns, and other unchanging geometry.  I also try to be consistent in how I apply constraints.  

[Gabriel_Watson]

A relationship/constraint between one object and another belongs to both components that lent some geometry as requirement to form such constraint. In Inventor the base components for a constraint are shown explicitly, and the reasoning behind this is that you can right-click and pick "Other half" to find out which other component shares that constraint.

I see it as a trade-off, between simplicity of visualization (having only the first base item as a reference for the constraint) and full access to how things actually work. Often in assemblies that are 1000+ components heavy you have to know where a component connects to another without dancing around whether the chicken or the egg was the first to come.

Ultimately, you would have issues only because of your current design practices. Think of it this way: if you add too many constraints to one individual component, you're doing it wrong. Try to constrain each component with as little operations as possible, and split the constraints across many components instead of adding them all to a central component. As @swalton above said, you should be constraining components to your origin planes/axes/point and construction elements as often as possible.

[Anonymous]

I try to do the same, use default planes as constraints and where ever possible I design parts symmetrically by the default planes so I can use those in assemblies. That way if the part changes shape the constraints remain.

@swalton guessed me well with CREO 🙂

And yes I understand what @Gabriel_Watson is saying about constraints, I don't over constrain. As to splitting constraints across many components it's not always possible. I try to do sub-assemblies where possible.

But even one part that has 3-4 other parts assembled on it will show me a lot of constraints on the first part.

And the worse thing that I've seen on a few designs is that you can drag these constraints and rearrange them.

I could get over this if the first constraints would be from the part being assembled and the rest from all its children's. But when people start shuffling the constraints in the list and they are all mixed up, it's very difficult to easily find the constraints you are looking for.

Seams to me like bad design practices from the other users.

So I guess there is no setting to only see one set of constraints and not all of them?

[Gabriel_Watson]

Well, sadly I guess, the best you could do for your case is right-click each relationship and pick "Isolate Components" to understand them better if needed (when highlighting the components is not enough after selecting the constraint).

Inventor does not allow grouping/subfolders within the Relationships folder. I would guess the only way to have more control over those is to dump all the relationship pairs into an Excel sheet or exported file via iLogic, and use it as a guide.

[BDCollett]

There are a lot of tools to help manage constraints. 

You can visually see them with mouse over, you can turn on the visibility and see in your assembly, mousing over the icon then highlights what is constrained. You can name them as well.

If you select the part you can "Show" all constraints for that part and get these visual guides in the assembly to help easily find what you need.

[Anonymous]

I don't want to use excel or any other thing to get to a simple constraint. I mean it doesn't make sense and is not practical from a design perspective, I need to be quick in finding the references and be able to changes them.

Isolate and show does not help. I know where my parts are in the assembly , I can easily pick them up in the window. I know each one where it is and how I assembled it. It's the after, when I want to redefine something I have a hard time finding the constraints in the list, having to go thru a big list of constraints.

Show constraints, even if I isolate the two parts, will show all constraints from all parts related to those parts.

As for naming them, I wouldn't spend time on that, its time consuming. I found a setting in the "application options"  under the assembly tab that will show you the component names next to each constraint. Its called "display component names after relationship names"

At least that is a start, I can now see to which part the constraints belong to.

It's still not ideal when you have a lot of constraints, that is still a problem in my opinion.

For example a fixture that I was working on, has a main plate and on that plate there are a lot of parts and sub assemblies. No way around this. Even if I make sub assemblies there are still a lot of constraints

See the picture I attached. Now to go thru all of those to see which one I need is a pain.

I don't understand why this functionality, I might miss something on what is the approach to work with these.

Right now I don't see any benefit in having all constraints show up. In the end I guess I will have to get used to this somehow.

thanks for the replies

[swalton]

Autodesk's decision to not have a history-based constraint solver can be awkward.  It becomes very helpful when I want to have kinematic/constraint chains that are independent of the order that I add components to an assembly.

Some more tips that you might already be using:

1. Build the assembly the same way you would in Creo.  Start with the obvious base component, fully constrain it to the assembly origin geometry, then add parts/sub-assemblies in a logical order.
2. Make the first 2-3 constraints on a component the ones that attach it to its parent.  Additional constraints should be used to attach child components.  Try not to mix-and-match constraints in that order.  
3. Redefine existing constraints instead of deleting them.  That way the list order won't change in the browser and you can quickly check the first 2-3 constraints to move a component.
4. Expand a component's listing in the model browser to see the constraints that affect it.  If possible, select the child component that you want to move, rather than the parent.  That should give you the shortest list of constraints to check.
5. Be consistent in how you build your constraint sets.  Because of my Creo habits, I pick the geometry of the child component first, then I pick geometry from a parent.  When I look at the Display Component Names information, I know that the first name is the child and the second is the parent.  That helps me remember the logic that I used to build the assembly.  I think that the Inventor developers expect people to pick the parent geometry first, then the child geometry, but I haven't been able to break years of Creo habits.  
6. Constrain to the real-world physical interfaces between components if possible.  To move a child, go to the parent model and move the interface, rather than adjust a constraint.  I'm thinking bolt patterns, pilot holes, tabs and slots, or other similar geometry. 
7. Conversely, you can constrain between the model origin geometries.  Those constraints are very stable because the origin geometry can't be altered.
8. Some people ground their components to minimize the number of active constraints that Inventor has to solve.  
9. The Relationships folder is almost useless.  In a small assembly the list is short and manageable, but in a larger (50-50k components) it is impossible to find anything.  I only use it when I want to delete every constraint in an assembly, or when troubleshooting a seriously broken one.

[Anonymous]

Yeah that's what I started to do. I started building my assemblies in a logical order like I would do in Creo.

And I'm grouping my constraints , the first ones in the list are from the current part. The rest I don't really care.

Not always possible because I'm not the only one working on the assemblies and the other Inventor users got used with this and they don't really care about the mess (yeah)

I can see the benefit of not having an order of assembly from a concept designer point of view. Because you can just put the parts in the assembly without any constraints, move them around, add some other parts and when you are happy with the design start constraining everything.

Which is fine, but I don't see why Autodesk decided to show all constraints from parents and children's together. At least have a default option to group them.

Or have the option to redefine them , do right click on the part and have the option to redefine the part and show you just the constraints for that part.

Maybe I should put this as an idea for future inventor versions, I've seen something like that on the forum

[Gabriel_Watson]

Several ideas worth voting for:
https://forums.autodesk.com/t5/inventor-ideas/relaionship-folder/idi-p/8776556
https://forums.autodesk.com/t5/inventor-ideas/leveraging-folders-to-manage-assembly-constraints-unde...
https://forums.autodesk.com/t5/inventor-ideas/grouping-of-constraints/idi-p/9234909
https://forums.autodesk.com/t5/inventor-ideas/group-constraints/idi-p/7466563
https://forums.autodesk.com/t5/inventor-ideas/assembly-quot-add-to-new-folder-quot-funtionality-for/...

https://forums.autodesk.com/t5/inventor-ideas/moving-multiple-relationships-at-once/idi-p/5567734

And an archived related one:
https://forums.autodesk.com/t5/inventor-ideas/delete-constraints-on-specific-components/idi-p/550013...

[jreidenbaugh2MD67]

Contributors on this site always default to defending Inventors shortcomings instead of answering the many legitimate questions that get asked. Inventor is mid-tier software in this arena, at best - the whole world knows it. The constraint GUI is terrible - period. I am forced to use Inventor periodically and always count the days until I'm free of it.

[johnsonshiue]

Hi! We are aware of the deficiency in the assembly constraint workflows. If possible, please be more specific so that we can understand your concerns better and make improvement accordingly.

Many thanks!

[jreidenbaugh2MD67]

I would think the easiest way to prevent the frustration I see all over the internet when it comes to Inventor functionality would be to actually address the problems, but I see no evidence of that. I last used Inventor 4 years ago and it was no different then. The impossible knot of relationships that are created in large assemblies is only exacerbated by the lack of information about any specific relationship and how it's presented.
My objection to the majority of the blogs that service the multitude of Inventor users who find the Autodesk help features lacking, is the default setting that all responders seem to have that causes them to flee to a defensive position when a simple question exposes the deficiencies in the software. Responses are often "you're doing it wrong", or "the work-around is this" - both are flawed answers for different reasons but they dominate the chatter out there.
I don't hate Inventor, it has some redeeming qualities, but it is currently my last choice and I wouldn't use it for a large, complex project. Take that as you will but it is what it is, and I'm not alone.





Please type your reply above this line -##

[SBix26]

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@jreidenbaugh2MD67 wrote:
Responses are often "you're doing it wrong", or "the work-around is this" - both are flawed answers for different reasons but they dominate the chatter out there.

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How would you like us to respond instead?

"Yes, you're right, it sucks."

or

"I'll fix that immediately."

or... what?

We users of the application cannot, of course, promise immediate fixes per your request.  Agreeing with you is not helping you get your work done.  The only thing we have to offer is possible solutions, which will tend to fall in the categories of "here's how it's intended to work (you're doing it wrong)" or "we know that functionality isn't available, but here's another way to get the result you need (the workaround is this)".

I'm at a loss to know what other response you think a user forum could offer.

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Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[jreidenbaugh2MD67]

Answer any way you want, it's your forum, I'm not trying to tell you how to run it. While my frustration shows thru in my attempts to find the answers to things I'm trying to do in inventor, I can honestly say I rarely find it here.

[SBix26]

Try us... you've got four posts in this forum under your current login, and none of them are problems seeking a solution.  I would categorize them as generalized rants.

Show us something that you're finding difficult with Inventor and someone here will provide an answer.  But please be professional (respectful), detailed, and specific.  You will get more useful answers that way.

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Sam B

Inventor Pro 2024.2 | Windows 10 Home 22H2

[BDCollett]

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@jreidenbaugh2MD67 wrote:

Answer any way you want, it's your forum, I'm not trying to tell you how to run it. While my frustration shows thru in my attempts to find the answers to things I'm trying to do in inventor, I can honestly say I rarely find it here.

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Sounds like a you problem honestly. We are all just users of the software, giving our free time to help people. Many get very valuable help.

If you don't like Inventor, then use something else.

If people offering workarounds or pointing out better ways to use the software offends you, we can't help that. No one says it's perfect, I am constantly pointing out where they can do better, I am also active in the Beta and posting in the ideas forum. Are you?

[johnsonshiue]

Hi! If you can share an example of the exact undesirable behavior, I will be more than happy to take a look to understand it better. So far I have not seen an example. I do feel your frustration. Inventor has a lot of room for improvement. Some aspect of assembly modeling is indeed lacking or unintuitive. But over generalization does not help us.

If possible, please share the image or Inventor files that exhibit the issue with me johnson.shiue@autodesk.com.

Many thanks!