Grouping features in the Browser Bar

[kmccoy]

I'm working on a fairly complex single part model in Inventor 2010 and I'm finding myself scrolling up and down the browser bar quite a lot to get to the Solid Bodies folder for example, and I was wondering if it was possible to group features into folders or something to make the journey quicker, with the benefit of also being able to just organize things a bit better.

I'm guessing if you could it would be fairly obvious, but still I have a feeling I have seen some mention of this before but I can't find where.

Thanks,
Keith.

[SteveMDennis]

Jimmy, I am not a Creo expert (or even novice) but I think one big differentiator of Inventor that you are overlooking is that the assembly solver is variational. Variational in that everything sort of solves at the same time. it is NOT deterministic and basically does not take any hints from the browser at all. (There is one case where browser order matters but I highly doubt that any customer has ever come up with a case where changing the browser order changes the assembly solve result but in fairness the case does exist). Any browser re-ordering restrictions in the assembly are not due to solving issues like they are in the parametric part world. Any implied reliance on order in the browser is only in your mindset (probably from your Creo experience it sounds like).

[JimmyDoe]

Thanks Steven, I appreciate your reply. Yes I know my mindset is still quite Creo oriented and I have to break that and get into the Inventor mindset. But I just wonder why Inventor didn't keep the same model of browser from the part modelling to the assembly model. Because I find the model browser so nice to follow because its like a flow chart and you can see more clearly what features reference what other features all by following the browser. But then when I get into an assembly, especially if it was created by someone else, I have no idea and no way of knowing their logic behind the model and I don't know how they have things constrained or what is related to the other. Is there a technique I can use to help me better understand how it is built? (I do have the setting set so I see the two part numbers that make the constraint) but I don't really see what that offers me. I guess because I'm used to having one part or datum control the other in an assembly, like a datum or edge reference controls another feature in a part model. You said:  'Any implied reliance on order in the browser is only in your mindset' So then what is the purpose of having the browser in an assembly?

I've had training with solidCAD but when I was talking about this, I didn't get any real clear answer or discussion, it was just like, 'no, learn this way' Do you understand what I mean and where I'm coming from? I just want someone from autodesk to acknowledge my thoughts and to see if they understand my way of thinking about assembly modelling. I just feel sort of lost when I'm working on an assembly because I can't tell what is related to the other and everything is just floating in space. It makes me a lot less confident when modelling now, than I was with Creo.

I would really like your opinion on if I make sense to you and if you could think of some techniques or excercises to help me try to wrap my head around this new (to me) way of modelling.

Thanks

[SteveMDennis]

Jimmy, In 17 years of Inventor development I can honestly say you are the first person who has asked us to be more restrictive in how we handle the assembly browser! People hate that they can't reorder the part browser like they can the assembly browser! When _I_ model (granted I am not a CAD designer) I place a bunch of my components all at once ("I need one of these, two of these, etc.") then I constrain them together. I may constrain part of one part then another and then another before going back to remove the degree of freedom on the first one. I don't see many users who seem to work like you. What I am hearing you say is you place something, fully constrain it then place the next thing, etc. Constraining is a free for all by design... based on my experience and customer dealings if we imposed restrictions in assemblies based on browser order and/or placement order we would be crucified.

[JDMather]

To me the part and assembly browsers work in a very natural and logical manner resembling the real world equivalents.

Part features are parent/child dependency based.  Simple.  A child (feature) cannot exist in history before its parent.

If I am putting together an assembly (in the real world) limits to degrees of freedom are restricted to assembly constraints (like adding fasteners).  I can work with all one level assemblies or more commonly with sub-assemblies assembled into more complex assembly.

Lets say I have these subassemblies and unassembled components laid out on a bench.  I can move them wherever I want on the bench. The only restricted degrees of freedom are those removed through assembly constraints (like fasteners).  So Inventor assembly browser works identically to the assembly lying right before on my bench.  Completely logical!

The purpose of having an assembly browser?

First off all, it gives me a named list of components.

Second - it gives me a record and list of assembly constraints.

Third - well, I am pretty sure I could come up with half a dozen other purposes, but 1 and 2 are pretty compelling.

[JDMather]

I prefer to make these two changes -

[JimmyDoe]

Hi guys,

I find it strange that this is the first you've heard of someone asking about this, because this is exactly how Creo works. Once you bring a component into an assembly, you constrain it and it has relationships to the geometry used to constrain it. You cannot move that constrained part higher in the model tree than the parts/datum features that it is constrained to. It works exactly like the model browser in Inventor. I guess that was something that I liked about Creo. These restrictions, as you call them, are what I would call structure.

JD, as for your statement: 'Part features are parent/child dependency based.  Simple.  A child (feature) cannot exist in history before its parent.' That is exactly what I'm talking about for assemblies in Creo. In Creo there are parent child relationships between the components in an assembly. And that is where all of my talk about how I think the assembly browser should be like the part browser is coming from.

But your example of assembling parts and subassemblies in Inventor is like having all your parts laid out on a bench and constraining them with fasteners or welding, or whatever, is actually very clear and gives me a better perspective/understanding about how assemblies are in Inventor.

However, to support my point, if you have parts on a workbench you can move them all around wherever you'd like. But once they are constrained to each other, they are not free to move anywhere you'd like anymore. So that is still part of my problem with how the browser works. But don't get me wrong, thank you for that analogy, I will keep it in mind and I think it will definitely help to keep my mind straight and on track while I get more used to Inventor.

Thanks guys 🙂

[JimmyDoe]

Sorry to drag this on JD, but I see you are a certified Solidworks professional and I'd just like to ask if the assembly browser works the same in solidworks as it does in Inventor? And do you have any experience with Creo or Pro/E?

And does it still make sense about the work bench analogy that once your parts are constrained to each other, you can't move the individual parts all around on the work bench anymore, so then why can I still move them anywhere I want in the browser, once they are fully constrained?

I will get the hang of things and will quit bothering/arguing with you about this but do you understand my point of view and my thinking about this?

[SteveMDennis]

Jimmy, You don't need to apologize. I am enjoying the interaction we are having and all POVs are welcome and valid. The main thing is that the relationships in the assembly are not order dependent for a solution, they are in parts. Since they are not order dependent (due to the variational nature) why should we limit your choice or organization? When we limit workflows for no reason most users get quite upset with us! There is no computational reason to fix things in the assembly browser (with a few exceptions that are usually complained about by most users). I do now understand your POV but I think it comes from a way of thinking about assemblies that doesn't apply to Inventor.

[JimmyDoe]

Ok, that's good to hear 🙂 I was just looking for someone to actually talk about this with, who understands where I'm coming from, and I finally have!!! It is just very different and still somewhat abstract to me. But I really did enjoy working with Creo, so it may also be a bit of stubborness on my part, trying to hold on to what once was...

But thank you for taking your time to listen and try to understand my thoughts. Most times I've tried to bring this up has not been productive and people think I'm just looking for an argument.

Now, with your title I'm thinking you've got some clout at autodesk. So how about pushing recordable mapkeys 😉 that has got to be the biggest feature that I miss, coming to Inventor. But I know that is an ideastation thing and it's quite off topic. So, thank you for listening and and taking the time to understand my thoughts. I will do my best to rid my mind of Creo and focus on learning Inventor.

Thanks again, major kudos to you!

[SteveMDennis]

Jimmy, Sr. Principal Engineer simply means I've been here are while :-) I have worked on Inventor since before R1 and I am probably one of the 2 or 3 most "senior" developers still on Inventor. I have done some architecture for Inventor and I am primarily what we call a technical lead, meaning I lead other developers on projects. Clout I don't have 🙂 but I do get consulted on many things. I am currently the tech lead for the F3/JDI team that does smaller well understand projects that customers suggest. One of our prime inputs is IdeaStation so please search for your idea there and kudo it or create it if it doesn't exist. We do use it.

[thpope]

I'm totally understanding Jimmy as I'm in the same situation. I simply don't believe everything is solved simultaneously in Inventor. That seems to suggest that the parent-child relationship doesn't exist. It must exist, Inventor just makes it near impossible to see it. But to the short of it, the real problem I'm having is when having to troubleshoot assemblies that I didn't create. I find a lot of sloppy assembly management and frankly, Inventor enables this too much. Not saying it's all peaches and cream with Creo, but I could at least get there, where in Inventor it just seems easier to give up and start over. Except with 1000+ part assemblies, that's not really a practical solution. I find parts floating around all the time. I typically have dozens of constraint conflicts. And most of them have been simply ignored by other designers (and now I'm understanding why).

I've found that assemblies in Inventor really lack clear design intent. Just a real problem when trying to fix someone else's junk. We're moving to SolidWorks, and I truly hope it's not set up the same as Inventor assemblies.

[dylanTEV9W]

I see I'm a little late to this discussion, but being able to group part features together into folders is a feature I've wanted in Inventor for a while myself and I thought I'd point out a few things.

1. Fusion 360 already has this feature and has had it for at least half a year if not much longer. As best as I understand it Inventor and Fusion 360 work off of the same CAD kernel so I can't think of a reason why this feature wouldn't be possible to implement in Inventor. 

2. You can already sort of group features in Inventor...just not all the time like a lot of people would like to be able to do. The stitch surfacing feature is one example of grouping features if it consumes the surface features that are used to create it then it is basically acting like a folder in your part tree. Of course it has some extra functionality that a normal folder would doesn't in that it's also a part feature. You can move the stitch feature up / down the part tree, provided you're not breaking dependencies by moving it to far up or down. 

So it seems to me like it would be very possible to add folders to the part tree without having them break anything. 

[SteveMDennis]

I am sorry to have to reply like this but even though Fusion and Inventor share a kernel that has nothing to do with how the application is architected ABOVE that kernel. The kernel is the low level shape definition code, i.e. how an extrude or loft is created.

Fusion was developed after Inventor as most know and they did endeavor to fix some of the limitations of Inventor while writing it.

Allowing features to be grouped however you want is still on our radar for a future project but it is not easy unfortunately.

[dylanTEV9W]

Thanks for clarifying the differences between Inventor and Fusion. I think we all understand that adding even simple features is no quick or easy task with a large and complex application like Inventor. That being said I was able to hack together feature grouping with only a couple lines of c# code using the client feature object built into the API. See the attached part.  

[SER4]

Here is the idea to vote for:
https://forums.autodesk.com/t5/inventor-ideas/browser-folders-in-part-environment/idi-p/3780620