Type of history

[Flowh64]

Hello, This question is asked to developers or mechanical draftsmen of trades (Design office).
Thank you to Fusion 360 makers and trainers for not intervening.
I would like to know the reason for the choice concerning the history?
industrial designer and user of Solidworks, Catia V5, and PTC Creo, I unfortunately did not have the opportunity to work in depth with Inventor but it will surely come. I've never had any problems adapting to most software, my questions are not related to habits on my part.
At first sight Fusion seems interesting but in concrete use on a study, I realize that certain technical choices seem disabling to me.
My first concerns this type of history. You know the one used by the software I mentioned above, so I won't dwell on it. The problem I encounter with this method which records all the user's actions, including movements, link modifications... a lot of things that are of no interest.
We find this type of history in the majority of software in the form of a list, and thanks to an Undo or Z control, we can go back. But you can never change anything and ultimately so much the better. When designing machinery, there is research, a lot of research, so a lot of actions and therefore a history that continues to grow! To alleviate all this, of course I use the activation for each part or subset, each one therefore has its own history. This is the case if I don't forget anything and since I am not perfect, you can imagine that it will happen to me.
But in fact it happens to everyone. So, as if that weren't enough, the histories get mixed up :s. And as I said above, the size of the history never ends (despite the activation of each part) and when I have to modify a function, a sketch... the whole history is recalculated! Which takes between 30s and 2min. It is therefore unusable.
So why this choice of history? You know Inventor or at least your colleagues who worked on it. So there is necessarily a technical or commercial reason, which escapes me and which pushed you to use this method. In any case, for my design office it is really very heavy to manage.
I have to make a choice of software, the license of Fusion is attractive, but if the product is not adapted to my use, useless for me that I waste my time and money.

Thanks in advance.

[Flowh64]

Hello,

26 views and 0 replies.
To put it simply, why this type of history:

Rather than this?

So what are the benefits?

Thanks in advance.
Hoping to finally have an answer.

[TrippyLighting]

Can you perhaps share what the nature of your work is and what specific problems you are encountering?

Looking an the small screenshot of the timeline you posted, I can already see potential for improvements.

I cannot elaborate why these choices were made, but the timeline at the bottom of the screen is a feature timeline.

The browser on the other hand shows objects that were created by the features in the timeline.

There are strategies that can help in reducing timeline re-calculations, e.g. working with linked components or assemblies.  Whether those work, depends on the complexity and structure of your design.

[TrippyLighting]

@Flowh64 I went through some of your other posts and I believe that I can speak to some of your concerns, some of which I share.

First I need to clarify that in the US the term "Industrial Design" does not refer to the design of industrial machinery. It is more associated with consumer product design, technical surfacing   etc.

In terms of CAD that results in very different workflows and tasks that need to be accomplished. At this time in my opinion, Fusion 360 is stronger in the area of Industrial Design and a skilled hand can create quite wonderful designs in Fusion 360.

Designing Industrial Machinery on the other hand would require a very, very close look at the specific area of industrial machinery, the specific business and its requirements and what the actual deliverable is.

As explained above, the timeline at the bottom of the screen goes hand in hand with the browser on the left side.

As a design progresses and features are recorded in the timeline, the browser populates with the objects that were created by the features in the timeline.

Where the objects are created depends mostly on two things.

1. Most objects will be created in the activated component.

2. Selection before feature creation. If you select the edge of a body, and create a fillet, the fillet feature will be tagged with the component that body resides in.

Activating a component filters the timeline for all of the  features that have been tagged for that component.

Any feature in the timeline can be edited at any time, regardless of what component is activated.

Editing a feature rolls the timeline back to the point in the timeline when that feature was first created.

Features such as fillets, lofts, extrudes, etc. can be selected in the viewport and right-clicking will pop up a menu with an "edit feature" option. That often limits searching for stuff in an ever expanding timeline.

In other Software, e.g. SolidWorks or Inventor, the feature tree is not an overall timeline of an entire assembly, but it is a timeline for one part (component in Fusion 360 ) only. 

However Fusion 360 allows to create a complete assembly design with all components in one file. Using the same feature tree paradigm as SW or Inventor would not have worked.

However, many users prefer to NOT design all components and the assembly in a single file, but use linked components and linked (sub)assemblies. From a performance standpoint that can make quite a difference as  recalculations of a timeline are limited to the actively open design and does not include linked components or assemblies.

One technique to battle timeline recalculations and to create "lighter" assemblies is to use a design without a timeline purely to assemble components and sub assemblies. No geometry is created in such a file. 

This also helps with another aspect of Fusion 360. 

Reordering co0mponets in the Browser in many situations is only possible with the timeline marker rolled to the end of the timeline and even then results in a slew of cut/paste features pollution the timeline. It can also result in quite frustrating warning messages "the timeline cannot be rolled back before the active component"

I use a number of CAD software packagers and one of them offers a freeze bar that allows to freeze the earlier part of the timeline. I find that very helpful!

To understand some of the UI and workflow choices it helps to understand a bit of Fusion 360 history. Initially Fusion 360 was very heavily geared to a top down workflow where all components are created as an assembly within a single file. Top-Down design, Concept design and designs with less than 1000 components is where Fusion 360 really comes to life and is a joy to work with.

Design of industrial machinery is mostly a bottom up workflow. I spent most of my 30 year career as a mechatronics engineer in the manufacturing automation industry. It is entirely an engineer-to-order business. Even the smallest machines we build at my current employer have 4000+ components.

When it comes to that amount of components you'll likely have to use numerous techniques to make sure that Fusion 360 does not slow down considerably. For use in my industry in production use that makes it very hard to recommend Fusion 360.

Usually BOMs (Bill of Materials, Parts list) are part of the deliverable. Unless you still deliver BOM in paper/PDF  form or as an obviously non-formatted .csv file, Fusion 360's built-in functionality is indeed so poor that you'll have to use an external solution such as the Bommer plugin , or OpenBOM

I use Fusion 360 in that industry for sales concept development and it's proven to be an absolute killer tool for that purpose!

[Flowh64]

Hi,
Thank you for your constructive answers, it's appreciated.
Where to start ? I realize the limits of google translate 😕 but we will get there. So sorry for the not quite appropriate terms.
For information and to understand my request, I am an industrial designer, I worked mainly for companies manufacturing special machines in different design offices. I worked for groups like Prodways or Volvo, to give you an idea of ​​the products I work on.
Before that, I have 10 years of experience in precision machining, mainly in the nautical and aeronautical industries, for Airbus and Safran.
Today I'm self-employed as a freelance designer, I make machinery on a human scale for my clients. Even if it's not, let's say a washing machine to give you an idea. I also work in other design offices as a service provider and at the moment I am working on Autocad.
My designs are based on the feasibility of machines, the rules of mechanics (isostatism, chains of dimensions, adjustments, calculation of resistance of materials, fundamental principle of statics (of which I find the Fusion simulation module very good)... ). I could very well go back to the drawing board, it won't bother me 😉
I am therefore not a Maker.

I make it a point of honor that my designs are as clear as possible. I avoid adding sketches, functions to modify.. but I directly modify the sketch or the function which does not go to its origin. My designs are therefore lighter, clearer and above all "MODIFIABLE", I insist on "the modifiable" because it is the main concern that I see with this type of history.

I have Catia V5 training but my preference is clearly Solidworks. I know PTC creo quite well and adapting to the software is no problem for me.
This is roughly how I work.

I see that you are going on several topics concerning Fusion, it's interesting, I want to discuss them but it may be long. If you don't mind, I'd like us to stick to the history, I'll come back to the other points that bother me, in other subjects.
By analogy, I see a history identical to that which can be found in the form of a written list in most software, with the difference that under Fusion you can modify it instead of simply being able to go back. It is therefore a true hybrid history.
When I design, I search, I create a lot of sketches, features, I move... which considerably weighs down the history.
For example, what is the point of recording the displacement of a part or an assembly or even a grounding? In the same idea, why not record all mouse movements? come on, let's not be silly, at least the clicks 🙂
I find it very messy and does not allow for a clean design. It is essential to have the possibility of directly modifying a sketch or a function already created, without it being linked only historically but above all functionally.

I don't draw the Top Down method, I already have it in my head. I draw the parts directly and then assemble them. This does not change this type of history.
Currently, I create an external component so that I can modify it quietly in another folder, for each part or directly in the assembly. I create a new file for the assembly, so I don't have in this file a history where displacements and assemblies are. This is typical of a Solidworks.
Despite this, my history can be long.

For the moment I see only drawbacks, it's badly put together, it's all-purpose, it's heavy and not clean (and yet I make it a point of honor that it is).

I think the developers made this choice for two reasons:
- Fusion wants to be the fusion of several design methods (mesh, parametric ...) and that only this type of history can be used.
- Either the developers have not taken care to approach the designers and know their working method, based on functionality, mechanical rules and machine feasibility. Especially since other points remind me of this.

Unfortunately, they remain very silent in the face of my questions.

[TrippyLighting]

Can you elaborate on the purpose of your questions ?

As I've explained already, I use a range of 3D modeling software including other CAD packages to do my work. 3D modeling and CAD and computer graphics in general is something I have explored for over 3 decades.

I've been on this Forum since late 2014 and have had plenty of interaction with Fusion 360 developers. That includes a Senior Software Architect and now Director of Software Development. I can explain why the history and browser function the way you do.

I can elaborate on some pro's and some con's and we can have a conversation about those and hopefully learn from it.

However, what I have absolutely no interest in is a conversation where a seemingly experienced user can only see his side of the coin and then tries to "educate" the developers on their wrong choices.

I've worked with SolidWorks since 1998. The history and browser in Fusion 360 are different from SW in a few aspect that relate mostly to the fact that in Fusion 360 you can design a compete assembly in one file, but overall they really are not that different.

Again, if you can share a few images and a design (export as .f3d and attach to post), maybe there are ways we can address some of the issues that you've come across.

After all, that is all we can do. 

[jeff_strater]

"Unfortunately, they remain very silent in the face of my questions."

I can distill your question down to this:  "why does Fusion support a history for assemblies?".  There are a couple of reasons for that, which I will get into below.  However, it is first important to point out:  If you don't like this history, don't use it.  You can use Fusion very similarly to how you are used to using Solidworks.  Make each "part" (Fusion does not have hard distinctions between parts and assemblies - everything is a Component - a Component can be like a part or like an assembly, it is very flexible that way) a separate design, exactly as you would do in Solidworks.  Then, you can create an "assembly" design as a Direct Model (no history), and insert each of your "parts" into this assembly.  You can then relate your parts to each other using Joints (this is one difference between Fusion and Solidworks - Joints vs Mates, but I think that is not the point of your question).

Now, to answer your original question.  One of the main reasons why traditional "assembly" operations such as creating components, creating instances of components, moving components, creating joints, etc are history based goes back to the point above:  Creating a separate design for each component is clumsy.  You have to do a lot of data management, inserting, etc.  Also, cross-component relationship are difficult in a fully external component world.  So, one thing we wanted to make sure to put in Fusion was the ability to create components without having to create a separate external design for each.  We call these "local" components.  We think it is very powerful and easy to use to have this ability to have all your components contained in a single design.  But, that does mean, then, that the creation and evolution of those components (in a parametric design) themselves have to be history-based.  So, component come and go as history progresses.  There is really no other way to approach it.

Second, this assembly history has one other advantage:  You can do "position-based modeling" using that history.  The sample that comes with Fusion, the Utility Knife illustrates this.  The geometry of the slot in the side of this knife is driven by the position of the slider handle in two positions - open and closed.  This does not require you to figure out the length of the slot by trial and error - it can be determined by the extents of the joint that is driving the blade mechanism directly.  We also think that this is an advantage over traditional CAD design.  But, this, also, requires assembly history - to be able to capture the geometry of the design in open and closed states, and to base sketch or other features on those components' positions.

Hopefully that can help clear up some of the "why?" in your questions.

[Flowh64]

I said in my previous message that I adapt to any software or situation, that I have no problem questioning myself, even if you think otherwise. My experience leads me to draw in this way. I am certainly insistent but not stubborn. I've been trying to get my questions answered for about more than a year and unfortunately the developers are turning a deaf ear (I assume they have other more important matters to discuss, and that's normal.) and on the other side I get insulted by the makers who can't understand my point of view as a designer. In the end, I am left alone with choices under Fusion that cannot be suitable for a functional design. If you are more of a graphic designer, I understand that Fusion suits you and that my question does not speak to you. I have to make software choices, SW is €10,000! Inventor is 3000 is better but still too much for me. Let's get back to the subject, can you tell me what are the advantages you see in this history, rather than that of Inventor, SW or Catia?

[Flowh64]

Thank you for your reply.

My question is not the one you are quoting. Surely google translation is causing concern.
My question is why not have kept a SW or Inventor type history? which are more efficient, clearer, less loaded and therefore easily modifiable.
As I said before, I have no problem adapting and changing my habits. I am not looking to work as under SW. But if I want to screw in a screw, I take a screwdriver and not a hammer, it doesn't matter what brand I would adapt 😉 I hope the analogy will be understood. This type of history is unsuitable until proven otherwise, whereas high-performance histories exist. I was able to exchange with other designers around me, who have the same question.
I saw that Fusion did not differentiate between assembly and part, but it is not penalizing and therefore does not bother me.

Concerning the design, under SW I can start from an assembly and make each of the interior parts, exactly the same way as under Fusion, called Top Down, except that I have the ability to draw them directly, c That's why I don't go through it and drawing everything in the same assembly is visually cumbersome, if not impossible in most cases.
I understand you are advising me the other way around and drawing everything in the same file, but then imagine the size of the Oo history.
But I don't see the connection with this history. Isn't it possible to avoid mixing up the history and functions like in other software? This does not challenge the Top Down design and will give real clarity and lightness to the files.
That's what I find harmful.

Delete the displacements and alignments (everything that pollutes), put the sketches and functions back in the tree on the left, leave the joints, in this history at the bottom as it is now. And, that changes everything. It's clear, efficient and during modifications, there's no need to recalculate the entire history!

Moreover, concerning the assemblies or the fact of drawing in the same assembly, introduces other questions, such as the projections (P key) which do not follow in real time the modifications made, it is a pity for Top Down , it loses all its interest. Or joints with offsets, mechanically (in reality) it's called magic, it doesn't reveal the isostatic problems you may encounter. I prefer to address these points in other topics that I will introduce and focus on the historical.

The translation of the second point does not work correctly, it speaks to me of a knife 😕 sorry.

I read and reread your answer, I still do not see any advantages in this type of history, what am I missing? 😞
It's extremely frustrating to have a product that meets 99% of the need, and to see all this spoiled by 1%. Anyway, that's how I see it.
I have another question, don't see any judgment on my part, do you work with draftsmen / industrial designers from mechanical design offices?

Thank you in advance and thank you especially for taking the time to answer me.

[TrippyLighting]

Well, @jeff_strater II'll leave you two to it then.

I was, yet again,  spot on with my initial assessment of the purpose of this users question and have lost interest discussing these topics with @Flowh64 

Enjoy 😉

[Flowh64]

It's a shame and I'm sorry, you have to succeed in convincing me with real technical arguments specific to my job as a draftsman/designer of which Fusion refers in advertising, I only ask that.
I hear what you are telling me but that does not answer my question related to my job. So I can't tell you that your answers suit me, I'm not here to please you 😉
For example, I have Catia V5 training, I worked on it during my first years, then I discovered SW directly in the design office. It was my former colleagues who made me discover it ... and yes the details are there, it's very well done, the devs have understood everything. It's powerful because it's fast, and above all the design is so clear, it's extremely easy to modify later. After information, we learned that he worked closely with the designers / mechanical designers and it is completely felt. I am not asking for Fusion to become SW, the proof if I was stubborn, I will stay under Catia and will only claim it since it is my first CAD software. Do not hide the face, SW is clearly in front for the mechanical design. But it would not take much for the trend to reverse, and it is precisely these points, including the history, which in my eyes are lacking, I only ask that.
I start from the principle that the devs at autocad are far from being bad and that their choices result from a long reflection. Therefore, I believe that it is up to me to question myself (even if you think otherwise) and to understand what their choice brings to my work.
But on the other hand, if it doesn't bring anything, seeing penalizes industrial design or if the devs think that my questions are useless, and that nothing will change on this side, then so be it, but at least what would I be for? stick to it.

You have to understand that I have an important choice to make, and if the balance tilts for Fusion, I should get used to the idea or at least circumvent what greatly upsets me in the choices that are made, see how to finance another software.

Glad to see you again anyway.

[TrippyLighting]

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@Flowh64 wrote:

It's a shame and I'm sorry, you have to succeed in convincing me with real technical arguments specific to my job as a draftsman/designer of which Fusion refers in advertising, I only ask that.

---

No, it is not my intention to convince you of anything else except, perhaps that I am trying to help you to determine whether Fusion 360 might be a suitable tool. I have no intention to "sell" Fusion 360 to you.

Just as every other tool it has its strong points and areas where it is not so strong.

I still don't know what exactly your job involves.  

If you want to continue the conversation with me you'll have to share some designs, images, screenshots, screencasts STEP files, or even .Fusion 360 designs in .f3d or .f3z format.

We can use that as the basis to discuss UI choices, and the consequences of these choices.

Again, it is then up to you to decide if these consequences affect your work positively, or negatively.

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[Flowh64]

Convincing me or helping me see if Fusion is right for my job is the same
thing.
We will try to do like that, knowing that it is not easy to share designs
or for the most part I have confidentiality clauses signed with my clients
or sometimes simply orally.
I am thinking of internal conceptions, specific to my company. I will see
how I can highlight the problems encountered.
At the same time, you must know the basics of mechanics on your side,
namely, isostatism, side chains, feasibility... This is essential, because
the designs are oriented around these points and without that it It is not
possible to know why we draw in this way and why, among other things, it is
necessary to have a clean history.

My activity in the end can be of importance, because the problem among
other things of the history I encounter it for everything. The idea is to
be able to modify quickly and simply, in order to keep a clear design.

I'll see what I share. Would you rather it be on this thread?

[Flowh64]

Here is a video that shows my job. Industrial designer and what we see is a special machine. The video is shot under Inventor we see the tree structure (history). Why keep this type of history under Inventor when the video clearly shows the type of work carried out, under that of industrial designer. And on the other side we have Fusion which highlights the profession of industrial designer with a different history, which for me is not suitable. Not clear, record everything .. anyway you know now. If this history is so great, you absolutely have to put it under Inventor! 🙂

https://videos.autodesk.com/zencoder/content/dam/autodesk/www/collections/fy22/product-design-manufa...

[TrippyLighting]

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@Flowh64 wrote:
Convincing me or helping me see if Fusion is right for my job is the same
thing.

---

That is easy to assume but is incorrect. There is a very distinct difference between the two. 

I will not explain this as it should become clear  throughout my post.

You have already not quite understood what I wrote several times. So read and listen carefully!

If you would apply for work in the US, you would not apply for a job as an industrial designer.

I've explained that in my first post and this is also the reason I asked you to at least provide a screenshot of graphic of work similar to yours. You design and engineer industrial machinery, but that is NOT the same as an industrial designer.

If you were looking for work here in the US, or in Germany for that matter you might apply for work as a machine designer and/or mechanical engineer.

That happens to be my area of expertise!

I am a German mechatronics engineer with more than 30 years of experience and I've spend more than 20 years of my career in the area of manufacturing automation. Nowadays I develop the sales concepts for automation equipment.

And for that - concept development - Fusion 360 has proven to be an absolute fabulous tool!

In general I find Fusion 360 is an very good concept development tool, not just for the automation concepts, but also for product/industrial design. Some of the collaboration features, the built-in render engine and the ability to directly share a design through a web-link make it very good as a communication tool.

However, when it comes to designing for production of such machinery , another set of features  becomes more important. I don't know how complex the machines are that you design, but the 2 smallest  projects that were recently on our shop floor already have over 4000 components. That's only the mechanical content and does not include any electrical/controls content.

A midsized project with has 15,000+ components and the larger projects can exceed $30000.

Fusion 360's  ability to manage the complexity that is associated even with the small projects is not at a point where I could recommend it for use in our mechanical design/engineering department.

What is the typical component count in one of your machines ?