Transitioning from Inventor to Fusion 360

[Anonymous]

I'm transisioning from Inventor to Fusion 360.

I'm confused the best approachI should be working with in regards to file/design my structure pertaining to assemblies, components and Bodies.

My typical Inventor work flow when starting a new Assembly with multiple parts designed inplace is:

• I start a Project folder with other folders in in name Designed Parts, Standard Parts, Assemblies, Sub-Assemblies, etc.
• I then either design a part by itself and insert it into the Assembly and/or start designing new parts in-place in the assembly and then finishing the etails in that part file.
• I can then use certain Parts in other designs or even Derived Parts and Parts diferences can proppagate accordingly.

My question for Fusion 360 is what is the best approach when starting a new Design/Assembly that will have multiple Components/Bodies?

• I understand it that I should be creating one Design that becomes an Assembly after I create more than one Component or Body within it.
• Should I have a Parts folder within the Project with individual Part/Body?? files that are inserted into the Assembly?
• When/why would you insert a Part into an assembly and have the "chain Link" icon showing that ther;s a link back to that file?
• I did a small test trying to figure out the above question by having a linke Part in an Assembly, I then made a change back in that file and those changes did not propogate into that linked Part in that Assembly. In Inventor, I'm accustumed to selecting the "Lightning Bolt" with propagates those types of changes through.

Can someone please give me some clarity to all this? I hope I'm explaining my challenges.

Thx!

[neljoshua · Accepted solution]

Having gone through the transition from Inventor to Fusion myself, I totally understand where you are coming from.

Regarding parts/projects and folders--make sure you think it through and get it right the first time.  Re-creating projects and moving files within them can be a pain and time consuming.  What we have done is to create one project for our whole company.  Within this project, we have various folders for purchased/sourced components as well as a number of folders for projects we are working on.  As long as all of the files you are using are within the same project, they will keep their associativity (shown by the chain link icon).  When I started using Fusion, I created a different project for each project I was working on as well as for each type of sourced part (fasteners, heat exchangers, etc).   Makes sense, right?  The issue is that associativity is not kept between projects.  This can be a real issue if you made a mistake or the sourced part is updated, as the changes would not be reflected in the instances you used the part in.

If the part that I am creating may be used in other assemblies or designs, I create it within its own file and insert it into the assembly.  If it is specific to that design, I create it within the assembly.

Fusion has a similar update feature to Inventor called "Get All Latest".  It is an exclamation mark/chain link icon that appears around the upper left corner of the window.

Clicking this should update all linked parts.  I say "should" because if you have inserted an assembly within an assembly, you may have to go back to the inserted assembly and update it before the larger assembly can be updated.  The Fusion team has plans to implement a "deep update", which would do this step for you, but this feature is not yet in place.

[Phil.E]

^2

@neljoshua

You have answered this as I would have. Well done. Great advice.

@Anonymous

My two coins: Inventor project = Fusion project. Strictly comparing the two concepts, what is missing in Fusion that Inventor has is cross project libraries for fasteners or other standard parts. So using the concept of a single Inventor project that runs everything (from what I gather is more standard approach to using Inventor) you should get similar results in Fusion. All of your designs will have access to the same user created libraries, which sounds like what you need.

Thanks,

[Anonymous]

Hi Josh!

Thanks for that response, I get it know.
I'm off to the races!
Thx again

Regards,



*Rick Steele*

231-943-0992 (*office*)

231-632-8273 (*mobile*)

www.linkedin.com/in/steelerick

*164 Carpenter Hill Road*

*Traverse City, MI 49686*

[Anonymous]

Great info!

In Fusion can a Linked Part in an Assembly be a Component? How do you make changes to the linked file as a Component? When I right click on the linked file I do not have the option to create a component out of it unless I break the link. The way I understand Fusion is that you can only "activate a Component" to make a change within the assembly.

Thx!

[Anonymous]

I don't have that "update all linked parts" option at the top of my user interface.
I get that icon only on the linked part itself within the browser. As far as I know I running the current version of Fusion 360, especially since it seems to update automatically when you boot the software. Which way is the current version supposed to be?
Thx!

[Phil.E]

Currently there is no in-place edit for linked components. You need to open it and work on it outside the assembly.

When you return to the assembly you can pick Get Latest to see the changes.

Things that are currently missing from linked design workflows:

In-place edit (described above)

Deep update (described by Josh above)

For these reasons, you should consider using linked components for the following reasons:

1. They are library components such as fasteners, or purchased items, things that have one definition and are unlikely to change.

2. Things that do not require references gathered from the assemblies they reside in.

3. Linked components do not participate in compute cycles, so if you can deal with #1 and 2 above, you can manage performance in a large model.

It's really quite different than the Inventor way of always, always, always, referencing linked components. Fusion 360 is built for top down design. You should only reference files that truly need to be used in multiple designs. Otherwise, keep it all in one design.

Thanks,

[Phil.E]

@Anonymous

Can you provide a screen shot showing your browser with Get Latest warnings and no Get All icon in the top menu?

Thanks,

[Anonymous]

My error! I didn't have my screen fully expanded!

[Anonymous]

OK, got it.

So if its better to do a Top Down approach, is there a way to make "Representations" like in Inventor so you can have many indiviual display views by part/component set up to make your workflow managable?

[Phil.E]

The short answer is no.

However you can use the Fusion 360 interface to achieve some of this.

Selection sets:

• Create selection sets of things you wish to control visibility on.
• Pick the selection set and right click to access the options, such as visibility.

Another tool is Capture Position. This is similar to pos-reps from Inventor, but not really the same thing at all. In Fusion all assemblies are flexible unless contstrained. So you can manage different positions for mechanisms by moving them and choosing to capture that position in the timeline. They are not a horizontal layer across time as the Inventor position tools are.

I'm attaching some documents from Autodesk University 2015, you might learn more from reading them than this slow back and forth. Please let me know if you have more questions, I'm glad to help.

Thanks,

[Anonymous]

I'd like to import my files from Inventor to fusion, to include the sketches.  currently I can import the bodies and fusion can see the lofts/extrude, ect. but none of the sketches associated with them.  I'd hate to have to recreate everything....again.  Any help would be appreciated 

[Phil.E]

This is the current state of Inventor to Fusion translation. The parametric table and sketches are not translated.

Thanks,

[Anonymous · Accepted solution]

Is this going to be updated?


Sent via the Samsung GALAXY S®4, an AT&T 4G LTE smartphone

[Phil.E · Accepted solution]

It's not on our roadmap.

What is it you hope to avoid or achieve? It sounds like you have an active project in Inventor that requires the use of all of your parameters in all of your parts. Is that true?

Thanks,

[Anonymous · Accepted solution]

I have a knife hade design that is semi complex.  It is close in deminsions to alot of handles but sometimes the screw holes or something need to moved.

In inventor I can change the sketch fairly easy and update everything.

I was hoping to import these file to fusion so I could easily adjust things versus reacomplish the entire process


Sent via the Samsung GALAXY S®4, an AT&T 4G LTE smartphone

[Phil.E · Accepted solution]

What you want is also doable in Fusion, based on your comment.

If all you need to do is move some holes around now and then, then you could do the following:

1. Import the knife to Fusion.

2. Delete the holes

3. Create a new parametric sketch for your holes.

4. Create new parametrically driven holes for your imported knife.

You can get what you need with very little modeling! 🙂

Thanks,