Assemblies in Fusion Ultimate

[sohnrog]

Hello Forum,
I am trying REALLY hard to adapt to Fusion Ultimate after using Inventor for over 5 years (Inventor 2008, 11, Inventor LT).  I don't understand why two programs made by the same company are so different when it comes to building assemblies.  

In Inventor, I used to build separate part files and then build an assembly from the various parts.  I watched the video tutorial with the tripod and assemblies (well, most of the video).  However, the narrator begins with a tripod assembly that has all of its parts already built as components, so this doesn't help me much.  

https://www.youtube.com/watch?v=V6Nm_1uTRqk&feature=youtu.be.  

Is there a way to build assemblies in Fusion Ultimate from separate part files that I created as "new designs"?  Or do I have to start over and build the parts in the same design file?  When building complex 3D parts that interact with other parts, do most Fusion users build them "as built" in the mated position or in a remote part of the UCS and then drag it or assemble it later?  It seems way harder to build a tripod with legs "as built" in the angulate position.  This seems like it would require positioning work axes and planes that are offset by various angles.  It seems much simpler to build the parts on the XY plane and then "place" and "assemble" them with constrained angles later.  

I bought fusion because of the subscription option (cheaper) and now I feel like I have to learn to use it all over again.  Was this a totally different product that Autodesk bought from someone else?  It's nothing like Inventor.  I'm willing to learn.  Please let me know if I'm missing something that would make it more simple.  

[jeff_strater · Accepted solution]

Hi, welcome to Fusion.

Yes, there are a few differences in Fusion, as compared to other CAD products.  We believe that these are generally good changes, and hope that you will come to think so as well.

Regarding assemblies, you can work both ways:  top/down or bottom/up (or a mix of both)

We wanted Fusion to be really good at top/down design, so we implemented "local components".  Users who are designing from scratch and iterating often are sometimes frustrated at having to create a bunch of separate part and assembly designs before they know for sure how their design will be built.  This can be restricting.  So, Fusion did away with the notion of "assembly vs. part".  A component can be either "part-like" (meaning it has geometry but no child components), or "assembly-like" (meaning it has child components, but no geometry of its own).  Or, it can be a hybrid (which is a very interesting concept).  Then, we allowed users to create components completely in a single design.  For top/down design, we think that this is really powerful.  You can create a single sketch, and generate multiple components from that sketch, all in the same design.  This works well when starting from a completely blank sheet of paper.

You can, however, also work bottom/up.  You can create separate designs, and combine them, using the "Insert" capability from the data panel:

However, in the current Fusion version, this Insert is not associative to the original design - Insert copies the contents to the active document (including all features).  We realize that this is a limitation for a true bottom/up workflow.  We are currently hard at work implementing true associative design references (we call this "distributed design"), to be released as soon as we can.  Until then, experiment with the local components and top/down design.

You can either model "in-place" or not.  Personally, I have come to appreciate the in-place paradigm.  I can see how components will fit together as I build them.  The other advantage is the "as-built joint".  This is a command that allows you to create an assembly joint relationship from components that are already in place.  It makes creating the joint much more efficient, IMO.  Just pick the components, and pick some geometry to orient the joint, and you're all set.  If you don't want to work that way, it's fine.  You can create components anywhere and put them together with the regular Joint command.

Thanks for posting your questions, please continue to do so.

Jeff Strater (Fusion development)

[fredsi]

sohnrog,

I don't think you're missing anything. IMO there are two elements to your question, one technical and one 'documentation'.

The type of assembies you are accustomed to are built around the concept of external references or Xrefs (assembly referencing external parts). This technology or a form of it are due in Fusion 360 some time soon - supposedly in the next few releases. No doubt there are others here who will jump in and give a more comprehensive explanation of what is involved.

You can certainly build assemblies with Fusion as it currently exists, and with some advantages over the traditional work flow, but it is not well documented (IMHO). There have been a few threads discussing the lack of fundamental tutorials which address subtle details of building parts,assemblies in context. Most of the good information is scattered in various posts on the forum (some of Trippylighting's for example). Recently Taylor Stein posted a video on Youtube showing the creation of an Arduino enclosure; very informative re: creating parts, simple assemblies in Fusion.

I agree that there is a certain culture shock in making the transition from an Inventor or Solidworks environment to Fusion - I've been at it for 5-6months - am only now beginning to 'get it'

Keep asking questions and pushing for explanations in the areas that are not clear to you...it will be to everyones benefit.

Fred

Edit: Once again, Jeff types faster 

[O.Tan]

First of all welcome to Fusion

Second, forget most of how things work in Inventor and give Fusion a fresh open eyes on how things are done, it took me awhile but now that I understand how the software flows, most things are faster now. Thought they're some things that I hope they'll change or improve on in future updates

Regarding modelling, as Fusion doesn't have a way to associate drawings now yet, it's recommended for you to build your project in a single file, if you have external standard components, you can import it in via the data panel into your model.

So let's say that with your project, you got a few standard items, what you could do:
1. Create a new project folder
2. Draw and save each standard item individually
3. Import the standard items into your drawing and start modelling using those item as reference. The reason why I asked to create the standard item individually first is so that if you need to add more of it in different locations, you're able to do so (not that there's no workaround to it if you didn't do as I mentioned).

Okay, in F360 you can mate components with the fixed joint, problem is in my opinion is because Fusion consolidates all the joints in the model under a joints panel vs in other CAD software where mates resides under the part. What I'll recommend is to select the group of components that'll move together as rigid group (select components > right click > rigid group) and only use the joints when there's actually some kind of motion involved. The downside of Rigid Group is that you'll have to suppress it if you want to modify any component in it, but the plus side is that you'll be more aware how your change will affect your assembly, it's a plus minus kind of thing and I hoped there's a better way to do this in the future.

As in Fusion, joints will fully constraint the parts (called components in F360) and at the same time add motion to it, which will take some time to get used to. The advantage of this is it gives Fusion a very solid motion study feature and to easily visualize how your assembly will move (you'll be able to preview each joint motion in relative to the model assembly by joint basis)

Interestingly enough, this project is build wholly by Autodesk and it started of as Inventor Fusion but has since tremendously improved and now is a standalone product. If I recall correctly, Original inventor (or thr product that end up being inventor) was bought by Autodesk.

[rsilvers129]

It is good that they didn't require to make it work the same way as past programs because it is not burdened by legacy and is a clean approach to how the developers think things should be done. The low price, I assume, is part of the deal with the newness to get people to give it a try.

[sohnrog]

Thanks for the replies.  I've been trying to use the suggestions I have been given and reply after experimenting.  I am still having trouble with assemblies.  The behaviour of the program seems to be inconsistent.  Sometimes, when I select faces or surfaces to mate, I get a grayed out box.  For example, sometimes, it will not allow me to select component 1 and only allows me to select component 2.  Also, There are times when I select the type of joint and then the ok button is grayed out.  I'm not sure if it is just a connection speed issue since the computing is done in the cloud.  On the other hand, it could be that I'm not doing something right.  

Other issues that I am grappling with:

1.  Since this new type of 'all-in-one' project modeling has all of the components in one file, will I be able to extract a component from my project and use it with another project?  

2.  I usually model parts in an assembly to see where collisions might exist.  However, I'm usually only interested in building 1 or 2 parts in the assembly.  Some parts might only be sample cutting blocks for modeling purposes.  Can I do drawings of just the parts I want?  

3.  How do I export just one part from an assembly or 'project' to send for 3d printing or CNC?  

Thanks for your help.

Roger

[SonicFlow]

This has been a helpful post, but it looks like Sohnrog's final questions, that I share, were not answered. 

Also O.Tan said:

""""""So let's say that with your project, you got a few standard items, what you could do:
1. Create a new project folder
2. Draw and save each standard item individually
3. Import the standard items into your drawing and start modelling using those item as reference. The reason why I asked to create the standard item individually first is so that if you need to add more of it in different locations, you're able to do so (not that there's no workaround to it if you didn't do as I mentioned).""""""""

What is the workaround for components that only exist inside an assembly, but you want to reuse them elsewhere (and maintain the link)? 

I'm very new (from SolidWorks). Thanks.