Where are the constraints / mates ?

[Dan_Margulius]

Hello

Maybe i am missing something, but it is impossible to built mates in Fusion.

How can we work in an assembly without mates???

Moving parts and Joints it's not it. 

Thanks

Dan

[TrippyLighting]

You are missing something 😉

Fusion 360 is not Solid Works or Soid Edge etc. and uses a differnt concept for joining components (not bodies!!!).
Play with the "Assemble" menu and perhaps watch the online video tutorials for some guidance.

[brucehuang]

Hi Dan,

Here's some tutorial to show you how to use joint origin, joint to assemble components in Fusion. Hope these help.

Create joint origins on components
http://help.autodesk.com/cloudhelp/ENU/Fusion-Function/files/GUID-47DB0A46-6478-44FA-BAF7-B80C4A2A50...

Position components using joints
http://help.autodesk.com/cloudhelp/ENU/Fusion-Function/files/GUID-6A781281-1D14-4C95-BAFD-8489E500D3...

Bruce

[jeff_strater · Accepted solution]

Thanks, TrippyLighting.  You are correct.  

When we started Fusion, one of the areas that we decided to try to improve over more traditional CAD software was the area of assembly modeling.  Customers new to CAD often struggle with such abstract and mathematical concepts as "flush" and "mate" for describing relationships (especially kinematic relationships) between components.  So, we decided to try to elevate the concept a bit to terms that are more familiar to mechanical designers:  Joints.  In our thinking, a "revolute joint" was more obvious than "Mate" between two linear entities that just happened to result in a circular degree of freedom.  So, we decided to go "all in" on the joints approach, and not offer traditional assembly constraints at all.  It was a bit of a risk.  To our knowledge, no CAD software had tried this joints-only approach to assembly modeling.

In our (admittedly biased) opinion, this works very well for describing kinematic relationships.  It seems pretty easy to created jointed component relationships.  Especially in a top/down workflow, with "As Built Joint", I find it really easy to create most common mechanisms.

In the interest of honesty, where this approach still requires some tuning is in trying to position components rigidly with respect to each other.  Fusion has always had Rigid joints, which definitely solves part of this workflow.  But the joint positioning choices didn't always result in exactly the correct relative positioning of components relative to each other.  So, over time we have added a few commands that help.  One is Rigid Group.  This command allows you to select a set of components and make them rigid with respect to each other in ther current positions.  The Align command allows you to position components with respect to each other, by aligning geometry, and Move allows you to do more freeform moving of components.  So, a very useful workflow is to use Align or Move to position components, then put them into a Rigid Group.

The other workflow is one that works well with top/down design.  If you create components in a top/down design manner (for example, one sketch that is used to create 3 components), and you build these components in the orientation with each other that you want, then a simple As Built Joint with a type of Rigid works very well.

We are always looking for ways to improve workflows in Fusion.  If you have ideas in this area, please let us know.

Jeff Strater (Fusion development)

[Anonymous]

Rigid is 0 DOF
Revolute is 1 DOF rotational
Slider/Cylindrical/Planar/Pinslot I believe are 2 DOF
And ball joint is 3 DOF

So you can imagine that a "joint" locks everything up and then releases degrees of freedom. I could be wrong on the exact number of degrees for each

It's counterintuitive at first, and then you realize it's actually extremely intuitive.

[kb9ydn]

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@Anonymous wrote:

It's counterintuitive at first, and then you realize it's actually extremely intuitive.

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Except that in real life objects are free to move around unless constrained by something. 

For computer modelling though I can see how defaulting to fullly constrained and then allowing movement could be simpler, since most of the parts in a typical design are likely to be stationary.

C|

[Anonymous]

I think the concept of joints stems off the idea that no mechanical object ever has more than 3 DOF, and more commonly has 1 or 2. A bolted or welded relationship is 0 DOF. And nothing will ever have 3 DOF that are strictly translational.... soo that leaves you with a few options, and each of those options are handled by the combination of joints provided by Fusion.

Lets say you do an axis constraint on a more traditional CAD program, even that is only 2 DOF. Planar constraint is 3 DOF (this also is a joint, though). In fact, most regular mates remove multiple DOF at a time. Joints just do it to match common mechanical situations.

I wish I could change my last message to say that planar was 3 DOF because I made a mistake.

[Dan_Margulius]

Hello,

Thank you for all the feeback here, it is great...BUT

if you people think that mechanical engineers will start to "mate" parts with clunky joints and "move" parts around 

then you got it wrong. Fusion should be better than SW, inventor and others and not missing key functionality just to be different.

Be the different and better and not different and worst! 

For example why do I need to go to the browser, search the part just to move it??? 

Why when i pick an edge Fusion does not know I want to do a fillet or chamfer...INV does know!

Again different and better. yes!

Thanks

Dan

[Dan_Margulius]

Another thing, if i click an edge to Fillet and give a radius I cant pick the second one and have the same radii

and the same with Extrude

Why is that? 

Dan

[Dan_Margulius]

More daily crashes :   

[Anonymous]

While I agree that it is easier for us mechanical engineers to work with low level elemental geometry to construct what we want... as we desire the ability to explicit define the world around us... joints are a completely acceptable alternative and do benefit someone who is new to cad who doesn't know what a degree of freedom is. This allows a new CAD user to not diagnose their work to create a working assembly. I'm with Fusion team on making the choice to use joints.

THAT SAID

If there were an option in prefences menu to use elemental mates instead, I'd probably use that.

[Dan_Margulius]

Fusion now is given free to Product Design Suites customers...That means that people who work with Inventor like my self will start to play 

with the software. As for now in my opinion, with all the problems i have encountered in a few days the software is not usable for production mode.

Maybe it is for Amatuers, Makers..whatever...

I like the CAM module though...it is very nice to import parts from INV and make the toolpaths in Fusion.

Thanks

Dan

[Anonymous]

I agree that Fusion should be considered a public beta. Most of the bugs I run into with Fusion is sketch related. I am constantly able to create really bizarre sketch behaviour and it often hinders my work. But as far as mates vs joints I would say that if you're willing to meet new users halfway you'll find that you are not hindered by their functionality, it just requires a brain twist for those of us who have been using CAD for a couple years at least.

[HughesTooling]

If you want to select more edges for fillets after the command is running hold down the control key and select more edges, when you release the control key the fillet is added to all selected edges. The same goes for extrusion but all the profiles need to be on the same plan.

Mark.

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@Dan_Margulius wrote:

Another thing, if i click an edge to Fillet and give a radius I cant pick the second one and have the same radii

and the same with Extrude

Why is that? 

Dan

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[prabakarm]

Dan, can you help us understand what you were trying to do with Fusion and what problems you faced?

Thanks,

Prabakar.

[Dan_Margulius]

Hello Prabakar,

I am trying to understand what workflows in Fusion will benefit our bussiness. 

I uploded some assy and tried to model some parts from INV and then troubles began...no mates, no section view in drawings (Alias problem) 

crashes all the time...click CTRL to add more than 1 fillet (WHY?) and the UI is BAD, very BAD! not user friendly at all...bottom line from a mehanical standpoint it is a tool of nice to have...

Good viewer, good CAM module not such a good modeler compared to INV.

Maybe things will be betten in a few months with more development, no rush.

Thanks

Dan 

[kgrunawalt]

To be clear, every occurrence of a component in Fusion is free to move by default. Fusion is different in that the component hierarchy does not constrain motion, except for joints, rigid groups, and motion links. Also, there is grounding of specific occurrences.

Commands like drag and move components will conveniently move children of an assembly when an assembly is moved. This grouping is temporary during the move operation. The children can still be moved independently as allowed by existing joints and rigid groups. This temporary grouping has caused some confusion because it makes it seem like the children of an assembly are rigidly attached to each other. They aren't by default.

A joint completely defines the position between two component occurrences in terms of six degrees of freedom (3 rotational, 3 translational). Some of those degrees of freedom are be removed by the joint according to type, the rest will have joint values that describe the current relative position. These values are what makes joints effective for Fusion. There is a reason we use joint instead of more "atomic" constraints, like mates and angle constraints.

Fusion is unique in that joints and positioning are part of the parametric history. This allows assembly positioning to be used to do "top down" modeling. For example, a lid on a box could be rotated so the revolute joint is at 30 degrees. This position can be captured in a "snapshot" feature. Then solid features can be added to create geometry referencing that lid position. This position can be changed parametrically and the features that use it will update accordingly. This is a very powerful "top down" approach.

Joints are more effective for the kind of deterministic positioning we need to accomplish this top-down approach than constraints. They can define positions parametrically using the joint values without adding hard constraints that would remove degrees of freedom. They also avoid having underdefined positions where no values exist to fully determine positions when the history is re-computed.

A joint-only approach does require a different approach to assembling things. There might be cases where regular constraints seems simpler, but we think these are rare once you get used to joints. The inclusion of joints and positioning in history is a huge gain and something that new users might not realize.

[Anonymous]

I'll give an example as well.

I had two components that I wanted to fit together only when they were in a certain position. I was able to joint them, move them into an interference position, then take a 'snapshot' and use the 'combine' tool to subtract the interference. This gave me a perfectly dimensioned relief that fit my existing geometry exactly and took about 20 seconds instead of 15 minutes.

[kb9ydn]

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@kgrunawalt wrote:

To be clear, every occurrence of a component in Fusion is free to move by default.

You're right.  What I meant by "defaulting to fullly constrained and then allowing movement" is that when using history you have to explicitly allow a component to move, either by doing a command that automatically creates a snapshot (like a joint), or by doing a snapshot manually.  I guess saying that components are "fully constrained" was a poor choice of words.  What I really meant was that because all movement is fully tracked, it has to be controlled more deliberately.

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@kgrunawalt wrote:

Fusion is different in that the component hierarchy does not constrain motion, except for joints, rigid groups, and motion links.

This is rather interesting, and it's something I didn't really think about until you brought it up.  By default in SolidWorks all sub-assemblies are treated as rigid groups unless you set them to be flexible.  The nice thing about this is that it allows for faster performance by compartmentalizing the part mate structure, so that mates only need to be solved at the top level.  Frequently the things I design in SW have multiple sub-assemblies with moving parts, so I usually try to layout assemblies so that they correspond to groups of parts that tend to move together.  Most times this is fine, but occasionally the way I want to organize the parts into assemblies doesn't match up with how the entire assembly and its parts moves.  This is where flexible assemblies are useful, and most of the time they work ok.  BUT, with larger assemblies and lots of moving parts, the mate solver sometimes has problems keeping up and you can end up with things moving in unexpected ways.

The other issue I run into is that because SW uses simple constraint based mates, you can end up with many hundreds of mates, which can be quite a hassle manage.

Now I haven't done enough modelling in Fusion to know how it would handle movement in larger assemblies, but I suspect the joint system along with history tracking of movement, might have an advantage in managing complex movement; partly due to not having as many items to reconcile (fewer joints vs greater atomic constraints) but also due to having more control over movement in general.

Or it might end up being really annoying, I'm not sure.  I really need to get more seat time in Fusion modelling I guess.

C|

[kb9ydn]

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@Anonymous wrote:
I'll give an example as well.

I had two components that I wanted to fit together only when they were in a certain position. I was able to joint them, move them into an interference position, then take a 'snapshot' and use the 'combine' tool to subtract the interference. This gave me a perfectly dimensioned relief that fit my existing geometry exactly and took about 20 seconds instead of 15 minutes.

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Ahh!  Now there's something you can sort of do in SW but Fusion makes it easier.  The difference with Fusion is that once you make the relief in the part, you can move it away without having the relief change.  To do this in SW you would have to break the link between the two parts before moving them apart, and once you break that link it's permanent.

C|