Having trouble with Fusion in general

[Anonymous]

So I'm having a bit of a workflow crisis with Fusion in general.

If I go top-down and just blast out stuff without a care in the world, it works out okay, but parametric relationships are terrible and none of the parts are drawn 'as manufactured.' This works out OK.

If I go 'bottom-up' and draw really concise 2d sketches I get really slow sketches and Fusion does a terrible job of handling constraints. I can't get a well functioning 2d sketch like is required of you in a program like SolidWorks. Then when I go back to make changes the whole thing explodes.

It seems like I can go willy nilly making random stuff and it works, but it's nothing manufacturable. Or I can go step by step and make something manufacturable but it's impossible to make changes.

I don't know what I'm doing wrong and it's extremely frustrating.

I'm at month 4 with Fusion and still feel like I'm making fun shapes and nothing that's real.

[jeff_strater]

Can you share a model where you are having problems?  It will help us a lot in figuring out what is wrong, and whether there is any way that you can avoid these problems.

Thanks,

Jeff Strater (Fusion development)

[Anonymous]

Jeff, it's like, every model I make. It's a workflow issue, not one model. I can't wrap my head around how you guys intend people to make manufacturable items. 😕

For starters, I have no problem making sketches that constrain well in SolidEdge and SolidWorks. I can't get a sketch to constrain well in Fusion.

And because of the way history works making changes to old geometry after a joint causes the part to move, so you can't do anything in relation to other parts.

So this lends itself to drawing in place but then you're rotating sketches around to try to find where things go, which gets back to constraint issues and sketch editability.

It's one giant catch 22 for me. Am I the only one?

[Anonymous]

Hi, just a matter of interests, what kinds of products are you designing with Fusion360? As a user myself for about two years, I really would like to know the limitations you had found in Fusion360. Thanks!

[Anonymous]

I'm having a really hard time exploring designs and maintaining manufacturability. The latest example is an electric bicycle frame. Add holes to one component, add features to another, lots of back and forth in design. I've never met a software package that was so difficult to make changes to adapt to new geometry from other parts without adding HUGE complexity in the timeline, which is the only way to edit features.

Why not just have sketches act only upon bodies within a component?

Then have top level sketches effect all parts

Then make projections link in present

And do away with this idea of "history"

But this isn't about how to change fusion, it's about trying to wrap my head around this workflow. I want something in-between History and Direct Modeling

Lets say you make a part, say, a frame.

Then you make your swingarm.

Then you add your shock.

Your frame doesn't have the right geometry to fit your shock because this is design and you cant see the future.

Go back to change your frame sketch, your shock and swingarm dont exist.

Make a new sketch on your frame to replace the old sketch and you've introduced complexity that obliterates the value of parametric design.

How do you reconcile this?

[Anonymous]

Hi, if the timeline had been giving you a little problem why not try to use the Direct Modeling Mode. There are some designs that I myself had to stop recording due to what you had been facing. 

This latest updates I had already found a few things that is a little complicated to place into this forum and I am testing that too. Yes I had seen a big problem yesterday night using a test file. But I could not duplicate the problem after that but that problem was real. In Direct Modeling Mode you can move edges, faces directly that you might not be able to do in Parametric Mode. Since you had been using this program for a while maybe you should test that out. Let us know what you think if you had a chance to test the Direct Modeling Mode. Thanks!

[Anonymous]

I figured out what the issue is.

Fusion maintains history for the document.

I would prefer it to maintain history within the COMPONENT only, and then have the top level component be a collection of COMPONENTS essentially in direct modelling mode, not a timeline for every part made. I feel this would solve a lot of issues.

Feels good for that to make sense.

Right now you can have it one of two ways:

DM Document & DM Components

History Document & History Components

But you cannot have DM Document and History Components

[Anonymous]

Also if DM had PMI style driving dimensions (like solid edge) it would be very powerful. I suspect Fusion core can't handle this though. That's where SolidEdge's power comes from. 3d driving PMI, live rules, and exquisite 3d constraints. A dream come true for 3d machine design. Everyone says Fusion is easy to work with, and for some things it is, but whenever I try to do manufacturable work it's like pulling teeth.

[Anonymous]

Thanks I think you really know the differences between the programs. Some might work better for specific tasks. Fusion seems to try to balance the philosophy between designers and engineers.

[Anonymous]

Right so the question is what's the point if you can't manufacture what you make in Fusion? Again I'm not trying to argue I'm trying to figure out how people are doing complex iterative design in Fusion. Whenever I do even simple iterative design I either get sketches that behave poorly, or I get timeline that is so long and complex it's nearly impossible to go back and make changes. Please help me. I feel like this would be greatly solved with a DM document and History components.

In Fusion you cannot form a design loop. Ie, component A influences component B which influences component C which influences component A. It seems to be impossible without destroying the hope of a parameter driven model or sketch.

Surely someone else has struggled with this. How did you reconcile this?

[Anonymous]

Hi,  I myself is a Professional Chemist and a Commercial Designer. I do not design mechanical stuffs (In fact I coud, since I did design Chemical Plants which are more complicated than a Single Automobile.) I like Aritstic stuffs and I had been in Plastic Injection Business for many years. I found this Fusion program a little more than 2 years ago. I had been designing products that can be made with Fusion. I actually improved my skills using new tools that came out from each updates. I had designed Jewelry, Pen Holders, furniture, etc.. Using Fusion I had been able to make Molds for my plastic factory successfully. Well I am not the Mold Maker, they do the Mold Layout but by using different components that can be exploded out of a main bodies, that made their job easier. I am not doing promotion of Fusion here but let me show you a product that had been made using Fusion, the real thing. This had been photographed by me.  This photo is in my catalog. So maybe you should give Fusion a little chance and try to work with it. I am not pushing sales of Fusion, nor my own products. Just users to users. This is a real product:

[Anonymous]

I have put approximately 200 hours into Fusion so far, should I still be so frustrated as to design a bicycle frame? Fusion team dumps out amazing models regularly and I have no idea how they are doing it without pulling their hair out. I can draw darn near anything in Fusion if I already have the geometry... but try to start from scratch and design mechanical items in Fusion.. hoo boy...

Strangely enough, all of their models are provided as DM models so I can't help but wonder if they are designing their stuff in another program, importing and then jointing the assembly. Their mountain bike, for example. Was that done in DM mode, in history? Did they do the entire process in Fusion? Did they have geometry from a program like BikeCAD before beginning?

[kinsleymark]

I can really relate to what you're saying. In theory, I love the idea behind Fusion360. I'm able to make some very fun "shapes" and exploratory forms. However, when it comes time to get down to business and create manufacturable designs, I get stuck. Stupid bugs will pop up (which is understandable for a WIP program). However, what's really frustrating is running into things that would normally be very simple or straightforward to do - but don't work as expected (so I need to do some strange work-around). There are many designs that I've had to restart from scratch because I was not able to go back and adjust things without the whole thing coming apart.

After 10+ years in CAD programs like SolidWorks, I can't tell if these Fusion360 issues are just personal workflow differences and that it truly is a revolutionary new approach I need to get used to? Or does Fusion360 really have a real-world workflow issue?

The team seems really dedicated to creating a great product and taking in feedback. So I'm definitely willing to put in the time and effort to learn a new way of designing in CAD. And competition from Onshape will help (which has a workflow more natural to me because of my SolidWorks background). I'm not completely sold yet, but overall, I'm excited to see where things are going!

[Phil.E]

Are there any specific examples of "strange workarounds" you can provide? It could be a forum post or a screenshot and some steps. Post a model, or invite one of us to your project. Let's have a conversation about the things you find are not working as expected.

[Anonymous]

Do a design loop in history mode, it's currently impossible without creating huge amounts of complexity.

Do a traditional assembly workflow and try to project geometry to a base sketch. Impossible in history mode and useless in DM.

[kb9ydn]

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@Anonymous wrote:

I figured out what the issue is.

Fusion maintains history for the document.

I would prefer it to maintain history within the COMPONENT only, and then have the top level component be a collection of COMPONENTS essentially in direct modelling mode, not a timeline for every part made. I feel this would solve a lot of issues.

Feels good for that to make sense.

Right now you can have it one of two ways:

DM Document & DM Components

History Document & History Components

But you cannot have DM Document and History Components

---

I think you're onto something here Luke.  This is something that has bothered me about Fusion from the beginning; e.g. the lack of clear distinction between components and assemblies.  Traditional parametric CAD like Solidworks (and I assume SolidEdge) maintain a clear separation between these things because they are different.  Things that make sense in the context of a component (feature history for example) don't necessarily make sense in the context of an assembly.  And some things are the other way around.  Joints for example don't make sense in a component because by definition a component is considered a single unit (rigid group), even if it has multiple bodies.

So (to me at least) trying to blur the line between component and assembly just makes things more confusing with no advantage that I can see (yet?).

As far as direct modelling vs history based, I can definitely see advantages to allowing both of them for shape creation.  Fusion seems to handle this reasonably well.  But when it comes to defining the relationships between shapes, it seems not so great.

C|

[kb9ydn]

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@Anonymous wrote:

Do a design loop in history mode, it's currently impossible without creating huge amounts of complexity.

Do a traditional assembly workflow and try to project geometry to a base sketch. Impossible in history mode and useless in DM.

---

This "design loop" you talk about; if I'm understanding what you mean, my gut tells me this is a really bad idea, reagardless of what CAD software you're using.  To me it sounds like the programming equivalent of an endless loop that you can't break out of.

In Solidworks for example, one of the best practices when mating parts together is to try and keep mate chains as short as possible.  So instead of doing something like A->B, B->C, C->D, D->E; it's better to do A->E, B->E, C->E, and D->E.  Of course it's usually not possible to mate everything back to a single part, but it makes the mate solver's job much easier if it doesn't have to recalculate a long chain of mates every time a single change is made.

The same sort of thing also applies when using existing geometry to drive other geometry.  It's very useful in some situations (especially in the early design stage), but after a design has stabilized to the point where you intend to manufacture it, I generally find it best to break most or all of the geometry links and hard code ALL the dimensions for every component.  Yes it is more work, but it saves a TON of headaches when you have to change that design later.  Nothing sucks more than having to change a single dimension, only to have the entire model explode because there were 29 other things that were driven by that feature.  It's great to have the option to do it, but you make a deal with the devil when you do.

C|

[Phil.E]

Great advice. A related workflow is to base sketch references on origin geometry, rather than part geometry, wherever possible.

[Anonymous]

Yes, that is excellent advice! As said before my issue isn't with drawing, it's in using Fusion to explore mechanical designs. As you say, there is a best practice that sometimes cannot be followed until the design is essentially done. My issue is in the interim, I find it to be like trudging through muck. Thanks for the excellent reply.

When I say design loop I don't really mean something totally recursive.

Lets say you draw your first component very simple, then you import your second component and mate it to the face of the first. If you want to project geometry from your second component to the first components sketch, you cannot. You must create a new sketch and a new extrude feature. This becomes painfully obvious when you're working with lots of flats, which is common for machine design such as a CNC router Z-axis. As far as I can tell, in Fusion you MUST draw all parts in place or you're screwed.

Surely I could have started with the imported component and built the first off of that, but that's building backwards, not forwards... ie I'm used to building a frame and adding components, not starting with a router spindle and building backwards to the frame.

[Phil.E]

I like this discussion. Finally we are getting down to specifics. Thanks. I'll take some of your thoughts one at a time.

"Lets say you draw your first component very simple, then you import your second component and mate it to the face of the first. If you want to project geometry from your second component to the first components sketch, you cannot. "

This is true. It's because the sketch comes before the inserted component in the history stream.

"You must create a new sketch and a new extrude feature. "

This is what most people do. Can you explain more fully why this is a problem? In my experience, multiple sketches in a design is a good thing. It helps break the geometry into distinct groups that perform design functions. Also makes for very easy to edit sketches. This is the absolute core of how to teach parametric modeling to people. My opinion is based on thousands of classroom hours teaching Inventor (and Fusion 360) and tens of thousands of hours designing mechanical parts and assemblies using Inventor and Fusion 360.

"Surely I could have started with the imported component and built the first off of that, but that's building backwards, not forwards... ie I'm used to building a frame and adding components, not starting with a router spindle and building backwards to the frame."

Depends on what you are doing, but generally the frame for anything I make is only a vague consideration (such as a layout sketch for proportion, or a surface body "envelope" to work in) until I design the actual working parts and solve the actual design problem. The "frame" is never the driver of the design problem. Do you design spindles? Even if you did, wouldn't you care more about the job the spindle does, and where it does the job, before you design the machine that holds it? In interested in your design philosophy in this regard.

Some examples below.

For the speaker box, the design problem is a configurable volume of air. I need to make the box first, thus solving the design problem, before I add any parts that create references.

The amp design is wrapped around the circuit board. So the circuit board comes first. If the circuit board is changed by the EE, then my model will update around it.