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.

[Anonymous]

OK Phil I see your point and I think it's a good one. Let me think on that. Now we're getting to the discussion of overall workflow and that is good.

Nice work, by the way. See, it's obvious that you can achieve great things in Fusion I'm just trying to get there.

[Phil.E]

No worries Luke, you'll get there. We'll help.

-p

[LMD001]

Hello Everyone,

Nice discussion!

My CAD track record from 1984 till now is AutoCAD - Inventor - Fusion 360, all Autodesk products. No real working experience with Solidworks, Spaceclaim or any other CAD software, we did do some tests with other packages but found that "the devil you know" is really a true saying.

Life is about learning continuously and it is very normal that software tools have evolved and new skills must be learned, but It should not be the aim to learn new software all the time, in the end it is about getting things done.

The concept of Parts - Assemblies like Inventor and I assume Solidworks, is in Fusion actually not that much different it only is presented in a more compact way. The basics of Parts and Assemblies is still there even if the names are different. The combination of Direct Modelling, Parametric Modelling and CAM however is.

In history based modelling the order in which you do things is all important. Knowing this order from the start of the design? Depends on the design and how experienced the designer is.

Now to the part where Luke and to some extent I think every Fusion 360 user could get just a wee bit frustrated is that it is not always clear that when you break a model, what exactly needs be repaired. A lot of features turn yellow, with little or no clue on what is wrong. Mostly the problems are lost references, and in a sketch these also turn yellow, for me, that is a big help.

Like all complex software tools, expect and accept a learning curve, and some are steeper than others. I am sure Fusion 360 will mature with every update and become one of the major 3D design/manufacturing tools.

Of course an A to Z workflow example/manual would be nice!

Best regards,
Ludo

[jeff_strater]

Very nicely stated, Ludo.

Regarding failures, it is a valid concern, and is also something that we are actively working on.  In our defense, I don't think that there is any parametric CAD system that does a really good job at this.  Most failures are failed references (there are other kinds, such as a failed shell due to an edit of the shell thickness).  Actually, I need to do a separate post about failed references, I think that would be useful.

But, to give an example of the kind of thing that we are working on in this area, we added this for the release we just put out:  Some extra feedback for some cases of missing references.  As a simple example, assume we start with this:

An extruded rectangle with an offset workplane from one side.

Next, the user edits the sketch, and deletes a line:

then, replaces it with an arc:

finally, exit the sketch, and recompute.  The offset plane fails:

What is new here is that we highlight the graphics (in red) of the plane that used to exist when the plane was created.  Now, this is a trivial example, with an obvious answer.  But, hopefully, you can see that, once we expand this everywhere, it can help to debug these failures.

More later, when I have more time...

Jeff Strater (Fusion development)

[LMD001]

Hi Jeff,

Thanks for the update on the failures and the additional feedback.

This will for sure be a great help in repairing models.

I tried this at home, but the red face does not show when the fail occurs, I assume that by "recompute" you mean the Compute All command, then I get the red face when clicking in the warning dialog box.

Here's a Screencast: https://screencast.autodesk.com/main/details/aa5fafea-e250-497e-bc0a-e33d5e6fac8b

Replacing the arc again with a line does not remove the failure.

Kindest regards,

Ludo

[daniel_lyall]

that's something I have come across before I just add a arc to it pull it up and join it I just use edit drawing to do it, but it stops that error happening (work around)

[fredsi]

Hi Phil,

So I'm looking at the amp design and thinking about your comment on how it would update. If that EE finds out that the gray connector located in the end (closet to the viewer) has become obsolete and changes it, what is driving the update to it's cutout? I would have thought the cutout was the result of 1) activating the end component, 2) projecting edges from the connector, 3) offsetting the edges for clearance, and 4) extrude-cut the cutout. 

Can that change be made and the end 'automatically' update? Or is it a question of reactivating the end component, deleting the original cutout/sketch and reconstructing it with project/offset/extrude-cut? If it's the latter, I can do that; but if the former I want to learn how that's done!

I come from a very humble, bottom-up background, but would love to understand the work flows of top-down design so I can leverage pre-existing geometry  And thanks for your comments and those of others in this thread....seems every post I read helps to clear up misunderstanding and refine my approach. 

Fred

[Anonymous]

I think for me the biggest thing I cannot reconcile is this idea of editing a previous feature and having the whole document (assembly) go back in time. I totally understand why this happens in History based modeling, I wont argue the CAD mechanics there, but it's extremely disorienting and frustrating. This is why I called for DM document and History components.

I think Fusion's choice to have no difference betwen assembly and component is a poor one. I have yet to see a benefit. In traditional CAD programs it's not like you can't edit your parts within an assembly.

In most other CAD systems you can edit your parts within the assembly to fit to your other parts and their geometry stays present, available for snapping or even setting up relationships.

In Fusion you get cast back to the dark ages before your other parts even existed, so you're forced to add complexity to the timeline to make even the tiniest changes (like the distance on an early extrude feature). This results in a very complex timeline that greatly reduces your ability to make changes. And god forbid you forget to activate the right component when you're mucking about trying to get things fixed because then you're really stuck downstream without a paddle.

Wouldn't it be nice to be able to snap that old extrude feature to the face of a part you brought in later? In Fusion you cannot, in darn near everything else you can. I strongly believe that the option for DM document and History components would allow this type of functionality. Just have it "auto break link" on all projected geometry between components that disappears as a result of an edit.

But who knows, maybe that's a terrible idea and you guys have it figured out beyond my current understanding. That's always a possibility. 🙂

Maybe I'm trying to turn a horse into a camel, as in, "a camel is a horse designed by comittee."

[Phil.E]

@fredsi

Sorry, didn't mean to mislead you. In the scenario you outline there would be necessarily manual updating to perform. I was speaking of a general workflow, where the EE might make changes to the PCB, and this would drive the overall design, but I was not talking about an exclusive F360 workflow. Just showing that a designer has to take into account the factors that drive the design, i.e. the design problem that needs to be solved.

Completely replacing a component requires a human being to ensure the new component is in the right spot, and then perform the necessary modeling functions. All CAD software operates this way.

If the connector model changed, and the user managed the relationship correctly, the sketch would update. Again, pretty much exactly as within the existing CAD paradigm.

[fredsi]

Phil,

No worries....not misleading at all. Many of the Fusion designs developed by you and your associates are very seductive, not just in appearance, but in their adaptability to modifications/deletions and substitutions - leaves me amazed at what I've yet to learn.  Creating assemblies of this nature, with all the advantages of top down,  is my goal, but I'm having a difficult time determining what of my prior experience I need to check at the door and whal I can still utilize.

It would be very valuable if users such as yourself could make presentations that distinguish traditional CAD approaches from 'the Fusion Method'.  Some blank sheet to finished assemblies of ten parts or so with detailed work flow would go a long way toward clearing up my lack of understanding.

Appreciate your response and continued insights.

Fred

[kb9ydn]

---

@Phil.E wrote:

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.

---

The problem with what you're describing is that it assumes there is always a one directional driving relationship between components; i.e. a root component always drives everything around it.  But this is not always the case, especially when you're trying to modify existing designs.  Lets take your amplifier design:  What happens if marketing says, we want to make next years amplifier model with a sexier looking case, so we need to change the locations of some of the board standoffs.  Now the "frame" is potentially driving the design of the guts.  Will you then need to rearrange the order of the components to make this easier?  I hope not.

In regards to adding new sketches vs. modifying existing ones, you really need to be able to do both.  If I already have a sketch for board holes to accomodate standoffs, and I need to add some new holes based on a change to the case, I'm not going to create a new sketch for those holes, I'll edit the existing sketch.

And beyond that, sometimes it's just nice to be able to edit a part in the context of the assembly around it, without requiring a specific ordering of the components in that assembly to see everything.  Even if I'm not modelling directly off of those external parts, it's helpful to be able to see where they are in space.

Is there some sort of advantage to having a history based assembly?  So far I'm only seeing that it's more restrictive.

C|

[O.Tan]

From the sounds of this dicussion, it seems what people would really want is the option to work in both history or direct in whichever phase they're in, be it during conceptual or later stages. 

For ex:

Main Assm (direct)

> Comp 1 (direct)

> Comp 2 (direct)

> Comp 3 (history)

> Comp 4 (history)

And they can swap between direct or history depending on the situation or phase they're working at. For example, when I'm just playing with ideas with no clear goal, I don't want to work in history, or some features like patterns is generally better done in history. So I might start with the model in direct and then swap to history, and if I go back to direct, I wouldn't want to lose my history tree (in this case the patterns I made in history).

There's both pros and cons for either direct or history and some tools work better in certain environment.

However there's a lot to consider on how to implement this. As a SolidEdge user, what SolidEdge does is, all changes that's done in history mode is kept in history, but what is done in direct is able to be seen in history. For example, if I start modelling a box in History, switching to Direct without converting the feature into a Direct feature will "hide" that feature, whereas if I build the box in direct and after that switch to history, I'll still be able to see the box and make the necessary changes. I can create holes on it, but if I switch back to direct, the holes will disappear. It does sounds odd about why would someone want this, but having used SE for 3-4 years by now, I find out that it's a really powerful feature to have. 

I understand that what I said might not be possible in F360 because of how it's structured or programmed but I'm just sharing how the other people are doing it. Hope it helps

[Anonymous]

This is obviously a great discussion!  My computer is processing a demo video covering some of this stuff, that should be ready tomorrow afternoon (darn bit chomper is taking its pretty time).

Jesse

[daniel_lyall]

just post something you wont to make and Jeff might do a vid for you 

[Anonymous]

Luke et al., please let me know how this video helps you regarding some of the matters discussed here.  Please note that this is just a hastily created video done late last night (), very unlike the comprehensive free guide software I'm developing.  Also in the part regarding moving an imported component 'back in time' before a sketch within the timeline, I forgot to mention it seems important that editing the spatial relationship between the two should be done by moving the coincident point after entering that relevant sketch.  If anyone needs clarification on anything please let me know!  And do enlarge the video and set its resolution as high as possible (may need to view it at youtube site).
Jesse

[Anonymous]

3:50 -- could Fusion team add better selection priority here for the two corner points? let original points take priority over projected points for example

5:30 -- I strive for as concise a timeline as possible so that I build "editability" (see "drinkability") into my projects... problem is, this can actually cause more issues than it solves. What's the benefit of having this move feature in your Timeline?

6:20 -- the idea that both bodies should 'jiggle' together instead of separate to mean that they are 'better jointed' is new to me. can someone comment on this? i've only noticed them both jiggling together. What does it mean when only one jiggles?

https://screencast.autodesk.com/main/details/af2caf41-c290-42d2-9fca-0279ccf8db19

7:05 -- how did that dimension appear out of nowhere?

10:40 -- OK back to the 1 vs 2 jiggle. It seems to me that Fusion is reporting the 2 jiggle simply because your sketch is inside the component that you're jointing to. But I cannot think of any reason why the resiliance of the joint would be any different than if you jointed to the base level sketch, since the base level sketch will always drive that projected point. I would assume that this is a case where the 2 jiggle is being shown because the "jiggle engine" isn't smart enough to realize that you're working of geometry projected from the base component sketch.

12:10 is a perfect example of why I hate leaving sketches in the base component. This is extremely counter intuitive having your sketches left behind in 3d space. Now go drag those live to adjust your geometry and see how it goes. 😛

time for class, i'll watch more when I get out.. thanks for posting this!

[HughesTooling]

I think the idea of having the Main Assembly as direct then having components as either direct or with history would work quite well.

Mark.

[Anonymous]

I understand the jiggle better and I see that you are correct. Sorry about the noise. I always forget to check/uncheck the mic button at the end. Wish I could delete audio on the Screencast website.

https://screencast.autodesk.com/main/details/271ac8db-7a46-4c6a-97e8-ff9d2b00fe32

[Phil.E]

@ kb9ydn

Agreed.

However I was trying to describe how it works. You and Luke are describing how you want it to work.

As for the nuances of what drives what, let's just say it hasn't blocked any one of my designs in Fusion. So it may be more restrictive, history assemblies, but I can work with it and wish that every one of the 10 thousand hours I spent on Inventor creating amps and speakers was with Fusion. I know I would have been more productive and creative. Inventor held me back in so many ways. No CAD system is perfect, and all systems fail. It's really up to the user to work with the tool on their own terms.

Your perspective is helping us build a better Fusion and we appreciate it.

Thanks for the feedback!

[Anonymous]

I realized I forgot to show a very important step in the video of how I moved the first two bodies into the new component I created (of which creation I also did not show, it first appears at about 8 min 8 sec in ).  I'm reproccessing the video and should be up fairly soon.