I'm near to giving up on parametric/history design again
It's hard to say what is going on without seeing the model. If you'd be willing to share it, we could take a look.
There are definitely some tricks to parametric modeling that can help, such as locking down degrees of freedom. While none of what goes on in a parametric compute is "random", some of the solving technologies that Fusion (and any parametric CAD product) use do allow unconstrained geometry to move in a variety of ways to solve the constraints. For instance, if you have two lines in a sketch, and set them parallel, all that you are guaranteeing is that those two lines are parallel. There are an infinite number of solutions that satsify that one constraint. And, with just that one constraint, you are telling Fusion nothing about the endpoints of the lines. So, either line can change length and still satisfy that one constraint. However, if you add dimensions to the lines describing their length, how far apart the lines should be from each other, what angle from the X axis one of the lines is, and lock down one endpoint of each line, then there is only a single valid solution. This makes for a lot less unexpected behavior on recompute.
Second, it is important to understand dependencies. If you create a component, then you sketch on a planar face of that component, you have created a dependency to not only that component, but the feature that generated that particular face. If, in that sketch, you dimension to an edge of that component, that is another relationship, this time to a specific edge. This is fine, and necessary, but then, when you make a change to that face or that edge of that component, the sketch and geometry in that sketch will react to it. Mostly that works fine. But, if you make a change that, say, removes the projected edge entirely from the other component, then you have a problem, because the dependency will be broken. Fusion tries to react to that as best as possible. In this case, it will keep the projected edge geometry in the sketch, at its former location, as "fixed" geometry (and give you a warning). But, it is no longer associated with the other component, so it cannot react when that component is moved or changed.
Anyway, if you would like to share the model, and maybe a screencast of the behavior you are seeing, we could offer some specific help.
Jeff Strater (Fusion development)
Jeff Strater
Engineering Director
@kjellhar: This is a nice summary. Thanks for adding to the discussion.
I think you have hit the nail on the head. The key to making parametrics work for you is the relationships. Understanding the relationships, and planning them out to some extent, can make your life a whole lot easier. The more of these you have, the more chance that an edit will break one, which leads to the "going all wrong" behavior.
In Fusion's defense, I don't think that we are significantly worse than other parametric modelers on this front. That is obviously a biased opinion (everyone thinks their own baby couldn't possibly be ugly...), but I think that comparable parametric design tools are only incrementally better or worse than Fusion. You will get failures in any parametric modeler, if you make certain edits, or if you don't think through your design as you go. That may not be a valid defense, but it does indicate that the problem is hard to fix.
One criticism that is definitely fair: I think Fusion makes it too easy to create unstable references. We talked about this a lot during the design phase of Fusion: How can we "guide" users toward creating more stable references, and away from more brittle references? We did a few things, but sadly, I don't think we moved the needle a whole lot. It is still too easy to sketch on a face with filleted edges, and to dimension to those edges in the sketch, both of which are really not good ideas.
The kinds of things that I think of as I use any parametric modeler are: Is doing this operation going to create a reference that I absolutely need? For instance, when creating a sketch, do I need to sketch on a face, or can I sketch on an origin workplane, or even a workplane offset from an origin plane? The latter are going to be way more stable than the former. The same with sketch dimensions: Can I project a stable work geometry into this sketch and dimension from that, or do I need to dimension to an edge? If I need an edge, it is better to dimension to an un-filleted edge than to a filleted edge, so delay putting fillets on until you really need them. Similarly, for a hollow design, deciding where to put the shell in the timeline can be an important difference between a design that is stable, and one that breaks easily - references to the unshelled faces are more stable than the shelled faces. Body references are more stable than face/edge/vertex references. Use Project with a Body filter, rather than projecting a bunch of edges. Split Body is more stable than Split Faces. And so on. It would be good to collect a bunch of these recommendations and put them in a blog, the help system, the tutorials, etc.
I also think about: What sorts of edits am I going to need to make to this design, and have I given myself the tools to make those easily? I don't always fully constrain my sketch, especially if I know that it is for a small feature that I am unlikely to edit. But, if I know that I am likely to edit this sketch a lot, I am much more careful to set up a scheme that is stable. An example: for a rectangle, you can dimension the length and width two ways: by dimensioning one horizontal line and one vertical line, or by creating distance dimensions between pairs of lines. Between pairs of lines is more stable - those will survive a sketch fillet, or removal of a horizontal constraint, where the first will not. I also like to set up parameter "favorites" for dimensions and values that I know will change a lot. And, before even exiting the sketch, I will "exercise" it a bit - change those parameters and make sure my sketch is well-behaved.
Also, your point about not having any tools to diagnose these relationships is a very good one. For my designs, I tend to just know what kinds of relationships I tend to build, but if I ever look at someone else's design, I am often lost. So, some diagnostic tools to help trace these relationships would be useful. Hmmm....
Anyway, this is a good discussion. I like these kinds of topics, and I almost always find some good suggestions and ideas in them.
Jeff
Jeff Strater
Engineering Director
I have to agree here with Jeff.
The fact simply is the more complex a model is with all those features the more complex the representation of that paramatric design tree will be.
So you as a user have to develop a repetative workflow to make it easier to keep an overview.
Here for example is OnShape - a web clone of SolidWorks.
Right is the part, left is the design tree with all features listed in the sequence order they were added, lower left are all the parts.
I really think the process you use is key here - obviously one also needs to know what is bad and good practice and what will work and not.
So for example if you want to build a bumper for a phone - create components first and in the first component I load a iPhone reference volume
and in the second component I only work the bumper.
The components in this case then can trim down the features in the timeline because only features applied to that component will be visible
thats a great way to keep an overview.
That said I think the timeline idea is pretty great but some other or further visual organization tools could be useful like break points similar to groups or so to enable me as a user to quickly sort features and see where they do what on what object. But the problem here is I can add one feature like a fillet and let that fillet work on edges of many objects.
That is why having a workflow disciplin is key:
first all components
then all sketches
then all hard edge surfaces
at the end do fillets at once
... as an example
At the end parametric design has its ups but also its downs and it is not key to a better experience by default.
The timeline is pretty nice because you can also move parts around but when you associate features to different bodies you need to keep in mind that you cannot
for example move a feature before an object was created and such. With experience I think foreseeing those bottlenecks will be easy.
Fact is also with Fusion you will have to do some explorative modeling before you get down to making the finale model.
My Personal preference are actally node layouts like in Grasshoppe:
The main advantage of them via Fusion or SolidWorks is:
1. You can see the flow of all parts at once nicely
2. You can reuse the same command / data like create one number field to drive many fillets at once.
The downside is with very complex nodes well it can get messy
But I feel the component approach is a great way to focus on object related features only.
And for my taste I like the timeline more then the way how SolidWorks or OnShape/Inventor appraoch the design tree.
Maybe what can be confusing in Fusion is the timeline beccause that build parts.
In Alias or SolidThinking you just draw curves when ever you want, add surfacing commands when you want and work on a per object basis.
That for me makes it easier to deal with the design and all the objects.
But then you cannot add a fillet feature and select edges from many objects like you can do in Fusion.
So it is like left pocket right pocket.
Claas Kuhnen
Faculty Industrial Design – Wayne State Universit
Chair Interior Design – Wayne State University
Owner studioKuhnen – product : interface : design
Regarding those "ghost" images that you see when a dependency fails: This was our attempt at improving the stability of compute. In most other parametric systems, when a dependency fails, any downstream feature from that point on that has dependencies to the failure will also fail.
So, when we built Fusion we distinguished two kinds of reference: geometry and topology. A topology reference is one that actually needs the item selected. For example, for Fillet, you select an edge. If that edge is missing, the Fillet cannot compute, no matter what. You will get a red failure in these cases. However, if you create a work axis from a linear edge, that work axis does not need the edge (in the sense that an edge has two adjacent faces), all it really needs is the geometry of that edge (a line). So, a work axis creates a geometry reference. Geometry references cache their geometry, so that the consuming feature can continue to compute even if the reference fails. You will get a yellow warning in these cases. These geometry caches are the "ghosts" that you see.
However, the jury is out as to whether this approach is really effective or not. This does, indeed, allow downstream features to compute in many cases. Whether that compute is useful depends on a lot of factors. Sometimes I find it very useful, other times, it causes features to compute in the middle of nowhere, which is not particularly useful, IMO. Anyway, we continue to try to make this experience better.
One topic that has come up frequently is better tools to "repair" broken references. Things like showing the failed reference, and some way to easily fix it. Sometimes this is pretty easy - for features, just editing the feature and re-selecting the profile or edge that you want. It is less easy for projected edges in a sketch, because just re-projecting an edge only fixes the sketch - downstream references to geometry built from that sketch curve will then fail, because it is a "different" sketch curve. We do need better tools for this kind of thing.
Jeff
Jeff Strater
Engineering Director
Yeah that is why I said left pocket right pocket - I am not sure if there is one ueber awesome CAD app or workflow - each process has also its downside.
In terms of freedom I can work better and quicker with less work in Alias than Fusion but then certain solid tasks are impossible in Fusion and where in Alias
I could have to undo untrim retrim work in Fusion I could re arrange features in the timeline and update their inputs just with few mouse clicks.
Claas Kuhnen
Faculty Industrial Design – Wayne State Universit
Chair Interior Design – Wayne State University
Owner studioKuhnen – product : interface : design