Models living with forms. Your insights please!...
"1) Is it common in your projects to mix model components with form (sculpted) components. If so, are there gotchas? (I have found some behaviors of interest, such as when you use a joint command to connect a model to a form, you have to select an edge or point (not a face!) on the form first, THEN select a suitable point on the model. Not the other way around.)"
For me it is very common to mix solids, surfaces, and T-Splines. In the end though I always convert my T-Splines to either a solid or a surface. I never use the T-Spline body with joints or assemblies. Once you figure out how everything works there are no real gotchas.
"2) Are there general rules that one should consider when choosing to start a body/component as a model vs a form."
This depends on what your trying to model, but in general the only rule I worry about is creating a component first then activating it then start working in it.
One thing you do need to keep in mind...there is no history in sculpt mode so beware of that.
Cheers,
Phil
Phil Procario Jr.
Owner, Laser & CNC Creations
Hi Kurt,
Yes it's very common to use both model types, sculpts and solids. What you are missing is whole concept of assemblies, what's their purpose and how they should be executed. Components (in other cad software usually called parts) serves to build an assembly. Main purpose of assemblies are motion studies. If your model does not have moving part, you don't need assemblies or components. Components still might be useful, but they are not essential. For example you can create whole complex design in software like 123D Design:
In this program we don't have components, only bodies. 123D Design is more like a hobbyist software, but other CAD software like Rhinoceros or Alias also don't have assemblies, and they are commonly used for product design. As I mentioned before, having components might be very useful even for "static" designs. Component can be reused in other designs, where trying to reuse just bodies from parametric modeler, would be very laborious. It is very important that I'm saying about components from parametric modeler. Components from direct modelers don't have that advantage over bodies. Even if we have such a feature (e.g. in SketchUp) they works mainly like groups/subgroups only. Why? Bodies in parametric designs are created through features, those features can be re-edit, and body will update, accordingly. Unfortunately "exporting" just bodies will remove those capabilities. If we would "export" component, it would keep model history, so in new design we would still be able to adjust bodies inside component. In direct modeling whole effort is pointless, because there's no way to re-edit features that were used to create body.
We can adjust geometry only through direct tools (push/pull, move, and others). Eventually there is no difference between reusing components and bodies in direct modelers. Because of that, direct modelers very rarely utilize concept of components (just to give some balance, parametric modelers don't use Layers, where in direct modelers is like main way of organizing design).
Fusion 360 have both, direct modeler and parametric modeler (to be exact, Fusion could be direct modeler or parametric modeler with direct inserts... yeah bit confusing), and regardless of that it have also assemblies, so we could add motion to our designs.
As you can see it's already confusing, so I would advise you to first learn about modeling in both of those modes. Don't touch assemblies tab at all, also for now, don't create components. Try to build everything as a single component (it's getting really complex, you need to know that when we create new file/design we work already inside of a component, and when you add components, those are sub-components, indeed. And of course we can create sub-components of sub-components...). When you'll be familiar with creation tools, when you'll know how history works in parametric mode, then you can start working with components. I know that Peter @TrippyLighting and Mark @HughesTooling (two well known forum users,) are great advocates of an idea that first rule of Fusion is "Before doing anything, create a component and activate it", but that's works only for those who understand purpose of assemblies and understand concept of "timeline" in Fusion. For beginners, it can only confuse them more (you know guys, ability to drag components, even accidentally; idea of snapshot... and other mystery stuff).
Now back to your original questions.
I would start form second question, and explain what "Forms" are indeed, then it will be easier to understand an answer on your first question. In Fusion we have 3 types of geometries, solid bodies, surface bodies and construction geometries. Solids are 3D geometries that enclose volume, surfaces are 3D/2D geometries that have no thickness, and construction geometries are 2D/1D geometries (and even further, point does not have dimensions, only position). Of course we have also sketch entities, but they are very difficult to define (very abstract, and I don't think you have problem with them). Solids can be define by single or multiple surfaces. We can imagine a surface that encloses volume, that doesn't mean it's a solid, but it could be. Surfaces that creates solids we call faces. For example a box have 6 faces, each face is in fact a surface. Please watch this youtube video made by Taylor Stein: https://www.youtube.com/watch?v=ikrk22h9D1Q , it should speak to your imagination.
It is very important to distinguish geometries (solids, surfaces), from tools and features that serves to create them. Tools from Model workspace will imidietly create solids. Tools from Path workspace creates surfaces, that will eventually serve to define solids. Tools from Sculpt can do both, the different is in way that surface is defined. From user point of view, surface is defined by control cage (generalization). My point is that all those tools have one goal, create solid body. When you asking when to use "model tools" and when "sculpt tools", you need to know how "organic" is your part. For prismatic parts, parts that have clear dependencies, like revolve (profile and axis- simple), best would be to start in Model workspace. Usually parts designed by engineers are created with use of solid tools, because geometry of their parts need to reflect simple dependencies, linear motion, rotation. Of course "today" solid tools can also work with more complex shapes defined by curves. We have sweep tools, loft tools, and many others. Nevertheless, there will be cases where non of these tools will be able to create certain shapes. Below you can see simple part. That "triger" button was possible in this shape only with use of surfacing tools (Patch workspace). "Triger" shape and trasition between "triger" and main "cylindrical" body was designed as surfaces:
You can try build similar part with solid tools, but it will be only similar. Surface here have different topology, different direction. I was able to create one surface in one "direction" other one in different. That not possible with solid tools (that's not 100% true, but explains my point). Here's another good example:
Top of that controler is build with simple planar face, some button (cylinders), trigers (revoved profile), and for sure they were bulild as solids. Everything below shiny top was build as surfaces, because each surface have different topology. Now about Sculpt. Surfacing is rather difficult task, and for certain ideas require a lot of skill and practise (also tools themself must be "advanced"). T-splines were indroduce to "replace" surfacing. You can simply drag cage points and surface will follow, you get what you see. For good surfacing you need to master your curves, t-splines could "live" without a single sketch (those are also reasons why developers called that workspace Sculpt). To summarize, which tool to use depends on shape, organic shapes or thought through faces, will require surfaces or t-splines, shapes defined by simple relations, prismatic will require solid tools.
Now, back to first question.
I don't know way you're using joint tool. Assemblies are for motion studies. To define those we need to set desired position, and set motion relation. Tool for that is Joint (As build Joint if for cases where possition is already set and you like to define type of motion). When you're using Joint tool, you can see how it "looks" for specific part of geometry:
Those are most "characteristic" points of those faces/geometries. What defines cylinder? Height, diameter, and axis, Joint will look for those. Reason why on sculpted body, or surfaces like that:
you don't get any interesting points to use, is because non of it would be "characteristic". On surface like that you can "draw" infinite amount of axis, perpendicular to that surface, infinite amont of planes, tangent to that surface. Dose it mean that we can't use sculpted bodies in assenblies, of course no. There is no point in trying to use curved surfaces, but we can combine sculpt body with other more "prismatic" shapes, and then use them to define Joint:
Pebble on this illustration was sculpted, but I've cut out cylinder. That cylinder allow me to joint my pebble with second cylinder.
Before I can answer your question, you need to ask yourself why you need Joints, maybe you were thinking about boolean tools (Combine tool), or maybe you need Align tool. And if only reason is that you like to "freeze" your components. It will be enough if you would design them as bodies, without turning them into component. Then you wouldn't be able to drag them, you would have to deliberately move them (use Move tool).
I hope that all my babble was helpful.
Cheers.
