Beginner: When to use Components; When to pattern a sketch Vs body?

[Anonymous]

Hi All,

I am a woodworker moving over from Sketchup.  Mostly I will be designing furniture, and don't anticipate using any moving joints in F360.

I have a couple best practices questions...

1) When should I break things into components?  For example, if I have a simple case with identical top and bottom panels, and then 3 identical vertical dividers... should those all be bodies within 1 component, or should I break that out into separate components in some way?  Also, say the general design of those dividers are the same, but the center one has a slight modification?

2) Patterning:  In some of the vids I have watched, the engineer will pattern parts in the sketch, and then extrude them all together.  Sometimes they sketch one part, extrude it, and then pattern the body/component.

Coming from woodworking, I will typically have a parameter like "NumberOfDrawers" that would be adjustable.  If I was patterning the duplicate drawer fronts that are just going to be repeated in a vertical pattern, it seems to be that creating one in a sketch and then patterning the body makes more sense... otherwise how would F360 know which of the patterned sketch features to extrude?

Lastly, when I pattern a body- am I better off patterning it as a component?

Thanks!

[TrippyLighting · Accepted solution]

First familiarize yourself with Fusion 360 R.U.L.E #1.

I might add that many woodworking projects fall into the Exceptions to the rule as they start with a skeleton sketch that several components are derived from.

In general, you should keep anything out of sketches aha can be done with solid modeling tools. A small pattern in a Sketch is fine but still, it might be better to use solid geometry.

[Anonymous]

Ah, thank you.  I can see how with typical solid modelling, you would design one part from one or more sketches, but it would be one, connected part.  If I was modelling more like a CAD engineer, I would tend to create a sketch for each separate part.

I think what you are suggesting is that I should extrude multiple bodies sparingly from sketches, and turn them into components as soon as their shared design features are complete.  This preserves the history/parametric modelling, so I can go back and change common features, but still treats the final parts as separate entities (For BOM, drawings, etc).

Thinking about this, it might be better to construct parts directly as solid bodies without the sketch, using constructed planes and/or constraints on the bodies rather than sketches with multiple extrusions.

Hmm... is it possible to define a macro such that I can add a CREATE BODY for say, a 5/4 board?  That is, I would select this macro from the CREATE menu, specify the plane and then the 2D shape... and have the macro automatically set the Z/Extrusion to 1.00"?  I could then create these for the most common plank thicknesses.  I'll look into that...

[Anonymous]

Answered my own question.  Looks like I may have to brush off my python skills.

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[chrisplyler · Accepted solution]

Sure, you might consider a cabinet shell or a drawer to be one "part" after you've assembled it. But really each board you cut should be a Component. Like this simple example:

Now, you can "nest" Components inside each other. For example, you might have a main Component to be your "Cabinet Assembly." Nested within that, you might have one Component for the shell, and four Components for four drawers. Nested within those five would be each board Component used in their respective construction. It's not unlike files in a folder inside another folder on your computer.

Nested within one of the drawer Components, for example, might be the face Component, two side Components, a back Component, a bottom Component, etc. Perhaps the drawer-mounted halves of a couple of roller guide components and a pull hardware component. Maybe a fasteners Component that has further nested within it any screws or nails or dowels Components or whatever, if you're going into that much detail.

Of course, once you finish one complete drawer, you could copy/paste it into it's "parent" drawers Component to end up with Drawer:1, Drawer:2, Drawer:3 and Drawer:4.

Maybe nested within the shell component is a hardware Component, and within that hardware Component is nested some of the shell-side haves of the roller guides.

Now all the drawer Components would be Jointed or Grouped together properly, and all the shell Components would be Jointed or Grouped together properly, and finally you would Joint those drawer-side halves of the roller guides to the shell-side halves of the roller guides.

Then you've got a functional cabinet assembly that represents the real world. You can pull DFX outlines from each board to physically cut the wood with. You can copy a drawer Component from this assembly and add it into another cabinet assembly. You can contract/expand the Browser in an organized way just like you would when looking for a file in a folder tree on your computer.

[Anonymous]

Thank you!  (I hope you didn't create that just for me though!).

I'm getting the hang of it... the biggest problem I have is when I create a new sketch to create something, but forget to create the component first or create it under the wrong parent.  Sometimes I seem to be able to move things around and change the nesting, sometimes it doesn't seem to work.  I am sure it's just something subtle I am doing- possibly basing my new component's sketch off of parts in other components, rather than user params and then joining or arranging.

I realize now that I have been watching a lot of beginner vids, but they are all mostly creating one part, just using sketches over and over on the same part to create details.  Woodworking is going to be more of an assembly of lots of relatively simple parts.

[GRSnyder]

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Woodworking is going to be more of an assembly of lots of relatively simple parts.

This is tangential to your original query, but woodworking is my main application as well. I'd encourage you to think in terms of a multiphase workflow for each project - you can use Fusion 360 for a lot more than just the basic design.

I usually start by modeling the desired product without worrying too much about the actual construction details. For example, if I was designing a bookshelf and I planned to set the shelves into dados on the case, I wouldn't model the dados; I'd just add shelves that spanned the inner surface of the case. This keeps the modeling relatively fast and simple and facilitates interactive design. (And to your original question, yes, a shelf would be a component, since it's going to be a replicated element distributed according to user parameters.)

Once I'm happy with the overall design, then I ask, "OK, how am I going to actually build this?"

Phase two usually starts by merging a lot of the bodies generated in phase one into composite masses. For example, I'd merge the sides of the case and the shelves into one body. Then I'd draw profiles for the dados on the front and use them to slice a representative shelf out of that mass, producing a shelf board that is wider than the interior dimension of the case, plus two sides with dados. Those are the parts to be produced in the shop; they're the objects that will participate in the actual physical assembly process.

In phase three, I reconstruct the entire project using the parts produced in phase two. There's no modeling here, just assembly. This operation verifies that the phase-two deconstruction was done properly and that the original design has been faithfully translated into a manufacturable plan. You can use Combine operations (e.g., intersection or subtraction) to verify that the object built from parts has identical 3D properties to the original design. Phase three also gives you a chance to think about the actual assembly process, step by step. You go through it in the virtual world, which often reveals potential issues well before you get to real life and things are harder to fix (e.g., "Do I own a clamp long enough to let me assemble things in this order?").

In phase four, I worry about the physical process of producing each part. For example, I pull the end of each board out a little bit to allow for some waste. This gives me some room to trim iteratively in the shop, either to achieve accurate dimensions or to sneak up on a perfect fit through trial and error during assembly. The result of phase three is a raw cut/milling list. I dump this into CutList Plus fx, which tells me how to make those raw parts most efficiently from the boards and sheet goods I have on hand.

The nice thing about this layered approach is that it's all completely connected; there's never a point of no return. At any time you can return to the parts, or the assembly, or even the original design, and make changes. Yes, you may need to adjust parts of later phases correspondingly, but that's usually pretty easy.

Components are a critical part of keeping this all organized. Top-level components mirror the phases: Design, Parts, Assembly, Milling. Components within Parts, for example, are based on elements of the Design, but they also have their own modeling path that you don't want to mix up with the base Design. When you look at the Design, you should see only the components and modeling history relevant to that phase. The Parts phase clones in elements of the Design, and the Assembly phase clones in only components defined by Parts.

TL;DR: See rule #1. 🙂

[Gigabeast]

I'm just beginning with Fusion360, and the answer given seems rather confused with regard to "Components" and "Bodies" !

I've had to watch several videos just to be able to get started with Fusion360 because it has so many ways of doing things. Primarily you have to choose your directional approach. The "Top-Down" approach (eg start by creating a Bookcase Component and then defining the various Bodies that make up that Component, such as sides, base, top, shelves) seems to be preferred in Fusion360 because you can develop relationships between the Bodies as you build the Bookcase, although it has the drawback that the project file can get quite large if there are many Bodies in the design so the program can slow down. The other approach is "Bottom-Up" where you design each item as its own "Component", so you'd have a top level item called "Shelf" which is saved as a file, then another top level item called "Base" which is saved as a file, and so on, and then you have to assemble the various Components into a final Project "Bookcase" which then itself becomes a "Component"! The best way I saw it explained was that the word "Component" in the context of Fusion360 is akin to a "Folder" in computing, ie merely a container. The word "Body" in the context of Fusion360 is akin to a "File" in computing, ie the instructions and data etc.. 

So to build a "Bookcase" you should start with a New Component and call it "Bookcase". You then create various "Bodies" which would be your shelves and sides, one Body per piece of wood. You can nest them to group similar items together and that would then be a "sub-assembly" I think. 

It would help a lot if everyone referred to the correct terms as used by Fusion360 - it's immensely confusing if people refer to "components" as individual items as they would in the rest of the world outside CAD, because in Fusion360 a "Component" is a group of assets like Bodies and Sketches and imported meshes, and not an individual item. 

Hope I actually understood correctly what I'm banging on about here or I'll be guilty of muddying the waters even further! 

(EDITED) Oh, maybe I got that wrong after all, hahahaha, sorry, you can have lots of "Components" in a top level Project, but the concept of using a "Component" as a container for all the various "Body" parts is still valid, rather than designing each piece of the bookcase as a separate Component.

[TrippyLighting]

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@Gigabeast wrote:

... because in Fusion360 a "Component" is a group of assets like Bodies and Sketches and imported meshes, and not an individual item...

.

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That is the same n other CAD systems, but often under a different naming convention.

A body is one contiguous piece of geometry. In Fusion 360, a body is always part of a component, because each individual file is already a component.

In a mechanical design most components contains only one body, but that isn't a hard rule.

A component is a collection of all those objects (browser) and features (timeline) that are used to create the body (or bodies) in that component.

If you create a component within another component, the upper level component will become a component group. In other CAD system a component is often called a part (SolidWorks for example), and a component group is called an assembly.

[Gigabeast]

Thanks 🐵

[terry_fusion]

Working in a custom fab shop has challenges that I wont even begin to get into on here.

But please allow me to add my .02 cents to the conversation. 🙂

What helps me is making some reference notes to follow as I move along in the design process notes that will detail out rough sketches, type of component to be designed with references or links to google searches, color choices, materials, etc.

I wish there were a way to attach said notes to the design, either as an embedded file or a link to an external file (text, pdf, excel spreadsheet, or image)

Having pregamed the design process makes the flow a lot smoother, for me.

I begin by creating a series of sketches spanned across however many will give me the profiles I'll need to generate each assembly/component group into.

Then I go nuts creating and naming components until I have what I need.

For example, I'm redesigning the interior my Shasta Starflyte camper.

I have a canvas for each of the 3 views of the camper from which I create a master component for the body.

Then each subsequent item in the camper is in it own component with a number sub-components underneath the parent level component, or depending upon the complexity of each component I may create that part as a built in place design or as separate file and insert it into my master design as a derived component.

This helps me keep things tidy and organized and lightweight, editing a part as its own entity helps keep the master file easier to manage.

A lot of it comes down to the scope of the project, how involved it will be and how many changes I expect to be making in the future.