Join Thom Tremblay for an in-depth discussion in this video Bodies or components, part of Fusion 360: Designing for Metal.
- [Instructor] Older 3D CAD systems required the use of multiple files to make even a simple assembly. Part of the power of Fusion 360 is shedding the baggage of complex file relationships so that people without years of experience can develop designs in a far more natural explorational manner. However, simplicity and flexibility still need some understanding to make the most of them. Starting with my completed sketch, I'll use the extrude tool to select some of the profiles to turn into 3D.
I can drag out the value, I'll set it to be symmetric about the sketch using the whole length and rather than typing in a value with a number, I'll start to use my user parameter. I'll begin to type width. As soon as I begin to type, it offers up any user parameter that has a name that could be selected. I'll pick it from the quick dialog and it's updated the value to 20 millimeters.
I'll click OK to create this new body. The sketch will disappear because it's been consumed by this new feature. On the timeline I see my sketch and the extrusion. In the browser under my top level component which could be looked at as the overall assembly, I have a body and the same sketch. The body right now is made up the extrusion. A body is simply a collection of three-dimensional features that can be contained within a component.
Right now it's contained within my top level component. What I should have done and many people using Fusion 360 will tell you is to use rule one which is to create a component underneath your top level, activate it before creating your bodies or sometimes even your sketches if you want the sketches to be local to that component. So, right now I have a 3D body that used a sketch but I don't have the component.
I can create the component, in fact, I can create it after the fact. I'll select the new component tool and I'll give it the name top. I'll create it as an empty component. Right now the top level of my assembly has been selected as the parent. I'll tell it not to activate it and say OK, so now I have my top component. In the timeline it's the last item. What I can do is drag this component to the left so that according to the timeline, I did create my top component before I created my sketch or my extrusion.
Well, it's really not true but we can use this to make modifications. If I want the body to be under the top component, I can simply drag it but that won't give me the results that I need. What I want is the extrusion to be under the top. If I simply drag the body, the extrusion will still be part of the 01-02 component. Instead what I'll do is I'll grab the sketch and because the extrusion is a child of the sketch by dragging the sketch into the top component, it will now be part of it.
Now, the way the timeline works in Fusion looking at the 01-02 component timeline it looks exactly the same. However, if I activate the top component I'll see that the sketch and the extrusion are now part of this top component which is great except for the fact that I have other components that I want to create from that sketch and Fusion will of course allow you to use any sketch and any component to create any feature or any body in another component but what I want to do is I want to have it all, I want to have my sketch to be part of the overall 01-02 design and have the extrusion remain in the top component, so I'll grab the sketch and move it back to the top level.
So, now if I reactivate the top level component I'll see that the extrusion is still part of its timeline and of course everything is part of the top level 01-02 component. Seems a little confusing but this level of flexibility is frankly impossible in other systems and much of the time, especially if you're creating things for yourself or you're not creating mechanisms that have to be articulated, you don't have to worry about any of this, you can just create the bodies but as soon as you want to introduce designs or you want to be able to detail individual components, you need to have separate components, so let's pause for a moment and start a new component and use it in the more traditional workflow.
So for example, now I have my top component exactly how I want it, now I'd like to create a bottom component, so I'll say that I want to create a bottom, I'll turn my sketch on, select my geometry and start the extrude tool, set the distance to width, make it symmetric and now I've got the bottom component as well.
I'll make one more component underneath the top level, call it Pin and I'll extrude it as well. This time I'll enter width again but I'll subtract a millimeter, make sure it's positioned correctly and say OK. Let's activate the top level and we'll see the beginnings of a design.
I can turn off the sketch and right now my pin has an unrealistic fit through the bottom component. What I'll do to rectify that is turn off the bottom component, I'll activate the pin so I capture this feature in the timeline and I'll use press pull to make the pin slightly smaller, say 2/10 of a millimeter smaller.
Now, I'll turn the bottom component back on, activate the top level of the assembly and see that there's a gap. The gap is good but thinking about it, I kind of wish I'd made this pin a little larger. So, I can go back to my parameters and update the pin diameter, give it the correct size. I'll say 10 and it will update both parts of the solid model.
The combination of flexible design approaches with the foundation of parametrics make it simple to explore ideas without the traditional burdens.
- Setting up parameters
- Joining components
- Animating and rendering the design
- Testing alternative materials
- Creating the setup
- Publishing and posting the design