7: Assembly Modeling

now that you've seen some of the tools and techniques for working with sketches and features let's start to tie these concepts together in a real-world scenario where you design an assembly using a combination of top-down and bottom-up workflows this will demonstrate the effects of using various modeling strategies in your fusion 360 designs here in this example I have a design which at the moment is a single body and it was created based on all of the sketches and features here in the timeline to get started I would like to bring an existing component into this design to do this I'll expand the data panel to browse for the design that is stored in this same project as the design I'm working with to insert it I'll right-click and select insert I can use the manipulator or dialogue to move or rotate it but I'll just click ok for now when I do a couple of things change here this is where fusion 360 stands out of course the part shows up in the canvas but also notice that the icon for the design in the top of the browser changed to an assembly icon and the new component is listed below if I expand it you can see this component contains its own origin or degrees of freedom as well as a single body the introduction of this component essentially made this design in assembly also notice a chain link icon next to the component this icon lets you know that this component was inserted into this design and externally referenced to the original design from which it came in other words if someone opens the original design and makes changes you will be notified that a change was made and you can decide when or if to update the model here in this design you can update the design by itself by right mouse clicking and choosing get latest or in case several inserted designs have been updated you can use the icon at the top to update everything all at once finally notice in the timeline that a feature was added showing the component being added to the design one of the key differences between components and bodies is that components are freely movable and by default have their own degrees of freedom when you attempt to move a body it is bound by the top level components degrees of freedom thus requiring you to use the Move command when you move a component you can simply click and drag that's because components are bound by their own degrees of freedom you can think of components as containers for bodies and each component has its own origins and reference planes unlike SolidWorks and other CAD tools fusion 360 uses something called joints for positioning and the motion behaviors of assembly components based on their origins I'll go into that in depth in another video for now I'll click undo to bring it back to its original position and I'll go ahead and hide it the browser to talk a bit more about working with bodies and components one of the powerful aspects of working here in the integrated concept of fabrication toolset of fusion 360 is that you can design as many bodies and components without ever having to worry about a particular mode that you're in or any complex external references for instance I'll show a couple of sketches that I created ahead of time I'll go ahead and create a revolve here you and before I click okay I'll expand the operation drop-down and notice here I have the options to create a new body with this feature and even a new component I'll use the new body option for now and I'll come back to the components option in a moment when I do you can see the new body listed here in the top level of the design to take this a step further let me go ahead and pattern this body I'll use a circular pattern you with four instances and go ahead and skip this extra body that's not needed when I click OK you can see in the browser that the bodies are grouped together here in the top level of the design but what if I need to make a design change if I add a chamfer here on the first instance as you might expect the other bodies were not affected by the change this is because the bodies were created in order here in the parametric time line and everything is behaving as a typical history based model I can of course just reorder this feature to come before the pattern and to the other instances update but let's contrast this behavior by using components for these instances instead of bodies to do this I'll delete the pattern chamfer and revolve features and if I go ahead and recreate the revolve feature you this time I'll use the new component option when I click OK the new component is listed in the browser with its own origin and with a single body in it I'll repeat the circular pattern I did a moment ago and this time I'll select the whole component from the browser all again skip the unneeded fourth instance and click okay when I do you can see the additional instances of the component appear here in the browser if I rename one of these you can see that the name updates for all of them followed by a number indicating each instance this time when I add a chamfer to any of the instances of this component the feature is applied to all of the instances regardless of where the feature was added in the timeline since I applied it to a component this time instead of a body all instances of the component are affected in fact if I right-click on the screen and bring up the appearances window and can drag an appearance onto any instance of the components the appearance is applied to all of them now before wrapping up there is one more thing I would like to point out when working in a design that has multiple components like I have here up to this point I have been designing everything here in the top level of the design and adding new bodies and components this is a perfectly valid and expected workflow in fusion 360 but in cases where you would like to build an assembly structure and have new geometry exist within a particular component all you have to do is activate it by clicking the icon next to it in the browser when I do the visibility changes leaving the active component opaque here on the screen at this point let me go ahead and create an additional revolve feature this time in the operation drop-down I'll again select new component when I click OK the geometry is added but also notice the component I have activated here now shows an assembly icon next to it and if I expand it it contains the new component so this method of activating either a component in the design or the top level of the design is how you can control the assembly structure you can easily make decisions about the items and your designs that you would like to behave like components and simply repeat it as additional instances or if you would like to add bodies that behave like other parametric features in the timeline which can become components down the road at any time

Channel: Autodesk Fusion 360

Views: 74,182

Keywords: fusion 360, autodesk, design, engineering, mechanical design, mechanical engineering, industrial design, product design, software, CAD, CAD software, Computer Aided Design, Modeling, Rendering, 3D software, Autodesk fusion 360, cloud based CAD, CAD in the cloud, cloud, Free CAD, Free CAD Software, Autodesk CAD, cloud manufacturing, free CAD program, 3D CAD solution

Id: SesuUThyZsU

Length: 8min 36sec (516 seconds)

Published: Sat Jun 20 2015