Distributed designs

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Distributed designs.

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In this video, we’ll create a distributed design and we’ll explore design reuse options.

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In Fusion 360, we want to carry on with our gear reduction housing assembly.

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At this point I'm going to go to Inspect and turn on my Component Color Cycling as we're starting to get a lot of different components.

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And I want to reiterate the fact that two of the idle gears are identical copies and you'll notice that they come in at the same color.

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Everything we've done so far has been contained in a single design file.

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This means all of the different bodies and components that we modeled and even the McMaster-Carr hardware that we inserted,

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these are all going to be inside of our Fusion 360 design.

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However, there are other types or other times when we might want to actually create what's called a distributed design.

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A distributed design means that there are external references or resources that we're inserting into our current design.

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In order to see how that works, let's go to our data panel and let's navigate to the sheet metal lever we created in a previous video.

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We're going to drag and drop this component into the canvas area of our current design.

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When we drag and drop it into the canvas of our current design, what we're doing is we're inserting that into our current assembly.

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We can then modify, manipulate and move it around and then we're going to say OK to position it and we'll minimize our data panel.

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The sheet metal lever is obviously much larger than the housing that we're dealing with,

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but it's coming in to scale in this case the exact size that it was drawn.

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In some cases the external references might be components that are off the shelf.

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They might be components that are machined or modelled specifically for the use of multiple assemblies.

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One thing that we need to keep in mind whenever we're talking about distributed designs are those external links.

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When we take a look at this in the browser, we can see that there is a chain link icon.

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That chain link icon instantly tells us that this component has an external link.

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If we expand it, you'll notice that the component inside is our sheet metal handle and we also have a Bodies folder.

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However, you'll note that the eye icons can't be clicked on and there's some assembly context that has a local option in a radio button.

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And this is because even though this component is external, we do still have some control over making modifications here inside of our current design.

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To do this, we have what's called Edit in Place.

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So if you're working with external designs, you can create a local reference or a modification that happens in the context of your current assembly.

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What we're gonna do is we're going to select the pencil icon and note that we get a pop up.

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If you've never seen this before and you haven't clicked ‘don't show me this again’,

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it will remind you that associativity for Edit in Place is turned on by default.

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This means that the references to other components will be captured in the assembly context.

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You can toggle this on and off after you select OK, by going up to the top center of your canvas area and selecting non-associative,

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or determining which reference objects in the design will have those associative links.

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We're not going to be diving real deep into the Edit in Place functionality.

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But it is important to note that as soon as we go into Edit in Place, now we are able to change some elements of the design.

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If we take a look at our sketches, there is a sketch for the original part that was created.

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And if we go into the handle itself, we have the sketches that were used to create the original handle design.

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For example, if I right click and I edit sketch 1, I can modify the overall height in this case we’ll change it to 140 mm.

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We're going to reduce this initial value to 25 and we'll bring it in a little bit closer at 25 mm.

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From here, we can finish the sketch and it's going to update the handle but notice that it didn't update everything.

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It didn't update the slot sketch that we used to go through the center of the handle because of the way that it was designed.

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So we're going to edit this sketch and instead of being 125, we're going to set that to 75 mm.

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And now we've updated that element as well.

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We're going to OK the Edit in Place and let's go ahead and save this design.

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And note that it was saving two designs, which means that if we reopen the sheet metal lever,

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now if we take a look at the sketches that were used inside of here, this initial sketch has now been updated.

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It's now 140 mm, it's now 25 and 25.

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If this was not the intention, then we need to be careful with how we deal with these references.

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If I change that to 150 and I save this design and close it, notice that I'm now getting a warning.

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It's telling me that the design in this reference has been updated.

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There's a new version and currently it's out of date.

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While you don't have to accept that, you will see these warnings in your design until you do.

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If we update it, you'll note that now that sketch is visible and the handle is now 150 mm.

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There are other things that we should be aware of.

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If we Edit in Place and we make it non-associative and we make some changes, then we can make some modifications to the design.

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But once again, we must be careful with how we approach this.

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Let's change this to 175 mm making the handle that much longer and hiding sketch 1,

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and then we're going to finish the Edit in Place and save this assembly.

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Once again notice that it is saving both designs, the sheet metal lever and it's saving the gear housing assembly.

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If we go back to our sheet metal lever, you can see it's still updating that design.

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If you want to have a component such as this handle inside of your design can be customized,

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then the path that you want to take is to right click and break the link.

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Once you break the link, all the elements of that design are going to be brought into your current design.

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But this does mean that you no longer have that external link to the original handle.

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If that's problematic, then that's probably not the workflow that you want to explore.

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The last thing that I do want to mention in terms of distributed designs is something called Derive.

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Derive is actually the opposite direction.

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Rather than bringing an external design into an assembly,

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Derive allows us to take a component or multiple components or bodies outside of our current assembly.

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So first we're going to save and then we're going to pick one of the components that we want to export.

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We're going to select this gear and I'm not gonna worry about parameters but note that you can bring parameters in from components.

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You can select those options if you wish, we’re going to say, OK.

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And now what we've done is we've taken just that single gear and we've brought it out into its own design.

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If we go to modify change parameters and we take a look at what was brought,

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you can see that we brought all of those user parameters over by selecting those options.

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And this can help us define some aspects of this gear.

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Now, it's important to note when we derive something out of the assembly, we are free to make modifications in here.

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For example, if I create a sketch, I'm going to use a rectangle and create a keyway in this gear.

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If I use extrude and I cut the keyway through my gear and then I save this design, I'm going to call this External Derived Gear.

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It's not something that we're going to be using in the context of our assembly,

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but I do want to make sure that I select and put it in the correct folder.

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I'm going to place it in my Basics of Assemblies folder.

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So now we have this gear that has a keyway cut in it.

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If we go back to the original design, the keyway is not there.

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However, if we make changes at this level, for example, if I create a sketch, I'm going to add a small circular hole inside of this gear.

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This is something that we are going to remove later.

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Let's go ahead and just make that recess, make a cut and save the design.

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When we save or modify a design in the context of the assembly, the Derive will get updated as well.

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You see now it's telling us that it's out of date and you'll notice as soon as we update it that it is going to bring over those new design elements.

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So once again, this is actually the opposite direction of that distributed design where we brought an external design into our assembly.

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In this case, we can take a design out of our assembly and we can continue to work with it,

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add additional details that aren't really affecting the context of our assembly.

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Once again, we're not going to be using this external gear, you can continue to play around with that functionality.

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But we want to go back into our design, we're going to select and delete that sketch and that extrude,

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because we want to make sure that we keep this gear, how we designed it using that script.

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But it is important to understand the functionality of those external designs coming into your assembly,

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as well as context of taking some elements of your assembly and taking them outside as a Derive.

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Once you're done playing around with that, let's make sure that we do save this before moving on to the next step.