Dealing with Assemblies | Viewer Request # 3 | Fusion 360 Tutorial

hello everyone my name is austin shainer and welcome back to my channel in 3d design there are really only two primary schools of thought bottom-up or top-down design the conventional method for most 3d programs is bottom up which means that you create each part individually in a separate part file and then bring them all together into an assembly file in which you can create relationships between components by joining or mating them together this is extremely useful when dealing with complex designs or large assemblies as our program does not need to recalculate every part in your assembly each time an individual part has been modified but merely change its position in space this method does have its drawbacks however when you need to make changes to an individual part you must first open that part separately make your change then go back to your assembly and update it this not only makes the modeling process slower but also introduces more opportunity for dimensional mistakes as the other components in your design may now need to be updated as well the other school of thought is top down design where you start with the assembly file and then create each component within the context of that assembly this means that the dimensions of parts can be more readily driven by other features or components in your design this is extremely useful when building parametric shapes and features and can make life much easier for developing new products when you may not know exactly what the dimensions of any given part should be the drawbacks to a top down approach however is that it can be very resource intensive all dimensions are contingent upon all other dimensions and locations of features in your design this introduces more opportunity for calculation errors because when you change the dimension of one feature the other features that were dependent upon that dimension may now be impossible to create all that being said there's really no correct method here each have their pros and cons and the approach you should use depends on the design you're trying to create so for this reason programs like solidworks and fusion offer a sort of hybrid approach to this but each specialize in one particular method solidworks primarily uses a bottom-up approach while 360 primarily uses a top-down approach both solidworks and fusion offer the ability to do either but they're both somewhat limited when out of their element so today i would like to cover how you can implement both a bottom-up or a top-down approach in fusion 360 and what key things you'll need to pay attention to as you generate your design so let's not waste any more time and dig right in okay so jumping into fusion we are going to cover primarily bottom up design today because fusion 360 is natively a top-down design software so most of you are already using a top-down approach in your designs so what we really need to figure out is how can we utilize a bottom up approach to enhance our designs and make modeling changes between different designs much more streamlined so what you see on the screen here is a water cooling loop that i developed for a friend of mine he wanted a water cooling loop in a computer based up around the aqua tube or sorry aqua computer aqua tube reservoir it's a very old reservoir in the market and it's still to stay one of the most unique and interesting ones out there and he liked the design so much he wanted this kind of like industrial slash steampunk vibe to it so that's what we're gonna do now we're not gonna model the entire thing because we don't have the time for that but what we are going to focus on is this reservoir right here so that's what we're going to be building today and if i pull this up you'll see that it offers a pretty good example of both bottom up and top down design so i have top down by building this component and some like this glass right here that goes on top but then we have bottom up by inserting a bunch of fittings and screws and all the little things that connect to it and so i'm going to show you how you can reuse those between designs okay so i've opened up a new design and we're going to sketch on the top plane now i'm going to create a circle representing the outer diameter of this reservoir so we're going to do 100 millimeters and then we're going to create another circle that represents the inside lip where the glass is going to sit so let's do 92 millimeters and we're going to create one more which is going to represent the main bore into the body where the fluid is going to sit so we're going to do 70 millimeters so now we can just use this to create a cylinder so select all three solid extrude i'm gonna go down negative 100 millimeters and then if i bring back my sketches i can take these two or i can just take this one it doesn't matter extrude it down i'm going to go down six millimeters and then i'm going to take this one and i'm going to extrude that down to object this bottom face right here and then we're going to offset negative 12 millimeters so that way we create some material on the bottom there so that way we have some strength so hit ok and that takes care of the main portion of the body so now what we need to do is create those little ridges that you saw so i'm going to insert a new plane an offset plane from the top and i'm going to go down negative 12 millimeters i'm going to sketch on that plane and then i'm going to project in this outer edge so let me hide the bodies real quick so we have that outer edge and so now we're just going to offset that by negative two millimeters which will give us the depth of the recess for those ridges then we can select this line or this face and then we're not face profile bring up our body and we go solid extrude and we'll bring that down negative three millimeters so that will give us our first ridge and so then we can go ahead and do a pattern so we'll go rectangular pattern and we're gonna wanna select this feature so let's change it to features and then select that again directions what we want to do is we want to go in this direction so in the z and we want to do extent so we need to figure out what is the depth from here minus 12 millimeters so i'm going to do a quick guess and then we'll measure and compensate so let's go ahead and do extent and we'll go negative 70 millimeters or sorry positive 70 millimeters no it should be negative there we go let's do that real quick and let's verify what our heights are here and compensate so we've got 15 so we're three millimeters off so let's go back here and let's go 73 millimeters let's inspect that now so this should be 12 millimeters yes so we are good okay so now we can come back in and update the quantity of the ridges until they look roughly equal to each other let's keep going almost there that looks pretty good so those look roughly equal to each other hit okay and there we go so now we've got those ridges or fins whatever you want to call them they kind of look like a heatsink and so now what we need to do is we need to create the flat spots on the side so that way we can have g quarter fittings going through so i'm going to create a new sketch on that same offset plane like that and then we're going to project in this inner line or this inner line right here hide our bodies and we're going to create a square that is tangent on all corners of that we'll go tangent tangent tangent and one more there we go and then all we need to do is give ourselves another rectangle so we can either do add another rectangle or we can do offset so let's do that since it's easier we're going to offset this by like one inch just to give ourselves a profile that we can use to cut with so hit ok and then we'll select that bring our body back and now what we can do is go solid extrude down you can see it's creating those flat spots i'm going to go to object this bottom edge right here so we don't want it to go past that hit okay and now you see we've got all four sides with the flat spot so we can add in those fittings so let's create a sketch on the side profile here so that way we can go ahead and get the geometry we need to place a g quarter fitting onto so i'm going to project in these two lines right here from this body and i'm going to create two lines from here to here actually i think i'm gonna end up creating three like that across and we're gonna make all these equal let's make these construction lines and now we can create a circle or a point in fact let's just do a point we need to set the point where these fittings are going to go and so now we have a sketch that we can drop a whole feature onto so if i hide this or finish it and then i go to hole i can click on each one of these and it will locate on those points and then i can change it so to distance we can go to object the inside face of this bore and then what we want to do is we want to come up here and say we know we want a simple hole we don't want a counter bore or a countersink but we do want it to be tapped so now when we click tap it gives us the ability to define what is our thread pitch or what is our class of thread so we're going to go thread type and in this case it's a pipe thread so i think it's british standard pipe threads i think that's what bsp stands for so go bsp i'm going to go one quarter and that gives us our quarter inch thread right hand and here's a really important tip when you're doing holes is do you want it modeled or not modeled so modeled means it's actually going to cut that thread into the actual part design but that creates some challenges later on when you're trying to join or make components together so typically it's fairly good design practice unless you actually need it to not include the threads in your model and most like the drawings and everything like that will still recognize them as g quarter threads but you don't end up having the actual curvature in there so i'm going to not have them modeled and hit ok and so now we have our first one and we might adjust the distance here in a second but now we just want to basically create a circular pattern of this feature to the top side and bottom so we can come up here and hit create pattern circular pattern and we can do type features we want a circular pattern this hole and then what is the axis so the axis is going to be this one right here it looks like it's not quite right no yes it is and so we want four so there you go so now you see that we have one on each side and we just hit okay and it didn't show up let's go back i think we need to change it from adjust to optimized or identical so let's try optimize there we go yes so it went ahead and included those in there so now we actually have the whole pattern in there as well so i did just double check my design and i need to increase the spacing between these two so we're going to go back to this sketch right here i'm going to take off the equal constraint off of this middle line right here let's take off all the equals actually and just make just these two outside ones equal but this middle one we need to be 35 millimeters hit okay and you'll see that the rest of the design has been updated so that is now what we want so moving on what we need to do now is create the bolt pattern for the m3 screws that will secure the glass on the front in place so we're going to select a great sketch on this plane right here so that's where the holes are going to be threaded into and then let's go ahead and create a circle from the center point and we're going to make that 83 millimeters so 83 millimeters and this is going to represent the where we place our first hole and then we don't need to really place the others because we can just do a pattern around so i'm going to create a circle here in fact let's just create a point like we did before instead of a circle we'll do point and we'll make these two vertical so it's at the top of the circle and then hit finish sketch and now what we can do is go create hole and we're gonna do the same thing so we're gonna we don't we just want a simple hole we want it tapped we don't need any offsets and it's fine if it's uh the end of the point is angled and then what we want to do is go to ansi metric m profile and we want to do three millimeter by point five hit okay and so now we have the first threaded hole and it's got the threads in there and now we can do is create another circular pattern so we'll go pattern circular pattern and we'll use this feature along the center axis again and we want to set the quantity to eight now we will get a nice little distribution across each one hit okay and the last thing we need to do is create a little o-ring groove so that way we actually provide a seal for the glass and then we'll start inserting some different components so we're going to sketch again on this face and we're going to project in this circle and then we're going to offset that so let's hide this real quick we're going to offset that by the amount of the wall thickness we want to have around the o-ring so let's do 1.5 millimeters then we're going to offset you can't offset off an offset line it's really quite frustrating so you either have to add that 1.5 millimeters into the dimension you want or you draw another circle dimensioning off of the previous one so that's what we're going to do so i'm gonna do this another circle and i'm gonna dimension between these two of 2.2 millimeters and let's bring back our bodies make sure we still have enough room here yes we do so that should be good and let's select that and we're going to extrude it down 1.3 millimeters that's a i want the wrong direction negative 1.3 millimeters okay i need to change it to cut sorry there we go okay so now we have our bolt pattern we have our little o-ring groove and we basically have most of this modeled up now so so far we have neither done top-down or bottom-up approach right now this is basically it could be an assembly file or it could be a part file so what we're actually going to do is we're going to turn this into a sub-assembly file now the first part we're going to do is actually top down so we're going to create a new component based off of the features in here within the same file and so that means that that is a top down approach but then we're going to go bottom up and add in the fittings so let's create a new component and we'll call this glass and then what we're going to want to do is sketch on this plane and we can project in this line outer line right here and actually let's project in these circles right here that come on select it a couple more okay project those in and that'll give us our base hole and we can then extrude that up to object this feature right here okay actually i apologize we don't want to have those circles in here so i'm going to deselect them from this in fact actually let's just go back to that delete that extrude go back to the sketch and we're going to delete all of these i apologize about this because what we're going to end up doing is we're going to end up creating another pattern of a different type of bolt hole so that way we have a clearance hole rather than a threaded hole so the diameter of this right now is wrong so we don't need that so hit finish and then we will bring back that sketch sorry that sketches in here and we will extrude that up to object the top face here hit ok and then you'll notice because now it's a component it can move it's not tied to this at all so what we need to do is we need to join it to this inner ring here so what you can do is you can select each edge that you want to mate together or join together like this one and this one and you can hit j on your keyboard or you can come up to assemble joint and it will automatically snap to the center point of both faces which and for in our case works out great but then you can either rotate it or move it as like an offset from that face if you wanted to so we're just going to say 0 and be good and then we're going to go ahead and sketch on that top surface and we're going to project in that little point right here to that top surface because that gives us our center point of our first circle from the previous bolt pattern so now i can go ahead and create a hole on that point and then we'll do another circular pattern wrapping around so in this case we don't want a counter bore or a countersink although we could do countersink we can just go ahead and do a simple hole and then we're going to do a clearance hole not a tapped hole because we need the bolt to pass through it and then we can just do flat and let's hide the body and we're going to go distance to object the back surface of this piece of glass and then on here we need to come back and select m3 clearance hole and do we want it to be a loose fit a tight fit etc we're going to say a close fit that's going to be a tight fit so that way we get less chance of mispositioning this hit okay and now we're gonna do one more circular pattern so let's go create pattern circular pattern and we're gonna do features this hole around the center axis and we're going to do quantity eight which will match up with the one we did before hit okay let's bring back our bodies and it's kind of hard to see right now but you can see that we are concentric with the two holes the inner hole and the outer hole and so let's go ahead and make this transparent so that way we can kind of see through it so hit a on your keyboard for appearance and we will type let's do acrylic acrylic clear like that and now you can see we can see through it but we still have that face there so that is good so before we do anything else let's save this and so we're going to save it to let's open this up what we're going to do is we're going to create a new project and we'll talk about this more in a second but we'll do new project and we will type reservoir or water cooling loop we're going to save it inside that project so save it there and we will type reservoir okay so we can now now that we have that saved we have the option to either utilize this as a stand-alone sub-assembly of two components or we can insert components into this design and further add to the assembly so right now i'm going to go ahead and further add to the sub assembly so we still have kind of a bottom up but i'll show you what i mean so if we go insert mcmaster car component this is a really amazing feature and one of the main reasons i love fusion 360 because i don't have to model bolts and i don't have to model washers or all the little add-ons that you can get on mcmaster i can just directly import them into my model and first of all thank you mcmaster for having nearly all of your components on your website 3d modeled and available to throw into my design that has been amazing for me so we're gonna go screws bolts and we're gonna do m3 so let's go m three by 0.5 thread pitch and we're going to do a socket head cap screw so we're going to do socket and let's just do stainless steel and let's do low profile and let's see if there's anything else we need the length so we need to inspect the length real quick so i want it to be eight millimeters long and let's let's make this a little bit bigger so we can see it a bit better so we have two options here what are the differences we have coarse fully threaded i'm not exactly sure what the difference is between these two oh super corrosion resistant 316 stainless or 18.8 let's do 316 because this will see coolant and we don't want corrosion getting in our coolant or anything like that so let's just click on this item number go to product detail or you can click right here it looks like they've added this recently and you can say do i want to download download this directly into solidworks or do i want to download it as a step file into whatever cad program i'm using so fusion 360 it's best to just use a step so we go 3d step download and that's going to insert this bolt into our design and then we can join it to this piece of glass now this is still basically top down not bottom up because this uh this bolt that we've inserted is only exists within the context of this assembly it doesn't exist in any other files or folder structures that i have on my computer so i can't really reuse this between different designs so this is an important thing to remember if i know let's say i'm going to be building different versions of this and i want to reuse this same bolt between different designs it might be a good idea to download that as a step file into its own part file so that way i can add it to my library here and insert it into future designs but if it's only going to exist within this one designed then it's probably not that necessary but let me show you how you would do that so let's go to our water cooling loop so we have our reservoir here and i'm going to insert this item number so i'm going to copy this real quick so we don't have to search for it again and we're going to create a new design and let's save it real quick because you can't insert things that um aren't saved already and we are going to save it to the water cooling loop and we're going to do m3 by eight millimeter hit save and we'll go mcmaster car component and i'm gonna search for that item number hit okay and i'm gonna download 3d step into this file hit ok and then we're just going to save it so now if i pull up my water cooling loop folder so let's go back to water cooling loop you'll notice that i now have both my reservoir and this bolt here and so what i could do and i like to do this and i'll show you more about this in my computer file but i like to create new folders where i can save common commonly used parts so i will do new folder bolts and then i can drag that i might need to close it real quick okay well let me drag it so you can right click and hit move and we're going to move it into the bolt folder so now i can save any bolts that i'm going to be using for this project or any other project like this in this folder and so let's go ahead and delete this file right here and we're going to insert that bolt into this design so now i can open that up drag it in and now i have my bolt and then i can let's rotate it around and let's join it to the first one so let's go top we want to do this one so i'm going to grab the one of the circles on it and i'm going to grab this circle up here and we're going to hit j on our keyboard and join those together now i have two options here i can either insert another bolt and then rejoin it or i can do a circular pattern of this component so let's try doing it that way because everything you add to the timeline is going to increase the complexity of what fusion needs to calculate when you make design changes so we're just going to do a bolt pattern so create pattern circular pattern and we're going to do components and we're going to select this one if we can let's see let's hide the other ones let's hide those bodies component well let me select it maybe hold on okay so it just wasn't letting me select it but i can select it from this design tree right here and we'll hit that and then we will go axis on this axis and so now you can see we have our our bolts starting to show up so we're going to go quantity 8 like that hit okay and let's bring back our other bodies and let's bring back the main hole okay okay so i made a mistake and what it's doing is it actually added in eight of the whole glass and the bolts and that's because i inserted this component into this top level component of glass so i actually need to undo that so let's undo this pattern go back to our main timeline and let's delete that one and so now we're just left with this component insert so let's delete that component insert and let's shorten this up and let's go make sure you're clicked on the highest level assembly file right here so not this component but this one and now let's insert that into here so now it's going to insert it underneath glass but not inside glass and that was the problem we ran into so let's rotate this around and let's rejoin it this bottom ring right here to this one join and now let's do our circular pattern so pattern circular pattern components and we're going to select this component right here along this axis and we will do eight there we go hit okay and so yes now we have eight bolts rather than eight bolts and the glass so that was that fixed a little mistake in mind so i apologize for that so let's add a new component and we'll call this hardware and what we can do is we can drag all of these into that component so now that is its own component where i can hide it and modify it move it etc and so that is an example of how we went top down from building this body and building this glass to bottom up by having a separate part file for this bolt and inserting that and making a circular pattern across our part so now what we're going to end up doing is going through and adding some fittings to this to match what we did in or match what i did for my design so let's go back to my pc folder where as you'll see i have a lot of folders with a lot of different files so like i have different sizes of radiators i have different sizes of fans i have different fittings and so in here this is like the g quarter fittings that i would end up installing on this reservoir so i can either just drag these in directly from this folder or i can create a new folder for this project for fittings and then i could create a copy of these into that folder if i wanted to so let's just assume that i didn't that i went ahead and created these in that folder and we can drag these into here what you could also do is if you needed to create a new folder you can hit upload and then you could upload any file that you download from grab cad or thingiverse or anything drop it in there as a reusable component and then all of this will still apply so let's do a g quarter let's look for straight hard line fitting so we'll use this one and we'll drag that into our design okay so this is interesting thing to think about it says designs inserted from another project will not be linked components from the selected design will be copied into this design so what that means is that it's turning it from a bottom up into a top down which means that part will only exist within the context of that assembly and if i went back and updated something in this fitting it won't be linked and won't update in this design and so if i actually hit cancel on this and i bring up my hardware you'll notice because we dragged in the bolts that there's a little link icon right here that means that the dimensions and colors and everything of this bolt are linked to that original part file so if i like right click and i open that part file and i change let's say like the color of it so let's go red real quick let's just drag that on there hit ok save and i bring it back you'll notice all of these have a little hazard symbol next to it and that means that that component is that component is out of date it needs it needs you to come up here and click the update button in order to bring in those changes so if i click that you'll notice that now all of those have turned red and that's from a change that we made in the original part file but if you didn't want that to happen so let me go back and hit save like that go back and let's update it again so now it's back to normal and if you didn't want that you could and you wanted to turn this from a bottom up into a top down design you can right click here and say break link and what that means is if i break the link of that individual part let's see here i didn't want to break that that might be because that is the top one let's try this break link okay it's not letting me do that because it's a circular reference or not a circular reference but a circular pattern but normally if you're inserting a design and it's got a link you can right click and hit break link and then you can make changes to that part within the context of this assembly without impacting this original file so this one will always remain constant but maybe like just one of these bolts i didn't want to have the hex on here and i wanted to fill in that gap i could break the link on that individual part and then make modifications and so that's really important to to remember so let's go ahead and let's copy this over so let's create a copy of this and we're going to bring it into our water cooling loop and we're going to create a new folder called fittings and inside fittings we're going to make a copy of that so now if we go back to our fittings folder or not things water cooling loop folder and inside fittings i have this so now now that this file is in the same project i can drag it in and it will be a linked reference so i dragged it into the hardware one and let's just move this out of the way a little bit and then we will create a joint on that i think that represents the o-ring so we will create a joint right here to that now it's it's flipped by accident so let's click flip and hit okay you'll notice that that didn't that did insert without the error message and it has the link here now if i right click and say break link it allows me to break it and so even if i go come in here and i open up this file and let's say i change this to red again let's do the same thing hit okay save that stupid editable documents thank you very much fusion 360. okay let's hit save and then i come back in here and you'll notice it hasn't detected that anything has changed because there is no longer a link between this item and the original document so we broke that link so if i undo you'll notice when i hit ctrl z it now says that it's out of date so if i update that file all of a sudden it's red now so i come back let's undo that save let's see save yep and let's undo again update it okay it's wanting to pull that in there so let's go and just delete this file and bring that back in so fittings that didn't save ah okay it created a new part file weird so let's open this back up okay i'm gonna have to recopy that i screwed something up there i'm sorry now i won't have to recopy it so let's just unassign and delete that right there and go steel knurled and then i think steel satin was on the internal faces there and on these faces so let's actually just do body steel satin and on faces we will have that face that face and that face and that'll be good okay let's hit save go back to our reservoir update it okay we're back to normal sorry about that i must have screwed something up somehow let's rejoin this oh i need to flip it i forgot edit joint there we go flip okay so now we're in a position where we could go one of two directions we could either bring this into our computer file and then start creating the pipes from there or we could create the pipes in here and bring all of that into the computer file and in this case because i need to reference geometry that is on the radiators and the graphics card etc i would actually choose to probably just get the fittings that i know i want to use in place in this sub-assembly and then bring that sub-assembly into the computer file and draw my pipes from there so let's go ahead and let's say we want to have this one as an outlet that is feeding into the pump and let's say we need to have that back one right here on the sides as an inlet where it's returning from the radiator so i'm going to insert this and let's rotate it around and let's join it here j enter and let's bring another one in and we could have mirrored it over that's okay but this isn't like a really complicated part so it's no problem just to create multiple joints and let's go j enter okay so i've got an inlet from this side and an outlet from this side now theoretically this one isn't exactly necessary but in my design i created a little a little valve between them which allows me to run a valve up to the top of the computer or i can fill it up so i can open that to let air into the system and close it to to seal it off so that way i never have to get inside here and try to fill my reservoir from like this little top port here so i can just have a valve that opens up let's air in and so i'm gonna go ahead and put a fitting there and there's one more fitting i'm going to do is i'm going to put some caps on these other ones so that way they don't leak like a sieve so let's go back to my pc folder pull up fittings and we need just the cap it's like right here i think that one should be good let's check yep so let's drag wait we can't we have to create a copy of it so copy into water cooling loop fittings copy and then let's go back to our water clean loop fittings that should be in here now and i can now drag that in as a linked file and let's go ahead and bring this up mate this to the top and i'm going to do this to all of them so i will see you back here in a second okay so i've got all of those closed up now thanks for bearing with me on that one and one little piece de la resistance i'm sure i butchered the name of that is let's go ahead and add in some water and that's going to be a really cool little final touch so let's hide the glass and let's create a new component and we're going to say water or let's rename it to coolant so rename where's rename all right we're just going to click there rename and we're going to sketch on this front surface we're going to project in that line from that body and i'm going to create a spline and i know you guys know that i'm not a huge fan of splines but i think this is a great quick use for one and let's create like that hit enter and use a fits point spline and then i'm just going to drag this like that to kind of create a little wave in there as if the water was kind of turning and then that'll be good i'll just select that and go fix on fix and we can now extrude that into the back of this so let's open up our bodies and hit extrude to object that back surface because we want it above this little water line right here and then what we can do is we can hit an appearance and let's look up liquid and let's do water clear and i can either leave it like that or i can change the color so let's do like a red to match the kind of the color scheme and then this absorption distance is how dense is that water how effectively does that water let light through so let's do like a hundred and oh i don't 100 inches want 100 millimeters well let me no okay so we're gonna do butter that's like four inches okay let's try rendering right that real quick and see what that looks like so render and let's make this the front curves view is front change our scene if we get some light shining in there a little bit oh back there we go okay and let's see how well that lights up it might be really dark it might be really bright okay that's actually very bright so what we can do though to make it shine a little bit better in there and this is a really neat trick a lot of people don't know about is i can use internal faces up here as an led so if i hide this i have this component right here which is that little cap right or this back one up here so let's do that one if i hit my appearance tab and i type led i can do like a 5000 lumen white and then if i select faces i could add an led to just that little back face let me see if i can select it here come on faces will it let me it might not because it's a linked file so what we're going to do is we're going to take this one and we're going to break the link let's go back to design and let's break the link on that one just that one then go back into render and apply an appearance to that face of led like that so the other ones don't have that that led applied to them but this one does so that's a useful way to break the link hit okay and the led doesn't show up when you're just looking at it like this but it does show up when you render it so let me go like this and hit render without the actual water in there and now you can see that the inside is lit up a little bit so if i bring back that water now you can actually see the led reflecting off the top of this surface right here so that's a cool little feature that a lot of people don't know about you could that's an easy way to add lighting to your designs is to use specific internal faces as an led texture okay so the last thing we're going to do before we close up this video because we've kind of showcased how you can use both a bottom up and a top down approach in this video is we're going to create a new assembly where we have two of these and we're going to join them together with some fittings so let's go ahead and hit save this and then we're going to go new design and let's pull up our data panel and go back to our water cooling loop and let's now add in the reservoir so now the reservoir is going to i need to save that first sorry editable documents okay and let's go back to water cooling loop save this and now we can add this reservoir into this file sorry for that so let's hit ok and right now this is a component that can move anywhere in space it's very good practice when you're building an assembly like this of multiple sub components or sorry sub assemblies or parts the very first one in the top of your tree tree should be grounded what that does is it effectively joins it to the origin point of wherever it currently sits another way to do this is you could open up like your origin point right here and you can join that to the origin point of your design and effectively do the same thing but ground is a very lightweight um way like calculation wise a lightweight way to do that so now this can't move well this one can because we didn't join it so let's join those actually we need to join that in the other design so let's go back to the reservoir we forgot to do it here join hit ok save and now let's check it in the other one so let's update that and good i can no longer move it so the joints carried over from the previous component and let's bring back our glass okay so now we have one so now we can either drag this in as another copied link or we can just copy paste this i'm gonna go ahead and drag it in so we have two hit okay so this one can't move but this one can and what we can do is we can join these two because this is what we care about we care about the mate between these two holes we'll join these together you'll notice it didn't show the whole body but that's okay and then we can do is say how far apart do we want these okay so consulting with my design on my other screen we need them to be 42.6 millimeters um separated from each other so negative 42.6 millimeters and that will set this so now these can no longer move and now we can add in like piping between them so like let's say i didn't want to have that valve and i just wanted to add like a copper pipe to join them so i could create a sketch let's say on let's hide this other component i could create a sketch on this plane right here let's look at it from the side and project that in and i just want to grab this one right here and so we will extrude that as a new component not a new body so that way we can um hide them separately and we want to now reference the inside face of this one so we will go to object here so you'll notice now we are actually back to top down so we built the body and this glass as top down and then we added in the bolts and the fittings as bottom up by having them as separate part files and then we added in this reservoir it looks like this these bolts got a little messed up so i might have to fix that but we added these back in as a bottom up as a sub-assembly and now we've created a pipe that is referencing in the context of this assembly so this is also top down so if i join these together i need to join the outer circle here like that hit okay and let's make it like polished copper so let's do copper polished like that and now i can have a pipe joining those two together so all i would really need to do now is take this assembly let's save it and then i so i've got my fittings my bolts the reservoir and the sub-assembly of both reservoirs together now i could take that whole thing and drop it into my computer design in which i could join it and locate it where i want it and then just start creating all the piping going to all the individual components and the radiators etc so bringing up my previous design you can kind of see what i ended up doing here so i didn't have the copper pipe between but i had the valve but i inserted these sub sub-assemblies of the fans and the radiators and i inserted the sub-assembly of these two and i inserted the pumps and the motherboard which is a sub-assembly with all the various components and the graphics cards which is a sub assembly with its various components and then in this file i could start creating piping linking between all the different components based on where they were joined or mated to and so that was a really interesting way of doing both a bottom up and a top down because i did bottom up by bringing in the separate part files but i also did top down by drawing in components that were exclusive to the context of that assembly so in summary bottom up is kind of like building legos you build your assemblies with individually modeled parts until you have your finished product by contrast however top down would be like starting with a single lego and designing all the other legos that connect to it in the same file but really the magic happens when you understand these concepts and can utilize each in different areas of your design so i would like to thank sebastian from my discord server who requested this topic i hope this helped you on understanding the differences between bottom up and top down as well as best practices for reusing common components between designs if you'd like to support my channel and help me to continue to produce high quality content you can find me on patreon at patreon.com forward slash austin shainer if you'd like to reach out to me with any questions or get help from me or other viewers on problems you are experiencing in your designs you can join our discord server or shoot me an email links will be in the description below but thank you so much for coming i hope to see you all in the next video this is austin signing out

Channel: Austin Shaner

Views: 1,861

Keywords: Autodesk Fusion 360, CAD, CAD Modeling, CAM, CAM Basics, CNC, CNC Router, DIY, Fusion 360, Fusion 360 Beginner, Fusion 360 CAM, Fusion 360 CAM Guitars, Fusion 360 CAM Tutorial, Fusion 360 Tutorials, Guitars in Fusion 360, Tutorials, Xcarve, fusion 360 tutorial, Autodesk, 3d printed knife scales, splines, T-splines, B-splines, Sketch constraints, Sketching basics, Fusion 360 sketching, Fusion 360 Assemblies, Fusion 360 Bottom UP, Top down vs bottom up design, aquatube reservoir

Id: 96pu7HnALho

Length: 53min 42sec (3222 seconds)

Published: Sun Aug 15 2021