Fusion360 Assembly Tutorial; Full practical assembly from scratch

hi everyone today's video is for people who have figured out how to make moderately complex parts in fusion 360 but who are struggling with assemblies and i find that this is also common among people who are coming from other cad systems because fusion 360 does do a few things a bit differently in this video i want to show you how to model this thing right here this is the pump module from the polyvent project it uses a stepper motor up here to turn this lead screw and as that lead screw is rotated this plate here moves up and down and that ultimately causes a bellows which would be mounted between these two plates here to be compressed and expanded which pushes the gas around now i'm telling you that because i want you to know that this is a thing that we've built in austria in real life this is not a contrived toy example and as we were building it we came to a couple of design improvements that we've captured in this new design over here though this design here lacks a couple of the features like the lead screw and the bearings so today we're going to create a combined design that captures the best features of both hi futurantal here this here is the model that we're going to have by the end of today's video the first thing i want to make today is this green plate over here which supports both the motor bracket these vertical routes over here and it also has a pocket for the bearing to go into over here so let's create a new design and here comes the first habit that you really have to get into for every new multi-component design the first button that you really have to press is new component so here i want an internal component i want this to live inside of this file and let's just give that a name of top plate or something we can change our mind later if we wish we also want to make sure here that we activate this component upon its creation next we'll create a new sketch and i'll put that sketch on this horizontal plane over here i hit r for rectangle and select the center point rectangle there and then i'm going to give this dimensions of 80 by 80 millimeters this is mostly an educated guess at this point though we can come back later to change our mind of course it doesn't make any sense for me now to come to these files here and start taking dimensions here that's just a chicken and egg problem then so let's just take 80 millimeters for now and i'm also going to create a second rectangle also from the center and i'm going to make the diagonal distance here let's say 90 millimeters and then i'm going to hit c for circle and create a couple of circles here and those will be the pockets that the rods are going to go into so select all these circles and give those the equals constraint and then d for dimension and make that eight millimeters now one of the things i'm interested in here is to check what the distance is between these two so you just hit d for dimension and you will get a driven dimension here and now i do have a little bit of a problem here because i am getting eight millimeters here which means that the distance between this circle here and the edge of the plate is only four millimeters and a little bit and that is probably not enough for what i want to do later so what i'm going to do right now is just change this distance to 80 millimeters and that will give me more distance here and again if we need to we can make this plate a little larger later on so finish the sketch e for extrude and then we are going to extrude this thing up to let's say 10 millimeters thick the next thing i want to do is create the hole for the lead screw and the pocket for the bearing so i'll create a new sketch and put that on the bottom of this plate and then hit c for circle and then one circle is going to be 22 millimeters that's the outer diameter of a 608 bearing and then the other one is going to be 12 millimeters because i want the hole to completely clear the inner race of the bearing so first i'm going to take this inner bit here and extrude cut that all the way and then i'm going to go back into the component unhide the sketch and then hit e4 extrude and then this thing is going to go up by seven millimeters also a cut and now we have a pocket for the bearing to go into and a hole for the lead screw the next thing i want to do is add the steel rods that come out of this plate and to do that the first thing i want to do is go here and activate this root component over here and once i've done that i'm going to create a new component and i'm going to call that let's say vertical rod again we can change the name later and we want to activate it and again have that internal then i'm going to create a new sketch on this top surface over here and i'll just p for project that top surface in and then i can already finish the sketch now hit e for extrude and then i'll just extrude this downward by some length and again this is going to be mostly a gamble at this point so let's make it 200 and again this is a length that we can come back and change later operation here is going to be new body so click ok and then we have a single steel rod and now we just need to make four of those before we get into that though there is an important problem that we have to fix which is that these components currently can just float around in space like this so hit ctrl z to put that back in its original position and what i will do is activate this root component again on the top left and then i will right click this top plate over here and select the ground so that now means that this top plate can no longer move around and what you eventually want to end up with is one component that is grounded that's usually going to be a base plate or a frame or a casement something to that effect and everything else is fixed or moving in relation to that one grounded component so what i want to do now is create a joint between this steel rod over here and the center of this hole over here and i'm going to select flip here because i do want it to point down and then under motion i want to ensure that i have a rigid and with all that set up i can click ok and now both of these components are fixed in space so now let's create some more of these rods and for that i'm going to right click this vertical rod component here and select copy and then i'll right click the root component and then i can select either paste or paste new now if i want these components to remain the same into the future then i will select paste and if i select paste new then the new component will live an independent life from the previous one now i want these rods to have the same length under all circumstances so here i'm going to select paste i want these rods to always be identical so i hit paste and then i can try to line that up with the hole but that's not going to work very easily because of the dimensions that we had before so i'm just going to drag it out in space over here and then i will create a joint again between this guy here and that guy here and again that's just going to be a rigid joint click ok and then we just have to repeat that two times over so now i can select both of these two vertical rods and select copy and then under the root component paste and then i can just move them over to the side here click ok and then again some joins click on this thing and then if you hit control it automatically snaps to this point of interest there and flip that and do that again for the other rod and there we have four rods the next thing we need to do is create a method for affixing these steel raws into this plate over here and currently our intention is to 3d print this top plate and so what we're going to do is use set screws in embedded nuts and the first thing we need for that is pockets for those embedded nuts so let's first activate the top plate here and create a new sketch on this top surface over here and then from the center of this circle i'll make a construction line and then i hit r for rectangle and create a rectangle like this and then this dimension here is going to be three millimeters and this one's going to be seven and we want the midpoint constraint between this line here and this end point of the line here and then we want this length to be five millimeters so that it is a little bit outside of the outer edge and now we're basically going to repeat the same thing on the other side on the top side and here we're just going to use equals constraint so that we have the minimum number of explicit dimensions to drive this and then these two need to be equal as well so now i can finish the sketch and now when it comes to the nuts you have two choices the obvious choice is to use regular hexagonal nuts but it is much easier to use and to model for square nuts now square nuts you can't find everywhere but if you look around a little bit you should be able to find them you can get them at the hornbach for example but also conrad and a few other places so now i can just hit e for extrude and we want to extrude this to the halfway point plus another half times seven which is going to be three and a half now we can do a little bit better than this so what we're going to do is construct a mid plane between this surface here and that surface over there and then click ok and then we're going to hit e for extrude again on these two profiles now we're going to do it to this object here and then with an offset of three and a half millimeters and in this way if we change the thickness of this plate then these pockets will still come out to the halfway point so now we can click ok on that and we can also hide this construction plane that we just made the next thing we want to do is create the holes for the set screws to go into so let's just create a sketch on this side profile over here and then hit p for project project this rectangle into our sketch l for line x for construction and then just draw a construction line straight down and then hit c for circle and in the center of this line you'd look for this automatic midpoint constraint and let's call that 4.3 millimeters that's a good clearance hole for a m4 set screw now hit e for extrude and we are going to do that to this surface over here and then we are going to enter an offset of five millimeters okay so minus five millimeters and that ensures that this cut ends up all the way in the middle of this shaft and hole over here so that it's certainly all the way through now the one thing you do have to keep in mind is that if you look under here under objects to cut we do want to cut the top plate but we do not want to cut into this vertical rod that's not our intention here so uncheck this and then we can click ok and then we just need to do the same thing on the other side so now we just go over to the other side create a new sketch here p for project x and l c circle 4.3 here for extrude and again to an object with an offset of -5 and again under objects to cut make sure that you uncheck the vertical route next thing you want to do is ensure that all four of these rods have these pockets so under create we go to a circular pattern and then the type will be features and it'll be this guy this guy and this guy and that will go around this axis over here this bore of the bearing and then under the quantity we want four of those and then we can click okay and then we have these pockets on all four corners of this plate the next thing i want to make is the bottom plate and that's going to be largely identical to this top plate over here but slightly different so for that i'm going to copy this top plate activate the root component and do a paste new in this case because again i want this thing to be not quite identical to the top plate so i'm going to pull this thing down over here and in this case i can probably align that exactly like so and then we can click ok now of course at this point this new plate is free to float around like this so ctrl z and then we can use a different method to fix this one in place so in this case we can use a rigid group i'm going to capture the position we're going to create a rigid group between the rod and this bottom plate and the advantage of using a rigid group is that for very large assemblies it has better performance compared to using joints that are set to a rigid motion so now we can click ok and now i'll go over here and first rename this thing to bottom plate and i'll activate this component and then we can go onto the timeline here and start changing some things up so the main thing that i want to do is find the sketch that is responsible for this feature over here and that is this sketch over here and we are going to redefine its sketch plane to be on top here and for this it moves itself back up to where it came from but that's okay so now that we've redefined the sketch plane we see now that the bearing pocket and this through hole here have reversed and so now we can put the bearing here but on the other end the bearing is over here yet at the same time the nut pockets are still all facing upwards on both of these parts one thing that i should point out about the timeline in my case is that i have this tick box enabled the component color swatch and that assigns a color to each of these components here that you can see with this small stripe and those colors match these colors above the features on the timeline and the other thing about the timeline that you may have seen just a moment ago is that if i activate a certain component the timeline constrains itself to that component and also the possible sub-components that we'll get into later the next thing i want to check is whether i can change the length of the rods while still keeping the model intact so i'll activate the root component and then if i have the color matching here i can easily see that this is the feature that i need to edit so let's make these rods a little bit longer at 220 millimeters and now in this case i see that the bottom plate hasn't moved while it should have so what i'm going to do is delete this rigid group that i've made and instead i'm going to create a joint i'm first going to select this hole here on the plate and then the end of that rod again i'm going to flip that just to make sure it's in the right place and that looks about right so we can click ok the motion is rigid so that's good and then once that's all set up we can go again into this thing over here and let's make that minus 180 or let's change it back to -200 and then everything keeps on working without any additional effort on our part now i want to modify the appearance of this model because at the moment it looks a little boring and white and here i really want to stress the difference between two different concepts one is the physical material and this has the full information of a particular material so strength properties thermal properties all those kinds of things and what we are going to do here is appearance which only determines how something looks now if you're interested in the total mass the center of mass moments of inertia thermal stimulation stress simulations all those kinds of things then you will need to have physical materials associated to all of your parts if you are interested in those kinds of things it may also be important to explicitly model all of these missing set screws and embedded nuts as well because those will affect for example the total mass and the center of mass for today though the only thing we're going to do is appearance and the first thing i'm going to do is look in the library for steel and then a stainless steel polish looks rather nice and because again these four raws are all linked they are always identical the other thing i'm going to do is duplicate this basic abs material that we started with and i'm just go i like to just apply bright colors to my parts just to make everything stand out from each other so you can just duplicate this edit give this a name let's call this red i'm not generally more fancy about it than this and just drag that onto the parts and then i'll edit this to be named green and then at least this far we have applied appearances now let's get back to actually just modeling stuff and the next thing i want to do is add the bearings that go into both of these pockets so first i'll activate the top plate component because i want this bearing to be a sub component of this top plate and then i'll go to insert insert mcmaster car component and then i can make this window a little bit bigger and then here we're just going to type 608 bearing and then here we are and then let's suppose that we are going for a sheet for a sealed bearing a 2rs bearing and then i want the product detail here and this icon over here tells you that a cad model is available so in our case we need a 3d step download and then we get that model in here so here i just recommend dragging it to a place where you can see it and click ok and then the next thing you can do is just make a joint between this guy over here and then this point over here and click ok on that and then the final thing you want to do is make this a 608 2rs just change the name from the default now of course we also want a bearing in the other plate so what we're going to do is copy this guy over here and then we activate this bottom plate we do paste because in this case we want the exact same bearing again we just drag this down to where we can see it we don't want to drag it directly into position and again we create a joint on this to this and click ok and then we have both of our bearings in place the next part that i want to model is the lead screw that will go through the middle of all of this so let's activate the root component and create a new component that i will call tr 8x8 lead screw or just tr 8x8 that's fine now create a sketch on the bottom of this bottom plate here c for circle make that eight millimeters finish the sketch e for extrude and then i'm going to extrude that all the way up to the top plate so to object this thing here and then we're going to give it an offset of 20 millimeters so it pokes out a little bit here and that gives something for the coupler to hang on to so click ok on this and then the next thing i want to do is go to thread here under create and then i'm going to select this thing here and then here we have the isometric trapezoidal threads and unfortunately the tr 8x8 is not available here so we're going to have to settle for this if we really need the exact thread for modeled we can do that if we need to but that's a bit too much effort for now the only thing that i want to point out here is that you have this tick box here for model threads or not model threads so if i tick that we get the real model of a real thread and if i untick it we only get really a cylinder with a texture on it now the latter is much better for your performance which is especially important if you have lots and lots and lots of screws that you have applied such a threat to the next thing i want to do is create a joint for this new lead screw so the first thing i'm going to do is activate the root component here and the way that i've done this i already like the position that this lead screw is in and because of that in this case i'm going to use the as build joint command so i want to joint this component here to this top plate over here and the joint type here is going to be a revolute and fusion wants us to put an origin for this revolute somewhere so let's put that in the middle here and that is looking pretty good to me so click ok on that and now we have this lead screw jointed to the rest of our model the next parts that i want to add to this design are the shaft collars that are going to hold this lead screw in place now to keep the file organized i want these to be sub components of the lead screw so i'm going to activate the lead screw component first and then insert a mcmaster car component again then we are going to look for a shaft collar and then we want a metric one of course and i want a one piece design and here we want a clamping shaft collar uh the type of shaft collar that pushes a set screw into the shaft or in this case the lead screw doesn't really work so it has to be a clamping variety now i don't want any of the aluminium ones and i also don't like black oxide so i'm going for this 303 stainless here and then download the 3d step and then we can put this off to one side here and now we need to make this joint and that's going to be a little bit more complicated now what we want to do for this joint is joint up the center of the shaft collar here to this lead screw but when we try to do that we can only snap it to either the middle or the ends of the lead screw and that doesn't really work now what we want to do is put it right over here but if we select it in this kind of a way then it will actually be jointed to this top plate and that is incorrect we want this jointed to this lead screw so what we're going to do instead is create a new sketch on this plane over here we're going to capture the position here just to make sure that this lead screw doesn't fly back on us and then we can just project this into the sketch and then finish the sketch and what we can do now is create a joint between the shaft collar like we tried before but now we can joint it onto the sketch geometry that we have here and now we can click ok on this we have a rigid joint so that looks good and now we have this shaft collar jointed to this lead screw as you can see like this as i'm turning this lead screw the shaft collar turns along with it and coincidentally so does the sketch so the next thing i want to do is create the next shaft caller and so first i'll go in here and rename this eight millimeter shaft collar again you want to have names on everything so you don't lose track of what's what i can now hide this sketch over here and the first thing we'll do is create a new sketch on this bottom plate here we can just press continue here we don't need the capture position we project all this stuff in so we get this center point of the circle now we can already finish the sketch we copy this thing and then again we press paste new paste on this here so paste here and we do it on this component here and not on the root component because again we want the shaft collar to be a sub component of this lead screw because that keeps everything a little bit more organized so now we can click ok and then finally we can do another joint between this guy here and this sketch point over here and here we want to flip it so that it comes out on the other side and then we can click ok on that and now we have two shaft collars to keep our lead screw in place and as we turn this they both thrown along with this lead screw so final thing here hide the sketch and we're ready to continue now one thing is a little bit weird here we have this component here that contains the lead screw and it has in a way three sub components the lead screw itself and the two shaft collars but the lead screw is a body while the shaft collars are components and that's just a little bit weird it's weird to treat them differently like that so what i'll do is create a new component and i will create that from a body and that's going to be this body over here so this single body here and then click ok but the issue now is that our joints are a little bit messed up so now this new thing here can just float around like this so what we can do for example is do an ass build joint now between this guy and this guy here and that's going to be rigid and now we have a revolute joint here between the root component or rather this top plate here and the whole lead screw component as a whole and then within that lead screw component as a whole we have these sub components that are appropriately jointed so now if i animate this model here we see that both of the shaft collars are turning correctly and also that the lead screw itself is also turning so now we fix the organization of the file a little bit while also making sure everything still works the next part that i want to add to the design is going to be the stepper motor that goes on top of the lead screw to turn it now the first time we built this thing we used a nema 17 stepper motor but we quickly found out that that doesn't provide enough power so in this case i want to use a nema 23 motor now mcmaster car has a couple of these in the catalog but not the exact one that i want to use and that is important because the length between them varies a little bit so i'm going to create a new design i'm going to create this motor in a separate file because i might want to use it in other projects as well now for this motor i'm going to be using two components the first component is going to be the motor body and the second component is going to be the motor shaft that will stick on the end with a revolute joint and now designing this motor is fairly straightforward you can find technical drawings for the face plates online and then some of the other measurements like the thickness of the faceplate and the length of the motor you can just measure on your motor so i'll just design this motor real quick here's the model for our motor we simply have a motor body with a shaft the body is grounded and then the shaft has this joint here so that it can spin and what we need to do now is insert that into our overall design so what we can do is open up the data panel here and then look where this motor is and then we right click it and then we do insert into current design and then i'm going to move it up a little bit and then rotate it because i just want to put it in rough position right now because the next thing that we need to make is a bracket so that this motor can be held there i want to pause here though to emphasize the difference between how fusion 360 handles files and components and assemblies versus how other cad systems might do that so in most cad systems you have parts that live in part files and so every part has its own little file and how they go together is described in an assembly file and then an assembly file can also reference other assembly files making those sub-assemblies now in fusion 360 there is no distinction between a part and assembly both of those things are a component now what you can also see is that every file can have has this root component to begin with but can also have components that live inside of this root component and components that live inside of those and so that is the fusion 360 equivalent of having an assembly with sub-assemblies and sub-sub-assemblies now if you want to you can just make a single part inside of a single file and then use the method that we use to import this motor to make what is essentially an assembly file if you are on the hobbyist license though that becomes a little bit tricky because you are only allowed 10 editable files at any given time and that becomes a bit of a chore because most of your product will have many more than just 10 parts whatever the case may be let's get back to this motor bracket thing so i'm again going to create a new component that i will call motor bracket and then i'm going to right click on the motor component here and select isolate and then i'm also going to unhide the motor bracket by pressing the little i here and that ensures that i can work on this without getting distracted by all the other stuff in the file so now i'm going to create a new sketch on the face here of the stepper motor i'm going to project all that in then i'm going to offset this circle to give me a little bit of clearance and then i'm going to create a rectangle out from the center and it's going to be 80 millimeters to match the width of the linear stage itself and the other side 60 millimeters should be enough so now we can hit e for extrude on both of these profiles and then let's go down here by about 10 millimeters now let's create the vertical legs for this bracket so i'm going to this surface over here and create a sketch and what i'm going to do first is create a construction line from the middle to the origin here and also from the origin vertically like so and those are going to be used as mirror lines in just a second i'm also going to draw a construction line here and a regular line like so and then we are going to put a circle here now i'm going to use m4 screws to tie the brackets to the rest of the assembly but i actually need eight and a half millimeter holes here because i want the full screw including its head to go in there so let's put this guy now let's say 15 millimeters above that center line and then i want these three lines to be symmetric like so and now we can check well first let's put in the polygon here so i want to use m5 screws to tie the motor to the motor bracket and so that means that this is going to be vertical and this distance is going to be eight millimeters because that's just the distance between flats of an m5 nut that i'm going to embed in here so that i can tie the motor in with an m5 screw so now we can figure out how much distance we can have here so let's try 10 so that still fits does 12 fit so 12 still fits that's nice and now we have 1.75 millimeters worth of meat here that's not great so let's see if we can improve that i'm going to create a center point arc here between the center of that circle to this line over here so let's make this coincident as well and then let's give this a radius well not of nine apparently but we can do eight millimeters here and now we're going to do a little bit of mirroring so we're going to pick up all of this stuff here and mirror that along this line here and next we're going to pick up all of this stuff and mirror it across this line here and now we are ready to extrude but first we need to figure out how far to extrude all of this so let's un-isolate this motor over here so that everything else comes into view and then i can see that if i select this surface over here to this surface over here that there's 21 millimeters so the shaft here is 21 millimeters proud of the bracket and if i go to the other side here we see that here these lead screw is 20 millimeters proud of this surface over here so in total that means we need 41 millimeters but we also need a little bit of space for the center part of the coupler to go into and so what i'm going to do is extrude this 55 millimeters so select all of these profiles and then do 55 millimeters and click and then the next thing we're going to do is go into this component over here and then unhide the sketch i'm going to take these hexagons here and do that -4 so that we can embed the nuts and we are also going to take the left click and hold this profile here here here and here and we are going to extrude that upward to this face over here and so the idea now is that we're going to take a screw and drop it all the way in there so we're not quite done yet with its bracket the next thing that we're going to do is create a sketch now on the top surface here i'm going to draw some lines out from the side here and make sure that those are tangent to this circle and then make them horizontal as well and that immediately completely constrains them and then i'm going again going to do the same thing with the construction line to the center like so and then again we can do some mirrors so mirror that this way and then take all of this and mirror it that way finish the sketch and next we can take these profiles over here and then extrude them to the bottom of the bracket and then we are going to offset that by 10 millimeters and we need to go in the other direction so like so and then we can click ok and then the next thing we are going to do is go to the bottom of this bracket and do the same kind of a thing so let's create a circle here of 4.2 millimeters that's going to be a clearance hole for a screw and let's just do the same thing on these over here let's make all of these circles equally large finish the sketch e for extrude and then this here is going to be 10 millimeters i don't think i did that right i did not 10 millimeters and now what we have here is here we have a place where we can put the screw in and there is also space here for the head of the screw and then it's going to stick out the bottom through this hole here notice also that in the last operation we also created these hexagonal pockets for these five millimeter holes over here and those line up exactly with the motor and of course that alignment is automatic because we projected the front face of the motor into that sketch now at this point we can start doing some more joints so let's close up a couple of these things that we don't need and the first joint i'm going to make is an ass build joint and that's going to be between the body of the motor and this motor bracket and that's going to be a rigid joint and the next thing i want to do is joint the motor bracket onto this blade over here and again for that we're going to create a quick little helper sketch so i'm going to create a sketch on here and create a construction line so let's project first and then create a line from the center here to the center there then finish the sketch and then we should be able to joint this point over here to the center of that bracket over here now at this point it only shows the motor bracket moving but as soon as i click ok on this first check the right motion then the motor will also come along with it and here we see that we have a little bit of space now between the two shafts and that's where the central bit of the coupler is going to go before we get into that though i'm first going to activate the top plate component over here and create a new sketch here on this bottom surface here and then i'm going to project these circles or these cylinders rather into the sketch and click ok and then concentric with those i'm also going to add some circumscribed polygons i miss clicked there i'm going to make all of these vertical next i'm going to make all of them equal as well and then the distance between flats is going to be seven millimeters because this is going to be for an m4 nut so e for extrude select the holes first go this way all the way and then under objects to cut if everything's going all right we will only be cutting through the top plate so click ok and then we're going to go in here and unhide the sketch e for extrude again and then we are going to extrude this minus three millimeter to create a pocket for the nuts to go into and i want to move on to what's probably going to be the final major part of today's video and that's going to be this follower over here so this thing is going to take that rotary motion from the lead screw and turn that into this up and down motion and as it does so it has these linear bearings to slide over these two rods over here so this is a component that has a whole bunch of sub components inside of it so we can immediately take that into account so let's activate the root component and let's first create a follower component and then once that component is ready and active we can create another new component and let's call that the thrust plate and now we can start modeling so i'm going to create a sketch and i'm going to put that sketch on the bottom surface here of the shaft collar because that's effectively going to be the end of travel of this follower next i'm going to include some geometry via intersection and that's going to be two of these vertical shafts and then the center lead screw over here and click ok and now we can isolate this component that we have here to ensure that we just get what we need here and we don't get distracted by everything else so at least on the outset i'm going to make this plate rectangular and i need to use a three three-point rectangle here because the it is not horizontal or vertical with respect to the coordinate frame so i'm going to make a construction line now diagonally between these two lines here i'm going to do c for circle that needs to be a knot construction line and this is going to be 15 millimeters also a circle here and a circle here this is going to be 10 and a half millimeters that's going to hold the t-nut the trapezoidal nut and of course these two have to be equal these two lines here have to be symmetric around the center axis and then we can start figuring out if i select this sketch point here how far i want to have this apart and now i need seven and a half millimeters for the bearing to begin with and then i also need about uh seven millimeters for an m4 nut because i want to clamp the shaft or the linear bearing in place with it so here i'm going to select 20 millimeters just to be safe and then i'm also going to create a construction line like so that doesn't need to go to the midpoint that just needs to be perpendicular like so and then i can make this symmetric around the middle as well so that the other side is also good driven by just a single dimension and then finally hopefully we're going to fix this and i think 30 millimeters will probably do the business probably need a little bit more uh for some of the stuff we need to add later so finish the sketch now we will un-isolate this and then we can hit e for extrude and then here we have a little bit of an issue that we have because we started the sketch on this thing over here so let's see what we want to do here actually we just want to extrude all of it so we want to extrude this and next how thick do we want this plate to be or i think 10 millimeters will do that looks about right to me so click ok and let's continue the next thing i want to do is create the holes for the push rods to come through so i'm going to create a sketch on this surface over here and then make a circle in the middle and let's give that a diameter of 30 millimeters and i'm again going to isolate this component here so i can see what i'm doing this can be construction geometry and then i will draw a construction line like this so that i have this point over here and then i'm going to create a four millimeter hole for four millimeter rods i'm going to create a circular pattern of this circle around this center point here and i'd like to have four of these rods and click ok finish the sketch e for extrude and then i'm going to extrude these four circles down this way all the way and the interesting thing here now is that under objects to cut we only get this thrust plate now so if we do this and we un-isolate this component here we see that there was a lot more stuff above here through which we could have cut but we didn't do that and we couldn't do that because that stuff was hidden so now i'm going to create the push rods themselves and for that i'm going to activate this follower component here i'm going to isolate it again and i'm going to create a new component that i will call pushrod and for this we're going to create a sketch on here project this in and then we can simply take this bit here and extrude that downward by let's say minus 250 millimeters again we can change our mind later now what we did before is we did a copy and then a paste new but that is actually a massive waste of time so what we're going to do instead here is a pattern a circular pattern of type components specifically this component here around this axis here i want four of those click ok and then finally i'm going to do a rigid group between the thrust plate and all four of these push rods click ok and then we have all of our push rods in place now when i go back into the root component and un-isolate this follower here we will see that we have these rods now sticking through this bottom plate over here and fusion 360 has a tool to automatically detect such things which is the interference analysis so we can just run that analysis on the root component and press compute and then what we get here is that we have four push rods that are interfering with the bottom plate over here and we also have the volume here that they're interfering in highlighted and we also use this tool before for example to check the meshes in the gear tutorials that i've done so this is a handy tool to have but let's move on with modeling at this point our pusher plate sub-assembly is still able to float around like this so of course we now want to joint it and for that i'm going to use an as build joint and it's going to be a joint between this thrust plate here and i'll take this vertical rod over here and let's put the origin of that joint over there and then we can click ok and now we can drag this thing up and down but it can no longer float around otherwise but one problem that we do still have is that it can just float straight through this thing here and also at the bottom here so that's up next to fix i first want to fix that interference that we had here at the bottom plate so i'm going to activate this bottom plate component and create a new sketch on the bottom surface of that plate and then hit b for project project these push rods into my sketch click ok and then i'm going to create some circles concentric with those push rods and then i'm going to make those all equal sized and that size is going to be six millimeters and that will either give us enough clearance so that we don't have any rubbing or we can put a bushing in there because the outer diameter of a bushing will be six millimeters in that case so we can just uh extrude this up up to this top surface over here and then we just have to ensure under objects to cut that we do not cut the push rod and click ok and then we should no longer have any interferences so inspect interference on the root component compute no interference is detected so now let's turn our attention back to that slider joint over here and the first way that we can fix this slider joint going through other components is by enabling contact sets so under assemble i will enable contact sets and then ensure that all body's contact is enabled and now i can push this thing up and down but as it hits either the bottom or the top it will basically stop there however this isn't completely perfect because if i basically apply enough speed i guess i can just phase through this wall over here so contact sets can work okay but they don't work that great and also i remove this interference here first because if you have an interference like that a contact set will basically bind up your model entirely and finally contact sets can also be quite difficult to compute so with all of that they are not a great solution but sometimes they are the solution that you want so for this model i'm going to disable the contact set i don't really find that as a great solution here and i will go to this slider joint and set that to zero and then i'm going to add some limits to this joint so the joint limits here are going to be a minimum of zero and then the maximum is going to be probably something like 150 so we can animate that it's going to be actually the reverse in this case so minus 150 to zero and then we see that we don't get all the way to the bottom here so we can actually cancel this for a minute and figure out how far this needs to go so we can just drag that down here and then we can read here that this is actually minus 150 so that was almost correct so let's now actually set those limits and the limits here again are going to be a minimum and a maximum with a minimum of minus 150 and a maximum of zero and then if we animate this we see that we get basically the right idea and once we click ok on that and we add and we just drag this up and down we see now that we have actual limits that we can't pass through by just applying enough speed that doesn't work and also now the push rods are again coming along again in the animations this doesn't always happen usually it doesn't but once you click ok everything will snap into place as expected the next thing i want to do is ensure that the rotation of the lead screw is tied to the sliding of this pusher plate here so for that i'm going to create a motion link i'm going to continue here i don't need to capture this position and the joints that i want to link are this rotating joint here and this slider joint here and what we want to do here is ensure that if we have a 360 degree rotation then this thing has to slide eight millimeters so click ok on this and then the next thing that we have to check is ensure that if we go in the right direction that we have the right direction on the slider and the rotation so right now it appears to be reversed because as i'm turning the lead screw i actually see the threads moving upwards from this perspective and at the same time the lead screw or the pusher plate is actually moving downwards so let's go back into this feature here let's just change this into -8 animate this again click ok and now we should see that as the threads here move up that the pusher plate also moves up along with it now the relation here isn't exact because on this texture here when we made this lead screw again we had that one and a half millimeter pitch or the one and a half millimeter lead between the full rotation that's a tr 8 by 1.5 lead screw but the actual lead screw that we want to use is the tr 8x8 which we don't have stock in fusion 360. again if we want full accuracy there we can model that correctly if we really need to one small detail that i also want to point out is that because there is a motion limit on this joint over here on the slider joint that also means that kind of automatically there's also a limit to how far this lead screw can turn because at some point if you try to turn it further you just conflict with this constraint that we have here so we don't need to do any extra work for that the final thing that i want to do for today's video is add the shaft coupler that are going to couple the motor shaft to the lead screw and for that i'm again going to insert a mcmaster car component and that component of course is going to be a shaft coupler and then it's going to be for round shaft metric clamp on and then this is a model that i do like i don't intend to buy exactly this one but it looks a lot like the one that i do want to buy so let's go for product detail it's going to be 3d step again download and let's put that off to the side for now and then what we're going to do is create a joint between this guy over here and the center of this shaft over there and then we're just going to move that up by let's say 10 millimeters click okay and now we want to see whether that actually fits any good so what we're going to do now is go into the origin here and then we are going to do a section analysis on this vertical plane over here click ok and now we can see that the coupler is actually a little bit too far above here so we're going to go back into this joint over here and move that down just a little bit like so click ok we could maybe have a little bit of less space between the motor shaft and the lead screw but whatever that's fine now we can hide the analysis here and the next thing we are going to do is an as built joint between the lead screw and this coupler here that's going to be a rigid joint click ok and now we should see that when we animate the model on this guy that the motor shaft is forced to turn along with it and we can also do that from the other perspective here so if we animate the model here we see that it works like that now here it runs into that motion limit again so let's just drag this down a little bit to the center like so and then again do animate model on this guy and we see now that we've basically coupled both of these rotating joints via the two rigid joints in this coupler so that's mostly the end of this video there is of course still a lot to do on the model itself but most of that should not present any new challenges uh all of the stuff that i wanted to teach you and show you today have basically been done so with that i'd like to thank you very much again for watching especially if you've made it all the way to the end of such a long video if you have any questions or comments about anything that i've shown you today you can of course leave those down below and if you don't mind you could hit some of the algorithm tickling buttons to help the channel out with that thanks again for watching and have a great night

Channel: Antalz

Views: 39,716

Keywords:

Id: HiSOCPizpCo

Length: 54min 3sec (3243 seconds)

Published: Mon May 03 2021

Reddit Comments

[u/Donorob]

Looks cool, I’ll give it a go thanks