Fusion 360 Tutorial – Easy Snap Fit Cases!

hey what's up everybody welcome back to another lair bellaire tutorial in today's tutorial we're going to find out how to make easy snap fit enclosures these type of enclosures that i make are normally a two-piece design where the enclosure piece has these nubs on the side the inside of it these kind of knobs and they connect and lock into this top piece where the top piece has this protruding lip and the lip has this sort of geometry where it locks onto the nub so if we look at this enclosure cross section we can see how it's working because the knob is basically fitted and locked into this area but there's a little bit of tolerance here there's a little bit of gap as you can see and that gap is necessary when you're 3d printing something so this is really good for 3d printed enclosures so we're going to learn how to make these a lot easier than our previous tutorials so let's make a new design and the first i'm going to do is create a new component and i want this to component to kind of contain the two pieces individually so i'm going to call this enclosure and then what i'll do inside of enclosure i'm going to make two more components and this one's going to be the case which is going to be a separate piece and then another one inside of the enclosure i'm going to call this one the top cover this ensures that if we ever need to add on to our enclosure maybe we need a bottom cover or we need a mounting thing all of that can be nested inside our main enclosure so just to kind of structure your project this way is really really helpful and healthy so i'm going to start off with the case because we're going to make first and before i start drawing anything out i'm going to bring up my change parameters window this is the user parameters and we're going to create some parameters to make it easier for us to adjust this design so what type of parameters well for example the width so i'm going to make this width 50 just for now we'll change it later we're going to make the length of the enclosure we're also going to make 50. we're going to make the height of the enclosure let's make that 25 and then we're going to make the shell of the enclosure and put 1.5 and then we're going to make the gap which is our clearance or our tolerances that we'll create that's going to be 0.2 millimeters so again we have the width length height shell and gap so those are going to help us kind of quickly create this thing and change it so i'm going to hit ok next i'm going to do is i'm going to draw a sketch right on this grid here on the bottom and with that created i will start drawing my rectangle and use the r key on my keyboard to bring up the two point rectangle and i'm going to start it from the center here so it locks into the center i'm going to draw out uh instead of clicking and then adding it i'll just type in length here at the bottom hit tab and then this will be width all right so now it's 50 by 50. now that's set i'm going to click on that rectangle hit e on my keyboard for extrusion and i'm going to type in height and that'll make it the height so now i have my box and we can start adding some stuff to it maybe some fillets i'll look at it from the front view hit the f key on my keyboard and then i'll create a marquee selection by clicking on the right and then dragging to the left let the thing go and then it selects all four edges easily so now i'm going to add a value here maybe three or maybe four hit okay so now i have my my nicely filleted box next i'm going to do is i'm going to add a shell to the top here so you click on the top right click and shell is right there for me in this little drop down so click on shell instead of typing some numbers i'm going to type in well shell because that's already set up for us so it's the 1.5 millimeters that we made so now that we have our box um we can play around with the with the diameters or the the dimensions the length for example you should probably make a little bit longer just to kind of go with the name so it's long and you can see that it updates really nice i can also change the height to something a little bit taller maybe 30. all right so now that we know that's working we could also change the shell of course maybe we want it a little bit thicker maybe we want to change it back to 1.5 that works well i haven't used gap yet but we're about to use it in a little bit so now that we need to find out or the next thing we need to craft is the nubs on the inside of our cases so it's up to you to figure out which actual ones you want i'm only going to make two of them and i'm going to pick the left and the right sides they're left and right because they are labeled such here like in the view cube if i click on left you can see that's the left and this is the right or you could do it on the front and the back but it doesn't really matter so i'm going to start up on the left here i'm going to select this edge or this surface because that's where i want the the nub to protrude from so i'm going to start on that with that selected i'll create a new sketch and that'll create a sketch right on top of that surface and kind of project that i'm going to use the rectangle tool again and i'm going to draw on top of this edge as you see my cursor changes and it gives me this little x that lets me know that whatever i draw is going to have a collinear constraint locked to this so basically it's saying that whatever i draw is going to stay locked there so i'll give you an example so i'll click here and i'll draw out sort of a a rectangle here like that there's no dimensions set to it but you notice that the the top here is kind of black and that lets me know that i have a constraint set there and the constraint again is this guy over here this this little icon and that's a co-linear constraint so that was automatically applied to me so whenever i drag these corners you can see i can manipulate the the i can freely manipulate it but what's always happening is that edge is locked to this edge and again that's done with this collinear here when i click on that edge this icon shows up you see that let me do it again click on that edge and then this shows up now lets me know that that is a linear constraint because it looks like that if i delete it with it selected i can hit the delete key and that'll break that relationship we don't need to do that here okay the next thing i'm going to do is i'm going to create a height for this for this nub with that selected i'll hit the d key on my keyboard to make a dimension and i'm going to make this actually the width of the or the the height of this is actually going to be driven with the shell but i'm going to make it double the shell so i'm gonna say shell multiplied by two just like that and it makes it three that's nice and i'm gonna do kind of the same thing for the width and click on that bring it out but instead of adding a number i'm gonna say i want this to be the width divided by 2 and that'll give me 25 because i think it's 50 right now the total width so now i have those locked but it's still free to move i can still move this and it kind of stays locked but it can move outside of the case so to constrain this to always be inside of the case i want to be to the center of this so to do that use the line tool and create some construction lines so do that i'm going to hit the x key and that will turn the construction line mode on as you can see you can turn it on and off here so what i'm going to do is i'm going to find the center of this edge by rolling over until i get this blue triangle and that lets me know that's the midpoint so i can click on that and as you see as i drag my line is dotted lines and that's letting me know that i have a construction line going on here i haven't applied it yet but what i'm going to do is i'm going to try to find the center point of this line here which is our nub and there's the center point right there now it's still free to move i can still move this around which is not good i actually did this wrong i'm going to delete this and the reason why it's wrong is because i was saying from that to this always be centered that's not what i want i actually want i'm actually going to move this away over here and i'm going to say um again with the line tool i hit l from the line tool and then x to turn on the construction line i'm going to roll over this because what i want is i want this line not this line yet so i'm going to click on that and then i'm going to go over to the bottom line of this and then click on that and now you can see that when i move this around that line is moving with it well to lock that line straight on there's a construction there's a there's a construction constraint rule called the horizontal and vertical when you click on that with something selected it'll just make it either vertical or horizontal perfectly straight and now it's fully defined so this is locked i can't move the corners anymore and it's perfectly lined up and and centered because we have those um those construction points like the midpoint is automatically applied for us so it's it's it's following its roles right next thing is i'm going to extrude this out this rectangle and if you add some distance to it you see what it's doing and normally what i would do is i would hit ok and then add some chamfers to this but you can actually if you hit the tab key you can actually do a tapered angle so that's where you kind of get this daily going on right so what i'm going to do is i'm going to put negative 45 degree because 3d printers can print 45 degree features and that's gonna not only does it make it chamfered on the top and bottom but also it chamfers it out uh on the edges here so you see the edge actually gets brought inward which is really helpful for the machine as well the 3d printer so i'm going to hit ok that joins to it uh if i double click on that extrusion you can see it is operation join so it's joining to the case is what you want and that's pretty nice and if we were to test this out let's go ahead and increase the width to like 65 you can see that it automatically updates when you apply that expression that number so it's really nice you can go lower as well and it just shrinks with it so that's really powerful and it's always going to stay in the center because those those midpoint constraints that we built earlier and it's always going to stay at the top as well because we have it locked with collinear so if i change the height to 25 it'll actually drop with it and if i increase it again it goes with it as well so that's pretty awesome so it's a great way to kind of test if your stuff's working out the next thing we want to do is all we want to do is we want to copy this nub and throw it over here and lock it to that area easiest way to do that was with the mirror command you can just mirror that but before we need we need to find out what the the middle point of this and that surface are those two surfaces we can use a construction line a construction plane called midplane which will create a mid plane between two work surfaces or two faces so it's going to be this face which is where our original knob is and this other face where we want the nub to be and of course they're both on the outside of the case not the inside they could be on the inside but doesn't matter so now that we have that we've we gotta hit okay and now we have this kind of um mid plane that we can work with so i'm gonna bring up the model toolbox with s that let's just kind of search for things i'm gonna search for the mirror command there it is click on that and the pattern type i want it to be features because normally what i would do is i'd add faces and then i would click on each individual face and like do that but i don't have to do that i could actually just say features and then i can select this extrusion feature and if i had other features i can actually select multiple features as well and mirror those but i just need this one and then for the mirror plane of course it's going to be the one we created just now which is that one there you can get a little ghosted preview where it's going to go and i'll hit ok and it gets added so the powerful thing about this is that it's just mirrored so if this enclosure height or width for example changes yeah they both change so that's that's really nice now the next thing we're going to do is we're pretty much done with the case in terms of like the nubs we can work on the top cover so when i select that i activated the top cover component and this kind of turned into a ghost lets me know that i'm in a different component but we could still reuse things from the case component we don't have to kind of recreate any of these things so what i'm going to do is i'm going to select this top surface or this top the top face of the enclosure and that's where i want my cover to start from so with that selected i'll create a new sketch and i'm not going to draw anything in here i'm just going to hit ok i'm going to select that inner profile in the outer profile with them selected i'll hit e on my keyboard and i'm going to make this about two millimeters thick and you see it's pulling up that's good i don't want to bring it in because it intersects with it so i want to be two millimeters going up away from the enclosure it's gonna be a new body so i'll hit okay so now that i have that um well what's really good about doing it this way is that if i were to change again if i were to change the the width and stuff it's being driven um with the geometry from the case so the so the cover will always update and always obey the uh the the geometry from the case because it's being driven from it as you can see here the next thing i'm gonna do is i need to create a lip that will kind of mate and lock onto those knobs from the case i'm going to hide the case for a second i'm looking at it from upside down and i'm going to i want it i want the lip to protrude from this surface not the top but the inside here the bottom so with that selected again i'll make a create sketch and what i'm going to do is now that that's um a sketch i have this thing i want the lip to be in to be an offset on the inside of this so there's an offset tool it's called o or up here under sketch it's going to be called offset i just use the hotkey o and then i'm going to select this outer edge here and i want to make sure that chain selection is on because it'll select this whole loop and click on that now it makes it um it makes it out i actually want this to be inward by certain amount and just for just to kind of make fusion understand things i'm going to hit ok and if i double click on this dimension that we set because it isn't offset we can modify the offset i actually want to be driven with this shell and i want to add gap to that shell and that'll make it 1.7 that's because the gap is 0.2 and the shell is 1.5 so if we ever need to change the shell or the gap as you see that i'm doing now it will update that automatically for us so that is really important to know the relationship between those two okay so now they have that i'm going to go ahead and extrude this inner profile i'm going to extrude this inner profile and drive it again with shell multiplied by 2. that gives me i think 3. yeah so now that i have that if i bring back the case you can see that the knobs will intersect with that sort of meat area the inner area so we need to create an indentation a cut out so we can do that by using the sketch that created the nub so i'm going to hide this i'm going to bring back the sketch from the case right i'm going to turn that on i'm still inside the top cover as you can see it's active but doesn't mean i can't use sketches from other components so i'm actually going to select that nub profile hit e on my keyboard if i start if i look at it straight on you can see that that gap is kind of affecting this right so i'm going to do is i'm going to change the start profile plane i'm going to change that to from object and this will let me select a starting point a starting surface i want the the extrusion to start from this surface and you can see that if you look on the side it is now starting from there so now i can do my shell times 2 and then i can tab and then put negative 45 degrees and it makes that that geometry i hit enter pretty quick but that's just cutting that object so now if i bring the case out you can kind of see through the ghost that there's a perfect 0.2 millimeter clearance between all of those faces we can even do a cross section by using the inspection analysis section analysis tool under the inspect drop down and then i'll click on this face for example and then just bring this inward and then you can see in between inside the case here and yes there is a clearance of 0.2 millimeters across all the surfaces including the side surfaces as well just kind of can't really see it there next thing i'm going to do is i'm going to optimize this for 3d printing or actually no as you can see i didn't do it for the other side yet so that's easy all we got to do is apply a mirror so let's do that and turn off the second analysis and i will hide the body for the case so i can just get a better look at this so i need to bring up the um sketch model toolbox type in mirror select it and then i will select that feature which is right here that extrusion i need to select the mirror plane which is this midpoint from the case um the case has that remember so that's why it's a little bit faded out but anyway you can still use it i clicked on it and i'll hit ok and there it is so now i have my mirrored feature the next thing i'm going to do is i'm going to create a shell right on top of this surface so right click on that surface shell and of course use the shell parameter hit ok and take a look at that fusion does such a great job with the shell that it even that even kind of shelled around this geometry here so you if i were to select like this bottom face and this face you can see the distance is yep 1.5 millimeters which is our shell so it's dynamic like that the last things i'll do is to make this a little bit more easier and less kind of kind of reduce the amount of friction and the amount of stress when removing and adding the enclosure you can add some fillets to this area here there's some chamfers actually so i'm going to click on that edge type in chamfer and then 0.6 is usually what i do 0.6 millimeters because any more than that and you you the the thing might not lock onto those nubs so i'll do one over here as well just like that and you can see um it's being applied to that because that's really where the nubs are going to meet so if i were to bring up let's go ahead and activate the entire assembly that way we can look at uh our things here so if i were to move this up you can see kind of how it'll click in like that so it kind of has to flex a little bit so having that shell right here really helped out um making it so that this kind of flexes a little bit and locks in like that hit the revert thing um so that's pretty much it now this is really kind of the the least amount of of steps that i was able to come up with maybe you could reduce it even more but in my older tutorials they were probably a little bit more lengthy because i would end up doing a lot of i would for example sculpt all this stuff out here i will not sculpt it but i would kind of draw it out with different sketches and i'd have a whole bunch of sketches now i'm just trying to leverage all the kind of sketches and construction planes from other components because you don't need to make a whole bunch of sketches all the time so this was a good lesson for me as i keep i keep um making this uh concept in different projects you and you end up kind of figuring out like oh i guess i don't need to do that step or i could reduce that step so hopefully that is um helpful for other people too that may be doing it sort of a more uh sketch approach you know with a bunch of different sketches uh so i've been applying this to a lot of different projects like this one here i also did it to some of the uh different shapes like this hexagon enclosure for the circuit playground if i hide the cover you can see that there's actually knobs on all the edges this was actually done not with a mirror but with a pattern so you can do a circular pattern across all these as well i'm using kind of the same techniques of course with a circle it's a little bit different but it's totally doable where you can you can do these curved nubs so you do it that way and of course the regular rectangle way and again the amount of knobs that you have versus the amount of size that you have it all depends on if you're going to actually put a lot of weight on your cover or not so maybe you don't need so many nubs but in this case there's only two that's pretty much it folks uh let me know what you thought in the tutorial if you have any um sort of tips for people is a great place to drop them and let other people know let me guys know if there's any other cool topics you'd like me to cover but until next time i'll see you next time yeah i'll see you next time

Channel: Adafruit Industries

Views: 271,085

Keywords: adafruit, projects, 3d modeling, tutorial, autodesk, fusion 360, enclosure, design, 3d printing, 3d printed, case, parametric, noe ruiz

Id: VVmOtM60VWw

Length: 21min 53sec (1313 seconds)

Published: Sun Jan 14 2018