 Hey, what's up folks welcome back to another layer by layer in today's tutorial We're gonna take a look at making snap fits using the sweep features and Fusion 360. Let's jump into this week's project So this is a little four-button keypad It's in the shape of a kiddie paw and there's a little display in the center there The idea is that this can be a USB controller or a midi controller if you want to do some music There are some cherry MX compatible switches some kale switches on the inside here and it's a snap fit enclosure that has a Really interesting way that it uses the snap fits they actually sweep along the path of the shape here So in today's tutorial, I want to show you how I put that together and some of the things to watch out for When you are using the sweeps command feature in Fusion 360 This was inspired by this little key cap by the way This is a little kitty tobing key cap that you put on a standard cherry MX compatible Key and that's really where it came from So here's this and then here's this ridiculous fun tobing thing and there's actually kale switches on the inside of these Like that. So if you want to build this, you're in luck. We have a learn guide that is Out in public so you can check it out. I have all the all the Fusion 360 files STL files as well full circuit diagram code code walkthrough wiring assembly It is all ready and and released for the world So if you really want to build your own you can follow along with the tutorial or if you want to use some of the parts That were used in this project. I have a lot of the 3d models like the Qt Pi RP 2040 available under GitHub repo I don't promote that enough and I really should so check that out. You got a link there I also have it in description of this video, but with that out of the way, let's go ahead and jump into Fusion 360 This is the kitty pad. This is what it looks like As a cross-section view you have a standard kind of 3p setup I have a front cover a bottom cover and a frame and these three kind of work together This right here is a key plate. Don't worry about that. It's really this that we're going to do We're going to figure out how to create the snap fit geometry for a very bizarre shape like this Cool Let me show you a quick the cat animation of this thing so I can show you kind of what the pieces look like Normally what I like to do is I like to have a 3p setup for an enclosure I have the frame which is normally something like this and I have two covers one being the top and one being the bottom Now the top and the bottom and the frame are all using the exact same sketch They just have some offsets that are built in so That is going to lead me to ten pole the last tutorial I did was focusing on how to create this kittypaw shape using the spline tool in Fusion 360 and then using sketch constraints like this like the symmetry and the equal the equal That's the name of the of the sketch constraints. It's called equal so definitely check that out. It's like a good half an hour of Walking through setting up Symmetrical spline so this shape is completely done with the spline tool. It's a complete closed loop. There are Bezier curves and the bezier curves are actually symmetrical So when one side gets changed the other side Reflects that change also the placement and position of the points are also mirrored They're mirrored and they're symmetric Actually, they're not mirrored. They're just symmetric. I get that this is confused But yeah, definitely check out the tutorial. I have a link in the description of course to that video and you can see how to how to Create a symmetrical spline shape like this because it's all done with the spline tool Now you could use a different program to create your your geometry like this But I tend to stick with fusions tools because sometimes when I bring in geometry from outside Things like illustrator. It tends to not work that well in fusion 360. So that's why it's a spline tool All right, so with that in a way, I'm gonna kind of step through this thing We're just gonna start off as if we have our sketch already laid out and we're ready to kind of start extruding so the first thing is to extrude it and The reason why I have this extrusion so long normally my extrusions are like one and a half millimeters But this time what I really want to do is to add more geometry so that I could really add a fillet on this on this bottom Edge here so that I can have an extreme fillet like three or four millimeters So that's why I have an extra extrusion. Okay, so that's this shape It's just a standard extrusion. The next thing is to kind of create another sketch and Project in this geometry and then do an offset, right? So the idea here is it's just gonna create a bit of a cavity for us so that we can optimize the print a little bit It doesn't have to actually be this thick so we can kind of eat away at this right here to kind of make it thinner So that's why that sketch is there The next sketch is what we're gonna use to create our snap fit geometry. So let's jump into this one Really, let me kind of recreate this just kind of show you so I'm gonna activate my component so I can work within it and When you do a inspect go to section analysis you can select any one of these default construction planes these little these little orange squares So I'm gonna click on this one and that gives me a cross-section of this of this of the side, right? So now I can see this is actually where I want my sketch to be so hit okay, and now I'll grab a Create sketch making sure I'm in the component and then I'll use that orange triangle to draw my sketch so Let's go ahead and just kind of create the geometry and I'll show you why you would want to do segments in your sweeps so for starters, I'm going to Grab an edge right so let me turn off the the analysis you can see my grid still here What I want to do is I want to project in this line or any one of these like if I were to bring this in I Could project that in but really I just need this line here Because I need a reference point to kind of work off of and this is kind of my my point So I have that selected I'll hit the the hot key P Which is the hot key for project and that will project that dot into the sketch and it'll show up as a purple dot That lets me know that it is a referenced projected geometry So now with that I can start drawing out my my shape for my for my my snap fit So it's gonna be a triangle so something like this and I just kind of freehand draw it The only constraints that are set up is this one here, which is perfect. That's the horizontal constraint That's what I want and I wanted to find this to be two millimeters tall And then I wanted to find these two lines to have a 45 degree Okay, and then I'll grab these two lines Right with the shift select and then I'll tell these two that they need to be perpendicular so that they're square All right, so that is my kind of base Thing and the next thing is to draw the this the lines that will create my kind of my shape to grab So it looks like this it goes out I want to make sure that there's a perpendicular constraint there You can see that fusion just automatically adds that for me as far as the length I'm just gonna freehand it right now click down I want another perpendicular constraint at this corner here between those two lines And then I also want this right here to be lined up nicely. So until I hit That right there that lets me know I'm perpendicular with that last line and I can come in here and then be perpendicular with this line up there and then that closes the shape The last thing I need to do here is to add a dimension a sketch dimensions to this line And this line is supposed to be kind of diagonal like that at a 45 degree and I'll make this one and a half millimeters All right So that now I can grab this whole shape and then I can tell it where it needs to go so I actually want to create a Line that connects these two dots this dot to this dot Okay, and then I want this line to be straight going across horizontal so I apply it a horizontal constraint and now I need to do is add a Little bit of a dimension to that line how much I'm gonna put two for now Two, okay, and then I can grab this line and then say I want this to be a construction line by hitting the x key Let's go ahead and do that to this line as well. And then that's Construction line by hitting the x key. So now what I can do is I can only select the geometry that I want Which is this thing here. Perfect. So now with that done. Let's let's apply a sweep to it, right? So again, if we do a section analysis, you see it's right in the center of our of our shape and our shape is Symmetrical and that's really super important. Okay. Well, let me turn off section analysis and then bring up my sweep command There's sweep. I just brought up the design shortcuts with the s key by the way My favorite thing of fusion is the s key wherever you hit it. It'll show up. So wherever your mouse is That's where your menu will show up. So let's say you want right here s key Sweep I don't even have to spell the whole word just a couple letters and here's the sweeps You want this one the blue one because we're in the solid workspace hit sweep first thing you need to do is select We'll leave this that single path the type and then for the profile I want to select well this profile here and then for the path we can select this entire thing Boom and right away. It's like it's done now. That's okay. If you have a pretty simple Design that doesn't have any components on the edges you can do that just fine hit okay, and you're done Right, but I had to be strategic about this because if we look at our kitty pad, let me go back to the design here You have to let me show you the Kind of remove this get rid of that Whoa, whoa, whoa slow down and then get rid of this We're just hiding it get rid of this this top cover what I'm trying to show you is the the components that are Uh need to be accounted for right? So I have a display. It's right here. I have this frame here Let me get rid of the frame. We're almost there folks, and then the cutie pie is right here Let me do a full activate the whole thing now. Look at that. You can see here that If we had a sweep going across this entire shape we would be intersecting the PCB here So I strategically said that I'd like to only have sections so that I can accommodate for my Not only just my components, but I it gives me the ability to actually wedge a spudger between the frame So that I can actually take it apart if you ever need to take it apart you need some area To kind of wedge your spudger tool into and that is why I have it segmented like that That's why there's this this separation between these these kind of snap fits And that just makes it so that it is easy to open and accommodates for that USB port So if I had the sweep going across this whole shape here, you'd see here that I wouldn't be able to do this hole for the USB port So that's why I needed to be strategic about the the type of sweep. It just can't sweep along the whole thing So I'm gonna go back into it and you have some options here So the main options is these two distance types And really the way they work is you have two of these arrows and you can define how much you want here so as you kind of drag this handle out you can kind of define how much you want and There might be an issue here. So let me Say like okay, so I have these two values here and let's say I want them to be the exact same. So one one five They're not actual numbers or more of a It's like zero to one is is basically how this works the distance. It's more of a bit of a percentage Just a whole number is one is a hundred percent and this would be like point I don't know ten percent or so So that's how that's working. So those those values are the same Now you want to be attention you want to pay attention to the orientation Perpendicular is the right one you want and then for the operation we want it to join because that's that's gonna join it To our solid body here. So I'm gonna hit okay and Sometimes it works Sometimes it doesn't and in this case. Well, it didn't fusion has a warning It says I could not do this. This isn't valid and that's kind of BS. It really is valid I mean it did it here it is but that's because of something else. So what happens with this is that we kind of need to Just do one side. So I'm just gonna put zero and one and then leave one of them here like that and hit okay It still gives me that error. So I'm gonna go back into it and hit okay. It keeps doing that over and over again so hit okay and This is where we let's try to let's try to reverse this. So let's grab this distance Put zero here and then put it on that side hit okay Okay, it's still not let me do it. So what I'm gonna do is actually delete that Because this is really shot highlighting how ridiculous you can be with these sweeps, right? So I'm gonna try again So I deleted that I'm gonna select the profile and select our path this the shape right here and Instead and you know instead of hitting okay, and then going back into it. Let's try that again that zero point 115 and Then hitting okay It's still not let me do it. It keeps giving me errors and this is the problem I kind of kept having with fusion I had to keep kind of messing with the with the thing until it let me do it and In this case, I think it's not let me do it at all, which is unfortunate. Yeah, look at that. It's going really book bonkers here Yeah I'm gonna keep trying though. Let me try the bottom sketch Maybe that'll work. You see how like I kept using the top now. I'm gonna try the bottom Okay, that's still didn't work. Let's try To do a chain to remove the chain selection right here. Let's turn that off So it only gives me half of the shape. So it's only sweeping that Half of the shape and then I'll go back in here and say I only want You know point one Point two. Yeah, okay, and that worked That is one of the the things you kind of have to do You're gonna have to keep playing with the sweep until it works Sometimes it just works out of the get-go But the answer there was to turn off the chain selection sometimes you have to sometimes you don't it's just one of those things That's why I'm doing this tutorial to kind of show like the inconsistency of it It works, but you kind of have to work around it now It'd be cool if I could do the other side right like I can say do this whole thing And I could keep playing with that but that's not working So the the thing that will work right away is if I could just mirror this feature So that's how I was able to do that. I'm gonna mirror the sweep I'm gonna pull up the mirror right there and then turn the type into the features and then in the timeline You just select that that sweep your mirror plane is default this this side here Because our shape is already in the center of the grid more or less. It's symmetrical with the origin It will just do a nice mirror for us symmetrically. So hit okay, and then there's your there's your sweep So that's how I was able to create that sweep Now the next sweep is done with a sketch that you kind of have to create a new Plane so construction offset plane here. I need to kind of get to where I need to go So I'm gonna start with this plane and then kind of work my way up Somewhere like that 28 trying to get in the middle here Because this is kind of what where I want my sweep to be on this edge here on this on this kind of paw right there So 20 it's okay. I'll click on that and then I can use this to create my sketch, right? so I'll create my sketch and then I Will grab one of these edges right and I'm gonna project it in so it's selected I'm gonna hit the the hotkey P and project that in and now I have some reference point And I have a reference point you'll see it's not perfectly on the edge here because this is referencing the most outer a Point of this shape So it's not gonna be perfect, but we're pretty damn close. Okay So from here, I'm gonna create that shape again. So let's start with my triangle like this Sometimes I get this automatic horizontal constraint, which is really nice. This is gonna be two millimeters tall and Then I need to define a 45 degree dimension and Then these two lines are perpendicular Like that and then this can move around cool Then I need to make perpendicular line going up like this and Then I want to make this go out like that making sure I get perpendicular constraint on the last two like that And then I close it off here. Cool. Then I add a sketch dimension here one and a half millimeters All right, and then I can grab these Grab this line and do a construction line out of it. Perfect I need to glue this to these two so I can use co-linear co-linear will let me do that and Then I wanted to find some space between this line and this dot how much probably like two millimeters like we did last time Get fusion a second and there we go hit finish sketch and Let's try to make a new sweep here. So again for help the sweep Click on that as my profile my path I'm gonna go ahead and turn off chain selection and just select that edge by default. It wants to like cut away Because there's it notices the digital geometry. So I'm gonna change that from cut to join and then I start playing with these arrows Maybe not even I'm just gonna put like point one point two type deal because playing with the arrows slows down fusion in my opinion In my experience so from here. I kind of want to smooth this out Maybe something like that and I want this to come a little bit further out So something like maybe that okay, and you know, you can play around these values if you want them to be cleaner Whatever more even but it really doesn't matter to me So just hit okay. Hopefully that works that worked fine. Cool. No errors Wonderful and then what I'll do is I'll mirror this so let me hit the mirror You can select that in your timeline now and then our mirror plane is our kind of default Plane and there you go. Those are our sweeps. Very cool. Now at this point That sketch that we have here in the center remember that well here. I want to kind of start to Eat away because you have all this thickness. It's four millimeters thick It really doesn't need to be so what I can do is I can grab that sketch the inside of the of the offset And I could change the direction to two-sided so that I can eat away the top and a little bit of the bottom here How much I probably like that much and that gives me a one millimeter bottom here from here to here It's one millimeter if you wanted to make that bigger Let's just go back into the extrude and say this side should be two and a half That way this and this is one mil one point five millimeters thick and now you have this kind of tray and Do you have this outer perimeter that has the snaps and it has this additive thickness and really why I did this But so that I can do this ready put a fillet and I can add a fillet to the bottom here And I can add it as much as I want I can go for the whole length of our distance here So you have a super curvy bottom and turn off the analysis You can see here how it looks out looks pretty good really bubbly at the bottom and it has all that geometry for snap-fitting This is just the bottom right another thing you do is you can maybe add a chamfer here Just kind of thicken it up a bit You put three now. It's too much too. It's fine looks good You can add a chamfer yeah chamfer there and if you do section analysis You can see how it's it's gonna add a little bit more smooth geometry to that. This is not so So abrupt so it looks really well and then For kind of quickness I'll add a frame because you kind of want to have your frame and your covers together So you can see how much offset you need so I'll create a new component with the hotkey Okay, and I will use the sketch from our First component by opening in it like that. It's a little grayed out But I can still use it and I want this to be like, I don't know 10 millimeters tall hit okay Let's go ahead and change the color of it so that it's more So they're more contrasty. Maybe do like a pinkish and then I'll bring back the cover body Do a section analysis you can see here. Okay, cool Is what I need to do so I'm going to now add a shell to this surface and also the bottom surface Right here of the frame To make it a frame right so I'll use the shell command It's one of my favorite features and how thick you want it I want to be one and a half millimeters thick and hit okay, and now there's our frame Right. It's completely open bottom and open top and now you can see where I need to add my sort of My little a little triangle to to snap into this little grabber so pretty similar I'm gonna come into You know into the sketch. I'm in the right component. I have this side profile here and I will project some geometry Which geometry this one right here this line just bring that in hit the hotkey P And that'll give me a point to select to so now I can do is I can make my triangle Let's just make a triangle like this We need to define the 45 degree angle. We need perpendicular Point here. So select those two perpendicular and then this is two millimeters tall Now that that's done. I can just drag this point and drop it. Oh and drop I don't know why it's not at me I'm gonna select those two points open up my design shortcuts and say Coincident and now they're coincidentally constrained So now I can sweep that hit finish sketch and I'm gonna hide the you know The bottom cover turn off this section analysis and I'm gonna just run the sweep command pretty default Let's just select that triangle Go to path and then select this as my path It's gonna by default it's like ah you want to cut nope I want to join it and okay and that joins it It does the entire sweep because the chain selection was selected and now you can see it swept along it now There is an issue you need to be now. I'm gonna show you where the issue is now It looks all good, and it looks like it did it, but if we look very carefully Let me do a section analysis on the other side now take a look at this from the side There is a itty-bitty tiny gap in between those things here I'm it's really difficult for me to show it to you, but indeed there is a tiny gap From here and here. They're not actually closed It's because there's some just weirdness going on with the geometry like it's not perfect So here's how to fix it and make it so that it's completely watertight turn off the analysis and go back into Into our sketch and all we need to do is to add some geometry Let me turn on the section analysis all we need to do is add some geometry that starts to eat into the In between the outer and the inner Surfaces we just need to add some more geometry to this so what I can do is I can grab a line and Then just kind of draw out this thing here Like that. It's just this little square. Let me turn off the body so you can see what I drew It's just this thing here, right now how thick I need this to be I can just take that one and a half millimeter divided by two and that's a pretty good point and now it's fully constrained So I have these two profiles that I can select and append that and if I turn the body back on if I turn the body back on you can see that yeah, that is Intersecting the the the actual geometry, which is what we want We need them to intersect because once this gets sweeped along at some point around over here It starts to not be perfectly flush with the surface So this right here ensures that you are eating into the surface essentially So my hit finish sketch double-click on that That sweep and then I will append that by holding down the command key or the control key on windows And then that will then ensure that that sweep is like going into the frame Into the geometry and it is so now if we do if we if we flip our our Analysis our section analysis and look at where we saw that gap There's no gap anymore. So that is how to fix that and that is a really critical thing to look at Cool, so now I'm gonna turn on my let me activate the whole doc the whole root of the document that way I can look at both of these pieces together and what we need to do here is to figure out how How how much space is between how much clearance do we have between our surfaces? So this surface here, I'll click on that hold down shift and then click on this and it'll tell me Well, how much distance it's at point three millimeters Which is a little loose in my opinion needs to be like a minimum of point two and a maximum of point three So I could leave that as is but just to show you I'm gonna Click on show geometry and you see this little thing here that two millimeters I can drop this to one point eight or one point nine and that'll effectively make my my my gap Point two it never remember it's not gonna be perfectly point two. It's point three one But that's okay. We're working with sweeps here. They're never gonna be act They're not gonna be a hundred percent accurate, but that's enough gap To kind of mess with there and then we can look at the other side here and it's basically a mirror So it's gonna be the same Distance between these two. Yeah point two three one So let's take a look at the other snap, which is this one here on this side This is kind of the back So if I click on this surface and then kind of rotate to this surface, it's a point three Five one which is a bit too much. So I'll bring up the the snap again I think it's this one right click sure to mention And change that to two one point eight like that and then we can see that This surface and this surface are point two oh nine millimeters away from each other and that's pretty good, you know That worked out pretty good there so If we wanted to create another sweep here the reason why we didn't create one there is because that's where the USB port would be Right, so that's why I'm kind of doing that and you can see that you have these These these separations these segments now in between the sweep so that you can actually get Into it if you want to take it apart because it's actually fairly difficult to try to open this with your bare hands if you got nails I think you could do it but Yeah, I'll actually show you folks now that I'm kind of pretty much wrapped up with the CAD stuff That's really it there for those two if you wanted to make the cover This in this project the cover actually had a sweep let me do another section I'll see it actually has a sweep going up over here because of because of the tallness of the enclosure I could make a sweep there and add a little bit of a jump of a Of a snap fit geometry because there was nothing there really It was just the bottom that needed that that's that that clearance there a little bit more excessive But yeah, the top also has pretty similar separations if not more so that you can get in there and open it So with that out of the way, let me go back over to the kind of overhead and show you opening this thing up I have a spudger tool. You're like, what's the spudger tool? It's this it's a tool designed to be super thin on this edge and this edge here so you can get and pry things open So you can kind of start to see where My thing would be and this is where you get your spudger tool in you just pop it out like that And then the rest of it can can pop out pretty easy with your hands This just kind of floats in there But yeah, here is the the sweep geometry going over here the side geometries here They're a little bit shorter in the final design, but Again, like the values are kind of weird, right? They're not super accurate and then the bottom here same thing Try to find a spot where it's open I think this side is a little bit thinner and then I found it to open it not that way But this way works better Like that once you get one edge in the rest of it pops open and now I'll have to disconnect the USB port there and Then there you go. There's the bottom. There's my cutie pie, and then here's the sides Here's the bottom and then the sweep goes along this entire shape here for the frame on Both the top and the bottom really really cool piece of design here All of this is modular so you can just take it all out and then here's all the sweepiness And then to put it back together just kind of line them up And then snap fit them right Right there. That's all that's left here is the back here And there you go pretty good type fit Yeah, and it stays pretty good In there, so that's the way it's working That's gonna do it for this tutorial. Let me know what you guys think Are you playing around with splines in sweeps? Have you found yourself with some of these issues? Let me know. I'd love to hear about them because There will be more crazy shapes with snap fits. That's gonna do it for this one folks Thank you so much for watching until next time. Don't forget to make a great day. Bye folks