Designing a Lasercut Laptop Stand with Fusion 360

hey everyone fusion 360 evangelist Taylor Stein here and in this video I will be teaching you how to design a laser-cut laptop stand as always I'm going to be recording myself throughout the entire process so you can see my thought process and the mistakes that I know I'm going to make and how I go about fixing them to kick things off let's go ahead make a new component for the legs of our laptop stand by right-clicking the top of our browser I'm choosing new component give this the name leg and we're ready to get started I'll start things off by creating a base sketch for the side profile of the legs on this work plane right here and I'll turn on the origin so that I keep everything aligned now what I want to do is sketch out a rough shape really capturing the design intent for this side profile so I'll snap one end to the origin here move until I have this nice horizontal constraint move a perpendicular line up maybe some angle over here and I might want a perpendicular constraint with that line and maybe I want this to align with the first point that I drew so I'll click and finish it off with one more point going down there so as you can see I have the rough idea but this is not exactly what I want what I can do now is apply any additional constraints that I need to eliminate degrees of freedom within my sketch and then add in the dimensions to lock everything down one constraint that I know I want to apply as a parallel constraint between these two lines so what I can do is choose parallel for my sketch palette and choose these two lines and now they're parallel I think that's all the constraints that I need so I'm ready to dimension it to do this I'll choose the sketch dimension tool from the sketch drop down menu and start dimensioning I want this distance to be 225 so I'll type that in and I want the overall height of this to be 125 and now we can see that I can move these points around and there's still a few degrees of freedom maybe I want this distance here to be 55 and we're almost done how about I want this angle is long that I really care about this is the angle that the laptops going to sit at when it's resting on the stand so I can still with the sketch dimension tool choose this line and this line and dimension that angle to be how about 22 degrees and lastly let's dimension this width from this point to this point to be 14 so there we have it you'll see that all the sketch curves are black indicating that I have a fully defined sketch and we're ready to extrude it I'll stop my sketch and we can see our sketch profile before I do this I'm going to set up a few user parameters so that this laptop stand is a fully parametric what that means is that for any material thickness or any width or any just certain aspects of the design I can change that as I see fit so one of the modify drop them and you'll choose change parameters and let's create our first user parameter I'm going to call this T for thickness and I'm going to set it to a quarter-inch some placeholder value I'm actually going to measure the material when I cut this on my laser cutter but for now let's go with a quarter-inch additionally let's go ahead and set parameter for the leg width how far apart the legs are and this is going to depend on the laptop that you have so I'm going to go ahead and create leg width and we can make this mixed units it doesn't matter that I'm using inches and millimeters I'll make this 270 millimeters and hit OK so now what I can do is make sure I use those parameters for all the features that I use from this point going forward to kick things off on the create menu I'll choose extrude select this sketch profile here and for the thickness or the extent of this extrusion I'm going to go ahead and type in T and now we're extruding by that quarter-inch distance that looks good to me so I'll go ahead and hit OK and we're ready to now add maybe some Phillips we don't want to really cut ourselves when we're putting this together so let's round off some of these edges by using the Phillip command and the modify drop down menu and to select all of them easily I'm just going to go to a top view rotate over and if I now do a window selection from right to left you'll see that we will select any edge that that rectangle touches so that's all the edges that I want and let's go ahead and add maybe a three millimeter radius fill it to all of those so that looks pretty good to me the only problem is we need two of them so I'm going to go back and activate the top level of my design and let's copy and paste make a duplicate of this leg so I'll right click on it and choose copy I'll now right-click anywhere and choose paste and I want to choose paste so that any changes that I make to the initial we'll be reflected in the copied instance and I won't have to do it twice so I'll choose paste I'll just go ahead and leave it there for now we'll see that we have leg one and leg two and now we're ready to really set the leg width of our laptop stand and I'm going to do that with a joint so I'll do the assemble drop down menu I'll choose joint and I want to align this piece of geometry with this piece of geometry and now what i can enter is for the offset instead of 0 let's go ahead and enter leg width I'll hit OK and now what I might want to do here is test out my user parameters make sure that it's working so again under the modified drop-down menu I'll choose change parameters and let's make this a little smaller and let's make sure that our material thickness changes so if we for some reason want to use half-inch material we'll see that it updates I'll set that back to a quarter-inch and what if we want it to be a little bit wider how about 300 so we see that it is a working model and this is a nice thing to check that it is working before you get yourself too far into a design so the next thing we can do is create a new component for the top of our laptop stand so I'll right click up here choose new component let's call this top and you'll see that it automatically is activated which I want and I'll create a new sketch off of this existing surface the top or sort of that slanted edge of our leg what I also want to do is project in the other geometry so under the sketch drop-down menu I'll choose project slash include and choose project or I could hit the hotkey P and I'm going to go ahead and select this face right here and hit OK and to get a nice view I'm going to choose look at and click on this face and now we're looking at it head on what I want to do now is draw again sort of a rough shape and then use constraints and dimensions to lock in the sketch profile so I want to draw a 2-point rectangle so to the sketch drop down menu rectangle two-point rectangle and as you can see I'm going to draw it really rough what I can do now is add in some constraints so how about I want to align the bottom of this top plate to this existing edge that everything is nice and flush so to do that I'll choose collinear and how about this line and we'll zoom in and grab this line so that's going to fit nicely and now I want this to be a little bit lower than the top so I'll drag this down and that's all the constraints the rest are going to be dimensions so when to the sketch drop down menu choose sketch dimension or the hotkey is D and let's set the distance from this top edge to this point to be 12 millimeters and let's set the distance from here to here to be 8 millimeters and let's just go ahead and do that on both sides great so that rectangle is fully constrained what we can do now is add in some tabs so let's all press this together I'm going to choose sketch and another 2-point rectangle and I'm going to draw one in here that starts on this existing edge and finishes on this existing edge so we have those constraints in place you can see the coincident constraints what I need to define now is the size of this tab and to do that I'll choose my sketch dimension tool and I'll set the distance from this point to this point to be 25 millimeters you could set this to any size that you want and now you'll see that if I drag this sketch it isn't defined how far it is from the top so we need to add that dimension too so I can hit the D hotkey and say that the distance from this line to this line is how about 30 millimeters so that looks fully constrained to me I do want more than one tab I want 4 of them so I need to mirror this across but I need some mirror lines to do that so to draw some mere lines I'll choose a line tool and I'll snap it to the midpoint of this line and connect it to the midpoint of this one and I'll do the same for the horizontal mirror line once I've drawn both of those I'll go ahead and select them holding shift and then I can hit X for the hotkey to turn them into construction lines or I can choose normal size construction up here and now let's mirror these across so into the sketch drop-down menu I'm going to choose mirror and a nice little handy trick is I'm just going to do a window selection to select all of those entities and I'm going to mirror them across this line and now we have it on both sides and let's go ahead and repeat the mir command by right-clicking and moving to the 12 o'clock position and for the objects I'm going to window select those entities as well as these and for the mirror line let's choose our horizontal line and hit OK and it looks to me like our sketch is done so we'll say stop sketch and we're ready to extrude from the create drop-down menu I'll choose extrude select all the profiles that I want it's going to be all of these make sure to not select any of the tabs that we want to poke through and now for the distance to the extrusion we want to go down because we're sketching on that top surface that's already there and we want this to all be flush so I'll type in negative T to extrude down by the material thickness that we've specified so that looks good to me so I'll hit okay we will operations new body that looks good and now if I return back to the top level we'll see that we have this nice top plate that rests in there but we do have some interference between parts so we need to use a boolean operation to subtract one from the other so do that under modify I'll choose combined and the target body is the one that this actions being performed on so I really want to remove material from this leg right here so I'll choose this leg and the tool body is going to be this one and I don't want to join them I actually want to perform a cut and I like the top of this so I'm going to say keep tools so that it doesn't get thrown away at the end so I'll hit OK you'll see that it subtracts material away if I hide the top it's gone ahead and subtracted it and because this instance over here is a paste and not a pace new it actually happens to both of them so look at that I don't have to do it twice I only have to do it once so that looks really good one thing I'm going to do is activate the top component and go ahead and add in a few Phillips here just to round this off just so the design isn't too sharp don't really want to cut myself when I'm putting this together let's go ahead and choose those I'm just going to add maybe a two-millimeter radius fill it something small that looks good to me and again what we can do is check that our user parameter still work so I'll choose my change parameters and once again check the material thickness if we make this really thick everything still seems to be good drop it back down and what happens if we have a really skinny laptop stand everything still looks good great so it looks like we're almost done but if we actually put this together it's going to be really wobbly there's no supports holding these legs together it's not be a great laptop stand so we need to do is model in a few supports so I'm going to go ahead and create a new component we call this support and I want to create a sketch on a plane that I don't really have yet if I turn on the origin don't want to sketch on any of those and I don't have any flat surfaces where I want to sketch which is somewhere here offset from this back face a little bit so to do that I'm going to create an offset plane I'm going to offset this existing face and let's go ahead and offset it maybe about negative 45 millimeters that looks good to me and to get a feel for this I can make this construction plane bigger so we can see really where it lives in 3d space so let's go ahead and create a new sketch on that face and what I want to do is really see the intersection of these legs with my current sketch plane so to do that under the sketch drop down menu I'm going to go to project slash include and choose intersect for the selection filter I'll turn it to bodies and I'll select these two legs right here we'll see that the intersections are projected in which is great and just like before what I'm going to do is draw a two point rectangle and I'm not really going to care about its size because I'm going to constrain and dimension it in just a second so the first constraint that I want to apply is a collinear constraint with this bottom edge in the bottom of our legs so that everything is nice and flush with the table so to do that again I'll choose collinear choose this line and choose this line and everything's collinear there and as far as the width it would be nice if this support matches the width of our top of the laptop stand so everything is nice and in line so I'll choose another collinear constraint between this line and you'll see that even though this edge isn't projected and yet I can still select it for my constraint and I'll go ahead and apply one more to the left hand side right here and now that is constrained so the only thing left to dimension is the height of this support and this is really however tall you want to make it I'm going to make mine how about a 30 millimeters tall so into the sketch drop down menu we'll choose sketch dimension and I'll select this line in this one and let's say that is 30 and lastly what I want to do is maybe model in some tabs so this can slide together and I can do that in this sketch as well so I'll choose line let's draw one that goes from the mid point of this to the midpoint over here and hit stop sketch and let's extrude the profile that we want so again create extrude and I want this to slide in maybe from the underside of the laptop stand so we have to think a little bit about which sketch profiles I want to select so that is these for sure and then I want to select the bottom right here and let's make it symmetric about the current sketch plane so I want to extrude by T divided by 2 and the direction I'm going to set from one side to symmetric and hit OK and now we see that we have those nice tabs right there and then how about you know we don't just want one support we probably want two of them so I want to mirror this about kind of maybe the middle mid plane of this laptop stand but we don't have a plane that already so I'm going to use another construction plane this time instead of an offset plane I'm going to choose a mid plane so under construct mid plane and let's select these faces the back face and the front face of our laptop stand and that looks like a good plane to mirror about so now under the create menu I'm going to choose mirror and pattern type I don't want to pattern faces or features I want a pattern bodies so I'll go ahead and select this body and for the mirror plane I'll choose that plane and hit OK and that looks good to me and let's go ahead and hide that construction plane and one thing that I realized is I want to round off all of these edges and I'm a little bit lazy I don't want to select all of them so let's go ahead and use the parametric time line to our advantage so I'll step back one step before the mirror feature and I'll go under modify and choose fill it and now let's select these edges that I want to fill it I for sure want to fill it these outside edges right here so let me zoom in and grab these and I want to grab these as well but actually I'll do that in another feature add those might want to be different sizes so for these outside ones how about two millimeters and I'll hit OK and that for these inside ones I'll right-click and go up to repeat the Phillip command and for these these are much smaller these are just so that the P is slide together a little bit easier they kind of ease in so let's go half a millimeter and hit okay and now what I can do is step forward and my mere feature that body that's entered into the mirror feature is now updated so a little bit of time-saving there I think it was faster maybe not but that looks good to me as far as the legs go I'll return back to the top level and that looks good except you can see a list here that this edge disappears because I haven't subtracted away material from the supports and the legs so again to do that under the modify menu I'll choose combine the target body is going to be this leg and the tool bodies I can select multiple to me both of these and remember because we pasted this leg over this boolean subtraction it should happen to both of them let's see so we hit okay I hide the support and there we go you see that it happens to both of them and just like we did before maybe let's go ahead and round off these that way everything slides together a little bit nicer and to keep things clean I actually want to do this in the leg component it's best to kind of add the features in the component that you need them so I'll go ahead and activate the leg component and let's add a fill it on these right here it should be reflected to the other one and how about half a millimeter again and we can select more as well maybe I want to add them here so I'm going to hold the command key on Mac or control on a PC to select the ones that I want and I'll select that one and let's go ahead and add these so that everything eases in a little bit easier it looks like I'm selecting the wrong edges there so let me hide at the top there we go and let's add those and lastly let's add the user right here I think that's all of them oops forgot one this one right here and let's enter half a millimeter it's already there so I'll hit OK and we'll see that that happens to all of those and it's reflected here on the other side perfect so I'll go back to my home view show everything and activate the top level and it seems to me like we are done so one last step is how do you get this out to a laser cutter so what I like to do is create new sketch on any existing face that I want to cut and then all of the existing curves and profiles on that plane will be added into the sketch automatically so you won't run into any double lines or worry about any construction lines in your fearing with the pass that you're going to be cutting on your laser cutter so to do this I'll choose create sketch and one of the pieces that I for sure when a cut is going to be this leg right here so I'll choose that and I'm just going to hit stop sketch and I'm going to repeat this for the top because I want one of those choose stop sketch and I want one of the supports so I'll create a sketch on that profile and now what I might do is open up my sketches folder and I might just call this side DXF we'll call this top DXF and support don't want to activate it I want to rename it support dxf and now for each of these all I have to do is right click on it choose save as DXF and there we go so I will right click on each of them save them out as a DXF and then import them into whatever 2d tool you like to use for laser cutting and you're ready to go one last thing that I want to double check before I send you off is that this is fully parametric so let's say I went to the shop I measured my material and it's a little bit thinner instead of 0.25 at 0.23 will see that it adjusts and let's say hence them a 15-inch MacBook maybe have a 17 inch macbook let's go ahead and up that to 300 and we'll see that everything adjusts there and one less thing that I like to check for laser cutting is any interference or coincident faces and to do that under the inspect tool choose interference and just drag a box over everything and we're going to leave this unchecked right here coincident faces and just hit compute to see if we have any pieces of geometry that are sharing the same 3d space so we'll see that no interference is detected which is good means that we don't have any pieces of wood that are sharing space everything is coincident and to double-check that I'll check this box and hit compute and now we can see all the surfaces that ideally are going to be touching and holding this laptop scene together with just friction if it's your measurements are a little bit off from the materia thickness you might need to use a little bit of wood glue but you should be all set to go so that is one handy tip there for checking any interference or coincident faces so there you have it that's how you design a laser-cut laptop stand in fusion 360 if you liked this video be sure to give it a thumbs up and as always if you want to reach out to me directly you can tweet me at taylor underscore Stein thanks for watching

Channel: Autodesk Fusion 360

Views: 331,198

Keywords: fusion 360, autodesk, design, engineering, mechanical design, mechanical engineering, industrial design, product design, software, CAD, CAD software, Computer Aided Design, Modeling, Rendering, 3D software, Autodesk fusion 360, cloud based CAD, CAD in the cloud, cloud, Free CAD, Free CAD Software, Autodesk CAD, cloud manufacturing, free CAD program, 3D CAD solution, lasercut, maker, DIY, laptop

Id: 7riGolu7BpA

Length: 20min 24sec (1224 seconds)

Published: Thu Feb 18 2016