Design your own Drawer Handles in Fusion 360 - Loft Tool

hey guys it's Latimer here again with another fusion 360 tutorial and today we are going to design a replacement handle for this file cabinet drawer so as you can see I've been missing this handle for this top drawer here and so for the last I don't know how many years the way I actually opened this top drawer is first I have to open the bottom and kind of reach in here open the top and then close the bottom and I can finally pull this out so I don't know how long I've been telling myself that I need to go out and design a 3d print to handle so I'm finally getting around to doing that today so I decided to do a tutorial showing you guys the whole process now there's multiple ways that could tackle this but I thought this would be a great project to demonstrate the loft command the loft command is a very powerful feature in fusion 360 as I'll demonstrate shortly so after designing this I sent it to my printer and printed it using black PLA which ended up blending nicely with the rest of the furniture now installing it just simply involves screwing in the two screws which lined up nicely and now it's a lot easier opening and closing my drawer I don't know why I didn't do this a lot sooner the handle we're going to design starts off white on the sides and then tapers to a skinnier profile in the center alright let's go ahead now and jump into the fusion 360 design we'll begin with a new sketch on our XY plane and I measured the distance between the two screw holes to be 96 millimeters so I'm going to begin with a line I'm just going to draw it across here and I'm going to make that 96 millimeters and hit enter now I want this line to be centered between the origin here so I'm going to grab my midpoint constraint click on the line and click on the origin and that's going to go ahead and center that next I'm going to draw a line from this point going straight down and I'm going to make that 24 millimeters now the reason for this line is because the handle has a gums and curves bound that flat surface of the handle here where the screw hole is going to be in his die measured that flat surface to be 24 millimeters from here so we're going to create that line and then we're going to select an X to make it a construction line alright next I'm going to draw an arc going here so I'm going to go to sketch arc grab my three-point arc click the end point here and then just for now we're going to put it somewhere here and then give it just a little bit of a bulge so that third click is going to be that bulge and we'll go ahead and set that okay now I'm going to go ahead and add some more constraints actually yeah let's go ahead and do some more constraints but I'll warn you ahead of time that things are going to end up breaking and I'm doing this on purpose to make a point so I want this line to be tangent to this line and actually I don't need this little extra slit right here so I'm going to hit T for trim and just take that off and you see this black line here don't get confused that's actually the dimension so if I hit escape and I move them actually move this dimension across we see you know you can see that it's just putting that line where that dimension is you can always move these over sometimes you can get confusing what's your lines and what's your dimensions okay so now we have this arc in this line here and I'm going to grab my tangent constraint because I wanted it to be tangent so I can have a nice curve going here so I'll click on the arc and click on the line notice how it went ahead and it gave me that constraint but it did that by making this line all crooked so let's undo that and what I want to happen is this line to stay perfectly straight horizontal so we'll go ahead and grab a horizontal constraint apply it to this line okay now let's try that tangency again so we'll hit this the arc in the line so I kept the line straight but it ended up moving this line across moving this down so our dimension here is all screwed up but that's okay we're going to leave that for now and a point I want to also make is a lot of times it's better to set your dimensions in reference to your origin because as things begin breaking and moving it can affect your other sketches but the origin is always going to stay in place so you're going to hit escape let's take this off and I'm going to hit D for dimension and I want this to be dimension from my origin so I'm going to move it straight down till it gives me that horizontal dimension and I want that to be that 48 millimeters and then I'm going to hit that point again come from the origin and that vertical dimension I want that to be 24 and I don't need this line right here anymore so I'm just going to delete that so now that that's in place let's we see that this line is still blue meaning you know it's still not fully constraint we can move it and we see the only thing that moves now is this point here so let's go ahead and lock that into place I'm going to hit the dimension between that in the midpoint and we're going to make that 24 millimeters now everything is locked into place so we have 24 millimeters going out this way and in this arc here which is 24 millimeters from this point here our origin okay so we have this curve in this arc let's go ahead and mirror this curve on the other side so we'll go to sketch go to mirror select this arc our mirror line actually we need to draw a mirror line because we don't have one in yet so let's do that I'm going to l4 line go straight up here make that construction line by hitting X and now let's try that mirror again so go to mirror our object is going to be this arc and in our mirror line is going to be what we just created there it goes I'm going to click OK I don't need this little extra section here so I'm going to hit t4 trim and trim that out okay so now move this up so we have basically this arc with this line here and then we mirrored that arc here and I'm going to do one more thing I'm going to draw a line from this point here going across I'm going to make that a construction line and the reason I'm doing is because we're going to use that line to create a construction plane so okay that's all I need for this sketch right now so I'm going to hit stop sketch and I want to draw here on this line so I want to make a plane first so I'm going to go to construct I'm going to go to plane at angle and I'm going to choose this line and you can see it's going to give me a horizontal plane that I can go in and enter an angle so I want that to be actually 90 degrees and you see a flip I'm going to hit okay so now I'm going to go to sketch choose that plane and be careful here because it gives you an origin here but that's not where I want to draw I want to draw actually right at this point here where that arc meets so I'm going to hit P for project and I'm going to project in that point click OK now I'm going to grab a center rectangle and let's go to a front view I'm going to draw this rectangle and I measured the other handle so I'm going to go ahead and make this similar to that which is going to be let's do 15 millimeters across by 22 millimeters tall and I'm going to go ahead and put in some Phillips on there so go down to Philip I'm just going to click each of these corners and do all four as a filler music and see it's got a radius of 4 I'm going to change that to 5 and that's that's actually going to break it so let's try 3 looks good we'll go back to 4 4 is fine so we'll hit 4 click OK and I want to mirror this on this side so we're going to do that same approach where we're going to draw a construction line and then mirror it so first let's project at this point here so I'm going to p4 project grab that Center Point click OK and then I'm going to draw a line from here and straight up make that a construction line and let's go to sketch go down to mirror and I'm just going to double click on this entire selection so give me that perimeter and then choose my mirror line from this box click ok and there we go so we have these two profiles here I'm going to click on stop sketch and next I want to draw a profile here as well and to do that I can just grab my origin since I've placed this right in the middle and I'm going to go to create sketch and then choose that plane and these are the same thing here I'm going to grab a rectangle sense a rectangle start at the center there this is going to be skinnier it's going to be we're going to make this 5 millimeters by 22 and we're going to also put in some Phillips there so we'll do the same thing we're just going to do these one millimeter Phillips just to give it a nice round look hit enter click slap sketch and let's go back okay so now we're ready to go ahead and apply some loft so we'll get rid of origin there and then we're going to go to creep 8 and go to the loft so with the loft tool we get this box and the first thing I'm going to do is select my profiles that I want to loft so I'm going to click this one the second one and in this third one we see we get a nice curve there that lofts all three profiles that actually looks really nice I actually might like this handle a little bit better but I'm trying to get it to match my original handle so I needed to actually follow this curve that I made so what I can do is I'm going to for guide type I'm going to go to centerline and then I could get to select my rail so that's going to be my rail what that the arc and line that I created so once I click on that it's going to take that loft and make it follow that profile nicely so that looks good I'm going to click OK and there's my handle now we just need to go in and make these screw holes so I can create a sketch on this surface here and create my holes but what I'm going to do is actually I already have a sketch on that plane and that's that second sketch we did when we drew these profiles so I'm just going to go to my timeline and double click it and I'm going to hit C for a circle and I can actually use that center point and go ahead and draw a circle here I'll make that four millimeters now you want to measure the thickness of the screw you were going to be using in my case it's going to be four millimeters so I'm going to hit enter there and then I'm just going to go ahead and mirror that circle to the other side so I'll select my circle and then select my mirror line which is here and that'll show me a preview of that circle click OK and to verify these dimensions I can click D for dimension and click on both circles and show that okay it's a it's going to tell me it's over constrained but that's fine I just want to verify that that's 96 millimeters and nothing changed so that looks good I'm going to click on stop sketch and I can go to my browser here and display that sketch too so I can see my circles he for extrude and I'm going to click on both of these circles and I'm going to go in the top of you here and I'm going to drag these in now you want to make sure you have enough clearance for your screw in my case I measured it's going to go in about 10 millimeters actually that's going to be a negative 10 so let's change that and we want it to go inwards and I'm actually going to go negative 11 just to give it a little bit of a little clearance room there so I'll do negative 11 click OK and I've got my holes there let's get rid of sketches and there's my handle with my screw holes we're ready to be mounted so let's go ahead and send this to the printer and see how well it prints if you enjoyed this tutorial and want to learn more make sure to check out my website at dusk top makes comm where you'll find full courses and designing for 3d printing with fusion 360

Channel: Desktop Makes

Views: 9,091

Keywords: autodesk fusion 360 tutorial, fusion 360 for beginners, fusion 360 help, autodesk fusion 360 guide, learn auto desk fusion 360, 3d printing, fusion 360 for 3d printing, 3d design, drawer handles, cabinet pulls, sketch constraints, loft, hardware

Id: 0oEwHD0xAK4

Length: 12min 58sec (778 seconds)

Published: Fri Aug 11 2017

Reddit Comments

[u/electrotwelve]

Awesome tutorial and thank you for making this. Practically, it would've been easier to buy a handle from a hardware store :)