Design Snap Fits in Fusion 360 (But Easy)

Creating the Base Body first thing we need to do is have the first body that we will be connecting so you will create your own body but I will be creating on the top plane an example rectangle to have it symmetrical above the or along the red line I will use the midpoint constrain so I will click on the midpoint then select the line and then the origin this way it is symmetrical now I can start basically dimensioning my rectangle so since it's an example I want to have 20 millimeters right over here and then I can just click on the equal constrain and click on both of these lines that way it creates a square instead of a rectangle now I can start making the the shape of the snapfit that I want to have Sketching the Snap Fit Slot so my favourite one is a slot one where I click on the centre one and then as you can see you can just start creating the slot I will give you over here my dimensions but you can completely customize this to yourself and to the size of the part that you are connecting so once you have this um the center line for me was 8 millimeters then from the center to the line which is basically the radius of the slot that you are creating for me is 3 millimeters and then I need to have it symmetrical above or or like along the red line again so what I will need to do is I will need to connect the origin to the middle of this line so I will take a line and then from the origin to the middle but as you can see right now it would be basically still at an angle so I need to make it horizontal doing it by going into constraints clicking on it and then clicking on the line again but since I don't want this line to interfere in my sketch I will just click on it and make it construction either by the short shortcut of X just as this or you can right click it and select normal or construction so once you have that uh we can actually start setting the distances of this uh of this slot so that it can actually have everything constrained so I will make one of the lines over here and the second one over here and then because we need even basically the whole that the slot will be inserted with I need to sketch even these lines that will create the insert hole over here I want this distance to be 2 millimeters of course as I said you can completely customize this to yourself I will hopefully input all of these dimensions or include like a photo of these of this whole sketch into the description so that you can replicate it and have the picture yourself so that you can have it a bit easier times replicating it so once this is done we can actually finish this sketch that will be all that we will be needing from this it's always good to keep the sketches Extruding the Insert Hole as simple as possible and now I will be creating the example body that I will be then connecting so I will click on extrude and then select all of the profiles now I want to have it symmetrical to both sides and because I want to have it 20 millimeters I will input just 10 because it's symmetrical so it will be on both sides it will create a new body but as you can see the sketch was hidden but because I need to work with the sketch a bit more I will go into sketches and then click on the sketch so once I have the sketch again there of course right now I couldn't reach it and a good way to reach it is always to hold down your left mouse button and then it enables you to basically pick anything from that is in the way of your mouse so once you select the profile uh you can just click on extrude again and right now select all of the profiles and we will be making the hole or the insert for the slot itself so select all of them and then just make sure you input a value that is a bit higher than the height of your final snap fit will be so for example I'm gonna have it 5 millimeters so I will make it 5.5 because then there will be 0.5 millimeters of clearance so once I have that I can just click on OK in the menu it cut it perfectly and as you can see this will be the inserting window in which it will go and now I need to create the hole that it will be sitting in so just again click on extrude and select both of these profiles and make the hole now either you can make it a bit deeper so that it sits there better or you can just make it 5 millimeters the exact same that you want your slot to be because then it will basically align perfectly so once you have that right now we can actually stop with this body so you can go and hide this body Creating the Male Insert Body go in the bodies just click on the eye and now create the second body so since I want to have it 5 millimeters I will select both of the profiles and extrude it 5 millimeters down and as you can see the operation is new body that's really important and click on okay now once we have that we can actually hide this first sketch so that it isn't interfering with this part right over here and now Sketching the Snap Fit Profile (Middle Plane) we will be starting a new sketch on the middle plane or the plane that is going straight through it and so you will click on Create Sketch New Sketch and click the middle plane that is going straight through this part once you do that we need to somehow have this wall inside of our sketch to be able to like start sketching on it and to do that you need to project it if you don't know you can either go in the pro create and over here you can select the project or include if it will allow you to see it yes the project or include and select the project but I always recommend to just learn the shortcut P which is a lot faster so if you want you can just click on P and select this wall that will give it us in the sketch itself so once you have that now we need to create the part that it will be snapping against that sketch will be 2 millimeters from down here so either you can create a line or you can just start with the circles so you create the first circle this one will be 1.1 in diameter and then the second circle that will be the exact same so you can just place it there and then go in the constraints and make it equal so click on both of them then also make them Tangent both of these and then all you need to do is create a line between these two that will be also Tangent to both of them so that it actually creates a creates like a basically the whole profile of the snapfit once you have that the only dimension it needs is the space between this circle and the bottom line over here so you can just click on d as dimension once you have both of them selected you can just drag it out and what I found out works quite good is to make it 2 millimeters then just make sure that this this point is on this line and to make it you can just go in in the coincident constrain and click on the point and click on the line itself and as you can see we have it right now fully constrain and that's the whole profile of the Snap Fit that we will be needing so again finish sketch once you finish sketch Sweeping the Profile to Cut the Hole you can go in the create menu and select the sweep function with the sweep function oh no I'm sorry my camera was in the way with the sweep function we enable us to basically select a profile and start moving with it along a path so select the sweep and then the profile that we will be selecting because we will be cutting it you need to select these three profiles again to select something that is in the way of your mouse but behind the body you can just hold down the left button of your mouse and then select the profile from the menu that appears once you have these three profiles selected you can select the path the top of the snapfit which is this whole part this is what you need to have selected and once you select that fusion will fully cut it along the whole path and then you have the beautiful hole created now we will need to be offsetting it so that Adding Crucial Offsets & Tolerances that it actually fits and it doesn't just and so it isn't too hard to insert it for this thing we will need to offset the whole thing by 0.3 millimeters and then even offset extra the bottom walls by 0.15 which will basically give it enough space to be fitted inside of the first body itself so select the offset feature and then do not have to select all the faces one by one what you can do is you can just look from the front just like this and select all of these as you can see and then just input minus 0.3 this will give it enough clearance to be inserted but to be able to snap it and then even basically take it out we need to offset these three faces down over here even by additional 0.15 so minus 0.15 perfect now that this is done this is basically all that you can do for this part now we could start filtering it and doing all extra work but this is really all that it takes for it to work so I will just stay with that and now to finish this part Designing the Flex Hole we need to just create the hole that it will be basically moving along so that it can have that flex there so create a new sketch on top of this body just like this and then just make a construction line which will be in the middle again and then sketch another which will be like an arc once you drag the line as you can see it starts creating the arc instead of a line so you can just create this body right over here as I have created and to fully constrain it we need to create another line that will be basically just a helper line from the point on top to the point on the bottom make the circle Tangent to this line and then make this point coincident to the construction line that we created and then make these two lines 3 millimeters apart or you will put here any dimension that you want depending on the size of your press fit that you are making and then just make any body that you want on this side of the hinge I will be making the example square as I made before exactly the same as was before so it's 20 millimeters and then the midpoint of this will go over here that's all that I need do and then just make both of the sides equal just like this once that is done I have basically all that I need from this sketch then just cut this from the body perfect and then extrude this and I will be needing to extrude it 10 millimeters down just like this so that it would basically fit with the first body as you can see right now it's perfectly aligned that's exactly what I wanted to have and now we can start operating with the second body Sweeping to Join the Male Snap Part because we have everything we need from the first body so again go in the sketches and reveal the second one which is the one that we will be needing to create the second insert for the first body and now we will be joining it select the sweep tool select all of these three profiles as we did before and instead of selecting the top path we will be selecting the path on the bottom it is exactly the same but we are doing it because we don't have anything to select on top of over here as you can see it creates the exact body that we need for it to snap in there so this is basically everything for the second body that you need How the Snap Mechanism Works Mechanically and as you can see right over here what it does is when the press fit basically when you start pressing it against over here it meets with the body so this is where the snap is created and then once you actually basically reach the down is when it stays together so like this it's locked in but when you are inserting it and basically taking it out it makes that sound of the snapping because over here it meets with these two walls and that's what creates the snap if you have any feedback or if you think I've skipped and over any of those steps uh make sure to comment it down below so that I can know to mention it better in the next tutorial and I will hopefully include all of the sketches in the description so that you can just copy them over there hopefully this was helpful until next time