In this Autodesk Fusion 360 tutorial, I’m going to show you how to make a 3D printed bracket that you can use with laser cut projects. It will have slots in it that you can put panels and then either put bolts or screws to them so then you can make boxes or furniture or shelves that are connected in the corners in a way that may not be able to be done with laser cutting alone. So let’s get started.
The first thing I want to do is modify some user parameters so I’m going to go modify > change parameters. We need a parameter of “ply.” This will be the thickness of the material that we’re using from the laser cutter. I’ll make it three millimeters for now. Then we need a parameter called “thick” and this will be the thickness of the bracket. I’ll make this 5 for now. That’s a little thick but I think that will be a good place to start. Then we need a unit called “height” and we’ll make this 25 and then we need a unit called “width” we’ll make this 25. We can always change these units later. And then I make a unit called “length” and we’ll make this 25. And then I want a unit called “angle” that way I can change the angle of this bracket for different projects because laser cutters can only cut at 90 degrees but with a 3d printer we can make it any degrees so that would be a nice parameter to have. So I’ll make a parameter of “angle” and we’ll start with an angle of 60 degrees. Just to show that we can make it at a different angle and then we also want a parameter of “hole” this will be the hole for bolts and things like that. And I’ll make this four and then we’ll press ok.
Let’s go ahead and create a new component and we’ll call this component angle bracket. Then we’ll create a sketch. Create it on the ground plane and then what I’d like to do is draw some lines from the origin. So I’ll draw a line this direction and then I’ll come back like this and I’ll come down, then come over, then like this, then back up. And then what I’ll do is I’ll erase this line because I really want this bottom one to be on the origin. Click from here to here, then I’ll make this one coincident with the origin. The reason I did this is I want to be able to set the angle now so I’ll go ahead and make this angle because I don’t want Fusion to accidentally put constraints in there. If you have that error sometimes you mistakenly put the wrong unit on your parameter so let’s go back and you notice that angle is 60 millimeters. That’s not going to work so let’s delete that parameter and then we’ll make a new one called “angle” and we want to make sure that the unit is degrees and then we can type 60. This time it will work fine. Then we edit this sketch then we press d and we can double click this and say angle and we can bring these down and we can make this one angled as well. Then we need to make this dimension “ply” and we need to make this dimension up here “ply”. It’s important to make sure all these corners are perpendicular. Excellent. And then we can decide if we want inner length or outer length. I’m going to use inner length so I’m going to dimension this “height” and then I’ll dimension this “length”. Then I can offset and will go out “thick”. Look at your directions. This will be negative “thick” in this case and then we need to draw a line from right here to here and we need to make sure this line is co-linear with this line. And then we can draw another line here and we’ll make sure it’s collinear.
Perfect, and then we can break these lines and make them construction lines, or we can trim them. So I’ll go ahead and trim them and it may say we’ve lost some constraints that’s okay.
And then what we need to do is just give this a dimension so we’ll give this dimension of “ply” plus “thick” times two and then we’ll give this dimension the same thing. We can move all these pieces around, so we don’t want that, so we need to give something a vertical or horizontal.
I think one thing we’ll do is we’ll go ahead and make all of these horizontal so I’ll click here and that’ll make all those horizontal and then we need to just center. Center one of these so then we can go ahead and press a dimension here and we’ll make this dimension “thick” and then we’ll do the same thing over here. We’ll make one of these dimensions “thick” so we could have done two thickness dimensions there as well there’s no precise way that you need to do it. Many ways will work so now we’ll go ahead and extrude up and all of these will extrude up “thick” and then we’ll go ahead and make another extrusion but we need to show our sketch and then we’ll extrude and we want to get these outside pieces so this one and this one and then we’re going to go up starting at this object on the top. And then our distance will be “height” and then we’ll say okay.
So now we have our angle bracket where our boards can fit in but we need to draw the holes. So let’s hide that sketch and we’ll make a new sketch right here and then we’ll project in that face and what we want to do is make sure we have the selection filter on entities so we get just that face. You can hide the bodies if you want and then we’ll get a line and we’ll draw from here to here and then we’ll draw from here to here because we want to get the center. Select both those lines, press x to make construction lines then we’ll get a circle and we’ll call this hole. Then we can press extrude. Show the body again and this time we want to go negative direction and the distance we want to go to is an object. That way when we change the size with our parametric model in Fusion 360 it will always cut all the way through.
So there we go and then we want to make one more sketch so we’ll create a sketch right on this face. We’ll project in and by projecting in we make our model robust so it will change parametrically and we press ok. We can hide this body again and then we’ll draw some lines I can press x first so I draw construction lines from the beginning and then make sure you switch back to regular lines. And then I’ll get a circle and this will be hole and then I’ll press e to extrude and then show the body again and the distance once again will be to an object and I’ll click this object and it goes all the way through.
We could add a chamfer to the outer edges if we wanted to but I think this looks nice. I definitely think we should add a chamfer here just so it’s not so pointy so we’ll go ahead and do that so click this edge and we’ll go modify chamfer and we can do it thickness but that might be too far or you could do thickness divided by two whatever you choose is a fine way to put a chamfer there. And if you wanted to add that chamfer to these other edges you could modify that as well by holding ctrl or command to get these other edges in. So I think these outside edges probably could use a chamfer just to keep them from being and then we’ll do thick divided by two. So you could do something like that and you could then add in these edges too by holding ctrl or command and then just have all these outside edges be chamfered off and then you can leave this connection to the plywood actually nice and square. How you do that is just a design choice and I’ll say okay.
And now I have a bracket that I can change parametrically. Let’s say I don’t have any three millimeter plywood then I can go modify change parameters and if I have lots of six mil plywood I can just type six okay and then my design updates automatically. What if I’m out of four millimeter bolts and I only have five millimeter bolts? I can go modify > change parameters and then I change hole size to five and I say okay. Great. And I can do the same thing with the length the angle so let’s go modify > change parameters we’ll make the angle be 75 degrees and say okay. And then our part updates automatically. So hopefully you can use this technique to make a parametrically editable 3D printable bracket that can take panels in its slots and the holes update also. This is a great way to make things go at angles that you wouldn’t be able to do with other techniques.
Happy 3D modeling in Fusion 360 and happy 3D printing.