Fusion 360: Design a 3D Printed Lampshade

hey everyone fusion 360 evangelist Taylor Stein here and in this video I'll be walking through the steps to create a 3d printable lampshade this design is based around the IKEA second chord set you can buy it for about $8 in this image right here you'll see all the dimensions that I took of all the parts in this picture you can see the final rendering of our design and it's also symmetric along its long axis or the z axis so what we're going to do is sketch its silhouette and then revolve it around to create our first solid to kick things off under the sketch menu I'll choose create sketch and I'm going to go ahead and choose one of these vertical planes it doesn't matter which one next what I'm going to do is draw one line so I'm going to select the line tool and I'm going to start it at the origin and this is an important step I'm going to click and move my mouse up and click again to stop drawing the line and then I can hit escape as you can see I have a line that's vertical and that's represented by this vertical constraint let's go ahead and dimension it so from the sketch drop down menu I can choose dimension I'll click on the line click again to place my dimension as we can see the light is 110 millimeters tall so our lampshade needs to be at least that let's make it 130 maybe 135 that way we have a little bit of breathing room next we need to draw two lines the top and bottom of our silhouette so again I'll choose the line tool I can click once down here move my mouse to the left and if I double click I'll stop drawing that line and I'll keep the line tool active I'll go ahead and do that for the top from this picture we can see that the lamp cord has a ring that's forty six point eight millimeters in diameter and because we're sketching half of the profile and revolving it this should probably be half of that so we'll go ahead and enter twenty three point four and hit enter for the bottom I'll go ahead and with the sketch dimension tool still active I'll select that line and place a dimension and we see that the limiting factor here is probably going to be the diameter of the light bulb it's 60 millimeters at its widest we also need to consider that we need to fit our hand inside this when we screw the light into the lampshade so let's go ahead and give ourselves a little bit of breathing room again maybe something about 45 millimeters that way it's ninety millimeters in diameter at the end of the day once we revolve it so we have the three main lines for our lampshade what we need to do now is connect the bottom left with the top left we could do that with a straight line but we're 3d printing this so let's make it interesting to kick things off I'll go ahead and choose the spline tool I'll start the spline from the bottom left corner by clicking once and I'm going to add a control point somewhere here in the middle I'll click to add my control point and I'll place my third point coincident with this point up here I'll click the green check to stop drawing a spline and we can see that we have a nice close profile now what I can do is move my control plane around to change the look of this curve and if I go ahead and click on the line you'll see that it brings up these green tangent handles what I can do is I can drag these tangent handles to change the tangency at that given control point and change the curvature of the shape that we have that looks good to me so I'll go ahead and hit stop sketch and I'll hit the home button to get a nice view of everything next to revolve it around from the create menu I'll choose revolve for the profile I'll select the profile we just sketched and for the axis I can either pick the vertical axis or this vertical line as you can see we create our first solid body with this revolve command I'm going to keep all these settings just as they are we want 360 degrees one side and a new body so now we have the main body to work with for this lampshade but there's a few things we need to do from this picture you can see that I only have the pattern running through the majority of the part but the top and bottom has a little bit of a ring that's unaffected by this pattern let's start by going ahead and splitting the body at the top to create that first ring I don't have any geometry located where I'd like to split the body so let's go ahead and create some to do that from the construct menu I'll choose offset plane and now I just need to specify a flat surface to offset from I'll select this plane and I can offset down by let's say negative 8 millimeters you'll see that I now have this construction plane going through my part but if I open up the bodies folder I still only have one body it hasn't split it yet to split the body under modify I'll choose split body I'll select the body to split and for my splitting tool I'll select the construction plane that I just created now under the construct drop-down menu if I hide the plane you can see that I have body 1 and body 2 let's go ahead and hide the bottom portion and I'll go ahead and hit home next what we need to do is to create a hole in here for the main portion of the cord to fit through the top of the lampshade from the image here we can see that it has a diameter of 40 millimeters so let's keep that in mind when we sketch out our circle from the sketch menu I'll choose create sketch and select this top face and now I'll choose a center diameter circle I'll place the center of the circle right here I'll click and now I can go ahead back and choose the sketch dimension tool select the circle and I can set its diameter to 40 to that we have a nice 1 millimeter gap all the way around I'll choose stop sketch and we're ready to extrude it all the way through from the create menu I'll go ahead and choose extrude I'll select this inner profile and you'll see that I can drag it down through the part to create that cut now this isn't really the cleanest way to do it by just dragging it all the way through we really want to do is tell Fusion that we want to extrude to another surface to do this will change the extent from distance to two and for the surface that we'd like to extrude to let's go ahead and click this bottom surface I'll hit OK and now if we ever change the location of that initial construction plane that extrusion will update properly as well next what I'll do is I'll hide body two and show body 1 now let's go ahead and shell this out to uniform wall thickness from the modify drop down menu I'll choose shell and now I need to select the faces that I'd like to remove in this case it's going to be the top face right here as well as the bottom face so I'll rotate around to the bottom side an important step is I'll hold the command key on Mac or ctrl on a PC and I'll add this bottom face to the selection set when I let go I can now enter in the wall thickness that I like let's go ahead and enter one point six millimeters I'll hit OK and you'll see that we have a nice hollow form for our lampshade just as I created the ring for the top portion let's go ahead and create that for the bottom again to do this from the construct menu I'll choose offset plane choose this bottom thin surface I'd like to offset from and let's offset this by 8 as well it's going to be negative just like last time again to actually perform the split from the modify drop down menu I'll choose split body select this body as the body to split and for my splitting tool I'll click my recently created construction plane so there we have it we have body one body to embody three that make up the main portion of this lampshade now the final step is to create our nice pattern through the middle section of the lampshade so I'm going to go ahead and hide the top and bottom next I'll create a new sketch and we want to sketch on one of these planes that runs through the middle of the part so I'm going to select this one right here the next thing I want to do is project in the existing geometry to do that under the sketch menu I'll go ahead and choose project and for my selection filter I'll change it to bodies and I'll click this body right here as you can see if I hide body 1 I'm still able to access all of the geometry projected into my current sketch next what I'll do is choose the line tool and I'll place one end over here and one end at the bottom right as you can see it creates these coincident constraints which define that the line has to start and finish on these two lines but we haven't specified an angle yet next I'll draw one more line just to the right of our first line and I'll go ahead and add in a parallel constraint to make sure that these two lines are parallel to do that I'll choose parallel from the sketch palette on the right hand side and I'll select these two lines as you can see I can still move these around and specify the distance between them let's go ahead and do that from the sketch drop down menu I'll choose sketch dimension I'll click on these two points and let's say that this is equal to how about six millimeters that looks good to me so I'll hit stop sketch and I'll turn on our main body here next from the create menu I'll choose extrude and I'll select the profile that we just sketched and this time I'm going to drag it all the way through and change my direction from one side to symmetric to make sure I extrude through both sides of the solid body that we have now we don't want to perform a cut we actually want to perform an intersect which is going to leave us the intersection between the extruded body and the existing body really what that's going to do is leave us with these two symmetric strips that we can pattern around in a circle so what I'm going to do now is from the create menu choose pattern and circular pattern change the pattern type to bodies and for the object I'll select this body and for the axis I'll select our z-axis that goes up and down I can now specify the quantity about 22 and I'll hit OK so we're just about done the last step is to pattern the mirrored feature all the way around so from the create menu I'll choose pattern and circular pattern with a pattern type set two bodies I'll go ahead and pick that one that is facing the other direction axis I'll choose the same vertical axis let's go ahead and type in the same number 22 so there you see that we have our pattern features all the way around I can turn on the top and bottom strips and now we have our finished lampshade if you want to change any of these features find the feature you want to change down here in the timeline right-click and choose edit so if I want a different number of strips going around I can right click and choose edit feature and I can change the value to something that I like how about 20 and I'll do that for both of these and this doesn't have to be a circular pattern it can be any feature if let's say I want the opening at the bottom to be a little bit larger or smaller I'll find that first sketch right click and choose edit sketch now I can edit this dimension down here let's say I wanted to be 47.5 I can enter that and hit stop sketch and everything that I've done will rebuild completely now as a final important step for 3d printing let's export everything as an STL to do this I'll right click at the top of my tree I'll choose save as STL I'll make sure the refinement is set to high and I'll go ahead and hit OK and now I can save this onto my desktop wherever I want so that's how you design a 3d printable lampshade in fusion 360 if you want to download fusion 360 there's a link in the description below if you like this video give it a thumbs up if you have any questions feel free to leave them in the comment section thanks for watching

Channel: Autodesk Fusion 360

Views: 487,343

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, 3D Printing, IKEA

Id: 3PnKBSOulwo

Length: 11min 13sec (673 seconds)

Published: Thu Oct 29 2015