Kettle

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Welcome to this Shapr3D tutorial for the iPad for industrial design. Today we are going to create this kettle design that I sketched beforehand. I would like to have it now in 3D and I'm going to use Shapr3D for this. The tools we're going to use are some basic extrusions for the body itself. Then some interesting features for the body.

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The spout which is not an extrusion. We're gonna use a sweep and we'll discuss why in a second. And also we are going to use an interesting technique here for the lower part in order to create this sharp edge here. Alright, I hope I sparked your interest in this tutorial and let's jump straight in. Alright, just before we start creating, let's check our

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grid dimensions and also the snapping functions. You can find them on the right upper hand side and here it says 10 millimeter grid spacing and this just changes when we zoom in to five and even one millimeter or from one to five to 10 millimeter grid size. As well here on the upper side we can see our snaps and I'd like to use them all so I have them all.

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activated. And if you'd like you can also change the camera angle. I have it set to 15 and some other options for navigation. Alright now let's start creating. So I'm here now in a new file and we are going to start with a sketch. So let's go and add a sketch on our top view and we are going to use a circle for that. So click on circle.

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And then I'm going to start out in the center and draw outwards. And let us change the diameter to 150 millimeters. Set that to okay. So now we have our base circle. We can exit that sketch and then turn in 3D and see what we did. We can just highlight the center here and it immediately starts us out in our Extrude tool. So let's Extrude that outwards. And then we can also type in a

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number. So let's go with 180. And also what we can do is we can add a draft angle. So this is the angle that we usually use for injection molding plastics. But we can use it here now to inform our angle for our kettle. So I think I'm gonna go something about between five and ten. So let's go with eight. I think that looks good. So this is our base.

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Now we want to add some additional elements. I do have a sketch here on my iPad that I can reference. So I know approximately how I want the shape to look like in the end. We can always switch back and forth between Shapr3D and our sketch. That makes it really easy to reference any ideas that you might have. You can always add an image to your file if you choose to do so.

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But for me, I like to work freely and just use the sketch as a reference. Alright, let's add the spout from the top. And to do that, I will create a new sketch plane here on top. So I'll use this plane to create a sketch. So let's click on sketch and it automatically uses the top view for that. And let's start with a line. So let's create a line starting from the center point. And I will go to the left side here.

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as long as you would like and I will set it to a 5 just visually makes sense to me. And also make sure to lock this line in place for that we go to the right side and down on the right toolbar we have a lock icon. So with that I can lock and unlock my line so we don't move it by accident. So now let's create another line starting from...

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the left end of our line and ending on the edge of our circle. Instead of the length of the line we'll create an angle dimension and to do that we select both of our lines and here you can see an angle dimension popping up and we can click on that in order to type in an angle that we'd like. The next step is to mirror that onto the other side and we can do that easily by first creating a new line.

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and now we don't need to worry about any dimensions. What we can do is select both of those lines that we just created and use symmetry. So on the right toolbar again, we'll find our symmetry and now it asks us for our axis for the symmetry and we can use our first horizontal line for that. Now the lower line is mirrored across the X axis and any change I will make to the first line

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will be reflected down onto our lower line. So for example, if I type in new angle dimension here, you can see both of the lines changed accordingly. What we also can do is highlight this line in the center and make that a construction line. And why? I can show you now. So when we exit now, the sketch itself will be not divided by our center line. The next step is we want to define how...

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this spout is protruding outwards in which angle I would like it. So what I'm going to do is add a new sketch on the side. And I think I'm going to use a new line to inform this angle. And what I can do is I can project these sketches from our spout. You can see here. And now I can highlight those two and create a new angle dimension here. Go with maybe 75.

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And that's fine. Let's exit the sketch and let's see what we can do with this now. So let's highlight our area here of the spout. And what I'm going to do is not extrude it straight down, but use our angled line here and create a sweep. So let's select the line for the sweep. And that basically just extrudes it in angle into the inside of our kettle. And the good thing about history is you can see on the right side, we can always go.

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into any of these sketches, extrusions or sweeps and change an angle and it automatically updates. So let's go into our sketch 3 that we just did with the 75 degree and let's change the 75 to 65. So let's exit the sketch and go back to the sweep and you can see it automatically updated this angle and maybe I like that more so let's keep it. What we can also do you can see all these

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we can go to our items and either create folders or just hide these sketches that we don't need anymore. And that makes it a little bit tidier. Now, while in the items, we can also highlight our two bodies and that automatically shows us a option to union these two bodies. So let's do that. And what union does, it's a boolean operation that combines all of our bodies. Alright, now let's add some details to our spout. So...

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First I'm going to highlight this first edge here and I will create a small fillet with a radius of 5. And I'll go into the settings and also choose G2, which creates a softer transition. Let's do that with this edge as well. So let's drag outwards and then we're going to choose appropriate size. That creates a nice soft transition from the body of the kettle to the spout.

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And again, if we want to change anything, let's edit our sketch 3 with our angle. And I'm going to change that to 75 again, go to our fillet that we just did, and that updated all our steps that we did in between. All right, next let's add our radius on the bottom. So you can see here, I have a rounded bottom here, and I also want to reflect that in our model here. What I really would like is to have an actual visible edge.

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running along the bottom part. So instead of just using a normal fillet, which would create a very soft transition, we can first add a chamfer. So let's push inwards and it creates our chamfer. I think 10 to 12 could be fine. Deselect, so that's fine. Now I'll have another edge that I can fillet. So let's select this edge and draw outwards.

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and it creates our soft transition down here. You can always go and use G2 to create an even softer fillet. So now that we did this, let's look at it from the side. And as you can see, it doesn't really fit the vision that I had in the sketch. So what I want is the angle to be less steep. So let's go in our History and find our Chamfer that we did, double-click. And now we can use the two-sided Chamfer.

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and change how the angle of the chamfer looks like. So let's go and add a second distance here. Now I can play with that side as well. So I can here now change the height and then also with the second arrow, the angle. And that in turn affects our fillet that we did afterwards. So let's use that and go into our fillet, check if that's still fine. I think that looks good. So let's go out of the history and you can see now.

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Our rounded bottom looks much cleaner and softer. So I think I'm quite happy with that. We can always go from modeling mode to our visualization mode and then choose a metal, for example, here in order to see how it looks with some reflection added to it. So let's choose our environment. I like with this gradient mood environment. I see the reflections quite well. Let's hop back into modeling and create a wall thickness.

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flat surface here, one of the options Shapr3D will prepare for us is Shell. And if I hit Shell, I can drag now the size of the wall thickness or just type in whatever wall thickness I would like. Let's quickly add a lid. And for the second step, last step, we're going to add our handle. For the lid, I'm going to recreate or reuse the outer edge of our top surface. But first of all, we need a new plane.

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Let's add a construction plane and the type is automatically set to offset. Let's zoom in here and use our rim here of the plane. Hit next and then choose how much of an offset we want to have. Since the lid should be almost touching the top surface but not quite, since we always have a little bit of a gap between two pieces, I'm going to choose a 0.5 offset of our plane. Let's go.

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Okay, and hit done. Alright, now that we have our offset plane, we can use the outer edge and the inner edge in order to create our lid. So let's click on the plane and a sketch. In order to use those lines, let's project them. So go to project, and we are going to use the inside as well as the outside edge. So let's go ahead and click along the edges. So now,

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When we deselect everything, you can see our parallel lines, which are colored magenta in order to tell us they are projected. And the next step is we want to offset our inner edge. So let's offset the inner edge. It doesn't let us offset it too much because it's quite thin on the front, but we can definitely use a 0.5 offset, and that just helps the lid stay in place.

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And this inner edge we can also make a construction edge because we don't really need it for our volume. So now we can exit the sketch and you can see we have two areas. And let us first use this inner area and just extrude it downwards for a few millimeters, maybe just one or two. And also extrude our other areas. So let's select those two areas of our sketch and extrude them upwards for two millimeters as well.

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We can give that a draft angle as well if you'd like in order to match this angle on the side here. Alright, now that our kettle has our lid, let's go to the items and hide things that we don't need. Such as our lid sketch and the plane. What we can also do is go into a visualization mode and move our chrome onto the lid as well. As you can see, it's nicely connecting the...

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angles and we have our small gap which makes it just this tiny bit more realistic. Okay back into drawing mode let's add our handle for the kettle itself but also for the lid. So with the sketch selecting the side view first let us draw some construction lines and the first one will run from the side of the body so let's select one of these edges here and then

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go up to this edge. And that just creates our construction line to be parallel to the body itself. And the other one is we can either project it or just use our points here in order to also create a construction sketch on top. Alright, next let's add a rectangle. I am going to hover over it and select a three-point rectangle in order to just create a rectangle that's fairly

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close to being parallel. And then we can select our two lines and use the parallel constraint here on the side to make them actually parallel. Now I'm going to use two circles. And starting from that center on top and as well on the bottom, create a rounded rectangle. We can keep it as is, but it makes it a little bit easier if we're going to trim the unnecessary parts of our sketch with the Trim tool.

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What we can do now is choose some dimensions. So let's first choose a dimension for the handle itself. Let's go with 25 millimeters. And also the length of our handle, we can choose to be a little bit smaller. And next is the distance between those two parts. Let's go with five millimeters. And I think I'll make that a bit thicker in order to make room for the fingers.

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The last step is to create an offset of our sketch in order to make the handle usable. I'll go with a 6 millimeter offset and then we can exit our sketch. So now that we have our sketch let's extrude that into both directions. So first into our left side and then go around and choose the other side and that makes it 20 millimeters overall.

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Now we can hide our sketch as well and just create some small fillets along the edges here, on the inside as well as on the outside. And if you ever want to create a smaller fillet than 1 millimeter, you can just zoom in to change it in smaller increments or simply tap on the number and type it in directly. Alright, let's add our lid handle on top and I'm going to use our sketch from before.

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Because we have already made our construction lines, we can also reference some dimensions here as well. So let's just add a quick circle here in the center and make that exactly 35 as well. And if we want to reference the distance, we can add a small line here, which should be parallel to our lid and also tangent to our circle.

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And we can make that a construction line. And now we can reference those two and choose our distance. I'm going to go with 2 millimeters. We're also going to offset this edge. And I think we had 6 millimeters before. And that's our lid handle done. Let's go exit this sketch. And let's extrude that. And I think it should be a little bit thinner than the actual handle. So let's go with 6 millimeters in this side. And then also.

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six on this. So after the extrusion let's add some fillets for these inside edges. Let's store that out to four millimeters and the outside edge for one millimeter and that creates a nice soft look. Let's hide our sketches now and that is our handles done. Now we need to just quickly attach them and then we're done. So for our body handle here let's hide.

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the body itself quickly, which is this one. We can always rename that. So let's hide that and use this side here for our sketch. Let's create an offset of that sketch, which should be around two or three millimeters. Exit that sketch because that's all we need. And we're now going to unhide our kettle and extrude that part outwards just enough so it's kind of touching.

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our body and we also want to be a new body because otherwise it would combine the handle with everything. So that's fine and we didn't use a rounded rectangle so now we need to round these edges quickly as well and for me that would be six millimeter to round the edges completely and the last step is to either highlight these bodies or go to tools

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Choose our union and then select those two elements and hit done. So now we have a common edge here that we can also fillet. And the last thing on our agenda is the same thing on top. So let's create a new sketch here on top of that lid, create a small circle that's just enough to not protrude outwards. So that could be around eight millimeters. Exit the sketch.

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and we're going to extrude that outwards until we intersect. We don't want to cut, we want to have a new body. And then again, I'm going to the tools here and under Union select those two pieces, hit Done, and quickly fillet this edge as well. Right now the finishing touches, we can select all of these edges here and give them a very small radius of...

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point three and then we have one more edge here which can also get a small radius. And for some housekeeping we can create a folder which we're naming sketches and we can move all our sketches into this folder and we're left with all our bodies. If you'd like you can even rename all of the bodies accordingly. But for now let's just quickly jump into our visualization mode.

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Give our bodies the correct materials. I'm going to use a plastic material for a handle. Give it a different color and let's marvel at our creation. So this is it for this tutorial on Shapr3D for the iPad, specifically for industrial design. I hope you learned something today and we'll see you soon.