Faucet

00:00

Hey everyone, Daniel here for Shaper3D. In today's tutorial, we'll take a look in how to create this Faucet design. And we'll utilize just one or two sketches and a lot of dimensions and relations in order to create a very flexible layout, to create variations or change the design along the way. So if we go here into the modeling layout, we'll go into the history.

00:30

And you'll see that we base all the design on one sketch. We can change any dimension, and it will update automatically through the history. We'll also use some different ways how to use chamfers and fillets in order to create dome surfaces or play with the radius of the transition. So I hope you're excited, and let's jump into it. OK, let's start. So like always, I.

00:58

like to work with my snapping features on. So I want to snap on the grid, also some guidelines and 3d points. And I'm working currently on a millimeter grid. So let's start with the initial sketch and we'll do quite a lot on the side view.

01:17

So I want to work with cylinders. And cylinders are quite easy to create by rotating a rectangle. So let's see how we can do this. I'll choose a line. And we'll start in the center here. And we'll choose our height of, let's say, 150 millimeters. So that's our basic height. Since I zoomed out now, you can see that the grid changed. And we now have a 5 millimeter grid.

01:46

just create the basic angle and direction of the faucet spout. So choose the line again, and we'll create a line, let's say, 1 third from the top. And it should be coincident of the main line. If you don't have automatic constraints, you can go in here in the Constraints Settings and set Auto Constraint to On. Now let's choose our appropriate length. I'll go with 80. Let's see what that does for us.

02:15

And also what we can do is use an angle dimension. So let's go for a nice round number of 100 degrees. And that creates our initial incline for the spout. And now we want to also choose our height. So let's go for this point here and choose this point on the bottom. And that can also get a nice round number. As you can see our line or point here jumped from the center point.

02:43

and we want to still keep working from the center point. And why I did it is I used this point here as the first point and then this one as the second point. So when I chose the dimension, this point, since this is seen as a secondary point, it jumped and changed the dimension and not this one. So we want to move this whole construction into the center point again and let us lock this point here. So this is now locked and we can still change our height.

03:14

And that just moves the top part and also choose the position of the spout. And this point over here doesn't move. All right. Next step is we want to decide on the width of the cylinders. The easiest way is to just offset these lines. We'll go offset edge and we'll just drag this out until we think it's a good thickness and keep in mind that the overall width will be double the one that we set right now, since it will be rotated around.

03:42

So this is now 20 millimeters and let us select both of these lines and set the dimension to fix it. The same thing we do with this line as well. So offset edge, I'll go down here and let's go with smaller width and then again select both of them that will pop up the dimension here and we want to click on it to set it and now it's fixed again. In order to create cylinders we need closed areas.

04:10

So with our line tool, let us just close these rectangles. And since all of these dimensions are already fixed, this will just create perfect straight rectangles. So if you go and exit the sketch now, you can see these are areas that we can work with and that's perfect. And anytime we want to go into the sketch, either go to items and then select the sketch here, or I like to go into the history and...

04:38

set the sketch here. And one more thing that we want to add is the outlet and we can do this in a different way as well. We can go to the rectangle. If you hold the rectangle, you can choose between a center rectangle, diagonal and three points. And usually the diagonal is selected on default, but oftentimes I like to use the three point rectangle. So let us use this one to create the outlet. I'll click on the rectangle and then select our

05:07

line here. So this first one that we created is the center line. And then we'll choose an arbitrary length and then go down and create a little bit of a outlet. So we can also set these dimensions. Let me zoom in. This will again be half the width that we will end up with and make sure that it will always be smaller than the diameter that we choose on the spout. So this one here is 12. So let us be sure and make this one 10.

05:36

And the next dimension, I will not use the whole rectangle as a dimension. I want to set the dimension from this line here, because that means that the outlet will always be extending beyond this cylinder. So if we want to change this diameter at some point, let's put it at 15. We always want to make sure that this distance from the cylinder is going to be the same. So let's go back to 12. And then set our distance.

06:06

between this line and this line. We'll find it here. And let us set this one to around five or four. All right, these are all the rectangles that we want to create. One more dimension is left, and that is the distance between the outlet and let's say the end of our spout. This one we can choose here to be 15 or maybe 10. Good.

06:32

So you saw that I chose to spend a lot of the time here in the initial sketch in order to make sure that all the references are correct. And in the end, I can be as flexible as I want in creating variants and changing the design. So let's exit the sketch and create a 3D model. So let's go ahead with the first cylinder. This will be the main one and then our center line. And it will already show us the revolve tool.

07:01

And a 360 degree revolve is perfect. So let's click away to accept that. And you will notice that our sketch is gone. That's fine. Let's unhide the sketch again and let's continue. So the same thing we'll do with this area, but we'll need to select all of these and select our center line. Click on revolve, 360 degrees, that's OK. And click away from that. Now we can zoom in. That would be our last rotation.

07:30

And in order to create that, let us hide our second body and then select this one, select our center line and go to revolve and click away to accept that. Perfect. So now if you want to look into our history, we'll have our sketch, which basically defines all of the tools that we used and we can always go into the sketch and then we'll see that maybe the spout is a little bit too high. Let's go here and change that to 80.

08:00

Revolution that we did, update it. And since we referenced also the outlet correctly, this one moved down as well. So let's exit and quickly combine all these items. So we'll use the body one, two and three and go here to union. And I will just put them all together into one body. If we want to hide our sketch, we can do that now. And that allows us now to go in here, select these edges.

08:28

and then create a nice soft fillet around here. I like to use the G2 option here, which creates a softer transition with the fillet. Let's go with a five millimeter fillet here. And then also here, I'd like to have one and that should be, yeah, let's keep it at two. And again, these fillets are also showing up here in the history. So if you want to change either one of those, you can go in here, open up this arrow and change.

08:56

all of these settings that you want to change. So changing the continuity between G1 and G2 or change the radius or even set the curvature if you want to be experimental and that will just change the sharpness of the radius. Now before moving on to the handle let us finish this part first. What I want to do is I want to add a little bit of an interesting cap here, here on the front and also on the top and

09:24

What I came to really like is the following approach. I will click on the corner here and then draw inwards to create a chamfer. And let's not be too big here on this side. So I'll choose a one millimeter chamfer. And then what you can do is go into the history, find your chamfer, and then play with these distances. So for now we have one distance of one millimeter. And actually the distance two should be also one.

09:53

which means it's a one-to-one 45-degree chamfer. If we now change either one of those to have a larger dimension, so let's go with three, you'll be able to see that the chamfer now is much shallower. So the angle changed. And that allows us to create interesting geometry with this part. So I'll just choose a really high distance for this first one. And this edge will still be selectable as an edge, even though it's very flat.

10:23

And it also allows us to create a radius, a fillet onto that edge. And if we just keep on going with this fillet, it will at some point be almost like a round cap. So let us create the same on the top here, but I'll be a little less subtle. So let's use a larger jumper. Let's go with two millimeters or even three, then go into history and then play with these distances. So let's go with 10.

10:52

for the inside and then select this one and go really, really big with the radius. And then again, I'll choose G2. And here you can see the domed surface. And we'll still be able to use this edge and add tiny chamfer to this edge to catch the highlights and create a little bit of a crisper appearance. Let's go with 0.5. Let's create one here as well.

11:20

And if we want to see the outcome or the reflections, let us move into visualization mode. Go here into the metal selection, and we'll choose a standard chrome. And I always like to change the environment to have a little bit more interesting reflections to the gradient mode. We can now see the interesting reflections of the domed surface here. So it's not just a flat cap on the end.

11:47

It's rounded and that creates just much more interest in the appearance. And then for the last step, let's use some of the tools again, in order to create our handle. So I'll go out of the visualization mode into modeling again, and I'd like to create a new sketch and let us add for that a new construction plane. What I want is I want to also reference the construction plane correctly.

12:14

So if we change any of the heights, the handle will always move correctly. So let's go into the items and then hide the body and show our sketch. We then can add a construction plane and the type should be a perpendicular to edge type. Let us select our main curve here from the first sketch, go next and then go all the way up to the last corner here and then type okay.

12:42

What that does is if we go here to 110 millimeter, for example, the construction plane will still be referenced correctly. So let's hide the sketch and go draw the body again. And now we'll see the plane is still there. And what I can do now is create another plane. So let's go in here and add a offset plane. And that just gives me the opportunity to offset the handle a little bit from

13:10

the main body and that we can always use and change. So let's go with two millimeters for now. So that's okay. We can now hide our first plane, go to plane two and create a sketch. That will move us to the top view. And now what I want to have is basically a pill shape. That means a shape that is a rounded rectangle. And what I can do is I can project this outer circle that we already have and

13:36

start from there. Now we have the circle, we'll create another one somewhere and then I will just actually reference those two and make them equal. So basically this one will always be the same dimension. Now let's create a line and select the center point here. It will give us the distance between those two circles. So let's go with 50 for now and then I'll move the circle on to the

14:06

the second circle will move accordingly. And then as a last step, let's create some additional lines here on the outer edges of the circle. And these should be tangent to the circles. So if they aren't, if the tangent symbol doesn't show up, we can check that by selecting the line and just moving it. And since they're movable, it doesn't have a tangent constraint. Let's add that. So we'll click those two and then click on the constraint and then

14:34

good measure we can also add a tangent here which is not necessary because they're already fixed but we can still do it. And then the same thing we can do here. Let's be sure to be horizontal here then select both of the line and the circle make a tangent and those two as well. Now we can trim if we want to. We don't need to but it's a good way to just clean up the sketch and make our distance line here a construction line.

15:03

And it's it for the sketch for the handle. So let's go out of the sketch. And it already gives us a nice clean area to work with. We now can just extrude that a little bit. I'll go with, I think four millimeters should be fine. And it should be a bit bigger or thicker than you want it to feel like, because we'll now add another design detail to it that makes it look thinner. So four millimeters fine. And then I'll.

15:31

move down to the underside and then we'll use the same trick that we used on the front and top surfaces and add a chamfer. And this time we can go also quite big so similar to the top cap we can go with a three millimeter distance and again we can go into our history go down to the chamfer and change those distances. So distance two we can go to five millimeter

15:56

make this angle also a little bit bigger. And again we can select the new edge here and then create a nice long radius until the edge and always select the G2 option and that will create a domed surface here which will look really really nice. So that's the handle done and we can always go into visualization mode and also choose our chrome material and move that to the handle as well.

16:24

Now we can look at that and I say last detail, we want to combine those two items. So let's go back to modeling and then we'll just hide everything that we currently don't need. So the top body and then maybe also choose the first plane that we made. So let's go in here, go to sketch and then we'll create a circle from the center point. So let's choose the center point and we'll go with 15 millimeter diameter.

16:54

And we'll also create a line through the center. So something like this. And then when we go exit the sketch, what we can do now, similar to what we did with the cylinders, we can select half of the circle and then go and select the line that we created. And when we revolve that, it will create a ball. So this will be the center axis around which the handle will move. So now if we unhide the handle.

17:21

You can see that a little bit of the ball is actually sticking out here on the top, which is not a big problem. We can go and select both the ball and the body, go to subtract. I will just delete the handle. But if we go to keep removed bodies and hit done, we can now select this top part and delete it. And now this part doesn't intersect with our handle anymore. So now I'm really happy with the design.

17:51

If we want we could even dome this top surface. So again using the chamfer method we'll go and do a really small one by with 0.5 millimeter distance here. Let's go down to our chamfer and change the distance here. So I think it's distance one. Yes, and then that will create a really shallow surface.

18:20

and now select this edge here and I give it a really large radius. Now as a last step I'll highlight all these edges that I want to be rounded over and to have some tiny highlights here. So I'll give that a 0.3 and if we go here into the visualization you will see that all these edges now have highlights and that makes it just a more

18:49

that little bit more realistic to look at.