Water bucket base

00:01

Hello everybody and welcome to this tutorial in which I'm going to show you how we can build this nicely designed water bucket in Shapr3D. In this exercise, I will show you all the individual sketches we only need for this design. And then how we can use the design history and parametric modeling to create all the individual parts.

00:30

This video lecture is broken up into two parts. In part one, we will create most of the main body and the rim on top. And then in part two, we will take a look at very easy ways how we can create the handle and then assemble everything and finishing design with nice surface fillets and create an attractive product presentation with materials and a fitting background.

01:00

in the visualization mode. And with all that said, let's start it. Here is a new file. Before we get started, let's go to the Snap options and make sure everything is turned on. And our unit system is set to millimeter. The first sketch we're going to create is defining the base at the bottom. So let's go to top view. Then we go to Sketch.

01:30

and ellipse. And at the sketch origin, we click, drag our mouse to the right side, type in 145 millimeters, press Enter and mouse click. And then we move the mouse up, type in 95 millimeters, press Enter and mouse button click. Now we can zoom out a little bit and there is actually our ellipse. Let's rotate the view. This is actually now defining

02:00

the dimension of the bottom part. You can exit the sketch. The next step we're creating actually our water bucket body. To do this, we select the sketch profile, and then we can drag this one up to a height of 250 millimeters. To add a little bit of draft, we can click and drag

02:30

this arrow, you can see this goes inwards or outwards. And here I would like to have minus seven degrees and enter. Beautiful. This water bucket design has between the top and the bottom, actually an offset surface detail. And that's incredibly easy to do. So take a look at this. In...

02:59

a side view, in this case, front. I will create a sketch, go to Spline using the control point version. And then I click and click. I'm using primarily the grid to align everything. And then right mouse button, click to end. I will go to the line command,

03:28

to their line, draw along the grid and finish it up there. And right mouse button to finish that drawing. I can exit the sketch now. What I will do now in a 3D view, I will select my sketch profile and then extrude this a little bit out. It will instantly start cutting into the main body.

03:57

Let's switch this to a new body. There we are. All I need is this curved surface, because when I select this curved surface and then holding Shift, mouse button, double click, I select the body. I can split this body along that curved surface. Click done. Now,

04:28

This body, which we use to split the first body we created, we can select, right click and delete. It will actually then in the history, create a delete comment. We don't need it anymore. This is good. To create this offset effect, I will select just the outer surface and then drag this in.

04:55

by 5 millimeters, not too much. 5 millimeters is really enough. And since we would like to create a blended surface in between, we also have to create a distance. So here I select this surface, and then I drag this one up 10 millimeters. And here I drag this down 10 millimeters. You see, we're creating a nice distance.

05:26

To fill that distance, this gap, I can select both of these surfaces and then call the Loft command. When I go now to the history, there's my Loft command, open the option, and then for the moment, we set this to G1. G1 is a tangent surface continuity. It's not as visually beautiful as for example, G2, but it calculates really fast.

05:56

And we can switch this later to G2 anyway. There we are. So when we take a look at this design, this looks actually really nice, but we aren't identifying a particular problem. Up here, if we want to add the spout, the outflow, we don't really have much of a vertical distance or surface to work on. And this is actually now where our second sketch, which we created, comes in very handy.

06:25

We can actually go into the sketch mode, select this spline, and then very carefully, we just drag it down. There we are. And we can move this one down and an eyeball, for example, that the vertical top and the vertical bottom distance is somewhat equal, like in this case.

06:55

This works much better. To clean up everything a little bit, the sketch, I will drag onto the other sketch. So I have a folder, right click, Rename, and I give this the name sketches. This way, for example, I can always turn this folder on off and show and hide all sketches at once. This looks really good.

07:24

Let's continue working. This bottom edge, I would like to round and give it a fillet. So I select the edge, drag this to the outside and select 30 millimeters. If I go to your side view and zoom in, pay attention to the curvature. When I go to fillet and switch this to G2, then you see that this is a much nicer flow.

07:53

Also here, we can keep this at G1. While we work, this will actually accelerate the processing of our design. And in the end, we just go in and switch those to G2.

08:10

to add a little bit of a groove at the bottom. So when we hold this water bucket with our hands, I can move my finger inside the cavity. I would like to move this surface up and angle it. Similar to the main body, also here we will use the Extrude command. 10 millimeters up is sufficient. And then we add the draft of 40 degrees.

08:41

Now to make these sharp edges look less sharp, also here we select one edge, give this a nice small rounding, and here's a bigger rounding. I will go in, collapse all these elements. And you see here, we can always go back if we would like to adjust the value.

09:06

of our individual features. This looks really good. Beautiful. So the main body at this point is actually done. Now we can start adding details to it. We would like to have an outflow on the left side. So I go to the top view, select this top face, click on Sketch.

09:40

And then right here, I'm going to add a circle.

09:48

And I'm gonna make a circle with 80 millimeters. Right click your escape, and then I can move this point to the left or right. And think about how far would I like this to stick out. I will go to here. Here's the midpoint of...

10:13

the circle that's a little bit inside the body. This is great. I'll go to a site now. I would like this to flow down.

10:26

So I need to create a path. Let's create a sketch. There is our spline. You see here is the plane intersection of the new sketch with the previous sketch and to the geometry, so it can attach this right to the circle. Then I go down, kind of like from there to there, and then I bring the last point in.

10:55

and right click. You see if we draw a line, 20 millimeters, 20 millimeters, so this is 40 millimeters of a height.

11:11

exit the sketch, I will hide these bodies right now, select the circle and this path, and do a sweep command. And for example, here it says, it sells intersect. Why does this happen? Well, probably this is too short. This is also very, very short distance. The circle is very big. So what we can do now is I go back to the sketch and add

11:40

For example, a line here and a line at the bottom. So this is kind of like a midline. I make sure these are horizontal and vertically constrained. And they start at the center and at the rim. And then I will do a sweep again. And look at that. Now this perfectly works. Let's take a look at everything we have. So there we are.

12:11

With all the bodies visible, I can now quite well see how this one sticks out. Is this too far? Then we can go into the sketch for the circle and move this back a little bit. And you see that then also the other sketch follows with it. Here I will have now to adjust the additional points.

12:39

There we are. And based on where I move these points, I can actually play around with the overall shape of the body the sweep command actually creates. Specifically in a 3D view like here, this is very nice to rotate around and then adjust.

13:07

the sketch and pay attention to the resulting geometry. Then we can exit the sketch. This part, so what will be this boat and the upper body, we want to join, we select both, because then I can select this resulting new edge, drag the arrow out and

13:37

give a really nice radius. 30 millimeters is very good. Can also explore 40 millimeters. We're not getting too close to this blend surface, so this will work really well. At this point, I can select all three bodies and join them together.

14:07

into one, this is now going to be just one piece. Because I now have all bodies selected, let's select the top face, click the shell command, two millimeters, and create a quick study of a shell part. Side view, section cut. This is perfect.

14:37

This goes straight up. We could adjust the sketch, move one point a little bit inwards to make this actually arc a little bit more. Down here, we have a really nice economic feature. The blend surface is beautiful. This is great. I am.

15:02

selecting the Shell command, right click and delete it for the moment. Because what I would like to do now is to add a nice rim to stabilize the sides. The rim might actually look very complicated. It is actually fairly easy. So let's go to the front view. I zoom in a little bit. I create a new sketch. Here I have actually a point. That's the intersection of the sketch plane with the geometry.

15:33

And I will select the rectangle diagonal from this point, drag actually a rectangle down. This should be 10 by 10 millimeters. To make sure that this also doesn't really rotate, I will select one line, horizontal or vertical, and add a horizontal vertical constraint.

16:02

Perfect. Now I can select this sketch profile, and then I very carefully select all these upper edges, and then use that as the path to do a sweep along it. There we are. This new swept body, I will

16:31

select and hit isolate. And then I go ahead, select all the vertical interfaces and the lower face and click Shell. Also here, two millimeters. I like to prefer keeping my sketches very simple and then do a lot of detailing with the direct modeling tools.

16:59

or the parametric modeling tools. This gives you then the ability to work more three-dimensional and your sketches are always nice and simple. We know that this face is not perfectly intersecting with the bucket. So we select one face and push this inwards.

17:29

And here, there, I needed to select a different face. 2 millimeters is fine. If I now go ahead and deactivate the isolate command.

17:49

There you can see now how we have a really nice intersection. These two bodies now I can select and create a union.

18:03

Now we have very clean, nice edges. Because this rim was created with two millimeter of material thickness, we can now select the top face, click Shell, say two millimeters and shell it. And it will just like before, shell just the inside. And it looks like magically our rim perfectly blends into it.

18:31

Let's go to a side view, section cut. There we see. I do not round any of these sharp edges yet. This is actually kind of like a detail we will do later. All those fillets will actually slow down a CAD program because the more steps we add, specifically when they're calculation wise, expensive, like fillet, the slower...

18:59

or the longer the computation always has to be. So these are details we add at the end. Currently, we just focus more on the blockout.