The Extrude tool

00:00

Let's take a look at the Extrude command. It is very good when you have a sketch and you would like to extrude it along one direction. So in a new and empty file, go to Top View, make sure all our snapping options are turned on and the unit system is set to millimeters. To extrude, we need a sketch. Go to Toolbar, click Sketch, select Circle.

00:27

And then from the origin, we draw out a circle with the diameter of 80 millimeters. While drawing, I can type in on the keyboard, 80, press Enter, and then I zoom out. There is my circle with 80 millimeter diameter. To extrude this one into a body, click Exit Sketching, click the Sketch Profile.

00:53

Then we can extrude this one automatically up. This jumps in right into the Extrude command. We can extrude this to 200 millimeters, or we simply type in 200 and press Enter. Let's zoom out a little bit. And there we have a body created, a cylinder, 80 millimeters diameter and 200 millimeters height. We need a cap. To create a cap,

01:23

We can select the flat top surface, then go to Extrude, type in body millimeters. You see this actually moved this face up. Here's a small icon. The Extrude command has various end results. So we can join, we can cut, we can find the intersection, or we can create a new body. This is what I want. Select it and there we are.

01:52

You see now we have the bottle and we have the cap.

01:58

Let's turn the bottom off and take a look at what we can do with this cap. So I would like to shell this cap. And to do this, we can select the lower face. Then we find here the Shell command. By the way, you can also call first the command and then you select.

02:26

the surface or edge you would like to manipulate.

02:31

We will drag this to 2 millimeters of material thickness. Click Done. Go to a front view. Then I click on section view, click on this plane, and there you see, now we have a section view. So we shelled this cap with the Shell command to a thickness of 2 millimeters. In the top, I would like this to be thicker. I can select that surface. It reads out

03:01

that this is two millimeters thick. When I click in there and say 10 and press Enter, you see it adds then material to it. So I, with that command, move the face down.

03:18

I will turn off the section view. And now I would like to add a nice detail on top, kind of like a cylindrical cut out with chamfered edges. To do that, I will do the following.

03:37

I can select the top surface and go to a side view. Then I click on Extrude. I extrude this one down. You see that this will remove the material. We go by 8 millimeters. I will then here again, click on this icon and say, make me a new body.

04:07

First body, I would like to hide. This is now this disc I have. And when I inside the history, click on Extrude, you see that then the command and all the features becomes accessible. And here I can add a nice 45 degree chamfer to it or a draft surface. If I then select the top,

04:37

surface and extrude this a little bit higher up. Now I show my cap. You see how I can see now this part we built and then this face, I move a little bit to the side.

04:53

And then I would like to remove this one. Think about your modeling with foam. So you build parts and then you join and you cut elements. So it could now go to tools and say, subtract from the cap. I would like this body to be removed and click done. It's going to a 3D view and you see what happened. Isn't this beautiful?

05:18

kind of like created this body and then we removed it. We go to a section cut, there you can see what we created. And all this, we just solved via direct modeling. We now also need to model something that actually will connect to the bottle, which is kind of like the neck. And we have the geometry for that already. That is this inner surface.

05:48

So then when I select, I click on Extrude, then I drag this one down till you see this is all together. I can also make this bigger. Then I say here, make me a new body, because as you see, I created a body that perfectly fits into that cavity. Turn the cap off, show my bottle.

06:16

show the neck I built. Can now double click and shift, double click, select these two parts, click Union, click Done. All is one piece. If I now show the cap, there we are. The thing that is missing is to shell our bottle.

06:42

We can select the bottom part to make this a little bit nicer, give this a fillet. So 10 millimeters. Now I select the top part and do the shell by 2 millimeters, because you can see by having this lower edge filleted first and then calling the Shell command, the inside surface follows that. And I'll show everything. There you can see.

07:12

how we created this bottle just out of one sketch. And then basically using the Extrude, Face Offset, and the Shell and the Boolean command.

07:34

Now let's do a variation of this process where we do 3D modeling of the main base. And then we are going to use in addition, the Revolve command to design the cap. So the way how we do this is I can go into the top view and I go to Sketch. I create myself here, another circle. There we are.

08:04

This one I extrude up by 200 millimeters. Then I will create my neck by 30 millimeters as a new body. I would like to have this 2 millimeter of an offset, so I can select this outside surface and then remove 4 millimeters, 2 on each side.

08:33

Then these two parts, I double click with Shift and then go to Union. Can also, if this is easier, with Shift, select the two bodies inside the outliner, click Union to join them together. We do have this fillet at the bottom. So I redo this and then I do the Shell command by 2 millimeters.

09:03

So you see very much the same process. Now to design this, this cap in front view, this is really important. Also very important. You will see that I created my sketches always along the X axis. So they are centered in the world. So let me go back to this.

09:32

front view and now I can.

09:40

create a new sketch and you will see this plane is intersecting with this bottle on the right side. And I have all these magenta dots. These are snapping points. These are here, the snap elements. And I can use those to create a sketch that follows it. So from here to there, I can go up, then I go...

10:08

over to here, I don't know how far I click there, right click. And then from here, I click, draw this one up. And then I draw to the other side of this endpoint. You see here, plane intersection point, click, and then right click, stop. There's a midpoint. I click this one, connect this to there, right click, right click, drop the line tool.

10:37

And what I can do now is the following. I will make sure that all these lines are horizontal and vertical.

10:48

This should be exactly 40 millimeters. And now you see everything is green. That means the sketch is fully constrained, so it can't move. This also means when I exit the sketch and go to this comment here, this is where I did the offset. If I change this to 70, and let's go with 70 so we can see this. You see how the sketch followed it. It's pretty awesome.

11:18

Good for example, built in a 2 millimeter threading that goes in there. So I will go back to the sketch, click on it. Then here's a midpoint. I do not want to click on it, so I click somewhere else. Go up to here and click there, right click.

11:46

There's one line, one line there, not to the midpoint. Right click, right click, exit the line tool. Then these lines here all will be horizontal vertical. The distance here should be two millimeters. I have this as three, so I can make this one millimeter bigger. The distance here, four. That looks good.

12:15

And I would like this to be 135. So it's a 45 degree. And here, this should be five millimeters. So you see how I can specify all these dimensions. Going back here to this offset command. If I set this now to...

12:38

72. You see how this adjusted. And now this is exactly 2 millimeters.

12:49

I have essentially, as you can see, I go into a section cut, drawn myself half of the cross section of this part.

13:02

I can play here with these values to adjust this a little bit more. We are. And then I select the sketch profile, then Shift click one vertical axis that is at the center. And then I can call the Revolve command. There we are. So you see in retrospect that here we...

13:29

really build exactly the same model by using very similar tools. And then just then the cap, I use the Revolve command. And however, the outcome of the geometry is literally the same. If I want to perfect everything, I have here a two millimeter gap. So here I could go ahead and change this to...

13:59

70, then this cap, I will hide. There we are. And then select this, bring this to 74. And there we are. However, like a one millimeter gap there, for example.

14:19

Let's take a look at the Revolve command more in detail.