Sketch with design history

00:00

In this exercise, you will see how you can create sketches, which are coincident constraint to intersection points of bodies and how we can drive modeling and sketch features through variables inside the History panel.

00:24

in a new and empty design. Let's go into Top View. Go to the toolbar, select Sketch, select Circle. And from the origin, we will draw a circle with a diameter of 40 millimeters. Click and right mouse button, click, drop the circle. Then let's select the 40 millimeter dimension. And here is an icon X with a plus where we can create a variable.

00:52

When you click on it, you get a small list. Currently, there's nothing there to select, but there is a button called Create Length 1 equal 40. 40 means 40 millimeters because we are in millimeters. And when you click this, you see 40 is replaced by Length 1. And in the history, we have now a new variable called Length 1 equal 40 millimeters.

01:21

When we click somewhere else, you now see that the dimension states Fx 40. Fx is short for there is a function, a variable working for this um dimension and the outcome is 40. When we go to the length and right click and change it, we can call this width.

01:51

but width of what? It's very easy to confuse objects later. So let's call this Base Width, that makes more sense. And then when we change the value of the variable, you see how this automatically then updates the sketch.

02:13

Let's go into your 3D view. We will select the profile of the sketch, and then we extrude this one up by 15 millimeters. Also here, when we click into the dimension, we get this pop-up. We can create a new variable. You also now see Base Width is actually listed. We have no angle or number variable. That's reason why it's empty.

02:44

Click on this, this is updating, and we can now do exactly the same. Let's call this one Base Height.

02:57

Here we have the extrusion command. You see also there, FX 15. If we click in, however, you see it states Base Height.

03:08

We can create variables also inside the Add menu. Here it is. Let's call one, Fillet and three, then Shell and two. Close this one. And when we fillet this corner, we can then select

03:38

the Fillet variable and press Enter. And to shell this one, we can shell this. also here, select then the variable.

03:52

Also here, one more time, when we change these variables, you see everything updates. Now it's time to draw a sketch that is intersecting with this base. That sketch will represent the cap and it has to really adapt also to changes of our base. To do that, we can select Sketch.

04:22

Then I select this construction plane and we'll go into a 3D view. It will go into 2D view. I will go back into a 3D view. And there are those intersection points to which now I can start drawing to. And when you start drawing from those intersection points, automatically you are creating a coincidence point to those elements. I will continue.

04:51

drawing this over and there, over and then up. We can also draw this really fast and loose. Right click, right click, drop line, because we will straighten this whole sketch with a double click, and then we state horizontal, vertical.

05:15

What is green means is already constrained to what is blue can adjust.

05:23

For the moment, since we drew the sketch, when I update the Shell command, you see how the sketch follows everything.

05:36

We go back into the sketch. I would like this to be 10 millimeters, but this should be a variable. We call this one, Cap Height.

05:52

And this line should always be 50 % of the value of Cap Height. To do that, we can click into the dimension, remove everything. We get a warning sign because this is empty. And then we can select Cap Height. And then we do a very basic equation divided by 2.

06:21

You see it states 5. When this is being updated to 8, you will see that now here it states 4. So you see, we can also not only assign a variable to an edge or a modeling feature, we can also write very simple equations.

06:47

To finish this cap, I will now draw a midline, then exit the sketch. I will select the sketch profile, select the axis, go to Revolve. To make this easier to see, I will only create a minus 180 degree revolution. This object I will isolate first.

07:17

this edge, we will fillet with the same variable.

07:24

And then these faces here, will shell with the same Shell variable.

07:34

Perfect. Unisolate. And there we are.

07:42

One more time to show you what happens when we adjust everything. Now you see the cap adjusts. If we adjust the shelling, the shell result for the base, as well as the cap adjust, you can see that this is a really huge time saver.

08:07

The cap of this water bottle is a very good example to visualize this modeling strategy. I will go to a side view and zoom in a little bit more. And there you can see how the cap really nicely and smoothly flows into the neck of the water bottle. Let me show you the process I use to create everything. In this tree, I will scroll up, right click,

08:35

at a breaking point. And there you can see that at the beginning, I only created a sketch just for the bottle itself. Then through a few modeling commands, I created then a physical representation of the water bottle with very sharp edges. Only at this point did I then add the sketch for the cap, which when we take a look at it, you will see that these lines

09:04

perfectly line up with those intersection points where the sharp edges of the body intersects with the sketching plane. And this then allowed me to continue building all the other elements. I will stop the breaking point. I will go to a side view and then we'll add a section view from the side. And then let's zoom in.

09:34

And there you can see now all these individual parts are built. The cap, we have the threading. There is also a silicone ring in it. There is the spout, which can be rotated. At the bottom of the history, I do have a rotate and move command feature added. So I can then prototype live how this design could work and function.

10:03

When you have so many different elements also intersecting and overlapping with each other, it can be quite complicated to find parts. If you want to find an object inside the item list, you can with your mouse highlight over it, right click, and then say, reveal in item sidebar. There it is. And also in 3D view,

10:32

when you press the right mouse button and then select, select through at this point, you then get a list of various options. You could select the profile of the sketch or the complete cap or the complete bottle or individual faces, which were created during specific modeling commands.