Learn about how constraints are what determine the shape and size of your curves.
- [Narrator] Here I want to talk about applying constraints. Now, there are several ways to apply constraints in V5, and to be quite frank, all you really need is this one icon, constraint. Since we're going to be using it over and over again, just simply double-click on it. That way, when you do go to use it, you don't have to continuously go back and select the icon. I've talked about this a little bit before, but I want to stress that point. So, I'm going to double-click on the constraint icon. Now that it's active, remember anytime something is orange, it means it's active, I can go ahead and start applying my constraints.
All sketches, every single sketch needs to be defined by its location, its shape, and its size in order to fully constrain a sketch. Now, a constraint is basically a rule, it's a law determining how big a line is, or length of a line, how big is an arc, where does something sit out in space, its relative position to external data, or internal to the sketch. Same thing with the shape. What shape are we going to end up with? In this case, it's going to be a rectangle with an arc on one of the corners.
So for this, I want to close off the sketch. Now, I can use a trim, but I just want to show you that I can also use a constraint. I'm going to go ahead and pick this endpoint to this endpoint. Now that I have that selected, you'll see a dimension, that's the distance between those two endpoints, appears, and it is tracking along with the cursor. With this, I don't want to click the dimension down. Once I click again, that third selection, it will write the dimension. What I want to do, and this is what I mean by you're able to pretty much get all the constraints that you need using this one icon, with the dimension active, I'm just going to right mouse click.
So, using that third mouse button on your mouse, you'll get a list of constraints that are available based off of the elements that you have selected. So, when I specify coincidence, coincidence means on top of one another. In this case, I'm taking two points and making them coincident, one on top of another. I also have the ability to put a line and a point on top of one another, or two lines, something co-linear. So in this case, I'm just going to simply select coincidence, and there you have it.
Those lines are now endpoint coincident. Next thing I want to do is I want to capture the position of the sketch, and I'm going to reference it back to the origin of the sketch. So, I'm going to select my horizontal, and select this line, and what you're going to notice is, again, I have a constraint attached to that line, and this is an angle constraint. Well, I don't want it to be an angle constraint. What I can do at this point is right mouse click, and specify that I want them to be coincident.
I can also specify a distance, which I'll do the next go, but in this case, when I specify coincidence you'll see that line now lines up to the horizontal axis, and I have this little green circle indicating coincidence. I'm going to do the same thing with the vertical and this line. You'll notice, once again, I have an angle. I'm going to right mouse click, and in this case, instead of specifying coincidence, I want this to be a certain distance away from my vertical, so I'll specify distance. As soon as I say distance, you'll see that line now is parallel to the vertical, and it's that far away currently.
So, I'll just double-click on it. And again, anytime you want to modify anything, just simply double-click on it, and specify, in this case, the value that I want, I'll just say 200, and I'm going to hit enter on the keyboard. That way, it just writes it right away. Now that I have these two curves basically defined where they're sitting in space, I can continue around my profile. In this case, I'm just going to pick this line to this arc, right mouse click, tangency.
Do the same thing, this end, tangency. Here I'm going to pick this line to this line, and instead of making it perpendicular, I'm going to give it an angle. Now, one of the great things about V5 is it's not pick specific. For the angle, you can pick anywhere you want to on the lines, and place it anywhere you want to, any one of the sectors. So, by selecting here, I'm saying I want this, by double-clicking on it, to be 110 degrees, hit enter.
And you'll see, there's my 110 degrees. If I double-click on that once again, you'll see that I have my angular sectors located here. So if I want to change that, I can change that. Next, I'm going to select my arc, and just simply place the dimension, double-click. V5 does a great job with your radius and diametrical dimensions. You'll notice right now, by default, because it's an arc segment, it's giving us a radius. I can change this to diameter if I want to, and it automatically doubles the value.
Remember, diameter is twice radius, radius is half diameter, and it does the math for you right away. This line to this line, right mouse click, distance, double-click, and give it a height. And the last thing I need is the length of this line, so I'm going to pick the line, put it down, double-click on it, and give it the appropriate value.
So, those are the basics behind the constraint. Remember, double-click on the constraint icon, you can pick one line, two lines, line and an arc, and by using that third mouse button, while going about using this constraint tool, you can pretty much get any constraint that you want. As we go through the course, and we create some of the sketches for the parts that we're going to be designing here shortly, you'll see me using that heavily.
- Working with the CATIA v5 UI
- Understanding the menus
- Part visualizations
- Part design workflow
- Creating a sketch
- Basic editing
- Creating and editing sketch curves
- Part design
- Measures and analysis
- Building a project