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When we looked at creating dimensions we talked about adding intelligence to a sketch. Parameters are what give dimensions the ability to add that intelligence. And I want to show you how parameters work right now. I'm going to start a new part file by selecting New from the toolbar Selecting Standard.ipt as my template and clicking Create to start a new part file. I'm going to get into a sketch by creating a new 2D sketch. I'm going to select a plane from the origin geometry that's presented. And I'm now in the sketch environment ready to create geometry.
Now, when we were creating dimensions, what you didn't know is that you were already using parameters. Inventor automatically is creating a parameter for every single dimension that is created in the system. It does it in a very hidden way, but you can access those parameters, because they allow you to do things like create formulas, and make relationships between pieces of geometry very easily. I'm going to start with a very basic shape. I'm going to create a rectangle. And what you're going to see here, I'm going to go ahead and enter a value of one for the width.
And I'm going to hit Tab on my keyboard. And I'm going to enter 0.5 for my value on my height. And I'm going to hit Enter. Now, what I've done here is created two dimensions on a single rectangle. What you didn't see is that in the background, Inventor created two parameters that represent these values. On the Quick Access toolbar you'll see a little function button. Or if you go to the manage tab, you'll see the same button here in the Parameters panel. If I click on that, it'll bring up our Parameters dialog box and you can see d0 and d1, which are 1 inch and 0.5 inches.
Which are actually the value of the dimensions on the model behind us. I'm going to, reduce the size of this so that we can see this a little more clearly. And, what I'll do here, is indicate that this dialog box is, a way to edit, bi-directionally, the dimensions that were just created. If I enter 1.25, instead of one and hit Enter, you'll notice in the background that the dimension changes and the model updates as well. If I go back and return that to 1 and hit Enter, it returns very simply.
Now, I'm going to close this and we'll come back to this dialog box in a little bit. Another thing I wanted to talk about is the naming. In that dialog box you saw d0 and d1. If you double-click on a dimension to edit it, you'll notice the name of that dimension or the name the parameter for the dimension listed at the title bar of the dialog box. In this case, the one inch dimension is tied to parameter d0. Now, d0 is not very descriptive. Inventor's just going to go d0, d1, d2 and select consecutive numbers.
And in most cases that's totally fine. You can even use those dimensions. For example, those names are perfectly acceptable. If I wanted, let me get out of that dimension and go to this 0.5. If I wanted that dimension to always be half the distance of this, with the text highlighted, click on the one inch dimension and you'll see that it enters d0 for me automatically. I can then use the slash symbol, or divide symbol, and enter /2, and hit Enter.
And you'll now see that I have a, a function indicator here. And the value hasn't changed. But what I've done is it connected these two parameters. So that, if this first one changes to, say, 1.5. Then, when I hit Enter, you'll see that the dimension that's driven by our function is automatically updated to be half the size of the dimension we just changed. Now, again, if you go back and double-click on this, you can see d0/2. UL indicates unit list.
It's just a value that allows you to do formulas rather than enter inches or millimeters for this specific formula. I'm going to go ahead and close this. And rather than use d0 or d1, I'm going to go back to this first dimension, double-click it, and instead of 1.5 what I'm going to do is I'm going to name the parameter on the fly. If I hit the Home button, here, I can say, I can type, width, and you'll notice that as I type, everything is red, indicating something's wrong.
At this point, this is an invalid value. It's not going to work. If we hit OK now, we're going to hit an error, and Inventor's going to tell us something's wrong. But as soon as I put an equals sign in here, you'll notice that the color changes to black. This indicates that we've entered a valid expression and Inventor can continue on. If I hit Enter now, it doesn't look like anything has changed. But what you'll find is if I double-click that dimension again, we've changed the oh, the name from d0 to width, and if we go over here to this function, Inventor has automatically updated d0 and swapped out width.
If we close that and return to the Parameter dialog, again you can get to it on the Manage tab, or if for example you're on the Sketch tab, you can always get to it from the quick access toolbar as well. Now here you'll see by naming it on the fly on the graphics window, it's automatically updated in our Parameters dialog box as well. The opposite is true as well. We can select d1 and perhaps enter height. And in this case, when I hit Enter, again nothing's changed, but if I hit Done and go back to this dimension, you'll see that it's height now instead of d1.
So these are the parameters that are most important to add intelligence to the sketch. It's not something you would necessarily use or modify in every case but, being able to center something by do, doing simple math, to ensure that a rule is maintained, for example. I know that no matter how wide this part is, its overall height has to be half that distance. So I can build in a very simple formula to ensure that my design intent is maintained, regardless of how the model changes.
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