Join John Helfen for an in-depth discussion in this video Parameters, part of Autodesk Inventor 2018 Essential Training.
- [Voiceover] Throughout this course, you've heard me talk about adding intelligence to a sketch. Parameters are one of the ways you can do that, and you might not know it, but you've already been using them. As a matter of fact, when you were learning about dimensions, Inventor was already creating parameters for you. In most cases, the parameters that Inventor creates automatically are gonna work just fine, but knowing how to manipulate parameters and use them to your advantage can be incredibly helpful during your design process. Let's look at parameters a little more closely. We're gonna need a new part file, I have that open on the screen.
If you don't have one, go ahead and open a new part file, and let's create a sketch. I'm gonna right click and select New Sketch, and I'm gonna select the XY plane out of the origin geometry. We'll go ahead and pan down and to the left to give ourselves a little bit of room to work. Now we're gonna right click and select Two Point Rectangle. We're gonna hover near the center point, and left click to initiate our rectangle. As we drag up and to the right, you can see that the heads up display is providing some values. Let's go ahead and enter 1 in the top value, hit tab on our keyboard, and hit .5 for the other value, and then hit Enter.
By doing that, we've created a rectangle that is fully constrained, and fully dimensioned. It's one inch long, and .5 inches tall. If I right click and select OK to get out of the command, what also happened that you don't see on the screen, is that Inventor created two parameters for us. We can look at the parameters in two ways. We can either go to the quick access toolbar, and select the function button here, or the parameters button, or from within the manage tab, you can also reach that same button. I'm gonna go ahead and stay on the sketch tab, and just use the one on the quick access toolbar, just so that I won't have to switch between tabs.
I'm gonna go ahead and launch that, and you can see our parameters dialog box now is filled with some information. Over here on the right, you can see the model parameters. These are the parameters that Inventor's automatically creating, and it's essentially just creating sequential numbers. You can also see the values here, and these are important, because this is a bidirectional dialog box, which means any change made here is reflected in the background as well. If we enter 1.5 as the value and hit Enter, you'll notice that the geometry and the dimension update.
Let's go ahead and set that back to 1, and hit Enter, and our geometry updates. We'll go ahead and close the dialog box for now, and then we'll come back. The next thing I want to do is show you that we also have these values showing up in the graphics window when you edit a dimension. If you double click on this .5, you'll notice that the dialog box says that we're editing dimension d1. The reason this is important is because you can build intelligence into this sketch using these parameters. Not just the names, and not just the values, but, if I know that this is always gonna be half the size of this overall length, I can simply select all the text, and click on this value, and you'll notice it enters d0, or the parameter for this dimension.
Now with that value there, we could simply hit Enter, and what we now have is both dimensions at the same value, which is exactly what we told it to do. This is d0, and this is a function that is getting its value from another location. The fx is the label that indicates that, and where it's getting that dimension is from this other value. If we double click this, you can see that we only have d0 here, but if we edit this dimension again and put in a slash, or a division symbol, and then 2, and then hit Enter, now we're back to where we started.
One inch long, and one half the distance of that overall length for the height. Now, I keep calling this length and height, but right now Inventor knows it as d0 and d1. Let's go ahead and look at how we can change that. We could go back into the dialog box, and we'll do that in a minute, but if we want to do it a little more efficiently, we can go ahead and double click this value. Right now, we're editing d0, and it's value is one inch. If we go ahead and click into that dialog box and hit Home, and then type width, you'll notice a couple of things.
First, we've got the text showing up as red, which is an indication that something's wrong. Second, this isn't really gonna work for us. What we need to do here now is enter an equal sign, and Inventor turns the text black again indicating that this is a valid expression. What we're telling Inventor now is we want to name this dimension width, and we want to give it a value of one. When we hit Enter, it doesn't look like anything's changed, but if we go ahead and double click on this value again, now you can see we're editing the dimension Width.
Let's go ahead and close that, because one other thing happened as well. If we go back and double click on this formula, Inventor's automatically updated this to switch from d0 to Width here in the formula. It also added the ul at the end. This means unitless, it's just something Inventor does so that you can create math formulas in the parameters. Let's close that and go back and look at our parameters dialog box one more time. If we go to the quick access toolbar and click the parameters button, we get back to the dialog box, and you can see all the changes that were made show up here as well.
The only thing we have left is we have this d1, which isn't very descriptive, and I've been calling it height this entire movie, so let's go ahead and update that. Let's go ahead and enter height, and again, because it's bidirectional, when we click done, and we return to this dimension and edit it by double clicking, you can now see that we're editing the dimension height, and it's gonna be width divided by two as its overall value. Hopefully you can see how parameters can be incredibly powerful in adding intelligence to your design.
It allows you to create rules that make it so that you have to do less work, and you let the computer do the calculations for you.
- Reviewing interface changes
- Projecting and importing geometry
- Working with Autodesk AnyCAD
- Understanding part modeling
- Building parts with placed features
- Working with partial chamfers