Setting up parameters - Fusion 360 Tutorial

- [Instructor] Every dimension added to a sketch and every value used to define a feature has a name given to it automatically. In this video we'll take a look at an easy way to improve your ability to quickly edit multiple features in Fusion 360 by editing parameters directly. I'll start out by accessing the project in the data panel and opening the file. This file has a sketch that's already been completed. In fact, this sketch is a layout of the entire design and to help me keep track of it I'll rename it. Now I need to activate the sketch. This will bring up all of the dimensions, it will bring up a grid if I want, I can turn the grid off in the sketch palette, otherwise, I can just simply make modifications and add dimensions to it. Right now most of the geometry in the sketch is black. That's because that geometry is completely controlled having its position and its size known. The entities in blue, however, are still flexible. Grabbing one of them and moving them will exercise the sketch. I'll start out by building a relationship using a dimension. I'll use the marking menu to start the sketch dimension tool and set up the thickness of the bottom of this top portion. I can enter a dimension value directly or I can relate it to another dimension such as the thickness of the ring portion of this design. However, I don't want it exactly the same as that but I want it related to it. So I'll say the thickness times two. When I press enter, it will update the model to validate this. Some of the dimensions you'll see, such as the one we just placed, have an fx at the beginning. It's also possible for them to have relationships to multiple dimensions. For example, if I double-click on this dimension, you'll see that it is developed by saying that d3 divided by two plus d2 plus d2 divided by two is how that value is found. Well, what is d3? What is d2? You could click around on the sketch and figure out what those dimensions are. Or, under the modify pull down, we can open the parameters dialog box by selecting change parameters. In the parameters dialog box we see a listing of what type of dimension was placed, the name of the dimension, and the current value. The 1.5 millimeter dimension I referenced and then said times two for the thickness of the bottom of that recess, is called d2. The thickness of the pin or the diameter of the pin is called d3. So that's where those values are. But trying to keep track of what the current value is to remember what the name means is cumbersome. So what I'd like to do is, with a slow click, just rename some of these values so they mean something. This is a great way to make it easier to keep your designs in check. It's not specific to working with metal but frequently, in metal parts, we are working with relationships between parts and these parameter values and the way that Fusion works can be very useful across multiple components. I can also select values if I want to change what those values are here rather than in the sketch. But for now I'll click OK and see that in the sketch absolutely nothing is changed. However, if I select that same dimension, I can now understand a little more easily how that was calculated. Let's go back to the parameters dialog and make some changes. Let me shrink this down a little. I'll come to the wall thickness and change it from 1.5 millimeters to three millimeters. By pressing enter, even with the dialog open, it will update the sketch. You can also make other types of modifications such as saying .15in and it will do the calculation for you continuing to display the metric value in the sketch. I'd like to return that to three millimeters, though. I'd like to also update the overall diameter to 39 millimeters. And then I'd like to add another parameter which isn't in the sketch. It will be a user parameter. I'll us this parameter a little farther down the road. I'll establish what the width of the overall part will be, I can choose what units I'd like to use, either using a length unit, a mass unit, area, depending on what you want to do with the parameter, you can use any of these values. I'll keep it millimeter and enter an expression of 20. So whatever feature I choose to make equal to width, it will be 20 millimeters. I can also add a note. When I click OK it will add this parameter to the dialog and if we scroll to the right we can see the comment has been added. I'll click OK to close it and see the updated sketch is still there. I'll now finish the sketch and be done with this step.