[MUSIC] So, let me first start out by hiding my body. Notice that when I turned it off, it hid just the body. You can hide things at both the body level and the folder level and this applies to every folder and every content in Fusion. You have to be aware of that and you have to take note of it because it's very easy to inadvertently turn off the entire folder when you want to turn off a specific component. Let's look at the origins folder for example. I turned off my folder, I can't see anything inside it. All the light bulbs are on inside, but I still can't see it. Check the folder to make sure it's on. I've made the mistake, you will make the mistake as well. So let me hide this body, and let's start talking about sketch base construction. Sketches are really good for fine construction. Okay, I'm going to start off by drawing a sketch. I'll click on my Create Sketch, and I need a specific flat item to draw on. Any one of my standard three planes will work, I'll pick my top plane, I'll look at it, and now, anything I draw is contained here. So, I'll come to the Sketch dropdown, I'll go to Rectangle > Center Point Rectangle. Draw out from the origin, drag it out. I have not clicked yet, notice I've got dimensions that are highlighted. I can access them now but I'll just proportion it, left-click and now it gives me my rectangle. The user interface shows you this yellowish orange color inside, that tells you that it is a closed profile. Closed profiles means that the computer can see between the two. As an example, I'll draw a quick C here that's open. Notice that it does not give you the orange detail. If I close off the left side, immediately, Fusion gives me that visual feedback that that is a closed profile. Closed profiles are very important to sketch base construction. You use those to create your information in 3D. So, if I come over and I change this line to a construction line by clicking on it and using the sketch palette to switch it to construction. Immediately, it shows me that is not a closed profile because the right side is not a constructed, it is not a true line, it's only a construction line. So, if I click on it, And return it back to normal construction, again, I'm presented with a closed profile. Let me delete this one, I do not need it. And let's make this real by adding a dimension. I click on the line, I drag up, I click again, quickly add 300 millimeters. Click, click, we will switch it to 200 milllimetrs, and now I have a fully parametric controlled rectangle. Stop the sketch. Notice that I have a sketch folder now with Sketch6. If I want to edit that sketch again, I right-click > Edit Sketch, and my sketch is open, or you could say right-click > Show Dimensions, gives you my dimensions while the sketch is still closed. I can double-click, I can edit them, change it into sketch updates. Don't forget that it's also marked in your timeline as a sketch action. So Create > Extrude, I grab my profile. I pull it out, and I'll say new body is perfect for my operation, hit Enter, and now I have two steps. My sketch, which is turned off automatically. I can turn it back on, and I have my extrude feature. It does not own the sketch. So, if I change my dimension on my sketch to 350 millimeters, the feature downstream will adjust when I change the sketch. Now, that is the power of parametric modelling, and when you do sketch based modelling it's very precise. It's not as fast as primitive construction which is really fast but when you need to do something precise, that's when you use sketch-based. So, I've got it built, I'm happy. We'll come to New Sketch. I'll draw a new sketch here. I'll look at that. I'm drawing on the top of that box. We'll do a two point rectangle and I'll just drag it out of space here. Now, notice that I have not left-clicked yet. My dimension is highlighted. It's asking for my dimension and I add 200 there, hit Tab, and enter 150. Now, I'm going to hit Enter. It automatically adds the dimensions for me. I do not need to do a secondary step operation to add those dimensions. So we'll add a dimension here between these two. And I'll say 50 millimeters, it will always be 50. We'll do another one here to this edge and I'll say 25 millimeters. My sketch is now fully controlled between the two sketches. It will always relate back and be driven by the parent sketch. Stop sketch, show my dimensions. So now, you can see exactly how I've made relationships between Sketch7 and Sketch6. So, when we say extrude now, Fusion is super smart on how you pick what you've used from your sketch data. It knows that when I select this profile here, it subdivides based on the relationships of where I built. I can pick either side that I want, any combination of these subdivisions to extrude. Now, that's not exactly what I want now. So I'll clear those, and I'll pick this profile, and this profile, and I'll drag it up, and we'll say 100 millimeters, and we'll let it join. The key is that these dimensional relationships on the sketches are parametric. And what happens to my second extrude if I adjust this dimension, and we make it 500. Will this box move as well? Hopefully, you said yes because that is the essence of parametric modelling, creating a parent sketch. That's information drives a child feature, followed by another parent sketch, followed by yet another child feature. Each one of those follows the previous leader. Do leverage this skill set. It is how parametric modelling works. My task for you guys now is to start building with sketches. Start to build and construct. Use some sketch construction, build one or two sketches, and then create sketch based positives from them, play with each one of these tools, read the descriptions, use the tools, there's nothing you can do wrong. Now, let's build. [MUSIC]
