Okay. So the first thing we're talking about right now is keeping our sketches simple. You'll notice that this model, although I could have actually done almost all of it in one sketch, I'm going to fully define and sketch each shape. Extruded, give it a feature, then do the next sketch. Now it's a circle. I'll extrude that then next sketch extrude it. Why do we do it this way? Well, I now have a sketch that can be edited for each one. My performance increases because my sketches aren't too heavy. So let's look at this a little bit closer. Here's the D pad example, and this is a good one. I saw this in one of the AAU classes on sketching, where if you take this model and you break it up by sketch feature, sketch feature, the performance is much better and the sketches are so much easier to manipulate, maintain, make changes to now.

So if we do the opposite and, and we're going to do multiple offsets, we could pattern that anytime there's a pattern, that's a good giveaway. You don't want to be doing sketch patterns for this much complexity. So now, so now we can extrude each profile. That's a full extrude. Then we turn on the visibility of the sketch. Find the next one can see it. This one is going to be trickier to work with. I can select through and find the right profile might want to hide the body. Find the next one, hit extrude, do the next join rule of thumb. Keep those sketches as simple as possible. Next one, sketch on these three planes as much as possible, the front top, and right plane, as well as use that origin strategically, if you can keep the origin at the center of your design, it's going to make your life a lot simpler.

And if I'm extruding this, if I can keep it symmetric about the origin, that even adds more value. So in this case, if I do a symmetric extrude, then that's going to keep my three points right in the center. So when we look at this, in an example, my planes, if they were all in the center, that makes my life so much easier. So let's, let's look at it when I first do this first extruded and do that right off the origin. So I extrude this my next one, when I want to do the cylinder coming from the middle, where are my planes? Well, I look there right there, right in the center. So I can easily select those planes and start sketching. I don't have to do a brand new plane so I can do that next sketch and extrude going up extrude, coming from the side, shrewd, coming from the middle. Right?

So again, rule of thumb, keep that origin in the center as much as possible. The other thing, when it comes to the origin, it is critical. As far as defining your sketch, I'm going to talk about why defining the sketch is so important. But even though I fully define this, a sketch with a bunch of dimensions, you'll notice that it's gonna stay blue. Even though I dropped on a bunch of different dimensions. And why is that? It'll move around because it doesn't know how it relates to the origin. So I either have to dimension to the origin. I got to do distance to the origin, both vertically and horizontally. Then my sketch will be fully defined. It's all black. That's good. Or if I simply connect to the origin, now it's fully defined things. Have to know how they relate to the origin to be fully defined. The next thing, constraints or dementia.

I had this friend and he would send me a CAD model from time to time. And it was always the same question. It's a Tyler, I'm going to add this dimension. And when I do, even though this sketch looks great, when I try to scale it up or down, it goes crazy. Right? It does this. Okay. That looks okay. But if he makes this one 50, how come it just went wonky like that. Right? And I'd always asked the same thing without even looking at it. Did you fully define your sketch? Did you use constraints in this case? It'd be really smart to do your constraints and think about how you would describe it to someone without a dimension. You'd say, well, it's a rectangular plate. I'd say, okay. So that means these two lines are parallel and are they equal? Yup. These two are equal.

Uh, these should be, that should be a horizontal line. That should be a vertical line. And what about the way the arc goes into the line? Well, I want tangency. I want that nice, smooth transition from line to arc. So I'll do tangency. So that's going to keep that corner intact with the round. The other thing we definitely need to do is connect it to the origin. Some point on this sketch should be connected to the origin or, um, case. We could do a sketch across the middle and make that construction line, select the line and the origin do midpoint. There we go. So at least we know it's connected to the origin in the center. Okay. So now add a dimension of 60 and this one of 30. What are we missing?

What drags. Okay. So it looks like I failed to put that at horizontal. What about the arcs? They should all be equal or we should put in a dimension for each arc. Okay. So that, so they're all equal and they're three. Great. I already have that. Now what happens? This is moving up and down. So I haven't related it to the origin. As far as maybe the hype of the origin, we could do a construction line or a distance. Now it's fully defined. So great idea. Use constraints first and then dimensions. The next one, troubleshooting a sketch. I always drag the blue points to figure out what's missing for constraints. But when you go to hit extrude and it will not extrude it, doesn't give you a profile and you can't seem to get it to work. I learned this line method. I love this.

This was from an AAU class as well. And basically you just sketch a line through it. And then when the profile wakes up, that tells me this side of it's fine. So you can start adding lines as you go. Okay. So it's above. Let's go there. Okay. So it's somewhere in that range and you don't have to keep these lines intact. You can even drag them and you can start to kind of pinpoint where the problem is. So it looks like it's somewhere in here. If I zoom in on that, that point was not connected. And now it's coming through just fine. So you can use that as a way to pinpoint what is missing in the sketch.

When dimensioning, if you add a dimension to the sketch, it's black and fully define meaning it's going to behave with the design intent that I have in mind. But when I place one more dimension, it gives you this message. It's saying it's over constrained. What does that even mean? It means you're adding one too many variables to the mix, right? So if you hit, okay, it's now a reference dimension and it's a measurement try double-clicking it doesn't do anything. Okay. How do you toggle something? I'm sorry. And I, that, that is duplicate. I didn't actually mean to do duplicates. Let's add a new dimension. This one over constrained. It's a reference. What if you'd rather have this one, maybe then the radius, or maybe then even this height, right? So what you can do is right. Click on one of your dimensions, an option. You can delete a dimension and then you can right click. Okay. So I delete that dimension. And now this drags up and down, and this is reference up this reference updates, but what's right. Click on it.

If you right. Click on the dimension and do it just right. Sometimes it's not there. You can toggle this to driving. Now it's an intelligent, smart dimension. It's parametric and it drives it. Another really good rule of thumb is to name your sketches. So if this is the main, so if this is the base profile, and this is the, and this one is the vertical cylinder, that's going to be a kit, a lot easier to work with in the future. If you saw my other video and I'll link to it, of how you can build this whole model from one sketch. What I did was I sketched a bunch of different profiles or sub regions in one sketch. And this is acceptable because this is a pretty simple model. It's not that overwhelming. There's not that many dimensions. There's not that many constraints. And so when we start extruding, I'm effectively extruding. Let's do it together. So I'm going to extrude the base profile first, right? And then I'm an extrude, this upper profile a little bit.

And then I can reuse.

Here's the little trick. If you want to select something, that's hidden by geometry, you can hide the body or you can do a select other and click with the left, click near it. And it'll let you pick the face or the profile or the other face. So that is what's called maybe a select other and other CAD systems and infusion. It lets you select through things. I love that one. So now if I extrude and this is a new join and also we want to get this profile too. There we go. So we're using the same sketch over and over again. And to keep that other rule of thumb, that it's better to do a sketch and then a profile and keep them simple. It makes they can edit easier and perform better. So the next one you don't really have to trim infusion fusion.

If I add this circle and I want to trim that off, whoops, it D for dimension and a trim that I can, but what you want to keep that as a reference, you don't have to get rid of it. You can just extrude that profile and use that sub region and leave that there. So it doesn't hurt anything. But if it's bugging you, there's a couple options. You can hit search as key for search trim, trim it out. Right. You can do that. But if you'd like to keep that reference there, here's another option. Do the search and do a break. If you break this, it's now going to be two entities. So it's been broken there in there. And now when I select it and hit X on the keyboard for construction, now it's just referenced geometry over here, but then the geometry where I need it, pretty cool.

How do you drive everything in a sketch with the same dimension? So if I find this dimension hover over it, it's D one. Okay. So if I go find my parameters, do a search for parameters. I can find all of my sketch dimensions right here in this first sketch. And then the other features and their dimensions. I could drive everything off of this. What's rename it and call this our master dimension or offset dimension or whatever it is you want. And now I can do everything is related to the master demand. It's a master dim times 1.3. We'll do this one. This is the master down by, by two master Dem kind of get where I'm going there. So times 1.3, five. Great. So I could go down the list and drive all of these with one dimension. So it's 70 and those others are going to update the little F X shows that it's a function that's being driven by the equation. Hey, one of my all time favorites, when I select a face or a plane and hit sketch,

I hit the S key. It wakes up my modular toolbar. This is intelligent based on that. I'm in a sketch. It gives me sketch stuff and it's got an awesome search. I love this thing. I use it all the time. If I'm looking for a, fill it from looking for a revolve, if I'm looking for a pattern, I start typing and it finds it a love that also we could, if we wanted the, one of the other rectangles, like the center rectangle, I can add that to the shortcut bar, hit this little arrow. It's going to add it right there. Now that is available for the next time. S find that rectangular centered rectangle, drag that in now. Okay. Or a note about rectangles, I'd say use those as often as possible. Y when you add those constraints, the vertical and horizontals automatically, as well as if I type in the number and hit tab, it goes to the next one.

So it's letting me add dimensions as I go and relationships. So that's a little bit more intelligent, faster way than sketching it line by line. Okay. What about the grid? Come down, find your grid, snap to grid, settings, and grid settings, adaptive based relative to what you're working in or fixed, which you then set up your own grid that you want, but it does have to be turned on in the sketch grid palette. So I turned this on and now I have these snapping points that I can sketch to. And so it's snapping to this large grid that we can use. What about these other options in the pallet construction line, select an item. It goes to reference the shortcut is X on the keyboard. I love the lookout option. This one just looks directly or normal to your sketch. So if your views are kind of out of sorts to where your front view is off it a little bit, it's helpful just to go straight.

You can now look normal to it with the look at mapping is kind of obvious that it wants to snap to, okay. The next thing, if you were to start a plane somewhere in the middle of this part, so I'm going to do an offset plane from this phase, somewhere in the middle of the part. How about right there? And you want to sketch in this geometry, maybe we're going to work on a cut or a special slot or key way, whatever it is. If I select the point, hit sketch. If this geometry is in your way, you can use the slice tool and it'll slice wherever you're at allowing you to sketch and work with this, which also gives us next to some of our other things, the profile and the projected geometries. I now can snap to this projected geometry. I'm using edges that are aren't really there, but they are the extension or the end of that virtual part.

Pretty cool. Yeah. The thing sometimes in a sketch, it's helpful to turn off the dimensions temporarily. It's also can be helpful to turn off those constraints if they're getting in your way, but keep in mind if there's so much on the screen, that might mean that your sketch is getting a little too complicated. Just keep that in mind. Okay. When you're sketching and you start a new part, how do you change the units right here in document settings and change it to any other units as well as this is where you can set your default, or you can do it up in the preferences. Some of my favorite sketching preferences are under design, go into design. I definitely like to have the auto predict project edges look right at the sketch by default. I want it to go normal too. When I drop a dimension, I want it to automatically edit or open up. I love that one. And then this scale, entire sketches, first dimension of love this one, one of my absolute favorites.

And if you've seen my other video on that for scaling the entire sketch, let's look at that real quick. So if you go to the trouble to get this fully nice dementia reign sketch you, you know, go to this trouble to sketch it just right. But if you're off by an order of magnitude, you can select the item. If I make this a thousand, instead of it going crazy and going just nuts, it's going to look like the same sketch. And that's because of that scale off of the first dimension. I love this one. When you're sketching lines, you click you click. And this is called chaining. When you'd like to stop, hit escape on the keyboard, that'll stop it. Another way that you can snap when you're sketching is you can DoubleClick really quickly. And it, it, it creates it, but then stops. Or as you're sketching, you can hit this little plus sign and it'll stop sketching. I like the escape key. It's probably my favorite.

Let's talk about the box select if this is overlapping and we've got some lines that kind of corresponded the same spot when I drag to the right, it's going to grab anything that touches the box or is in the box. So it grabs everything that I was near right now. If I select to the left a box to the left, that is going to be more liberal. If it's trending to the left more liberal, it's going to let anything that even touches the box. Sorry. I think so. If I, if I select to the right, nothing's going to get selected in this case, because that's not fully in the box, go to the left. It grabs that line.

Sometimes you need to dimension from midpoint to midpoint shortcut to do this hold shift on the keyboard, get near the mid in a, wake it up, get near the midpoint. I'm holding shift. And now I have a dimension to mid points and I could do the true distance or maybe the horizontal distance or the vertical distance. Okay. Let's talk about the quick measure. I love this one. Anytime you want to measure a line, just simply select it down at the bottom. It gives you that distance. If you hold control and select two lines at an angle, it gives you an angle. So it is intelligent, kind of based on what you select. If I select these two points, I think it's just the distance between them. All right. If you have slots, if I do as an S search for slot and I drop in my slot, we'll make it horizontal. Okay. If I want to dimension from arc to arc, when I hit D for smart dimension, police it, guess what happens? It goes center to center of those arcs, not what I wanted. So I'm going to right. Click do arc tangent before I place it. Now I'm gonna right click it's arc tangent, still

And click on it. And now it goes, arc arc. There we go. Okay. Here's the pro tip that I just figured out. I'm so excited about it. Sometimes you need to be able to reuse geometry, right? So maybe you say like, I need to get rid of this block right here. Well, it's very easy to do with the extrude command. I can hit extrude and it's just going to reuse that profile and cut that out. That's great. That's not really a big new secret, but when do you want to sketch something again, without having to, there is the project tool. Now, when you're sketching and you hit project, it redraws that, but the thing is those really aren't sketch lines that I can reuse. And maybe there is a way to do that. I don't know how to do it. So here's my workaround. If, if I want to reschedule this face, I'm going to start a sketch and I'm going to do offset and I'll select the edge, the outer edge, and I'm gonna do an offset of zero. This was pretty exciting to me. So it reschedules that. And now if I find that constraint for offset right there, that little tiny icon and hit delete. Now these can be maneuvered and redefined. I could add dimensions to this, let's hide the body so you can see it. So now I have this brand new sketch based off of something that was already drawn, but I can add new constraints and design intent to it. Pretty cool.

Last few bonus tips, of course, the line to our command. Hopefully you already know that one clicking as I'm clicking. If I drag at the end points can add a tangent arc, okay. When you're sketching. Um, and this can be especially helpful. Like when you've got a bunch of parts or components like this one, when I'm sketching on this top face, it naturally wants to infer to everything underneath. It's got all these snap points that it wants to go to. So if you don't want to add a constraint, you can hold control on the keyboard, and it's not going to snap to anything. This allows you to kind of sketch freely without any concerns that it's going to snap into place or add a constraint.