From the course: SOLIDWORKS 2021 Essential Training

Basic steps for 3D modeling - SOLIDWORKS Tutorial

From the course: SOLIDWORKS 2021 Essential Training

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Basic steps for 3D modeling

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- [Instructor] In this movie, we're going to be covering the basic steps for creating a model inside of SolidWorks. To get started, I'm going to cover the six steps of Modeling. The first one is to select a face or a plane. When you first get started with SolidWorks, you don't have anything besides the three fundamental planes and see if you can choose one of those to get started with. Number two is starting a brand new sketch on one of those fundamental planes or if you work through the model a little bit, you have some planes or faces, you can choose then go ahead and choose those. Once we started a new sketch, we want to draw some geometry and then we want to take that geometry and we tie that geometry in to the origin. So it knows where it is in space. We're going to add relationships and dimensions to that geometry, and then go ahead and create the feature, whatever it's going to be. It's going to be an extrude, if it's going to be a cut, if it's going to be revolve, we're always going to be pretty much do the exact same six steps for each one of those features. Now there's some more advanced features that might not use these exactly. But in general, we're going to go ahead and follow these six steps from most of our modeling. Now let's jump back over to SolidWorks and see how it all works. All right, so the first step is to select a face or plane. Now, right over here on the left, you can see I've got the front plane, I got the top plane, I got the right plane. I can choose any one of those to get started. And in fact, if I come up here to sketch, if I choose sketch, the first thing it's going to ask me is, Hey, select a plane on which to create a sketch for the entity. So it's already telling us what exactly it needs so I can do it either way. So let's go ahead and choose something like the top plane. Now, step two is going to be start the new sketch. We just did that. Step three is draw some geometry. So let's go ahead up to the sketch tool bar. Let's choose this two point rectangle, and I'm going to choose this lower left-hand corner up to the upper right-hand corner and draw out a rectangle, all right there it is. Now notice we get these little green boxes that pop up as I draw. Now, those are relationships. So these ones over here are saying, it's a vertical line. And over here, it's saying, this is a horizontal line and you can add and delete relationships by clicking on them and hitting Delete in your keyboard. And you can also add them using the relationship toolbar, which we're going to cover in a second. We want to tie this geometry into the origin. So here's our friend, the origin, and here's our geometry. So let's go ahead and tie those together. Now I have this point here. I can just grab that point and just drag it over so it snaps on top of the origin. Notice what happens is when I do that, it does add this little relationship, which is a coincidence relationship. And now this line and that line over there are black. The other ones are blue. And when a line is blue, it means it's undefined or under defined. So it knows something, but it doesn't know everything. Whereas black knows it's fully defined. Now let's go ahead and see if we can get all these lines to turn up black. So to define these a little further, let's go ahead and add a dimension. So come up here to smart dimension. I'm going to make a dimension from this side over to that side. And I'm going to place the dimension right here, type in six, and then same thing over here. I'm going to save this dimension here, this one dimension over here and type in three. Now, as soon as I add those two dimensions, notice this line and that line both turned black 'cause now they're fully defined. They know exactly how long they are. They know their relationship to the origin and so on. So everything is good. Now there's a couple of other colors for lines that we generally don't want to see. Those are yellow and those are red. And those means we got issues. So let's go see how we can create some issues and then see how we can resolve them. So right over here, this line here, clearly it is set up as vertical, but what if we said, Hey, you know, let's make it horizontal as well. So if I do that, it's all over says, Hey, what's going on here? Notice it says item conflicts or this item is unsolvable. So we're trying to tell this line to be both vertical and horizontal at the same time. Clearly it can't do that. So it's either saying you need to delete one of these yellow or red things so I can solve or something else you got to fix. In this case, if I deleted the horizontal, that would probably fix it. If I deleted the vertical, that probably wouldn't fix it because this line, if it tried to go to horizontal because a lot of other issues, but let's go ahead and try it anyways. So this one here, delete it. And now it's saying, Hey, wait, this line is red because I just can't solve what you've asked me to do. So let's go ahead and go back. So undo this time. Let's go ahead and delete the horizontal. Hit, deleting the keyboard, and then bam, it's back to being all black and everything is fully defined. So make sure every time you're creating a sketch, you create a sketch on a facer plane. You start that new sketch, draw some geometry out, tie that geometry into the origin. So it knows where it is and then add those relationships and dimensions. So everything is fully defined and black. And then finally, we're going to go ahead and create that feature. So come up here to features, I'm going to choose the extruded box or base, drag it up to whatever dimension you want. You can type that value in right over here. I'm going to type in three inches and then click on, Okay. And just that easily with those six steps, we've created our first solid here. Now, if you want to go ahead and create maybe a hole on this, we're going to do exactly the same thing. We're going to go up here and we're going to choose a sketch, choose a sketch. It's going to ask us, Hey, do you want to start a sketch either on a plane or face? Right? So step number one of the six steps is select a face for plane. Let's go ahead and choose this top one here. Notice we're now in a sketch environment, go ahead and drag out or draw a circle. There's my circle. And I'm going to spin my part around. So I'm looking at the top of it. So then I'm looking straight on it. Let's go ahead and tie that into the origin. So you can do that a couple of ways. One is I could say, Hey, I want to dip dimension from here over here to the origin, right? That's one way to do it. But if you wanted that in the center of this face, there's a lot better way to do that. So instead of choosing a regular line, I'm going to go ahead and choose a center line. I'm going to snap to the midpoint here and the mid point here. Now those two midpoints are defined because it's black and it knows where the midpoint of that line is. And so if I grabbed this circle here and I snap that to the mid point of that line, guess what happens, defines where it is. If I added dimension then of the size and say, maybe two inches notice everything's fully defined because you know, I said, we tie these into the, these lines, which are related back to the origin. And then the center of this is related to this and of that line. So everything's fully defined. That's what we need. We have everything fully defined and black. We tied it into the origin and now we're ready to create the feature. So come up here to features, go over here to extruded cut. Let's go ahead and cut a hole right through there and there you have it. So a couple different ways to create extruded features, extruded cuts. They're both using those six steps for pretty much all the features you'll ever see inside a SolidWorks.

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