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SOLIDWORKS is the world leader in 3D software for product development and design. Start creating manufacturing-ready parts and assemblies, as well as detailed drawings and bills of materials. In this course, author Gabriel Corbett shows how to create 2D sketches that will become the basis for your 3D models. You'll use the Extrude and Revolve tools to turn 2D sketches into 3D parts, then create more complex geometry with sweep and lofts. Then learn how to use the cut features to remove material and shape parts, and use mirroring, patterning, and scaling to modify parts. Next, you'll combine parts into movable assemblies and subassemblies. Finally, you'll create accurately annotated drawings, complete with itemized bills of materials that relate the final parts and assemblies to a manufacturer.
To use the sketch text command, there's a few different options and a couple tricks that I can show you. To get started, before I actually start a sketch using text, what I want to do is actually create a layout sketch prior. So what I have here is I've got a sketch on the top plane, or the top face of this part here, called sketch three. If I open that up and I take a look at it. I've actually defined three different lines. I have a line that spans all the way across the part, I have one that goes from top to bottom over here, which is still free-floating. And then what I also have is three lines connected together, all in a row.
So I'm defining a distance over here, and a distance over here. And you can think of those kind of like margins on a sheet of paper. I'm going to start my text and put it right in this section here, and I want to make sure it's starting about an inch and a half from this side, and about an inch from the other face. So I'm going to make sure it's right here in this center section. Go ahead and exit out of that sketch. And this time I'm going to start a brand new sketch on that top face. Click on Sketch and we're going to jump right into the sketch text command. Go ahead and click on Text and go ahead and type something out. In this case here I'm going to type in SolidWorks.
And notice, by default it just places that right in the center of your workspace or in the center of that sketch starting in the origin. But instead I could choose a curve that i'd like to define that alone. If I pick this line here, notice it automatically puts it over here on the left because I happen to be left justified or left aligned. I can click on the center point to put it right on the center or I could put it on the right as well. I can flip it upside down. I can flip it forward and backwards. Get a bunch of options for what I could do here. And in fact, if I want to flip it back to left justified. Flip it back left side up as well as going the right direction I could then if I want to move it around I can change the line its defined to so instead of this line here I can use this line here.
That starts at left-justified, starting on the line here, but I defined those margins ahead of time. So it makes it a great way to lay out words or text anywhere in your sheet or on that sketch. When you're happy with your sketch, click OK. If you're not quite happy and you want to change the font or the size, you can also come down here to Use Document Font. And turn that off, and then go and choose your own font. And you can use any of your standard fonts from your file system. But some of them work better than others, depending upon if you're going to be making parts out of these. Whether you're going to, maybe, cut them into the part or engrave them.
So keep that in mind when you actually create or choose a font. I'm going to choose this one, here, and I'm going to define the height of quarter of an inch, and go ahead and click OK. By the way, I can also choose points, if I wanted to. Click OK. You can see there's my text and before you create anything with the text, make sure that you are not overlapping anywhere. Sometimes you look in here really close and make sure there is no overlaps of the text and if there are you can always expand the words a little bit by changing the spacing between the letters. Like so or you can even shrink them down.
But if you shrink them down, notice you start getting overlaps which would cause errors. To make sure that you have no overlaps and that everything fits nicely on the line. When you're happy with that go ahead and click OK. And now I have text as a sketch in my design. From there I could always go to features and do like an extrude. Click OK. And you can see I've extruded that text directly out of my part and it looks pretty good. The other thing you could do is instead of an extrude and if it deleted that. I can come over here and do an extrude cut using that same sketch. And change it to maybe only 0.01.
Which is barely cutting into the material. And this would be great if you were going to do something like laser engraving or some kind of just engraving on to the material to show what it is. If you do the boss extrude out, that might be an example of maybe doing a paint or a logo or a graphic overlay of that nature. You can also change the color if you'd like, if you've done extrude cut into there, you can come up here and change the color of it. Maybe I'll make it red. Click OK. And that'll stick out. So it makes a couple nice way to see that. If you don't want to see those layout lines, you can always go back to that sketch here and hide the sketch.
I also want to point out that the text feature also works on curve surfaces. There is one more advance tools like rap that you can use, but really those aren't essential. And so we won't be covering those in this course, but I do want to point out that they are available.
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