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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.
The next step in the thread creation process, is to generate a helix that will guide the Cut tool. To do this, we need to draw a circle that will be the same size as the helix. Let's get it in a Helix Creation tool and get started. We're starting off with the same sketch we were in the last movie. This is the sketch we're going to be cutting through the path of the Helix. So let's go ahead and exit out of the sketch. And you can see, there's our sketch there. And I'm going to go ahead and show it, and make sure we have a view and we have sketches turned on so we can see that sketch in the model.
Now I want to create a Helix on top of that. So I'm going to click on the very top of this part here. This is where I want to create my circle that will define the size of the Helix. And come up to Insert, Curve, Helix. And by default it puts you in a Drawing mode, right when you click on that top surface, and what I want to do is draw out a circle. SolidWorks doesn't really explain this very well in their Cmds. So, you have to just draw out a circle, the same size as your part is, and in this case here, I'm just going to make the outside surface here and my circle the same size.
So, I'm going to say coradial, so I don't need to add a dimension at all. And then when I, soon as I exit out of that sketch. It automatically puts me into the Helix Cmd. So that's a little bit undefined in their tool. Sometimes, its actually easy to draw this circle first and then jump into the Helix Cmd. But basically you are going to choose a surface to draw a circle on. Start the Helix Cmd and then draw it out. Now, over here we have constant pitch or variable pitch and what we want to use a constant pitch. And we can also define how we'd like to draw that Helix. Pitch and revolution, or height and revolution, or height and pitch.
So we're going to use height and pitch in this case here. For my height, I'm going to type in 1.0, for one inch, and my pitch, remember, is going to be 1 divided by 16. And my starting angle will be, the same location as where, my sketch is. An notice over here, you can see I'm starting right there. So in this case here it's 270 degrees, clockwise. But notice, this whole thing is going in the wrong direction. And so let's go ahead and reverse the direction. And you can see, oh, actually, we're not going quite far enough.
So I want to, maybe type in two inches. And two inches are going to bring me all the way past, and actually going to be cutting into this next section here. So this is a point you might want to finesse it a little bit. And adjust that height of it a little bit so you get full threads but the thread actually ends in this little thread relief here. So in this case maybe I'll type in 1.95. And see how that looks. You always click in the box next to it and see how it's going to look. So you can see the endpoint here. If you spin it around a little bit, there it is. And that looks just about perfect. It's going to end right in the middle of that thread relief.
So we're pretty good to go. And you might need to adjust that a little bit depending on how you create the thread. When you're happy with that, go ahead and click on OK. And now what we have is a profile and a path. The profile is going to be that triangle we created in sketch three, and the path is going to be the Helix. And that's all we need to create a Swept Cut. So let's go up to Features. Let's go over here to Swept Cut. We're going to do a profile sweep. And first choice is going to be what is the profile. So let's expand out the tree, let's come down here and my profile is going to be sketch three, okay? My path is going to be the Helix.
And as soon as I choose those two, it gives us a preview of what's going to happen. Notice, if you zoom in over here, you can see that my last part of the Swept Cut is going to clear that thread relief and it's not going to cut into the back part of the bolt, so we should be good to go. Go ahead and click on OK. And there it is. We've cut those threads on the outside. And these are real threads. If I 3-D print this part, it's going to generate these real threads. I can thread this together with another piece, and it should work. The Sweep tool can be used to make a variety of shapes, and the thread profile is just one of them. The key point to remember in creating threads is that the process will be exactly the same every time you create a thread.
But make sure you're using real values from a look-up table from maybe the machinery handbook or some other source. To get those values as the inputs for both the profile and the path values. Also make sure to specify the correct thread and class on your drawing.
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