Viewers: in countries Watching now:
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 process to create internal threads is the same as with creating external threads. However, there's a few subtle differences that I'll review. First, let's go ahead and open up 15.3-1, which is just a simple part with a hole in it. I've created a revolved cut to create the hole, and let's go ahead and take a look at that cut first, and look at the values. First, it's sketch 2. I'm going to go ahead and open that up, and there's my values I'm going to be looking at. I get a value here as my internal diameter of .393 which you are going to be getting from a look of value from the machinery handbook.
And I'm the edge here by a 100,000s with a 45 degree angle. So lets go find out where we get these values from. Go ahead and exit out of the sketch. Then I also have a sketch font defined here and let's close on edit sketch. GO ahead and take a look at that again. If I change over from display view from my regular shaded with edges over here to wire frame, you can see I've got a 60 degree triangle define, it's got a .031 pitch divided by 2 value, and you can see that I'm snapping on to this edge down here, as well I've got that value for the pitch diameter defined right up here.
So both of these values come from the machinery handbook. So I'm going to flip over there to the machinery handbook and show you the look up values. So I'm on this page here and you can see that I'm looking for the one in 16 thread, and from that table, we're not going to be looking at the external thread data this time, we're going to be looking at the internal thread data. So if you look at that 2B thread, you can see the major diameter of that 2B thread is going to be .932, 2.946 for the max and min, and my pitch diameter is going to be The 0.9594 to 0.9659.
Now we're going to take the average of both of these values. So the average for the diameter is going to be 0.939. And I'm going to take the pitch diameter average, which is going to be 0.963. Those are going to be my input values, when I get back over to SolidWorks. So, let's go ahead and do that now. Jump back over to SolidWorks. Use these values and input them into the sketch. So back in the sketch here, you can see those values here are input directly into our sketch, so our pitch diameter here is the 0.963, I'm going to type that directly in.
And same thing over here, is if you remember from the earlier movie of how we defined the size of a thread, this length of this line here is pitch divided by 2. Because we have 16 threads per inch, which is 1 divided by 16, which is 0.0625. And then we again divide that by 2 to get the length of this line, and that's what that input value is right now. Then again, we're just snapping it to the inside of the hole, and we're snapping it to the end of that part. Exit out of that sketch. And let's go ahead and flip back over to shaded with edges, you can see our part.
Now what we need is the helix to define the sweep path for that little triangle. So' m going to choose the top surface, I'm going to start a sketch, and I'm going to start a circle here, right at the origin, drag it out. And let's go ahead and click on the space bar. And I'm going to make that circle the same size as the inside of the hole. So I'm going to hold down Control, choose them both, and I'm going to say, make co-radial. Go ahead and click OK. And then I can jump up here to Insert Curve, helix, and it automatically because I've already pre-selected that circle, I get the shape, and you can see that I've got it extending kind of past the end of the part, and that's totally fine.
You don't need to have it extend past the part, but you could if you wanted. So in this case here, I can type in 1 inch, would be inside of the part. So, as long as we're extending a little bit past, I'll say 1.25. Which will be then at least going through the part, and I can define the length of this many ways. I can do height and pitch, I can say pitch and revolution, it really depends on how you want to input those values. But one thing for sure, is we want to make sure we have the correct pitch of our thread, so you can see, I have the right value already in here. But I can also use this input bar to do the math for me. So I can say 1 divided by 16 and notice that as soon as I click in a different box, it automatically does the math and gives you that pitch of .0625.
Now if I was going the wrong direction, I could always flip this direction here to go the other way. Or I have it going facing down right where we need it. Okay, looking pretty good. We're coming through the part, we've got the correct pitch, we've got the correct distance. Click on OK and there's our helix. Next, let's jump into the Swept Cut. So in Swept Cut, let's go ahead and, as far as our profile I'm going to choose from the tree over here, not from the window. So if I expand out the tree, I can come down here to sketch 4 and choose that as my profile.
And for my path, I'm going to choose the helix, and as soon as I do so, you can see I get a nice highlight of what's going to happen in my part, and click OK. There it is. There's our cut. Perfectly cut into here. And this is now ready to send out to a 3D printer, that you can actually take this part, take a real bolt, and thread it directly in there, and it should work just fine. One thing I do want to point out, if you are going to send these parts our for 3D printing, notice we took the average of the max and min for both of those threads. Sometimes, threads produced on a 3D printer will be out of speck.
And generally will be a little bit large. So I would recommend for an internal hole like this, I would go to the max size you can on those variables for your input values. Don't do the averages, do the max value. And same thing within External thread, and we want to go to the min value. So you have a max and min values, so you get the highest chances of the 2 parts fitting together smoothly, and having a nice fit. Otherwise, many times I've had to tap a hole or try to do external cut because 2 parts didn't fit together perfectly, because when you actually send it out to the 3D printer, the actual model built a little bit big, and it causes some issues.
So in general, try to play it safe and hedge your bet and actually, in this case here, we would maximize both the pitch diameter as well as the hole size. To make sure that both parts will fit together smoothly. Threading is used extensively in product design, and having these basic skills is essential. The threads we created in this movie are standard 60 degree threads. However, the same techniques can be used for ACME, ball screw, or any other types of threads you'd like to create.
There are currently no FAQs about SolidWorks 2014 Essential Training.
Access exercise files from a button right under the course name.
Search within course videos and transcripts, and jump right to the results.
Remove icons showing you already watched videos if you want to start over.
Make the video wide, narrow, full-screen, or pop the player out of the page into its own window.
Click on text in the transcript to jump to that spot in the video. As the video plays, the relevant spot in the transcript will be highlighted.