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Understanding internal threads

From: SolidWorks 2014 Essential Training

Video: Understanding internal threads

The process to create internal threads is

Understanding internal threads

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.

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This video is part of

Image for SolidWorks 2014 Essential Training
SolidWorks 2014 Essential Training

97 video lessons · 8147 viewers

Gabriel Corbett
Author

 
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  1. 1m 51s
    1. Welcome
      1m 7s
    2. Using the exercise files
      44s
  2. 31m 13s
    1. Launching SolidWorks for the first time
      3m 55s
    2. Accessing and customizing the Ribbon
      4m 14s
    3. Touring the shortcut bar and identifying essential keys
      7m 27s
    4. Saving, renaming, and managing files
      10m 28s
    5. Working with the new view cube, or View Selector
      2m 36s
    6. New features in SolidWorks 2013 and 2014
      2m 33s
  3. 14m 11s
    1. Understanding the 3D world
      2m 31s
    2. Creating your first part
      3m 15s
    3. The virtual, parametric prototyping environment
      1m 56s
    4. The FeatureManager and feature-based modeling
      3m 43s
    5. History-based modeling and the rollback bar
      2m 46s
  4. 28m 32s
    1. Starting a new sketch
      6m 50s
    2. The six steps used in almost all modeling features
      52s
    3. The Line and Centerline tools
      3m 25s
    4. Using the Circle tool
      1m 51s
    5. Adding and removing relationships and dimensions
      6m 56s
    6. Understanding relationship types
      3m 58s
    7. System options, units, and templates
      4m 40s
  5. 18m 28s
    1. Drawing rectangles
      5m 31s
    2. Creating arcs in a sketch
      4m 8s
    3. Drawing splines in a sketch
      4m 57s
    4. Sketching polygons
      3m 52s
  6. 36m 5s
    1. Trimming and extending portions of a sketch
      3m 54s
    2. Creating offset geometry
      3m 13s
    3. Moving, copying, rotating, and scaling elements
      3m 13s
    4. Erasing, undoing, and redoing actions
      2m 24s
    5. Using the mirror tools
      2m 24s
    6. Creating repeating patterns in a sketch
      4m 55s
    7. Using construction lines to build robust sketches
      3m 25s
    8. Applying fillets and chamfers to a sketch
      2m 32s
    9. Working with slots
      3m 46s
    10. Adding text to parts
      4m 1s
    11. Using the Convert Entities command
      2m 18s
  7. 9m 33s
    1. Working with planes
      5m 28s
    2. Placing and using axes
      2m 22s
    3. Placing a coordinate system
      1m 43s
  8. 17m 50s
    1. Extruding a sketch into a 3D object
      4m 36s
    2. Using Revolve to create 3D parts
      2m 42s
    3. Using Loft to create complex shapes
      4m 40s
    4. Refining a loft shape with guide curves
      2m 22s
    5. Using the sweep to create wire and pipe shapes
      3m 30s
  9. 20m 23s
    1. Modifying parts using the Extruded Cut tool
      5m 42s
    2. Working with the Revolved Cut tool
      6m 19s
    3. Using the Lofted Cut tool
      3m 32s
    4. Cutting holes and grooves with the Swept Cut tool
      4m 50s
  10. 21m 5s
    1. Using fillets and chamfers to smooth corners
      5m 58s
    2. Creating repeating rectangular patterns
      3m 16s
    3. Creating a circular pattern
      2m 27s
    4. Mirroring objects
      4m 0s
    5. Using the Shell and Draft tools
      3m 52s
    6. Scaling parts
      1m 32s
  11. 9m 39s
    1. Working with reusable sketches and blocks
      2m 47s
    2. Creating blocks
      3m 51s
    3. Designing with blocks
      3m 1s
  12. 29m 45s
    1. Understanding the tools for beginning a new assembly
      4m 46s
    2. The basic steps in creating an assembly
      3m 18s
    3. Mating parts together in an assembly
      6m 43s
    4. Working with subassemblies
      2m 9s
    5. Linear and circular assembly patterns
      4m 56s
    6. Downloading premade parts from the Internet
      3m 32s
    7. Using Toolbox
      4m 21s
  13. 15m 8s
    1. Mating parts with coincident, parallel, and distance mates
      4m 35s
    2. Mating parts with width mates
      5m 53s
    3. Mating parts with path mates
      2m 5s
    4. Mating parts by aligning planes
      2m 35s
  14. 10m 20s
    1. Getting started with the Hole Wizard
      4m 38s
    2. Positioning holes in layout sketches
      5m 42s
  15. 15m 27s
    1. Linking sketches to other parts
      4m 28s
    2. Linking to layout sketches
      6m 48s
    3. Using the Hole Wizard in context
      4m 11s
  16. 17m 15s
    1. Understanding threading concepts
      7m 17s
    2. Using a helix and Swept Path to create a thread
      4m 2s
    3. Understanding internal threads
      5m 56s
  17. 17m 25s
    1. Using equations to drive a sketch
      5m 5s
    2. Working with complex calculations
      2m 6s
    3. Integrating Microsoft Excel to manage design tables
      7m 10s
    4. Building assemblies using part configurations
      3m 4s
  18. 23m 17s
    1. Working with drawing templates
      6m 49s
    2. Setting up drawing options and sheet properties
      3m 43s
    3. Choosing the correct projection angle
      2m 21s
    4. Adding model views to a drawing
      10m 24s
  19. 16m 8s
    1. Creating general dimension notations
      6m 37s
    2. Creating ordinate and running dimensions
      3m 0s
    3. Dimensioning holes and curved features
      3m 8s
    4. Using the autodimension tools
      3m 23s
  20. 14m 38s
    1. Creating holes and callouts
      5m 8s
    2. Adding center marks and centerlines to a drawing
      3m 46s
    3. Adding item notes
      2m 57s
    4. Making drawing revisions
      2m 47s
  21. 11m 42s
    1. Adding assemblies to drawings
      2m 10s
    2. Including a bill of materials
      1m 42s
    3. Adding balloons to specify parts on an assembly drawing
      1m 39s
    4. Adding a title block and sheet properties
      2m 8s
    5. Building an exploded view for an assembly drawing
      4m 3s
  22. 1m 2s
    1. Next steps
      1m 2s

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