SOLIDWORKS 2014 Essential Training
Illustration by Richard Downs

Understanding threading concepts


SOLIDWORKS 2014 Essential Training

with Gabriel Corbett

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Video: Understanding threading concepts

SolidWorks has several ways to represent threads, including the hole wizard and cosmetic thread. However, if you need to create true threads, we need to do a swept cut and actually cut the threads. This can be time consuming and adds a complex feature to your model. As with all sweeps, we need a profile and a path. The profile is just a 60 degree triangle, and the path is a helix. Now for the hard part. We need to input the correct values into the helix in the profile sketch to get the correct thread when finished. Let's take a look. Over here in solid works I've got a bolt and the bolt is going to be a one inch, and sixteen thread.
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  1. 1m 51s
    1. Welcome
      1m 7s
    2. Using the exercise files
  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
    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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Watch the Online Video Course SOLIDWORKS 2014 Essential Training
6h 20m Beginner Dec 09, 2013

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.

Topics include:
  • Creating your first part
  • Starting a new sketch
  • Adding and removing relationships and dimensions
  • Sketching polygons
  • Creating offset geometry
  • Moving, copying, and rotating elements
  • Working with planes, axes, and the coordinate system
  • Using Revolve and Loft to create 3D objects
  • Trimming with the Revolve, Loft, and Sweep cuts
  • Creating smooth and angled corners with fillets and chamfers
  • Designing with sketch blocks
  • Working with subassemblies
  • Creating threaded parts
  • Integrating Excel to manage design tables
  • Adding dimension notations to a drawing
  • Rendering an image of a part or assembly
Gabriel Corbett

Understanding threading concepts

SolidWorks has several ways to represent threads, including the hole wizard and cosmetic thread. However, if you need to create true threads, we need to do a swept cut and actually cut the threads. This can be time consuming and adds a complex feature to your model. As with all sweeps, we need a profile and a path. The profile is just a 60 degree triangle, and the path is a helix. Now for the hard part. We need to input the correct values into the helix in the profile sketch to get the correct thread when finished. Let's take a look. Over here in solid works I've got a bolt and the bolt is going to be a one inch, and sixteen thread.

The outside diameter or nominal diameter is one inch, and what I want to do is I want to create a little triangle to sweep and cut around the outside of that to create the sixteen thread. So let's take a look at the sketch first. So over here is the sketch three. I'm going to go ahead and open that up and take a look. And click on the Space bar so, I'm looking straight at it. I'm going to zoom in here. I can see I have a 60 degree triangle here and you can see I've got a distance here of 0.031. I've got a little radius here at the corner of 0.003, and you can see I have a value here of 0.955, which is the pitch diameter of that thread.

And you're saying, well where do these values come from? And the answer is, I look them up in the machinery handbook, or you could look it up online. So, I'm going to point you first off in the direction of where do we get these values from. So the book I'm going to be referencing is call the Machinery's Handbook and I'm using the 26th version in this course. However, there's newer versions available. In fact, you can go to the website. Industrial Press has been producing this book for over 100 years, and there's a bunch of different versions of the same book. There's a small one that fits in your toolbox, or you can get the larger, large print edition, or you can even get a CD-ROM version.

My suggestion is to get the CD-ROM version of the book, that way you can download it, put it on your computer or your flash drive. Anytime you need the values, you open the PDF document, look at the values, you can even print them out if you need to. That's a really handy way to not have to carry this huge book around with you any time you're working on a design. You can also buy it from, notice they have the full book version here. If you scroll down a little bit you can also get the CD-ROM version. So either one is a great way to go. You can always look up the values depending on your preferences. Now looking at the threading profile in the machinery's handbook.

You can see we're going to be using this profile here to define our sketch inside of SolidWorks. So, all we really need is a triangle to define this. So, the value of the triangle's going to be this section here. We're going to have a pitch line here, which is actually one half the pitch. So the pitch of the thread you notice is going to be 1 in 16 so 16 threads per inch and we're going to divide that in 2 to get this length of this value here. And you could see we've got the basic pitch diameter here and those are the values that we're going to look up from the table now let's jump over to the table.

In this example, we're going to be using the one in sixteen thread. We're going to be using the two way external thread. And, you can see from the table, we're going to be looking, first up the major diameter of the thread. That's going to be the outside section, that we're going to model in SolidWorks. In this case, here, there's both a max and min diameter. We're going to take the average of the two values. So, in this case I see I have a 0.9985 on the max and a 0.9891 on the minimum. If I take the two of those and I average them together I get a 0.9938. If I jump over to the pitch diameter column you can see my pitch diameter is 0.9579 on the max and 0.9529 on the min.

Again, let's average those together and get a 0.9554 value. We're going to be using those values as our input values inside of Solidworks. Now that we have these values, I want to also point out how they're used. The thread pitch in this case is a 1 inch, 16, or a 1 inch with 16 threads per inch. So therefore, the thread pitch is equal to 1 divided by TPI or one divided by 16 that's 0.0625. So pitch divided by 2 is 0.0625 divided by 2, which is at 0.03125. That's the value here.

0.5 pitch, we're going to be importing for, and the basic pitch diameter here is the value we looked up from the table. Let's go back to SolidWorks and put those values in. Okay, you can see here, which is that pitch line here. If I open it up, you can see it's the 0.03125 value. And if I come over here, I can see this value here, which is the pitch diameter, which is 0.9554, and that's the value that we got from the table. Now, before we move on, I want to point out how we actually draw this triangle here.

So I'm going to move these couple of values in. Move this stuff so we can see it a little easier to make sure we are doing exactly the same thing. Okay? I'm going to draw out here the same type of triangle. So first things first, I'm going to draw line. I'm going to start with a vertical line and then I'm going to draw out a triangle. Then I'll be perfect in fact it can be a little bit in the beginning, no big deal. Grab these center line tool. From the point of that we are going to draw a line to the mid-point of the vertical one. Then all I have to do is click on the line and say make horizontal to get an equilateral triangle.

Now I know it's going to be sixty degrees. So click on the first line. I'd say the other outside line and type in sixty degrees. And then what I need is this pitch line. So I'm going to go ahead and create a line between the two outside edges of the triangle. Notice, I don't want to snap to the midpoint on either sides. So I wantna make sure I'm going to be far away from the midpoint. Just create a line from the top, all the way down here to the bottom and make sure it's a vertical line. Make sure you've got that relationship here, showing it's a vertical. Then I should be able to drag this line back and forth along that triangle and verify it's not snapped to anyone of those midpoint lines.

Once you have that line, we need to determine the length of the line. So go ahead and click on Smart Dimension, click on the line itself, and let's go ahead and type in the value. Now remember, our pitch is 1 divided by 16 for 16 threads per inch, so I do that value here, I can say 1 divided by 16, then again, divide that by 2. If I do all that, click, OK. It should give me that 0.03125. What I did there, was I actually used the input bar as a calculator. If we open it up again, it's very simple to do. You just type in 0.0625, divided by 2.

And as soon as you click anywhere else, it puts that value. And does the math for you. So it's really handy way to use the input project should do some math for you. Once we have this here we can grab this triangle, and drag it over here. We can resize it, put it where we need it. And what I normally do is connect it here to the end of the park as well as to the outside diameter of that threaded section to make sure we have it aligned in the perfect location. And then what we need to do also, is connect it to the pitch diameter. So, I'd come up here, to the diameter.

I'd go from the center line to one of these corners on the end point, type in the value, and notice it's a double diameter, so if I come here, it's only a single diameter. As soon as I move past the center line, notice the value doubles. So, if I click here, then I can type in that 0.9554. Click, OK, and that moves that new triangle right to where we need it. I can drag it up here for a second just to show the value is locked in. Now I still needed to find where the back of this thing is, and where it is up and down.

However, we can see this line here is fully defined in black because it knows what diameter we're using in this example. It takes a bit of work to create a real cut thread. So, I would not recommend this option in all situations. However, if you're going to rapid prototype your parts, and want threads included, or if you want them to visually look correct, then this is the option to choose.

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