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Cutting holes and grooves with the Swept Cut tool

From: SolidWorks 2014 Essential Training

Video: Cutting holes and grooves with the Swept Cut tool

Swept cuts allow for a tool or profile to be used to cut along a path.

Cutting holes and grooves with the Swept Cut tool

Swept cuts allow for a tool or profile to be used to cut along a path. The creation is almost the same as using a regular sweep, with the addition of something to cut through. I've got three different example here I'm going to go through. The first one is I'm going to have a little cut or tube that actually go through the inside of this part. So what I'm going to do is I'm going to first start off with the path that I want to go through. So I want actually this hole to be on the mid-section of this part, so somewhere between the top and the bottom of the part. In this case here, I can look at the planes I have available, the front plane, the top plane, and the right plane, and none of them really seem to be in the right location.

So let's go ahead and create our own plane. Come up here to Reference Geometry, choose Plane, and I'm going to choose the top surface. And I'll rotate my model around and choose the bottom surface. And by doing that, it places a plane between those two faces. Click OK. And that's what I want to draw on. So I'll go ahead and choose that plane, start a sketch, and press the space bar to look at Normal Two. Then, come up here. And, let's use the Line command. Let's just start, right here, at the bottom edge. Come up. Come over. And come down. I know that I want to add a Fill It to those corners.

So, I'm going to choose the Fill It command. Click on the corner here. Click on the corner there. And, 3/4 inch looks good. Click OK. And, then, I want to make sure I'm centered up. So I'm going to choose the origin. And I'm going to snap to the mid-point. And notice as I go over that line, a little mid-point dot shows up. Click on that and then say, hey this line here, I want to make that vertical. Let's go ahead and add a couple of dimensions from here to here. Let's make it five inches. And from the top to the bottom of the part, let's click and place the dimension, making it 9.0. That is going to be our path. Go ahead and exit out of that sketch.

Now, I'm going to come down here to this face at the bottom of the part. Start a sketch. And what I want to do is choose the circle command. And I'm going to start right in 3-D here, choose that endpoint and I'm going to draw a circle. Jump over to the smart dimension Add a dimension of half inch. And then exit the sketch. So now I have everything I need to create that swept cut. I have the path and I have the profile. And I'm ready to go. So go ahead and jump up to Features. Come over here to Swept Cut. And as far as my profile, I'm going to do a Profile Sweep, and I'm going to choose my profile.

And go ahead and choose it from the tree. I'm going to expand that out. And I'm going to choose sketch nine. And for the path, I'm going to choose sketch eight. There's my two cuts. Click OK. And there it is. It cuts right through the part. And it's a little hard to see, because it's inside, but what you can do is, you can come up here to the section view. Section it in half. Click OK. You can see how that path is cut all the way through the part. And it just takes basically that simple little circle and drives that circle as a cutter all the way through the part following along that path. Click OK, bring it back. Alright, that's example one.

Example two is we're going to take this profile here and we're going to drive that profile all around the outside edge of this part to create a nice, decorative finish. To do that let's go up to Swept Cut. As far as the profile, I'm going to come up here and choose sketch two. As far as the path, I'm going to choose sketch three. And it's just going to take that and just drag it around the outside of the part. Click OK, and there it is. We've created a pretty complicated part now with pretty much a simple sketch and a simple path. But it looks pretty neat. In the final example, what I'm going to do is what's called a Solid Sweep.

So in this case here, I've what I've determined is a end mill, and that N mill is going to be plunging into this part at an angle. This type of cut would be extremely difficult to model otherwise if you weren't using a Solid Sweep. And I'll show you why. First off, come up to Solid Sweep. And this time I'm going to go to Solid Sweep option. And it gives you some heads-up information here as far as what you want to choose for using a Solid Sweep. And what I did was I actually created a separate revolve feature here which I modeled in end mill. I'm going to use that end mill now to cut into the part. So as far as my profile or my tool body, I'm going to choose this end mill.

Which just happens to be a simple rectangle that I rotated around the central axis. And then as far as the path, I'm going to come down here to choose sketch five. Click OK. And you can see what happens. When it cuts down there, it takes that shape and drives it into the part. And if you look at this, if you actually can see a little of a rounding of the backside of where the end mill was. And you can see when it's down to the bottom, it has this nice round circle, exactly what it would be if you did take an end mill and run that part into there. Otherwise, besides using the swept feature, this would be extremely difficult to create that exact shape.

It can be very hand when you're working with machine parts to get an accurate representation of what's going to happen when the end mill cuts into a part or you have different features you're going to be working with. The Swept Cut command can be very useful. It's great for creating special features. The concept is the same as with creating Sweeps. We need to create a profile and a path. The two sketches cannot be on the same plane, and they need to have an orientation that allows the shape to be built.

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This video is part of

Image for SolidWorks 2014 Essential Training
SolidWorks 2014 Essential Training

97 video lessons · 7289 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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