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Working with the Revolved Cut tool

From: SolidWorks 2014 Essential Training

Video: Working with the Revolved Cut tool

Creating a revolved cut is exactly the same as creating a basic revolve. And notice down here, we have this thing called selective contours.

Working with the Revolved Cut tool

Creating a revolved cut is exactly the same as creating a basic revolve. However this time, we need something to cut, and the features act a little bit differently. This command also builds on plane creation and sketching skills, so make sure you're up to speed if you're working with complex cuts. In this case here, what I have is a extruded Hexagon and I've got a sketch, Sketch2 here laid out already. Let's go ahead and open that up and take a look. So one of the requirements for a revolved cut is an enclosed boundary. Notice I have a sketched layout here with just the line tools.

So I have a line tool going here all the way around this outside perimeter and goes back and closes itself off. So just to give you an example, let's go ahead and just try out some of these sketching skills. Let's go up here to the line command. I'm going to start right on this upper corner and draw a line over here, draw a line back over here, down to here. I'm just kind of snapping to those corners, down and back over, and then I'm going to drive it all the way back up and close that sketch. So I have one enclosed boundary, all just using the simple line tool. Now what I want to do is add a few of the relationships.

Notice there's a few relationships already added like this on here, perpendicular, so I can define one of those angles, and the other one will automatically update. To do that, let's go up to Sketch Dimension. Come over here and click on this first line, click on this second line. And type in the dimension which is already at 45 which is great, click OK, and then I want to define this length here. So if I hit escape to get out of the dimensioning tool, I can see I can drag this up and down, move it around, and what I want to do is add a dimension. So in this case, I'm using what is called a double dimension.

So I can dimension from this line to the center line of the part. And notice as soon as I put the value in, it gives me a radius value from that line to the center line of the part. And notice as soon as I move past that center line it actually doubles, then turns into a diameter value versus a radius value. So sometimes that's really if you're working with diameters and not radius' to be able to type in the full diameter versus the radius. So it's really dependent upon whether you're on the left hand side, or the right hand side of that center line. I like to kind of use these double dimension values because it makes it easy to type in the values as their full diameters.

Go ahead and click OK, and let's type in 2.2 for instance. These are obviously not the right values. I'm just giving an example of the size. The correct values are right up here. Now, a couple of other things we might want to add. Maybe another dimension here between these 2. So click on the first one. Over here to the second one, and type in the value. And notice as I put these values around, it changes. So inside of here, I've got this 52. If I move out here, it changes the way the value is inputted. Same thing over here. Same thing over here. So make sure you're placing the value where you'd like.

For instance right here, it may be 45. And then once you have the value placed, you can always move it out. And out of the way differently, as long as you're placing it correctly the first time. Once everything looks good, we can probably add a few other dimensions, but I'll skip that for right now. I'm going to go ahead and actually just delete these values and sketches, so we're ready to actually revolve the original sketch that I had. Let's go back to Features, let's go to Revolved Cut Choose our axis of rotation which is going to be that center line, and by default it's using a blind rotation of 360 degrees.

Go ahead and click on OK, and you can see what happens. It just trims out that material off the part. Now let's go back and take a look. Go back to Revolve Cut 1. Click on Edit Feature. And you can see that I've got a couple of other options here I can play with. So instead of Blind, I could use maybe Up to Vertex. In that case here, it's taking this sketch, and it's going to revolve it around till it sees a certain point. And if I choose a point like this one, notice it revolves around and cuts up to that point. Pretty handy. Click OK. You can see what happens. And go back again.

Modify that feature again. This time I'm going to come down to up to surface. The problem with up to surface is that it needs a surface to completely end that feature. In this case, we don't have one of those surfaces, so it's not going to work. But if you did have a surface that was extending maybe from the center line of the part out to one of these points, you could use that to end that revolve. Offset from surface, exactly the same thing if you had a surface you could offset from it. But its not really going to work on this example, but I did want to point it out. And finally mid-plane. Mid-plane allows you to go both directions with whatever angle that you want so in this case here maybe I'll type in 90 degrees.

And you can see that it's going 45 this way and 45 this way to make a 90 degree cut. And I can click the up arrows or down arrows to continue that on, and it goes both directions with that cut. So, pretty handy. When you're done, click OK. And you can see what we have. Again, go back to the feature. And I'm going to go back to the original blind cut. At 360 degrees. And notice down here, we have this thing called selective contours. Selective contours allows us to choose multiple items to revolve. In this case here, I only have one enclosed boundary, so it's really not going to make that active.

So I want to go back and actually show how that works. So click OK, and let's go back and delete that feature altogether. So click on Cut Revolve 1. Press delete on your keyboard to delete the feature, click Yes. Notice if I delete the feature, the sketch is still there. So this time I'm going to go back to that sketch, edit the sketch, and I'm going to add a few other items to the sketch. Number 1, I'm just going to add a rectangle directly below this. And I'm going to not add any dimensions right now cause I'm just going to use this as an example. Now, go up to Features, jump up to Revolved Cut, and choose my axis for rotation, which is this.

And by default, notice it revolves both of those shapes. Click OK. And there's an example of how it's going to look. But if I go back to Revolved Cut, I can actually go down to Selected Contours and I can choose Maybe just one of these contours that I want to revolve. So even though I have 2 shapes in that sketch, I can only choose to revolve maybe just one of them. Or go back to the feature again, this time here I'm going to choose the second one, and I'm going to get rid of that first one by hitting Delete on my keyboard, and click OK. And you can see it only does one of those cuts, or you have the option to go back and choose both of them.

So go back into this box Choose this other contour, click OK, and you can remove both of those shapes with one Revolve Cut. Revolve features can do a lot with only very simple input. The basics are, choose or build a sketch, choose an axis of rotation, and then select the degrees of rotation and just simply click OK.

Show transcript

This video is part of

Image for SolidWorks 2014 Essential Training
SolidWorks 2014 Essential Training

97 video lessons · 8200 viewers

Gabriel Corbett
Author

 
Expand all | Collapse all
  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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