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Linking to layout sketches

From: SolidWorks 2014 Essential Training

Video: Linking to layout sketches

Much like linking to other parts in SolidWorks, we can

Linking to layout sketches

Much like linking to other parts in SolidWorks, we can have a layout sketch that drives a series of parts. SolidWorks has a built in layout function, or we can use standard sketches to lay out designs. To start using layouts, we need to create a layout in an assembly mode of SolidWorks. If you open up 14.2 Assembly, you can go ahead and see that I've actually created a layout sketch first, and I have one part already pre defined and designed off that layout. Now what I want to do is actually want to built out a secondary little frame bracket, it's going to build off that as well. Before we do that, let's go ahead and take a look at what the layout sketch has inside of it.

Notice I have a layout because I have this little four bar mechanism up here, this little wooden frame looking thing, that tells me I do have a layout derived in this assembly. So right-click on that Assembly. Come down here to Layout and take a look. You can see, if I click on the space bar and looking normal to it. That I've got a 24 inch circle to find. I've got a couple dimensions here, and I basically just have some lines defining that octagonal shape. That's all I really need to define this whole shape here. Go ahead and exit out of the layout sketch, come back to the assembly, and you can see I already have one part already defined from this.

So I have a sketch that's linked. And by the way, if you ever see these little arrows at the end, that means there's some kind of reference outside to some other part or some other sketch. So go ahead go to the Sketch. You can see I basically just got a few different lines. And then we off set these lines a little bit. And pretty basic, right. And that's all based upon those, there's no dimensions here. We're just referencing or converting the entities from that layout sketch to define that shape. The only dimension I do have is this quarter inch here, it's defining the thickness of that plate. Okay, go ahead and exit out.

And then come back to the assembly. Now, I want to put a new part in this assembly, so I have a couple of ways I can do that. One, I can go out and click on you know, New > Create a New Part, drag that part into the assembly. And it can be a blank part, there can be nothing in the part, that's totally fine. But the problem is that you make sure that you mate that part up. So, one way you can do that is you can mate the origin of the new part to the origin of the assembly, that brings it all together. That's a great way to do it. Or the other way you can do it is basically go over to insert components click on New part. What that will do is actually create a virtual component or virtual part within your assembly.

And make sure first before you do that though, you have actually a part name here. So 14.2.assembly. Make sure you save the assembly first so it's not just a new document when you open it up, because this part here will be created based upon that name. I can, if I want to save out this part here right-click on it and click on Save Part in External file, and I definitely recommend doing that sooner than later. Click on that, notice it's called Part2, and whatever path it's going to be stored in. In this case here, we're storing it in the Desktop.

So, I want to overwrite that path. So I'm going to go ahead and call it 14.2- 2 because I already have a -1. And make sure you're overriding that. And then click on, OK. And now I've saved that part out to the file system and it can be used and opened just like a regular part. But right now, that part is blank. So, let's go ahead and create something in it. So first things first, click on the part and make sure we're editing the part. I want to go and look at which plane to start drawing on. And it looks like the front plane is the one that I want. Go ahead and click on Sketch, start a sketch on that plane.

And we'll go ahead and choose the line command, but before we do that, let's first go ahead and convert a couple of these. We've already got lines behind the scenes in that layout sketch. Why not just use those? So click on this first line here, hold down Ctrl, pick on the second line here and convert those over. So convert entities brings them directly into the sketch here which is great. And we could do the same thing over here except those lines would extend too far so, I'm going to use the regular line command here. Snap to the end point and instead of going to the end let's just snap right here to this intersection of the inside of that plate and then come all the way down here.

So we enclose that shape. And just so you know, you see that little blue dot there I accidentally just double clicked too quick and it created another little line segment? Just delete that if It's a real common error to quickly double-click and it creates a smaller line segment and that'll screw up your drawings. So make sure that all of your points are clean points. And don't have any type of little artefacts like that. Anyways notice I'm snapping to the inside here so if this plate were to get thicker later on it would automatically update and be fine. I'm converting some entities here. All of this is based upon that layout sketch so there's no dimensions.

So, anything that's going to change in the layout sketch is automatically going to adjust in the sketch as well. Okay. When we're ready to create a feature, go over here to Features, Base Extrude. Type in a half of an inch, click OK, and there's our little bracket, okay. When you're ready get back over to the assembly. So exit out of this part. We're back in the assembly mode now. And what I want to do is I want to pattern these parts around. So I already have a pattern predefined, so I'm going to take this history bar, I'm going to roll it forward. And you can see I've already patterned this part here just by choosing the center align as my axis of rotation, and patterning that part around.

I created the axis just by grabbing the top plane and the right plane, coming up to reference geometry, and creating axis. Pretty quick. Okay? Now what we want to do is, edit that circular pattern. So come up here to Edit feature. And, go ahead and choose, notice I already have the 14.2 in there -1, and I want to add the 14.2- 2, so I'll just go ahead and click on that second item. It's going to add it to the pattern, click, Ok, and now you can see we got both those in the same pattern, looking pretty good.

Now let's go ahead and go back to the layout sketch and change the sketch and make sure that all the components are going to automatically change and move. So, right-click, Layout, and this case here, let's change it to 36. The layout sketch is going to change. Go ahead and exit out of the sketch. And notice that all the components automatically update. They change size based upon the layout sketch. And then the pattern automatically updates as well. I can also go ahead and choose a component maybe like this first one here, one.

And let's just play around, and say maybe instead of this being a quarter inch, what if we change it to a one inch. It gets a lot bigger. Update the sketch and notice that this component here also automatically updates. If I go back to that, exit out of that part, the secondary part, because we based upon the inside there, you can see there's a nice line. Defining where that is, because those automatically update based on the thickness of that material. If I want to go back, I can always go back here, edit the sketch back to the quarter inch. And notice again, it automatically updates based upon that.

It's all in-context modeling. It's a really great way to design things, because if you change one thing like a layout sketch, all the other components will automatically update. It's a very powerful way to work in SolidWorks. Layouts can be very helpful, and give the ability to derive a large amount of parts from the same layout sketch. It also creates a clear order of what's driving what, all by changing just one sketch.

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This video is part of

Image for SolidWorks 2014 Essential Training
SolidWorks 2014 Essential Training

97 video lessons · 6272 viewers

Gabriel Corbett

Expand all | Collapse all
  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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