Join Gabriel Corbett for an in-depth discussion in this video In-context features, part of Cert Prep: Certified SOLIDWORKS Professional (2015).
- In this video we're going to go ahead and start creating an assembly and then we're going to make in-context features to relate the two together. I'm going to start with this base piece here, and I'm going to right-click on it, and then click on "Make Assembly from Part." I'm going to use the the Lynda Assembly and go ahead and start that up. Choose that part right there and click "OK." Now I have Assembly set up here, I'm going to click on "Tile Horizontally" and I'm going to drag this part here into my assembly. Once I have that, I'm going to go ahead and open it up.
I'm going to basically just put this piece directly over the other piece and then create an assembly. So click on "Mate." I'm going to choose the outside of the circle here with the outside of that one there. Click "OK" and then we're going to click on the top surface here and the bottom surface there, and bring those together. Now what I want is this circle here, or this cylinder here, to be the same size as this cylinder down here. Then I want to have some counter sunk, or counter board, holes in here that relate to where these holes are here.
So to do that, I need to create an in-context feature. Click on this part here, and come up here to "Edit Part." It's going to ask you to save the assembly. Let's go ahead and call this 2.25 and then click on "Save." So here's a new assembly and I'm editing this part inside of that assembly. Click on the drop-down here, and click on the "Boss-Extrude 1," and the shape itself. Click on that sketch, and you can see it's an undefined blue sketch.
So what I want to do is, instead of adding a dimension like I would normally, I want to relate this size to the size of the cylinder directly below it. I can just click on this cylinder here, hold down "CTRL", select the second circle. I can then click on "Coradial" to make those exactly the same size. Once I'm done with that, exit out of the sketch. and you can see my part automatically adjusted in size to the other part. Any changes to this part down here will automatically relate to this part on top of it.
Let's go back to the assembly now, and see if that's going to work. I'm going to click on this part here, edit the part, and I'm going to change the diameter. Oh, that's the first part. Hold on, we need to go back to the very first part, which is this one here and make sure we're going to change the diameter of that one. Click on that. Instead of 200, let's change it to 150. Click on "Exit Sketch" and you can see both parts automatically adjust to the correct size because this cover is based upon the size of the bottom piece.
Now, what we want to do is use the "Hole Wizard" and create some holes directly in-context. I'm going to go back again and edit this part here. Then, I'm going to go to "Features" and I'm going to go over to "Hole Wizard." I'm going to use a counter sunk screw here. We're going to use "inch" There it is and I believe it's going to be 1/4"-20.
Once we have all of that defined, let's choose a position and then choose the top surface here. Then I'm going to switch over to the wire frame view so I can see directly below and then I'm just going to snap to the center points of where these tapped holes are directly below. It's a very quick and easy way to make sure these two stay aligned. Then any changes to this pattern will automatically be reflected in my parts. Go back to "Shaded View" and you can see, there is my counter sunk screws directly over my holes.
Then, let's go ahead and change the assembly again. This time I'm going to go back to that first part. Edit the part. Change it back to the 200. 200. And then exit out of the sketch. You can see both parts automatically adjusted, as well as the holes because these holes here, are tracking where the holes are directly below it. So that's in-context modeling You can do it in Assembly and relate one part to another part, or one part to multiple parts.
You can use it with the Hole Wizard with sizes with relationships, as well as just straight dimensions.
He also breaks down the three segments of the test (part modeling, configurations, and assemblies), providing strategies that will help you pass each section. At the end of the course, there are two sample exams to practice what you've learned.
- CSWP requirements review
- Working with sketch entities, tools, and relations
- Using the boss and cut features
- Performing sweeps and lofts
- Smoothing corners with Fillet and Chamfer
- Creating linear and circular patterns
- Setting up equations
- Creating multibody parts
- Setting mass properties
- Working with materials and constraints
- Inserting components
- Setting up reference geometry
- Arranging features to change the part
- Working with suppression states
- Using a design table to build configurations
- Establishing standard drawing views
- Annotating your drawings