Linking sketches to other parts

- One of the most powerful things you can do inside of SolidWorks is to link features from one part to another. In this case here, I'd like to have this cap automatically adjust its size to the size of this base down here. If you take a look at the parts themselves, so click on this one this here, click on "Open the Part", and you can see I've got a basic revolve here and it's defined by this three-inch diameter. If I then go over to the other part and click on "Tile" and look at the assembly, I can take a look at this part here, you can see I've got a very similar sketch.

This one is also defined by that three-inch diameter. Go ahead and exit out of that sketch, and let's go back to the assembly. Now what I would like to do is I would like to link these together by separating that dimension from the individual part and linking it to the base part. So, to do that, I need to edit a part in context, and what that means is clicking on this part here, and instead of clicking on "Open Part", go over to the next one over here, you can click on "Open Part in Position", you can say "Open Drawing", you can say "Edit Part". That's the one I'm looking for is "Edit Part".

You can see the other part is now transparent, and I can now jump into the tree for the original part here, and link it together. So, notice I have sketch number one, I'm going to go ahead and edit that sketch. Click "Normal To" so you're looking straight at that sketch. Now what I'd like to do is delete this dimension here, so now I have the ability to drag this in and out, and then I'd like to link this diameter to the diameter of this outside of the base part here. So, to do that, I'm going to click on this line here, and hold down control and pick the outside edge there.

I'm going to say these are co-linear. Notice everything becomes fully defined again, and then exit out of that sketch, and then exit out of the part, and now I have those two linked together. Now, it looks exactly the same, but here's where things get interesting. Let's click on this part here, come over here and edit that part, go to the original sketch, which is right up here, and instead of three inches, let's go ahead and change that value here to six inches.

It will automatically update, and notice the cap automatically resizes the same amount. You can add in-context features all over your part, linking to all types of different features, dimensions, and sizes, and this is just a very simple example, showing you just one linked variable, but you can add hundreds, and you can have one part as the driving part, and you can have multiple other parts all referencing it and adjusting as that part changes. It's a very powerful feature inside of SolidWorks, and allows you to make a lot of edits and changes, all based upon one master part.