Viewers: in countries Watching now:
SOLIDWORKS is the world leader in 3D software for product development and design. Start creating manufacturing-ready parts and assemblies, as well as detailed drawings and bills of materials. In this course, author Gabriel Corbett shows how to create 2D sketches that will become the basis for your 3D models. You'll use the Extrude and Revolve tools to turn 2D sketches into 3D parts, then create more complex geometry with sweep and lofts. Then learn how to use the cut features to remove material and shape parts, and use mirroring, patterning, and scaling to modify parts. Next, you'll combine parts into movable assemblies and subassemblies. Finally, you'll create accurately annotated drawings, complete with itemized bills of materials that relate the final parts and assemblies to a manufacturer.
Mating parts together is a fundamental skill of working with assemblies. Mates are very similar to sketch relationships, we choose 2 or more faces planes lines or points and then choose how we want to have them connected. The most basic is a coincident mate, this is basically just saying you want the two items touching. Let's take a look. Over here we have an example of a block and we have a couple of components we want to attach to that block. We want to make those components together. This component here is the first component in our assembly and it's fixed. It's not moving around. Now what I want to do is I want to add these other components to it.
So, come up here to the assembly tool bar at the very top, or on the assembly ribbon. And come over here to mate. And the way mate works is it automatically will help you choose the correct mate depending upon your selections. So, in this case here, I want this face here to touch this inside face here. And, if I just click on those two faces, notice what happens is it actually moves over till those two faces happen to be aligned if you look at it. From this angle here, now the parts not perfectly aligned because still down here but that's our first mate in fact it takes 3 mates in general to full define where 2 components are in relation to each other.
So my very first mate notice it's this face here and that face there, and those are going to be mated together. Go ahead and click on OK, to accept the mate, and notice, the default mate that it chose, was this one called coincident. That means those two faces are going to be touching. You can also make them parallel, you can make them perpendicular, you can just lock it in place. You can define the distance, and the angle. You can flip the direction, or you can even undo the last one. So, if you're happy with it, go ahead and click on OK, and it mates those together. Next the thing I want to mate together is maybe one of these faces here so, in this case here I'm going to choose this front edge and spin it around and choose this edge here once those mate together.
Again, it's using a coincident mate. And go ahead and click, OK. This way I should be able to actually grab this component now. Actually slide it back and forth. And you can see that it, because this face and the back face are mated. And these two top faces are mated. This will actually slide. And you can actually take a look at the motion that's going to be happening between the components. Next, if I slide it all the way in here, I can define, maybe, a mate between these faces here. What I can do is I can say, this face here is going to mated along with maybe one of these bottom edges.
As soon as I do that you can see these components come together. Click OK, when you're happy with it, and now you can notice, we have a couple of issues in our design. This is one of the key points of many things together inside a solid work before you build the components. You can see, well this is sticking out just a little bit here, and you know these angles really aren't the same, so maybe we want to go back to our design, see what these errors are in our design. Why these things don't fit together perfectly like we would expect them to. A quick way to do that, you can always jump right back into those parts and make the modifications.
Click OK, when your happy with the mates and if you do want to go back and change a part click on the part notice we have an in context menu that pops up with a bunch of options and I just want to go over those really quickly. The first one is hey, let's go open that part number 2 is let's edit that part inside this assembly. We can come over here, we can hide that component. We can change its transparency. We can suppress it or turn it off or take it out of the assembly temporarily. We can obviously add some mates to it. We can view the mates that are attached to it. We can come over here and take a look at some of those component properties. Click on again and come back here and edit the feature itself.
I can go ahead and edit the sketch. I can change how it looks. I can copy those appearances and paste them somewhere else. Here I can paste an appearance that I copied from somewhere else. Down here, I can select others, I can select sketches, I can zoom in, I can look normal through this, I can fill it and chamfer. So, I've got a bunch of things I can do all within this assembly environment, just by clicking on the part. In this case here, if I wanted to modify the part, let's just go ahead and click on, Open part. It opens it up. I can open up that Boss extrude. Make some change, maybe I'll change it to 3.5.
Click OK. Exit out of that. And as soon as I close out of this it saves the part. Open the assembly, and notice that I automatically updated the part, and now it fits perfectly in the assembly without having to bring it in again, or any other things we have to might change on it. And now obviously works perfectly, and you can always go back and change things as needed on the fly. Lets go through a couple other mates. In this case here, I'm going to go ahead and I'm going to go grab this wash looking part and I want to place that over this pin. I'm going to go ahead to mate and I'm going to choose this outside cylinder.
And I'm going to choose this inside cylinder. And notice those two parts slide together and by default it chooses for you. It can concentric mate. Go ahead and click, OK. And now I have this mate. I can click, OK again. And notice I can slide this component forward and backwards. In fact I can spin it around. But, it's still not touching this face here, so I might want to add one more mate. So go back up to Mate. Or, if you don't want to choose that originally, you can actually click on the face, hold down Ctrl, move the model around. Ctrl+click the other face, and then click on Mate, which will automatically bring those right together for you.
Click, OK, and there they are mated together. Next, let's mate these two components, here. You have a couple different options there. One of them, I could just choose the outside cylinder here, and choose the inside. And those would slide together. Or if you didn't want to do that one, you could choose this face here and you could choose this face right here, and again, those would slide together, and actually, you kill two birds with one stone on that one. Because not only does it make them concentric, but it also brings them together in the right location. So you can really think through a lot of different ways to put these things together in different methodologies.
Also, if that were to happen to flip upside down, you can always flip it the other direction. And flip it other ways. So, you can modify how these components go together and you have a lot of options. Click, OK. Things are looking good. All your components made it together. And notice I want to point out a couple of other things over here on the tree. Notice these components here have a little minus sign, right next to the icon. This one down at the bottom does not, because it's fully defined. Whenever an item is fully defined in an assembly, it will not have a minus sign. If there is still some degree of freedom for that item to move, it will have a little minus sign.
So both this component here and this component here, both have the ability to still spin around their shafts. And that's why they're not fully defined. Now, in this case here, it doesn't really matter, but I just want to point out that sometimes, you can look at a component, and make sure you know that it's undefined, or under defined, and that's why. These basic mate tools will help you build your models. When building mates, try to choose items that are stronger. Versus weaker items. For instance, parts start off with three fundamental planes and we can not remove them. So, if you choose to make two planes together there's no way to break this mate.
However, if you made a corner point to some other part anything that changes that point will break that mate. Try to think about the easiest and most robust ways you can mate your parts together.
There are currently no FAQs about SOLIDWORKS 2014 Essential Training.
Access exercise files from a button right under the course name.
Search within course videos and transcripts, and jump right to the results.
Remove icons showing you already watched videos if you want to start over.
Make the video wide, narrow, full-screen, or pop the player out of the page into its own window.
Click on text in the transcript to jump to that spot in the video. As the video plays, the relevant spot in the transcript will be highlighted.