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.
Mates are very similar to sketch relations. We need to have a minimum of two parts to mate together, and an idea of how we would like to connect the parts. Much like relations, we have a basic way of aligning parts. For example, we can use coincident, parallel, co-linear, distance, and a whole bunch more. Coincident is the most common. We've already seen a few examples of this in earlier movies. This mate attaches two items together by touching the sections, or faces, or lines, or points. In general, most parts will require three mates to fully define the location and orientation of the part.
To get started, what I have here is an assembly created which is 12.1, and that's created from this part here. I've already used that one, so I can go ahead and just close that file down. Now what I want to do is get these other two components in there. So i'm going to click and drag those components into that assembly. Go ahead and close these other one's down. We're not going to be using them anymore. And then go ahead and expand out your original window to full size. Now the very first mate we're going to look at is the coincident mate. Like I said we've done this a little bit in the past. However, I want to point it out again.
So this case the first step is rotate the component around by holding down the right mouse button, and get it close to the orientation you'd like to be using. This one here I'm not going to be using quite yet, so I'm going to move it over here. Now, I know that i want this face here, to be touching that face there, and that's generally the best way to think about mate, is to say them out loud. I want this to touch that. I want this hole inside of that. You know, say things out loud and it makes a lot of sense. Because all you are going to doing when you choosing mates is picking pairs of faces that'll be touching each other or at distances apart, or at parallel, or something like that.
So first things first. Let's go ahead and choose mate. And my first selection is going to be this face here. And my second selection is going to be this face here. Now keep in mind it's always better to pick faces or planes to mate first. And secondary would be lines. And last choice would be picking a point. Because a point can be easily destroyed if you were to maybe radius a corner or a corner or modify the part. As soon as that point is no longer there, that mate is now broken and your whole assembly falls apart.
If you choose big surfaces like a full face or a full plane, then they're really hard to break. When you're happy with what you have, click OK, and you can see this parts are now mated together, but we still need a couple other mates. If I drag it around, notice it slides around here and it looks like it's maybe off in space. But in reality, it's not. It is on that face, it just needs a couple other mates to define where it's going to be in space. Now, the next mate I wanted to point out is the parallel mate. So parallel means this face here and this face under here aren't necessarily going to touch, they're just going to maintain some type of a parallel relationship.
Let's go over to mate. Click on this face here, and spin your model around and choose this face here. Now by default what happens is the mates try to come together and automatically chooses coincident. In this case I don't want coincident, so I want parallel, so let's go ahead and choose that one right next door. Choose parallel and then click OK. Now what I have is, this can still slide around, but my orientation is now locked to this parallel relationship between the two. Finally what I can do is a distance mate.
So a distance can determine how far maybe a face is from another face. By default, it's going to automatically choose coincident, but that's not what I want again in this case, so what I can do is just go either here or over here on the left and choose a distance I would like to put in there. And notice as soon as I click on that distance icon, it automatically moves back to the place it was prior. I'm going to type in 1.0 for one inch. Click OK and it gives you a preview of what's going to happen. You can see, yeah that looks pretty good. And if I want to change that I can always type the value in here, or if I didn't want to what I can do is I can flip the direction so I can put it the other direction so it's actually inside.
That's not really what I want to do here either, but I just want to point out what you could do. And when you're happy with that, go ahead and click OK, and now this part here, notice, it's defined by that one inch dimension, from here, and it's in parallel, but it still has the ability to move up and down. I defined the three different mate pairs. I've got a coincident mate, I've got a parallel mate, and I have a distance mate. And that's all I really need to show in this example. These three mate types will generally handle most parts with flat sides. As you get used to the mate tools, you'll see that SolidWorks automatically chooses a mate based on the selections you make, and we may need to override those if we're looking to do something a little bit different.
You still have the option to change the mate, however it gives you a nice starting point to put things 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.