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.
We can use the patterning tools to save ourselves a lot of time for building an assembly of sub-assemblies or individual parts. And we're using the same part over and over and over again. Let's give you an example. This is the tray we're going to be putting the parts on. Here is a little sub-assembly that we actually created that we want to put into these individual holes. Now, if we weren't using a sub-assembly, what we'd have to do is we'd have to take each one of these individual parts here. Lay them out in these individual holes. Then grab the individual covers and the parts that are going to go inside, and again, assemble all those together.
That could take a lot of time. To give you an example of how we might do that is, I would open this file here. I would say File>Make Assembly from Part. Click OK. Once that part's open, I'm going to go ahead and choose that very first one. Click OK, and that's going to put that right at the origin for me. Now, I can click on Window>Tile Horizontally. And I can drag the parts in that I'd like to use. In this case here, I'm going to drag in this cup, cover and let me just see this little point here that's causing trouble. View this, cutout here and hide points.
Do the same thing over here. Hide it. Then you can grab the individual item. Drag it up, put it in the assembly. Now I can expand this assembly out. You can see I've got the components here. So to get started, what I do is, well maybe I'd want to copy this component here. And I can do that by holding down the control key and dragging a second copy out. Now what I need to do here would be to use the Mate command, and I'd maybe choose the bottom of this, and the bottom of the cup, mate those together, mirror the outside of this and the inside of that cylinder, I'm going to mate those together and then I'll do the same thing again over here.
Mate this and this, click the bottom of the cup. Mate those together, click OK, and continuing on, I'd have to drag out more copies of those things. Then, what I'd need to do is grab these components here, and start mating those inside of these individual cups, and then put the covers on again. That's a lot of mating, a lot of extra work to do. That can be eliminated by simply creating a sub assembly first, and then using the Patterning commands to do so. So what I'm going to do is go ahead and cancel this, click on these and delete them. Now I'm going to come up to Window>Tile Horizontally, and take a look at this other little sub assembly they've already created.
So I'm going to go ahead and close these other components, so I just have these two open that I'm going to be working with. Here's my sub-assembly, and here's my top-level assembly. You can see inside of the sub-assembly here. If I cross-section it, I've got the base cup, I got a cap for it, and then I have this little cone inside of it representing some type of material. Go ahead and turn the section view off, and now what I'm going to is I'm going to drag that entire sub-assembly into my top-level assembly. Once I have it in there, I'm going to go ahead and mate that component. So I'm going to go click on Mate, click on the outside cylinder here, click on the outside of the cup, and then I'm going to pick the bottom and the bottom and mate those together using a coincident mate.
And click OK. Now that component is fully mated in this assembly. And now what I want to do is, use the component patterning tools. Come up here to Linear Component Pattern. First off, we're going to choose our very first direction, which is going to be any linear edge going in the direction I want to go in. I can choose the top edge here, bottom edge here, this one back here, really any edge going in this direction. So, choose that first. Come down here to Components to Pattern and I could choose it from the window here, or I can come over here to the tree and pick the entire assembly.
Then, we're going to space it out. How many do we need? So, right now if you click on two, you can see the spacing's not totally correct. If I change its value here, I could say, well maybe I want to make this at three inches. Well, that's not correct. How about five inches? No, must be four. So you can see four inches is the spacing. If you didn't know that value, you can always go back and measure it using the measuring tools. In this case here, it does happen to be four. And as I click on the quantity, I can just add a coupe more, and then if I want to add more to fill up the other spots, you can always go in direction to.
Choose the direction with any linear edge going in that direction. And then choose how many you'd like. Notice we're going the wrong direction to start off with, so go ahead and flip this the other direction and adjust that spacing and the quantity you're going to have. So we're going to have three, and our spacing in going to be four inches. So you can see they all fill up all the holes, and since you're happy with that you can always go ahead and click OK. I also want to point out before we do that is, if you come down here to instances to skip, I can choose in that box and then pick anyone of these little pink dots to remove those items from the array of parts if you wanted to.
When you're happy with it, go and click on OK. And just that easy, we did all those mates, made out all those parts without having to individually mate all those little individual parts or those individual sub assemblies. So it really is a big time saver. Patterning can save a lot of time and provides an easy way to modify the spacing and quantity of parts in an assembly. If you find yourself adding more than a few of the same part to an assembly, maybe a pattern can help out.
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.