Start learning with our library of video tutorials taught by experts. Get started
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.
The shell command takes a solid and turns it into a thin walled feature. This is used a lot with molded parts. This feature can do amazing things with just a few clicks. I've opened up 9.5-1, and I have a part here that we're going to work on, doing some shelling on. So the shell command is under the feature tab, and come down here to Shell. So the cool thing about Shell is all you have to do really is select the face you want to remove, and you don't have to remove any if you don't want to. In this case, I can also choose the thickness, so I'm going to type 0.1, and over here, I'm going to not choose any faces at all for remove, and go ahead and click on OK, and it looks like it did absolutely nothing, but in reality, it actually did.
If you click on Section View, you can see, it actually removed all that material on the inside, and it's actually a shelled out part, or a hollow part now, so that's pretty cool. Go ahead and turn that off, and come back to Shell. This time, let's choose a face to remove. I'm going to choose the top face click OK. You can see, it removes that top face and shells out the rest of the part. So this is perfect for doing something like a molded part, when you want to remove all that material from the inside of the part. I can also go back to Shell. Edit the feature, and I can choose to maybe remove the face like this, and again it removes all the material, and comes up with a nice part.
In this case here, I also have this little radius, and maybe I want to get rid of that as well. Again, I come back to the Shell, edit the feature, click on the face, remove, click OK, and it just removes that altogether. Also, what's used a lot of times with Shell, is Draft. If this part was going to be a mold part, we'd actually like to have some draft on the inside and outside faces of this part so they can pull out of the mold. So what I'm going to do is go back to the shell command, and I'm going to turn these faces off. So we're back to the kind of simple part we have, click OK, and then directly before we do the shell, I'm going to take the history bar and roll that history right up above the shell command, and we're going to add some draft to the features.
Come up to Draft. In this case here, I'm going to choose the inside face here. And this one over here, and over here is called, what we call the neutral plane. And that's going to be this top face here. That's where we're going to be creating the directional pull from. Next, I'm going to change the angle. So in this case here, I want to change it to three degrees. Click OK, and see what happens. oh. What happened here? We've got an error. Sometimes when you're draft commands, it can cause other issues that you might not know about. So, before we use this draft feature here, we actually probably want to do that before the fill it command.
So, go up here, come back to this draft feature. Let's go head and delete that for right now. You see there's a fill it here, so let's actually move that history bar up above where that fill is. So now you have all these hard corners, there not fill it or anything like that. Now let's add the draft at that point and time. Click on Draft, three degrees is fine. My direction or item to draft is going to be this face here. It's going to be our neutral plane, and my face is, I want to draft to this one here, and click OK. What that does, if I look down the top down view, you can see it makes a little draft; so the bottom of the hole is actually smaller than the top of the hole.
Now, I can do the same thing to the outside of the part. Let's go again to Draft, choose that face, choose the same three degrees, and I'm going to choose these outside faces. Click OK. And again, it drafts it out. But look what happened. If I look at it, it's actually drafting the hole, making it smaller in the bottom. But outside here, it's actually making it bigger. That's not what we want in this case, because I want a direction of pull on the bottom side to go the other direction. Don't worry. Click on Draft. Click on Edit Feature, and just flip the direction of the draft And then click OK.
Now, we can roll that feature forward. We can see that I can now fill this corner here and looks good. I can come over here. I can mirror the part, and then when I shell the part, everything works out just fine. Using Draft and shelling a part gives us ability to quickly create a part that's a uniform wall thickness and has drafts so it's easy to mold. It's amazing tool for building complex parts, and it's very easy to use.
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.