Learn how to use the Mirror command on features and bodies.
- [Narrator] The mirror command inside of Solid Works is a great way to have Solid Works do a lot of work for you. Instead of designing an entire part, if you have a symmetrical part you can design maybe one half or one quarter of the part and then use the mirror command to then mirror that one part into the other quadrants. Let me show you how to do that. First things first, let's open up this sketch directly below that feature. And you can see here we have the entire part designed. I want to go ahead and just delete the entire sketch and now I want to draw out just one quarter of that.
So the first thing I want to do is just jump up here to the corner rectangle let's grab that one here and just draw out a rectangle. Now for fun I'm also going to add in a couple of center lines. So starting from the origin I'm going to make a center line going directly down. I'm also going to make one more that goes from the origin out to the left and I'll show you why I'm going to be doing that. Next thing I want to do is place a circle in this corner up here and let's add a couple of dimensions so this dimension from the circle to the edge is going to be one inch and from this edge to the circle is also going to be one inch.
Now you could also make those equal if you wanted to but in this case a couple of inches is not going to hurt us. All right, now, we want to define the size. So I could define a dimension from here to here which would be half the dimension or if you go from an edge to a center line, it gives you the ability to use what we call a double dimension so notice as I go past that center line that dimension automatically doubles that way I can type in the full width of my part as 10 inches and it works just fine. Same thing over here from the top to the center line, as soon as I go past that center line it gives me the ability to add that double dimension.
Let's go ahead and place it here and type in six inches. All right, now let's add one more dimension here for the one inch hole, and now we have a fully defined sketch and we're ready to extrude it. But keep in mind we already have a boss extrude feature over here because we deleted the original sketch so all we really need to do here is just exit out of the sketch and they automatically already have our part. All right now we have basically one quarter of our original part. Now go over here to features come up here to mirror and we have a couple different options here. One is I can mirror a face or plane.
I can also mirror features, faces or bodies. And body mirrors are my favorite one to mirror. I'm going to take the entire body, all the features that when into creating that body that I can mirror them all over at the exact same time. So the first thing I want to choose is that mirror face or plane so for this example I'm going to go ahead and choose this face right here and the body to mirror, remember, not a feature, not a face, but a body to mirror is going to be this entire body. Click on okay, and now I have that double body right there.
Let's try it one more time. Come up here to mirror, mirror face or plane is going to be this one here and then not a face, not a feature, but a body, go down to the body one and choose that body. Click okay and now we've mirrored the entire shape over to create our part. The great thing about this, if you want to make any changes all you have to do is make a change to one quarter of it and the mirrors will automatically work. Let me show you how that works. Let's go back here to my original sketch. Anything I add to this sketch here because we're actually doing a body mirror will automatically propagate to the other four quadrants.
Let's go ahead and add maybe like a triangle in there so I'm going to use the polygon tool we're going to say three sides, and let's draw out a little triangle. There it is. And exit out of the sketch. And as you can see, because we did a body mirror that triangle automatically propagates to other quadrants in that design. So pretty cool what you can do with a mirror command. Now let's make it a little bit more fun and jump over here to features let's do another mirror face or plane let's go ahead and click on this face right here and as far as our body to mirror let's choose this entire thing so now as you can see we can start building these parts and mirroring things around to create some really complex geometry all with a couple of simple commands keep in mind this all started from just one quadrant with one hole and one triangle and you have a pretty complicated part now.
I also want to point out you can do a feature mirror in this case let's go ahead and choose something like a hole. So in this case let's go ahead and choose something like a hole so I'm going to start a sketch here on the top surface and I'm going to design a circle right over here. Cut that through my part, so I'm going to do an extruded cut right through my part I'm going to say through all click okay and now I have that hole. Now if I want that hole over here on the other side I don't want to do an entire body mirror I just want to mirror just that hole so I need to have a face or a plane to mirror that over.
If you look in here you can see we don't really have a plane in the middle of the part now so you might want to go ahead and add a reference geometry plane between the two faces out here, so this face and that face, we'll put a plane right there in the middle and then once you have that plane and you have that cut you can then click on mirror and it will automatically do a feature mirror over to the other side. So there's a couple different ways you can mirror things. You can mirror body you can mirror face and you can also mirror just a feature itself so keep that in mind when you're working try to design maybe just one quarter or one half look for symmetry in your design and really try to just do a portion of the work and then use that mirror command to do the rest of it for you.
First, see how to how to use the sketch tools to create two-dimensional sketches that become the foundation for 3D objects. Next, look at extruding and revolving 3D features; creating complex objects using the Sweep, Loft, and Surface tools; and modifying parts. Learn how to create uniform holes with the Hole Wizard, and explore more advanced modeling techniques using equations, mirroring, and pattern tools. Then review best practices for putting parts together in assemblies and building robust structures. The course wraps up tips for creating detailed drawings that relate the final parts and assemblies to a manufacturer, complete with an itemized bill of materials and drawing notes.
- Working with templates
- Creating sketches
- Extruding and revolving features
- Applying materials
- Sketching lines, shapes, and polygons
- Trimming, extending, and transforming geometry
- Adding fillets and chamfers
- Working with planes and coordinates
- Creating patterns
- Modeling advanced parts
- Making holes
- Designing with blocks
- Building assemblies
- Mating parts
- Linking sketches
- Using design tables
- Creating part and assembly drawings
- Creating dimensions
- Adding annotations