ANSEL: Hi. My name's Ansel for CS50 [? R and D. ?] Today, we're going to walk through some of the basics of mechanical part manufacture. So let's jump right into it at kind of a high level, I'll just over the basics of what we're doing. I'm going to CAT up which stands for-- it's just like Computer Aided Drafting, which is just a medium of designing a part in a computer program called SolidWorks. And then from there, we'll be able to 3D print our part, which is a different medium for manufacture. If we wanted to make it out of maybe metal perhaps, we could machine it out of maybe aluminum or steel. But 3D printing is kind of a nicer way to do that for simple parts that are not subjected to really precise or intense stresses and strains, just because it's a really quick medium by which we can prototype. Like I said, we're going to be using SolidWorks today. So let's go into SolidWorks, and I'll kind of walk through the basics to make a new part and walk through some of the subtleties that are easy to gloss over. If we go into SolidWorks here, and we go to our file, let's open up a New. And we'll just click Part and select OK. 

We have this blank canvas by which we're able to draw our part. And first, we're going to kind of create the skeleton, and then build it up, and then add in some of the more intricate features. At first, let's just go to Sketch, which is a kind of in the upper left-hand column over here. And we click Sketch, Sketch. And then, it will give us a choice of different planes that we can sketch it on. 

I'm going to build this part, which is this little iPhone dock, from the ground up. It's almost as if we're looking down on it. And then, we'll build it up. Naturally, we'll select the top plane over here. And it will highlight itself in orange. And then, SolidWorks kind of does the rest for us. 

SolidWorks is nice in that it does a lot of the heavy lifting. If you give it a geometry, it'll just figure it out. That'll become more apparent as we walk through the design. 

At a high level, the dock is just a rectangular base. And then it has kind of this lofted feature here, that's just an extruded base which holds the phone. And then, it's tilted at an angle. Some of the dimensions are kind of arbitrary. I think I chose in this specific model to make the tilt something like 15 degrees. But that's all up to you. One thing we do need to take into account is that when the phone is sitting in the stand, it has some center of gravity or some center of mass that needs to hang over the stand. For example, if we did not include this part right here, then when we put the phone in it, the center of mass would extend beyond the base. And it would just fall over. 

What we can do is make this base a bit wider in the back such that the center of mass of the phone is over the base, with some extra kind of comfort that's built in there such that when you put your phone in it, it won't fall over. That's just something that we need to take into account. That's pretty simple physics. 

Let's start out with the base. And so we're already in our sketch plane. If we go over here and we select the rectangle-- it's a little bit small, so I'll just point to it-- select the rectangle here. And I'm going to start it at the origin, which is kind of arbitrary. But that's just how I'm going to do it. And we draw a rectangle. Now we have this rectangle. And SolidWorks knows that for instance, the bottom and the top lines are parallel. And the side lines are parallel. And they're all horizontal and vertical, as denoted by these green boxes. These green boxes a really important. And I we'll kind of talk through them a lot as we continue through the design process. But essentially, they're just saying that there is some relation. For example on this line right here, there's a green box with a vertical line next to it. That's saying that this line is vertical. It's constrained to being vertical. We can move it around and drag it, but it will never be at an angle that's not vertical. 

Those green lines will make your life a lot easier because it will allow you to make relations and not have to do is much work. SolidWorks will figure it out for you. And I'll kind of talk through that as we get to it. 

What I just did to kind of enlarge that sketch is I just hit F on my keyboard, which fits your current sketch to your screen. For example, if you're maybe really far away and you just want to make it fit nicely, just hit F on your keyboard. 

Now that we're here, we can start to add dimensions. One of the most important themes in designing a part is that you can do all this CADing and make a really pretty looking part, but it needs to be physically applicable to something. That something in this case is a phone. Our dock needs to physically adapt to the phone. 

The way that we do that is we measure the phone. And then, we had a little bit of a boundary in And there will be some tolerance to its manufacture. The tolerance concept is just saying that when we manufacture it or when we print it, the printing head is not exactly at the location that we want. 

It's going to be off by some very, very small amount. And that small amount is the tolerance. And we design in that tolerance if we're making a really sophisticated part. But in our case, it doesn't really matter. And I'll get to that a little bit later. 

Let's add some dimensions. And you can do that by clicking this button, which just says Smart Dimension. To Smart Dimension a line, we just click on it and up pops this dimension. You can move it around, place where you want. We'll place it up here for now. 

And then when we click, this box pops up and allows us to enter a number. Just as kind of a higher-level theme, it's important when you're dimensioning a line to not have your dimension for this line cross over other dimensions, as it makes your drawing or sketch pretty cloudy. So we want to make it as clear as possible. 

Luckily, this dock is a really simple part. And we can design it pretty readily with not that many dimensions. But just kind of at higher level when we're adding in more dimensions, we don't want to cloud up the sketch. We add this in here. 

We have no idea how wide to make it. So the first step is where I'm just going to grab my phone, which is a pretty simple kind of rectangular prismatic shape with the corners rounded off. And let's measure it. 

This tool is called a pair of calipers. This is a digital pair of calipers. And I'm just going to turn it on with the on/off button. I'm just going to clean the inside faces of any dirt or grease, and then, zero it. It's already zeroed. 

It's in millimeters, which we don't want. We want it to be in inches. Our whole part is being designed in inches. And if you don't know what your current units are, in the dimension box it says 4.4329 whatever inches. 

You could design in any units and still have a beautiful part at the end. But I'm just choosing to design this in inches. That's the standard in America. I'm just going to change the units up here to inches. And wha-la. 

Let's measure the width of our phone. And that'll give us an idea of how wide to make the base. I'm just opening up the calipers here. And I'm just going to close it down on the phone. And we see that it is 2.30. Kind of wiggle it around a little bit to get the smallest dimension-- 2.305 inches wide. We want to make the base a bit wider than that. So let's say we make it, I don't know, maybe 2 and 3/4 inches wide-- so 2.75 inches wide. That seems about reasonable. Just as kind of maybe a sanity check, we can open up the calipers to 2.75 or pretty close to it, and see that there's kind of enough wiggle room outside of between the phone and the calipers to add material to support the phone. So 2.75 inches sounds reasonable. 

Hit Enter. And our dimension is constrained there. Now we need to do the same thing on the vertical line here. This is kind of the tricky part that requires-- I guess it's not tricky, but it's a little bit more sophisticated than just guessing a number. This dimension that we're adding is this distance. Like I was saying before, we can't make this too short. We need to make it long enough such that the middle of the phone, the center of gravity of the phone, is over the base. You could do this by drawing out like a free-body diagram, finding the center of mass, and then just kind of drawing this out and using geometry to find it. That will certainly work. 

I'm just going to ballpark it and say we can make it two inches, as that seems to be just by eyeing it, plenty. You're welcome to draw it out and figure out the geometry. It's pretty simple. And it won't take you too long. Two inches sounds like there'll be plenty there. 

I guess as a sanity check, this is a dock that I had made a while ago. And if we place our phone in there, we see that it doesn't tip over. And this width is 1.8 inches. So two inches will be plenty. Cool. 

Again, we hit Enter. And now, here's something that is really important. We see that all of our lines are black and all of the points are black. The line and then the points or the nodes where they intersect, are all black. 

When everything in the sketch is black, that means it's completely constrained. By that, I mean that you can't drag anything around. Every point in this sketch has been defined. We can't change its location because there are no degrees of freedom. If I click on this dot here, this intersection of these two lines, and try to drag it and move it around, it doesn't move. 

Whereas if I kind of delete one of these dimensions, I'll just do this for the purpose of this example. If I delete this top dimension, notice that this line is now blue. So I can move it if I just maybe click on this point. It's no longer completely defined. I'm just going to undo that. And our sketch returns to black. Great. 

I'm now going to exit the sketch. And we will create an extrusion from it. There's this theme in SolidWorks of creating sketch is to design at a high level what you want to do, and then extrude it, which means to kind of create material out of your sketch. In this case, we've sketched a rectangle. Now we're going to extrude it, which means create a prism out of the base of that rectangle. 

You can do more sophisticated things, but we'll get to those a little bit later. There's no need to do anything tricky right now. It's pretty straightforward. 

The next parts of these designs will incorporate a lot of relational geometry and relational symmetry. And what that means is when you create a feature of your part or really anything, you want to relate everything in your sketch to something else-- something that's defined. In this specific case, we have the origin, which is where I started. There are these two small red vectors here. 

Everything is defined in relation to our origin. So we don't have to worry about it. But if we wanted to define a feature that was symmetric, we wouldn't have to draw it twice. We could draw it once, and then define the mirror image of it to just be based off of the symmetry from the first part. That might sound a little bit confusing. It'll become clearer as we walk through the design. 

I'm hitting Exit Sketch in the upper left-hand part of the screen here. Now we have some sketch, which is this kind of gray. We'll go to Features. We're going to click on the sketch. And it's highlighted in blue. The dimensions pop up. And now, I'm in this Features tab up here in the top left. You'll see that there are a lot of them on my screen. We go to Extrude Boss/Base. And now our sketch has become a prism. I'm going to make this-- and you can kind of choose a side somewhat arbitrarily-- let's say we're going to make this 0.15 inches thick. I'll say 0.150 inches thick. 

And I'm entering that into this box here that says D1, or that's just the thickness. That's the box that SolidWorks defaults to. I'm just going to turn my sound off there. And we hit the check mark. And great. Now we have the base of our sketch defined. Cool. We hit that green arrow and it goes away. I said that you can choose the thickness somewhat arbitrarily because the stresses and strains that the phone is imparting on this part are minimal. The phone is really light and there is plenty of support at the base. If we were defining this for a phone that was maybe were incredibly heavy, we would have to run some more sophisticated analysis on this to ensure that the base wouldn't like buckle, or crack, or deform, or deflect under the stresses and strains. 

But I think for the context of what we are doing here and kind of anything that's associated with 3D printing, that analysis isn't really required. You just can kind of assume that it'll be strong enough, because we're really not putting much force on it. That's just kind of side note. 

We have our base here. You can notice that I may be panning around a little bit. The way that I'm doing that is I'm holding down the jog wheel on my mouse so it can jog but you can also push down it and physically hear it click. I'm pushing down on that. And then, I'm just moving the mouse around. Push down the middle of the jog wheel, and we see it we can manipulate our part in three dimensions. 

Now we want to sketch this side feature here, which is actually going to end up holding the phone. And I said that that'll be at a 15 degree angle. The way we do that is we can define a sketch on the side here and then extrude it down. We want to kind of look at this face of the base, sketch this, all of these curves and everything, and then extrude that up. Let's do that. 

We want to look at just this side. Well, we can tell SolidWorks that we want our view to be kind of normal to this plane. If I click on this plane, you'll notice that this little box pops up with all these options. And of these options, there's a little blue rectangle with a normal vector popping out of it. If we just hit that, now are looking at the normal to this plane. We're looking down on this side plane, which is what we want to do. 

As this is still selected, we go back over here to Sketch which is in this View tab over here. And we'll hit Sketch. And now we're sketching on this plane. Great. Now we're sketching on this plane. 

We will add-- this is not going to be kind of a standard rectangle because the top line and the bottom line are no longer parallel, because we decided to put the phone at an angle. You don't need to put your phone at an angle. If it were vertical, that would still work, though it might not hurt have kind of tab in front. 

That would look kind of silly. Having it pointed at an angle is just a nicer design. Also, if somebody's walking up to your table or your booth and your phone is on display displaying an app, it's just kind of visually more pleasing to have your phone tilted back a little bit, kind of in the way that your computer screen is tilted back a little bit. 

Let's see. How did I design is the first time? Let's go like this. We're going to go to this bottom corner here. And I'm just going to draw a line up here. And I'm just kind of roughing out the shape here. Don't worry about the relations. We'll take care of those in the second. 

To exit the line drawing, I just double click and that gets you out of there. If you hit this green arrow in the left pane over here, that means that we can exit drawing a line. Now we have something that kind of resembles what we need. 

But here is an important part, and this is what I was saying before. We need to add a relations to everything. The analogy could be drawn to when you're writing a script and you're using a constant pretty frequently, you might define the constant at the beginning of your file, and then use it kind of throughout your code, such that if you need to change this number, you only need to change it one time. And then, it will kind of propagate through your code. 

It's a very similar case here. If we define all of these relations, we only need to add the dimension one time because everything else is going to be redundant. So that later on if we want to go back and tweak the design maybe, you only need to change one dimension. For example, this line and this line need be parallel. But they're not right now. So let's make them parallel. 

We click on one. Now I'm holding Control on my keyboard and I'm clicking on the other one. And now, they're both selected. And this little box pops up. And there, one of these options is Make Parallel. We select that, and now these two lines are parallel. Cool. 

We want this line, and again holding down Control to select both at the same time, this line to be perpendicular. One of these options is Make Perpendicular. If you select these two lines and maybe you're not seeing this box, you can hover over to this left panel over here and it has all of the same options-- perpendicular, parallel, equal. Equal means equal in length. 

We're going to again do this. Just by induction because I made these two perpendicular and just by geometry, these two have to be perpendicular. But it can't hurt to add in that second relation. 

Now let's make this point and this line coincident. Again, I'm just hitting this option Make Coincident. Now we have the general shape of the structure that's actually going to hold the phone up. I'm going to just hit F there to kind of center this out. Looks pretty good. 

I'm just going to go back here to viewing this plane at a Normal . If that box is not popping up for you, there is a panel up again here at the top of your sketching field where there's kind of this like box outline. You can hit that, and this little menu pops up. And again, you have the Normal to operation available to you. 

Now let's define that 15 degree tilt that I was saying before. We're going to go to Smart Dimension. Smart Dimension is just that smart. It can dimension the length of lines. It can dimension angles between two lines. It just figures it out. 

If we select this vertical line and then select this angled line, it shows us kind of the angle between them. If we click on that, this is in degrees. I guess you could do it in radians. Degrees I think is more natural. I'm just going to 15.0 degrees, hit Enter. Cool. And now, it's completely constrained. 

We can also define the length of this line, again using Smart Dimension. And we can say, I'm just ball parking this kind of by eye, seems like maybe 5/8 of an inch would be enough. I'll just say 5 divided by 8. You can do operations in the Smart Dimension field like addition, multiplication, subtraction. 

And we hit that. And now, we have these dimensions. You might say oh no, two of these dimensions, the angle dimension and the length dimension, are crossing. That's not too pretty, which I would definitely agree with. You can bring that in here to eliminate that. 

We'll notice though that one of our lines are still blue. We want everything in this sketch to be black before we do any type of extruding. We need to constrain this. If you look at this, it might not be obvious to you where the degree of freedom is. If we want to figure that out, we can exit Smart Dimension-- which I do by just clicking it again to turn it off-- and then drag one of these points. 

We notice that this can move along this degree of freedom, which we can prevent by describing the length of this line. We'll go back to Smart Dimension. And we're going to dimension this line here. And we'll call that the thickness of the phone plus the thickness of our material. I don't know how thick that should be. We can pretty simply measure it. I'll just go grab our calipers here. And I'm just going to measure the thickness of the phone It's showing here 0.303 inches. I have a screen protector on my phone. It's probably not going to make too much of a difference. 0.303 inches plus two times the thickness of the wall-- we can kind of I guess at the thickness of the wall. 

Like I said, this structure will be plenty strong. We don't really need to worry about making the walls too thin, unless your paper thin. So let's say 0.303 inches plus parens two times the wall thickness, which I'm going to say is-- I'm just guessing here-- I'll say 0.15 inches, which is the thickness that I made the base. It seemed to work. Cool. 

SolidWorks does all the math. We can kind of drag this dimension to make it look a little bit prettier. Nice. Hit our green arrow and we are completely defined. Everything is black. This is great. 

One thing, and this is just an aesthetic point, is there's this little triangle here. Well we don't want that triangle to be sticking out when we extrude it, because it'll look like a hump in the front face. We want it to be smooth. To eliminate that, we can do what's called an extrusion. There are two types of extrusions. There's kind of extruding to create material and extruding to remove material. We'll extrude to create material in making this feature here that will hold the phone. And then, we can remove material here. And I'll get to that in a second. 

Let's first exit our sketch. We have the sketch here defined. We can go over here and click our sketch. One thing that I will note is this list of things on the left-hand panel is called the Feature Tree. Just like when you're maybe creating variables in your code, you want to label them in a way that's pretty self explanatory. We should label everything in our Feature Tree to also be pretty self explanatory here. 

This Boss Extrude 1, if we click on that, it highlights in blue what the feature is, which is the base. But just glancing at the Feature Tree, if I saw Boss Extrude 1, that's not at all illustrative to what it does functionally. We can rename that. And the way to do that is just once it's highlighted in blue, just click and hold. And now, you'll see that you have the ability to rename it. Let's call that Base. 

Now if we click on Base, again the base will highlight. And I think that's just a lot more helpful. It might not really make a difference in a simple design like this, but for a really complicated part or one that has a lot of features, it will help you. 

Let's now extrude this part. We're going to click on our sketch, go back to Features in this tab display pane here. And we are going to go Extrude Boss/Base again. It's asking us reverse direction to sketch. Well, that might not initially be obvious to us which direction that is, so we can hit Yes and kind of correct it later. 

We're going to click on our feature here. And oh no, we see that it is extruding in the wrong direction. That's a pretty easy thing to correct. We just need to tell the extrusion to extrude it in the opposite direction. 

In our left pane over here, you'll notice that there are these two arrows. And when we hover over it, it says Reverse Direction. So if we click on that, now we notice that it is now extruding in the correct direction. 

Right next to that is kind of a drop down. And there a bunch of options in here-- Blind, Through All, Up To Next. We want to, I guess we could enter the thickness of our base as the dimension for how deep to extrude it. But that's kind of sketchy-- no pun intended. Let's go to Up To Next. Oops, sorry. I believe it iis-- I thought it was Up To Next. You can just click on the surface here if you don't know which one it is, like I did not just. SolidWorks will figure it out for you. We'll hit our green arrow. And now we have the feature that will be actually holding the phone. It's now starting to resemble what it will look like in the final product. 

You might think at this point well, in the finished product there's this kind of curve here. And it's curved on the back I don't know if you can really see that. And we didn't sketch that in. Those features are what are called fillets. Fillets are something that we use in mechanical engineering to eliminate stress concentrations. 

You can imagine if you have a part that has two lines coming together at a really shallow angle, they'll create kind of a really sharp point. And if that part is subjected to any stresses and strains in that plane, all of those stresses will concentrate at the vertex of that point. So to eliminate that, we add a fillet, which just rounds that surface off and smooths everything out. 

If you're interested in kind of the logic and the material science by that, just Google "stress concentrations." But at a high level, fillets make it look nicer too. So we'll add those in. We'll do that kind of at the end, as that's pretty quick. 

You'll notice though that there's this hump that I was talking about. And it does not look good at all. So let's get rid of that. We're going to just highlight this face here. Oops, I did not mean to do that. Highlight this face here and go Normal to it. And we're just going to add a sketch here that will get rid of this little triangle. 

Let's relabel this Boss Extrude 2 to be, let's just say Phone Support. And if we hit the little Plus button right here, you'll see that there is a sketch here. By default, SolidWorks kind of hides the sketches away from you once you're done with them, as it will kind of cloud how the part looks. But we need to reference some of the geometry that's in it. 

If we just kind of hover over it, this little box pops up. And there are these I guess they're little glasses. We can hit that button. And now the sketch is visible to us. Or at least, it should be. Yeah. If I just hit F here to zoom in, you'll notice that now that we have access to all of these lines and their dimensions. 

The cool thing about this is we can create another sketch that actually references the geometry of a different sketch. If we sketch on this plane, which we can do by just highlighting it, hitting Sketch in this upper toolbar over here, and then Sketch again, now we're sketching on this plane. And we're actually just going to create a little triangle here that references all of these points that we made before. And then, we're just going to extrude that away or cut it away. 

Let's just go create lines are here, zoom in a little bit so this is clearer. Start at the vertex down here, you can see I'm drawing a line. I'm going to bring it to this point, bring it to this point, and make it closed. And you'll see that all of the lines are black. And we didn't even need to add in any dimensions. That's because we've already defined those dimensions in a previous sketch. And now, we're referencing those geometries. 

We hit Green Check, Insert Line, Green Check. Now that's completely defined. We'll exit this sketch. And we're going to cut that little triangle that we made away, and down the arrow or I guess in this orientation, down the direction of our support. Cool. 

I'm just going to go here. Now, we're not going to Extrude Boss/Base. We're not going to create material. We want to cut material away. A few options over, there's this option to Extrude Cut. Let's hit that. And you'll notice now, that SolidWorks is going to take material away from this triangle that we've defined. Let's go and let's just click this surface. No. And you can select the option Through All in this drop down. All that does is it will extrude this forever. Our part doesn't exist forever. It only exists for a couple of inches. It will take everything that we need off. 

That's typically a pretty easy way to do cuts. You just kind of cut all of that material away. Whereas in extrusions, you want to define how much material you want to create. We'll hit our green check mark. 

And all of that material goes away. And now, we're left with this smooth face. We don't really need this sketch anymore, so we go back and hide it, which we can just do again by right clicking and now hitting the Hide button. And it has disappeared. 

I guess we can label this cut by just saying Front Face Cut, hitting Enter. We'll just make it a little bit clearer. Cool. We're getting there. We just have a couple of things left to do. 

What we're going to now do is add. You'll notice that there is a rectangular cut in here. It's what the phone actually slides into. And then I just made a little cut here so that you can access the Home button of this particular phone while it's sitting in the dock. Let's add those two features in. And we'll add a couple of finishing details and we'll be done. This is, you might think, well, how are we going to sketch on this? We don't want to sketch on this face. We can just sketch on this face. We're going to hit Normal to. And now we have access to sketching on this face. And we're looking down it. 

It's kind of the same process here. There's kind of this rhythm where we select a face that we're going to sketch on. We look at it at the normal, so that we're looking down on it. And then, we create some sketch. And then, we do something with that sketch. Maybe we make a cut or we create some material with Extrude Boss/Base. 

Same thing again here as we've done the previous two iterations. We're looking down on it. We want to select it as a sketch surface. It's highlighted in blue. So again, we hit Sketch, Sketch just as we've done before. And now we've created our sketch and we'll make that cut. One thing that we need to be aware of though, and this will come into play in just little bit, is that the corners of our phone are rounded. If we just make this kind of a prismatic cut, the phone will still fit inside, but it might kind of wiggle around. It might not be as secure. 

We can add little complements in here to complement the rounded corners of our phone. It's kind of a small detail. And it won't make too much a difference, but it's nice to kind of design the part in its entirety. 

Let's go here. We're going to just draw a rectangle on our surface here. And cool. Now let's define it. We're going to go to Smart Dimension here. Let's define it to be the width of our phone, which I've already forgotten. I'm just measuring it here-- 2.305 inches. 

And we're going to kind of add a little comfort zone to that so that you can easily take the phone in and out of the dock without having to kind of pull them apart. That would be kind of what we call that is that they're interfering. And we don't want that here. We want it to be easy to take it in and out. 

We said 2.305 inches is the width. And then, we'll add kind of a comfort spacing or a buffer spacing on each side. So let's say two times some thickness. What is that thickness going to be? We can just kind of guess arbitrarily here at some thickness. If you have calipers with you, you can maybe open them up to say, I don't know, 25 thou. 25 thou is 25 thousandths of an inch or 25 times 0.001. I'm just kind of guessing here, but I think that'll be enough spacing. We'll do that on each side-- say 20 thou-- two times 0.020 inches. 

That is now the width that needs to be. And we'll define its height. This will be the thickness of our phone plus that same buffer. I think it was 0.303 inches, but I'm not sure. 0.303 inch is the thickness of the phone. 

Let's say 0.303 plus two times 0.020. | at 20 thousandths thick buffer on each side. And I just multiplied it by two because, there's a buffer inside, the front and the back and side and side. Hit Enter. Cool. 

Now you might be thinking, oh my gosh, why is this all blue when we have just defined the width and the height? That's because we haven't located it on this plane. We can do this pretty easily though. We don't need to add dimensions in because we want it to be centered. 

We don't need to add dimensions in to say this line should be so and so inches away from this line. We don't need to do that. We can have SolidWorks figure that out for us. And one way to do that-- and this is kind of I think one of the easier ways to do it-- is to add lines and then add relations to them. And these can be called construction geometries. A construction geometry is just a line that you don't plan on doing anything with as far as extrusions are concerned. You're not going to cut with it or you're not going to create material with it. You're just going to use it as a reference. That might sound kind of lofty. I'll nail that down here. We're still in Sketch mode. If we go the Line and hit this little arrow next to it, this drop down will come. And we have a Normal line option, which is what we've been using before, or a Center line, which will create a construction geometry. Let's hit that. And this will create a dashed line. 

Let's draw a line between this side and here like so. Zoom in and you can see that it's dashed. And then, let's do it again over here. If we make these two lines equal, our smaller rectangle will be centered at least horizontally inside the bigger rectangle. They don't need to necessarily be co-linear, meaning that they don't need to be on the same line. But they do necessarily need to be perpendicular to both of these faces. 

Let's hit OK and let's start adding relations. SolidWorks is smart enough to know that just by the way I drew it they are both horizontal, as you can see by these horizontal lines here-- this little green box. So we don't even need to do anything with that. All we need to do now is equate them. And SolidWorks will now center the box. 

We highlight one, go over here and highlight the other-- again, holding down Control and clicking on it. And say, make them equal. And like that, SolidWorks has centered the box. Again, I'm just zooming out by rolling on the jog wheel on the mouse. And we could, if we wanted to, pan around by again holding down on the jog wheel. Let's do the same process to center it vertically. I'm just going to go down here. I'll go a little bit faster this time, create this vertical line, create another vertical line. Again, I'm double clicking to get out of Line mode. And then, we hit our green arrow now. 

And let's equate them-- click one, Control click, highlight the other, and then Make Equal. Now everything's black, and we're going to go. Exit the Sketch, kind of the same thing. Now we're going to make an extruded cut down here. And it's up to us now how thick we want to make that cut. 

This doesn't so much matter. It's kind of up to us. I'll say just based on the geometry maybe it'll be double what it is right now. Right now, it's at 0.15 inches thick. If we make it 0.3 inches thick, that looks pretty good. We can probably go a little bit deeper-- maybe 0.40 inches thick. Yeah. That looks good. Hit the green arrow. And now we have this slot that the phone will sit in. 

Now, we need to add kind of this little cut out for the Home button. I guess this is not completely necessary if you don't need to use your phone while it's in the dock. But it's a nice feature to have. And it takes little effort on our end, so we may as well add it in. Same thing. Let's highlight this face, go Normal to it. And we're just going to sketch on this face and we'll be done. Again, his Sketch, Sketch. Now, we're going to draw a circle. We can just kind of go up here into our shapes menu and click Circle. And let's just draw a circle kind of in the middle of nowhere. And we'll start to add relations to it. 

We're going to create a vertical line that the center of the circle will be coincident with. And that way, our circle is centered on the phone. And when we slip the phone into the dock, the Home button will line up with the cut out for the Home button, because we know that the Home button on our phone is in the center of it. 

We're going to go here and create a center line. And I'm just going to find the midpoint of this bottom line. If I try to start a line on this bottom line, you'll notice that there is a little yellow button. And when we hover over that, this little icon pops up next our pencil. And that icon is aligned with a green dot in the middle of it. 

When you see that icon, that means that that's the center point of that line. So if we draw off of that, we click and draw upwards, we've just drawn a vertical line from that midpoint. I did that kind of quickly, so I'll just do it again. And let's say that I don't see that. It's not popping up for me. We can do it even a simpler way. 

We'll go to center line. And we'll draw. We have this line here. But it's not at the center point. It's not centered against here. So what we can do is, we can draw a point, which we go to our Shapes menu, see a Point, find the midpoint here. You see that it pops up when we get close to it-- drop point there, here. The one thing you may notice that's different about all the other shapes is the point thing is still highlighted, even after you click the green check mark. Just hit it again to unhighlight it. And that will make this point and the base of our line be coincident. It accomplishes the same task. 

Now we're going to take the center of our Home button, Control click our vertical line, highlight the both of them, and make them coincident. Now our Home button is centered. We can't move it left to right. We can only move it up and down. And we can change its diameter. 

How big should we make it? I don't know. Let's measure it. If we look on our phone here, we take our calipers, and we can measure the diameter of the Home button. And it's nice to give it kind of a little bit of wiggle room, so we'll make it a little bit bigger than it needs to be. 

That's because when your phone is sitting in the dock, if it were exactly the size of the Home button, you kind of have to stick your finger like perpendicularly in to be able to access the Home button. Whereas, if we make it bigger, you can kind of hit it at an angle and see all the snapshots that you have missed. 

Let's go here and we'll measure on the phone. And I'm just eyeing it again here. That looks to be comfortable. it says 0.674. We'll make a round number. Let's say 0.65. Yeah. That seems comfortable. Some of this is kind of guesswork because we're not designing a really kind of nailed-down part. This part's not accomplishing any real task. It's just holding something. So it's OK to do a little bit of guesswork. 

Let's Smart Dimension this diameter. We just said it was going to be 0.65 inches. We go up in our menu up in the top left. Again, hit Smart Dimension. If you just click anywhere on the circle, it's smart enough to know that we're talking about the diameter. Whether you kind of drag it off to the side here and it gives you that little phi symbol or you hold it directly above, it's the same thing. You're defining its diameter. 

Let's click here and we're going to say 0.650. Hit Enter. And now, the diameter is defined. And what we need to do now is define the height from the bottom. This is probably the trickiest part of this whole operation. 

In doing so, we want the center of our circle to line up with the center of the Home button. Just by kind of eyeing it again with a pair of calipers, we can measure the distance between the center of our Home button at the bottom of the phone. Ideally, we would have a really detailed spec sheet of our phone and we could just look at the spec sheet and figure out oh, the center of this button is so and so inches from the bottom plane of the phone. 

But we don't have access to that, so we'll just measure it. And it'll be pretty accurate. I'm just kind of eyeing it here, the center of the Home button to the bottom of the phone. It looks to be about 0.329 inches, maybe a little bigger. Let's call it 0.348 inches. 

We now know that the bottom plane of our phone is 0.348 inches away from the center line. But the bottom plane of the phone is at some angle, so how are we going to figure this out? I don't know. Let's go to our Cut Extrusion here, which I notice now that I did not label, so we can do that now. We'll call this Phone Slots. And there are a couple different ways that we can do this. We can say, we can Smart Dimension it in a couple of different ways. By this angle-- and this gets into of this is a little bit more tricky-- let's look at it at an angle where we have access visually to the plane where the phone is going to be sitting on and our Home button. 

We go into Smart Dimension, and I'm going to dimension from this line to the center of our hole here, which gets highlighted. And now, I don't even remember what the number. I'm just going to quickly remeasure it. I think it was 0.348. Yeah, 0.348 sounds good. Now we'll add that 0.348 in-- 0.348. Hit Enter. And our phone is defined. Our button is defined. Hit the check mark. 

And here's kind of a subtle point that would be kind of easy to miss. You'll notice that the center of our circle actually sits below this line. That means that if we extrude through the sides where the Home button cut out is made, we'll actually start to curve back up. We can just eliminate that by drawing kind of a rectangle above the phone. 

If we go to our square thing here. And we go to this point, just kind of draw a rectangle randomly in the sky, and then make the other edge of it be-- I'll just click over here-- make this point be coincident with the circle. Now when we extrude, we can extrude the circle. And by extrude, I mean extrude cut-- extrude cut the circle and this little sliver in here. That might be a subtle point. And in our case, it wouldn't make a huge difference. But it's nice to add all these finishing details in it. It distinguishes kind of a quickly, hastily made product and one that had a lot of thought into it. 

We'll click our green check mark here. And we're good to go. You'll notice that this is blue. This is kind of an exception. We don't really need to define it here, because it doesn't matter how tall our rectangle is. It will still accomplish the same task. 

This is pretty rare that you don't need to define something in a sketch. In 99.9% of cases, you need the whole sketch to be black like I had mentioned before. In this case, it doesn't matter. We'll exit the sketch, again go to Features, kind of this common theme here, find the plane, Sketch, Extrude. And we'll go to Extrude Cut. 

And now, SolidWorks prompts us to pick what we want to cut. Let's select these bottom pieces. And now, let's get these little slivers. We'll do it on the other side too. Again, just zooming by scrolling on the mouse. Now we have everything we need. 

We don't want to do Blind. I guess we could do Blind, but it doesn't really accomplish what we want. Let's do Up To Next, and that will only cut through the first layer of material. When we say we want to cut up to next, that's meaning we want to cut everything up to the next face. 

Well, the next face is the layer behind here. We don't want this Home cut to go all the way through. You don't need it to go all the way through. There's no Home button on the back of the phone. If we just hit the green check here, now we have the phone cut out. Now we can start to add in the finishing details, because we're almost done. I mentioned before that we can add in fillets, which make everything look a little bit nicer. These are super easy to do. This is probably the easiest part of this whole CADing process. 

In our Feature Tree up here, in this kind of tab pane, we go to Features where we were hitting Extrude Boss/Base and Extrude Cut before. A couple of options over, we have this option to Fillet something. Let's click on that. All Fillet wants is an edge. You can give it a face, and it'll figure it out. But it really is looking for edges to which it can add a fillet. 

I'd mentioned before that we want to add a fillet to the back here. If we just click on this edge, it sketches out the fillet here, which is pretty cool. That required minimal work on our part. SolidWorks just defaults to some arbitrary value for the radius of this fillet. It looks good. We can make it a little bit bigger. I just think it's aesthetically more pleasing. 

This is when it becomes kind of less scientific and more aesthetic. The radius here is set to 0.10 inches. We could probably set it to I don't know 0.15 maybe. That makes it a little bit bigger. That looks nicer, I think. This is up to you. This is kind of customization. So we hit the check mark there. It adds in the fillet. Looking good. Now let's fillet this back edge here. And what this is doing is that first fillet that I added in was this one right here. We can also add in a fillet to smooth this edge down. 

Let's select again Fillet and this back edge here. And it does the same thing. It's again defaulting to 0.15 inches, because that's what I'd entered last time. That seems a little excessive here-- maybe 0.075, half that. That looks a little bit nicer. Again, this is totally up to the designer. 

That looks a little better. Maybe we can actually make that a little bit larger. I'm going to show you now how to make an existing fillet larger. And this is kind of a theme in SolidWorks where when you've already made a feature, you can change it pretty easily, pretty painlessly. 

Let's go through and label some things that we have not labeled. Cut Extrude 3, we don't know what that is, so we just click on it. And we see that it was the cut for our Home button. Let's just label that Home Button Hole. The fillets are kind of a tertiary feature, so to speak. Labeling them is not as crucial. 

But you're looking at this and you say oh my god, Ansel, my life is falling apart. What do I do about that? And I say you need to change the radius of this fillet. Let's click on it. And we're going to right click on it. And now, this option pops up. We have all of these options. We can hide it, suppress it. 

The top left option is this Edit Feature option. If we click on that, now we return to the Feature pane which we had access to before. And we can change everything. 

We had set it to 0.075 inches before. Let's now maybe bump that up a little bit. I think it will just look nicer-- 0.10. I accidentally added in a zero in the wrong place. That looks pretty good, maybe 0.120. I think that looks pretty nice. This part is effectively done. It will do everything that we want it to. It will hold the phone. It looks good. Yeah, it has a spot for the Home button. This is pretty much what we wanted to accomplish. 

Some things that we can think about are we need to be sure that the center of the phone, the center mass of the phone, if looking vertically will hover over this base and not kind of beyond it. As I had mentioned before, if that's the case, the phone will fall over. I just kind of eyed it. It might not hurt to just sketch it out on paper using pretty simple geometry. It's a super simple problem. 

I chose in this specific example to add the letters CS50 in the front. You're welcome to add whatever you want on the front. But one thing that I will caution you with is that some 3D printers don't have infinitely granular resolution. 

And by that I mean that if you write really small text with a really small font, it's going to look really kind of cloudy or blotchy. If you make a really big text, the letters are really large, and it doesn't require a whole lot of resolution on the 3D printer side, so it'll just look way better. So if you're printing in text into something, definitely make it as large as possible. 

I'll just briefly show you how to do that. If we highlight this face here, you'll notice that we can, we'll sketch on it again. Let's look Normal to it. Hit Sketch, Sketch again. Instead of drawing a line or a circle, there is this big A here. Some people call me Big A. 

We can hit that. And now we have the option to add text on to something. Let's type in CS. You might be able to fit CS50 all on one side. It certainly wouldn't be symmetric. I don't think it would be aesthetically appealing. So I did CS on one side and 50 on the other. That was just a decision that seemed to work at the time. 

We will hit the green arrow. Now we'll notice that these letters are blue. And that's because they are just floating around in space. They are kind of free to move wherever. What we want to do is, I'm actually going to delete them by right clicking, just hitting Cancel. I'm sorry, right clicking when you're not in a feature. And then hit Delete. 

We can do a nicer job in defining them. When you write text, and text is kind of something that's a little bit weaker, you want to create a line that the text will sit on, and then define the text to be kind of adhering to that line. We do that by just drawing a center line. 

Make sure that it is horizontal here. Double click to get out of drawing the line. And then hit the green arrow. This line is just floating around here. We have freedom to move it. Let's not define it just yet. Let's add the text in before we set where it lives. 

Again, we'll go to this big A here. We'll hit CS. And then, it defaulted to this Line 1 as where it will live on. But if that didn't exist, we'll just delete this. You can kind of select the line by just clicking on it. And SolidWorks knows that you mean to put the text on the line with the green arrow. Cool. 

Now the text is really small so we can actually just double click on it and edit the font. And we do that. It defaults using the document font, which we don't want to use, so we uncheck that. And now, this font box becomes un-grayed out. It's at 12 point right now. Let's maybe bump it up to like 48. That looks pretty good. And you can hit the green arrow. 

And by moving where the line begins around, you can move the text around. For example, you should be able to-- I'm just going to zoom in a little bit, select this point. You should be able to move that. And you can see that the text moves with it. 

You can do this, put the text wherever you want. You can define it by fixing this point, like so. And then, now our baseline becomes blacked out, Exit that. The sketch still exists. You can go into the sketch like I did before and extrude it. We don't want it to go all the way through. We only want it to go maybe, I don't know, 0.05 inches in. You don't want it to go all the way through, just because it won't look nice. Hit the green check. And now CS50 or the CS part of CS50 is in there. Cool. Then you can do 50 on the other side. 

That's your total freedom as to what you want to do there. You'll notice that I just suppressed it in the Feature Tree. If you have a feature that's kind of causing problems with dimensions or something is awry, you can suppress it. And it will kind of get rid of that feature and everything that's referencing it or everything associated with it. Just kind of a side note. Let's save this part, which I should have done a long time ago in case my computer crashed. We can just go to File, Save As. I'll just save it on my desktop. We'll call this iPhone Dock. And it saves is a part. 

Once that you have created a part, we encourage you to use 3D printing as a means by which you're able to manufacture it. If you're interested in more sophisticated methods of manufacture, do look into ES51, which is Computer Aided Machine Design, because that's kind of a more exhaustive course long, semester long introduction to more sophisticated manufacture methods, like using a mill to make it out of metal. But we're not as concerned about that right now. This is a pretty simple part. And it's going to be plenty strong by 3D printing it. 

Now, before it can be given to the 3D printer, we need to do a little bit of handiwork that makes it in a file format that the 3D printer will play with. We can do that by using MakerBot's own software, and just import this and then create it into a dot MakerBot file. And we do that by exporting this as a dot STL file. 

If we go over here, we can hit File, Save As. The default is to save it as SolidWorks' own extension, which for [INAUDIBLE] is dot-- I don't even know-- SLDPRT. We don't want that. If we had this drop down, we can change the format to STL. And we'll say again, we'll save it on the desktop. 

Let's go-- I'm actually just going to save in my Dropbox so that I can easily access it in my Mac partition on my computer. But you're welcome to do whatever-- iPhone Doc. We'll hit Save. It'll give us this little prompt box. It's like, do you want to save it as an STL? And you're like, hell, yeah, so you hit Yes. 

Then I'm going to just jump over to Mac here and go into my Dropbox. I'm going to [INAUDIBLE] my CSP set up that I'm diligently working on, go to Dropbox, and I should see it here. Cool-- iphonedoc.stl. Just drag it on my desktop. 

I'm going to fire up the MakerBot software. And by doing so, I will just import the file that we just made in a dot STL format. And then from there, we'll create the dot MakerBot file format. It kind of gives you what the printing stage looks like. 

Let's just that are part file to it, which we do by saying Add File, kind of in the upper-right menu over here, Add File. I'm going to put it on my desktop-- iPhone Doc. Hit Open. Do you want to put the object on the platform? Yes, I do. So it says, I say move to platform. This is in a really weird configuration. We don't want it to print like this. It'll take forever and it will be really unstable. We want to print in a really stable configuration. And by that I mean, we want to have it print with kind of this face on the bottom. And then, start it from the bottom, work our way to the top. We'll do that by rotating this part 90 degrees. If we select the part, and you can know that it's selected because it's outlined in yellow, hit Turn here. A little menu will pop up. And I believe we want to turn it-- nope, that's not right-- turn it 90 degrees in I guess it's the x way. You can just play around until you get it right. Then hit Lay Flat, and that will bring it down to the bottom of the build platform. I don't need to rotate it. 

And now, we are actually ready to print. It was that simple. If you want to kind of in a more sophisticated setting, you can adjust some of the print parameters. Infill just means how much of what's being printed is actual filament and how much is air. 

For example, 100% infill mean that this is a completely solid part. Whereas 10% infill, which I guess is MakerBot's default, means that only 10% of this volume is going to be filament, and the remaining 90% will be air. And it's able to maintain most of the structural integrity by creating a honeycomb that MakerBot figures out on their own. They have an algorithm built into this program that takes care of that. We'll just leave all these settings. I'll say Save Settings. And now, we're going to Export Print File. Cool. And it's ready to go. It says it'll take about an hour and a half for it to print. You can probably a little bit of work done while it's printing. 

We can hit this Print Preview. It's just kind of a cool feature. And this allows us to get an idea of how it will print. 3D printing is done by kind of adding one layer on top of another. So if we see over on the left side of our window here, there it says Layer 83. 

There's a little slider that allows us to kind of scan through our part. If we scan through here, you can actually see the honeycomb that it prints. You can kind of see that's kind of hard to see here. It may be a little better if we look on top. MakerBot figured all that out on their own. They have an algorithm that took care of that. We didn't design that honeycomb in. That just makes it a more efficient print process. 

The high-level takeaways for this are you design the part, prepare it, in this case, where you can print on a MakerBot 3D printer, but you're welcome to use something of the like that is not MakerBot. Prepare it in their software, and then give it to the 3D printer on maybe the network or on a flash drive in the correct file format. And then from there, you have your part and you're ready to go. The way that you can do this, and you'll notice that I use kind of a lot of different software packages on here, I happen to have SolidWorks installed on my computer. But it's not a free product. Definitely if you're a member of the college, you might not want to go through the strain of it runs on Windows, kind of downloading Windows, having to get your hands on the software, which can be a pain. 

If you want to do something like this or pursue a mechanical component to your project, definitely utilize the computer workstations in the basement of Pierce Hall in G11 specifically, as they are open nearly around the clock. And they have all of the software that you need. They have SolidWorks and they are very powerful with fun large monitors, so it will make [INAUDIBLE] pretty easy for you. They're very quick. 

Once you're done with that, you can actually download the MakerBot software package on your own computer. It's free. And I believe they do have both Mac and Windows versions of it. And then from there, you're good to go. Utilize Pierce, SolidWorks, export it, MakerBot, print it. 

Try to add in relations as much as you can, so that you don't have to add redundant dimensions. That's important. It might not be a big player in a pretty simple part like this, but it's just kind of a good practice definitely. And if interested in doing this on kind of a more intricate level, a more granular level, definitely look into taking ES51. 

That about concludes it. I hope you have enjoyed listening to me. And if you have any questions, don't hesitate to shoot me an email. I believe that my email is attached to the invitation of this event in some way. Thank you.