>> ANSEL DUFF: All right, hi, everybody.
My name's Ansel.
I am, as you know, a senior in mechanical engineering in [INAUDIBLE].
Today, we're going to spend a little bit of time
reviewing how to design a part from scratch
and how to ensure that it will suit the needs of whatever its application may
be.
>> So today, we will first design this little lens support.
I have a couple of them printed out here.
And I have one actually attached to the mount that I just sat down right here.
And this just holds up a lens like so, mounts onto some
rails-- I don't have enough hands to hold this-- just like that.
So we'll go over how that was designed, and then
move on to another part, which is an iPhone
dock, which I've displayed here, in orange.
We'll go over how to CAD those, how they were designed,
how to take measurements, and how to ensure that this won't tip over,
for example, or this won't buckle under loads.
>> All right, so before we get started, I just
want to talk about some overarching design principles
when you're designing a part from scratch.
Much like when you're writing code, you want
to be very explicit in what you tell the computer.
You never want to leave anything ambiguous.
Luckily for us, in SolidWorks, when you sketch something,
all the lines are blue when you initially draw them,
and they become black once they're constrained in three dimensional space.
So if you have a sketch with some blue lines on it,
you know that you need to fix some of those things before you move on.
It's just like a sanity check before you make a picture out of a sketch.
>> So like I said, you want to be really explicit in how
the sketches are defined.
The way that it works is you start out with one point.
SolidWorks gives you an origin in three dimensional space.
And that point is fixed.
And it will always be there and will never move, ever, ever, ever.
So you base your whole sketch around this one point.
And then you relate every line to either the origin or another line
that's related to the origin.
So I know this sounds a little abstract right now, but once we get started,
it'll be a little bit clearer.
But just like I said, make sure that everything is black,
everything is completely defined, before we move on
and you won't run into problems later.
>> Another thing that I'm really big on is putting a lot of emphasis
on making sure that you design your part for scalability such that you can tweak
it later if a measurement is a little bit off with no negative consequences
or effects.
And the way do we do that is we add a lot of relations.
So for example, when we define this part, we have two parallel faces here.
Well, we told SolidWorks that they are parallel,
and you can draw two parallel lines, and SolidWorks
will snap your lines to a grid.
But unless you explicitly tell it that these lines need
to be parallel, maybe later on down the road when you try to extend the top
or maybe extend the base, if you hadn't added that relation in,
everything can become a mess.
>> So let's get started here.
And if at any point you have a question, please feel free to interrupt me.
It goes without saying.
But we'll get started.
So SolidWorks comes with tutorials that teach you the syntax of the GUI.
I think it would not be an efficient use of our time
to go over which buttons to click.
So I'll go very slowly today and walk through every step that I'm taking.
But just know that if you feel lost or confused,
there are tutorials that explain exactly what I'm doing here
but on a little bit of a lower level.
And I'm going to put a lot emphasis today
on adding relations to everything.
I'm going to go over that a lot.
You guys are going to get sick of it.
But it's super important.
And you'll see down the road that if we want to tweak a dimension,
it's really useful.
So we'll get started here.
We'll select new.
And we're going to design a part.
SolidWorks has three different types of files you can have.
There are parts, assemblies, and drawings.
Assemblies are just multiple parts with relations,
so the parts are related to each other in three dimensional space.
And then, a drawing is a document that you might send to a machine shop
or whatever to actually manufacture your part.
>> So we'll start with a part here and click OK.
Now, we have a blank canvas.
So we're going to start out with this.
And what we first are going to do, and this is true for every part,
is we need to create some sort of stock, some sort of material.
And then, once we have the material, we can extrude these web features.
I even wrote CS50 on the front of it, and then a hole in the bottom.
So first, let's start out.
We're going to select Sketch over here, and then Sketch again.
And SolidWorks prompts us with three different planes.
You can add planes later on down the road when you're designing your part.
But we're first going to have these three orthogonal planes.
And we will select top plane right now.
Oops.
That was not the top plane.
Just go back here and--
>> There's always this tree that is floating around here.
And this allows you to select features of your build or planes
or any relations.
And then, the part material.
So we're going to sketch on the top plane.
So we hit top.
And we are normal to it.
And then, here's our origin point.
So let's just make some sort of shape here.
We know that there is going to be a curve on the bottom
and a curve on the top.
So this is actually designed to fit onto this piece here.
This is actually a lens support that was given to us by our production team.
And it wasn't tall enough.
>> So the purpose of this part is actually to just extend this a little bit
by-- we'd chosen two inches, what we measured.
And it will just bolt on.
There's a hole that already existed in the bottom of this.
So we know that we want the width of our piece
to be the same as the width of the support.
And then, we want the radius on the bottom to be the same as the radius
here so that it fits nice and snugly.
And then, we'll add a hole on the bottom that we can bolt it onto it.
>> So we're just going to start out with the footprint of this feature, which
is just this base.
It's like a rectangle, but with curves on the top and bottom.
I don't know if I can make this stand up.
So to do that in SolidWorks, we could start out with a rectangle.
But that won't be exactly what we need because we
need a curved face on the top and bottom.
So I just selected line over here.
And now, when you see the pencil tool moving around now,
that means that we are ready to draw.
So we're going to start at the origin.
And we're going to draw vertically.
>> You'll notice that as the line becomes vertical, it'll snap to vertical.
And you see that this little yellow box right to the bottom right
of the pointer, that means that SolidWorks is automatically
adding a relation for you.
So that's the theme of today, what are the relations.
So when we click this, you'll notice that it's black
because SolidWorks knows that it's a vertical line
and it began at the origin.
But the endpoint is blue because we didn't tell SolidWorks
how long the line is.
So we're just going to make another one of these.
In fact, I'll even draw it purposefully off vertical
so that we can add the relation in.
>> You'll notice that it automatically wants
to add another line from the endpoint of the first line.
So if you just double click like I did here, we have another line.
If you just double click, it will cancel that.
So we can hit the green arrow.
I'm just going to delete this.
On most keyboards, there'll be a delete key.
But on a laptop keyboard, you have to hit the function key and then delete.
So we select it, and hit function, delete, and it goes away.
So we need to add the relation telling SolidWorks
that these lines are, in fact, parallel.
So I select one.
And then I'll hit the Control key, hold it down, and select the other.
And then this dialogue box pops up right near our cursor.
So we have a couple different options here.
>> We can make them both vertical, make them both horizontal, parallel.
In this case, making them parallel and making the vertical
will accomplish the same task.
But we can just hit parallel.
And then, we're going to add one more relation, which
is we're going to again hold down Control, select both, and tell
SolidWorks that they're the same length.
Cool.
So now, what I'm going to do is add what's called a center line.
>> So if we hit the line tool and the little arrow,
this drop down will pop up.
And we have the center line option.
You'll know that something is a center line because it's dashed.
It's not a solid line.
So let's draw one in.
And we need to tell SolidWorks that this is going to be horizontal.
Cool.
>> So this is just going to be the baseline upon which we will make sure
that these, like this one, isn't too high up.
So it seems to have already did that automatically.
But just to be safe, we'll make it explicit.
So if we select this point here, and then again, holding down Control,
select this line, we have the option of making them coincident.
So we'll select that.
Do that again one more time.
And now, we know that these lines are the same length.
They're parallel.
And they start on the same-- this will become a plane,
but it's a line for now.
>> AUDIENCE: So is it the second one you clicked
on that is made coincident with the first one, or is it--
>> ANSEL DUFF: So both lines have endpoints that are coincident with this line.
So since everything is really simple right now because it's orthogonal.
>> AUDIENCE: Is one always moved to the other?
ANSEL DUFF: Oh, OK.
Yeah, so it's the order that you click it.
So if I had clicked the point and then the line versus the line
and then the point, yeah.
But luckily, the origin is a fixed point in space.
So now, we need to define their length, which
we can do by clicking this smart dimension in the upper left.
And then, select something that we want to dimension.
So this is probably one of the most important things in design,
dimension all of your pieces.
This is how you tell the program how tall it's
going to be, what the radius is for the top and bottom curved faces, the depth,
and so on and so forth.
And that's all done through the smart dimension tool.
>> So if we click on the line, this little arrow pops up.
And this can tell us once we click, we get a prompt wherein
we can type that we want this part to be 2 inches tall.
We had measured, and 2 inches seemed like it would be plenty of space.
So we hit 2.00.
2 is also fine.
Hit Enter.
And then, you'll notice that both lines are now 2 inches tall.
>> Now question, our first line is completely black.
It has two black endpoints and the line itself
is black because it's completely constrained
in this two dimensional plane.
But this line is blue.
Why is that the case?
Why is that line blue?
We've told SolidWorks that it's parallel to our original line.
AUDIENCE: How far it is from the original line.
ANSEL DUFF: Exactly, correct.
So here's where we need to measure.
We don't know how far this is going to be.
How wide is this supposed to be?
So we can hit Smart Dimension, then select the first line.
You'll notice that it's blue.
Then, select the second line.
And we get this width prompt.
So we can click it.
And SolidWorks now wants to know how wide the part is going to be.
But we don't know.
So we have to measure.
So we take our part, and we use a pair of calipers.
And we're going to just measure the width here.
>> So calipers are a really precise way of measuring any dimension, really.
They have two measuring prongs, I guess.
There's one on the bottom that can measure externally.
So you'll clamp down on something.
And then, there are two prongs on top that can measure internally,
like the diameter of a hole, for example.
So calipers are typically good to about a thousandth of an inch,
meaning that each tick on the front face here
represents one thousandth of an inch.
Typically, engineers will speak saying thou.
It's slang, almost.
Saying a part is 80 thou thick.
It's like, this is 80 thousandths of an inch, just
some lingo to cue you guys in on.
>> So since they're so precise, the first tool,
or the first step when using calipers, is you open the prongs up.
And then you wipe them to eliminate any gunk that
will change your measurements.
And then, we close them.
And we ensure that it is zero.
I'm not sure if you can see all that well,
but once they're closed, the needle lines up with zero pretty well.
So we don't need to adjust anything.
So now, we open them up.
We're going to clamp down.
And I'll try my best to hold it up here.
>> There are inch indications on the actual stem
of the caliper, every tenth of an inch.
And then, there are hundred ticks, thousand, so 1/10 of an inch
all around.
So we clamp down here.
And we see that it's just past the one inch mark.
And it goes to four ticks past.
So one inch plus 4/1000 is 1.004 inches.
I suspect that whoever designed this part designed it to be one inch,
and then the anodizing added two thou on each side,
so 1.004 inches is our measurement.
>> AUDIENCE: How important was the vertical height measurement
that you originally talked about?
ANSEL DUFF: This is kind of the specificity of this part itself.
But you'll notice that there's a bolt holding this in.
Two inches was more than enough when we were
talking about how tall this part should be.
It only really needs to be about an inch.
We just held a tape measure up and eyed it.
So we added another inch just for safety.
And if it is too long, this can slide down and accommodate that extra height.
So two inches was not measured that accurately.
We just kind of eyed it knowing that it could be adjusted and accommodated for.
So we'll enter in 1.004, hit Enter.
>> Cool, now both lines are black.
We're good to go.
So now, we need to put in an arc here and an arc here.
Spoiler alert, this is just kind of another specificity of this part.
They are the same radius because it's just an extender.
So if you had made the top radius and the bottom radius different,
you might be able to accommodate a larger lens.
But that wasn't our goal here.
So we have no idea how big this radius was.
But we knew the lens that it was trying to accommodate.
So much like we had just measured the width using our calipers,
we will do the same thing, if I can get them, for our lens here.
>> So I'm just going to open them up wide here, fit them around the lens,
don't press too much because it's rubber.
We don't want to deflect it.
And we see this 3.465 is the width.
So that 3.465 is going to be the diameter
that we are going to make these radii.
We're going to go over here and select the arc tool in our shape plane.
Hit the drop down, you'll notice there are a couple different types of arcs.
We're going to use center point arc, which
is us defining the center point and then two endpoints.
>> But as you can see, there's also a tangent
and three point arc option available.
So let's go here and just hit a center point arbitrarily.
And then, let's draw it here.
And I'm going to purposely go past what we need.
So everything is blue here, and that's because we
need to somehow make this point be completely
between these two and some specified distance away.
So let's add in another center line.
Just going to draw it vertically.
SolidWorks again snaps to vertical.
If you're ever wondering if in fact this is vertical, if you select it here,
you'll get all the relations on a line listed in this box.
>> So we see vertical, too.
That's telling us that the line is in fact vertical.
I have the option turned off right now to show relations.
Relations are shown by this little green box with some symbol.
In this case, it's a vertical line.
They can get kind of cluttered, especially when
you have a lot of features happening in your drawing.
So I just to turn them off.
But if ever you need to know the relations on a line, an arc,
a point, what have you, just select it, and then there's a list here.
>> So vertical was done by SolidWorks.
We added in the parallel to the second line.
Equal radius, equal length was just us telling
SolidWorks these are both the same length.
And then the distance was specified by this one inch.
Cool.
So we will add in the center line, can extend it down.
And then, we need to tell SolidWorks that it
is equidistant between these two.
So I'm going to add in another center line here.
>> And you'll notice that it's coincident on both of these.
But we have no way yet of saying that this line needs
to hit the midpoint of this line.
So we can add in a point.
We go over here and select Point.
Looks like a little asterisk.
Then, as we move it along this line, you'll
notice that there is that yellow box in the middle of it.
And when we hover over the box, the symbol
goes from those three lines in this little yellow box to just two lines.
And that's SolidWorks's way of saying, this is the midpoint.
So we make a line there, make a dot, rather.
And in our relations box, it says midpoint.
So we know that's in the middle.
And then, hit the green check.
Undo the point box, because it'll just continue drawing points every time you
click, which we don't want.
So this point is already selected.
Now, we're going to make this point and this line coincident.
So hold down Control.
Select this.
Select coincident.
And you're good to go.
Sometimes, I'm just going to undo that.
Sometimes, when you have these two selected,
that little box doesn't pop up.
You can always just pop over to this left plane,
or left pane, rather, and then hit coincident,
and it'll have the same end result.
Cool.
>> So center lines are black if they're partially defined.
The end points in this are blue because we haven't defined its length.
But we don't need to.
It's not really relevant.
So now, we're going to put the center point of our arc on this line.
So we've selected it.
Again, hit Control.
Select the line.
Make it coincident.
Now, we know that this arc is going to be symmetric to the lines.
And now, we're going to make the endpoint of our arc
and the endpoint of our line coincident.
So I just was holding down Control, selected both of those,
and I hit merge in the left pane.
And now, we have a completely symmetric arc on the bottom.
>> So we need to have another one up top.
I'm going to highlight this just by clicking on it.
And then hit Command C, and then move the mouse away, Command V.
And now we have another one.
So again, we need to add all of our relations just to mirror this up top.
And select it, or select this center point.
Hit Control, select this line, make them coincident, cool.
I want to just move through this.
All I'm doing now is I'm just going to merge all the endpoints.
And then one last time.
Cool, so now we have two arcs.
>> But we need to tell SolidWorks that they are of the same radius.
So we'll select them both and say equal.
Cool.
And now, we will finally define their radius.
So I believe we said-- I don't remember what the number was.
I think it was .
3.465.
Yeah 3.465 was our diameter.
But you'll notice that we're defining the radius.
So what we're going to do is say 3.465 divided by 2.
The dimension box can understand algebraic expressions.
You can use parentheses, multiplication, division, et cetera, et cetera.
So that's all we're doing here because we
need to divide the diameter by 2 to get the radius.
Hit Enter.
We're fully defined, we'll notice that everything
is black except for this center line.
That is fine, doesn't need to be.
So now we have our footprint.
We have the platform that we will extrude to make the solid.
Then, once we have the solid, we can add all the other features.
The hole in the bottom, this webbing to save a little bit of material, and then
this bridge in the middle that says CS50.
>> So we're going to exit this sketch, and we're going to extrude it.
SolidWorks is based on sketches and features.
Once you've created a sketch and everything is completely defined,
you can exit the sketch and make a feature out of it.
In this case, we're going to extrude, we're
going to create material from the sketch.
But when we do the hole, you'll see that we create a sketch for the whole
and then make an extruded cut from the hole.
So if we go over from the top left and hit Exit Sketch,
we go to features pane, only most everything is grayed out.
But we do have the option to extrude boss base, which
is what we're going to select.
>> Once we hit this, you'll notice that the solid actually comes out.
SolidWorks has some default, maybe a tenth of an inch,
but we'll define the height.
So we hit extrude boss base.
Now, you'll notice that it's a solid.
And we need to define the depth, this d1 over here.
So again, we're going to measure the height using our part here.
We want the height to be the same height as the arm
here that the part came on so that it looks clean and does overhang.
There's no need for it.
>> So again, with our calipers, we just measure here.
This is pretty similar to what we did before and wiggle it
around a little bit, make sure you have nice, firm grasp.
This is made out of aluminum, so it's not going to deflect at all.
And we see that it is 0.751.
Awesome.
So we'll just type in 0.75.
And now, we have our solid.
So this is what will become the lens support itself.
We have a couple more features to add in.
>> So before, we were sketching on the top plane.
But now, we can sketch on any plane of the solid.
Or we could create our own plane using what's
called reference geometry, which is not necessary right now,
but could be later.
So let's just select this plane.
And then we're going to hit-- you'll notice that this little box pops up
when you move the mouse around.
If you lose it, it's always available on the top here.
There's this web of a box with a little arrow beside it.
You'll notice that there is a plane with an arrow coming out of it.
If you click this, this will make the view that you're looking at,
the computer's view, normal to the plane you've selected.
>> So we hit that.
And we have the plane that we're going to sketch on.
So if we go over to the sketch box over here we hit sketch,
SolidWorks is going to say, I don't know which plane to sketch on.
Which one did you intend?
And it won't even let you sketch anything.
It won't let you do anything.
That's why there's this error message.
So we hit the x.
We need to select the plane first and then hit sketch.
Now, we're going to go.
It didn't give us any errors or warnings.
So all we're going to do in this case is really just to find some webbing.
And then, I made a little bridge to say CS50.
We can keep that in there.
So one neat little feature that we can do
is we can unhide the sketch that we made for the footprint
and use all those geometries in this sketch.
So in our feature tree, we have this boss extrude one.
And then, I hit the little plus arrow underneath it.
And sketch two pops up.
So we can-- it's always a good idea to label things,
just like when you're writing code.
You want to appropriately label your variables
so that it's clear how you're using them.
It's the same case in SolidWorks where you
want to label all your features so that you know exactly what they do.
>> So if you select a feature and then hold your mouse down over it,
it prompts you to rename something.
So we'll call this base.
And then, same thing here, we'll just call this sketch base.
So by default, once you've exited a sketch, it becomes hidden.
But you can change this just by hitting this.
And then, this little box will pop up with a pair of glasses.
And you hit show, and now we have everything back.
You can see that there are endpoints here.
Cool.
>> So now, what we can do is we will sketch-- we can just hit line here
or even I'm going to just select all these entities, again,
by holding down Control.
And I'm going to go up here to offset entities.
So we want to add some wall thickness.
And that can be done by just taking the base footprint,
and then offsetting entities on the inside.
>> So then, we'll specify the depth.
So SolidWorks, by default, goes for the outside, apparently.
You could see this yellow line around the base of our feature.
So if we just hit reverse, now it becomes inside, which is cool.
A tenth of an inch sounds fine.
We hit the green arrow.
And we have our dimension down here.
Now typically, if we're defining this part to be like a load bearing part,
I guess technically it is varying the load of the lens.
But the plastic that we're using to print these
is actually pretty strong, so we're just going to guess on the wall thickness.
A tenth of an inch is plenty, probably a third of that is really required,
but we'll just add a little bit more for rigidity.
>> If we were designing it to be a part on, say, a race car,
we would run it through a computer simulation called Finite Element
Analysis, FEA, wherein the computer meshes up our part into arbitrarily
many little mesh segments.
And then, we subject it to loads and fixtures like saying,
don't let the base move, but subject the top curved face to a load of 150
Newtons normal to it.
Or I guess it's a curved face, it can't be normal to it.
But downward, and then it will tell you when the part will fail
and which areas of the part are under the most stress.
It's overkill right now.
But we'll just eye it, a tenth of an inch is plenty.
>> Cool, so now we have all this.
And we're going to add in another centerline to bisect this part here.
Just the same procedure as before.
I'm going to start to go a little bit faster
because this is becoming a little repetitive.
We'll add a point.
That is the midpoint here.
In fact, this is even unnecessary.
>> We can just draw the centerline from the midpoint.
So we find it.
That yellow box pops up.
So we hover over it.
Draw it across again.
Now, we have this line is bisecting this line.
This vertical line here.
>> So again, we can offset entities.
We want to.
We're going to create the bridge on which we will later extrude cut, CS50.
We want to add some thickness to it.
So we hit offset entities, and by default, it adds a line on one side.
But if we just hit bidirectional, there's a little check box down here,
it adds two.
And let's make this a little bit thicker.
So say 0.15, maybe even a little bit more than that.
So this is 0.2 inches on each side, so 0.4 inches in total.
Can move the dimensions out of the way so that we don't clutter the drawing.
That looks good.
>> Typically, when you're dimensioning a part,
there are seemingly infinitely many ways to display all the dimensions
on your sketch.
In the interest of not cluttering it, it's nice to move your dimensions away.
And there are other rules that kind of follow,
like you don't want them to crisscross or overlap,
because it becomes ambiguous.
But this is good for now.
So hit the green arrow.
Now, we want to add in this webbing, which
we're going to do in the same way with offset entities.
>> So we hit center line.
And I'm just going to draw two x's in here on the top and bottom.
Here is one.
do the same thing on the bottom.
And you'll notice that all of these lines
are black because all of the points, all their endpoints,
are completely defined.
So that's cool.
We don't need to add any more relations.
And let's select them and hit offset entities again.
And that ought to do it.
You can only do one at a time, which is fine.
Offset entities, whoa, that looks crazy.
I accidentally selected more than one thing.
Offset entities, that's weird.
Don't know why it's doing that.
Hm, didn't expect that.
That's fine.
We will just do it by hand.
>> So we will add in-- I'm just going to draw in some lines
here that we will add relations to in a bit.
So we want these lines to be parallel to this line.
So we just hit make parallel.
Then likewise, on the other side, cool.
And we'll just make the endpoints match.
>> AUDIENCE: All of these varied thicknesses,
is this just experience and insight?
Or is there math that's behind the choice
of these thicknesses for the structural integrity?
>> ANSEL DUFF: Yeah, so right now, I'm just kind of going off of instinct
and eyeing it, guessing.
We had made a version zero prototype.
It's around here, and clear.
And I had guessed a tenth of an inch, and I
had the idea to just print one, a dummy, try it out.
Maybe modify a couple of the dimensions, and then go for the actual part.
But a tenth of an inch was fine.
If we wanted to be really a bit more thorough, what we could do
is we could calculate the axial stress under which it's
placed from the weight of a lens.
>> A great engineering practice and one that is upheld universally
is to design in a safety factor.
So let's say this lens weighs three pounds.
I just made that up.
But if we weighted this lens, and it weighs three pounds,
and you design your part to be able to sustain three pounds,
but buckle after that, then that's not really great practice
because there's going to be impulse when you pick the camera up.
This will experience greater than three pounds.
So you always want to design your part for greater
than it will actually ever experience.
So typically, a safety factor of two is fine for something like this.
But honestly, at a 1/10 of an inch wall thickness,
this probably has a safety factor of like 15.
So right now, we're just going off of instinct.
>> But if we were to do it out of a material that's
a little bit easier to work with, like aluminum or steel,
we could calculate the stress and then compare that
to that material's yield stress or ultimate stress.
AUDIENCE: Does this kind of plastic such numbers associated with it?
Or is it [INAUDIBLE]?
ANSEL DUFF: No, it does.
So what we're using out of our 3D printer
is PLA filament, which is like a bioplastic.
And although I haven't personally looked these up,
I know there are figures available for yield stress and yield
sheer associated with this plastic.
We did not design for that because it's actually hollowed out.
The MakerBot software processes honeycomb, and it adds it in.
So it's not completely solid.
So those calculations would be faulty.
They would not be accurate, unless we made this completely solid.
But it would take days to print in that case.
So just in the interest of time, we let the hollowing happen and test.
>> So now, we're just going to tell SolidWorks
that these are the same distance away.
So there are two ways of doing this.
One way is to go to Smart Dimension and dimension both of these lines
and to make them the same number.
That's not a great practice because down the road,
if we find that this webbing is too thin, we would have to go
and change eight dimensions just for one fundamental property, right?
>> If we said that these webs are buckling, let's double their thickness,
you don't want to have to go in and modify eight dimensions.
It's like when you're writing code, if you're
going to be using the same number over and over
and over again, you define a constant at the beginning of the file,
and then use that constant throughout.
And then, when it's time to change it, you only have to change one number.
It's the same principle here.
So our constant is adding relations.
>> So we'll dimension it one time.
So we'll go Smart Dimension, we can go 0.05.
And I'm making this half of our 100 thou thickness
because there'll be two sides to it.
So we define it once, and then we add center lines to make the relations.
So we go here.
We make two.
And then, we're just going to make these equal length.
The dimension will be taken care of.
So highlight both, make them equal, and now this line is black.
So we'll do that again.
Just going to go a little bit faster.
>> You'll notice that when I'm hovering the mouse over the line, it becomes orange.
And then, I click.
You can be sure that the line is-- these two lines are coincident.
They meet at this end point because it was highlighted orange
when we selected it.
So make these parallel, likewise for this piece.
We're going to do the same thing with our center lines, zoom in a little bit.
Just select these.
Selected a face there, that's why it turned blue.
>> And I'm going to go back to the original and make them all equal.
So we dictated the length of this with this dimension, 0.05 inches.
And because we made these all equals, SolidWorks just figured the rest out.
I'm trying to think.
>> One option is we could take all these, in fact,
we probably didn't even need this x.
And we could mirror them.
You could manually redraw them.
But it's a bit redundant because the features are the same.
So what we will do is-- actually won't be
able to mirror it because these are not mirror images.
Whoops.
>> So what I was thinking is this bulges out, and this bulges in.
So this is concave and this is convex.
If they were both convex or both concave,
you could highlight all of these, mirror them about the center line,
and then everything would be taken care of.
But if we were to do that, this line would
translate to being a convex line down here.
But we need it to be concave.
So that's no good.
We'll just draw it in by hand.
Adding in the cross of our center line.
Great.
Go back, select actual line, can zoom in.
>> In SolidWorks, you can just zoom by scrolling on your mouse.
And then, the middle click, so if you have a mouse with a jog wheel,
if you hold down that jog wheel, that will
allow you to change your view orientation.
Some mice, like mine here, they do not come with jog wheels.
It's a touch pad on top effectively.
So I've configured my mouse using a program called Magic Press, which
is a free Mac preference program to be able to just hold
two fingers down onto it and move the part around for view.
So if you're using a Mac and running a Windows virtual machine like I am,
I've seen a lot of people with the same Magic Mouse,
I would recommend Magic Press.
It's free.
So you can make these parallel.
Oops.
Not what I want.
>> So sometimes, when you're working at an obscure angle,
it can be kind of hard to see the relation.
So we're just going to select this little box here and then go back
to the normal.
And that'll make everything a lot easier to look at.
So sometimes, the part will be really far away.
If you want to zoom in and have it fit your screen if you just
hit F on your keyboard, that zooms in.
You can see it's kind of far away because these center lines are
a bit longer than they need to be.
But if we just shorten these down a bit, like so, and then hit F again,
now zoom in.
So we make these parallel.
Awesome.
Do likewise here.
>> And then, we'll add in those little support structures,
these center lines to dictate the depth or the thickness of these lines.
You'll notice that when I'm drawing, SolidWorks
creates that yellow dashed line.
That dashed line is normal or orthogonal to the line
that this line that we're drawing started on.
So if you follow that dashed yellow line,
you can be sure that it is in fact orthogonal.
We'll do it again.
>> Just for good measure, we can double check
once we're done sketching just by selecting a line,
and all the relations come up here, perpendicular, awesome.
We'll make these all equal length.
Select them all.
Then, we're going to go back to the original line that we dimensioned.
Select that, hit equal, and then we zoom out.
These lines are all black.
Cool.
>> So we are ready to exit our sketch and cut out these webs.
So we hit Exit Sketch notice that the sketch is still highlighted here
because we're going to do something with it.
Now, if I go to Features and I hit Extrude Cut, which is now an option,
it's going to freak out because it doesn't
know which sketch we're going to use as the base.
So leave that.
We can hide this.
We don't have any need for it.
>> So we select the sketch that we just made.
We can even label it.
We'll call it webbing, or just web sketch.
Now that it's highlighted, we can extrude
it, which is-- we don't want to create material.
We want to cut material away.
So we'll go and we'll use an extruded cut.
So now, there are a lot of geometries happening in our sketch.
>> We need to tell SolidWorks which pieces, which triangles and rectangles we
want to cut.
So if we go down here and we hit Selected Contours and highlight
this box, it becomes blue.
And then, you can click on different parts.
I'll just click on everything we want gone.
And it will cut everything away that is highlighted.
So there's the option now of how deep do we want to cut.
We could cut partially.
We don't have to cut all the way through.
We could do like 0.751 divided by 2.
This will cut halfway through.
You can see in the preview there.
But that's not what we want.
We want to go all the way through.
>> So this little dialogue box, we just click.
And select Up To Next, and that'll cut all the way through.
Hit the green arrow.
And our sketch is still highlighted, but if you click away,
now we have the webbing done.
So you'll notice if you look kind of closely at this part
that the corners are rounded off internally.
That's a feature called a fillet.
What a fillet does is it eliminates what are called stress concentrations.
If you have really sharp points at any place in your part,
whether it's made of some composite or steel or aluminum or what have you,
really sharp points can cause stress concentrations
when they're subjected to loads.
>> So if we were to really push this part, it
would likely break at one of these really sharp nodes.
So to combat that, we use what are called
fillets, which is just really gentle rounding in there.
So we go to this fillet feature.
We have a dialogue box.
I find it helpful to select this full preview option.
And all we have to do is just click on a line, and it creates a fillet for us.
So it defaulted to having the radius be a tenth of an inch.
That's a little extreme.
So we'll do maybe 20 thou.
That's a little small.
Split the difference, say.
Not split the difference.
Let's do 50 thou.
That looks good.
So now, we're just going to select all these other fillets.
Kind of just fly through this.
>> So once we complete the part, I'll go back and show you
how painless it is to modify a dimension.
Like I said, it's helpful to print out kind of a dummy version,
test it, see if it's strong enough.
Maybe you want to make the letters larger or something of the like.
Oops, I selected a face accidentally.
We don't want that.
Select this line, one more time.
That was the wrong one.
If it's hard for you to deselect that line,
you can go over to the box here that's listing everything, right click,
and then say delete.
Do not say Clear Selection because that'll delete every line,
unless that's what you want to do.
Cool, just one more to god.
Oh, missed a couple at the top.
All right.
>> AUDIENCE: There's more up top, the left triangle at the top and bottom.
>> ANSEL DUFF: Oh, god.
That is code red.
All right, now we have our fillets.
Now, it looks a little weird.
They look a little bit bigger than they need to be.
So if we want to adjust that, let's just label this web fillet.
We can right click on this, and this box pops up, and we hit Edit Feature.
And we just have to change one number.
Let's do maybe say 30 thou.
And they become smaller and get the green arrow.
So if we wanted to change all those features, there were a lot of them,
you just had to change one number.
And that's really helpful for us.
>> Something that I've not yet done is save my part, not a bad idea
during the middle of it.
We'll just hit Save As.
We'll call it lens support 2, since I've already made one.
And now, we want to just add in letters, and then we're ready to go.
>> So to do that, we're going to make ourselves normal to this plane again.
Now that it's selected, we can go and sketch on it.
And now, we're going to add letters in.
So part is actually upside down.
This probably wasn't a good face to sketch on.
I'm going to sketch on this one.
So sketch, SolidWorks has a letters feature.
But we need to orient the letters in space.
And that's done, again by making a center line.
In case you haven't noticed, that's kind of the theme,
to make center lines for anything you might need it for.
>> So for now, let's just add a Smart Dimension from this line.
We'll say 0.01 inches.
I'm just eyeing that.
We're going to go back and change that in a second.
But for now, it just constrains this line in space.
Cool.
So now, we go to our little font feature here.
It's that big A. So we just hit that.
That's A for Ansel.
So we type CS50.
Cool.
But we need to type the curve that it's going to sit on.
So just click on that line, awesome.
Now, it's a little bit small here.
We want to make it a little bit larger.
So by default, it uses the document font,
which is just defined in some property list somewhere.
>> So we'll deselect that, hit the font button,
and make this a little bit bigger.
I like to use this units option because it
allows you to specify the height in inches.
So I believe before we had made this bridge 0.4 of an inch high,
so perhaps making the letters 3/10 of an inch tall, it'll look big.
That's pretty good.
Get the green arrow.
Make this a little bit smaller.
Let's halve it, so we could go divide by 2.
And then, we'll just drag this dot over to where I think it looks good.
This is what we call a code orange.
The letters look a little bit too big.
So we're going to select them.
Go back to font, and let's make them a quarter of an inch tall instead
of 3/10.
Make them a little smaller, move them into position.
Cool.
That looks pretty good.
We'll add a couple, say, maybe bigger there.
>> SolidWorks is really interpretive in this dimension box.
I had mentioned before that you can use algebraic expressions.
But let's say we wanted to be in millimeters.
We could say make this 5 millimeters, and it will understand it.
So it'll automatically convert it to inches.
So 5 millimeters, SolidWorks tells us, is 0.19685039 inches.
So we'll go back to inches.
We'll say 0.07 inches.
My program is set up to default to inches.
Everything we do in the States is in inches.
But if you want to convert something, there's no need to go to Google
and convert it because SolidWorks will do it for you.
>> So this is just about centered.
If we really wanted to be very, very precise,
we could measure the width of the letters
and then center it against the center line of the piece.
But that's kind of overkill here.
We'll just visually center it for now.
That looks almost there.
We'll drag it over a little bit.
Sometimes, when you want to drag a point by a very small amount, if you
click on it and try to drag it a little bit, it won't do anything.
So it's nice to move it far away, and then come back close to where you were.
>> So hit F to bring us back out.
That looks pretty good.
We'll hit the green arrow.
Oh, wait a minute, somebody said in the back.
The sketch is still blue.
So what are we going to do?
You'll notice that we have put all the letters on this line.
But we haven't constrained them in this dimension, left to right.
So the way we do that, this is the point that we're
moving that dictates all letters, we will fix this point in space.
And it will not move.
So in our pane left here-- in fact, we'll
deselect it-- we click on this point.
This point dictates how the letters are placed left to right,
like I had mentioned.
>> Select this point.
We see all the relations over here, it's an empty box.
Nobody's home.
We hit fix.
Boom.
Oh my gosh.
What happened?
We have over defined the sketch.
So what this means is you have multiple relations,
multiple dimensions referring to the same entity.
So for example, if we had made two lines parallel,
and then we added a dimension up top to say that these lines are one inch
apart, then we add another dimension at the bottom to say these line are two
inches apart, SolidWorks is going to scream at us and give us the same
warning because you can't-- both dimensions are referring to the same
entity.
Somehow, we have done that here.
>> So we can let's just rebuild it.
If at any point you want to rebuild your sketch, or you change a dimension
and it didn't take, if you just hit this little stoplight at the top here next
to the mouse, hit that, SolidWorks will process it.
>> So this sketch has a little yield flag next to it,
which means something's wrong.
So if we right click and hit what's wrong,
we get a really unhelpful error message.
This sketch is over defined.
Consider deleting some-- so that didn't tell us anything new.
We'll go back to sketching it.
And what happened?
>> Oh, we can't fix it in space because it's already
defined to be 70 thou off of this line.
So if we just delete this and refix this point, it should be fixed in space.
So I know the letters are still blue, but they are fixed in space.
That I'm sure of.
So we'll just move on.
>> Now, we're going to cut these letters into the material.
If we wanted to, we could cut them all the way through.
But that might compromise our part structurally.
Not really, but it's not really great practice to add an aesthetic feature
or have an aesthetic feature be structurally compromising.
So we'll just cut them to be maybe 10 thou deep or 100 thou,
depending on how it looks.
So we highlight our sketch.
We'll label it because we're good people.
Computer froze for a second there.
We'll call this letters sketch.
And now, we will do an extruded cut.
And we can change how deep they go.
>> So right now, they are halfway through.
That seems a little much.
Let's do 200 thou.
That looks pretty did.
Hit the green arrow.
And we are cooking, ready to go.
So there are a lot of things that could be the next step in our manufacture.
We've completely designed a part.
We can build it in varying ways.
But what we first want to do is double check that all of our measurements
are right.
It's very painless to change the dimensions
when you're in this build state.
The part is completely defined, and you just
have to change maybe a number here or a number there.
But it's not that fun to build it and then measure it or try
to fit it and realize that you messed something up.
We're not actually going to manufacture this part right now because it
takes a very, very long time to print.
But we would go back and double measure everything.
Measure twice, cut once, and ensure that everything is correct.
Let's hypothetically say that we messed one of the measurements up.
>> Let's say that the webs are too thin.
They were buckling and we want to make them thicker.
It was kind of a pain to add in all those dimensions before, all
those relations, and make all those lines of equal length.
But now, if we want to make the webs thicker,
we can just go-- oops, forgot to label this guy.
We'll call this web cut.
And this is letters cut.
>> You'll notice that we have a very neatly organized tree.
In fact, if we're going to make this part, we want to learn more about it,
we need to define its material.
So in this material box, we'll right click, and then hit Edit Material.
And SolidWorks gives us a very long list of things that we can choose from.
Let's say we're going to make it out of aluminum.
We'll do 6061 P6, that's a tempering rating.
We'll hit apply, close.
And now it's out of aluminum.
It looks slightly brighter.
Doesn't really do much for us.
>> But it allows us to measure some really interesting or cool aspects
about this part specifically being made out of aluminum.
For example, if we go to the Evaluate tab and hit Mass Properties,
we see that the part weights 0.09 pounds.
Volume is not going to change based on material.
But weight is dictated by which material you use.
It's pretty cool.
If we were to run a stress simulation, the material that you choose
will drastically alter the results.
So that's pretty cool.
>> If we wanted to make it look different, we
could pop out this tab here just by hitting these double arrows and right
click here and say appearance.
And then, we can change to make it blue, whatever you want.
And then, in a final render, if we wanted
to make an actual render of this part, we can choose its surface finish.
So a lot of times, you'll design your parts.
They have this flat gray or flat black aesthetic to them.
But that just lightens the load on SolidWorks
so that you're not using superfluous graphics power
to render your part while you're designing it.
But if we did want to do a render, we would
have to define the surface finish.
So let's just say that it's polished aluminum for now.
Notice that polished aluminum pops up over here.
Hit the green arrow.
Cool, that took.
And let's just change this thickness of these webs.
So all we have to do is go over to our very neatly organized feature tree.
And we see web cut.
Expand that.
Click on the web sketch.
And then, we're just going to change one number.
>> So let's change it to instead of being 50 thou on each side,
so 100 thou total, let's make it 80 thou total.
Cool.
You see the webs got a little bit skinnier.
Awesome.
So we just changed all those features just by one number.
We changed the thickness.
SolidWorks automatically recalculates the fillets to make them fit.
It changes all the geometries.
And it works because we had defined them to be all symmetrical
and all defined off of one dimension.
Like I said before, it's analogous to defining
a constant when you're writing code.
>> AUDIENCE: Does it work if you use any TrueType font,
or are you limited to what they [INAUDIBLE]?
>> ANSEL DUFF: It works off of your system font,
so if we go back to our letters cut, we had just gone with the default font.
If we hit Edit Sketch, zoom in a little bit, double click on the letters.
If I can do that.
Take a second to trace them out.
And hit Font again.
So we have a list of fonts here.
And those are system fonts.
If you want a specialty font, and it's not on this list,
you're going to need to install it on your system.
Just a little bit of Googling around on how to do that on Windows.
>> AUDIENCE: Also, does this thing know what font size or changes are not
going to be [INAUDIBLE]?
ANSEL DUFF: Yeah.
So the question was how do we know how thick or thin to make the fonts?
How will the machine be able to handle really thin features?
So of course, it's going to vary from machine to machine.
But just by reading the spec sheet of our printer,
we know that it has a resolution of about 4 thou, four
thousandths of an inch.
So we want to make all the features be well beyond that.
So if you were to make a font that was, say, 10 thou tall, that's
like two sheets of paper, you wouldn't be able to read it obviously.
But just hypothetically, if we wanted to make
a font that was on the order of the accuracy of the machine,
it would look horrible.
So in our case, we know that we're well beyond the accuracy
of the machine in terms of the ratio of the height of our font,
or even the thickness of any feature in the font
to how accurate the machine is capable of being.
>> So we're in the clear here.
But if hypothetically you were using a machine that
had an accuracy of maybe 250 thou, like a quarter of an inch,
then our font would look really crappy because it's
on the same order of how accurate the machine is.
Another thing that we need to pay attention to,
and this is specific to 3D printing, is how thick are our layers going to be.
So I'll go over to MakerBot settings in a little bit and we can play with this
and talk more exhaustively about it in a second.
But the way that the 3D printer works is it
extrudes filament in a very fine thread almost.
And if we make the thread or the filament strand really,
really large, then it's going to look kind of blotchy and not
that clear when we actually print.
>> So again, just as a rule of thumb, you want
the size of your fonts or all the features
to be well beyond the order of the thread size.
Yeah, so Exit Sketch.
And it takes.
If we were to change the font, again, we can just hit this.
And it will recalculate it automatically for us.
So we'll go font here.
Choose Comic Sans.
Great, looks atrocious.
Hit the green arrow.
Exit the sketch.
And you'll notice that it still looks so bad.
Wow.
I can't even look at that.
I'm just going to undo that.
Great.
It will recalculate all the curves and make the cut.
>> So cool.
We are good to go.
So now, the next step.
You're going to want to grab a Snickers at this point
because we've been working for a while.
It's a good idea to take a breather.
So what is the next step in manufacture?
We could 3D print it.
We could mill it.
Those are the two popular options.
If we were to mill it, we would have to write
what's called G code or CAM, which is going to take a while,
and we're not going to do.
All that does is it tells a tool, like an N mill, which is basically
a fancy drill bit, where to move around this piece
to create all these features.
Some things are impossible to do with a mill.
>> For example, if we go to our fillet here, should be in web fillet,
and we suppress that, which is done just by hitting this little downward arrow,
all the fillets go away.
We have all these really sharp points.
This is a horrible design practice, and you should never do this.
But hypothetically, if you did want to design a really sharp corner in here,
you could not create that corner with an N mill of finite diameter.
You cannot have-- you can conceptualize it as a fancy drill bit.
You can't have a drill bit moving around and just
bumping off the bottom of that corner node and leaving a very hard corner.
That's just impossible.
>> So those are things to be aware of.
And when you create CAM, those will all become apparent.
But just things to be aware of.
Luckily, the 3D printer is really cool because it
can create really obscure geometries and really obscure fixtures.
So we're in the clear here, but it's nice to think about those things.
So one last thing we want to add in is a hole on the bottom.
Like I mentioned before, there's a mounting hole in our piece here.
And that's how we bolt it in.
>> When I made the version zero, I did not CAD in that hole.
I just went and took a Sharpie and held it up and marked it
and drilled it by hand.
That was kind of a pain, and not really excited about doing that again,
so we'll just CAD it in.
So here's a really exciting time because we need to add in a reference plane
because, shock, you cannot sketch on a curved face.
Something that you cannot do.
This face is curved.
We had provided it with a radius before.
I'm going to move this dimension out of the way.
You cannot sketch on it.
>> If we select it and try to hit sketch, oh my gosh,
cannot sketch on a non-planar face.
Wow, good thing your buddy Ansel told you about that.
And he also taught you how to create a reference plane.
So we select this.
We hit Reference Geometry, Plane.
Now, we have a plane that is tangent to our face.
Or maybe we don't.
That's not good.
I don't know why it's doing that.
>> So we need to-- if we were to just select this face and create tangency,
the plane could be at infinitely many angles
while still being tangent to that face.
So we need to constrain it again using a second plane.
So I had selected the side of our face here.
And SolidWorks defaulted to perpendicularity.
But you could select that yourself, and it would give the same result.
>> So all we've done is just define this plane
that is tangent to our bottom face here but then
orthogonal to the side of the part.
So when we create our hole, our hole is going
to extrude normal to the plane, which is going
to be parallel to the side of the part.
That's what we want.
If we were to create tangency on a different plane,
then perhaps the hole would be at an angle, and nothing would line up.
So this is a nice, simple example for us.
So we just hit normal to, now we're normal to the bottom of the part,
and now we can go through the same procedure of CADing up a hole
and extruding it.
>> So again, we'll just create a circle here.
A better idea would be-- we're not technically sketching
right now, which is why SolidWorks just yelled at us.
It's kind of like your mom, yelling at you to clean up the room.
So let's sketch here, add in some center lines.
I don't know why it doesn't want me to sketch.
Oh, we forgot to select the plane that we're going to sketch on.
So let's rename our plane bottom plane, hit Sketch, make a center line here.
Something that's really cool is even though we're normal to this
and we haven't unlocked or unhidden any sketches,
SolidWorks will still allow us to create a sketch that is making relations
to features of the part that we did not tell it to do.
>> So you'll notice, when I hold the pencil over the corner
here, that little orange bubble pops up.
We can create a relation to the corner of the part.
But we didn't tell SolidWorks that we want it to do that.
So I think that's super cool.
So we'll just make a center line up top here.
Make another one down the center.
Uh-oh.
I did not do it off the midpoint.
That is offensive.
All right, go down the middle here.
>> It's vertical.
Cool.
It's all black, so we're good to go.
We'll make a circle.
And dimension its diameter.
I'm just going to arbitrarily say 0.10 inches, a tenth of an inch.
Everything's bolted together, so we don't have anything to measure off of.
But we would, if this were threaded, you could stick several different screws
in there and then just find which matched.
But it's not just a clearance hole.
So there are two different types of holes,
threaded or tapped holes, that will accept threads, accept a screw.
And those will not be able to move.
That's how you bolt things together.
Or there are clearance holes, which are larger
than the biggest diameter of the threads.
>> And that allows threads to just pass right on through.
So the way our fixture works here is that we
have a clearance hole in the metal.
And then, another clearance hole in the part.
And then, just a nut on top.
You could go in and measure with calipers using the interior prongs here
what the diameter is.
But everything's bolted together, so we're not going to do that.
We'll just set it at 1/10 of an inch arbitrarily.
Then, you would measure this height.
I'll just set it at 0.250.
>> Again, this is arbitrary.
But you would ideally measure that and be good to go.
So hit the green arrow.
Exit the sketch.
Sketch is done.
Now, we're going to make it into a feature by hitting extrude cut.
We want it to only go through the first layer, so we hit Up To Next.
Hit the green arrow.
Now cool.
So another cool thing, I'm just going to hide this plane because it's not
doing anything for us right now.
>> So another cool thing is that we did not tell SolidWorks
how deep we wanted that hole to be.
We just said Up To Next, which means that there are many, many layers here.
There's one, two, three, four, five layers that it could have cut through.
But just by saying Up To Next, it knew to only cut through the first one.
If we were to say Through All, hit the green arrow,
it sketches through everything.
You can see daylight on the other side of it.
That's not what we want.
So Up To Next.
There are a lot of options here, but Up To Next is what we want.
Cool.
So now our part is completely done, and it is time to machine it.
So like I said, we're going to step through doing this
with MakerBot 3D printer.
But you can do it with anything.
So we'll go here.
We're going to save our part as a .stl file.
So we do Save As, lend support to, and select .stl.
Hit Save.
I'm actually going to save this in my Downloads folder.
Hit Save.
SolidWorks prompts us.
Do you want this to be an STL?
Hit Yes.
Cool.
And now, we are ready to fire up to MakerBot desktop application.
>> So let's do that.
All right, ready to go.
So at this point, I always like to view the plate from the top.
It's nice to be on top.
So we'll just go here.
Add file.
We're going to go to our downloads.
I think we called it lens support 2.
So here we go.
Open it up.
It is on our platform.
>> So this is kind of an impractical way for us to print the part.
If we zoom in a little bit here, you'll notice
that the arc is touching the base.
So the 3D printer is going to try to figure out a way to print this.
But it's going to freak out unless you add supports to it.
But that's kind of a headache.
>> The easy way to do it is just to select turn.
The part is selected because it's highlighted in yellow.
Turn, and then we're going to want to go-- whoops.
We're just going to push it back 90 degrees.
Hit Lay Flat.
Lay Flat ensures that its bottom face is touching
the bottom face of the build plate.
And we're good to go.
So our maker bot is not right now connected
to the network for some reason.
But that's OK.
We can just hit Export Print File.
It'll take a second to process.
>> And you can put it on a flash drive and then
plug that flash drive into the printer.
So it's a good idea sometimes to mess around with the settings.
When you first open this box up, it'll say-- it has a couple presets.
Do you want low resolution, high resolution?
But we can actually change these at a much more granular level.
So I'll just walk through a couple of these parameters and what they mean.
>> Infill is percent of the volume of the part is being actually printed.
So if infill were at 100%, everything would be printed.
It wouldn't do any null hollow features, no honeycombing.
It would print a completely solid part.
It would take an eternity.
So we will set it as 15% here.
I think the default that MakerBot comes with is like 10%.
But 15% is fine.
If you print the part and then try it out and it buckles or breaks
or it seems kind of weak, then you can just bump that number up
and it'll be a lot stronger.
The plastic filament itself is actually pretty strong,
so just bump that number up.
It'll make it a bit stronger.
>> Number of shells is how many shells on top
of the honeycomb, how many layers on top of the honeycomb it prints.
I set it to five to give it a nice finish quality.
And then, layer height is the diameter of the thread that is being extruded.
So right now, 0.2 millimeters, a fifth of a millimeter
is what it's printing at.
But I think it goes all the way down to, wow, a hundredth of a millimeter.
That is tiny.
So that will take-- if we set this to 100% infill with five shells
at 0.01 millimeter layer height, hit Save Settings, and then Export Print
File, you'll see the expected time is going to be huge.
We'll just let it process because I'm curious to see how large it would be.
>> I think this part using 15% infill, 0.2 millimeter layer, and five shells
took about two hours to print.
But you can see it's even taking a really long time
to prepare and to create the actual MakerBot file for it.
>> So something that's MakerBot about specific is that from this desktop
application, it will export in a .makerbot file format.
That is only file format that the machine will accept.
If you try to give it an STL, it will freak out, maybe explode.
So always a good idea to export in a .makerbot file format.
So that's going to process.
>> In the meantime, let's just hop back to SolidWorks here and look at our part.
So this was kind of a nice example of a part
because it allows you to design for something that already exists, right?
We had to measure all the supports that already exist.
In reality, there are a lot more considerations
that you need to take into account for when designing a part.
For example, I won't do an in depth demo of this little phone dock,
but there were a couple more considerations
that we needed to take into account.
>> So you'll notice that when the phone is sitting,
and I'll try to give you a side angle there.
When the phone is sitting in the dock, it
is kind of raked back by a little bit.
I think I set that at 15 degrees.
That's somewhat arbitrary.
But as it's raked back, the center of gravity of the phone
is going to be displaced from its base meaning that,
if when designing the part we had just cut it off and not had this back panel,
but it was only this much, then when we put the phone in,
it would've just toppled over.
>> That's because the center of gravity of the whole part
of the phone, the heavy part, would extend proud of the base.
And it will create a tipping moment, and it'll fall over.
So a way to combat that in design is to just make a quick mock up
of your phone, which will take like two seconds.
We'll just make a new part.
Make the fastest mock up of an iPhone.
So let's make a rectangle on the top plane.
Here, create, define these.
Just going to measure quickly with calipers.
The width is 2.308.
And then, the height is 4.880.
And then, the depth, this is the number that everybody cares about in tech,
0.30.
I have a screen protector on it, 0.303.
>> Cool.
Extrude it.
And then, I'll add some fillets.
It's a little bit trickier to measure the fill diameter.
You can use a gauge, but I don't have one on me right now.
We'll just eye it, and that'll be fine.
That looks about right, just visually.
This is like a dummy phone that we just made in like a minute.
So we'll save this as iPhone dummy.
And now, we can create an assembly with our dock and measure
how far the middle of our phone is from the base.
So I had mentioned before that we create parts, assemblies, and drawings.
Drawings are not really something that you'll
mess with unless you're designing parts that will be made out
of house at a machine shop or what have you.
And it's a little bit more involved to properly dimension a drawing
and make sure that every dimension is clear.
And you also have to add tolerances, and that gets a little bit more
involved, so we'll just kind of gloss over that.
But let's say we want to make an assembly with the phone dock that I've
already designed and our dummy phone.
>> So we've already saved this.
Let's go up to File.
Make Assembly From Part.
And then, we're going to hit Add and iPhone dummy.
Also, nice to just select this graphics preview.
That'll show you the actual part itself.
And then, insert another component will browse for the iPhone dock, CS50 dock.
Cool.
So now, it's a nice sanity check just to double check
that the phone will actually fit in the dock that we've designed
and how it will look.
So let's make this face coincident with the bottom of this face.
And these relations are all handled through what are called mates
in assemblies wherein you have two parts,
and you need to join them by a list of defined joining features.
>> So for example, we need to put our phone which is being currently blown up,
call you later!
In a dock, and we need to say that the bottom face of our phone
is coincident with the inside bottom face of the dock.
And then, this will be centered inside.
We've given a little bit of a tolerance so that it's not a super tight fit.
And that will completely define it.
We'll make these two coincident.
Select mate up here, and it defaults to coincident, but it's inverted.
So if we just hit this little button down here, it'll flip it.
We hit the green arrow.
So looking good.
I've actually forgotten what the tolerance was on the spacing.
Like I said, I gave it a little bit of extra space
because it doesn't really want to be a tight fit.
So what we can do is measure the difference between them
and then split the difference.
>> So we can use the measure tool in SolidWorks.
We go up here to evaluate, measure.
Little tape measure comes up and that annoying window
in the middle of your part.
And we're going to select these two faces, they're highlighted in green.
And their distance is 2.36 inches.
So I think we said 2.36.
We'll remember that.
This was 2.308.
So we'll just split that difference with space.
Whoa.
So we got a mate.
Select these two faces.
Coincident.
Whoa, gotta add a little bit of space in there.
So it was, I think, 2.36.
We'll make this in parentheses to be clearer, minus 2.308 divided by 2.
That's splitting the difference for space.
Good to go.
But if we eye it, it looks like the phone is actually
extended in this direction beyond the dock.
So we just need to flip it.
It made very little difference.
Can't really see all that well.
Hit the green arrow.
And then finally, we'll make this back face coincident to the back there.
>> Realistically, there's also a tolerance for, you can see there,
space in the front.
We could split that difference.
But it's just the same procedure, so it's redundant.
Cool, so let's look at it from the side.
Mate is still selected there.
>> If we were to draw a line normal to this in the middle,
you'll actually see that the center of gravity of the phone
is somewhere in this region.
It's in the middle of the base.
We purposefully extended the base well beyond where the center of gravity
falls such that it will be able to sustain a tipping moment,
like when you place your phone in the dock.
You don't have to do it super gently.
You can just put it in.
It doesn't fall over.
>> If the distance between where the center of gravity falls on the base
and how far we extend the base back was really small,
it would take a very, very small tipping moment to actually tip it over.
So that would just be very impractical because you
would have to very delicately place your phone inside.
So I just added maybe a quarter of an inch or half
inch beyond what we needed.
I did not calculate the required tipping moment to take this over.
I think that might be a little overkill.
>> But physically, that's how it would be done.
Cool.
So now, we have this assembly saved.
You could make a more detailed iPhone if you wanted dimensions.
I had made this little extrusion for the Home button,
and this is iPhone specific.
But if your phone's in the dock, you can just
turn it on without having to take it out and look at all the text
messages that you're getting or SnapChats, my preference.
>> So another assumption, viewers at home might be thinking, Ansel, you idiot!
You assumed that the phone was uniformly distributed mass wise,
like that mass inside the boundaries of the phone is uniformly distributed.
That is not the case.
But I think that's a fine assumption.
So we can save this assembly.
We'll call it iPhone in dock.
We're good to go.
>> So you can create really complicated or ornate, involved assemblies
from many, many parts.
Just know that each part has a certain number of fixtures and lines associated
with it.
So if you have an assembly with a lot of parts
and you want to move it around and measure and do a lot of things,
it can become laggy depending on how powerful your computer is.
Just something to be aware of that will happen.
>> So that is kind of an intro to CAD.
The takeaways, I would say, are definitely add relations everywhere.
You will kick yourself in the rump if you don't.
It's very painful to go back later and change redundant dimensions.
It's useless, right?
You always want to dimension everything such that you dimension one number,
and then add relations from that number.
That's a huge takeaway.
Just being clean, just like when you're writing code, being clean and labeling
everything.
Labeling your features-- you'll notice that when we made this little lens
support, everything is labeled.
If you don't make this in house and you ship it to somebody,
most places, maybe 95% of machine shops or whatever,
will take a SolidWorks part file, you don't even
have to make drawings for it, you just send them this file.
And they'll be able to get every measurement they need off of this file.
And it's a lot easier for them to work with if everything is neatly organized.
You can even add folders.
We can select the bottom feature, hit Shift, or rather hold down Shift,
and select the top.
And everything in the middle becomes selected.
And then right click adds a new folder.
We'll call it awesome folder.
And now, everything is in a folder.
Things like that, just making everything very neat and organized,
another takeaway.
>> And then ultimately, being very explicit.
So there are relations between something that you've already defined
and other things that are related to it, but then there
are also dimension relations.
So it's really important to be explicit and make sure
that everything in your sketch is completely black before you move on.
So at this point, I'm going to open the floor up to questions,
and we can start to talk a little bit more about that.
And then, once questions are done, I'll show you the render process pretty
quickly wherein we can generate a really realistic looking image of this.
When you're looking at this in CAD, it just looks kind of a dull gray blob.
But when you do a render, it will be very, very realistic looking.
So questions?
>> AUDIENCE: MakerBot stuff?
>> ANSEL DUFF: Any other questions?
The MakerBot is, no fault of our own, actually, no, it's
definitely fault of our own.
We have lost a couple sheets, the tape sheets on the bottom.
So once we get those in, we'll be able to print again.
>> AUDIENCE: [INAUDIBLE].
ANSEL DUFF: Oh, what's that?
Oh, yeah.
I thought you were talking about the actual MakerBot.
76%, wow.
It's going so slowly.
I thought you meant can we print yet.
AUDIENCE: You put together the tutorial online.
Does that include the best resources for people to remember what to click
and how to do some of the things you went through today?
ANSEL DUFF: Yes.
So there is-- the MakerBot tutorial, is that what you're referring to?
>> AUDIENCE: The one you put on the website.
>> ANSEL DUFF: Yeah, this one.
So this is MakerBot specific.
This is not SolidWorks specific.
I hope that this video will be available in high resolution
as a reference to the syntax and the GUI associated with SolidWorks.
But the tutorials, I think, are super helpful as far as getting started goes.
So when I hit New, or even use a hot key for that, but if we go to File, New,
we get this prompt box where we would typically select part.
But if we hit this tutorials box, then we
are venturing into the world of the tutorial.
>> So this is how I learned SolidWorks, was doing a bunch of these tutorials.
In fact, if you take CS 51, which is kind
of the intro to computer and machine design class,
they will require, I think, the first p-set zero
is doing all these tutorials.
They're super helpful.
They're quick.
You follow along in your own time.
They're a good way to learn the commands.
I know I was starting to go a little bit quickly towards the end.
>> AUDIENCE: Do they have cheat sheets or PDFs you've come across?
ANSEL DUFF: Yeah, so there is a page.
I'll put it on the staff site.
There is a page with a bunch of hot keys for SolidWorks.
SolidWorks is also super configurable.
Like, you can change just about everything.
If we go back to the main page-- I'm just going to cancel this.
If we go back to the main page, if you don't like this toolbar being there,
you can drag it and put off to the side.
I'll put it back up top, because I think it's the cleanest.
You can change just about everything.
If you want everything to be in millimeters, you can change that.
You'll notice, when we were dimensioning something,
let's go back here, that everything's to two decimal places.
That's rubbish.
Let's make it to three.
We'll go to Document Properties up here, which
is two icons over from the stop light.
Document Properties, Dimensions, and then we
set this to three decimal places.
Hit OK.
Everything changes to three decimal places.
You can customize up the wazoo.
>> But the biggest thing, I think the most useful user aspect of SolidWorks
are hotkeys, just like many programs out there.
I've been using them a lot, mainly holding down Control
to add relations, Shift to highlight multiple things, and F to fit,
like if we zoom out and then hit F. It fits the part in our view.
But there are many, many, many, many more hotkeys.
And I will put the page on the staff site that lists all them,
and they're super useful.
And just little shortcuts like double clicking
when you're drawing a line to exit.
Any other questions?
>> AUDIENCE: Where do you [INAUDIBLE]?
ANSEL DUFF: That's hidden.
That is hidden.
>> AUDIENCE: Why is the MakerBot printing that [INAUDIBLE]?
ANSEL DUFF: So that's actually a bug.
I contacted the manufacturer.
There's somebody with the same name at that organization.
>> AUDIENCE: The random one when you did the plane tangent to the hole,
is it then possible once you've drawn on the plane
to make the plane itself curve to fit on the surface?
What if you drew something on the plane to eventually go
onto the surface itself.
ANSEL DUFF: Great question.
So let's go back here to bottom plane, normal to it.
Sometimes after a restless night, my bottom plane is not there either.
But hit bottom plane.
We're good to go.
The question was, if we draw something on the plane, can it wrap around?
Or rather, can the plane itself wrap around to a curved surface?
And the answer to that, disappointingly, is no.
You cannot wrap a plane to a face that is not planar, not completely flat.
But if we did, watch, let's go back and sketch on here.
And we'll write, I don't know, let's write SolidWorks.
>> If we wanted extrude this here, even though we sketched it
on a plane that was tangent to the curved surface, it will still work
and it'll still take to a curved surface.
If that makes any sense.
You can make holes, any feature that you want in a sketch,
and then apply that to a curved surface.
But all the sketching has to be done on a plane.
Also, the nice thing about the feature tree is that once you create something,
it's easy to pick and choose what you want in your assembly.
So like this, SolidWorks looks ridiculous because it's overflowing.
>> So if we wanted to kind of put i on a shelf and use it later down
the road, we don't want it right now, if we just hit Suppress, it goes away.
So all I did was I left clicked, and then this little dialogue box pops up.
You have a ton of options here.
I just hit suppress.
>> AUDIENCE: [INAUDIBLE].
>> ANSEL DUFF: If we want it gone, or rather if we want it back,
we just hit Unsuppress.
It's back.
So that's a really useful feature.
Not so much in parts, but when you have an assembly,
there are a couple other-- I'll go back to the assembly
and show you some cool assembly features.
So if we wanted to see how the phone how the fillets morph
to the fillets of the dock, we can highlight this.
So we go to dock.
Then we hit Change Transparency.
This makes it semi-transparent.
You'll notice that the fillets that we made here, there's plenty of space.
>> Additionally, we'll change that back.
You can also view in plane while moving through the depth of the part.
So this little count, it's like a half donut.
It's called Section View.
If we hit that, actually, we want a different plane.
Let's do top plane.
>> So we hit Section View, and then move this in and out.
Kind of hard to see.
We'll zoom in a little bit.
But this actually takes your field of view, your plane of vision,
and pushes it through the part.
So what's blue is actual material.
There's a phone, there's a fillet.
It's not that interesting for this part.
But this can be done in both assemblies and parts.
So if we go back to our lens support, then
hit the same thing, little half donut here.
It's kind of cool to see.
>> Sometimes, when you're designing a complicated internal feature,
this is really useful to check clearances,
as a sanity check to make sure that holes are concentric, what have you.
But you can just move it up and down.
I'm just holding it down, left clicking, and it will show you everything.
This can be done on any plane.
So we'll see if the MakerBot is done.
Oh, 80%.
We'll do the render and we'll come back.
>> So we had defined this part to be aluminum.
We had also defined its appearance to be gray.
We'll do polished aluminum.
So as far as SolidWorks is concerned, it's appearance
is completely taken care of, completely defined.
So now, we're going to go and we're going
to make a really realistic render of it.
It's going to look as it would in real life.
So the package I have enabled here is, actually, I don't have it enabled.
If there's something, you can pick and choose which tools are displayed.
>> The package that we have in our office has everything available,
the academic license has every feature that SolidWorks
makes incorporate in our package.
But not all of them are showing.
So if you want to add or subtract from this menu, just right click.
Nope.
You right click, and then you get this list here.
So we want Render Tools.
Render Tools uses an engine called Photo View 360, which may or may not
be enabled.
So to double check, we'll go to Tools, Add-ins,
and then we select Photo View 360.
Hit OK.
Now, we're good to go.
So we go to Render Tools.
You can do a preview render.
But it's not going to do anything for us.
So we're going all the way, final render.
And this will take a little bit of time to process.
But it'll look pretty cool.
>> So there are all these parameters on the right hand side that we can adjust.
The resolution, lighting, where the light's coming from,
the diffusivity of the surface.
Those are all adjustable.
But we're just using the defaults.
You can even move it around a little bit.
You can see it's really shiny.
All the fillets are glistening.
Oops, just lost my power.
All the fillets are glistening.
Sky is the limit as far as that goes.
It's pretty cool.
>> For some letters, and in fact a doorknob that we
had designed a little bit earlier, I had done a render of the door
handle also in false aluminum, and this is what it looks like.
There are some more advanced features with renders,
like you can add-- like if you were designing a battery pack, for example,
you can have a sticker that says high voltage or decals.
You can import your own decals and add them.
So it's very product designy.
85%, I'm dying to know how long this is going to take.
Yes?
AUDIENCE: You are printing something that's solid,
and then you have something that's [INAUDIBLE] in the middle.
MakerBot and SolidWorks work together and printed in a way that [INAUDIBLE]?
>> ANSEL DUFF: Great question.
So the question was, is there a way for us to print internal features?
Internal features are something that's suspended.
A good example is like if you were to print an A,
the center triangle of the A is an internal feature that's
completely suspended.
Or rather, if you were to print a hook that's overarching,
when the printer wants to get to the level where this part of the book
first starts, there's nothing holding it up.
It can't just print in mid-air.
Those are called internal features or suspended features, many names
for the same idea.
>> But the answer to your question is yes and no.
SolidWorks does not do anything to that extent.
SolidWorks is a CADing and simulation program.
And we can design really precise and advanced parts.
And even create CAM and G code for them.
But it doesn't really care about how we make them.
It only cares about us designing them very precisely and very efficiently.
>> However, once we've exported our part as a .obj or .stl-- side note,
if you have the option to choose between exporting using the file formats .obj
and .stl, always go with STL.
Once we've exported and we put it into the MakerBot desktop application, which
is what we're looking at right now, we have the option of creating supports,
printing these little support structures.
They're little towers that taper off at the end
and then hold those internal features.
So if we wanted to print a hook, for example,
when it prints this part of the hook, it would also
start to print a little tower.
And then, when the tower gets close to this base of the hook,
it would taper off into a really, really small plastic feature.
And that will support this part of the hook.
Then, it would just join the two.
>> And we do have the option of printing like that.
That option is turned off right now.
We haven't really needed it.
But yes, we can do that.
And that's how it's done.
You print supports.
And then, once everything is done, just break it away
and you can peel the supports off.
Any other questions, concerns, comments, remarks?
>> AUDIENCE: Yeah, supports.
Within the shapes?
I'm thinking like going back to the A example, what
if the A had something hanging down from the top?
Then the support is latched onto the A itself.
ANSEL DUFF: I can't say for sure without actually trying to do it.
But it would be cool.
I would imagine that they could print supports
that are on the side of the A that don't interfere with your part.
Some internal features are going to become kind of a lost cause.
For example, if you wanted to print a sphere with a smaller sphere located
internally, they're both independent, not attached at all,
it would probably try to print supports inside it.
But then, you'd never be able to remove those supports unless you cut a hole
and peeled them out.
>> So it almost takes a little bit of foresight
when you're designing the part and getting the part prepared
for print to ensure that it will be printable.
So like this feature, when it first imported, it was vertical.
That would be really challenging for the printer to print.
So always make sure that you lay it on its side.
And you'll be set.
88%.
We will sit here until it's done!
>> [APPLAUSE]