Transcripts
1. Introduction and How to Use the Course: Hello and welcome
to this course. My name is John Ellison and I'm a product designer
and design engineer. And I've been using
solid work since 2006. I've previously made courses in solid modeling and sheet metal and some other solid
work subjects, but my students often asked
me about surface modeling. I decided to make this
standalone course as an introduction to
solid work surfacing, as it's a great collection of really powerful tools and it's a really good way to take your solid work skills
to the next level. Before we actually jump into the specifics of surface
modeling and get started, we'll have an introduction
in the next video explaining a little bit about how surfacing works and
why you should use it. Before we do that
though, there's just a few short details
about this course, what it covers and how it works as the name suggests,
Surfacing fundamentals. This course will cover the
basics of surface modeling. It won't just be a
list of all the tools covering every single
sub option and use case. But hopefully it will
give you the skills that you need to explore
them further yourself. I always say in
my other courses, the best thing to do
is just practice. So maybe you can take these
skills and use them to challenge yourself to recreate some models of things
you see around you. We will, however, go through all of the main
tools and we'll have examples along the way that can show you how to use
these features. The course does assume
that you already know how to use solid works for
basic solid modeling. If you're not already
a solid works user, then I'd highly recommend
learning solid modeling first. If not, a lot of this probably won't make complete
sense to you. It is completely
up to you there, no steps are skipped
out in the videos. Some areas are speeded up
slightly just for time, but if you want to, you can just follow along with the videos. Exactly. And try and
pick things up that way. If you do get stuck anywhere, you can always send me a
message or you can ask a question in the Q
and A. I would just ask that you
consider maybe doing a quick search
through the previous questions or online first, as a lot of the questions
that come up have previously been asked
and answered before. When you're watching the videos, the speed controls are
down below and so are the subtitles and quality
settings obviously. Feel free to slow the
speed down if you need to, and you can pause and skip
back as you follow along. This course does have some
example files and resources. These can be found
under the project and Resources tab and then
download resources here. To use those files, just
download that zip file and then unzip it and all of
the files are in there. The example files are
from Solid Works 2022. You'll need 2022 or
newer to open those. If you've got an older version, those Solid Works files
won't open for you, but they're not actually
needed for this course. They're all just for reference. There's also some step and STL files in the example files. These should work with any
version of Solid Works, and to open them you can just
drag them into Solid Works. And then finally, this course uses millimeters as the unit. But this isn't really important
to any of the models, so you can use any
unit type you like. You can easily
switch the units by clicking down here in the right
hand side of Solid Works. With all that out of the
way, let's have a look at what surface modeling is
and how we can use it.
2. Introduction to SolidWorks Surfacing: What is surface modeling? When we model in solid works, we can either use solid
modeling or surface modeling. When most people start
out learning solid works, they usually start off
with solid modeling. And lots of people
only ever use that. And that's perfectly fine. Because solid modeling
in solid works is pretty powerful and you can usually use it to make exactly
what you need. Surface modeling just gives a different way to
build things and it gives you a whole load of new techniques that you
can add to your toolbox. People often think in terms of either solid modeling
or surface modeling, but actually it's good to
use a combination of both. I personally tend to use mostly solid modeling just because I'm a bit more
familiar with it, so it's a bit easier for
me and a bit faster. But then if I can't make
something in solid modeling, then I'll switch to surfacing
to give a simple example. Here I am in solid works, I'm going to start
a new part and say, for example, we wanted to
model up just a simple cube. What we do is probably start
a sketch on the top plane, and then we'd get something
like a center rectangle. And we'd just draw a
center rectangle at the origin and
then set the size. I'm going to use Smart
Dimension to fully define it. I'm going to set it as
100 by 100 millimeters. As we said in the introduction, I am working in millimeters, but you can use any
unit type you like. It doesn't really
matter for this course, and you can change it. Down here we have a sketch that just has a square that's
100 by 100 millimeters. Now I'm going to go
to the Features tab. Choose Extruded boss base. And I'm just going to do
a blind extrude upwards 100 millimeters like so. And then press okay. Then we have our cube
100 by 100 by 100. It's got six outer faces. And we can see here in
the feature manager, the solid body's folder has got a little number
one next to it. And if we expand
that, we can see we've got one solid
body in there. That's our solid cube
that we just made. If we do a cross section view and we drag through the model, we can also see it's
fully solid inside. Then finally, also, if we
add a material to this cube. So if we right click on
material here on the left, and we choose, say for
example, just a steel. And then we check the
weight by going to the Evaluate tab and looking
at the mass properties. We can see it's got a
weight of 7,800 grams. So it's 7.8 kilograms. That's how much a cube this size would weigh if
it was made out of steel. However, instead of making
this with solid modeling, we could also basically make the same thing with
surface modeling. So let's have a look at
how we might do that. First off, I'm going to start another sketch on the top plane, the same plane as we
started on before. And I'm going to go
to a normal two view, so we're looking
down from above. Going to get the line tool
from the sketch tab and just draw a straight
horizontal line along here. I'm going to use the
smart dimension to set that as 100
millimeters long, so it's the same
as the other cube. Then I'll make it say 50
millimeters from the first cube. And I'll select the line
and hold down control. And also select the bottom
face of the first cube. And then we can add
a colinear relation. That line should now
be fully defined. So if you look in three D, we've just got a single straight line which is going to
make the bottom of one of the new cube faces. To actually do this, first we need to find the surfacing tab. You might have it already up here on your command manager. If you can't see it there,
like it's not on my screen, just go to some
empty area on one of the tabs like here
and right click. Go down to tabs and then put a little tick
next to surfaces. You should now see that
you've got a surfaces tab. I'm going to select
that surfaces tab. I'm still in that
sketch, the line sketch. Let's select extruded surface. It's the first tool up there, and now you should see a preview of that extruded surface. Using that line, something like this, you don't see a preview. It might be that you
exited the sketch first. If you're seeing something
like this yellow message, it just means that you
have to select the sketch that you want to use with
this extruded surface. You can do that just by left
clicking on the sketch, but you should see some
preview like this. We can now create the
extruded surface. If you look at the
tool, it's very similar just to the
extruded boss base. We've got all the
same end conditions, things like up to next
mid plane and so on. Let's select blind, the
first one and we'll set 100 millimeters and just
extrude upwards like this. And then press. Okay. Now I've
created our first surface. It's basically the same as our bottom face of the first cube that we
made that was solid. However, if we look on the left, we can see we've got a new
folder here on the left, above the solid body's folder, we've got one called
Surface Bodies, and that's got a
little one next to it, which indicates we've
got one surface body. If we expand the folder, we can see that we've got
one surface in there. That's the surface
that we just made. Now this surface and
any surface that you make in solid works has
got zero thickness. It's got no thickness to it. If you imagine in real life, even if you had like
a piece of paper, it would still have
some thickness to it. Even if you had some kind
of fancy nano material, it would still have a
tiny bit of thickness. But here in solid works, in the computer
three D model we can actually have a surface
with zero thickness. Okay, so now we've
made that end face. Let's continue and make
some more of the cube. Let's make the
sides. To do this, I'm going to spin
the model around. I'm going to select that face, and I'm going to start a
new sketch on that face. So you can select Sketch
from the pop up menu, or you can go to the Sketch tab and you can choose Sketch. Now make sure you have
that face selected, so it should be blue
if it's selected. And then on the Sketch tab, let's choose convert entities. We've now converted
the outside edges of that face into a new sketch. So we've basically got a
square in this sketch. We're now going to use that
square to do another extrude. So I'm going to go back
to the surfaces tab. Going to choose that same
tool, again, extruded surface. Again, let's extrude
blind, 100 millimeters. If you're going in the
wrong direction like this, you can just flip the direction
by pressing the button. The same as the extruded
boss base tool. We want a length of 100
millimeters and then press okay. Now we can see that
the sides are being created in the surface
bodies folder. We've now got two surfaces, so we've got the end one
that we just made and now we've got another one with
all of the sides on it. If we spin the model around, we can see we've got
a hollow box there. Although we made four faces, they're actually all
joined together into one single surface because they just come from
that single sketch. Before we close this box
and make the final phase, what we can do is grab the measure tool from
the evaluate tab. If we measure between
these outside faces, we can see the distance is
100 millimeters exactly. If we then clear
that measurement and we measure to the inside faces, we can see the distance. There is also 100
millimeters exactly. As I said, these faces
have got zero thickness. In real life, this
would be impossible. You'd always have a
slight difference between the inside and the outside based on the
thickness of the material. But here in the
computer, the inside and the outside are
exactly the same. Now we have this open box. Let's try adding the final face. And there's lots
of different ways we could do this with surfacing. In this case, let's select that bottom face
and start a sketch. And then I'm just going to
select that bottom edge. Go to the sketch tab and
choose convert entities. Now we have a line that goes
along that bottom edge. We can then use
this line to create another extruded surface
on the surfaces table. Let's choose extruded
surface and we'll go blind upwards 100
millimeters and press. Okay, now we see we have another third surface in
the surface, body's folder. Now we have two cubes in
the model from the outside. They're exactly
the same visually, but one of them was made using solid modeling and one
was made using surfaces. If we go back to our
cross section view, when we drag through the models, we can see the left
hand one is solid, but the one on the
right, as you would expect, is completely hollow. It's basically just made
of the outer shell. Again, if we go and check
the mass properties again, we can see the mass is
still the same as when we only had the first
cube, 7.8 kilograms. That's because, as we
said, these surfaces have got no thickness, So they've also got no mass. Now that we've got
the outer shell, we can actually
use these surfaces to create a solid object. We'll cover this in more detail as we go through the course. But in order to make these
surfaces into a solid, we need a completely
enclosed shape with no gaps. And then we need to do what's called knitting them together. To do this, we can go
to the surfaces tab. We can choose knit
surface, which is here. Then when the tool opens, make sure you're in
this selection box, it should be blue. Then we just need to select those three different
surfaces that we made. There should be the
two outer ends, and then we've got
the surface in the middle that's got
the four faces on it. Then here on the left,
let's check this Create solid box and
then just press okay. Right now we can see that our surface bodies
folder has disappeared. We don't have any
surface bodies anymore, but we've got an extra body
in the solid bodies folder. We've now got two solid cubes. Those surfaces
have actually been consumed in creating
this solid cube. Now if we go back to our cross section view and
we drag through, we can see both of the
cubes are completely solid. Also, if we go and check the
weight on the evaluate tab, we can now see we've
got double the weight, 15.6 kilograms, because
we've got two solid cubes. This is the general process
that we use in surfacing. This is a very simple
example, but in general, you build up an
outer shell using these surfaces that
has no gaps in it. And then you knit those surfaces together and you
can create a solid. We've seen how we
can use surfacing to create a solid using
this simple example. But the big question is,
why would you want to do that when it's so much easier just to use solid modeling and
create the same thing with one single feature in a process that takes
you about 10 seconds. As we said, this is a
very simple example. It's got very straight
geometric lines. But if we wanted to
create something with curves in
multiple directions, then surfacing is
really good for that. It's really powerful
for creating more curved, organic
looking shapes. Also, as I mentioned
earlier on in the course, your models don't have to be entirely solid or
surface modeling, they can be a
combination of both. So you might have
something like a really troublesome
corner that you're trying to get a nice curve on that you just
can't quite get. With solid modeling and
with surface modeling, you'd be able to do
that a lot more easily. I should also say at this
stage that it's quite important to understand the
limitations of solid works. The kind of models
where solid works really excels are generally more kind of mechanical with
quite geometric shapes. If you're looking to create something that's very organic, maybe like people or animals
or something like that, you might be better using a
different kind of program. Maybe something like
the Blender program. That's a free open source
three D modeling program. And it's very popular
and powerful. And it's used for lots of
things like animations. To recap this video very
quickly, with solid modeling, we create the solid
shape directly using sketches and things like
extrudes, revolves, and lofts. However, with
surfacing, we build up the outside shell
of the model first. And then we make sure we
have a shell with no gaps. Knit all those
different surfaces together and that allows
us to create a solid part. Surfacing is especially
useful when you're creating more organic
and complex shapes. And it can be very powerful
when you're making something that you
just can't quite get with solid modeling. In the next section,
before we jump directly into the
surface modeling, we're going to look at two kind of pseudo surfacing tools. That's the delete face
and the move face. These are very useful in
all kinds of modeling, both solid modeling
and surface modeling. If you don't have time to
complete the whole course, I'd recommend you at least
watch the next two videos. Because you'll hopefully
find something quite useful from
those two tools.
3. 3 Delete Face: Before we actually start with
the full surface modeling, we're going to have
a look at two tools which are technically
surfacing tools, but they're actually more
like standalone features that are very useful in
all different situations. They're both counter related and the names are quite
self explanatory. And they're called
the Delete Face Tool and the Move face tool. In this video,
we're going to have a look at the delete face. As the name suggests,
this tool deletes faces. It also allows you to easily
patch your fill faces. We'll have a look
at some examples. I've opened our previous model
with the two solid cubes. This can also be
found in the course downloads if you want
to follow along. If you're working with an
older version of Solid Works, there's also a step file version of it that you can import into solid works just by dragging that file
into solid works, and it should work
just the same. Looking at our cube, we left
the model in this state. The surface cube that
we created had been knitted together and it had
been turned into a solid. If we delete the
face of a solid, we will turn it back
into a set of surfaces. First, let's find
the delete face. Here it is, on the surfaces tab. If you can't find any tools
throughout this course, you can also search for them
up here in the search bar. Just click on the drop down and make sure you want commands. And then you start to type
in what you're looking for. For example, delete. And here we see Delete face. I'm going to click on
that to select the tool. Here on the left, we've
got the selection box. And we can choose which
faces we want to get rid of. But we've also got three
different options here. We can just delete, we
can delete and patch, or we can delete and fill. Let's just go with
the first option, just a simple delete. And I'm going to choose
this top face here on the left when a press. Okay, you can see that that
top face has been deleted. Now if you look in the
feature tree on the left, we can see we've lost
one of our solid bodies, but we've gained a surface body by deleting that part of the outer shell of
the solid cube, we've actually turned it
back into a set of surfaces, even though this cube
on the left was the one that we actually modeled
as a solid body, even if it's a solid body, if you delete one
of the outer faces, then you turn it
into a surface body. That's because
obviously if you don't have a fully enclosed space, then it can't
physically be solid. That first option that we
use, the basic delete. It can be useful in
certain situations. Maybe you say you want to add a curved surface on
the top of here, or you want to manually create a boundary surface or
something like that. But actually the really
useful part of this tool is how you can patch up these gaps that you create when
you delete faces. Let's move to the
second example model. So I'm going to
press control and Tab to go between
my open documents. And this file can also
be found in the course downloads as both a step
and a solid works file. So imagine this is
something you've been asked to
create by customer. Maybe it's an injection
molded cover or something. It's got a curve on
the bottom here. And you've sent it to
the customer you think you've finished and they come
back to you and they say, actually we don't want that
radius around the inside. Can you get rid of it? Or maybe can you change the size of it? Now the problem with this is if we look in the feature tree that inside fill it isn't
actually a separate feature. It's driven by the outer fill it and by the shell feature. We can't just
delete it directly. Maybe instead we could
delete the outer fill it and then maybe we could read a
fill it to just the outside. But actually imagine if you've
got a really big model, maybe you've got other
features further down the feature tree that are
linked to that fill it. And if you delete
it, potentially it's going to mess
up your whole model. You might also have
just been sent this file as something
like a step file. You might not have access
to any of those features. You might just have one single
imported feature there. In that case, you'd
have to somehow manually cut away that, fill it all the way around the inside following
that curved line. Maybe you could use
something like a swept cut, but it's not a particularly
easy process, luckily. We can use the delete
and patch option to do this pretty easily. To do this, let's open the
delete face feature again, here it is on the surfaces tab. This time let's choose the
delete and patch option. Then in the selection box, let's choose all of these
inside faces of the filler. There should be eight
of them in total. And now when we press okay, we can see those fillet
faces have been deleted. And they've been replaced by a nice square edge
around the inside there. So we could then use that to add a new fillet whatever size we want or we could
just leave it as that square edge if
that's what we want. When we use the delete
and patch option, the adjoining faces are
basically extended. This side face is extended down and then this inner face is extended outward
until they meet each other and form a nice
sharp edge there. That's delete and
patch. Let's have a look at the Delete
and Fill option. I'm going to edit
that delete face feature just by clicking on
it and pressing Edit Feature. And let's change it from
delete and patch to delete and fill and press Okay. You should now be
able to see that all of those inner surfaces, those eight surfaces
that we selected, have been replaced by
one single surface. But if you look at it closely, you can see it's not a very high quality surface in the corners. It looks a bit strange,
it doesn't quite join the rest of the body
at the correct angle. What we can do is just
edit that feature again. And then we can select
Tangent Fill, and press okay. This will mean that
the new face joins the existing edges or the
existing faces at a tangent. So it'll be a much nicer
face all the way around. Basically, delete
and patch extends the existing faces to
form a new straight edge. Whereas delete and
fill replaces those selected faces with
a new single face. We'll also have another look
at the differences between patch and fill in another
example in just a moment. But before we do that,
let's have a look at how else we could use delete
face in this model. Say for example you wanted to get rid of this
hole in the middle. In this model it'd
be really easy. We could just suppress or delete that center hole feature. But as we said before, you
might have other features further on in the model that
depend on that feature. It might be that you
want to actually keep the feature itself, but you just want to get rid
of the geometry of the hole. It might also be a
part that you've imported from a step file
or something like that. You can't actually manually edit the feature tree, in this case. You could probably manually fill in that gap using something like an extruded boss base and maybe the up to surface
command, just a bit of a FF. And there's an easier way to do it just by using
the delete face. To show this, I'm
going to select the delete face feature again. To remove that hole,
I'm just going to select this small
inside face here. We're going to select
delete and patch. When I press Okay,
what's going to happen is that blue
face is going to be removed and then these large faces on the
inside and the outside, they're going to be
extended and patched. If I press okay, you can
see the hole is gone and the face continues perfectly smoothly on the inside
and the outside. Hopefully you can see
the value of that in filling in holes
and openings. Now before we recap, we're going to have a look
at one more example. I'm going to go to the third
file in this selection. It's a part that
looks like this. It has a fillet all the way around the base of
this raised area, but it's actually quite
a messy fillet there. It's made up of quite a few
different small surfaces. What we can do with delete
faces, select the tool, and then we can select all of those curved faces around
the edge here, for example. We can choose delete
and patch and press. Okay. And you see we've now got that nice straight edge
all the way around. So we could either leave
that straight or we could add a new fillet
with a different size. We could also, if I edit the feature and change
it to delete and fill, we could replace all of those small faces with one single face all
the way around. That will make it a nice, smooth surface all the way around. Now, just one thing
to note is that the automatic
patching or filling doesn't always work
in every situation. If you've got quite
complex geometry around the surface
that you're deleting, then the automatic patch
might just completely fail. Or it might give you a
really weird surface which bulges out in different directions and
isn't what you want. In those cases, it's
best just to use the basic delete and just
completely delete the face. And then maybe you
can manually create a patch using something
like a boundary surface. We'll cover how to do that a little later on in the course. To recap the delete
face feature, as the name suggests,
it deletes faces. However, it also allows you to patch and fill those faces. If you fill a face,
it tends to replace multiple surfaces with one
single smooth surface. But if you patch a face, then it will generally extend the surrounding faces and give
you more of a square edge. There's tons of different ways that this tool can be useful. In particular, it's very good
when you're working with imported parts where you
can't edit the feature tree. It's also very good for things like removing and adjusting fillets and removing
holes and openings. In the next video,
we'll have a look at the move face tool which is related to this Delete face tool and it's also extremely useful.
4. 4 Move Face: Welcome back to the course. In the last video, we had a look at the delete
face feature. There's also quite a
similar tool that can be used in all kinds of modeling
and is also very useful, and that's called
the move face tool. Let's open this example file. And it's just a simple bracket, maybe it's a sheet
metal bracket, but let's say we've imported it from something
like a step file, so we don't have access
to any of the features, so we can't edit the
features directly. If we want to make fairly
simple changes to this model, then it won't be
that easy really. But thankfully, we can use the move face feature to
simplify these changes. Now you won't find
the move face tool on the surfaces tool bar. It's actually in
the Insert menu. Insert Face Move. But personally, I use
it so much that I've added it to my toolbar
as a shortcut. To do that, you can go up
here to this search box, click on the drop down and
make sure you're on commands. And then just start to type in move so we can find move face. But instead of just
clicking on it to open it, let's left click
and drag it and put it somewhere on the command
manager, somewhere like here. We've now created a shortcut to that tool that you
can use any time. And then I'm going to
left click on that, move face to actually
open the tool. Here on the left, we've
got a selection box at the top like you have with
a lot of different tools. And we've also got three
different options. So we've got offset,
translate, and rotate. Let's have a look at the
first one which is offset. If we choose this and then we select a face like this one, we've got an offset distance
of 10 millimeters selected. So we're just going to offset that face outwards
by 10 millimeters. For example, I can select
different faces like this, and in this way we can increase the overall size of the part. You can also flip the
direction if you want to offset in the other direction
and make the part smaller. And you can do that
just by pressing flip direction down here. If we wanted to make it smaller, it would look
something like this. So that's the basic
offset feature. I'm just going to delete
that feature so we can have a look at
another way to use it. It's also really useful for
adjusting the sizes of holes. So for example, if we wanted to make this hole
bigger or smaller, if we made this part
in solid works, we could just adjust the
whole side directly. But because we don't have that
feature, we can't do that. We could maybe fill
it in manually and then recut a
different size hole, but we can actually just use
the offset face instead. To do this, we can just
choose that inside face. And then we can set the
offset distance that we want. You can see on the preview,
nothing has happened. That's because the offset
that's currently set 10 millimeters is too
large for this hole. So let's change that
distance to say two. And now we can see the preview. That will make the hole
2 millimeters smaller. And if we flip the direction, it'll make the hole 2
millimeters bigger. So we could say, let's
make it smaller like this. And we've now just
easily and very quickly reduce the
size of that hole. The next option, if I go back to the move face command,
is the translate. This allows us to translate or move faces in
different directions. Let's choose any
phase, say this one. And then we can
just move it using these arrows in any direction. You can also directly write in the translation amount
down here on the left. So you can translate
in x, y, or z. If you're not sure on the
direction that you're going in, you can look at this little
triad or you can just pull the actual face using those orange arrows
in the graphics area. The translate can
be really useful. Say for example, we wanted to make this whole bracket longer, but we wanted to
keep that hole in the same place relative to the left hand side of the part. We could actually select
all of these edges, including the curved edges and we could translate
out to the side, say for example, like this. You can also set end
conditions here on the left, so you can do things like up
to face using this box here. You can also set a specific direction
for the translation. If you don't want to go
in the XY direction, you can click in this box. And then you can select an edge. Say if you wanted to make
the translation at an angle, then I'm just going to delete that offset feature
so we can have a look at the final
option, the Rotate option. If I open the tool again and
choose rotate this time, and then I'm going to
say that top face again, we can rotate in
the XY direction using a number of degrees. You can also set
the rotation point. If you select a face, the point selected will
automatically be at the center of that face that
you can move it manually. You can also drag your
rotation around using these circular sliders
here in the graphics area. You can do a combination
of different angles. You can make a composite
angle like this, as well as moving where
the rotation point is. You can also click in this
box here on the left. And then you can choose a
specific axis of rotation. You can choose, for example,
an axis or an edge. Say for example, I could
choose this edge here. And then we're just going
to set an angular amount to rotate the face around
that edge that I've selected. Hopefully, you can
see that this tool, the move face tool, is
quite a simple tool, but it can be very, very useful, especially when you've
got these imported parts. Just one thing to
note, with this tool, you might have to
have a little think about your design intent. Say for example,
we had this part in an assembly and it was mated to another part using a mate that was on
the end face here. If we then use the move
face command on this face, then the mate would still apply, but to the new
position of the face. If we moved this face inwards, then the actual position of your part in the
assembly would change. Just to give another
example of that, let's say on this
part we wanted to add another hole
somewhere like this. Let's make it 80 millimeters
from this end face. If we then later on decided
that maybe this part on the left is too long and we went back and we
moved that face. If we created the
move face feature before the whole feature. So if I got my moved face again, select this face and
moved it inwards, say 20 millimeters and then we drag back after
the whole feature, that 80 millimeters
that we set for the hole will be from the
new position of the face. So you can see the
hole has disappeared there because it's right on
the edge of the part here, but it's still 80
millimeters from the face. But that face has now moved. The position of
the hole relative to where it was
has moved as well. That's probably a fairly
obvious thing to say, but just to let you know
that if you move faces, it can affect your
other features if they're pointing to
those faces as well. That is the move face tool, a very useful one in both surface modeling
and solid modeling. You can find it in
the Insert menu under Face and then Move, Or you can just put it as a shortcut directly onto
your command manager. You can use it to offset
things which is move them outwards or inwards
including holes. You can also use
it to translate, which is move things in x, y, or z directions or any
specified direction. And you can also use
it to rotate faces. So it's a very useful
little tool that one. In the next video, we're
actually going to start using some surfacing to
make a surface model.
5. 5 Extruded Surfaces 2: We're now going
to actually start creating some models
using surfacing. Over the next few videos
we're going to build this. It's a candlestick holder, it's quite an abstract model
and it's fairly simple, but we'll use this to learn
some basic techniques. And then in the next section, we'll build upon those so we can create something more
complex and more useful. Let's get started. Let's open a new part and start a
sketch on the top plane. Get the circle tool, and let's put a circle at the origin. And use Smart
Dimension to give it a diameter of 20 millimeters. So we have a circle at the origin that's 20
millimeters diameter. And we're now going
to use this to create the stem of the
candlestick holder, similar to when
we made the cube. Let's go to the surfaces tab. Let's choose extruded surface. And we're within the sketch, so you should automatically
just get this preview. We're just going to
do a blind extrude upwards 80 millimeters
like this. And then press, okay. We now have a closed profile,
which is that circle. And we basically made a surface, that's a tube that goes upwards. This is the upright part that the candle will
actually fit into. Next up, we're going to start
creating a curved dish, and this will collect
all the melted wax as it runs down the candle. We want to start a new sketch on the plane that cuts
through this tube, and that is the front plane. Let's select the front plane, start a new sketch and
go to a normal two view. You don't have this
view menu. You can just press the Space bar
and it should pop up. And you can choose normal two, or you can choose
the front view. And either one of those will
take you to the same view. Now we just want to draw a simple arc to create
this curve dish. But before we do,
we're going to add a center line just to help us line up the
rest of the sketch. Let's go to the sketch tab. Go up to the line tool and click on the drop
down next to it, and then select center Line. Then we're going to
draw a center line from the midpoint at the top of the tuper all the way
down to the midpoint at the bottom where the
origin of the part will be, where those two little
red arrows are. That center line should
be fully defined, if it's midpoint at the
top and the bottom, if you're not fully defined, you might just have to
drag one of the end points around to pick up that
automatic relation. Next we'll get the Arc tool, which is also on the sketch tab, and we'll select a
three point arc, which is this last option here. And then we'll just start to draw an arc,
something like this. It doesn't have to be
exactly right at this stage, because we will add the
dimensions in a moment. Start on the left hand
side with the first point, and then add the second point
on the right hand side. And then just make sure it's
curved downwards like this. It should look
roughly like this. And we can now start to add some relations and dimensions. First up, we'll make the arc symmetrical left click to
select this first point. And then hold down control. And then also select
this right hand point. And then keeping
control held down. Also select the
vertical center line. You can then release
control and we'll choose make symmetric
from the pop up menu. You can also choose it
on the left hand side. That's just going to center
the arc on that center line. Next up, let's add the
radius of the arc. So I'm going to get the
smart dimension to, I'm going to click on the arc, and let's add a radius
of 120 millimeters. If your arc moves around, you can always
just drag it up to roughly the correct
position about here. Then using the smart
dimension tool. Again, let's start from the bottom end of the
construction line, where the origin is and then let's set a distance
to the bottom of the arc. So when you select the
bottom of the arc, you'll have to hold
down the shift key and that will allow you to
dimension to the arc. And then we'll set
a distance there of 65 millimeters like this. The arc should be
almost fully defined. Now we've just got to set
the width of this dish. To do that, we'll use the
Smart dimension one more time. And we'll set the width between these two points as
120 millimeters. And that should fully
define the sketch. So all the points of the
line should be black. If anything is still blue, it means it's under defined. So you might just need to add some more relations
or dimensions there. And then if we look in three D, we've got that upright tube, and then we've also
got this single arc, which we're going to use to create the surface for the dish. At this point, we're
still in the sketch. We haven't exited the sketch
and we can go directly to the surfaces tab and we can
choose extruded surface. Again, you should get
preview, something like this. Let's set the width
as 100 millimeters. And this time instead of blind, let's choose mid plane. For the end condition,
you should have something like this.
And then press. Okay. And that surface is created. Now we can see we've got two
different surface bodies. We've got that upright tube and we've also got that
curved dish on the top. In the surface bodies
folder on the left, we can see we've got those
two different bodies. They're both separate
to each other so they're not
connected in any way. You can see when we're
creating these surfaces, we can either use
a closed profile, like a circle, or we can use an open profile like the
arc we use for the dish. That's it for this
video. We've made a pretty simple model so far. To quickly recap, we just drew a circle and then we extruded that upwards to create
this tube shape. And then after that,
we sketch the arc, and we extruded that using mid plane to create a
surface for the dish. In the next video,
we'll have a look at the trim surfaces tool. And we can use that to trim away the areas of
the surfaces that we don't want so we get closer to the final end
shape that we need.
6. Trimming Surfaces: In the previous video, we made the basic shape of this
candlestick holder. In this one, we're
going to look at the trim surfaces
tool that will allow us to trim those surfaces so they're closer to the
final shape that we want. Let's get started with
our previous model. And you can also open this using the exercise
files for this section. First up, we want to
around the edges of this rectangular section,
so they're not square. If this was a solid model, we could just use the
fillet tool and we could add some fillets to the
edges in the corners. But because this surface doesn't have any
thickness to it, there's actually no vertical
edge there to select. Instead, we have to use
the trim surfaces tool. There's a few different
ways we can do this. We'll start off by
showing you how you can use sketches to trim things. Let's start a sketch
on the top plane and I'm going to
go to the top few. We're looking down from the top. This rectangle here is
the curved disc shape. I'm going to left
click to select that. Then from the Sketch tab, let's choose convert entities. We've now converted
the outer edges of that surface into new entities
or lines in the sketch. But the sketch is actually on the plane that we selected,
which is the top plane. If you look in three
D, it looks like this. We're now going to use
the sketch fill it tool, which is this one. And we're going to fill it, the outer edges of
that rectangle. Let's set the size of
something like 45. And select those
four outer corners, so they're rounded off like
this. And then press okay. And then we've got
a shape like this, which is basically
like rectangle, but with the rounded corners. If we look from the top,
it looks like this. We want to cut
away these corners outside of the rounded
part that we've sketched. To trim the surfaces, we're going to go to the surfaces tab. We're going to choose
the trim surface tool, which is this one. We can see firstly for the trim type, there's two options. There's standard
and there's mutual. We look at these in
turn, but basically, standard lets you trim surfaces with things like sketches, other surfaces, curves,
planes, and so on. But with mutual, you
can actually trim multiple surfaces
using those surfaces themselves and we'll look
at that option next. For now, we'll just
stay with standard in the trim tool box. We want the sketch
that we just drew. It'll probably
automatically be there. If it's not, you might just have to click in this selection box, the trim tool box, and then left click to select that sketch
in the graphics area. Then down here we've
got two options. We can either keep selections or we can remove selections. In this case, let's use the
removed selections option and then make sure you're
in this box underneath. Then if we go to the
graphics area and we basically hover the
mouse over the surface, we can see different areas get highlighted based on the shape
of the sketch underneath. So what we want to do is click the areas that we
want to remove. So I'm going to left click on these corner sections,
all four of them. And as we select them, you
see they become highlighted. And they also go into
this box on the left, which is the areas to remove. And then when we press okay, those highlighted areas
are removed like this. And we've got a nice
curve shape on the top. We've now trimmed away
those corners like that. Next up, let's trim away the
top of the tube here again, we're going to use
the same feature. We're going to use
the trim surface. We're going to stay
on standard again, but this time
instead of choosing a sketch for the trim tool, let's choose actually
that top surface. We're going to stay
on Remove selections, then make sure you're in the
selection box underneath. And then just hop your
mouse over the tube. And we want to left click and select that top
part of the tube. That part will be removed
when we press okay, like this, we're getting a bit closer to the
final shape now. But what we also
want to do is remove this circular area where
the tube joined the dish. That's where the candle base actually fits in, so
we need a hole there. Again. Let's go to
the trim surface, but this time instead of
standard, let's choose mutual. With the mutual trim,
you can basically trim multiple surfaces
using those surfaces themselves in the surfaces box. Let's choose both of
those existing surfaces. And then let's stay
on Remove Selections. Let's click in the
selection box underneath. And then hover over
the graphics area. Basically, we want to remove this little circular area where the two surfaces
join each other. Left click to select
that if we press okay. We've now removed that area. With that mutual
option, you can trim the surfaces where they actually meet and where they
touch each other. That's the surface trim tool, as you've probably
noticed so far, similar to quite a lot
of solid works tools, the actual tools themselves
are fairly straightforward. The actual basic building
blocks are quite simple really, but you can use
these to build up more complex models and
shapes step by step. To recap the trim surfaces tool, it lets us trim surfaces
using things like sketches, planes, surfaces, or curves. Or we can use that
mutual option, and we can use multiple
surfaces to trim themselves. In the next video, we'll
develop this model a bit more by adding a base using
the ruled surface tool.
7. Ruled Surface: This was how we left our model. In the previous video, we had trimmed away some of
the excess areas of the surfaces that
we didn't need and it looks like our
candlestick holder. But if you tried to
use this in real life, it would probably fall
over because it doesn't really have a base,
it's top heavy. To fix this, we can use
the ruled surfaces tool. This can be found on the
surfaces tab. Here it is. And as you can see, we've got quite a few different
options here. Probably the best thing to do is first let's select an edge. And then we can run through what these different options do. Down here in the
edge selection box, I'm going to choose this bottom circular edge for the distance. Let's set 20 millimeters just so we can see what's going
on nice and clearly, basically the ruled surface
makes a new surface that extends outwards from
the selected edge in a specified direction. If we look at the preview, we've added this yellow
area at the bottom. So we're on the first
option tangent to surface. So we've basically added that 20 millimeters tangent that's directly in line with the selected edge and the
surface that joins it. The next option is the
normal to surface option. And as you can see now we
flip the surface 90 degrees. It's now normal or perpendicular
to the edge and surface we've selected because this is quite a simple vertical tube, and this is quite
an obvious example. This base would
be pretty easy to add just using an
extruded surface. But imagine if you have
a really wavy base here. This tool could be quite useful in following the edge around. If I press okay, we could
just add a base like this. I'm going to go back and
edit that ruled surface feature again just by clicking on it and
pressing Edit feature. And then we can have a look at the remaining three options. The next one is called
tapered to vector, and if I select that, we can see nothing happens
on the preview. That's because we
first need to select a vector instead of just
going normal or tangent. In this case, we can select a specific vector and then we can set the angle
to that vector. I'm going to click in this
box, the reference vector. And we don't really have any suitable straight lines
or edges in this model, but you could choose
an edge if you did. In this case, we're
going to use a plane. I'm going to extend this
second feature tree and I'm going to
select the top plane. We're now creating a
new surface which is 20 millimeters in length and three degrees to
that reference edge, which is the top plane
that we selected. We can change the angle here to make it a bit more obvious. Let's say maybe let's
set it as 45 degrees. And you see we're now going
45 degrees to that top plate. This one can be really useful for adding things
like draft angles. Let's press okay to add that. And then we're going to
use this new feature to demonstrate the
final two options. Let's select the ruled
surface feature again. This time for the edge. Let's
choose this new outer edge. If we run through the
first two options, you can see tangent to surface
extends along the surface. Tangent, so it's directly
in line with the surface. Normal to surface is 90
degrees to the surface. Like this taper to vector we just added
for the fourth one, perpendicular to vector.
Let's select that. Again, we need to
choose the vector. This time I'm going to
choose the top plane. Again, we can see
the extension is now perpendicular to the
direction of the arrow, to the direction of the vector. Then the final option is sweep. This will sweep the edge you've selected along a
specific vector. You can also click the
coordinate input here, and you can change exactly
how the input works. And that will change the exact
direction of your sweep. In this case, if I just turned
off that coordinate input, the sweep would just
go directly upwards. Now because this is a
fairly regular shape, you might not be able
to visualize some of these directions and options
quite as well as you could. Let's have a look at
a different example using a bit more of
an irregular shape. I'm going to press control
tab, change to this model. If instead maybe we
had a shape like this, almost like a Pringle shape. We select the ruled surface
and choose the outer edge. I'm just going to set
the distance as say, about 200 so we can see
exactly what's going on. For the tangent to surface, we're following the
surface exactly. We're basically extending
it and keeping a nice, smooth outer surface and curve there for normal to surface. We're extending
upwards at 90 degrees. If we turn it to the
side, it looks like a sailor's hat or
something taper to vector. Again, I'm going to set the
top plane as the vector. And we can obviously adjust the angle here and change
it to whatever you want. This one is particularly useful
perpendicular to vector. In this case, it gives a
really strange squash shape. But if we change the vector
to another plane like this, then we can see it gives
a much nicer shape, maybe closer to
what we want often. It's really just
a case of playing around with these
different settings and finding the one that suits exactly what you
need for your model. Then finally, with
sweep, as we said, you can change the
coordinate input, so you can change
the direction of the sweep to whatever
you need for your model. It's really a case of
exploring the settings and just finding what works
for your specific model. If we go back to our
candlestick holder, now I'm going to delete this ruled surface
that we added before, and I'm going to add a new one. We're going to select that edge, let's go normal to surface,
which is this one. And further distance. Let's just set 25 millimeters and press. Okay. And we've now added
a base there very easily. And also if you turn
the model over, we can see we've still got
that hole in the bottom. So to recap, the ruled
surfaces feature, it allows us to extend a surface
in a specific direction. There's five different options. They could all be useful
in different situations, especially if you
have more complex, nonstandard geometry. And you can play around
with the settings to find something that works for
your specific model. In the next video,
we'll finish off this model by having a look
at how you can add fillets, and we'll also look at a
different way that you can create a solid model
from these surfaces.
8. Fillets and Thicken: This was how we left
the candlestick holder. We've got the basic shape
there that we want. We've trimmed away some
sharp edges and parts that we didn't want and
we've added a base there. Now we want to round
off some more of these sharp edges using fillets. And we'll also look at a
different way that you can make this surface
model into a solid. Let's say we wanted to
fill this top edge here. If this was a solid model, we'd actually take
away some material when we make the fillet there. But we can't really
do that in this case because we've got no
thickness to these surfaces. If we took away an edge there, it would just leave us a gap. Luckily, there's a fillet tool,
especially for surfacing. However, before we get there, we can see that we've got three different surfaces
and they're all separate. Up here in the surface
bodies folder, we can see there's three
separate surfaces. You might remember
from solid modeling that you can't add
a fill it between separate bodies first
we've got to join them together somehow
with the surfaces. We can do this using
the knit feature. Let's go to the surfaces tab, choose knit surface, and then let's select all
three of our surfaces. We don't need any of
these options selected. So you can uncheck all of
those and then press Okay. And now we've got
one single surface. There's a combination of those
three previous surfaces. We can now use the fillet tool. Let's go to the surfaces, tap and let's choose fill, and let's say add a ten
millimeter fillet to these faces. You can choose either the inside edge or the outside edge. It doesn't make any difference
because like we said, the surfaces have
got no thickness. Whether you choose the
inside or the outside, it will give you the
same end result. The fillet tool parameters
are pretty much the same as the normal fillet tool
from solid modeling. With all the
different options for types of fillets and everything. Let's set that ten
millimeter one and let's press okay to add
those two fillets. Now we basically have
the shape that we want, but because it's made of
surfaces, it's got no mass. We won't be able to
three D print this or machine it or
really do anything with it apart from maybe make some basic renderings until
we make it into a solid. You might remember
from the cube video, we said that to make a solid you need an outer shell
with no gaps. And then you need to knit
all those surfaces together. But in this case, we
haven't really got an outer shell because we've
just got that overall shape. But with no thickness. For models like this where you don't really have
an enclosed space, there's actually another way
that we can make them solid, and that's using
the thickened tool. This will basically take
a surface and it will give it thickness. Let's
have a look at that. Here it is on the surfaces tab, it's called thicken and
it's quite straightforward. First, we need to just
choose the surface. We've only got one in the model, Let's select that then. We can choose the thickness. I think 1 millimeter
is good for this one. Then we can choose to either add the thickness to the
inside, which is side one, to the outside side two, or to both sides evenly
like a mid plane. Although technically this is
called thicken both sides. Let's go with that one thick on both sides and let's press. Okay. Now we can see our
surface model has been made into a solid model that's 1 millimeter thick,
all the way around. We can see here the solid
body's folder has appeared. We've got one solid body. The surface, body's folder
has disappeared because those surfaces have been
consumed making the solid body. We can also go to a
cross section view and we can see as we
drag through the model, we've got that 1 millimeter thickness everywhere
in the model. That's the candlestick
holder, pretty much finished. You could maybe add
some fillets around these outrages just to
smooth them off if you want. It's quite a simple model, but hopefully it's showing
you some basic techniques that we can use to build
more complex models. To recap this video,
we wanted to add some fillets to the model,
but before we could do that, we had to first join
the different surfaces together using the
kit surfaces command. We could then use the fillet
tool from the surfaces tab. This is very similar to
the normal filip tool that hopefully used a lot of times
in normal solid modeling. Then finally, to make
the surfaces solid, we used the thickened tool. To use this, you can just select the surface
you want to thicken, then you set the
thickness value, and then you can choose
whether you want to thicken on the inside or the outside
or equally on both. That's a really
easy way to convert your surfaces into solid models. In the next section,
we're going to look at some more advanced
surfacing techniques, things like sweeps, lofts,
and filling surfaces. And we'll be making
something like this, which is a host
pipe spray ahead.
9. 9 Revolved & Lofted Surfaces: Welcome back to the course. In the last section, we
looked at the basics of surfacing things like extruded
surface and trimming, as well as knitting
and thickening. In this one, we're going
to start to look at the more advanced techniques and we'll be making
something like this. Maybe it's a paint sprayer
or a hosepipe head, or maybe some kind
of prop for a film. Maybe an advanced
gun or something. But as you can see, it's a
pretty unusual shape really, and it would be hard to make
with normal solid modeling. In this video, we're
going to look at the revolve surface and
a basic lofted surface. And then in the next one we'll start to
look at sweeps and then filled surfaces and more
detailed lofts later on. So let's get started
with a new part. Start a new sketch
on the front plane, and then get a center line from the drop down next
to the line tool. And let's draw a
center line going straight up vertically
from the origin. You don't have to set a length, this will just represent
the center of the part. Then we'll just get
a normal solid line and draw a little
zigzag shape like this. So we'll go vertically up, we'll go inwards a little bit, and then vertically up again,
and then outwards again, and then vertically up
again for a third section, and then we'll add some
relations and dimensions. Let's make this lower point
horizontal with the origin. You can do this by
left clicking on it. Then hold down Control and
also select the origin. And then release control
and press Horizontal. Then let's also select
these two outer lines. And we'll make those co linear so they're lined up
with each other. Next up, let's get the
Smart Dimension tool and set some sizes. Click on this lower
vertical line and then click on
the center line. We want the total
diameter distance. We want to set it
as 35 millimeters. If you select that line and the center line and you
move over to the right, you should get that
diameter distance. You could also set this distance just between the center
line and the line itself. That will be 17.5 It would
give you the same position. And then let's do the
same for this one, except let's make
that 30 millimeters. And then these three
vertical sections, let's set the lower
one as 10 millimeters. And then let's select
all three of them. So hold down control
and select them. And then just press make equal they're all the same
length, 10 millimeters. That should fully
define your sketch. If you don't see
fully defined down here and one of your
entities is still blue, you might just need to
add a few more relations or dimensions to make
it fully defined. We're now going to
use this profile to create the revolved surface. The tool is found on the
surfaces tab. Here it is. It's the second one,
Revolved Surface. If we click on that,
we can see it's very similar to a
Revolved boss base. I selected the tool when I
was already in the sketch, so we've automatically
got this preview. If you can't see the preview, you might just have to select the sketch that we just drew. So as you can see,
and as I said, it's very similar
to the revolved boss space here on the left. We can choose the
axis of revolution, that's where the profile
will be spun around. And in this case,
that's automatically been chosen as that center
line that we added. You can revolve either in one direction or two directions. By default, it's a full
360 degree revolution, but you can set it
to a smaller amount if you want to revolve
in two directions. So you can do those
partial revolutions, but we don't need
that for this case. Let's keep it as 360 and press okay to
create our revolve. So you can see it's a
very simple tool, really. We've just revolved that
profile around a center line. The next tool we're
going to look at is the lofted surface. This creates a shape from
a series of profiles. Firstly, we need to draw
those separate profiles. Before we do this, let's add some new planes to
help us with it. Let's select the top plane, then let's go up to
Reference Geometry. This should be on
the Surfaces tab. It's also on the Features tab. You can get it from
there. Let's go reference geometry and
then select plane. You don't need to change
any of the selections, we just need to make sure
we have top plane here and let's set the distance
as 30 millimeters. When you press Enter, you should see we've got
a new plane which is at the top of that revolve and it's parallel
to the top plane. We've got the first new
plane there, plane one. Then let's select that new plane and then do
the same thing. Let's go to reference
geometry plane. This time let's set a distance of 50 millimeters and press. Okay, we've now added a second plane that's
parallel with that first one, but 50 millimeters above it. And then let's select
that second one that we just made and do
exactly the same thing. Again, select the second one, reference geometry planes,
and we'll set a new one, 50 millimeters above that. We've now got three planes,
something like this. And we'll use these to create
the profiles for our left. Start sketch on the
lowest one plane one. Just click on it
and press Sketch. And then I'm going to
select the top edge of that revolve that we made. And I'm going to press
convert entities, which is on the sketch tap. This will make that
edge into a new circle that's on the plane that
we've selected, plane one. That's all we need
for that sketch. So let's exit the sketch then. We'll do a similar thing on the uppermost
plane, plane three. Select plane three,
Start a sketch, and then choose that edge
again of the revolve, and again press convert. This will convert that edge into a new circle on
that plane three. You can then exit that sketch, and then for the middle
one we also need a circle, but it's going to
be a bit larger, so let's just start a
sketch on that plane two. We'll get the circle tool
with a center point circle. And we'll draw a circle
at that origin point. And let's set the diameter
of it as 75 millimeters. And you can then
exit that sketch. We now have these
three different circles on the three
different planes, and we can use these
to make the loft. To do this, let's
go to surfaces. Lofted surface, similar to the revolved surface feature
and the revolves space. This lofted surface is very
similar to a solid loft. What we need to do is just
select the profiles in order, make sure you're in this
selection box on the top. And then just select
the profiles in order from the
bottom to the top. You should get preview
something like this with a nice
smooth line like this. These green connectors should ideally be lined up as
straight as possible. If you end up with a
preview, say for example, something like this where
it looks really twisted, you can move these
green connectors manually to try and fix it. But usually it's easier just to completely
clear the profile. And then when you select
the profiles, again, try to click on roughly the same position on each profile. As I click on each profile, I'm on the left hand
side front area there, so it's roughly about the
same place on each profile. And that should give you a
nice smooth curve there. You can also just move
the green connectors a little bit if it's
still not quite lined up. And you can also use
specific guide curves if you want to follow a
really specific line. But in this case, I don't
think we really need it. The preview looks
okay at the moment, but if we look at where the
loft joins the revolve, it's a sharp edge at the moment. We want a bit of a
smoother transition there. We can scroll down here and we can expand start
end constraints. For the start constraint,
I'm going to change it from default to
normal to profile. You see that changes the
shape of the preview. It now means that the loft joins the revolve with a much
nicer transition there. You can also adjust
this value here. I'm going to change
it from one down to 0.5 The transition isn't
quite as long there. And then I'm going to do
the same for the top one. For the end constraint,
I'm going to say it as normal
to profile and put the value as 0.5 The preview should look
something like this, so you can press okay to
make that lofted surface. We now have two surface bodies. We've got the revolve
at the bottom and then we've got
the loft at the top. If we look at a cross section, we can see the loft
probably could have just been an
extension of the revolve. We could have just extended that sketch profile that
we used to make the loft, and we could have
maybe used a spline to create this top shape. That's because the loft shape here is completely circular. It's symmetrical about
that center line. But if it, instead, it was oval, or it was flattened or
squashed a little bit, then a loft would
be better for this. But I just wanted to show that as with a lot of
things in solid works, there's different
ways that you can achieve the same end result. So that's the very start
of our sprayer model, and you can save your
part there To recap, the revolved surface
is pretty simple. All it does is take
a sketch profile and it revolves it
around a center line, similar to a normal
revolved boss base. In solid modeling for
the surface loft, we use a number of
different profiles. So first we added some
different planes, and then we sketched different
profiles on those planes, and then we used the
loft to connect those. When you select the profiles, make sure you select
them in order, and try to make sure you select roughly the same
position on each profile, and that will help avoid
your loft becoming twisted. You can also manually adjust the shape using those
green connectors. Or if you need a
bit more control, you can use guide
curves. There we go. It's quite a simple start. In the next video, we're going to build on this
further by using swept surfaces to add
a nozzle and handle.
10. Swept Surfaces: This was how we left
our sprayer model. We had the lower connector area, which was a revolve, and then we had this bulb,
which was a loft. Next up we're going to make
a handle and a nozzle, both using swept surfaces. Let's start a sketch
on the front plane, and we'll draw a center line
upwards from the origin. And then let's add two
points using the point tool. One of them is on
the center line and the other one is out here
to the right somewhere. Then we'll get the
smart dimension tool. This first one is 230
millimeters up from the origin, and then this next one is 240 up and it's 72 millimeters
from the center line. They should both be
fixed like this. Then we'll get the splying
tool and we'll just draw spline between
those two points. Like this. You can then press Escape to
exit the Spine tool. And then left click on
the spline itself and use these little handles to drag it around to give it a
slight curve like this. Now if you don't
see those handles, you might just need
to turn them on. You can do this by
clicking the options up here and then in the
box type spline, we're looking for
this option that controls whether you can
see the spline handles. Just make sure that you
have a check in this box. Enable spling, tangency and curvature handles.
And then press okay. When your sketch looks
something like this, let's exit that sketch and
start on the next one. Again, it's on the front plane. Again, we'll add two points
in roughly this position. And then we'll get the
smart dimension tool. This one is 175
millimeters upwards, it's 32 from the center line. Then this one is 75
millimeters from the center line and it's
220 millimeters upwards. Then again, get the spline tool, join the two ends
of those splines. Then click on the spline
itself and adjust the handle so you've got a bit of a curve, something like this. And try to make
sure it's not too tightly curved near to
the end of the spline. It should be something
like the video. These two splines will be the top and the
bottom of our nozzle. And we now need to draw the
actual cylinder profile, which will be the nozzle itself. To do this first, we
need to add a new plane. To add this plane, let's first pre select the front plane, so left click on it, and then go to Reference
Geometry Plane. As we said in the last video, this is on the Surfaces tab, but it's also on the
Features tab as well. We should have the front plane here for the first reference. Then for the second reference, click in this box and then choose the endpoint of
one of the splines. And then for the
third reference, choose the endpoint
of the other spline. You should get a preview.
Something like this. Press okay to add that plane, and then let's start a
sketch on that plane. Then let's choose a
center point circle. Draw a circle
roughly about here. The exact position isn't too
important at the moment. Then we just need to
connect that circle to the splines left click on
the end of the top spline. Hold down control and
also select the circle. And then release control
and press coincident. Then do the same on the bottom. Select the end point
of the spline. Pull down control,
select the circle, and then release control
and make those coincident. And you see the circle isn't quite centered on
the splines there, So what I'm going to do is select the center
point of the circle. And then select the end
of one of the splines. And just press vertical, and that should
line the circle up, should make it fully defined. And you can exit that sketch. Now you can see a wire frame view of what
we're going to do. We're going to sweep that
circle along those two splines, but it will follow those
splines as it goes to the left. The circle will get larger. To do this, let's
go to the surfaces tab and choose swept surface. This is very similar, again, to the swept spas base. We want to choose
a sketch profile, and then for that profile, we'll choose that
circle that we drew. Then for the path, let's
choose this top spline. So we can see we're
just sweeping that circle along
that top spline. But actually we want to use
the bottom spline as well. So to do that, we can expand this guide curve section
and then click in that box. And for the guide curve, let's
choose that second spline. So you should have a preview.
Something like this. If yours doesn't quite work, you might need to go out of
the feature and then just adjust your spline so they don't have any really
tight kinks in them, especially near to the ends. If you get really stuck, maybe you can try just deleting the spline and then
redrawing it again. And try and copy a similar
curve to what the video has. The preview looks pretty good,
but before I press okay, I'm just going to go
down here to curvature display and then turn
on the mesh preview. And I'm going to increase
the density so we can see exactly what's
happening with this mesh. As we zoom in, that
all looks okay. We've got a nice
smooth curve there. If you expand this option,
start an tangency. If you had a different
kind of tangency, for example, like path tangent, you might find that the
end of your surface is all wrinkled like this and
we don't really want that. So I'm just going to
turn off all of this, start an tangency, and we've got a nice
smooth curve there. So let's press okay
and make that surface. We've now created the nozzle, and next up we're
going to use a similar process to make a handle, but just use a bit more
of a complex guide curve. Again, we'll start a
sketch on the front plane. I'm going to go to
a normal two view, going to get the point tool. And I'm going to add
two points again, these ones should be up
to the left hand side. The lower one is 85 millimeters upwards and it's 150 from
the origin to the left. Then the upper one is
165 millimeters up from the origin and it's 120
millimeters to the left. The top one is 120, 165. I'll just move these around
so it's a bit easier to see. The bottom one is 150.85, We can then join these points, but this time
instead of a spline, we'll just use a
three point arc. Let's get three point arc tool, join those two endpoints, and just make an arc that goes outwards,
something like this. Then get the smart
dimension tool and set the radius as 500 millimeters. That should now be fully defined and it should
look something like this. And this will be the
back of the handle. We also need a similar sketch for the front
of the handle. Let's exit this sketch, start a new sketch also
on the front plane. The first thing to do is offset a line from this previous
sketch that we just drew. If you can't see that
previous sketch, you might just need to
go to the feature tree and click on that
sketch and press show, make sure that it's visible. Left click to select that first line from the
previous sketch. Then from the sketch tab,
let's choose offset entities. And let's offset 45
millimeters inwards like this. We also want the offset line
to be a construction line. Before you press, Okay, down here under
construction geometry. Just make sure there's a tick in the offset geometry
box. And then press. Okay. So we've got
construction line that's parallel to
that first line, but 45 millimeters away. If you have any problems
with that offset line, sometimes the offset tool
is a bit temperamental. So if you do have
problems first, you can try converting that line from the
previous sketch, and then you can offset
from that converted line. Just make sure that
both of the lines in your sketch are
construction lines. We've created that
first offset line, now we want another
offset one as well. Let's select that
new offset line that we made, the
line on the right. And then we'll click
Offset Entities again. This time we want 6 millimeters and we want to offset
to the right hand side. And this should also
be for construction. When you press okay, it should
be something like this. Next up, let's just get a normal construction
line from the line tool. Click on the drop down
next to the line tool, choose center line or
construction line. And then let's start
from the lower point of this first line here and go all the way down to
the origin like this. Now we just want to extend
these two offset lines down so that they hit that new straight line
that we just made. To do this, you can use
the Trim Entities tool. This is on the sketch tap. Select the Trim Entities tool, make sure you're on power
trim and despite the name. As well as trimming, this also allows you to extend lines. So to do this you
can just left click and drag down from the
bottom of the line. You can drag it through the straight line
that we just drew, something like this, and do
the same for the other one. And then when
you're done, we can just left click and drag through that excess part just to trim away that excess
at the bottom. And then you can close the trim tool and we're going to use these lines as guides to create the wavy front of the
handle that we want. So what we're going to do
is grab the spline tool. We're going to start
at this point where that inner offset line
joins the straight line. And we're basically going
to draw a wavy line upwards that alternates between those
two construction lines. So start down here and we're
going to click eight times. Alternating between
those two offset lines. 12345678. You should finish at
that top point there. When you're done, you
might just need to move a few of them
around a little bit. I've picked up an
automatic relation here, so I'm just going to delete
that and move this one upwards a little bit so it
doesn't have to be perfect, but it should be something
roughly like the video. The main one that's important is this first point down here. If you had more time,
you can maybe go in and individually dimension each
of those points on this line. But for now, just for
the sake of speed, I'm just going to
leave it like that. Then I'm going to
exit that sketch. We've now got the back
of the hand grip, we've got the front
of the hand grip. Next we need to draw
the profile that we're going to sweep along
these two lines. Again, to do this
similar to the nozzle, we need to add a new plane. Let's pre select the front plane just by left clicking on it. And then go to Reference
Geometry plane. We've got front plane here
as the first reference. For the second reference, I'm going to choose the
end point of this line. Then for the third reference, I'm going to choose the start point of the spline down here. You should get preview,
something like this, press okay to make that plane and then start a
sketch on that plane. The first thing
we'll do is just add a center line between those
two end points of the lines. Then we're going to
draw the sweep profile. Let's get the arc tool,
let's get a three point arc. And draw something
roughly like this. We're going to add
dimensions and relations later so it doesn't have
to be exact at this stage. Let's just start on the
left hand side here, finish on the right hand side. And the curve should be going in this direction,
something like this. Then we'll do a similar thing on the bottom,
start on the left, finish on the right, and then the curve should be
going in this direction. Then we can now fully
define these curves, starting with the left hand one. Let's right click on it
and select Midpoint. And then hold down control and select the start of
that construction line. And then release control
and press Coincidence. Then next, select the left
hand point of the arc, hold down control, select the right hand point of the arc, and then keeping
control held down. Also select that center line. And then release control
and press symmetric. This should just center that
arc onto that center line. Then we'll do exactly the same down here, Right
click on the arc. Press select midpoint,
and then make that coincident with the end point of the
construction line. Then select the two
endpoints of the, select the center line and
then make those symmetric. We can now use Smart dimension. Let's make the width between these two endpoints
on the left, 22. Let's make the radius 12. And it should give you a shape, something like that for this
one on the right hand side. Let's make the width 25 and
let's make the radius 13. If I now go to a normal two view to make things a bit
clearer for you, you should have two fully
defined arcs in that sketch. The left hand one is 22
wide with a radius of 12, and the right hand one is 25
wide with a radius of 13. We can then just join these arcs with a spline to
close the profile. Let's get the spline tool, and let's just draw a
spline between, say, these two open points. We can then exit
the spline tool. Let's select the spine
and one of the arcs, just by holding down control and clicking
on both of them. And then we'll make
those tangent. Then we'll do the same thing with the other arc
in the spline. That just gives a
nice smooth join between the spline
and the curve. And then for the second side, we can just mirror it.
Let's select this line. Let's also select
the center line. And then press mirror entities, and that should mirror across. We now have a closed profile there that we can use
for the sweep so you can exit that sketch similar to
when we made the nozzle. You can see we've got like a wire frame outline of what we're going to
do with this sweep. We're going to sweep that oval profile along that back line, but we're going to
get it to follow that wavy line at the front. It's the same process as
when we made the nozzle. Let's go to the
swept surface tool. We want to choose
a sketch profile. For the profile, we'll choose that closed profile that we
just drew, the oval shape. Then for the path, let's choose that line at the back,
that straighter line. Then for the guide curve, let's choose that wavy
line at the front. And you should get
something like this. If you don't get the preview,
I'd go back and check the sketches for both the
path and the guide curve. In particular, with
the wavy guide curve, make sure you haven't
got any really tight kinks on the spline there. And make sure it doesn't
self intersect anywhere, so it doesn't overlap
itself anywhere. When I was actually making this example file
for the first time, I couldn't get it to work
for the first time either, so I just had to delete the spline sketch and
make a new one. So this tool can be
a bit finicky if it can't quite follow the
guide curves correctly, but as you can see, it can
give pretty powerful results. So it can be very useful
when you're happy press. Okay, and we've now created
that hand grip shape, and you can see it's
quite a complex shape. It'd be pretty hard to make
that with solid modeling. We've now created the
nozzle, the handle, the bulb, and the connector
area at the bottom. To recap this video, we
made two different sweeps. The nozzle was a bit simpler, but they both followed
the same principle. Basically, we swept
a closed profile, which was that
circle along a path. But we also used
the guide curve to adjust the shape of that profile as it moves along the path. Then with the handle again, we swept a closed
profile along a path. But we had a bit more of a complex guide curve
at the front there. In the next video, we'll
start to look at joining these different
surfaces together using more complex lofts. And we'll look at
how you can split up the surfaces to make them
easier to work with.
11. 11 Lofts 2: This was how we left
our spray model. We've got these three
different sections, but they're not actually
joined together. In this video, we're going to revisit surface lofts and we're going to use these to join these surfaces that
we've already created. Before we do this,
we're actually going to split these two surfaces, the nozzle and the ball, into smaller sections so it's
easier to create the loft. If we look at the
handle, for example, we've got this surface
here at the back and we want to loft it forward
to this front surface. But that front surface is just one single
surface all the way around and we only want to loft to a small section
of it in the middle. If we split up that front
surface into smaller faces, it'll be easier
to make the loft. We'll make this split now.
And then hopefully it will be a bit more
obvious why we do this. It's quite easy to
split the face up. We can use the
split line command. Before we do this, let's
create a sketch that we can use to draw the lines that we're going
to make the split. Start sketch on the right plane, get a center rectangle and
then start the origin here. And let's make a rectangle
that's 22 millimeters wide and the height
of it isn't too important as long as it completely covers
the whole model. So I'm going to drag
it out to something like this so it's
larger than the model. And then I'm going to get
the smart dimension and I'm going to say set 600
millimeters there. You can see in three
D, the whole sketch is much taller than the model. We can now exit
this sketch and we can use this rectangle
with a split line. The split line feature can be
found on the features tab, and it's under the curves
drop down, here it is. You can also find it in
the search commands box. As usual up here on the right, I'm going to choose split line. And then here on the left, we want to choose the
projection option. Then first we need to choose the sketch that we just drew. Click in this box and
then select the sketch. If you can't see the
sketch for any reason, you might just need to expand this second feature tree and then select the sketch in there. So we've got the
sketch selected. And then here in the
faces to split box, let's just choose that face on the ball and also the
face on the nozzle. So we're going to
project this sketch onto these two faces and split those faces along the
lines of that sketch. So let's press, okay, and it should look like this. And now you can see we've split those surfaces up
into smaller faces. I should say at this stage, the surface body itself
isn't actually split up. It's still one
single surface body. It's just got
smaller faces on it. The terminology is a
little bit confusing. So we've got one surface but
with multiple smaller faces. If we expand the
surface bodies folder, we can see for
example, we've just got one single surface there. But as I say, multiple
smaller faces, right? We can now use these faces
to create the new loft. So I'm going to go
to the surfaces tab. I'm going to choose
lofted surface. Let's just choose the
profiles of the loft we want. We're going to go from
the handle to the nozzle. So I'm going to select
roughly here on the handle, then roughly the same
position of the edge, in the middle of the nozzle. And you should get a preview.
Something like this. It's a nice straight
loft like this. If you find that your loft is twisted or the preview
doesn't show up, if you've got something
like this, it might be that your connectors just
aren't quite straight. If this happens, the
easiest thing to do is probably just clear the
selections and then re, select those two edges. And make sure you try and select roughly the same
position on each edge. I'm selecting the right hand side of the edge
at the back here. And then also the
right hand side of the edge at the front
on the nozzle here. We can now adjust the start and the end constraints to give
us a nice smooth curve. So I'm going to expand this section, start
end constraints. And I'm going to
change the start constraint to tangency to face. And you can see as we
change it, it changes. The preview gives a
nice smooth curve. I'm going to do the same thing with the end constraint as well. Set that one to
tangency to face. The value for both of
them is set to one. You can adjust this and it will change the length
of the tangency. It will give you a
slightly different curve. You could also use guide
curves here if you want to really define
the shape of that loft. To do this first,
you have to draw in the guide curves before
you create the loft. And you can do this by maybe using a three D
sketch with flying, or you could add a
new plane and then use a two D sketch
just with lines and arcs or something like that go all the way
down to the bottom. We can also turn on
the mesh preview. If you expand curvature display, then we can see the
shape of the surface that we're creating
a lot more clearly. You can also turn on
the zebra stripes. And we'll come back to
these in just a moment. For now, if you
preview, looks good, let's press okay to
add that surface and we can see we've got a
nice curve along the top of the sprayer there to quickly just go back to the zebra
stripes. Or zebra stripes. If you're American, we can
go to the evaluate tab. We can choose zebra stripes. You should see
something like this. Now, these are basically
just the visualization that show how your surfaces
all join to each other. We can see here at the top as the two different surfaces join, you've got a nice smooth line of the black and white
stripes there that shows that you've got a
really nice transition without a really
sharp corner there. But if we go down
here, for example, we can see the stripes do join, the black and white
parts do join up. But there's a very obvious
change in direction, and that's because
this upright part is straight and then it goes
to a very curved section. You can see there's a very obvious change
of curvature there. The zebra stripes are basically
just a tool that let you visualize exactly how your
surfaces work with each other. And then I'm just going
to click the button again to turn off
the zebra stripes. Next up we're going to add two more lofts using
the same surface. So I'm going to go to
surfaces, lofted surface, and then this time I'm going to choose the front
of the handle here and then choose roughly the same position on the edge of the
bulb section here. Again, on the preview, we've got a lofted surface like this, it's very straight, we don't
necessarily want that. So I'm going to expand the start and end constraints again. I'm going to make both of
them tangency to face. And then I'm just
going to play around a little bit with the values. I'm going to keep this
one on the handlers one, but I'm going to try and
increase this one on the bulb. If we put that up to
three, you can see it just increases the length
of that curvature. So it gives a bit of a
wider curve around there. I'm going to put it down to two, and I think that looks good. So I'm going to press okay, to create that lofted surface. Finally, let's do the
same thing at the front. So I'm going to go to
lofted surface again. Let's choose our two profiles. Let's say go from here to here. And then in the start
and end constraints, let's again, make them
both tangency to face. And I'll keep them at one, but if you want to play around with it, that's
totally up to you. So I'm going to press, okay, create that new surface. And we've now joined all
of those parts together, and we've got quite a nice
curve on all of those pieces. To recap this video,
first we split up the surfaces using the split
line command to do this, first you have to draw a sketch, and then you can
project that sketch onto the surfaces that
you want to split up. You will still have
one single surface, but it'll have multiple
smaller faces on it. And you can then use those to create the lofts
or other features. Next up, we created
the lofted surfaces. So we chose that
tool, we selected the two profiles using roughly the same
position on each edge. And we changed the
starting intangency to get exactly the curve that we wanted for these lofted surfaces. You can also use guide curves
if you want to control exactly where the surface goes
with a bit more precision. In the next video, we'll
learn how to fill in this gap using the
filled surfaces tool.
12. 12 Filled Surface: In the previous video, we made these lofted surfaces that join the other parts
of the model together. In this one, we'll
look at filling in that gap using a filled surface. Now, I just mentioned that we
join these areas together. Actually, if we look
at the surface bodies folder here, they're
not joined together. They're all separate surfaces. The filled surface,
tool patches, gaps or holes in surfaces. And it's much easier to use if all the surfaces are
connected before you use it. We'll first knit all
of these surfaces together into one large surface. Go to the surfaces tab, and then choose knit surface. Let's select all the
surfaces of the model. You don't have to tick, any of the check boxes, just press. Okay. And now we should have
one single surface here. If you do have more
than one here, it just means that you missed selecting one of the
surfaces somewhere. Just go back and edit
the It feature and make sure you have all of the
surfaces in the model selected. We can now use the
filled surface tool. Here it is, on the surfaces tab. For this tool, all we
need to do is select all of the edges around
the area we want to patch. You can select them
more manually. Like this, I'm selecting all of the edges that go around
the area I want to patch. Then you can see we've
got the preview. Or you can select
them automatically. To do this, I'm just going
to clear the selection that we've already got.
Just so I can show you. What you can do
is right click on one of the edges and then you can go down and
press Select Open Loop. That will select the
entire loop like that. So we've got the
same preview there. We can now select exactly how the patch joins the edges
and the surfaces around it. I'm going to go to this box and change it from
contact to tangent. As I do that, you might see a small change in the preview. I'm also going to check
the apply to all box, then you probably see more
of a change in the preview. That just means that
all of the edges are going to be tangent to the surfaces and the
edges that we've selected around the
outside of the patch. The preview looks like
quite a nice shape there. So I'm going
to press okay. And we've now created that patch that perfectly
fills in that area. The sprayer is looking pretty good there and we
could leave it there. But just one more thing to
note with the field surface, you can also use what I
call constraint curves. And these are basically
guide curves. And we can also
use single points, which are known as pull points. If you had a point out here that you wanted the
surface to touch, you could add in those
constraints using pull points. And we'll quickly
go over that now. Now to use pull points
or constraint curves, you need to draw the
sketch that you're going to use before you make
the field surface. So I'm going to drag
the rollback bar above the field surface
and then I'm going to make a new sketch on
the right hand plane. And I'm going to add
a single point that's 170 millimeters up from the origin and 50
millimeters out to the side. And make sure it's
on the same side that you just made
the field surface on. We've just got a
point that's 170 up and 50 millimeters
out to the side here. I'm now going to drag back below that filled surface feature now. Just make sure your point is on the same side as
your field surface. If it's not, you
might just need to edit that sketch
and then flip that 50 millimeters around so the point moves to
the other side. We can see here
that the sketch in the feature tree is
before the surface fill. We can now edit the
surface fill feature, and we should be able to
use that sketch as one of the constraints down here
in constraint curves. I'm going to click
in that box and I'm going to select the
point that we just drew. If you can't see it
in the graphics area, you might just need to expand that second feature
tree to select it. Now when you select it, you
should get a new preview. If it doesn't work
for any reason, as seems to have
happened in my case, you might need to change
some of the settings. So maybe move the point closer
to the previous surface. Or you can try adjusting
the settings up here. So I'm going to
change these from tangent to contact and
see if that works. Now we can see on the preview, we are actually now
hitting that point. That looks pretty
good on the preview. If you wanted to bulge
to go out to this point, all you need to do is select that point on the
constraint curve. And if I press okay, that new surface is updated. We've got a bit of a
stranger shape now, but it's still nice
and smooth and it's going out to that point
that we selected. You could also use
a number of points, or you could use curves to define the exact shape
of that surface. To recap, field surfaces, these are used to fill in or patch a gap or a
hole in surfaces. And they work best when all
the surfaces around them are knitted together using
the knit surface command. You can then select
Field Surface and you can select the
boundary edges either manually or you
can right click on one edge and you can
press Select Open Loop. You can then adjust
how the patch joins the edges around it. And you can use things like
pull points and constraint curves to exactly define
the shape of the curve. In the next video, we'll finish off the sprayer by
looking at things like mirroring planer surfaces and
knitting versus thickening.
13. 13 Planar Surfaces: Our spray model is now almost
done. We left it like this. There's a bit of a
hole on this side, and then there's some
gaps on the end. First up, we're
going to close this gap on the left hand side. To do this, we could create another field surface just using the exact same parameters, and that would work
absolutely fine. But you can also just mirror this existing surface
with surface bodies, you can mirror them
and pattern them just like you can with
normal solid bodies. It's very simple to do this. Just select the mirror feature
from the features tab. Then first let's
select a mirror plane. In this case, it's
the front plane that goes down the
middle of the model. Next we need to select what
we actually want, a mirror. And your mirror
feature might have automatically filled this
features to mirror box. But actually because
this is a surface body, we need to use the
bodies to mirror option. If you do have anything here in the features to mirror box, just clear that selection and then expand
bodies to mirror. And just select that latest
filled surface body here. And then you'll probably
get some preview. If that looks good, press okay, and now we have that second surface body on the
left hand side. Our shape is almost
finished at this stage, we could use the
thickened feature to turn this into a solid. To do this, first
we have to knit everything together. We'll
have a go at doing that. Now, select the knit surfaces
tool from the surfaces tab. Let's select those
three surfaces. We've got the main one,
and then we've got the two patches,
one on each side. And then press okay. Now we
have one single surface. Then we can go to
the thickened tool, we can select the body. Let's set say 1
millimeter again. I'm going to leave it on thick
on both sides and press. Okay. It might take a few minutes just because
it's quite a complex shape. It's working out exactly
how to thicken it, but when it's done, you should
have something like this. We've got a nice 1 millimeter uniform wall thickness
all the way through. At this stage, you could
maybe split this in half and use it for
injection molding, or maybe even vacuum forming
or something like that. However, instead of thickening, we could also make this into a completely solid
body at this stage. This could be useful
maybe if we wanted to add some more detail
inside the model later on. Things like screw holes or maybe differing
wall thicknesses. To show this, I'm
going to delete those last two features
that we just added. The surface knit and
then the thicken. I'm going to delete those.
Then to make this solid, we need a completely
enclosed outer shell. But at the moment we've got
three holes to the outside, we can fill these in using
the planer surface option. This tool is here on
the surfaces tab, and it basically just makes a flat or planer surface using
an edge or a set of edges. And to make these, all of the edges need to be
on the same plane, the created surface
is totally flat. To show an example, let's select this planar surface tool. And then let's just select this circular edge at the front. And we can see on the preview, all we're going to
do is close off that circular opening with a completely flat surface there. Let's press okay to add that. It's a very simple tool,
but it's quite useful just for quickly closing flat
surfaces like this. We'll do the exact
same thing down here. So let's choose planar surface. Let's choose the
outer circular edge, and the preview looks good. So let's press okay to add
that flat surface then, with this hole at the
bottom of the handle. Even though it's made of
multiple smaller edges, we can still use
the planar surface on it because they're
all on the same plane. You might remember
from a few videos ago, we added that plane,
plane five in my model, to create the sweep. So let's open the planar
surface tool again. And then let's just manually
select those four edges. And you can see as
I click on them, it fills in a partial
planar surface there. And then when I get all of them, we get a fully enclosed surface
there. Let's press, okay. And we've added
that new surface, so we've now got a completely
enclosed outer shell. We've just got to knit all of these faces together
and create a solid. Let's go to knit surfaces and let's choose all
of those surfaces, so there should be six in total. We've got the main
body, the two sides, and then we've got
those three new planar surfaces
that we just added. And then before you press, okay, let's put a check in the create solid box and then press Okay, now we've got a
completely solid shape. We can see here it is in
the solid bodies folder. That's the paint spray done, well done on
creating that model. To recap this video,
at the start, we mirrored one of the surfaces
over to the other side. You can mirror and
pattern surface bodies just in the same way as you
would with solid bodies. Make sure that within
the mirror feature, you choose the bodies
to mirror option, not the features
to mirror option. Then at that stage, we
could either knit all of the surfaces together and use thicken to make a solid shape. Or we could close the outer
shell using planer surfaces. These are just simple
flat surfaces that are made on edges that
are on the same plane. Then once we have that
enclosed outer shell, we used the It surfaces and
we created a solid from that. In the next section,
we'll start a new model, the vacuum cleaner nozzle. And for that one,
we'll mainly be looking at the boundary
surface feature. This is a similar to the lofted
surface in lots of ways, but it just gives you
a bit more control.
14. 14 Boundary: In this section,
we're going to make a fairly simple model using
the boundary surface feature. This is quite similar to
the lofted surface tool, but it's a bit more powerful. And it was only
actually added to Solid Works around 2008. So it's quite a new tool
to show how we can use it. We're going to create
an example part something like this,
Vacuum cleaner nozzle. Start a sketch on the top plane. And let's draw a sensor
point circle at the origin. Give it a diameter
of 40 millimeters and then exit that sketch. Next we'll add a new plane. Select the top plane, then select features,
reference geometry plane. Make sure you have the
top plane up here. And then let's type
in 19 millimeters. So we're creating a new
plane that's 19 millimeters above the top plane and
parallel to it like this press. Okay, and then start a
sketch on that plane. First, let's get the
center line tool. We'll draw two center
lines at the origin, one vertical and one horizontal. We'll make the length of the horizontal one 30 millimeters. And then we'll get the
circle tool and we'll draw a center point circle at the left hand end of
that horizontal line. Let's make that ten
millimeter diameter. And then select that
circle by clicking on it. And then just choose four
construction here that should turn the solid line of the circle into a
dashed line like this. We then also want another identical circle on
the right hand side. So let's select that circle. Hold down control and select
the vertical center line. Then choose mirror entities. And this will copy that circle
over to the other side. If your mirror doesn't
work for any reason, just choose mirror entities
without selecting anything. And then choose the circle
in the entity to mirror. And choose the vertical
center line in the mirror about box.
And then press Okay. And that will add the circle
to the right hand side. We should have two circles,
60 millimeters apart. And everything in the sketch
should be for construction. All of the lines should
be dotted like this. We'll then get the arc tool, we'll get a three point arc. We'll start an arc on
the left hand side, somewhere on the
circle on the left. But it needs to be to the left of center point of the circle. It shouldn't be
at the top point, it should be somewhere
to the left like this. And then we'll go
over to the right and we'll finish it on the
right hand circle, somewhere to the right
of the center point. Then let's set the size going upwards,
something like this. We can now add some
relations in dimensions. Firstly, let's select the arc. Let's hold down control and also select that
left hand circle. And then release control
and make those tangent. Do the same thing on the right
hand side, select the arc. Also select the circle
and make those tangent. Then let's get the
smart dimension tool. Start at the origin and we
want to dimension to the arc. You'll have to hold down, shift to dimension to the curve. And let's set that
as 7.5 millimeters. And this should fully
define your sketch. It should look
something like this. We then also want a
similar arc on the bottom. Let's select the Arc
hold down control. Also select the
horizontal center line. And then press mirror entities, and that should mirror it
to the bottom like that. We can then just close this
profile using more arc. Let's go to the arc tool, this time we'll choose a tangent arc. Then let's just close the
gap on the left hand side, starting at the bottom arc, going round to the top arc. And then the same thing
on the right hand side. If you find that when
you draw your arc, it goes in the wrong
direction like this. Just try to move your
mouse over to the right. If you still find
you can't get it, just press escape to close
the tool. Then try again. Make sure when you
first start the arc, you go over to the
right hand side. When you finish, you should have this fully closed profile that's stretched out oval shape. And you can then
exit that sketch. The large circle at the
bottom is the part that fits onto the tube that
goes to the vacuum cleaner. And then the stretched
out oval part is the part that actually
collects the dust. Next, we need to
define the shape a bit more by drawing
some guide curves. Let's start a sketch
on the front plane. I'm going to go normal two, and we want to draw
something like this. First get the line tool and draw a vertical line somewhere
out to the left like this. Then get the arc tool
and a three point arc. And draw an arc from the top of that vertical line that
looks something like this. And then draw another three
point arc from the top of that first arc that
looks something like this. It doesn't have to be
exactly the same because we can now add some
relations and dimensions. Firstly, let's select
the vertical line and also the first arc, and let's make those tangent. Then let's select both of the arcs and make those tangent. You might just have to drag around some of the
points as you do this, because it might move
your entities around. Next up, we want to make
it so the bottom of this straight line pierces or touches that circle
at the bottom, Select the endpoint of that
line, the lower endpoint. And then hold down
control and also select that circle from the previous
sketch release control. And then choose Per, this just means that
that endpoint will always touch that circle. Then we want to do the
same thing on the top. Select the end point
of the top arc, then also select the left
hand arc of that top profile. And then release control. And then press P. Then it
should look sort of like this, and we can add some
final dimensions. Get the Smart Dimension tool. Let's make the height of this bottom vertical line
15 millimeters. Let's make this point
where the two arcs join, 50 millimeters from the bottom. Then for the horizontal position
where the two arcs join, let's make that 7
millimeters to the left of that vertical line that should
fully define your sketch. If yours is still blue, if it's not fully defined, just make sure you've
got all of those. The two arc should be
tangent to each other, and the lower arc should also be tangent to the vertical line. Then the top of the upper arch should pierce that
upper profile. And then the bottom
of the vertical line should also pierce
that lower profile. Now before you exit, we're
going to add a center line up the middle because we also need this guide curve on
the right hand side. Get a centerline tool, Draw a center line vertically
up from the origin. Then you can press
control A to select everything in your sketch
and go to mirror entities. This will automatically mirror that line on the left
over to the right, because we've only got one center line in
the sketch that will automatically be used as
the mirror about point. When your sketch
looks like this, you can exit that sketch. We now have some guide curves on the left and right hand side, but we also want
some in the middle. So let's start a new
sketch on the right plane. We'll go normal two and we'll
draw sort of similar shape. First we'll get the
line tool. We'll draw a vertical line up
from the bottom. We'll get the arc
tool again and draw a three point arc this time it wants to go
in this direction. Then we'll draw another
three point arc from the top of that arc,
something like this. And then we'll get
the line tool again, and we'll draw a
small vertical line upwards at the top like this. Then we'll start to add
some relations again. Let's select this
lower vertical line and the curve and
make those tangent. And you might find that
you just need to re, drag around your lines like this so they're in
the correct position. Let's also make those two
arcs tangent where they join. Then let's make
that upper arc and the upper vertical
line tangent as well. Then we'll add the
pierce relations again. Choose this lower
point of the line. Then also select the
circle at the bottom, and press P. Then choose the
top of this line at the top, and also select the outside of the profile at the
top. And press Pi. You should end up with
something like this. So we can then use the Smart dimension and add some heights. This lower vertical
line is 15 high, the upper vertical line is five. Then the point where
the two arcs join is 50 millimeters
from the origin. Again, that should fully
define the sketch because of the combination of
relations and dimensions. Again, let's mirror this over to the other side. Let's
get a center line. Draw a center line vertically up from the origin
and then press control A to select
everything in your sketch and press
mirror entities, we should have the same profile, but opposite on the
right hand side. And then you can
exit that sketch. Now if we look in three D, we can see a wireframe view of the part that
we're going to make. We can now use the
boundary surface tool with all of these profiles to
make the part that we want. Let's go to the surfaces tab. Choose boundary surface.
Here on the left, we've got two selection boxes, like the lofted surface tool. With the lofted
surface, you've got the profiles to
select at the top, and then underneath
you'd have the guide curves to select. It's quite similar with
the boundary surface tool. Instead of profile
and guide curve, we've just got direction
one and direction two. This just gives us a
bit more control of the shape because we can
individually set all of the different
parameters for each of the directions. Let's
have a look at this. Let's click in the
direction one box, and first we'll choose
the two profiles. We'll choose the
circle at the bottom. And then roughly the same area from the oval shape at the top. You should get a preview.
Something like this. It doesn't matter too much at this stage if it looks
a little bit twisted, because we'll add
direction two in a moment. You can then click in
the direction two. Box first up. Let's select one of these
lines here on the left. When you click on
it, you should get a little selection box pop up. We want to choose this
option, select open loop. This just means
that we'll select all of that loop on the left, but we won't select anything
else in the sketch. In this way, you
can have multiple guide curves in the same sketch. Select that one on
the left, press select open loop,
and just press okay. And you'll see that
the preview now matches the shape of
that guide curve. We'll then do the same
thing on the right. Select that line on the
right from the pop up. Let's choose select Open
Loop, and press Okay. Now the right hand
side of the preview also matches the guide curves. Then let's do the exact
same with this one. Select the line and choose
Open Loop, And press okay. Then finally, we'll do the
same with the fourth one. Select press, select
open loop, press Okay. We should now see
that the preview exactly follows those guides. The great thing about the
Boundary Surface Tool is that we can now
individually control all of these points using the
drop down menus so we can adjust the tangency options
anywhere in the surface. We just have a bit more control
than the lofted surface. The boundary surface tool can be really useful for
creating patches. If you're having problem
with the filled surface, you can use direction
one to select, say, two edges of the patch, and then you can use direction
two for the other edges. It's also useful for
creating partial patches, so if you've got an area where the hole isn't fully enclosed, you can use a boundary
surface for now. We'll just press okay
to make that surface. Now we have our
basic nozzle shape. That's the introduction to the boundary surface
tool in this video. First we sketch some profiles
and some guide curves. And then we use these
to make the surface, the boundary surface is quite similar to the lofted
surface in many ways, but instead of profiles
and guide curves, we just have direction
one and direction two. This makes the tool a bit
more powerful because we can control all of the individual
points separately. In the next video,
we'll add more to this model by
trimming away the top. And we'll have a look
at the combined offset and copy surface tool.
15. Offset/Copy Surface and Project Curve: In the last video, we introduced the boundary surface feature. We started making a nozzle
for a vacuum cleaner. In this one we're
going to develop it further using
various techniques. And we're going
to have a look at the offset surface tool. This is how we left the model. It looks okay, but let's say actually we want a
curve on the top here. Maybe just to help you get right into the edges
When vacuuming, let's trim away the top
using another surface. Let's start a sketch
on the front plane. First, let's draw a
vertical center line from the origin at the bottom all the way to the
top of the part. Just so we can line
everything up the next. Let's get the Arc tool and draw a three point
arc like this, starting on the left and
going over to the right. Let's select the midpoint by right clicking and
pressing Select Midpoint. And then make that coincident with the top of the center line. Then let's select the left
and right points of the arc, and also the center line, and make those symmetrical. Then we can set the
width as 80 millimeters. And then finally,
let's put the height here as 8 millimeters. We should have a fully
defined arc like this. If yours isn't fully defined, just make sure you've got
that symmetrical relation on there between the
two ends of the arc. We can then use this arc to
create an extruded surface. Let's go to the surfaces tab
and press extruded surface. Let's do a mid plane extrude
and we'll go outwards. So we cover the whole nozzle and let's say make
it 50 millimeters. Now we've got a new curved
surface at the top which basically goes right up to
the edge of the part there. We can use this to trim the
top of the first surface. Let's go to Trim Surface, make sure you're on
the standard option. And then let's
choose that extruded surface as the trim tool here. And make sure you're
on Remove Selections. And let's just choose those
two regions to remove there. And press Okay. We've now removed those and we've got a nice curved edge
on the top there. We don't need this
curved surface anymore, so we could just hover over
it and press Tab to hide it. But instead what I'm
going to do is delete it. To do that, we can go up to
this search box up here. We can start to type delete, and we'll choose delete. Keep body. Remember
this is a surface body, so we need to use this tool. Let's open that
tool and then make sure you're on the
delete body option. Then just choose that curved
surface and press okay. And that should now be
deleted and we've got that nice smooth curve on the top to create this
curve like we just did, we could either trim
it like we just did, or we could have just drawn
it curved in the first place. To do this, we could have used
the Project Curve option. This is on the Features tab and it's under the curves drop down. There is Project Curve. I'll just quickly show you
how we could have used this. So we could choose
project curve, we could choose the
sketch on sketch option. And for the inputs we'll use that initial oval shaped
profile that we first drew. For the second one, we'll use that curve
dark that we just used to make the extruded surface
that we used for trimming. If we were to use both of
those sketches together, we would have created a curve
like this yellow preview, you see exactly lines up with the part that
we've cut anyway. But we could have
used that curve with the boundary surface to make the shape in
the first place. Instead of using that arc
afterwards to trim away, it would give the
same end result. So I just wanted to show
you two different ways you could do the
same thing there. Now that we've got this surface, we can thicken it using
the thickened feature. This is on the surfaces
tab. Let's choose that. Let's select the surface, set the thickness
as 1 millimeter and let's thicken it on
both sides and press. Okay, so now we've
got that solid with a uniform 1 millimeter wall thickness all
the way through. Now we're going
to have a look at the offset surfaces tool. So imagine we were
suddenly told, actually we want
the inside diameter of this nozzle to be smaller. Maybe the tube that fits
on has changed size, but we only want to make
it smaller at the end. We want the rest of the nozzle or the inside to stay as it is. We can use the offset
surface tool to do this. First, let's split up
the inside face of this nozzle so we can just offset the
section that we want. Start a sketch on
the front plane, and then draw a center
line upwards from the origin from
that center line. Let's do a horizontal
midpoint line. You can find the
midpoint line by going to the drop down next
to the line tool here. And choose midpoint.
We'll start at the top of that center line
and we'll go out to the left. And you can see as we do it
also goes out to the right. Let's make that line
50 millimeters wide and set it as 20 millimeters
above the origin. In terms of the
position, it's just above the area where the
nozzle starts to curve. Then use this line to
split up the inside face. If you remember, we'll go to
features curves, split line. We'll choose the
projection option. Then for the selection, let's choose that straight
line that we just drew. And then for the
surface, let's choose that inside surface.
Then press okay. Now we split that inside
surface into two smaller faces. We can use one of these
faces with the offset tool. Let's go to the surfaces tab. Choose the offset
tool, which is here. It's a very simple tool. All we need to do
is select the face that we want to offset
and select the amount. Let's choose that
inside face and set 1 millimeter and
let's offset inwards. If you do need to reverse
the direction of the offset, you can just click
this little burn here. Let's offset 1
millimeter inwards and press okay. To
make that new surface. We now have a new surface
inside there that's 1 millimeter away from
the other inside face. If we wanted to, we could now use thicken with
this to show this. Let's go to surface thick, let's choose that new face
that we just created. Let's thicken 1 millimeter and this time we'll go
outwards like this. It's basically going to
fill in that gap between the offset surface and the main surface that
we initially used. Let's also put a tick in
the merge resort box here. What that means is when
we create the new solid, it will be merged with any
other solids that touches, it'll merge with that
main outer solid. So let's press Okay.
Now we can see we've just got one single
solid body in the model. That thicker section
at the bottom of a smaller diameter is also an
integral part of the model. If we hadn't checked
that merge result box, I'll just show you. So if I edit it and uncheck it, we can now see we've
got two solid bodies, and potentially we could join these using the
combined feature. We'll have a look at
that in just a moment. There's also almost like a hidden function of
the offset surface, and we'll look at that now. Firstly, I'm just going to delete those last two features, the offset and the thicken. So I'm going to select
them and press Delete. We just have the basic
shape of the nozzle. We now want to achieve basically the same thing as we just did, but in a slightly different way. We want to make that
inner diameter smaller. I'm going to go to the
surface tab and I'm going to choose
offset surface again. When we open it, you'll notice up here it says offset surface. If we change the
offset amount to zero, that text up there
changes to copy surface. You see if we have
say, 1 millimeter. It says offset surface. If we have zero, no offset, it changes to copy surface. We'll keep the distance to zero. We'll choose that
inside face again. And then we'll
press okay. If you look in the graphics area, maybe it doesn't really look
like anything has happened. We've got this slightly
dotted edge around, but actually we have
added a new surface in if we hide the
main solid body. So I'm going to
hover over it and press the tab key to hide it. We can see that what
we've got left is that surface body inside there. That's exactly the same
of that inside face of the body that we just
hit this feature. Copying the surface can be really useful if you want to use a surface from a solid and then use that for some
surface operation. We could now maybe
use this surface and thicken it inwards, but we could also do
something like this. I'm going to hide that
solid body again. And then I'm going to
select the offset tool. Again, select the surface
that we just made, and this time offset
1 millimeter inward, like this and press. Okay, now we have two parallel surfaces,
almost like rings. One of them is slightly
smaller than the other one and it's offset 1 millimeter
in all the way around. We've got this small 1 millimeter
gap between them and we can fill that gap using
something like a ruled surface. Let's go to surfaces and
select ruled surface. And then in the selection box, I'm going to choose
this inside edge on the bottom and also the
inside edge on the top. For the option, let's
choose normal to surface. Let's set the distance
as 1 millimeter. And then if you need to, let's just reverse the direction. So we're filling
in that little gap between the two
parallel surfaces. It should look
something like this. We don't need any of
these options down here. Selected Uncheck both of those. Press okay, and we've created
those two new surfaces. We can then knit
these four surfaces altogether and we can
create a solid from them. Let's go to the surface
tab and choose it surface. And select all four
of those surfaces. And put a tick in the
create solid box and press. Okay. We've now created a solid using all
those four surfaces. If I re show the main body, you can see we've
basically created that same inner ring there. We've just done it in a
slightly different way. These bodies are also
now two separate bodies, but we can combine them
using the combined tool. You can go up to the search
bar on the top right and start to typing combined COM B. There's combine open that tool, make sure you're on
the ad option and then just select the two
solid bodies and press okay. And now they've been merged
into one single solid body. That's the nozzle completed. It's quite a simple part
to recap this video. First we practice
trimming by making an extruded surface and then using that with the
trim surfaces tool. We could also have used the project curve option
to make a profile that was curved in the
first place and we could have used that with
the boundary surface tool. We then looked at the
offset surfaces tool. As the name suggests, this can be used to offset surfaces, but it can also be
used to copy them. If you set the offset
distance to zero, this can be useful
if you need to duplicate a surface
from a solid. Use that in a
surfacing operation. We looked at two
different ways of creating that thicker
ring section. The first was just by offsetting the surface and
then thickening it. That's probably
easier and faster. But we also looked at offsetting and copying two surfaces, and then filling the
gap in between them, using some ruled surfaces. And then finally knitting all of those together and
creating a solid, which we then combined
with the main solid. In the next section, we'll
be practicing some more of these techniques by
modeling up a spoon.
16. 16 Spoon Setup: Welcome to this new model. In this short section, we're
going to practice some of the techniques that
we've learned so far by making a spoon like this. It's a fairly simple model, but hopefully it will show
you how you can use things like boundary surface
and lofted surfaces. And it will give you a little bit more practice with those. So let's get started. Let's open a new part
and start a sketch on the top plane with surfacing. It's often a case of doing a bit of groundwork in advance, and then when you actually
make the surfaces, it's fairly quick
because you've got everything sketched out already. In this video, we'll just set up all the sketches
that we need, and then in the next one we'll actually use those with
the surface tools. We're on the top
plane and we want to draw the profile of
the sketch from above. Firstly, let's get a
center line and draw a horizontal center line
out to the left like this. Then we'll also add
three vertical uprights, one from the origin, one about here to the
left of the midpoint, and then one on
the left hand edge of that horizontal center line. Then we'll use Smart Dimension. And the first distance here
should be 110 millimeters. Then the second one
is 65 millimeters. This will just help us lay
out the rest of the sketch. We're now going to use the
trustee three point arc tool. Let's get the Arc tool,
choose three point arc. Firstly, let's draw an arc on this end on the
right hand side. Let's start on the top and go down to the other side.
Draw something like this. Then we'll do a similar one on the other side but
just opposite. Start on the top, go
down to the bottom, and then pull it out
to the left like this. Then let's right click
on this right hand arc and press Select Midpoint. And then hold down control. And also select the
right hand edge of that horizontal center line.
It should be the origin. And then make those coincident. Then next let's select
the two ends of the arc and also the
horizontal center line. And we'll make those symmetric. This just lines up
the arc so that it's centered on
that center line. Then we'll do the same
thing on the left hand, one, right click on the arc. Press select midpoint. Also select the
left hand edge of that horizontal line and
make those coincident. And then select the two end of the arc and the
horizontal center line. And then make symmetric. Then we'll get the
smart dimension tool. And this arc on the right,
let's add a radius of 7.5 millimeters and then a
width of 15 millimeters. We can leave the left hand
one undefined for now, and your sketch should
look something like this. We're then going to use the
three point arc tool again, let's select it and
I'm going to start here at the end of this arc
on the right hand side, and then finish somewhere
on this vertical line. Then let's make the distance
here 3 millimeters. So it should be 3 millimeters
above that center line. And then you can exit that tool and you can select
both the arc that we just drew and the arc on the right hand side and
make those tangent, and that should fully define
that section of the sketch. This is going to be the
handle of the spoon. Next we'll draw the head
or the bowl of the spoon. We'll get another
three point arc. We'll draw one from this point, from the top of this arc on the left to roughly about here. And then we'll draw a
second one from the end of that arc to the end of that other arc,
which is the handle. You might have to zoom in a
bit and select that point. You should have
something like this. Mine looks pretty
wonky at this stage. It's not really like the
actual head of a spoon. So we'll get the
smart dimension tool and we'll add in
some dimensions. This point where the
two arcs join should be 20 millimeters up from the
horizontal center line. And then it should
be 18 millimeters to the left of
that middle point. Now if you find that when
you add your dimensions, you get a problem, your arcs all overlap or the turn
into strange shapes, what you can do is
press control D, undo and just go
back to the point before you added those
last two dimensions. Just drag your arcs
around so they're roughly in the same
position as the video. And then add those
new dimensions in, 20 millimeters up and 18
millimeters to the left. And then that should give you
about the right position. We can see that the arcs are nowhere near fully
defined at the moment. So what we'll do is add
some more relations. So I'm going to select this arc on the left and also the arc next to it by holding down control and
selecting both of them. And then we'll make
those tangent. We'll do the same thing
with these other two arcs. Select the middle arc and the one that goes to the handle, and then make those
tangent as well. Then next, we'll add
a radius to this arc. Let's make that R 12. Finally, let's make
this point here 10 millimeters above
the horizontal. That should fully define
your sketch like this. It should look like half
a spoon at the moment. We've got some gaps in the
profile on the bottom. So we're going to mirror
some entities over. I'm going to select
these two arcs on the left and then the arc
of the handle as well. And then also select the
horizontal center line. And then press Mirror Entities. You should have the
full profile like this. Now, before you exit, we'll just round off that
transition between the head and the handle using the sketch fillet that's
on the sketch tab. We'll set say, 10 millimeters and you might just
have to zoom in and select that point where the two arcs join on
the top and the bottom. Now we've got the full spoon profile from the top like this, and you can exit that sketch. Next up we'll draw
the side profile. So we want to start a
sketch on the front plane, then go to sort of three D view. Get the center line tool, and let's draw three
center lines going down. The first one goes down
from the origin here, from the end point of that
previous horizontal line. Then I'm going to do one about
here, about halfway along. And then a final one on
the left hand endpoint, They should all be
going down vertically. Then for this middle
one, I'm just going to select
the top end point. I'm going to hold down control. I'm also going to
select this point on the previous sketch and then make those two
points coincident. These lines will just help us line up the rest of the sketch. Then we can go to
a normal two view. We're basically looking
from the side of the spoon. Let's get a center line again. Let's start from this
top corner and go down diagonally to that
middle center line. Then I'll continue downwards, but with a new line to this
left hand center line. Those should be two
separate lines. The top one should be ten degrees from the
horizontal, like this. Then the bottom one should be
lined up with the top one. Let's select both of those
lines. Select the first one. Hold control, select
the second one and then choose make colinear. We now need more
three point arc. So let's get the arc
tool going to start at this top corner and I'm going to finish at that point
in the middle, then I'm going to do a new one. From that point in the middle
to that left hand point. The right hand one
has a slight curve. The left hand one, where
the head of the spoon is, has much more of a curve. Then with the Smart dimension, I'm going to make this first
one 700 millimeters radius. It's only a slight curve there. This bottom one should be 50, so it's got much more of
a curve than the top one. Next up, let's add a radius
where those two arcs joint. Get the sketch file. We'll
set 20 millimeters this time, and you might just
have to zoom in and select the point where
those two arcs join. This will just give
us a nice curve where the head joins the handle. Then just before we exit, one final thing,
let's get the point. Let's add a point in the middle of this left hand angled line. If you hover over the midpoint, you should be able to pick up
that midpoint of the line. This will just help us line up the planes
that we'll add in a moment to give us the correct cross
section of the spoon. If we exit that sketch,
we can see we've now got a top profile
and a side profile. However, the spoon also has a curved cross sectional area. We'll add some new planes
and we'll draw some slices of that cross section
to help us with this. Let's hover over the right
plane and click Show. You should be able
to see the right plane in the graphics area now. And then a quick way
to add new planes. If we hover over the right
plane with the mouse, hold down the control key and then left click and
drag from the plane, it will add a new plane. Then you can release the control key and we can zoom in and we can select exactly where we want that plane
to be anchored. I'm going to choose the endpoint
of this first arc here. And then you can press okay, and that new plane is added. Then let's do a similar
thing for the second one. So I'm going to hover
over the right plane, hold down the control key, left click and drag outwards
to add a new plane. And then release control
for the point to select, let's zoom in and let's select the start of this
sketch fillet here. You should add a
new plane there. Then let's do the same for
the third and final one. Hover over the right plane, hold down control, drag
the new plane out. And then for the
point to select, let's choose the midpoint of that angled line that we added. It's that small point that we just added in the
previous sketch. It's right in the middle of the head of the spoon like this. We'll now use these
three planes to draw the cross sections of
the spoon at that point. So as I said, it's quite
a bit of groundwork. Sing all these sketches, but once these are
done, it's much easier to actually use
the surface tools. The first profile at
the top of the handle. Let's start a sketch on
that new plane, plane one. Let's get a three point
arc tool and we'll start an arc on the left
hand side of the profile. And we'll finish it on
the right hand side, it should be straddling
the center line like this. Then we can right
click on the arc. We can select Midpoint, hold down control, and also select that angled line
that's going down. Then from the menu that pops up, let's choose S. The
midpoint of that arc is now exactly on that angled
line from the side profile. Let's go to a normal two view. Let's get a center
line. And draw a center line vertically, straight down from the origin. Like this. Then select both ends of the arc and
also that new center line. And then press make symmetric. This will just centralize
the arc on that center line. Then for the width of the arc, let's use Smart dimension
to set that as 20. Let's make the radius 16. Then you can exit that sketch. We should have
something like this. It's quite a shallow
arc at this stage, That's basically a slice
through the handle. At that point, we'll then do the second
cross section slice, so start a new sketch on
the next plane, plane two. Get the three point arc
tool again and again, draw an arc that straddles
the center line. It starts on the left, it
goes over to the right, right Click on the arc and
press Select Midpoint. Then also select that
angled line again and press P. Then go to a normal two view. Add a vertical
center line again, select both sides of the arc, select the center line and
then press make symmetric. You can see at the moment
the arc is a bit one key, but once we make it symmetrical, it's perfectly lined up. Then let's set the width of
the arc here as 20 again, and the radius as 16. Then let's exit that sketch. Now looking at the arcs, I realize that I've made the first one the wrong dimension. I'm going to go back in and
edit that first Arc sketch. You should be able
to do this just by double clicking on the Arc, or you can go back and
edit sketch three. I'm going to change that
radius instead of our 16, it should actually be
60, 60 millimeters. Now you can see it's a
much shallower curve at the top of the handle there. Now that that's fixed, let's go and add the final cross section. Start sketch on the new
plane, plane three. Get the three point
arc tool again. And draw an arc that straddles that center
line like this. Then select the
midpoint of that arc. Then let's also choose that
curved line and press Per. Then we'll go back to
our normal two view. We'll add a vertical
center line. We'll choose the
outside edges of the arc and the center line
and make those symmetric. Then let's make the total
width 50 millimeters. And for the radius, this
is quite a big radius, so let's make that
40 millimeters. And you can then
exit that sketch. We can see the shape of the spoon that we're
going to make. So we've got quite a
shallow profile at the top, then we've got more
of a curve here. And then we've got even more
of a curve in the head. We've got the side profile and we've also got the top profile. Sometimes with surfacing,
it can feel like you're just drawing endless construction sketches like this. But then once you actually
start to make the surfaces, it's so much easier and faster if it's all laid out like this. First to quickly recap, first we drew that top profile of the spoon with
the load of arc, and then we mirrored it
over to the other side. Next up, we drew the
angled side profile. We added some points along that, and we used those
to add new planes. And then on those planes we drew a cross sectional profile of the spoon at those
various points. In the next video,
we'll actually start to use all of those sketches
to create the spoon.
17. 17 Spoon Finish: In this video,
we're going to use all of those sketches
that we made. In the last video, we
had something like this, All the different
profiles of the spoon. We'll start off with
the boundary surface, Select the tool from
the surfaces tab. And we want to choose just
this single arc in the sketch. But if we click on it like this, we'll end up selecting
the whole sketch, and we don't want that. I'm going to clear
that selection before we select anything. Let's right click in
some empty space in the graphics area and
choose Selection Manager. This will let us just select certain entities in the sketch. We should get a little
pop up menu like this. We want to choose this one. Select group. It's the one that's got multiple
cursors stacked on it. Choose that option and then just select this arc on the left. And then press,
okay, now we've just selected that arc instead
of the whole sketch. Then for direction two, let's
click in the selection box. And then let's choose
this cross sectional part of the head, just this arc here. As you do, you should see a preview of the
surface like this. We can leave all of
the default settings as they are and then press okay, and we'll make a
surface like this. We've now added roughly the
head of the spoon there. Next up we're going to
make the handle for this. We're going to use a loft. Let's go to lofted surface. Then for the profiles,
I'm going to choose the left hand edge
of this arc here, and then also the corresponding left hand edge of
this one up here. Should get preview like this. Try to make sure you choose roughly the same corresponding
place on each of the arcs. If you find that your
preview doesn't appear, it might just be that your
loft is a bit twisted. So if so, you can move
these green connectors, so they're lined up in a
straight line like this. If we look at the preview
from the side like this, we can see actually it's
a very straight loft. But we wanted a little
curve on that handle. And we can add this
using guide curves and that side profile
sketch that we drew, but at the moment we
can't see that sketch. That's because we used that sketch in the previous feature. In that boundary
surface feature, When we used it, it was
automatically hidden. We can still use it
in this feature. It can be shared between
multiple features. But first we just
have to re show it. Let's expand this
second feature tree. Let's find that sketch. For me, it was sketch two, so it should be underneath
the boundary surface feature. If you expand that feature, you should see the
sketches under there. Let's click on the one we
want and just press Show. And now we can see it
in the graphics area. Now we can use it
for the guide curve. Click in the guide curves
box here on the left. And then just click on
that profile sketch. And you should get a
preview like this. So we've got a
nice flowing curve down along the handle there. And then you can press okay
to create that surface. Next up, we'll join these two
surfaces with another loft. Select the surface loft tool. And then we want to
select the edges of the existing surfaces rather than the sketch profiles
that we've already drawn. This will just allow
us to use the tangency controls to give a nice smooth
join between the surfaces. Now if you have any of the
previous sketches showing, for example, sketch
four showing like this, when you try to select
that edge for the loft, you might accidentally
select the sketch instead because it's exactly
over the top of that edge. If you find this is happening, if you're selecting the
sketch instead of the edge, what you can do is just
turn off the sketches temporarily by clicking this
option here. Hide all types. That will just turn
off the visibility of everything like the
sketches and the planes. We can then select the
edge that we want. Let's click around
here on the edge. And then click around
the corresponding area on this edge. And you should see the edges
joined with a preview. Like this, you can then
re show the sketches and the edges if you need to by clicking that same button. Again, the Hide
all types button. Now before we press okay
to make that surface, we've got quite a
sharp joint between that loft and the
two other surfaces. So let's expand the start
and end constraints, and let's change both of
them to tangent to face. And that will give us a
much smoother transition between the three faces by creating the
surfaces in this order with this loft that joins them
in the middle at the end. It just means that we can make this loft tangent to both
surfaces on each side. If we had made the head
first and then made this joining section and then made the final
piece of the handle, it would just be trickier to
add that final transition. Still keep both the
tangency that we want and also the correct guide
curve from the side. But by making in this order, it's quite easy to do all that. Let's press okay to
add that new surface. The model is looking like
a spoon at the moment, Maybe more like a shovel. But if you look closely, you might be able to see that the end of the handle
is a little bit short. Luckily, this is
a very quick fix. We can extend this using the extend surface tool that's
here on the surfaces tab. First, we'll make sure
we're on the same surface. Then we'll choose
the edge to extend, which is this end edge. And then just set
the value so that the extended edge totally
covers that top profile. For me, 10 millimeters extends that edge completely past that top profile.
And then press. Okay. And we've added that new section next up we can trim away
the excess material. And that will bring out
the shape of the spoon. But before we do that, we'll
knit the surfaces together. They're one single surface. Let's go to knit surfaces. Select the three surfaces, and then you don't
need to select any of these
options, just press. Okay. Now we just have
one single surface that's roughly in the
shape of the spoon and we can trim away the excess. Let's go to Trim surfaces. Choose the standard
option for the trim tool. Let's choose that first
Sketch the top profile, and then we'll use
Remove Selections. And then we just want
to click the areas we want to remove for me. When I click it, it
selects the entire area, depending on how far you
extended the handle. At the top, you
might need to click a few different areas to
trim away all of the excess, but when it looks good, press. Okay. And now we've really brought out the shape
of the spoon there. And if I turn off the
sketches in the planes, we can really see the
shape of the spoon there. To finish this off,
we can turn it into a solid by using thicken. Let's select thicken up here. Let's choose the surface
will thicken on both sides. And for the thickness, let's choose 1 millimeter
and then press okay. There we have created
our solid spoon. As we said, it's
quite a simple part, but we practiced a few
different things in this video. We used all of those sketches
from the previous video. First, we created
a boundary surface to make the head or
the bowl or the spoon. And we used the
selection manager to just select one single
entity from the sketch. Next up, we used the lofted
surface to make the handle, and we used the guide curve
to give it that slight curve. Then we joined the handle and the head using another
lofted surface. And this allowed us to make the transitions
tangent to each other, so they were nice and smooth. The handle was a little
short at the top. We extended that using
extended surfaces. Then we knitted
everything together. We used the trim surfaces
with a sketch to cut away the excess material that
revealed the spoon shape. So we finally used thicken to make that surface
into a solid. We've now covered the majority of the surface tools
and techniques. In the next section,
we'll start going over some tools that
are a bit more niche, maybe aren't used as much, and we'll start off with
the flattened tool.
18. Surface Flatten: Welcome to the last
section of the course. As we said in the
previous video, we've now looked at all of
the main surfacing tools. In this one, we'll
go over some of the remaining tools which aren't really used
quite so often. The first one is
flattened surface. Now if you've ever
used solid work, sheet metal, you've
probably come across something quite
similar to this. It just lets you flatten
curved surfaces. First, we'll have a look
at a basic example, then we'll talk about a
more practical example to show you how the tool works. I'll start a new part and
I'm going to start sketch on the front plane and sketch a
three point arc like this. I'll make the two
ends horizontal. I'll set it as 200
millimeters wide, radius of 100 millimeters. Then we'll use this to
make an extruded surface, so let's go mid plane. 200 millimeters wide also. And then press, okay, and we have a curved surface like this. Now let's say we need to
flatten this for some reason. Maybe you're making a
decal or you're making apart from fabric or paper
or even sheet metal. To do this, we can
go to surfaces. We can go to surface
flatten, which is here. First we need to choose the
surface we want to flatten. Let's choose this
one. Then we need to choose an edge or
vertex to flatten from. Let's choose this lower edge. You should get a
preview like this. This is the flattened
or unfolded version of that curved surface. You've got the
accuracy down here. I'll set the accuracy all
the way down to zero. You can see the mesh is quite
big there when we press. Okay, we've now got
that flattened surface. We've still also got the
original curved surface as well. Now if I just get the
measure tool from the evaluate tab and
I measure this edge, we can see it's
314.16 millimeters. But if I measure this one, it's actually slightly less, 313.98 That's just because we set the accuracy as
low as it would go. Those two lengths
don't quite match. For example, if
we go back and we edit that surface
flattened feature. Now if I put the accuracy all
the way to the top right, to the end of the
slider, it's going to take a little while to think
about what it's doing. And then eventually we'll have a mesh that's so dense you
can't really even see it. It just looks like the
entire surface is filled in. You can then press okay, and then we'll create the
new flattened surface with that higher accuracy. Again, it's going to take
a little bit of time to calculate how it
actually does that. You can set the accuracy
higher if you want, if you really need a
very accurate surface, but it will take a bit
more time to calculate. Now if we get the
measure tool again, remember this one was 314.16 Now this one is also
exactly the same, 314.16 You can set the accuracy all the
way up to the top, but it will slow down
your model and it will only be a little bit
more accurate really. Now I'm going to
delete that feature, the surface flatten
that we just made. And we'll have a look at a few
more options in that tool. Firstly, let's start a
sketch on the top plane. We'll go to a normal two view, so we're looking down on
our model from above. Let's get a center line and draw a center line across the
middle of the part like this. Then get a center point circle. And draw a circle at the
midpoint of that center line, give that 100
millimeter diameter. And then also get
the line tool and draw a line straight up the
middle here to the edge. And then another one down the
middle here to the bottom. You should end up with
something that looks like this. We're now going to
use this sketch to split that surface
into smaller faces. Go to features,
curves, split line. Then make sure you're on
the projection option. Make sure we've got
that sketch that we just drew in the
selection here. And then for the
surface, let's choose just that surface we
made, press okay. And we've now split that surface into three smaller faces. Now we can do the flatten again. Let's go to surfaces
surface flatten. This time we'll choose
this first surface, we'll choose the
same lower edge. And you can see we've just flattened that face
in the preview. We can also choose the rest of the faces and the law
be flattened together. But before we press okay, we can also click here
in additional entities. Then we can select
the two halves of that circle that we sketch. And we can see that that
circle profile will now be projected onto that
new flattened face. If I press, okay, we've now
got a new flattened face, and it's quite hard to see, but we do have that circle projected onto the
flattened face. This can be really
useful if you're trying to make maybe
some labels or decals that you want to put onto a curved or
rounded surface. Then finally, if we edit
that feature, again, the surface flattened feature, we can also add some
small relief cuts. We can put a check in the box. And then we can choose those
two straight lines that we added on the right and the left. Then you can press
okay. If a zoom in, you can see we've added two small slits here around
where the circle is. In this case, we probably
wouldn't need them because we're basically just
flattening in one plane. We're unrolling the shape. If this was more of a dome
shape rather than a cylinder, we might need to add more
relief cuts to help it flatten out from three
D to two D properly, without tearing or crinkling. You can manually add
these relief cuts in like that in terms of actually using the
flattened surface feature. Personally, I've used
it quite a few times. One in particular
where it was useful. I was creating some plywood
furniture for a client. And they had plywood curved
sides on the furniture. Normally, I model these in
solid work, sheet metal. Flatten the parts. And
then the factory uses those two D templates to cut out the flat plywood and then
curve it around the chairs. But for some reason I had one part that wouldn't
flatten properly. It must have been a
nonstandard bend or something. Instead of using the
flattening in sheet metal, I was able to just copy that surface and then
use the surface flatten. And then I could use
that two D flattened surface to make a
two D DXF file, which could then be used
to make the template. Another example I've
also seen online was somebody making a pair
of shoes In solid works, they were then flattening each of the faces and
then printing out those flattened faces and tracing around them
on leather or canvas. And then using all of
those different parts to make the different
parts of the shoe that they could then
stitch together. And then finally,
another example that I've also used myself. I've previously modeled up some bicycle frames for clients. Often these have tubes that
join at different angles. So I'm going to start a new
part to explain this one. You don't have to
follow along with this. You can just watch when
modeling these bike frames, we have tubes that join
at different angles. Say for example, we have a
tube that's 1 " in diameter. It's 25.4 millimeters, it's got 1 millimeter
wall thickness. Let's say it's 100
millimeters long, like this. This isn't necessarily
pure surfacing, but you can use the
surfacing tools to help you do things like this. If we had another tube joining this one from
the side like this. So let's say we had another one that was also 1 " diameter, 1 millimeter wall thickness, and it came in from the side. Let's offset it, and let's
go in up to next like this. I'm going to make it so
the two parts don't merge. So we can see the join there. If we have two tubes
that join like this, when we cut this
tube on the left, you have to grind away
this curved shape here, so the two tubes fit
together nicely. And then you can
weld them together. And it can really speed things
up If you have a template so you don't have to
go back and forth and constantly check the fit. What you can do is
make a two D template, print it onto paper, and then cut it
out with scissors, wrap it around the tube, and it basically shows you
where you need to cut. When you have a straight tube like this, it's
pretty easy to do. You can basically
model up the tubes as sheet metal parts and then you can unroll the tube
or flatten it. Then you can get the profile
and use it as a template. The problem comes when
you have a curved tube, because you can't
actually flatten a curved tube in solid
work, sheet metal. If we had a tube that
was more like this, maybe something with a
radius of 100 millimeters, 50 millimeters out to the left, and 15 millimeters upwards. And then I'll add a new plane
on the end of that curve. I'll draw out the tube profile, also 1 " 1 millimeter
wall thickness, and then sweep
along it like this. And then I'll
finally trim the end of the tube using the other one, using a combined feature
and the subtract option. And we should end up with
something like this. So it's a curved
tube and we need to cut away that profile
on the end of it. But unfortunately,
it's not possible to flatten these curved
tubes in sheet metal. Instead, we can use the
surface flatten to do this. First off, I'm going to
cut a very small slit along the top of the tube. Just so that we've got two half of the tube that we
can flatten along. I'm going to use the
center rectangle. I'm just going to make
it 0.01 millimeters. So it's basically like,
you can ignore it, it's so thin going to make
that cut all the way through. And we might have to go in both directions to ensure it cuts all the way
through the tube. Then finally, we can go
to the surfaces tab. We can choose flattened
surface or surface flatten. Let's choose that face
here for the edge. Let's choose that edge
of the cut we just made. And we can see on the preview, we're going to make a
shape that follows that cut all the way around as
it wraps around the tube. And if I press okay, it's a surface like this. We could now save this
surface as a DXF. We could print it out. We could
cut it out with scissors. And then we could wrap it
around the curved tube. And that will give us a guideline of where
we need to cut. There probably are
some areas where it will be a little bit
crinkled or a little bit stretch just due
to the nature of a curved face turning
into a flat face. But it will definitely be much easier than just trying
to eyeball letter. So that's the surface
flattened tool. It is a bit of a
specialist tool, but when you do need it,
it's very useful to use it. Just select the
surface, then select the edge of the vertex
you want to flatten from. You can also add in
additional entities, things like sketches, which will be projected onto
the flat surface. You can also add relief cuts, which you're manually sketching, and they can sometimes
help with flattening a three D surface out
into a two D surface. In the next video,
we'll be looking at the surface from mesh tool.
19. 19 Surface from Mesh: Surface for a mesh
is the next tool and we're not going to
spend too long on this one, because most people probably
won't really use it much. And also the use of it really depends on the
type of model you use. Personally, I don't think
I've ever really used it. Apart from just testing out and figuring
out how it works, We can use this feature
to convert a mesh model, which is something
like an STL file for three D printing into surfaces. And then we can create a
proper solid works model from that that we can use
for further modeling. To get started, let's
import this example file. It's an STL file and it's
a little measuring spoon. You should just be
able to drag it into solid Works and it
will appear like this. And we can turn on the
shaded with edges view like this and we can see it's made up of loads of small triangles. That's how STL files
are built from a mesh of loads of
different triangles. Here on the feature
tree, we've just got one single imported feature. First up, let's find the
surface from mesh tool. It's here in insert
surface, surface from mesh. We've got some information
up here on how it works, but basically what we
need to do is first choose the type of
surface planer, spherical cylinder and so on. And you can see as we hover
over the different options. If you've got the
dynamic help on, it'll give you a bit
more information on how everything works. First up, let's choose planer. This will let us select
various flat surfaces. We need to zoom in and choose
some flat planar surfaces. For example, we can
select this one. This one. We can select
all of them if we need to. It can be a bit tedious
sometimes using this model. What you can do
instead is click on this paint brush
icon, paint select. Then you can just left click and drag your mouse over surfaces to select them instead of having to click all of them one by one. Now it's just a
case of selecting the surfaces that
we want to convert. The little quirk of
the tool is that before you use the
paint brush select, you actually have to
click on a face directly. You need to make sure
that you have a face in that selection box on the left before you use the
paintbrush tool. Otherwise, it won't
work properly. You also don't always have to select the whole set of faces, especially if it's
a planar surface. So we've got a few of those top planar surfaces
already selected. Let's press. Okay. And
it's kind of hard to see, but we have added a
new surface there. We're still in the tool,
but if we exit it, we can now see we've got a new surface body in the
surface body's folder. I hide the original body by expanding this folder
and pressing hide. We can see that new surface
that we added on the top. It follows the whole shape
of the top of the spoon, even though we didn't select
every single face on there. You can also extend the surface
when you're creating it. For example, if I edit this
surface that we made here, then you can extend it
here by a certain amount. You can see in the preview
there, it's changing. Next, I'm just going to re
show that graphics body. And let's try again
with the same tool but with a spherical surface. This time instead of finding the tool in the menus this time I'm going to go up
to the search bar. Going to make sure I'm on
the commands drop down. And then in the box
start to type in mesh. We want to use this
one surface for mesh, let's click on that
for the mesh type. Let's choose spherical. Remember, let's select one
of the faces manually first, before we start painting them. Then let's select the
Paint Select tool. And we'll try to select all of those spherical faces inside the head of the
measuring spoon there. Sometimes it can be
easier if you zoom out and just paint the
whole area like this. If you accidentally get
some areas you don't want, you can hold down the old key and then when you
paint over those, it will remove that selection. I'm going to try and select
everything in there. It's worth taking your
time and trying to make sure you've got
everything selected. It can be a bit of a slow, tedious process and the tool is a little bit temperamental. Often, especially if it's quite
a simple model like this, it can be easier just to
recreate the surfaces manually. For example, for
this curved bowl, you could use something
like a revolved surface and then just to
revolve it 180 degrees. When you're happy
with the selection, you can press okay to
make the new surface. If you find you press okay
and you get an error, you can try adjusting
the facet tolerance. If you do get the error,
it's worth reading through all the different
options there and making sure you fulfilled all
of those conditions. I did get an error. I'm going to reduce the facet
tolerance a little bit. And then try again. Press
Okay, that did seem to work. If we expand this
second feature tree, we can see we do now have
a second surface in there. Another surface was created. I'm going to close that tool
and hide the original body. Now we can see we do have
a new spherical surface that doesn't cover the hole
inside of the spoon head. So we might just have to go
in and re edit that feature, make sure we've got
a full selection, and make sure there are
no missing parts there. As I say, this tool can be
a bit finicky sometimes. It can probably be worth trying this tool and if it
doesn't work straightway, maybe do 5 minutes
of troubleshooting. And if you still can't get it, maybe just make the
parts manually, but assuming everything
works properly, when you're done, you can
edit these surfaces further. So for example, we could make that whole sphere and then
we could thicken it and then we could use that top surface to magnifying glass shape to
do maybe another thicken. Or we could maybe convert
the outer edge of it and then use that with something
like an extruded boss base. That was a very
quick introduction to recap the surface
from mesh tool. It can be used with mesh models, things like STL files. When you open the tool, first
select the surface type, for example, planer, then
select the surfaces you want. You can also use
the paint select. If you need to speed up the selection, then
you can press okay. You can also edit the tolerance
if you're having issues. And you can extend the
surface size if needed. In the next video, we'll have a look at
the free form tool.
20. Freeform Surfacing: We're nearly at the
end of the course. Now we have two more
tools to look at, free form and cut with surface. This video covers free form. This tool basically
just lets you go completely free form and make
whatever shape you want. Let's start a new part
and have a look at it. Start a sketch on the
top plane sketch. A sent a rectangle at the
origin and make it say, 200 millimeters
wide and 100 high. Then select planar surface. We should just have a flat, rectangular surface like this. Free form can be found
here on the surfaces tab. Let's select it first. It looks like there's
tons of options, but the principle is
quite simple really. We're going to do is
add control points to the face we want to change. And then we can
drag those points around and that will deform
the shape of the surface. First we have to
select the surface. Let's select this
one we've just made. Then you'll see grid on
the surface like this. You can also choose the
face of a solid body. It doesn't have to be a
surface just on its own. As I said, we'll use control points to
deform the surface. But first, we need to add what
are called control curves. These are basically lines
that criss cross the surface, and then you can
place the control points on these curves. Let's click here,
Control curves. Let's click Add Curves, And then hover the
mouse over the surface. And you should see we've got a green line that
follows the mouse. I'm going to left click
to add a line here. And then another one on this
side, somewhere about here. We can also press
flip direction, and that I'll spin the
line around 90 degrees. Let's add another
line about here, and then another one about here. We've now got four control
curves that cross the surface. We can then place control
points on these curves. Let's go over here,
let's choose add points, then let's hover over those
control curves we just made. You see, when I
do hover over it, we've already got some
control points on there where the control curves
intersect with each other. But we can add more points. Just add maybe a few
like here and here. If you go onto another
control curve, the first curves
points will disappear. They are still there, they're
just not visible anymore. Let's add a few more
control points like this. Then we can click
the button again to stop adding new points. We can now select any of
these control curves. We can choose one of the points. We can click on it
and we can drag it around to deform the surface. You can use the triad
arrows to drag it around. And you see as we do it changes the shape of
the surface like this. You can go up or
down, left or right, any direction we could say get this one and
move it down like this. You can see it's a
very powerful way of deforming the whole
surface like this. And this blue plane that we can see is basically the midpoint, or the starting
point, of the face. You can see if we
look underneath, we've got some parts of the surface that
are now below it, and on the top we've got some
parts that are raised above it when we select the lines. And then the control points, you can drag the control point directly around or you
can use the arrows, or you can adjust the value
down here on the left, if you set a value
of zero down here, it just moves the control point back to the original location. Take a little bit of time,
have a play around with those control points and see
what shape you can make. When you're happy
you can press okay, and now we have that
new free form surface. Hopefully you can
see potentially, this is a very powerful
way of modeling. I'm now just going to delete that first free form surface. We'll create a new
one so we can have a look at some of the
options of the tool. Now we've just got
that flat plane again. I'm going to choose
free form again, and I'm going to choose
that face again. The first option
we can use is that we can make the
face symmetrical. So you can go symmetrical in direction one or direction two. I'm going to choose
direction two. The face will now
stay symmetrical about this gray
plane in the middle. If we now add a control
curve, say here, and then we add a
control point like here, then we've automatically got the same point on
the right hand side. Whatever I do to
this one on the left will also automatically be
done to the one on the right. If I drag this one up, now you can see the one
on the right also moves. This is a really
good way to make your surface completely
symmetrical. If you didn't have
this symmetric option, it'd be really difficult to make your surface symmetrical. Another option you
can change is from three points here
to control points. This joins the control points
with these polygon lines. And basically it just
gives you a little bit of a different visualization
of how the points are linked together and how
your surface is being made. Next, we can change the direction of the
coordinate system. Here we're currently on natural, You can change it
to user defined. When you change it, it will clear any control
points that you already have and then you can rotate the direction to
whatever you want. I'll just add a few more
curves and points back in, say here, just so we can
see the next options. And then say, let's pull up
this control point like this. These options, the
triad orientation, that adjusts where the
triad arrows are pointing. You can see as I go
through the options, it changes exactly where
the arrows are pointing. And that will help
you control the triad a little bit more
accurately if needed. Then the options down here at the bottom are all
just visual, really, we've got things like
the mesh preview, the zebra stripes, the
curvature combs and so on. If you want to use
the zebra stripes, it doesn't always show
directly within the tool. Here it seems to be a
bit of a graphic glitch. Instead, you can make
the feature first, then check the zebra
stripes later by going to the evaluate tab and
pressing zebra stripes. Basically when the stripes
are close together, it means you've got more of
a gradient on the surface. Then I'll just turn off the
zebra stripes and I'll go back in and edit that
free form feature again. Then finally we've just
got these edge options. These allow you to control how the surface joins
the edge around it, we're currently on contact. If I change this to tangent, you see it changes the
shape around that area. It now means that the surface is joining that edge tangent. So it's going to be flat
when it joins that edge. You have those different
options and you can choose whatever suits
your model the best. That is the free form tool, it's potentially a
very powerful one. What you do is
select the surface. This can be the face of a
solid or a separate surface. Then you add those
control curves, which are lines
along the surface. Then you add control points on those curves and
you can drag those around or adjust the values and use those to
deform the surface. At this stage, let's just save this surface as we'll also
use it in the next video, which is the last tool
and is cut with surface.
21. Cut with Surface and Thickened Cut: We're now on the final tool, or the final two
tools of the course. These are the cut with surface
and the thickened cut. I initially wasn't
going to include these because they're both
quite straightforward, but I thought I'd just add
them for completeness. We left the previous video like this with a
deformed surface. You've probably got a little bit of a different shape to me, but it should look roughly
something like this. If you don't have this,
it's just a planer surface that's 200 by 100 millimeters. And then we use the
free form Deformed tool to create something like this. We can use surfaces
like this one or ones made in any other
way to cut solid. To show this, let's make a
solid cube in our model. Start a sketch on the top
plane, go to a top view, and then draw a center
rectangle that's 100 by 50. It's inside the footprint of the surface that
we drew like this. Then let's do a
midplane extrude and we'll make it 100 millimeters. Basically, it should strand
on the entire surface. The surface should cut
through it like this. Now we've got a block in
the middle of that surface. We're going to use that
surface to cut the solid. Go to the surfaces tab and
choose Cut With surface. Then just choose the surface. This arrow shows the
side we're going to cut. We're currently cutting down. If you click this
reverse direction box, we'll then cut up and then
press okay. And that's it. If we hide that surface by hovering over it
and pressing tab, we can see we've cut the top of that solid block
using that surface. This tool is a very simple one, but it can be really
useful if you've made a nice flowing surface and you want to use that shape
on a solid part. When you're doing
cuts like this, try to make sure that
your surface extends all the way past the edge of
the solid you're cutting. This can just help avoid any
issues around the edges. You can also use the extended surface to do this
if you need to. That's the cut with
surface. Let's delete that Cut with Surface feature. And then there's a similar
option called thickened cut. This will basically thicken your surface and then cut
that away from the solid. This can be useful when
making things like mold or adding
clearance to models. To use this, let's go to
surfaces thickened cut, choose the surface,
set the thickness. Let's go with 10 millimeters and then choose
the sides to cut. Let's go with both sides, so it'll be 5 millimeters
on each side. And then press, okay.
You'll probably get this pop up the
parts now, split in two. This is asking you which of those two parts we want to keep. We can just keep all of them. You can also click
Selected Bodies, and then you can
choose either the bottom one at the
top one, or both. For this, I'm going to
choose both. Going to press. Okay. Now we see we've got that cut all the
way through the block, 10 millimeters all
the way through. If we had tried to make this
cut with solid modeling, it would have been
pretty difficult. But it's actually
completely trivial. With a mixture of surfacing
and solid modeling, that's the cut with
surface options. Both are quite simple. For the cut with
surface, just choose the surface and then set the
direction and press. Okay. Try to ensure that
your surface extends past the edge of the area
that you want to cut. Then for the thickened surface, again, you just
choose the surface. You set the thickness
you want and the direction, and
then you make the cut. You might also need to choose which bodies you want to keep. If you've split the bodies
up into multiple parts, we're now pretty much at
the end of the course. Well done, and I hope
that this has given you some new skills that you can use to take your modeling
up to the next level. In the next and final video, we'll have a recap of
everything we've learned and we'll whizz through
all of those tools again.
22. Conclusion: This is the last
video of the course. So we're just going to quickly recap everything we've covered pretty quickly in regards
to solid work surfacing. In the introduction, we made
that cube and we looked at the differences between solid modeling and surface modeling. We talked about first making an outer shell out of surfaces and then knitting those together and using that to
create a solid. We also mentioned that
surfaces have no thickness. Then before we actually
started surfacing proper, we looked at the delete face. This is great for
removing fillets or adjusting holes and
openings in parts. Then the move face tool was quite similar in a lot of ways, but this one allows you
to offset, translate, or move or rotate faces
in any direction. It allows you to very quickly
adjust preexisting parts. And it can be useful for imported parts where you don't have access to
the feature tree. After that, we made our first model, the candlestick holder. This was quite a simple one, but we learned a bit about extruded surfaces and
how you can trim them. We also looked at the
ruled surface tool, which allows you to easily add material in a
specified direction. And then we knitted
all of the surfaces together and we saw that you
can easily fill it edges. And then finally, we
used the thickened tool, which is a great way to convert your surfaces into solids. Next, we started
to look at some of the more advanced techniques by creating the host pipe
spray or the paint sprayer, Initially with revolved
and lofted surfaces. The lofts can be quite powerful, especially when
they're used with guide curves and pull points. Then we looked at swept
surfaces both to create the simple front nozzle and also the more complex
handle grip shape. With the swept surfaces, guide curves can be
used to create shapes that otherwise would be
very difficult to make. Next, we developed the
model further by connecting the previous surface bodies using more advanced
lofted surfaces. To help create these, we
use the split line tool to split surfaces down into
smaller multiple faces. Then we also use the filled
surface tool as well as planer surfaces and mirrored surface bodies to close
off the sprayer body. So we could either
knit it into a solid or we could use thicken. For the next model, we learned about the boundary surface tool. This is a bit like the
lofted surface tool, but it's a bit more
powerful as you can control direction one and
direction two separately. Rather than just using
profiles and guide curves, we use this tool to create
the vacuum cleaner nozzle. And then we develop that
model further looking at how you can use things like
project curve to make curves. And we also looked at
the offset copy tool and the different
ways we can use that. Next, we practice some of the tools by making
the spoon model. First, we set up all the
construction sketches, and then we use the
boundary surface and lofted surfaces to
make the spoon shape. We also learn how to use
the selection manager and the extend surface tool before
trimming the spoon shape, and then using thickened
to create a solid. After finishing the spoon model, we've got into some of the more specialist
surfacing tools, starting with surface flatten. You can use this to
flatten surfaces and it can be useful in
lots of different ways, especially things like
creating labels or decals or making templates
for prototyping. Next we briefly looked at the
surface from mesh tool that allows you to extract
surfaces from three D meshes, like STL files, which are normally used for
three D printing. Then came the free form tool. This is a very
powerful way to get organic looking
shapes and surfaces. You can then use
these for things like cut with surface
or thickened cut. Those are the final two
tools that we looked at. That's everything we
covered in this course. As we mentioned, you
don't always have to use only solid modeling or
only surface modeling. It's usually good to
use a combination of both sets of skills to get
the end result you want. Surfacing is really just
another set of tools that you can layer on top of your
basic solid modeling. With that in mind, happy
modeling and good luck with your Cad careers if
you're going down that route. If anyone makes any particularly cool models with surfacing, then please just add them
into the Q and A below so we can all see them and get
some inspiration from those. Finally, thank you for
taking the course.
Johno Ellison, Professional Design Engineer
