Video summary
The video demonstrates how to model a ceramic mug in SolidWorks by separating the process into two main components: the central body and the handle. The creator begins by setting up a sketch on the front plane to define the cross-section of the mug's center part, utilizing a construction line as an axis of symmetry. By drawing arcs and lines that represent both the inner and outer surfaces, the user applies specific dimensions such as a 4.5-inch radius for the top arc and a height of four inches. To ensure the wall thickness is consistent, the sketcher uses the offset entities tool to duplicate the profile lines by 0.085 inches before closing the region with a line at the top, which is essential for SolidWorks to correctly identify the area intended for revolution.
Once the two-dimensional profile is fully defined and closed, the modeler employs the Revolved Base feature to generate the three-dimensional body of the mug around the central axis. With the main structure complete, attention shifts to creating the handle on the front plane using an Extruded Base feature. The design involves two semi-circular arcs that form the shape of the handle, which are also offset to create the necessary thickness. A critical technical detail highlighted in the tutorial is the method used to attach the handle to the curved surface of the mug; instead of starting the extrusion at the outer edge where it would float in space, the sketch points are constrained to coincide with the inner surface of the mug. This ensures that when the handle is extruded linearly, it remains attached to and follows the curvature of the mug's interior rather than intersecting or floating away from it.
To finalize the handle geometry, the creator addresses a geometric challenge at the bottom of the handle where a straight line would not perfectly align with the curved inner surface of the mug. To maintain precision, an additional arc is drawn to connect the two points on the inside surface, ensuring that this new arc shares the same center point and radius as the mug's inner profile through co-radial constraints. This results in a fully defined sketch with no under-constrained elements. Finally, the handle is extruded with a thickness of 0.5 inches using the midplane option, successfully merging with the mug body to create a seamless attachment. The video concludes by rotating the completed model to an isometric view, showcasing the finished mug with its properly integrated handle.
Read the full video transcript
I'm going to be trying to make this mug
and there are a couple of ways I could
approach that but all of them pretty
much have the same thing in common I'm
going to be trying to generate the
center part of the mug and then the
handle separately
the center part of the mug could be done
using a shell or a thin feature but for
the moment I'm going to be drawing the
inside and outside surface on the same
sketch and then revolving them around a
center axis to produce my shape then
once I have my shape I'm going to draw a
cross-sectional view of the handle on
the front plane and then I'm going to
extrude it to create the handle
so if I jump into SolidWorks I'm going
to be creating a new part
and I'm going to start with a sketch on
the front plane
so I need to draw half of what the cross
section of just the center part of the
mug would look like
so the basic shape of that is going to
be a line and I'm going to start that at
the origin
a line and then I need an arc so I'm
going to draw a let's go A Center Point
Arc here
and then I'm going to draw another line
so that'll give me my basic shape now I
can start to constrain and dimension
that shape so I know that the inside
is going to be the same basic shape so
if I Dimension and constrain the outside
I can just copy that to make the inside
surface so let's start with that Arc
that Arc needs to have a radius of 4.5
inches so I go up to Smart Dimension and
then click the arc I can give it a
radius and I'm going to say 4.5 inches
then I can also recognize that the
outside of my mug here that or should I
say the outside top part is going to
have a diameter of
let's see here three and a half inches
so I'm going to make a construction line
in the center to represent my Axis of
Symmetry and I'm going to make that
infinitely long and vertical
and then I'm going to
constrain that to the origin because I
missed that click now I can tell
SolidWorks that this top outside part of
the mug should have a radius of one half
of three and a half inches so 3.5
divided by two
cool broke it already
now I'm going to be dragging in this
point down here in the corner so I'm
going to exit out a sketch Dimension or
smart Dimension and then shape this a
little better
then I'm going to click this line and
shift-click the arc and tell SolidWorks
I want those two features to be tangent
to each other
I'm going to give it the horizontal
distance of the bottom part of the mug
which I know from the sketch has a
diameter of 1.75 inches so 1.75 divided
by 2 would give me that radius
now you see how the entire sketch is
fully defined except for this blue dot
up here that blue dot if I drag it
around is not vertically constrained so
I should add a height to my mug which is
shown over here in the side view
that height is four inches so if I click
the dot and the line and then drag that
out to the side I need that to be four
inches tall
and that's the basic shape of my mug
now I'm going to duplicate those so I'm
going to repeat the same I guess I could
repeat the same process generate an arc
generate a line generate a line or if I
wanted to I could highlight these
three lines that I just drew and use the
offset entities tool as kind of a
shortcut
so I want to make those lines be
duplicated a certain dimension in so I'm
going to look at my part here and I see
that I want the thickness of that wall
to be 0.085 inches so I want this to be
0.085 inches and if I hit OK it will
duplicate those lines
create a copy of them
.085 inches in so I'm very nearly there
I need to close this sketch by adding a
line at the top
to represent the actual top surface of
my mug and then I'm going to close down
here
so that SolidWorks knows the actual
region that I want to revolve around
this axis if I left that open
it would have had to guess that I wanted
the axis to be the center sort of like
using the fill tool and paint you know
if you don't have that region closed it
could fill everywhere SolidWorks so get
a little bit confused so I'm going to
use features and then I want to use the
revolved base
to create
my 3D part around that axis of
Revolution that I already defined that
was my construction line and then I want
to select the Contour to revolve and I'm
going to click this region
and hit OK
and I'm now looking at a mug without a
handle so that's okay we're starting to
get a handle on this so if I look at it
from the front view the reason I chose
the front view is because I'm going to
be drawing in the front plane the reason
I know I'm going to be drawing on the
front plane is because I want that
handle to be visible from the front view
if looking at it from the side I should
see just a rectangle
so on that front view I'm going to add a
sketch to represent the shape of the
handle and then I'm going to use the
extruded base to actually generate the
3D object
so I'm going to create a new sketch
and I'm going to create that sketch on
the front plane
now I know that that handle actually
consists of two semi-circles there's
this semi-circle up here which has a
radius of 1.15 inches and that starts or
rather the center point is right here on
the edge of the mug and at this
intersect between the arc and the line
that we use to generate the middle part
so that Center Point will be on the edge
of the mug and then I want it to end
horizontally aligned to that Center
Point then the second semi-circle has a
Center Point horizontally aligned to the
center point of the first Arc and that
has a radius of 2.15 so I'm going to
create those basic shapes I want to
create a Center Point Arc I'm going to
click here to represent the center point
of my arc I'm going to click up here
and then I'm going to create an arc
that ends horizontally from the center
point of that Arc
now I'll add a dimension
I want that to have a radius of 1.15
then I'm going to add another Center
Point Arc so I want that second Center
Point to be somewhere else horizontally
aligned with that first center point so
I'll click over here and then I want the
arc to start
with this Arc and then go down and stop
at the edge of the mug
and then I can Dimension that and say it
has a dimension of
2.15 inches
then I want SolidWorks to know that
these two arcs need to be tangent to
each other
and now you see that line is fully
defined
so I can repeat the same process I did
earlier I can highlight these two arcs
and use the offset entities tool to
create a duplicate of them in a certain
direction in this case that offset needs
to be 0.15 inches so I'm going to say
0.15 inches
and then I will accept that and it'll
create that duplicate so there are a
couple of issues here the first issue is
the fact that this region still isn't
closed I need to close this region in
order to extrude it so SolidWorks knows
what I actually want to extrude
the second thing is that if I were to
start this handle at this surface of the
mug
like if you looked at it from the top
if I extruded that line away linearly it
wouldn't actually follow the surface of
the mug the mug is Round And if I
extruded linearly I would end up out
here in space I wouldn't actually be
touching the mug anywhere but at this
Center Point
so what I need to do to fix that is not
actually start my handle at the edge of
my mug I want to start the handle a
little bit inside of the part of my mug
so by starting inside of the mug when I
extrude those bodies will all be
combined and I will end up with a handle
that follows the surface of the mug
so
I'm going to jump back to my sketch
and I'm actually going to remove this
constraint that I added earlier I'm
going to click on that green box
and now that dot has turned blue
and I can drag it around I clicked on
that box and hit delete by the way so
I'm going to drag it inside and then I'm
going to make this follow that dot I
want both of them to be inside now how
much inside uh depends I really only
need enough to ensure that when I
extrude that it isn't outside of the
surface of the mug but just for
convenience's sake I'm actually going to
constrain these two points to the inside
surface of the mug so if I change my
view style from shaded with an outline
by clicking this button up here the
fifth button from the left or sixth
button from the left
and then change it to hidden lines
visible
now I kind of have an x-ray view of my
mug
and if I click on this dashed line
that would represent the inside surface
of the mug so if I click on that line
and then I shift-click this point I can
hit coincident
and now that dot is actually aligned
with the inside surface of my mug so by
starting from the inside surface and
extruding linearly I ensure that I never
actually go into the inside of my mug
and I am definitely going to have a
handle that is inside the the mug
thickness the whole time the nice thing
about constraining it as opposed to
dimensioning it is that now if I needed
to resize the mug it's likely that the
handle would follow this and not be
screwed up another way to approach this
would be to create a single entity for
the big mug add a handle and then add
the cut after the handle the cut
representing the inside of the mug if I
cut out the enter the center of the mug
after I had added the handle then it
would cut out the material of the handle
as well and I wouldn't have to worry
about it
but
continuing this process I'm going to
click that point shift-click this line
hit coincident now both of these two
points are on the inside surface I'm
going to repeat that process down at the
bottom I'm going to click this point and
then click the line and then click cons
excuse me
coincident so let's try that again point
line coincident
and SolidWorks is throwing up an error
so I'm going to remove
the coincident and try to diagnose the
error here
let's try that
maybe the third time's a charm if
something doesn't work just continue to
try it until it works for some reason
great
I'm going to remove this coincident and
repeat the process
there we go now I have my handle
constrained to the inside surface of my
mug now I need to close the sketch which
on the top part is pretty easy I just
add a line between these two points
now on the bottom part if I were to just
use a line to connect these two points
then geometrically speaking that line is
going to be not quite aligned with The
Arc that represents the actual inside
surface of the mug and that line in
reality would be on the inside of the
arc representing the curve of the inside
of the mug so for good practice here
let's create an arc that follows the
actual inside surface of the mug so I'm
going to use the center point Arc tool
again and I'm going to start my arc from
the center point of the arc that
represents the inside surface of the mug
so the way I got that Center Point to
appear is just kind of by hovering over
the inside surface and then the relevant
geometry kind of popped up so this dot
over here on the left represents the
center point of that Arc so if I click
that
and now click on one of these points and
then the second point
I now have a fully defined excuse me I
now have an arc connecting the two
points so I'm going to click on that Arc
and now click on the inside surface
again shift click and I want those two
arcs to be co-radial
and concentric
so they have the same radius and they
have the same Center Point now that line
is black it's now fully defined so if I
look at my sketch I don't see any blue
Parts which means that I have a fully
defined sketch
now I can use the extruded base
to add some thickness to my handle I'm
going to use the midpoint or mid plane
Extrusion and I need that handle to be
0.5 inches thick so 0.5
then I accept and I have a handle
so if I switch back to my shaded with
edges then change that to an isometric
view there's my mug