Video summary
The video demonstrates a comprehensive tutorial on modeling a large-scale 96-inch model rocket using SolidWorks, beginning with the creation of the main fuselage. The process starts by sketching half of the cross-section from a front view and defining key geometric features such as a 50-degree nose cone angle, a six-inch tall nozzle, and specific diameters for different body sections. By setting an axis of revolution at the origin point located at the bottom center of the nozzle, the user employs the Revolved Base feature to generate the complete cylindrical body shape in one operation.
Next, the tutorial focuses on designing and attaching three fins using a patterned approach rather than modeling each individually. The designer sketches half of a single fin profile with precise dimensions for angles and heights relative to the rocket's nozzle, then uses an Extruded Boss-Base feature set to merge results to ensure the fin attaches seamlessly to the curved body surface. To replicate this geometry around the cylinder, a circular pattern is applied by selecting the extrusion as the object to copy and defining a central axis derived from the intersection of two planes, resulting in three fins evenly spaced at 120-degree intervals without any gaps between them.
The final step involves creating an internal cutout for the rocket engine mount using another Revolved Cut feature. A new sketch is drawn on the front plane to define the geometry of this hollow section, including a half-inch thick nozzle wall and a specific height extending up the body tube. The user carefully positions this sketch so that its centerline aligns with the origin rather than an existing axis, allowing for independent manipulation if needed before executing the cut. This method ensures that any material protruding beyond the intended internal diameter is automatically removed during the extrusion or cutting process, leaving a clean and accurate model ready for assembly.
Read the full video transcript
I'm going to be making this rocket and I
recognize that I can split it into a
couple of different components I'm going
to start with a revolved base to make
the fuselage shape this Center body part
and then I'm going to create a Single
Fin and extrude that using an extruded
base and then make a pattern of them
around the center of the rocket to
create the three fins that I need with
an offset of 120 degrees each and then
I'm going to use a Revolt cut to remove
the center part so if this were a model
rocket that might be where you put the
rocket engine although this is 96 inches
tall so maybe it's just a really really
big model rocket
anyway I'm going to start with a sketch
representing half of the cross section
of the main body of my rocket from a
front view
so if I jump into SolidWorks
and create a new part
I can create a sketch on the front plane
and then I'm going to be making the
basic geometry first and then going
through and dimensioning it so I
recognize that I want to have
a vertical line up the center and then
an angle down and then a vertical line
down and then a little jut in here for
the nozzle and then an angle down and
then a horizontal line to complete the
sketch I'm going to arbitrarily decide
that the origin point of my model should
be the center of the bottom of the
nozzle so I'll be using that
now if I jump back into SolidWorks I can
add a
let's try that a line of the center
then an angle line for the nose a
vertical line for the outside a jut in
for the nozzle
and then an angle line and a horizontal
line
that's my general shape now I can go
through and add dimensions so I know the
height of my rocket or rather the height
from the bottom of the nozzle to the tip
which is 96 inches so I will add that
here that is 96 inches
then I know that my nose should have an
angle of 50 degrees I'm drawing half of
that so that angle should be 25 degrees
I'll use the smart Dimension tool and
that will if I click on this line in
this line that'll figure out that I want
to Dimension an angle so I'll click
there and then make this 25 degrees
because that's half of 50.
next I know that my nozzle should be six
inches tall so I can Dimension from
this vertical line
to this vertical line
tell it that should be six inches
now I will add my diameters of the
rocket which are going to be radiuses
here so if I look at my top view of my
sketch I notice I have a lot of
diameters but the first one the outside
one is 16 inches which means that this
radius here should be half of 16 which
on most days is 8.
and if you didn't want to do that math
in your head by the way if you just type
16 2 it'll do the division for you
next I notice that I need a I need
diameters of 14 and a half 14 and 12.
and if I look closely at these arrows I
see that the second line is 14 and a
half and if you picture how this would
actually look from the top that second
line is going to be this distance here
that's going to be the line created by
the top of my nozzle
therefore I'm going to make that half of
14.5
which is 7.25
and then I'm going to make the bottom of
my nozzle 12 inches in diameter which
would be a six inch radius
if you're having trouble recognizing the
distinction between these hidden lines
if you look at it from the front
see if I can get down there if you look
at it from the front you can see that
this edge of the nozzle is further out
from the center than is the inside
surface of the cutout so the second line
you see from the outside from a top
perspective is that top of the nozzle
so now I have my dimensions for the main
body everything is black which means
it's fully defined I can add a an axis
of Revolution and create the part
so I'm going to create this as an
infinitely tall vertical line from the
origin to make sure it's centered
and now I can go to Features revolved
base
and I get my basic rocket shape
cool
now I'm going to add a fin
so I'm going to add the fin on the front
plane because I want to make my model
match the model indicated in this
drawing
so the first fin here on the right
is visible perpendicularly from the
front view which means it would be drawn
on the front plane then when I create
the pattern
I end up with fins that aren't aligned
to any of the primary planes
so if I jump into the front view
and create a sketch on the front plane
I can create the shape of the fin
so I'll have
a line and then a line
little line
and then a line
how's that for a good fin
now I can add Dimensions so I need the
angle at the top to be 25 degrees so
again I'll use the smart Dimension and
then click this line and this line and
tell it that I want it to be 25 degrees
and you'll notice that that brought all
the other lines around which kind of
broke the shape of my fin but it's okay
I can bring it back by quitting the
smart Dimension tool and then dragging
this point over to where I want it to be
I'm going to tell SolidWorks I want this
line on the outside to be vertical
that way it won't uh get all Kitty
Wampus again
then I'll add another angle at the
bottom which was 45 degrees
and I'll Dimension a width which I
believe is 10 inches yes 10 inches
and I will Dimension a height from the
bottom
so I know that
the bottom of the fin is going to be
three inches below the bottom of the
nozzle
so if I click this point
and then hover over the bottom of the
nozzle and select that face
I can Dimension this as being three
inches
and then I need to add in
the fact that the height of the outside
of the fin needs to be 21 inches and
that should fully Define my fin
so
21 inches
and there we go the fin has turned black
which means it's fully defined but
here's the problem if I were to just
create a base Extrusion now I would end
up with a fin that didn't actually touch
the rocket if you look at it from a top
top view
you see how the outside surface of the
rocket is a circle I mean it's actually
a circle SolidWorks is showing a preview
view as a polygon here but it's actually
a circle this is just to save video
memory I believe it's trying to make it
easier to render whatever the case if I
were to extrude linearly here I'm going
to be going away from the body of the
rocket I want the fin to be touching the
rocket the whole time it's it's extruded
so the easiest way for me to do that is
to actually bring the Inside Edge of the
fin inside the body of the rocket
when I create the Extrusion SolidWorks
will actually join all the bodies anyway
so it doesn't really matter
so if I go back to my sketch
I'm going to first remove these two
coincidences which I Do by clicking on
the green box and hitting delete
and now I'm free to move the fin left
and right
so first of all I'm going to get rid of
this line that I didn't know was there
interesting I must have clicked a couple
too many times
and now I'm going to start my fin inside
the actual body of the rocket that's why
I chose to create the cut representing
the inside of the rocket after the fin
that way if I extrude the fin too far
the cut will remove that material as
well
so I'm going to kind of arbitrarily set
the inside of my fin as being I don't
know an inch
inside the outside surface of the rocket
and now I need to fix the rest of my
Dimensions here
so first of all I need to specify that
that 10 inches is no longer from the
inside of my sketch to the outside of my
sketch and that is from the actual
outside surface of the rocket which
again I hover over that and click and
then click on this line and now I can
add the 10 inches
there we go that brings it back I could
have also dimensioned from this line to
this line and made that 11 because it's
10 plus 1 but this way is a little bit
easier a little bit more elegant in my
opinion it doesn't actually matter what
dimension I use here I could say one
inch I could say six inches it's
actually okay because again I'm cutting
after I create the fin so the cut will
remove any extraneous material that's
going too far into the inside of the
rocket for the moment let's just stick
with one
now I have a fully defined sketch I go
to features and create an extruded base
and I need this Extrusion to happen
symmetrically so I'm going to use the
mid plane
and I need it to be a total thickness of
0.75 inches
so you see this checkbox it says merge
result that's what I was referring to
earlier SolidWorks is going to join the
bodies
and there we go we have a fin
so even though SolidWorks is showing
this again as a polygon instead of a
round surface it actually is behaving
correctly
so there isn't a single Gap
at the edge of my fin everything is good
cool
now as opposed to trying to draw two
more fins then extrude them I'm going to
copy this one Fin and create a pattern
and the type of pattern is going to be a
circular pattern not a linear pattern
because I want it to go around the
circular surface of the rocket so if you
click on the Arrow below linear pattern
you have a couple of extra patterning
options I want to use circular pattern
So within circular pattern
I have a couple of boxes this box is
currently highlighted is where I would
select my Extrusion that represents the
fin
but you'll notice nothing is happening
that's because I also need to specify
something in this box that is the axis
around which to revolve to create the
circular pattern so I don't actually
have a nice middle line
you know if this were to sketch and I
was creating a revolved Extrusion I
would create a construction line there
down the center and revolve around that
but I can't just use a construction line
here I can't use a line within a sketch
I need to use the three-dimensional
equivalent
which if I exit out of my pattern here
is an axis if I go up to reference
geometry and click on axis I can define
an axis on my part for reference so I'm
going to be creating an axis down the
middle of my rocket and I'm going to be
revolving around that so when I click on
axis I have a couple of options
SolidWorks is basically saying hey uh
where do you want that axis and I have a
couple of ways to tell it exactly where
so the first option here is I could
select a line that already exists on my
part you know if I were to select this
line on the outside my fin I could make
that be an axis but that isn't helpful
here I've got other options like two
points which is where I could select
two points on my sketch or excuse me on
my part and SolidWorks would create an
axis between them I have point and face
which I don't really have any convenient
examples of here I guess maybe this one
I could select this as the face
and then
this is the point
and SolidWorks will create an axis that
is perpendicular or rather normal to
that plane and intersects the point that
I selected that would actually work here
but it's not the one that I would prefer
to use
I have cylindrical face which if I click
on a face of a cylinder we'll create an
axis down the center that again would
work here but my favorite option for
this particular circumstance is the two
planes option SolidWorks will create an
axis at the line resultant from the
intersection of two planes so if I were
to click the front and top planes
those intersect at a line that extends
horizontally here
so because I my origin is at the bottom
center of the nozzle that horizontal
line is extending away from the bottom
center of the nozzle
so in this case if I choose the front
plane and the side plane the right plane
the resultant axis is right down the
center of my part because I revolved it
around the origin
so that's perfect that's the one I'd
like to use here
now I have an axis so if I jump back to
a front view for convenience and I go to
circular pattern I'm going to select
that Extrusion representing my fin again
and then up here in this box I'm going
to select that axis that I created
now I have some options here for example
right now I have equal spacing ticked
that means that it'll take the number of
number of iterations in the pattern and
space them equally among this angle so
right now it's taking that Extrusion and
creating three of them that are equally
spaced around 360 Degrees which is
actually what I want if I had unchecked
equal spacing I would have to specify an
offset between the fins so here I could
say 120 degrees and I would end up with
the same result
but by making this be 360 degrees and
equal spacing
I have kind of a convenient way to add
or subtract fins if I wanted to make the
worst rocket in the world I could add
just
dozens of these fins
and end up with something that looks
like a heat sink more than a rocket
and would probably fly straight but not
very far
but if I jump back into that pattern
which I did by right clicking and
clicking on edit and make this be three
now I end up with the number of fins and
the offset that I wanted three fins
spaced equally around 360 degrees
I'm very nearly done I now need to add
the cut representing the middle section
of the body
so the cut representing these hidden
lines here
and again I created the cut after the
fins so that if the fins extended too
far the cut would remove them and I'm
going to use a revolved cut because of
the rotational symmetry so I'm going to
be drawing half of this cut and then
revolving it around a center
so I'm going to create another sketch I
could do that on the front or side
planes but I'm going to do that on the
front because you know if it ain't
broken Etc
then I'm going to draw the basic shape
again which is going to go vertical line
up from the origin
over down
at an angle and then horizontally at the
bottom of the nozzle
then I'm going to add a relation for
this angled line that it needs to be
perpendicular to the outside of my
nozzle
sorry parallel to the outside of the
nozzle
and now I can start to Dimension so I
read that I need I read that I need a
half inch so the nozzle has a thickness
of half an inch
so I click on this line and this line
with the smart Dimension tell it to be
half an inch
next I'm going to add a height
so over here in the front view again I
see that the height of that cutout
section is 60 inches
so this line needs to be 60 inches tall
then I can add a radius distance
which I go back to the mess of a top
view I have here and read well that
Hidden View
that is going to be not the first hidden
line because that's the top of the
nozzle it's the second one now and that
has a diameter 14 inches
so that 14 inch diameter would mean that
I specify a radius here of 7 inches
now that sketch is black
I think
yeah it's fully defined
definitely fully defined he said
confidently
oh I see
okay
I want to make sure that that center
line that I drew is coincident to the
origin
and not the axis
okay
so I have a sketch now representing my
revolved cut and then I'm going to add a
construction line
again infinitely tall and vertical to
represent
the axis of revolution
and the reason I'm doing that instead of
just using the axis that we created
earlier is because I like the uh
the geometry in my sketch to be kind of
con contained as much as possible that
way I can mess with the axis if I wanted
to and it wouldn't interfere too much
with my sketch
then I go up to features and revolved
cut this time
and then I'm going to use the Contour
defined by this region
and then accept that cut
and you notice how nothing changed
that's because the cut is inside so if I
jump in
to a bottom view I can see that region I
just removed and to make sure that it
looks correct I'm going to go back to a
front view I'm going to change my view
settings to Hidden lines shown now I
kind of have this x-ray View
and I see that that looks pretty good
that is
pretty much exactly
what is on the drawing
excellent
and I've completed my rocket