Drawing an Involute Spur Gear from Scratch in Fusion 360

Drawing an Involute Spur Gear from Scratch in Fusion 360


hello everyone Dustin here and today I’m
gonna show you how to draw a spur gear from scratch in fusion 360 there’s
actually lots of videos on this out there but the one difference that’s
going to be shown in this video is I’m gonna show you how to draw an involute
gear tooth profile from scratch alright so the first thing we’re gonna do is
just set up some parameters that we can use for our gear creation I’ve got this
nomenclature photograph here on the side here that we can use as a reference
but there’s actually only three parameters that we need that really will
serve to define the rest of the gear properties so let’s go ahead and add
some parameters so the first parameter we need is called the modulus we’re
gonna set that to be 2 what that is is essentially a number that defines the
size of the gear teeth next we’re going to add a parameter that defines the
number of teeth on the gear call that numteeth
it doesn’t have any units and we’re gonna for this example just say that
we’ve got 20 teeth and the third parameter that we need is called the
pressure angle and what that is it’s essentially the angle that the gears
mesh at so it defines the curve curvature of the tooth so we’re going to
set that to 20 degrees there’s really only a few standard angles that are used
for the pressure angle 14 and 1/2 20 and I believe it’s 25 we want degrees for
that and those are our three primary parameters now from those we’re gonna
actually calculate a number of other parameters that will help us from having
to calculate them in line when we’re creating our model so let’s create one
more so knowing the number of teeth and the modulus we can define the pitch
diameter so the pitch diameter is simply going to be the modulus times the number
of teeth the pitch circle that’s essentially the diameter that we
is calculated we need a few other diameters that’ll help us out so the
next one we’re going to calculate is the base circle diameter and this will be
used when we get into defining the involute so we’ll come back to that here
in a minute but the the base circle diameter is
simply the pitch diameter times the cosine of the pressure angle next what
we want to do is we want to define the top the tooth and the root of the tooth
so if we look at the diagram here the addendum is shown as a measurement from
the pitch diameter to the top or the tip of the tooth and the dedendum is from the
pitch circle to the root of the tooth so let’s define those two first we’ll
define the addendum in this case to be just 1 times the modulus and the dedendum
is going to be one point two five times the modulus so now that we have those
two calculated we can actually calculate the addendum circle and the dedendum
circle or in this case I’m going to call it the addendum diameter and the dedendum diameter so I’ll called I and addendum diameter so that is going to be
the pitch diameter plus two times the addendum the reason it’s two times is
because remember we’re talking about diameter here so we have to add the
addendum to both sides of the gear to get to get the proper diameter and lastly we’re going to calculate the
dedendum diameter which is going to be the pitch circle or the pitch diameter
minus two times the dedendum okay so those are really all the parameters that
we need in order to define at least the basic geometry of our gear I’ll come
back in a minute and show you how we’re going to do the involute now that we
have our parameters defined let’s go ahead and start laying out the basic
geometry for the gear I’m go ahead and create a new component we’ll call it
spur gear and it’s already activated so let’s go ahead and create a sketch I’ll
put it on this plane here and let’s start out by laying out some
construction lines for some of the the basic geometry of the gear we’ll create
a circle with a diameter for the pitch diameter so that’s forty zoom in here
let’s lay out another line for the base diameter which is just slightly less
than the pitch one more for the route of the gear which is the dedendum diameter and the last one we’ll put on here is
the tip diameter or the addendum diameter and last I’m just going to add
a line here for the center line just like that so that really defines the
basic geometry or at least the diameters that we need for the full gear full gear
definition but next we want to get into drawing the tooth profile and like I
mentioned at the beginning we’re actually going to draw a true involute
tooth profile so it’s gonna have the proper curvature
instead of just shape like you see in some other videos to develop our
envelope gear tooth profile I’ve actually put together a spreadsheet that
will calculate the curve for us so let’s jump over to that now so the link to
this spreadsheet will be in the description below it’s free to use so
feel free to check it out and hope you hope you find it useful first we just
need to put in the input parameters that we have for our gear so it’ll be the
same ones that we put into fusion 360 earlier so we’ve got a modulus of two
number of teeth is 20 and the pressure angle is 20 degrees that’s really all
there is to it so the spreadsheet goes ahead and calculates the pitch circle
diameter the base diameter and the tip diameter and then it goes through a
series of equations here to calculate the gear tooth profile points at various
radii from from the origin so what it does is it starts here at half of the
base circle diameter so it’s half of thirty seven point five nine is eighteen
point seven nine and then I’ve designed it so that it produces 15 points at
equal increments up to half of the tip diameter and you can see in the formulas
there we’ve got pretty simple formulas for the first and the last and then the
interim points basically just divide the radius into equal steps the end result
is a series of x and y coordinates that define these points for the curve now
you’ll notice here that I’ve got results of millimeters and in centimeters one of
the quirks in fusion 360 is that we’ll see in a minute but when we import this
into fusion 360 it expects the numbers to be in centimeters not millimeters
which is a bit counterintuitive since the coordinate system we’ve defined as
millimeters but now that we’ve got our curve generated this is actually one
half of the shape of the gear tooth from the base circle up to the tip we’ll see
how to handle the the route portion of the of the tooth
once we get back into fusion 360 but all we have to do now because um using
fusion 360 I’m going to copy the centimeters and we’ll go into a new
sheet here paste those as values and then what we want to do is export this
as a CSV file so basically just a text file with the numbers separated by
commas so let’s go ahead now and import the gear tooth profile into our sketch
to do that though we need to first actually close out of the sketch we were
working on and what we’re going to do is use an add-in or a script to import the
CSV file so we’ll go up to tools add-ins scripts and then if we scroll down
there’s one here called imports blind CSV that one’s going to let us import
the points that we we have saved in our CSV file
so we’ll go ahead and run that we’ll click on the file and open it and as you
can see it actually imports the spline right into our into our model here if we
look closely at it it looks like it’s lining up properly so it actually starts
on the base circle and goes all the way through to the tip so what we want to do
now is define a mirror line that we can use to project the other side of this
tooth so we’ll go ahead and we’ll draw a construction line from the origin out to
the tip diameter of the gear and then what we’re going to do is we’re actually
going to define the angle of this line so if you think about it we’ve got a
gear that’s 360 degrees total and to break that into the portions of the gear
for each tooth we can divide by the number of teeth if you think about it
though that spacing actually includes the space between the teeth as well as
the tooth itself so to get just the toothed portion we divide by 2 and that
would be the entire width of the tooth we only want half of it to define our
mirror line so we want to divide by – again essentially what we’re doing is
just divided by four so that works out to an angle of four and a half degrees
there’s one more issue we need to deal with though if we live look at the pitch
circle diameter which is this third construction line here we can see that
the tooth is already up from the x-axis by that point because of the involute
curve the width of the tooth is defined on the pitch circle so we actually want
to define or determine what angle this is and add that to our mirror line so
that we can get the full width of the tooth so let’s draw another line from
the origin to the intersection of the gear profile on the pitch circle
diameter we can determine the dimension or the angle of that line 0.853 degrees so now if we go back up and change our
formula for this gear we want to add 0.853 degrees to that and that
should be the true center line of our gear tooth so what we want to do now is
just define half of the tooth tip and then also define the portion of the gear
that goes down to the root so let’s use our line tool turn off construction
lines because this is going to be actually part of the tooth profile and
we want a line for your tooth tip and then we want another line from the lower
end of the spline to the D denim so that’s half of our gear tooth fully
defined now what we can do now is actually mirror that across the the
center line that we just defined so we’ll choose our mirror tool
for the objects we want to choose all three components of our tooth and then
for the mirror line we’re going to choose the mirror line that we just
defined and there is our fully defined tooth now that we have the tooth fully
defined we just need to add in the the gear body what we can do there is we can
just select the dedendum gear diameter and project that into the current sketch
and that defines basically an enclosed object that we can use to extrude but
before we do that let’s just zoom out a bit and let’s add one more circle in the
center here for the shaft let’s say that we’ve got a 10 millimeter shaft that’s
really all we need to finish our gear so let’s close the sketch let’s go ahead
and press e to extrude we want the main gear body as well as the tooth and let’s
make our gear 5 millimeters in thickness and new body is fine okay so there’s our
gear with just one tooth let’s zoom in here and I want to add a fillip to the
edge there so we’ll click on fill it we’ll choose that edge as well as the
one on the other side here and let’s just use a half millimeter
radius fill it and let’s zoom out here again and now what we want to do is just
use a circular pattern to copy that gear tooth all the way around so we can go up
here to the create menu choose pattern circular pattern and the pattern type we
want is bodies we want to we want to duplicate the body here so let’s go
ahead and click on that and then for the axis we want to rotate around the z-axis
so we’ll choose that for quantity it’s actually just the number of teeth that
we want on our gear so we’ve already got that defined as a parameter called num
teeth we’ll choose that there hit OK and it actually produces our gear for us now
one one small thing we need to correct here is we actually generated 20 bodies
what we can do is we can actually combine those into one so we’ll up to
the modify menu and choose combine target body you can choose any one of
them and then the tool bodies is really just the rest of them so if we draw a
box around the rest it selects the rest of them we want a joint operation and we
don’t want a new component we just want it to combine it into a single body
within our current component so we’ll click OK and now we just have a single
body so that’s our gear fully defined with an involute tooth profile so one
check I like to do is actually to compare the gear that we’ve produced
from scratch to one of the ones that’s produced by the add-in so if we go up to
tools add-ins and then scripts there is actually a script built in to fusion 360
that produces spur gears automatically so let’s go ahead and run that and what
we’ll do is we’ll put in the same parameters that we used to produce the
gear that we we just did from scratch so the pressure angle was 20, module was 2,
number of teeth was 20, root fillet radius was half a millimeter,
gear thickness I think we used 5 and the hole diameter was 10 so let’s go
ahead and hit okay and what that does is produce another spur gear on top let’s
go ahead and activate that component and try to rotate it so that it perfectly
overlays the gear that we produced ourselves so let’s just play with the
rotation here whoops I’ve got faces selected so let’s try that again let’s hit okay there and just go back to
the base objects that we can see both and it actually looks like it’s
perfectly overlapping if we turn this one off and on looks like the rotation is just off ever
so slightly but it’s essentially the same gear so that’s it for today guys I
hope you liked this video and found it helpful if you did like it please go
ahead and hit the like button and subscribe to the channel thanks very
much bye bye

One thought on “Drawing an Involute Spur Gear from Scratch in Fusion 360

  1. This is my first video so please let me know if you found this helpful or if there was anything I can do better! What other types of topics would you like to see covered here?

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