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

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?