This is step by step guide how to create gear using CATIA.
I'm not CATIA expert. Someone might find that CATIA doesn't
have much with TCP/IP and FreeBSD. However I'm B.Sc.M.E. and I
find playing with CATIA very interesting. I coulnd't find
much about gear design using GOOGLE or YAHOO. Since I enjoy
learing and practicing what I learn, I also enjoy sharing that
with others (often seen on overnet/edonkey: please share :)
don't be selfish. Here is step by step guide how to make spur gear
using CATIA. Note that this was inspired by document I have
found at website www.piovision.com (credits go to the unknown
designer).Also note that spur gear design we use today was first
sugested by Swiss mathematician Leonhard Euler (15.4.1707-18.9.1783)
(Euler was also credited for this on old 10 Franc Swiss banknote,
checkout Euler on wikipedia).
Robert Willis of Cambridge Universty was the first who demonstrated
advantage of involute shaped teeth over popular epicycliod shaped
teeth. Epicycloidal shaped teeth design belongs to Danish scientis
Ole Romar, but it is also worth noticing that Nicholas of Cusa
(1401-1464) and Albreth Durer (1471-1525) studied epicycloid, so it
is not clear who was the first who invented gear.
But let's start. This document assumes that you have basic
CATIA experience and that you are not a complite moron.
Also, this document assumes that you know basic spur gear
geometry. Here is excellent document from www.bostongear.com
in case you are not familiar. Some basic notations:
rb - base cylinder radius
r - pitch circle radius
rk - outside circle radius
rf - root radius
a - presure angle (20deg)
m - moduo (in our example 20) m=p/3.14159 where p is circular pitch 2r=m*z
z - number of teeth (in our example 20)
When you start CATIA, go to TOOLS->OPTIONS->infrastructure->
part infrastructure and in Display select Paramteres and Relations.
Then in Options->General in Parameters and Measures select with value
and With formula in Parameters Tree View.
Now it is time to go to Generative shape design:
You will see something like:
Bring Knowledge toolbar out:
Then by clicking on arrow pointed down near table icon:
Fog and f(x) are two most important things you will use for gear design:
Now it is time to enter some basic parameters that define gear
This is done by clicking at f(x) icon:
And then when you see dialog box: Formulas: Part1
fist select Parameter type (real, lenght or angle) click new
parameter of type and then edit value. You can do this until
all parameters are enered.
When you enter parameters it is time to enter some formulas.
For, r, rb, rk and rf we enter formulas by naming them and by
clicking Add Formula. Formula editor will appear:
After typing all formulas and expanding specification tree you
will see something like this:
It is time to add laws that will define our involute. Click
on fog icon, name law x add parameters, t and x select their
types and add law:
Same should be done for y. This law will help us to create
points that define spline for our involute. Involute is line
that is trajectory of point belonging to line that is always
tangent to base gear cylinder. It is used for tooth profile.
If gears had profiles formed by straight lines they wouldn't
work.
After expanding specification tree you should be able to
see something like this:
Now it is time to start creating our points for involute spline.
Click on point icon, select xy plane for support and when asked
to enter H and V cordinates right button click should bring menu
where you should chose edit formula:
You will be prompet by edit formula dialog. Type in:
Relations\x .Evaluate(0)
You should do same for V except you should use Relations\y .Evaluate(0).
You will get starting point for involute:
After repeating this step for .Evaluate(0.1)-.Evaluate(0.5) you will
get this:
Click on spline icon and chose all 6 points:
Your involute is created!
This is how it looks in sketcher:
From this point everything is more or less simple.
Create base cirle by clicking on cirle icon.
Right click on radius and chose rb from formula editor:
Now it is time to extrapolate our involute. For lenght
also right click and chose formula (rb-rf)*1.5
You can use View-> zoom and pan to see what actually you are
doing. Create plane. Use formula: inv(360/z)/4. You will get
-4.5deg angle offset from ZY plane.
After this create rf circle and from inser menu use corner to
create corner. Corner dialog will apear:
This is what you should get:
Now use trim and result should be:
It is time for simetry. Tooth starts to get shape:
Create rk circle and use trims to get tooth shape:
Circular pattern:
First select tooth (trim.3) and then for reference
element select Z axis.
Gear is almost done now it is time for joining all teeth:
Turn off check manifold and check consistancy:
Apply one more trim and here is our gear in normal plane:
So in case that you want all process as .CATPart here it is:
SpurGEAR
If you find this useful buy me a beer ;)