How I design Bevel gears for 3DP

I posted some questions earlier - last year and all methods mentioned appeared to me to distort the tooth shape. As they might work - i.e. one gear turns the other - my goal was to come up with a better way to do that more accurately. I did it in inventor but the method should work in other cad systems too - I am sure it works in F360.

First a little sketch from KHK gears


A bevel gear is a gear where the axis intersect and therefore conical shaped and the cones touch on the pitch line and it can be viewed as an infinite number of gears in that cone perpendicular to the pitch line who -as its a cone are getting smaller and smaller and still are in the same relation to each other so IOW the modulus decreases but the gear shape stays the same. So you need the pitch angle delta and a starting profile for the gears

This is based on “export tooth shape” in inventor and the spur gear generator.
Next I crown the gear with a filet that calculates .4 + .1 * Modulus ( so for a 2mm modulus it woult be .4 + .2) the .4 is 1/2 the nozzle diameter as I print with a .8. Its a 3d printing thing to help avoid a corner bulge
Next I create a sketch like this

I copy the geometry of the crowned gear profile and put a straight line tangental to the circle on top and put to vertical lines down
When extruded (usually very small like .01mm or so so if I forget to delete it later the slicer ignorse it. It will be my ever smaller cutting tool

And then delete the initial Cylinder

Now I grab the top edge that was touching the initial cylinder and rotate that “tool” into a position so that it is 90 deg to the pitch angle. Now if I project it it will not be distorted and I preserve all things like tooth shift if I want to make a gleason style bevel etc
Next I sketch the body of the Bevel

I put all camfers and fillets in that will help with making it print well
Now I rotate it into a body

Now I create a point where the center axis meets all the different lines in the cone that was initially determined by the pitch cone But head and root also meet in that point - obviously

Now I loft it from the “tool” to the point

Now all that is left is a circular pattern to get this

Here is a test print of those bevels

Seems to run pretty smooth


Neat. I’ve seen a couple generators for these that leverage openscad. One in particular that I came across was written with the documentation in German so I had to find a speaker the last time I played with it. Would be cool to see those brought over into OnShape as featurescripts.


Sorry never worked with Onshape . Inventor and F360 is what our school does

It was more a statement to the wider community on the forum who might be using OnShape and have the desire to implement something.

That being said, I’m sorry your school is so restrictive about the software you are forced into using. I guess you can’t try out the openscad generators that exist. It’s a shame, they are pretty cool and output stl files for printing:


I don’t think he was saying he isn’t allowed to use other softwares, just that he wasn’t familiar enough with onshape to make a featurescript

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You can just @ me directly. Stay tuned


Some people don’t think it be like it is but it do.


I am an old retired dude and can use whatever I want. When I did designing I used to use a paper and ruler etc and made actual blue prints. Then Autocad came along and then I switched to computers and electronics. Now the school has a license for inventor - there is a class for that - so in robotics I get kids who know inventor there is now also and F360 class starting so I will get kids who know F360 for robotics. So I learned inventor and now F360. There is plenty to teach in robotics and no need to add another cad program. Now if you like openscad and it works for you and produces all you need for you well I think thats just great


Inventor has a pretty nice and powerful bevel gear design tool as well. Should save you some hassle for the next time.

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Its great to get the math done - only the bevels - just like the other gears are just an aproximation for show - not for actual use if you take a close look the gears even overlap in some places and in real life to solid objects cannot occupy the same place at the same time - says so too in the inventor documentation. So yeah we use the “generator” to help with the math. just like the spur gear generator is great for that too. Now the spur gear generator has a feature that will export the true involute tooth shape so you can then design a proper gear that is way to complex to animate in an assembly (hence the “for show” spur gears and bevels etc), Now you can print a gear like that and it will kinda mesh but don’t expect any math to work out like center distance or the axle distances or proper angle on a bevel etc. You just get something that looks like a bevel. Now if you don’t care for an involute profile and can work with adjustable center distances etc etc then that works - kinda - but in this case - and most we care that the parts (gears) are actually were we intended them to be

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I think the point was that you can use the specific openscad generator to automatically generate models, which you can then import into your assemblies in the program of your choice, instead of spending all that time designing manually


To add onto this, .Step files are universal to any professional cad suite. As far as I am aware .STL I’d too but I’m not entirely sure. So importing objects from one cad suite to another shouldn’t be an issue.

Please don’t try to use STL as an interchange format for CAD. It’s really not built for that and you lose a lot of data. (Such as representing circles…)


Adding on to this, from personal experience I know that modifying STLs is no fun if you need to do anything at all that isn’t like extruding a box in a very specific place.
That was a fun couple of days I wasted…
Also, Solidworks at least generally manages to screw up importing STLs in some way or another, which is no fun to fix.


For those wanting it the bevels are in the stp here

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