PDA

View Full Version : how to make a custom cutter for a spiral bevel gear



doctordoctor
09-21-2014, 04:54 PM
the goal: machine a spiral bevel gear to reasonably tight tolerances (i.e. not just a cosmetic gear, but a functional one) on a 3 axis CNC mill with a tilting rotary table

the plan:

using the excellent designer spreadsheet from these people: http://spiralbevel.com/spiral_bevel

I've been able to get a real design into SW and camworks seems happy with it too.

I've chosen to make the part setup in CAM at the same angle as the gear face so that the maximum amount of gear tooth area can be seen. I'm not sure if its 100% but it looks like it.

I could make a 3 axis toolpath right now that would machine the tooth profile 100%, but it would need to use 1/16" end mills to get all the way down in there, and would take forever.

I'd like to, instead, make a custom cutter to rough out the tooth profile fast, and then use tiny tools just for finishing.

So all I need to do is make something like a flat end, 25 degree taper end mill that has maybe 0.6" long flutes.

Id like to make my gears out of steel so this custom tool will need to be hardenable.

As far as tools to make this tool, I have a 3 axis CNC mill and a tiny hobby lathe.

I'm thinking I can buy the ceramic inserts for the hobby lathe, and a cylindrical blank of M42 HSS, turn the the blank down to 25 degrees taper, and then somehow gash out/cut out the flutes.

Is that how its done?

Or maybe I could just find an off-the-shelf end mill thats close..it doesnt have to fit the tooth taper perfectly, just enough to rough it out as fast as possible.

http://i242.photobucket.com/albums/ff197/acannell/GEAR_zps386ab526.jpg (http://s242.photobucket.com/user/acannell/media/GEAR_zps386ab526.jpg.html)

doctordoctor
09-21-2014, 05:01 PM
heres a picture from the perspective that the 3 axis mill will be setup to machine the tooth..

using the rotary tilting table I should be able to tilt the workpiece so its facing where the teeth will be just as shown

then rotate for each tooth

also shown are the toolpaths to machine the tooth using just a 1/8th and 1/16th ball mill..as you can see it gets 99% of the surface machined, but its going to take 5 to 10 minutes per tooth I'm guessing. I havent done an accurate time study because I would need to first get accurate cutting speed tests done on whatever material I'd use. I'm pretty sure it would be hours to do just one gear like this though.

http://i242.photobucket.com/albums/ff197/acannell/gear1_zpsc8e13426.jpg (http://s242.photobucket.com/user/acannell/media/gear1_zpsc8e13426.jpg.html)

http://i242.photobucket.com/albums/ff197/acannell/gear2_zps997dc202.jpg (http://s242.photobucket.com/user/acannell/media/gear2_zps997dc202.jpg.html)

TGTool
09-21-2014, 05:27 PM
You can purchase tapered end mills off the shelf for use in mold making. I haven't looked at them recently so I don't know if the angle you're looking for is standard or not.

If you're making it yourself from HSS you'll have to grind the whole thing - taper, flutes, cutting edges etc. Of course you can buy HSS annealed and machine it soft but you can't heat treat it at home so what you save by machining you spend on heat treat. You'll need a tool and cutter grinder and several hours of research and head scratching to get all the angles set up right so I'm telling you that's hard but not impossible.

The other choice is to go to a shop that does tool and cutter grinding and tell them what you need. They'll grind it for you out of the solid, HSS or carbide. It won't be cheap, but if you really need exactly that they can do it.

"Good luck Mr. Phelps." You'll need it.

doctordoctor
09-21-2014, 05:37 PM
You can purchase tapered end mills off the shelf for use in mold making. I haven't looked at them recently so I don't know if the angle you're looking for is standard or not.

If you're making it yourself from HSS you'll have to grind the whole thing - taper, flutes, cutting edges etc. Of course you can buy HSS annealed and machine it soft but you can't heat treat it at home so what you save by machining you spend on heat treat. You'll need a tool and cutter grinder and several hours of research and head scratching to get all the angles set up right so I'm telling you that's hard but not impossible.

The other choice is to go to a shop that does tool and cutter grinding and tell them what you need. They'll grind it for you out of the solid, HSS or carbide. It won't be cheap, but if you really need exactly that they can do it.

"Good luck Mr. Phelps." You'll need it.

Thanks for the advice!

I'm thinking now that its very likely I could find an off the shelf tool that would have 90% of the right geometry. I have tapered end mills but they are all for profiling on injection molds and have 1 to 3 degrees of taper at most. I need more like 25 for this I think.

I was hoping I could hack something out that would get the job done even if its not perfect, it would only be for roughing. I've seen videos online showing people making gear hobs for worm gears and hardening them with some refractory materials to make a basic furnace and what looks like a hand held weed burner (???)

But this project isnt about making the cutter, its about making the gear, so the less I have to do for the cutter the better.

Is there such thing as a 25 degree, 3/8" dovetail cutter? That would probably be perfect. Anything less than 45 degrees would probably work. I guess at this point I can look it up myself but I'd like to hear thoughts on what else might work, just for fun.

Or what about the possibility of making a custom end mill that takes inserts, which I can set at an arbitrary angle, just like those insert style counter bore/chamfering "drills".

olf20
09-21-2014, 06:10 PM
Go to http://www.gearotic.com/. Art has done a wonderful job with his program.
Lots of information and lots of gear cutters.
olf20 / Bob

doctordoctor
09-21-2014, 06:19 PM
Go to http://www.gearotic.com/. Art has done a wonderful job with his program.
Lots of information and lots of gear cutters.
olf20 / Bob

I already have the models of the gears, what are you mentioning about the cutters? Does he have cutters?

MrSleepy
09-21-2014, 06:19 PM
You should also take a look at George Britnells youtube page. His engine build logs are on here and HMEM.
https://www.youtube.com/user/gbritnell/videos

Rob

doctordoctor
09-21-2014, 06:22 PM
You should also take a look at George Britnells youtube page. His engine build logs are on here and HMEM.
https://www.youtube.com/user/gbritnell/videos

Rob

in his helical gear cutting he says "the cutter is home made, out of drill rod and tempered"..thats what I was thinking originally..cant I just make something like that?

basically just a keyway cutter/single flute threading tool, but with a 25 or so degree angle..id have to change the setup but thats fine..it would just be a different tilt

mc_n_g
09-21-2014, 06:27 PM
Several options are available but you will be limited to a single cutter instead of a 'hob'-style cutter because of the angle.
First I strongly recommend a copy of Ivan Law's Gear and Gear Cutting. Read it then read it again to get the parts you missed.

I made a 'hob'-style cutter from O1. Mine is not a true hob as it does not have an axial lead. This style is shown on Shorty's YouTube series (look them up)
Here are a few pics of what I did. Nothing new I have shown them before.
http://s10.photobucket.com/user/mc_n_g/media/machinery/Making_hob_zpsd2c3dcbf.jpg.html
http://s10.photobucket.com/user/mc_n_g/media/machinery/Cutting_flutes_zps22b0e78b.jpg.html
http://s10.photobucket.com/user/mc_n_g/media/machinery/Cutting_flutes2_zps43446c03.jpg.html
http://s10.photobucket.com/user/mc_n_g/media/machinery/Cutting_18DP_teeth_zps8d836b29.jpg.html

Some useful links would be
http://www.astronomiainumbria.org/advanced_internet_files/meccanica/easyweb.easynet.co.uk/_chrish/geardata.htm - All the formulas and example of a rack gear
http://www.deansphotographica.com/machining/projects/multipoint/multipoint.html -An excellent page by Dean Williams!!

You can make a cutter to remove the bulk and leave some for the final cnc passes.
I also do not get any scale of dimension for your gear.
Are you sure a 1/16" will give you the clearance at the bottom of the cut?

doctordoctor
09-21-2014, 06:37 PM
Several options are available but you will be limited to a single cutter instead of a 'hob'-style cutter because of the angle.
First I strongly recommend a copy of Ivan Law's Gear and Gear Cutting. Read it then read it again to get the parts you missed.

I made a 'hob'-style cutter from O1. Mine is not a true hob as it does not have an axial lead. This style is shown on Shorty's YouTube series (look them up)
Here are a few pics of what I did. Nothing new I have shown them before.
http://s10.photobucket.com/user/mc_n_g/media/machinery/Making_hob_zpsd2c3dcbf.jpg.html
http://s10.photobucket.com/user/mc_n_g/media/machinery/Cutting_flutes_zps22b0e78b.jpg.html
http://s10.photobucket.com/user/mc_n_g/media/machinery/Cutting_flutes2_zps43446c03.jpg.html
http://s10.photobucket.com/user/mc_n_g/media/machinery/Cutting_18DP_teeth_zps8d836b29.jpg.html

Some useful links would be
http://www.astronomiainumbria.org/advanced_internet_files/meccanica/easyweb.easynet.co.uk/_chrish/geardata.htm - All the formulas and example of a rack gear
http://www.deansphotographica.com/machining/projects/multipoint/multipoint.html -An excellent page by Dean Williams!!

You can make a cutter to remove the bulk and leave some for the final cnc passes.
I also do not get any scale of dimension for your gear.
Are you sure a 1/16" will give you the clearance at the bottom of the cut?

those pics are awesome!!!

yeah I 'll definitely need to be using something more single tooth for this, unless I abandon the CNC method and actually hob the gear

heres a picture of a projected outline of one end of the tooth..the other end is not the same, probably a bit smaller. the dimensions are in inches

camworks lets you simulate the machining operation and view the result, thats the multicolored picture above..the green means its within a thou and thats with a 1/16" cutter. the little yellow spot is a 1 thou overcut but thats close enough for me. I can always make the finishing pass more precise if needed, its the roughing pass that really eats up the hours if I'm going to be doing it with small tools.



http://i242.photobucket.com/albums/ff197/acannell/diensions_zps01759b78.jpg (http://s242.photobucket.com/user/acannell/media/diensions_zps01759b78.jpg.html)

becksmachine
09-21-2014, 08:51 PM
All this from a "lathe newbie"

Dave

gbritnell
09-21-2014, 09:19 PM
A spiral bevel gear or more commonly called a hypoid gear is mostly used for automobile differentials. That's not to say that there aren't different applications but this would probably be the most common use. When I drew up and built my 1/3 scale automotive differential I studied how hypoid gears were made. Youtube has some good videos on the subject. Hypoid gears are generated by rotating a multi-tooth cutting head into a gear blank that is mounted on an angle and is rotating on it's own axis. For my model I deemed it nearly impossible to do with standard tooling so I went another way. When CNC cutting anything requiring very small cutters and needing small stepovers the tradeoff is time. I would say if you wanted to rough the gear blank then you would have to use a flycutting type holder that would be able to cut the arc between the teeth. The gear blank would have to be mounted on an indexing head that was capable of tilting. You could then swing the cutter across the blank and remove a great deal of the stock. Once roughed you could then proceed with the CNC work to finish the teeth.
That takes care of the gear. Now what about the pinion?
The teeth on the pinion are quite radical given the diameter, pitch and helix. This would probably have to be completely CNC'd.
I'll really be interested to see how you progress.
Attached are a couple of videos of the gear set that I ended up making for my differential.
gbritnell
http://youtu.be/up1-lQm_32c?list=UUPvNzXJm9KOlaQwjAmYW9Xw
http://youtu.be/fW5wzl9lGaM
And the finished differential center section.
http://youtu.be/oOkmKkvC-PE

iMisspell
09-21-2014, 09:59 PM
And the finished differential center section.
http://youtu.be/oOkmKkvC-PE Im always in aww... when i see that.

TGTool
09-21-2014, 11:35 PM
For Pete's sake, use your resources. http://www.mcmaster.com/#end-mills/=ttspeb They've got 10, 15 20 25 and 30 degree end mills. There's two pages of forum here running around the countryside looking everywhere but in the right place.


Thanks for the advice!

I'm thinking now that its very likely I could find an off the shelf tool that would have 90% of the right geometry. I have tapered end mills but they are all for profiling on injection molds and have 1 to 3 degrees of taper at most. I need more like 25 for this I think.

I was hoping I could hack something out that would get the job done even if its not perfect, it would only be for roughing. I've seen videos online showing people making gear hobs for worm gears and hardening them with some refractory materials to make a basic furnace and what looks like a hand held weed burner (???)

But this project isnt about making the cutter, its about making the gear, so the less I have to do for the cutter the better.

Is there such thing as a 25 degree, 3/8" dovetail cutter? That would probably be perfect. Anything less than 45 degrees would probably work. I guess at this point I can look it up myself but I'd like to hear thoughts on what else might work, just for fun.

Or what about the possibility of making a custom end mill that takes inserts, which I can set at an arbitrary angle, just like those insert style counter bore/chamfering "drills".

doctordoctor
09-22-2014, 01:10 AM
For Pete's sake, use your resources. http://www.mcmaster.com/#end-mills/=ttspeb They've got 10, 15 20 25 and 30 degree end mills. There's two pages of forum here running around the countryside looking everywhere but in the right place.

"I guess at this point I can look it up myself but I'd like to hear thoughts on what else might work, just for fun." forums are for discussing. If I wanted to do all the research myself and not see other peoples neat gears and ideas I wouldnt have started a thread. I'm aware of mcmaster and that the endmills with angles exist.

BTW thats probably the easiest way for me to do this..a chamfer mill with a 0.6" stickout from a solid tool holder should be about as rigid and fast (and wet) as I could ever want to get. But I like hearing what people have to say about all this. And the idea of making a fly cutter with a custom tooth profile is intriguing.

doctordoctor
09-22-2014, 01:15 AM
A spiral bevel gear or more commonly called a hypoid gear is mostly used for automobile differentials. That's not to say that there aren't different applications but this would probably be the most common use. When I drew up and built my 1/3 scale automotive differential I studied how hypoid gears were made. Youtube has some good videos on the subject. Hypoid gears are generated by rotating a multi-tooth cutting head into a gear blank that is mounted on an angle and is rotating on it's own axis. For my model I deemed it nearly impossible to do with standard tooling so I went another way. When CNC cutting anything requiring very small cutters and needing small stepovers the tradeoff is time. I would say if you wanted to rough the gear blank then you would have to use a flycutting type holder that would be able to cut the arc between the teeth. The gear blank would have to be mounted on an indexing head that was capable of tilting. You could then swing the cutter across the blank and remove a great deal of the stock. Once roughed you could then proceed with the CNC work to finish the teeth.
That takes care of the gear. Now what about the pinion?
The teeth on the pinion are quite radical given the diameter, pitch and helix. This would probably have to be completely CNC'd.
I'll really be interested to see how you progress.
Attached are a couple of videos of the gear set that I ended up making for my differential.
gbritnell
http://youtu.be/up1-lQm_32c?list=UUPvNzXJm9KOlaQwjAmYW9Xw
http://youtu.be/fW5wzl9lGaM
And the finished differential center section.
http://youtu.be/oOkmKkvC-PE

I was thinking of a fly-cutter too, I will be getting my tilting rotary table this week so I think I should be able to get everything at the right angle for that.


My question is this: wouldnt a fly cutter be less rigid and therefore significantly slower than a stubby chamfer end mill?

Or do you mount the fly cutter on a very short, thick arbor, with as little stickout as possible?

I am enticed by the fly cutter because I figure I could actually machine its cutting edge geometry using the mill and then harden it, which would be interesting. CNC designed and machined arbitrary geometry cutting tools..hmmm

Your ford diff is SICK btw..

That inspires me to wonder if I could make a full size ring gear for my car? And if I could make that, then why not a full size limited slip? AND if I could make that? Why not a spinning ring that lets me visit an alien world where I can walk on the beach and meet my dad?

iMisspell
09-22-2014, 01:44 AM
Your ford diff is SICK btw..
You'll probably dig this then...
http://bbs.homeshopmachinist.net/threads/61294-Ford-300-I-six-engine-%28working-scale-model%29

{edit}
bla... ment to add this also (its in the thread i just linked)
http://www.youtube.com/watch?v=blaZ5tz0_6E&feature=youtu.be


_

gbritnell
09-22-2014, 08:02 AM
It's actually very hard to describe the compound action for generating hypoid gears. When I said flycutter I meant that as a substitute for the cutter that the Gleason machine uses to generate the tooth shape. On the Gleason cutter (more accurately a face mill) the cutting teeth cut both sides of the tooth, which have different profiles, as you can see from your CAD drawing. As the cutter engages the gear blank the gear spindle rotates at the same time the face mill is removing stock.
http://youtu.be/gj2szHk0OCU?list=PLBIbUDMKUJcoROf-5O5yDPbmQ6HTH50ka
http://youtu.be/aulqG3Ioxxo
To answer some of your hypothetical questions, why not? Given the right machinery and inventiveness a person can make practically anything. That's not to say that a home-made ring gear would be capable of going from New York to Los
Angeles but could work.
With the help of others, reading books, searching the internet etc I learn new things about machining every day. I figure just about the time my knowledge base peaks I'll be headed for the worm farm.
gbritnell

doctordoctor
09-22-2014, 06:14 PM
for the moment I'm experimenting with a different approach to see just how bad (or good?) it might go. Simply using small tools and optimizing the toolpath so they remove material as quickly as possible.

I dont have very much real world speed and feed data for small tools and steel, so I had to start somewhere.

First off is a 1/8" carbide 2 flute, 0.707" stickout, 7000 rpm, 0.010 radial DOC, 0.4" axial DOC. Flood coolant. 7 ipm.

In conventional it chattered a bit.

In climb it was absolutely silent!

So I think I can mark this up as usable for climb.

And that stickout of 0.707 is definitely more than required here. So even better performance could be had by reducing it I'm sure.

Now I need to test how it plunges.

The goal being to create a slice toolpath for roughing that crosses from crest to crest on the tooth, using this end mill.

The witness mark is where I stopped to take the picture. The finish is very nice.

http://i242.photobucket.com/albums/ff197/acannell/20140922_150339_zps27mgq6oj.jpg (http://s242.photobucket.com/user/acannell/media/20140922_150339_zps27mgq6oj.jpg.html)

http://i242.photobucket.com/albums/ff197/acannell/20140922_150430_zpsftavf0qh.jpg (http://s242.photobucket.com/user/acannell/media/20140922_150430_zpsftavf0qh.jpg.html)

doctordoctor
09-22-2014, 06:29 PM
Heres the toolpath with a 0.010" stepover running at 7ipm, just like the test. I'm not going to test the plunge rate, I think this end mill can plunge at 7ipm with a 10 thou radial engagement okay.

This is the roughing toolpath. Camworks says it will take about 5 minutes per tooth. For 17 teeth thats 85 minutes. I'm not happy with that so I'm pretty sure I'll be trying to out do this, but its a start.

http://i242.photobucket.com/albums/ff197/acannell/toolpath_zps0f371a9f.jpg (http://s242.photobucket.com/user/acannell/media/toolpath_zps0f371a9f.jpg.html)

http://i242.photobucket.com/albums/ff197/acannell/cut_zpsec14d83f.jpg (http://s242.photobucket.com/user/acannell/media/cut_zpsec14d83f.jpg.html)