Gear hobbing on a CNC actually the right way to go

[Mr.Chipeater]

I need to make 5000 spline components out of 45HRC 8720 with the following spline



Now I've read ad nauseam on this forum about how worthless everyone views gear hobbing on a CNC turning center is. However, wouldn't this be a perfect application for it? We've got an NLX1500 and Mori claims that gear hobbing has "achievable quality <DIN 7"

I don't see any reason why that wouldn't be sufficient tolerance for this application unless there's something I'm missing and given how small the spline is, I don't see rigidity being an issue.

If not, why and how else would you do it for the quantity?

From what I've read on the forum, everyone loves dedicated hobbing machines but where does one actually buy one of those machines? I can't seem to ever find any used ones for sale and we've had an absolute nightmare experience dealing with gear "specalist" outfits in the past producing absolute junk despite them having dedicated hobbing equipment. We ended up having to get custom form tools to mill splines ourselves which turned out great. We'd just do that again but I thought the high quanity could justify the investment for a faster cycle time and possibly be helpful on future jobs.

 

[Ox]

I have not the experience thus far, but these guys would likely be my first call.

I think that this is the right link as I can just barely see what appears to be a broaching insert behind the COOKIES banner blocking my view.

OD Broaching | Schwanog LLC

Complete production on the machine. No further work on any additional machine is necessary. Production up to the federal government possible. Can be used for almost all materials.

www.schwanog.com

-----------------

Think Snow Eh!
Ox

 

[SeikiCorp]

We milled them on a robodrill with a indexer and on our mill-turn lathes.
Ours were smaller than a 5/8 shaft dia.

 

[implmex]

Hi Mr Chipeater:
That's kind of a funny drawing you've got there...it's unclear whether the portion of the spline to the left or the groove (the flange end) is supposed to represent the permissible lead out scallop from a hob...kinda looks that way but it's not drawn that way.
Another way to cut splines on a stubby shaft is with a gear shaper like a Fellows, but that needs an undercut right at the termination of the spline which this drawing doesn't show either.

Which way you are forced to do it depends on the design.

I have no experience with hobbing, but those who do, and whose opinions I respect are unenthusiastic about hobbing attachments on CNC lathes as you've said, but the negative commentary was usually in relation to gears.

Whether they'd have the same negative reaction to a 10 mm spline I do not know, but since (as you point out) many of the problems relate to the rigidity of the setup, you may have no issues whatsoever on such a tiny part.
On the other hand, the material is moderately hard at 45 RC.
Fortunately the tolerances seem pretty open except on the major diameter.
Can you get the tool life you need from a carbide hob on a less than ideally rigid setup...anyone's guess.

Emanuel Goldstein once remarked on grinding small gears from the solid...I don't remember which thread it was in , but apparently there were gear grinders made specifically for that task.
Maybe he will chime in again.
Zahnrad Kopf and Dan from Oakland are the other current contributors to the forum with gear and spline expertise...maybe one of them will also speak to this.

The hobbing gadget may well end up to be the proper way forward...but I certainly wouldn't lay down a nickel until I knew the rig could have a decent chance at doing the job.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

 

[Ox]

We ended up having to get custom form tools to mill splines ourselves which turned out great. We'd just do that again but I thought the high quantity could justify the investment for a faster cycle time and possibly be helpful on future jobs.

Why not just go this route in the lathe?
Not enough Y travel?

I would think that the broaching tool link above would be quicker / cheaper tho.
Unless the 45Rc would be an issue?

I don't see the actual hobbing process being quicker?
But the $10K and 25# attachment would seem a hurdle?
Not sure what would be gained on this app?


------------

Think Snow Eh!
Ox

 

[Mr.Chipeater]

Why not just go this route in the lathe?
Not enough Y travel?

I would think that the broaching tool link above would be quicker / cheaper tho.
Unless the 45Rc would be an issue?

I don't see the actual hobbing process being quicker?
But the $10K and 25# attachment would seem a hurdle?
Not sure what would be gained on this app?


------------

Think Snow Eh!
Ox

Y travel isn't an issue. I forgot to mention I spoke with a broach tool supplier about this part and they said 45Rc was a no go. They also said expected tool life if broached prior to heat treat would be ~50 pieces, so we'd be looking at $10,000 in just broach tooling costs for 5,000 parts which just seems bananas.

Speed advantage is being able to effectively cut all the teeth in one pass with the hobbing process vs having to index 18 times milling one tooth at a time. Say it only saves 30s cycle time (highly likely it'd be even more) spread over 5000+ parts that still saves over 40hrs of machine time which just about pays for the fancy WTO live holder. Once you factor in the cost of custom tooling you'd have to buy for milling anyways then the cost between the 2 processes pretty much becomes a wash.

I guess since I've read so many negative things about gear hobbing on a CNC lathe on this forum that I was looking to see if I'm missing something here or why it wouldn't be a good fit for this job.

 

[Ox]

I would think that the gear ratio of the head, and the OD of the hob it'self would go a long way to making the "Electronic Gearing" work well. (Keeping live tool motor wound up a bit) I would think that the 10mm OD would have much less surface area in the cut - as compared to a larger gear, helping to make it a better result. (Timing issues from hit/miss effect)

Be interesting to hear what others say.


When you say that you talked to someone about broaching it, was you ref something like I posted, or a rotary product?
(Florida or Somma)


------------------

Think Snow Eh!
Ox

 

[Mr.Chipeater]

When you say that you talked to someone about broaching it, was you ref something like I posted, or a rotary product?
(Florida or Somma)


------------------

Think Snow Eh!
Ox

It was for a wobble broach

 

[EmGo]

Nah, it'd work. Kind of, I'm wondering about the 8720 at 45 Rc ? You sure can't get 86 to that hardness unless you carburize it and then the case is only going to be x deep, core will be much less but how do you plan to cut 45 Rc ? And carburize entire bars ? Turn it at 45 ? Carbide hob ? That part is very strange.

Anyway, just did a couple thousand splines very similar in size, they took a tiny bit less than a minute apiece total. That's total, from opening the box to putting the clean finished parts back in the box. That's not the quickest you could go, just the quickest I could stand at my advanced age - switch one, locate (these had to be timed), tailstock in and clamped, push go, advance cutter, wash the last one, dab grease on the center of next one, repeat repeat. Every tenth one go get a cookie. It's an easy mindless job but have to concentrate. You don't need advanced knowledge to cut these teeth is what I'm saying.

A hob attachment for your lathe thingy should work fine (except for that hardness spec which doesn't make sense ?), in this case it's a matter of cost. Used Barber-Colman 6-10 is probably easiest to find altho there's other smaller hobbers that would be faster. The hobber is easy to run and probably cheaper so it's a choice of where you want to spend the money I guess. btw, looks like a major diameter fit ? The size tolerances on tooth thickness are wide open but o.d. is a couple of tenths, you are going to grind after ? Oh wait, it looks like they have the same diameter dimensioned with two different numbers ? 'scuse me ? Or is that just the reduced size of the print ?

Anyway, if you want it'd work. Just a matter of time and cost as to which is more effective. There's one just like this for sale, price is probably less than the lathe attachment but I dunno which would be more useful to you in the future. Part is just about like what you want to do.

https://files.catbox.moe/6s9tcx.mp4

 

[Garwood]

You'll probably never use the hobbing attachment again. Good luck selling it for much used. But, it doesn't take up much space.

If you buy a hobber you'll probably find other jobs to run on it- They are infinitely more versatile. If you buy a used B-C 6-10 for $XXXX you can sell it for about the same $XXXX. If you have a spare 50 square feet for a small hobber do it. If space is too tight don't do it.

 

[Dan from Oakland]

What EG said about the 8720- it will not direct quench to 45Rc. 8620 will only direct quench to around 32Rc and its got the same amount of carbon. Pretty sure you will have to carburize and draw them back to 45Rc. Might want to discuss that with your customer as there is no mention of case depth on your print. You will need a carbide hob to get any decent life cutting 45Rc material.

 

[DouglasJRizzo]

We did this in the showroom a few times when I worked for Doosan. It was "ok" but just barely and the holders and such were *VERY* expensive.
If you really wanted to, I guess you could, but I would not. Plus, this type of work is tough on live tool drives.
Having grown up in a gear house, I know how valuable a good hobber or shaper is.
Google search "used gear machinery" and there are plenty.
- D

 

[Mr.Chipeater]

We did this in the showroom a few times when I worked for Doosan. It was "ok" but just barely and the holders and such were *VERY* expensive.
If you really wanted to, I guess you could, but I would not. Plus, this type of work is tough on live tool drives.
Having grown up in a gear house, I know how valuable a good hobber or shaper is.
Google search "used gear machinery" and there are plenty.
- D

I watched it a few times when I worked for Mori so I understand what's involved though I never did any of the test cuts so knowledge on the quality side is a little lacking for me.

On the flip side, I admittedly have 0 experience evaluating used gear machinery to know if its in good shape or not. Man-hours is also our biggest bottle neck in production which makes me hesitant to spring for an all manual machine from the 90's. It's without a doubt the best way to go for low volume work but I don't know if the same can be said when talking about 5000+ parts annually.

Has anyone tried hooking up a co-robot to one of these old hobbers?

What EG said about the 8720- it will not direct quench to 45Rc. 8620 will only direct quench to around 32Rc and its got the same amount of carbon. Pretty sure you will have to carburize and draw them back to 45Rc. Might want to discuss that with your customer as there is no mention of case depth on your print. You will need a carbide hob to get any decent life cutting 45Rc material.

My apologies, its 8740, not 8720. I would spline prior to HT but they also want a 16Ra on the teeth and my experience with HT's is that will never hold post HT.

 

[implmex]

Hi again All:
Just a quick comment on the diameters; the tight tolerance appears to refer to the shaft between the flange and the spline.
The spline is reduced diameter and doesn't even need to be very concentric to the shaft.
There's a note that states the tips of the teeth are not required to "clean up"
I suspect that it's just a means to keep some kind of coupling from slipping and doesn't need to carry a sliding element.

The comments about case hardening and case depth are noteworthy.
I wonder if the designer intended the parts to be turned and hobbed, then case hardened and last cylindrical ground on the shaft.
If the part were hobbed after case hardening, the teeth are 0.0208" deep so the case would have to be minimum 0.040" to have enough at the roots to keep the case from just spalling off under load.
That's my guess.

Cheers

Marcus
www.implant-mechanix.com
www.vancouverwireedm.com

Whoops; ignore everything I said about case hardening...the OP was typing while I was.

 

[EmGo]

On the flip side, I admittedly have 0 experience evaluating used gear machinery to know if its in good shape or not. Man-hours is also our biggest bottle neck in production which makes me hesitant to spring for an all manual machine ......

Has anyone tried hooking up a co-robot to one of these old hobbers?

They had autoloading even in the fifties. Harder to find one with that tho, mostly when they get retired smaller shops pull that stuff off.

Automated part measuring too. Y'all cnc guys ain't as fancy-pants advanced as you think you are

You could probably load one with a robot pretty easy. Liebherrs commonly come with autoload these days but you don't want to know the price.

My apologies, its 8740, not 8720. I would spline prior to HT but they also want a 16Ra on the teeth and my experience with HT's is that will never hold post HT.

That's not going to be fun. 8xxx likes to grow on the o.d. and shrink on the i.d. when you carburize it. Except for the one or two times it decides to mess with you and either doesn't do anything or goes the wrong way.

I had a little David Brown grinder that would have done these from solid but then you'd have the case problem. I'm assuming that with this small a part they want like .015" case ? And why 45 Rc then ? You're going to get 60-ish with case, no point to making it softer really ...

I'm gonna go out on a limb and say cutting teeth is the least of your problems here. The heat treating is not going to be any fun at all.

 

[Ox]

I watched it a few times when I worked for Mori so I understand what's involved though I never did any of the test cuts so knowledge on the quality side is a little lacking for me.

On the flip side, I admittedly have 0 experience evaluating used gear machinery to know if its in good shape or not. Man-hours is also our biggest bottle neck in production which makes me hesitant to spring for an all manual machine from the 90's. It's without a doubt the best way to go for low volume work but I don't know if the same can be said when talking about 5000+ parts annually.

Has anyone tried hooking up a co-robot to one of these old hobbers?


My apologies, its 8740, not 8720. I would spline prior to HT but they also want a 16Ra on the teeth and my experience with HT's is that will never hold post HT.

A 16 on milled teeth?

The comment earlier about ground threads may be where you need to be looking?


------------------

Think Snow Eh!
Ox

 

[Mr.Chipeater]

They had autoloading even in the fifties. Harder to find one with that tho, mostly when they get retired smaller shops pull that stuff off.

Automated part measuring too. Y'all cnc guys ain't as fancy-pants advanced as you think you are

You could probably load one with a robot pretty easy. Liebherrs commonly come with autoload these days but you don't want to know the price.



That's not going to be fun. 8xxx likes to grow on the o.d. and shrink on the i.d. when you carburize it. Except for the one or two times it decides to mess with you and either doesn't do anything or goes the wrong way.

I had a little David Brown grinder that would have done these from solid but then you'd have the case problem. I'm assuming that with this small a part they want like .015" case ? And why 45 Rc then ? You're going to get 60-ish with case, no point to making it softer really ...

I'm gonna go out on a limb and say cutting teeth is the least of your problems here. The heat treating is not going to be any fun at all.

No carburizing or case hardening.

Its a through hardening HT process. Oil quench and temper.

 

[EmGo]

No carburizing or case hardening.

Its a through hardening HT process. Oil quench and temper.

Okay, I'm still back at the xx20 .... could do any number of things then, much less scary than when we were talking post-machine heat treat.

A little misinfo leads us far down the wrong path

Are you going to turn them hard ? Carbide hob should be able to do the teeth, or even grind from solid. A Reishauer would eat those up, even an old old one, but maybe you don't want to go there for 5,000 parts ...

 

[Mr.Chipeater]

Okay, I'm still back at the xx20 .... could do any number of things then, much less scary than when we were talking post-machine heat treat.

A little misinfo leads us far down the wrong path

Are you going to turn them hard ? Carbide hob should be able to do the teeth, or even grind from solid. A Reishauer would eat those up, even an old old one, but maybe you don't want to go there for 5,000 parts ...

I suppose I should have been quicker to respond to whoever threw out carburizing first (to be fair I'm surprised its a though harden process too but the customer has assured me several times that it is)

We regularly machine post HT in 15-5 and 4140 so anything <50Rc doesn't phase me. Hob life is really the only unknown to me. I'd assume you could at least get several thousand parts per hob. The teeth are *only* .025 deep or so.

 

[DouglasJRizzo]

I watched it a few times when I worked for Mori so I understand what's involved though I never did any of the test cuts so knowledge on the quality side is a little lacking for me.

On the flip side, I admittedly have 0 experience evaluating used gear machinery to know if its in good shape or not. Man-hours is also our biggest bottle neck in production which makes me hesitant to spring for an all manual machine from the 90's. It's without a doubt the best way to go for low volume work but I don't know if the same can be said when talking about 5000+ parts annually.

Has anyone tried hooking up a co-robot to one of these old hobbers?


My apologies, its 8740, not 8720. I would spline prior to HT but they also want a 16Ra on the teeth and my experience with HT's is that will never hold post HT.

Those old hobbers are very long lived and easily rebuilt. Dad had '40s and '50s vintage machines still producing good parts.