Involute Spline - CNC Mill w/ Rotary - Can it be done?

[pmurdock]

I have a situation where I would like to cut an involute spline on a shaft. I have solidworks and mastercam, but no GEAR HOBBING machine..

I am thinking that if I design the involute spline explicitly in Solidworks (perhaps using Camnetics GearTrax plug-in software) that I can take it into Mastercam and using a regular ball endmill create the involute gear by having mastercam surface cut the spline on my rotary chuck. This would avoid having to get any special tooling and I could create a variety of splines with varying parameters and only need one tool (ball endmill).. I would like to avoid having to buy any special gear cutters, etc.

Does this approach seem feasible? What would be the downsides to cutting the involute splines in this manner?

cheers,
Paul

[HuFlungDung]

It is possible, but the downside is that it would be relatively slow to do. The root of the spline typically has almost zero radius corners, so a very small ball mill would be required.

If you can acquire a taper endmill with a small enough tip diameter to fit in the tooth space, and a taper which matches the pressure angle of the spline specification, you could likely generate a close enough approximation of the involute in 3 to 6 passes down each side of each tooth. However, this may not be the most friendly style of tool to surface a cad surface model with. Nonetheless, through a combination of rotation of the work, coupled with a lateral offset of the taper tool, it would be possible to generate a curve and get down into the root of the tooth space to cut away those troublesome last bits.

[pmurdock]

So my sense of it is that it would probably be best to go with an involute spline cutter and then just cut each spline then rotate on the indexer and cut the next and so forth. Is this the prevalent method amongst shops who don't have gear hobbers?

the only drama is I have to buy a different cutter for each style spline I would want correct?

cheers,
Paul

[HuFlungDung]

Originally Posted by pmurdock So my sense of it is that it would probably be best to go with an involute spline cutter and then just cut each spline then rotate on the indexer and cut the next and so forth. Is this the prevalent method amongst shops who don't have gear hobbers? the only drama is I have to buy a different cutter for each style spline I would want correct? cheers, Paul

Yes, that is how we would do it.

I think that a custom cutter would be reasonably productive and is the way we used to cut splines in quantities of one, most of the time. We would grind a flycutter to match the sample spline. If possible, it can save wear on the custom tool to use a slitting saw first to open up the grooves. It is fairly important to get the rough groove to full depth first. This permits the custom tool to take a clean chip off each side of the tooth, without undue wear of the corners, and quite a bit less vibration and noise.

If you are going into mass production, then you'd probably want something more efficient than a flycutter.

[cam1]

I'd recommend getting a copy of the ANSI B92.1 Involute Spline handbook. It lists the method of generating (CAD) involute spline profiles, along with the methods of Gaging the finished product (measurement over pins etc.). In my opinion the final requirement of the product ie. farm tractor (flat root major diamtere fit) or HS machinery (fillet root side fit) will ultimately dictate the need for an off the shelf cutter, or a home made cutter. Also try this link for some basic dimensional info.:http://www.omnigear.us/involute_spli..._diameter1.htm


regards

[RICHARD ZASTROW]

FYI: You might be able to rent the form cutter(s) from either a gear shop (unlikely) or from a cutter supplier like Ash. I know Ash rented gear hobs and gear shaper cutters before I retired. Also, companies like used machinery dealers often buy lots of cutters etc. at auctions, might find what you want there.

Dick Z

[pmurdock]

Thanks for all the suggestions thus far..

I've been looking at Hu's comment about making a form tool to cut the splines.. Are these just made out of high speed steel and the other point is instead of manually grinding these tool blanks is it feasible to make the form tools on a Haas VF-2? I'm just getting started with a new business and none of the machines are here yet, so I'm just trying to see what the limits are of a CNC Lathe - with C-axis and a 4 axis VF-2. Can I make custom form tooling on the VF-2?

cheers,
Paul

[RICHARD ZASTROW]

Paul, I strongly suggest you take the advice cam1 offered. If you are to be in the highly specialized business of involute splines, gears etc. you must be knowledgeable in that area. If this is only an occasional requirement, do what many others do, subcontract that portion of the work. Commercially, this is demanding and critical. For a DIY hobbyist, you only have to satisfy yourself.

You will need precision tooling and measuring equipment, $$$$$$$$$$ to do this commercially.

I'm not trying to be a "wet blanket" just make you aware of preventable problems.

Good Luck

Dick Z

[HuFlungDung]

Originally Posted by pmurdock Thanks for all the suggestions thus far.. I've been looking at Hu's comment about making a form tool to cut the splines.. Are these just made out of high speed steel and the other point is instead of manually grinding these tool blanks is it feasible to make the form tools on a Haas VF-2? I'm just getting started with a new business and none of the machines are here yet, so I'm just trying to see what the limits are of a CNC Lathe - with C-axis and a 4 axis VF-2. Can I make custom form tooling on the VF-2? cheers, Paul

Maybe try to get ahold of a standard (cheapo) involute gear cutter so you can familiarize yourself with the geometry of such tools. Do this before you decide to commit to making your own tooling.

Making form-relieved cutters from HSS is a complex undertaking and I would say that a typical machining center is not the machine for the job of making those cutters. I suppose that you would need a lathe with what is called a form relieving attachment. As you may come to know, a form relieved cutter can be resharpened simply by grinding the radial face in front of each tooth of the cutter, thus preserving the cutter profile, albeit at a slightly smaller diameter after each sharpening.

Whether you grind the flycutter used to cut the spline directly, or grind a form tool to make a HSS cutter with, you've still got to cope with grinding profiles. A really determined machinist could grind a single profile with a wheel mounted in the spindle of a machining center, but you'd almost be breaking new ground to do it. It would be slow going to figure it all out. You might be better to farm the work out to a competent toolmaker, but being able to supply your exact tooth profile in a cad format would probably be a plus for you.

A carbide flycutter can be run at least 4 times as fast as one made of HSS, just the nature of the different tool materials.

Running a flycutter or a form cutter on the mill without an outboard support for the tool mandrel likely is a limiting factor on both cutting accuracy and feedrate for the tool. Compare that to a hobbing machine where the hob is well supported.

A circular form-relieved cutter from HSS would probably be 2.5 or 3 inch diameter, whereas a single point flycutter can be mounted in perhaps a 1" diameter bar and the tip running at 1.5" dia. So the small diameter tool can run at twice the rpm of the larger tool.

If you combine the small diameter of the flycutter, with the advantage of brazed on carbide, you can accomplish as much with a single tooth carbide flycutter as you can with a larger 8 tooth HSS cutter.

The advantage of a flycutter is that it is relatively easy to profile grind the clearance that the tool needs behind the cutting edge. You can use a comparator or something to compare your flycutter to the theoretical shape that you could likely generate in CAD.

For larger quantities of splines, I think you'd want to get a spline hobber, as this will free up your machining center to do other things that it does better, plus the spline hobber can use off the shelf cutters, one hob covering many tooth numbers in a particular pitch.

I know next to nothing about hobbing machines, but its almost a different class of machine to learn to set up and run, compared to a machining center. A hobbing machine has facilties to set the hob at an angle to the workpiece blank, to cancel the effect of the helix angle of the hob. Plus, the hobbing machine will provide gearing between the hob rotation and the workpiece to keep the timing correct. Apart from that, generating the proper shape to an involute tooth on a hobbing machine does not require any smarts, nor even any detailed cad file to work from, as the hob generates the tooth shape, beginning from a very well defined shape on the hob itself. The hob tooth looks something like an Acme thread profile.

[pmurdock]

Thanks Hu!

I've been looking at another option - an EDM machine.. If I were to look at adding one more tool to the arsenal I would like to add an EDM. I'm wondering how it would handle doing external and internal involute splines. It seems like it would eat those for lunch - especially for internal keyways and splines.

Can an EDM machine have sufficient accuracy and clean flinish to produce splines and keyways? I'm wondering if this might be a good way to go as well? Can an EDM electrode be say 12" long to cut some blind keyways?

cheers,
Paul

[HuFlungDung]

I imagine EDM might work fine although I have had no personal experience using one, to know if the time required makes it economic to produce the parts. Depends what your parts are

From what I imagine, the machining of the electrodes for EDM just shifts the profiling problem one step farther from the actual part.

Wire EDM would make it relatively easy to profile cut splines in open bores, and also to cut involute profiles in tools, should you want to go that route.

What kind of work will you be taking on? Is it general job shop machining, or would it be a relatively small variety of splines for a dedicated project?

[pmurdock]

Originally Posted by HuFlungDung I imagine EDM might work fine although I have had no personal experience using one, to know if the time required makes it economic to produce the parts. Depends what your parts are From what I imagine, the machining of the electrodes for EDM just shifts the profiling problem one step farther from the actual part. Wire EDM would make it relatively easy to profile cut splines in open bores, and also to cut involute profiles in tools, should you want to go that route. What kind of work will you be taking on? Is it general job shop machining, or would it be a relatively small variety of splines for a dedicated project?

Here is a picture of some of the parts we are looking at doing.. A lot of internal and external spline work. Probably 10-15 per month..

I'll probably just get an involute spline cutter to cut the external splines on my Haas VF-2 with rotary 4th axis, and then cut the internal splines with a broach - until I can justify some new machinery. I wonder how much a manual gear shaper or keyway cutter would be?

cheers,
Paul