Thoughts on reproducing a pre-1900 spindle

A reason t opt for the 4140ph is the taper socket. it may not really get much wear, but the 4140 in the prehardened form will take more than 1018, and takes a bit more abuse to get dings, etc. Probably worth the effort and $$ IMO.

It looks like I might have a piece of 4140PH by this weekend. If it machines easily enough that I can bore a 3/8" x 16" hole through the middle, ream a taper in the end, and cut threads for the take-up nuts, then I'll go that route.

This little mill won't be cutting chips for a little while yet. In addition to getting the mill complete, I still need to get my overhead stuff all hung and belted and get my power source established. Having a viable spindle gives the mill a real chance though IMO.

4140 ph cuts great. I easily get great finishes with good inserts. But personally I’d say if you want to do it right make it from 8620 and carbo nitride?? (May be wrong words) from what I understand that process minimizes distortion. Leave a few thousands for finish grind on the bearing surfaces and ID grind the bore. Hard turning is also an option.

If you need I don’t mind throwing the shaft on the cylindrical grinder for you but I cannot do the ID grinding.

Also Carburized 8620 is a good option aswell but you need more grind stock and could have more distortion

Ianagos said:

Leave a few thousands for finish grind on the bearing surfaces and ID grind the bore. Hard turning is also an option.

Click to expand...

I generally leave a good .005" on a side for parts of this size. Check and straighten to less than that after heat treat, and that'll leave you a little room to get the taper out of the grinder before you get to finish size.

On the bore, if he's gas carburizing, which is the most common ? Plug up the far end and good chance it won't get much of a case at all. Or maybe even none. You'd be working with about 40 Rc then. Long deep holes like that don't get much circulation, that's where salt bath does a much nicer job. But few places do that anymore because it's poisonous and dangerous.

He's not going to do this anyhow, but just for the record

EmanuelGoldstein said:

I generally leave a good .005" on a side for parts of this size. Check and straighten to less than that after heat treat, and that'll leave you a little room to get the taper out of the grinder before you get to finish size.

On the bore, if he's gas carburizing, which is the most common ? Plug up the far end and good chance it won't get much of a case at all. Or maybe even none. You'd be working with about 40 Rc then. Long deep holes like that don't get much circulation, that's where salt bath does a much nicer job. But few places do that anymore because it's poisonous and dangerous.

He's not going to do this anyhow, but just for the record

Click to expand...

If I was carburizing then I’d leave .01” per side on a shaft that long and skinny. I was talking about is nitriding or I think I’ve also heard it called carbo nitriding. From what I know it happens at lower temps and has less distortion

Ianagos said:

If I was carburizing then I’d leave .01” per side on a shaft that long and skinny. I was talking about is nitriding or I think I’ve also heard it called carbo nitriding. From what I know it happens at lower temps and has less distortion

Click to expand...

Both exist. Carbo-nitriding is sort of a combination, it has the same distortion liability as straight carburizing, I guess gives a slightly better case but ... Nitriding, on the other hand, is a much lower-temp process, gives a harder case but much thinner. It's also pickier about the alloy, results vary widely depending on material. But yeah, a lot less distortion - to the point of none. You wouldn't grind a nitrided part. It's not quench and temper so has to go on *over* an already-heat-treated part, otherwise the hard thin case will spall off if there's much load. Maybe would not be a problem here but we're doing theoretical now, OP has decided to go another way

It would probably work well here, some hi-po auto crankshafts used to be nitrided. And his internal taper would come out harder than cat shit and no need for post-machining. In fact, if he uses prehard 4140 he could nitride it at the end. No dimensional change and a skin of about 70 Rc. It's hard.

The trouble with leaving so much stock is, carburizing gets softer as it goes inwards, so you're grinding off the best part of your case if you leave too much grind stock. If you just case it deeper then you tend to make small features brittle - corners on splines and such - and you're still losing the hardest part off the surface. So, ime, it's best to use just a little more than the amount you need, then straighten the shaft after heat treat but before grind. It's not that hard to do.

Another option might be salt bath nitride or melenite. It has a slippery hard surface that would work quite well but very thin. Nice polished black appearance also with a good surface finish


When I find it I don’t need it
When I need it I can’t find it!

Turbowerks said:

Another option might be ... melonite.

Click to expand...

That's not a half-bad idea, actually. With the gun forum here someone should have a good source for getting it done reasonably.

Got to meet Miles and he picked up his 4145 "iron". What this is is CORE STOCK - a waste product of any oil country trepanner shop. I doubt that any of this stuff is ever trepanned in the annealed condition - simply because the chips (which MUST come out) would fight you from dawn to dusk.

So - that means it is very likely in the "pre hard" condition

Enjoy

Here are some 1930 Packard shackle bolts I made from core stock about 30 years ago

M.B. Naegle said:

View attachment 333781
View attachment 333782
Here are a couple pictures of the bearings. I whittled a little on a corner and think they're soft enough, so unhardened 1018 could be an option. As I noted before, my only concern with that would be how the tool taper holds up.

Click to expand...

looks like a 235 chevy head setting in the back ground

Big thanks to John for the 4145 today! When I start cutting on it, the first feature (after sawing it to length) will be drilling out the draw bar hole.

Another tick off the list was a bought a bundle of old Brown & Sharpe taper reamers including x3 #7's. Unfortinatly the seller didn't wrap them at all leaving lots of dings, but the price was fair and besides the dings, the 7's were the newest and sharpest. So another step on the list now will be sending them out to be reground (any recommendations?). Silver lining is that taper reamers don't get smaller when ground! After they're sharp, I'll be happy to loan them out. If they all sharpen as expected, there's a #5, #6, #7, #8, #10, and #11.

1yesca said:

looks like a 235 chevy head setting in the back ground

Click to expand...

That it is. Out of a 54' Chevy 4-dr. It's about to get some port polishing and a valve job.

Doing some research on the 4145H properties, and came across this video. OT for the thread, but I think this is the kind of work that produced the core pieces that John had. At first I thought it crazy that such a large chunk of steel would be considered fall-off, but it makes sense now. The 4145 core I have is a little rough on the OD, but measures about 3 1/4", so plenty of meat to true it up to 2 1/2". It's going to be fun to get this turning in the Hendey!


Fast-forward to 6:30 to see the core removed.

I like the "Dean,Smith,Grace" joke they have hanging from the head stock (1:30).

Amazing - all the trepanners I was around had induction heads to force feed the high pressure coolant - and the endless supply of chips exited thru the hollow trepan "bar" - but these would do 15 foot deep no problem and the majority were double end working from both ends of a 30 foot bar at the same time

Example

making a spindle tube...

I would likely run the bore, and then put the part/tube between centers and tickle any features of the Od.

or mandrel it between centers and tickle the OD

or make bore end plugs and tickle to Od between centers.

Bore end plugs made between centers or turned in one chucking and parted off.

one bore end plug having a knock-out hole,

I would tool-bit scalp the center of the end plugs to be sure they were dead-true to the OD.

if making a spindle shaft, I would finish it between centers.

My original plan was to make a B&S7 plug/test bar, cut all of the ID surfaces to size, then use the test bar to plug that side and hold between centers while cutting the OD surfaces, but I think it won't be necessary. I'll still bore and hold it between centers, but I'll do the tool taper last and indicate the spindle to be dead center between a 4-jaw and a steady rest before reaming.

At some point I'd still like to make a B&S7 test bar to help inspect the machine, but I can do that later. The ways of the machine have a lot of galling and pits, but not enough to take it out of service (since it's "just a mill," not a precision grinder, etc.). For now everything will be cleaned and stoned, and scrapping the ways will be a project for later. My 3 year old needs to learn to scrape someday.

The tube bore need be straight and to size..with enough finish stock on the OD to return the bore to center.

If a bearing tube the bearing diameters should be made true to the finished tube ID.

Just my opinion. I think it is near impossible to bore a part to the dead center, and straight of the OD

but is possible to OD a part to the center of a bore.

Re: might 4 jaw the close end and steady the far end and be lucky to get .002 or .0005...that is a lot of error.

I have seen guys chuck one end to 2 or 3 tenths and then turn a part around and run the other end ..for a very crappy shaft.

Much better when an average lathe was .003 or so off and one had to use proper techniques.

Remember you want to step bore or rough bore the taper in the setup before applying the reamer. Getting the shaft to run true in the chuck *and* true in the steady is a bit tricky. If the fingers on the steady are close but not quite right, the shaft can nutate out of the chuck while you are working on it.

When cutting the 16" bore, the plan is to drill from both ends with a 1/4" jobber drill followed by an extra long 1/4" drill, 8" deep from both ends to create a rough pilot. The tool taper side I'll open up to the taper's minor diameter so there's more room for chip evacuation and less distance for the long drill to pass through, then I'll follow with a 3/8"+ extra long drill from both sides. If the two ends line up within .05" and I can get a 3/8" bolt through, it'll work. The Hendey has a high pressure cutting oil pump working, so I should be able to keep the hole flushed. A coolant induction drill would be very helpful and I might look at getting one as there are other jobs it would be helpful for. With the taper minor diameter cut, I'm really only looking at a 5-6" deep hole in each end, so I don't think it's going to be that tricky.

While everything's set up to bore the ID, I'll face the ends to the finished length and put a nice chamfer on each end for the centers to register. Once it's turning between centers, I'll cut all of the OD and leave a little for a later finish pass.

After that in no particular order: cut the take-up nut threads, cut the cone pulley key and set screw flat, rough cut the taper, and mill the tang slot through one side. I'll make a press fit plug to cover the tang slot, and with that in place take the finish pass on the OD surfaces. After that, I can test assemble in the machine's bearings and see how concentric the rough bore is before I chuck it back in the lathe with a steady and ream the tool taper.

Could you bore and ream the taper in-situ once the machine is set up to run?