Driver machining order

[thunderskunk]

Hello!

Real quick; For a driver wheel, do you drill the axle and crank holes on a mill, then mount the casting on an arbor to cut the flange or do you cut the flange and drill the axle hole on the lathe then drill the crank hole on a mill?

[Harold_V]

I'd like to express a few random thoughts. Feel free to disregard, secure in the knowledge that I am anal about precision.

Drilling holes isn't generally a precision operation. The spacing between the axle bore and the crank pin should be identical for all wheels, otherwise you can expect binding of the rods. Drilled holes are rarely on location, although they may be quite close. (Twist) drills have a way of drifting, both when being started, as well as when deeper in the hole.

In order for the holes to be properly spaced, it is highly recommended (at least by me) that they be rough drilled, then bored to proper location, using a mill equipped with a boring head. If you feel confident that you can hold acceptable tolerances by boring, you're best served to bore each of them to size, avoiding reaming. Reamed holes are notorious for being slightly tapered, not being round, and for having some bell-mouth, and can, and often do, vary, hole to hole. Boring would eliminate those issues, with proper location being an added bonus.

If you are not confident in your skills, and boring would present a problem, I would recommend that the holes be bored undersized by a few thousandths (no more than ten, no less than five), and then reamed to size. That would assure the holes are properly located, which may or may not be the case without the boring operation.

Reaming in a lathe tends to be troublesome unless there's dead alignment of the tailstock with the headstock, and that's rarely the case. A floating reamer holder helps.

It is important that the hole being bored be dead concentric with the spindle holding the reamer. A reamer will not relocate a hole, and will ream a less than straight hole when it is not properly aligned.

H

[FKreider]

Lester Friend of Yankee Shop fame would tell you to chuck up the wheel casting in the three jaw with the back facing out. Clean up the back of the casting and shoulder the flange area. Now it will sit nice and flat in the chuck when you flip it around and clean up the front, taking the casting to its proper final thickness. Before it it removed from the chuck again, center drill then drill and ream, now the outside wheel turning can be done on a stud arbor.

[Marty_Knox]

Before I do any machining on spoked wheels I paint them. You can get a good heavy coat on the spokes, then a nice thin coat on the machined surfaces after they are machined.

[ChipsAhoy]

I have a suggestion, and understand I am not a machinest, nor am I an accomplished steamer builder.
I would use this sequence if at all possible.
Knock off all the flash from the drivers so that they can be resonably placed on your mill table to accomodate.....
Bore the axle holes
Broach the axle holes
Put the drivers in a jig then bore the crank pin holes
Put the drivers on the axles (along with all the items required on the axles) with the intent never to be removed again
Turn the complete tread, flanges, front and back faces between centers.
Scotty

[DavidF]

I would machine the back of the wheel first so it could be mounted flush to a backing plate in the lathe, then machine the rim of the wheel, face it off, and bore for the axle in one set up. Then transfer to the mill and indicate off the axle hole, move to the position of the crank pin and drill and bore it.....Provided the casting and your tooling will allow you to do it this way...

[NP317]

I have always turned wheels on the lathe, boring the axle hole without removing the wheel from the lathe.
The crank pin holes get drilled/bored on the mill using a fixture for accurate alignment.
RN

[SteveM]

Take a look at the videos from our own trainman4602:

https://www.youtube.com/user/trainman46 ... el+turning

Steve

[rkcarguy]

I have always turned wheels on the lathe, boring the axle hole without removing the wheel from the lathe.
The crank pin holes get drilled/bored on the mill using a fixture for accurate alignment.
RN

This is how I'd do it. Make sure your mill head is trammed in so its nice and flat! Our mills at work are old and the tables tend to sag a little, so I always use my dials and check flatness across the entire work area. If you get your axle holes consistently sized, you should be able to make a fixture on the mill for the wheels to drop onto a tight slip fit locating pin, and then drill/bore each crank pin hole without moving the table. I would load each wheel, drill, change to boring bar, and bore, then repeat. Drill the hole close to finish size and do the boring in one pass. Because the boring bar could deflect differently, best to get it to size in a practice piece and then check it again once it's bored in a single pass. I've snuck up on the bore size only to have the bar deflect and the hole come out undersize when bored in one pass. That said, I'm not afraid of using a small brake cylinder hone or even a small flap wheel in a cordless drill (so you can control speed) to take a few .0001" out of a hole to get the press fit just right either.

[cbrew]

this is the order i machine driver castings.
1) using the 4 jaw, mount the castings face in,
A) surface the back.[/list]
B) drill and bore the axle hole.[/list]
C) cut the over all (.05 short of finished of over the flange).
D) add the rear flange taper.
2) mount on face plate with arbor (face out),
A) machine the face.
B) counter weights.
C: tread and rough in the flange.
3) using a fixture, drill and bore the crank pin hole on the mill.
4) using a fixture, key the key referencing off the axle and crank pin holes.
5) final thread and flange machining is done after the assembly is pressed together.

[thunderskunk]

Definitely several ways to skin this cat, which sounds good.

I do remember seeing talk about the bend in a Bridgeport table. I’ve only ran into one project that it caused an issue on, and it wasn’t too hard to work around anyways.

My boring head is an absolute piece of junk; if you want it to adjust nicely, it needs to be loose. Use it once and it’ll either cut differently on the second hole or many other possible issues. Tighten it whatsoever and it cocks the cutting edge in one direction or another, and becomes unadjustable. Even made by Bridgeport supposedly. I probably need to stone the wedge and the set screws at some point, but I’ve cleaned it before with no good results. I tend not to beat on anything with a hammer that’s not in an expandable collet, but maybe it needs some “influence.”

Could be operator error though, more than likely.

[rkcarguy]

I don't think it's "bend" in the mill table, but as you move away from center in the X-axis direction the heavy end sags. So I'll indicate the area I'm working in, and either tram it in or remove the vice from the center. Last time I got lucky and it was right on in an area about 12" wide, left of the vice mounted in the center of the table.
That is frustrating with the boring bars moving, I've struggled with that as well...keeping the wrench on the adjustment dial screw while tightening the setscrews so you can feel if it moves. For anything with any quantity, we always ordered a reamer and drilled or bored it close so it was only taking out around .008-010" and it seemed to work pretty good (in steel). Casting inclusions are hard on reamers though.