When to ream!

[RSG]

I posed a question earlier regarding roughing and now have one more sort of related to it.

It was agreed that roughing with a final pass is a good idea in order to hold accurate dimensions but I just wondering where reaming fits in to this equation. In the drawing below it shows the internal lathe operations required for some upcoming parts and the bore in the middle must be reamed to an accurate dimension.

Should I be machining the entire face including boring the journal to a close dimension, then ream as the final operation? Currently I do the journal first, drill, bore and ream, then move on to the rest of the facing operations. My concern with reaming as the last operation is chatter since the material in the center has been thinned down seriously.

I'd appreciate any input.

[ChipMaker4130]

I would face before reaming. You don't show dimensions, but reaming would typically only take off the last 5-20 thousandths or thereabouts, depending on bore size. There shouldn't be any chatter problems with the reaming operation. (The main reason to face before reaming is to provide smooth entry for the reamer. I assume you'll be using a chucking reamer and not a hand reamer.)

[RSG]

Hi Chipmaker,

Sorry, I might not have been clear in my post. I am referring to doing all the machining of the profile including drilling and boring the hole slightly undersized. Then, the final operation would be to ream the hole. Yes it will be a chucking reamer and the parts size is 5" dia with a .625" journal.

The chatter I'm concerned about would be a result of taking all the material from around the journal away (as illustrated in the drawing).

[pete]

There's a hell of a lot I don't understand about chatter if you delve into the physics and mathematical concepts that model what happens. All of it's way above my understanding.Fortunately we don't really care about all that other than not causing situations where it happens. In a nut shell it's a natural frequency (harmonics) for the material, cutting tool type, tool sharpness, cutting tool angles, depth of cut, rpm, rigidity for both the part and tool, condition of the tool slides, or even sometimes lubrication types or amounts, plus probably a few other items I haven't thought of that all combine. The materials natural frequency can sometimes even change along the same length of bar stock the part was cut from. When or if that combination happens to get into that natural frequency range chatter starts. Not 100% effective every single time, but loading the cutting tool differently or dampening it somehow when you have that chatter start will change that natural frequency. The general rule of thumb is to drop the rpm and / or up the feed rate. Very rare when upping the rpm or a lighter cut doesn't make things worse in my limited experience. There's multiple other items to try depending on the cutting tools used, part shape and it's cross section etc. A lump of plumbers putty, plasticine, applied to or tightly wrapped solder wire around the end of a boring bar or reamer shank, wrapping a thin walled part with rubber bands, bungie cord or whatever else you can think of all help to dampen that vibration and change the harmonics. Even a hose clamp can help on small diameter parts. Real machinist's would be a whole lot better at picking a method that's proven to work in the past without a lot of trial and error. That's why they get paid and I don't.

But best guess, since reaming is only a light cutting operation and there's a fair amount of material backing up the sides and length of that hole it might go just fine. It could also have a lot to do with what your holding the reamer with. But I think you mentioned you were looking for a floating reamer holder? My best guesses still don't make parts so let us know how it goes.

[RSG]

Thanks Pete,

That's pretty much why I did the journal boring/reaming at the beginning, because there's so much mass in the part it doesn't chatter, but I'm now concerned with making sure the finished hole is the most concentric it can be so by doing the reaming last might be better, or would it make no real difference.

[whateg0]

If the part isn't removed from the chuck, and the hole is bored before reaming, how would the concentricity be affected?

Dave

[RSG]

Whatego, from what they tell me just the act of machining the part and removing material causes distortion from the stress relief, how much I don't know because currently I do it all in the front end and don't seem to have an issue, however, I'm open to learning how to do things right so if it's better to ream last then I'm in.

[Harold_V]

The policy for machining is that all features should be rough machined before any finish cuts are taken. That assures that any changes in the material, due to the relieving of stresses, will be corrected by the finish cuts. That should apply across the board, with few, if any, exceptions.

Chatter with a reamer is generally the result of somewhat excessive speed, but, more importantly, how quickly the reamer is introduced to the part. The faster, the better. You can rise above chatter by simply feeding it very quickly, keeping in mind that reamers are multi-toothed cutters and will handle rapid feeding.

As much as I am not a reamer fan, when I built the light switches for my home, I chose to use a 3/8" diameter push button for on/0ff. As there were many plates, most of which had multiple switches, I reamed the holes for the buttons. I did this on my Haas CNC mill, reaming at what I recall to be 1,200 rpm, with a feed rate of 20"/min. The reamer entered the hole silently and reamed what I'd call a round hole, perfectly free of feed marks, with an excellent finish (the buttons were made of Delrin, so it was important that the hole not be rough). The holes were consistent for size and finish from beginning to end.

I had to experiment with feed rate, as the test pieces started out with chatter at the entrance. When I upped the feed rate adequately, there was no chatter.

When reaming in a lathe, you may discover that you can achieve better results by pushing the tailstock by hand than by using the feed handle, which can't be turned fast enough to enter a hole without chatter. All depends on the speed at which you ream.

H

[pete]

I haven't machined much aluminum and nothing with as much removed as your doing so I've no real idea how much it moves after machining. I'd guess some with a part shape like that. Do you rough the parts out, let them stabilize out of the chuck for awhile then finish machine? I only found a mention of stress relieving 6061 alloy at 343 C for 1 hr and the temperatures required to do the same for 7075 warns it will result in over ageing of the material and "significantly reduce it's mechanical properties". So at least some thermal stabilization gets done during machining for some alloys of aluminum. Doing the bearing bore last should give a concentric round hole and the bearings should maintain that condition. I'd think you'd need to run a few tests to see if the rest of the part features remain concentric to the bore. Elliptical shaped reels wouldn't work to well for your customers.

Edit, I see Harold has already mentioned the rough, finish machining idea. Schablin, Myford http://www.myford-lathes.com/accessories21.html and others plus a great many watch maker lathes sold accessories usually called Quick Action Tail Stocks that uses a simple toggle action to drive the quill with a hand lever. Shaublin and probably others went so far as offering a second and even third complete tail stock that could be ordered with the lathe or later. Depending on what you were doing the whole tail stock got switched out. Some were also set up with a rack feed on the tail stock quill. At least one company offered that system as a retro fit for the Super 7 lathes in the UK. I'd assume all of them were for that fast feed of reamers and retraction of drills when chip clearing.

[RSG]

Thanks Harold, Pete,

Pete, annealing like you mention is a real no no with aluminum. loosing it's temper is one thing but more importantly it effects the outcome of the anodizing process so its definitely not something I will attempt.

Harold, pushing the tailstock is interesting, at first I thought it won't be aligned properly since it's not locked down but that really doesn't matter does it. I might just try that. As I mentioned before I sent my reamer to a friend in Ohio to have ground to .6247" and did some test cuts and the result is a smooth hole so that part is good.

I guess I just have to decide of reaming last will benefit things. At $40.00 per billet and the time it takes I don't want to spend too much trying to figure it out when what I've been doing has worked for years.

[Harold_V]

Harold, pushing the tailstock is interesting, at first I thought it won't be aligned properly since it's not locked down but that really doesn't matter does it.

Alignment when reaming is always critical, but it's almost impossible to have what would be perfect alignment with a lathe tailstock. When new, they're high, and as they wear they become less than parallel, wearing more at the headstock end of the tailstock than the opposite end*, and end up below center over time. They are also often offset a small amount.

That said, in order for a reamer to find center without creating a bellmouth, I have a policy of gripping them by the shortest possible amount, so the cutting end is free to seek center. If you remove a few thou, the margin, being circular ground, will readily center the reamer in the hole under that condition.

You want to make sure that there's enough shank gripped to ensure it doesn't pull out, or spin during the cut. If you're interested in exploring this method, chuck up a reamer by about ¼" of its shank and see how it feels at the end. You should be able to move it about with just a little effort. If you can't, back off a little on chucking pressure, or grip by a slightly shorter amount. Note that the shanks of most reamers, like the shanks of twist drills, are not hardened, so the chuck jaws will indent, which prevents the reamer from spinning during the cut.

The one thing that can be troublesome with the floating tailstock is if you've left too much material to be reamed. In aluminum, if you're leaving ten thou or less, I can't imagine it being a problem. In tool steel, with a larger reamer, 15 thou may cause the tailstock to tip under cutting pressure. With that in mind, ensure it isn't a problem by keeping the tailstock ever so slightly restrained. Mine has a cam lock, so I just let gravity pull the handle down and that seems to be adequate, but then I've not done a lot of reaming.

H

*The tailstock wear I mentioned above is generally the result of routinely moving the tailstock before wiping the ways and oiling. While it may be moved away from the headstock on occasion, in my experience it's usually parked well out of the way, and must be brought towards the headstock when needed, thus the wear at the headstock end. For that reason, I NEVER move my tailstock without first wiping and oiling. It takes just a moment to do so, and ensures a longer useful life of the machine.

[RSG]

Thanks for the added information Harold.

Regarding the wear comments, for the first 3 or 4 years I didn't pay too much attention to wiping the ways nor using the proper oil. After reading here (particularly your posts) regarding its importance I changed my ways and started doing it along with the correct oil. Now, I find myself cleaning them before starting the day and stopping mid way through the day and wiping/re-oiling the ways....including the tailstock ways....