QCTP - better late than never

[schwabw]

Hello all,

I finally got a Phase III AXA attached to my 12x36 geared head lathe; add a couple of extra holders for turning and facing use and a couple of commercial parting blades. I was able to grind something that parts, but it takes a fairly wide cut, and for $12, it seemed reasonable to try the 0.040" gizmo off the shelf. With luck, this will be more flexible than I was with my 4-position tool post, and certainly more convenient. You might recall that my main gripe with the 4-position post was that the indents were a whopping 90 degrees apart! It would lock into place parallel and perpendicular to the compound, and that was it - honest. Nice post otherwise, but the lack of indexing was ridiculous.

Hopefully, I have reasonable left (just what I seem to use) cutting toolbits that will let me turn and face. For benefit of the parting blade, I have the post set up (visually only so far - suggestions welcome) square to the bed. I can of course set the post to any angle I want, but to have it square for the parting tool means that turning and facing tools are not as off-square as I might like. By mounting the toolbits a little skew in the holders, I think it will be ok. That seems to be the usual answer, but I figured I'd mention it in case there is a much better way to do things.

Bill

[JackF]

Bill,

I am still learning every day in this machining hobby of mine but I don't think that clamping the turning and facing tools a little askew in the holder is good practice. Not being supported on the side against the tool holder they could slip causing the cutter to gouge the part ruining it and or causing a crash. Others more seasoned please join in.

Jack.

[Harold_V]

Tool holders tend to be wider than the tool they are to accommodate, for just that reason. There are times when you wish to have more or less lead on a turning tool, or to create clearance on a boring bar, so setting them in the holder at a slight angle isn't an issue. Unless a tool is poorly clamped, it shouldn't move without a crash, at which point it really makes no difference how it's mounted. Rule of thumb may be to set tools such that pressure causes them to move out of a cut instead of deeper, but we don't always have that option. Use good judgment when setting your tools and choose the angle that suits the operation.

Harold

[schwabw]

Harold,

One other question has been rattling around my head. At one point, I asked about making several copies (a large run in my world ) of a part, and you said that I should be (for lack of better words) running them all through a given step before moving on to the next step. At least I _think_ that's what you said; it made sense.

Is there any conflict between that and what I think is the correct way to make some bushings I have in mind? My plan is to (suggestions/corrections welcome, as always): (1) set round stock in the chuck; (2) face the end; (3) maybe turn the sides (not really needed in this case); (4) drill the center hole; (5) part off the bushing.

Is the "take them all through one step" approach something that one would do mostly when turning on centers? Would you not work that way when the plan is to part off as the last step? Is that the only exception? Am I making sense? There was a time when running a mill was always confusing; now it's just intermittently humbling. I assume running a lathe will eventually end up that way too.

Bill

[Harold_V]

Bill,
My comments in regards to how to run a part would be typical of a part that was not simple, or was not reliant on a stable temperature (tight tolerance). Two important functions happen in that case. By roughing the part entirely on the first end, stresses are relieved, so when finish cuts are taken the part is stable, plus the roughed part has time to cool. Second---if there's both roughing and finishing required, tooling for finish cuts is often different---details that are not roughed are included, such as O ring grooves and minor details, such as specific chamfers.

So then, good judgment is the name of the game. If you can perform all the required operations without issue, it makes no sense to handle the parts more than once, but if there's a benefit to roughing completely before beginning the finish operation, that method is preferred. In the case of working with a square block tool post, you may not have the options that are open to you with your new post. With that system, you are limited only by the number of holders you possess, very unlike the square block, where you can find yourself limited to as few as three tools in a particular setup.

It is almost always a good policy to rough parts before finishing. There are exceptions.

Hope this helps, Bill.

Harold

[schwabw]

Harold,

Understood about roughing, and I'm pleased to say that I did think of that. In this case, it probably would make sense to face crudely, center drill, drill the "real" hole, face, and then part off. That way the stresses relieved by the drilling would not affect the parallelism of the ends - the outer surface is not important. If I have spare time when I actually make them, I might turn them for practice, but they are simply spacers and the raw stock OD and finish is fine.

I guess my question is really about workholding with and without parting off as a step. The parts that were the subject of my earlier question (where you recommended working in steps) is the one with the nickel in the photo. The OD had to be pretty good; ideally it would be a cylinder (or two concentric pieces of same) with a wall/band between them, also concentric with both. In reality, I doubt I achieved concentricity, but it was all a waste of time anyway - long story. Continuing, the bored holes ideally end in flat surfaces aligned with the band. In truth, that's not critical, but it was my goal. The point of the part is for that thin wall to be drilled on center to a specific size; different copies of the part having different size center holes. They are flow constrictors.

Given that I knew even less then than I do now about lathes, I was pretty happy with the results. How would you make them? One cannot simply face/turn/bore/part-off because the parts have to be bored from both ends and there is a lot of potential for the boring to alter the shape. I ended up using a 3-jaw chuck and accepted any error in concentricity, but I'm curious about other approaches in case that were not acceptable.

The other photo shows the spacers in their natural habitat. Design changes will force me to shorten them; I'm tempted to make new ones to practice with the QCTP and parting blade. If time is tight, I might simply face them down to length and move on to other work.

Bill

[Harold_V]

How would you make them? One cannot simply face/turn/bore/part-off because the parts have to be bored from both ends and there is a lot of potential for the boring to alter the shape. I ended up using a 3-jaw chuck and accepted any error in concentricity, but I'm curious about other approaches in case that were not acceptable.

In an example such as you've shown, tolerance would dictate my procedure. Assuming that none of the diameters required less than a thou tolerance, I'd face, rough turn the first diameter, drill, then bore. I would then finish face to length and turn the first diameter to length. If the bore was to a shoulder, I'd finish face before boring, so I could establish the proper depth. I would part the piece, then hold them by the first diameter in soft jaws that had a shoulder. That would create a reliable stop so lengths could be established. Gripping the part on the diameter in question, I would then face to length and turn the second diameter. Movement of material on a lathe isn't usually as serious an issue as it might be on a mill, where material isn't removed uniformly, as it is running a lathe. Round stock will tend to move slightly, so unless you're working to tenths, you generally have little to worry about. I suggest you make a thou as the break point. If your tolerance is a thou or greater, you generally have nothing to worry about when machining the second side of a part. The sole exception may be if you have to remove a huge amount of stock--at which time roughing fully before finishing is always a good policy. There are times when a finished surface is simply too fragile to sustain the kinds of pressures involved in roughing the second side.

The only difference I'd make, assuming that the parts required consistent concentricity and tight tolerances would be to rough the first side, drill the hole, part, then rough the second side. I would then grip on the roughed turn and start finish cuts. Soft jaws should be reliable to less than a half thou for concentricity, and a tenth or two for linear dimensions. By machining the jaws with stops, lengths are never a problem.

The other photo shows the spacers in their natural habitat. Design changes will force me to shorten them; I'm tempted to make new ones to practice with the QCTP and parting blade. If time is tight, I might simply face them down to length and move on to other work.

In either case, soft jaws will really aid in the process. The moment you move away from a single part, or if you must follow a part with a second operation, it's rare that you won't benefit by using soft jaws.

It's been easy (and fun) to talk with you on these subjects. You don't "cop an attitude" when suggestions are made. I like that.

You can be justly proud of your progress, Bill.

Harold

[schwabw]

Harold,

As always, thanks for your help. Others have taught me things over the years, but you stand out as the most influential of my mentors in metalworking.

I have yet to use soft jaws, but they make sense. There are two challenges I have, one being easily, though not necessarily cheaply, correctable. The first is that my chucks have one-piece jaws, so I *think* that prevents my readily making custom jaw "tops" and bolting them into place. That is what you do, right? The second problem is that I frequently make very few copies of any given part, so I would be making jaws specific to just one or two parts. Of course, if I wanted to hit really tight tolerances, that might be the best or only way to do it. I might also end up with a few weird dimensions and be able to re-use the jaws. Is that realistic, or do they get bolted in place, machined to size on the lathe, and then need to be left in place to be useful?

For the flow constrictors, the OD is set by outside forces, so it is unlikely that I would have a 5C collet of the right size, though I could buy machinable collets and build a small collection of them with known/weird IDs. For many things that I make, I control the design and could often choose diameters to match 5C collets that I have on hand. In fact, I bought "every other collet" to save money, knowing that I can always fill the gaps any time there is a good sale some place. A 5C chuck is making its way to the top of my "next toy" list.

Thanks!!

Bill

[GlennW]

Hello Bill,

You should be aware that soft jaws can be far more accurate than some inexpensive 5C collets. I've seen cheap 5C collets with as much as .004" TIR even though they claim far less.

I was centering a collet fixture beneath my spindle and nothing seemed to be working out. I was using a no name 5C collet with a 3/8 dowel pin to do so. I had the pin and collet in and out of the fixture numerous times to check for debris etc that may be contributing to the runout and found nothing. I swept the bare spindle with a .0001" dti and it was nearly perfect. I switched to a Hardinge collet (which I have been harvesting off of eBay for a fraction of new cost) and the first try yielded .0001" TIR.

I then checked some other no name collets and found them anywhere from .0005" to .004" out.

Not all are a problem, but just don't assume that you are in good shape runout wise just because you are using collets!

Using a collet chuck and boring "emergency collets" should work out well as long as you index the chuck to the spindle for repeatbility when removing and installing the chuck.

A chuck to be used for soft jaws does not need to be expensive or necessarily accurate as you bore the jaws in place.(as you alredy know) Therefore a used chuck with two piece jaws from eBay or other used tooling supplier should suffice without investing much money in it. Occasionally, you run accross a chuck with the top jaws missing, which considerably devalues it to most people.

I use an old worn out chuck with sloppy bell mouth jaws that I have had for years and it works just fine as long as you pre-load the soft jaws properly prior to machining them.

Just a FYI sort of suggestion!

[Harold_V]

I have yet to use soft jaws, but they make sense. There are two challenges I have, one being easily, though not necessarily cheaply, correctable. The first is that my chucks have one-piece jaws, so I *think* that prevents my readily making custom jaw "tops" and bolting them into place. That is what you do, right?

That's correct. Not all three jaws have the capability as sold---they tend to come with two sets of jaws, neither of which is what I call a set of master jaws. They are the ones that have a set of tapped holes and will accommodate soft jaws. Some chucks are sold with three sets of jaws, with the third set for soft jaw use. Others come with master jaws and reversible hard jaws, while still others come with two sets of hard jaws that mount on master jaws. In order to make soft jaws easily, master jaws are pretty much a requirement, although not mandatory. There are cases where guys have made jaws that clamped to their hard jaws. More labor intensive, but a bail-out when you are faced with holding a part that is difficult to chuck. That's one of the reasons for soft jaws---not just for precision. Ease of fast and reliable chucking with registration ability is one of the chief reasons they are used.

The second problem is that I frequently make very few copies of any given part, so I would be making jaws specific to just one or two parts.

Depending on the nature of the part that requires chucking, it's often faster and easier to use soft jaws, even for just one piece. A good example is holding a very thin object---a washer, for example---one that must be faced or bored, and must be concentric and parallel. Soft jaws do that without effort. Another good example is holding a thin walled object without distortion. Wide jaws, known as pie jaws, can be used, which encircle the part almost entirely, so it doesn't crush. Chucking such items can be an exercise in frustration using hard jaws.

I might also end up with a few weird dimensions and be able to re-use the jaws. Is that realistic, or do they get bolted in place, machined to size on the lathe, and then need to be left in place to be useful?

All depends on the nature of the jaws, Bill. I use a set for gripping round stock and don't bother boring them unless the job is critical. They, by nature, run quite true, always parallel to the spindle. Long pieces of cold rolled or ground material, by nature, tend to run in an irregular pattern when gripped by hard jaws, especially if the chuck in question has a few miles to its credit and the jaws are slightly sprung. When that condition exists, the material may run true at the rear of the jaw, where they contact the part, but because the jaws are not parallel to the spindle centerline, it tends to run off center at the ends. Even if you can true it, because it's not supported by the jaws at the jaw end, you risk chatter, plus movement of the material. That can all be eliminated with soft jaws, even with an old, well worn and used chuck. Glenn's comments in that regard are right on the money. He is exceptional in his talent and skills and can advise you perfectly well, too. I trust his judgment.

Ok, back to the question at hand. Can the jaws be reused?
Yes, they can, and for various configurations. However, what is generally desirable is for the operator to have a selection of jaw sets. You can also reverse a set in the chuck, so it is like having two sets, each with their own configuration. If you have a few styles, you can often match a set of jaws to the task at hand, install them, then, using a spider, set them such that all they require is a skim cut to run true. Soft jaws can enjoy a lifespan of years, and, if made of steel instead of aluminum, can be rebuilt by welding a section of steel to the well used jaw. I've done that with one set of mine, and have enjoyed using them since the late 60's. They're still going strong.

For the flow constrictors, the OD is set by outside forces, so it is unlikely that I would have a 5C collet of the right size, though I could buy machinable collets and build a small collection of them with known/weird IDs.

I would also mention that you can use step chucks for holding items. They aren't cheap, but they can answer some of your questions. Still, soft jaws are really the best possible solution. Rarely do you see them in home shops, but they are the norm in commercial shops. They are simply the finest possible way to grip items so long as you don't require a tenth or two of concentricity.. I have relied on them routinely for work that has .0005" tolerance or greater for concentricity.

For many things that I make, I control the design and could often choose diameters to match 5C collets that I have on hand. In fact, I bought "every other collet" to save money, knowing that I can always fill the gaps any time there is a good sale some place. A 5C chuck is making its way to the top of my "next toy" list.

I don't own a broad selection of collets, in spite of enjoying them when appropriate. What I've done in several cases is to turn a sleeve that adapts the diameter to a larger collet. I try to choose one that is very close to the size in question, so the sleeve is very thin. It's easy to make the sleeve, and it need not be split in order to work well Give a sleeve a thou of clearance on the part it's to adapt, so it goes on and comes off easily, and it will hold a part as if it was collet size, even without splitting the sleeve. This can bail you out when it's Saturday afternoon and you must get the job out, with no prospects of buying the collet you need.

Bill, here's a link that will take you to a rather lengthy post I made years ago. It talks all about soft jaws, and will explain the spider I spoke of. If you explore the link, you should find enough information to answer almost any question you may have about soft jaws, and how to go about their use. I hope it helps answer some of your questions.

http://www.chaski.org/homemachinist/vie ... =44&t=4266

Harold

[schwabw]

Harold,

Much reading will need to happen on soft jaws. I just finished my first real use of the new post, and I'm sold. In particular, the parting blade and holder worked wonders. Well, it would have if I had drilled the hole as far as I thought I had The really embarrassing part is that I did it again on the second spacer

One thing that I am noticing: I have been drilling 0.25" diameter holes and I'm getting what looks like work hardening[*] and even some metal sticking to the flutes. Any idea what I am doing wrong? The bit is not exactly new and the metal is some mutt Al round stock that was standing in the corner of my garage.

[*] please keep in mind that metallurgy is a lot like chemistry, and any time something looks white to me a chemist will come along and say it's black. Translation: I could be completely wrong about the abuse that has befallen the metal.

Bill

[John Evans]

Aluminum likes really sharp tools, a drill that is a bit on the dull side will soon have metal sticking on it. A bit of lube helps and if the hole is more than 2-3 diameters deep back out and clear the chips.