PDA

View Full Version : Boring bar setup selection



Subarubrat
01-15-2014, 11:33 PM
Taking the advice of more experienced people I ordered the Elderberry steam engine kits and they really do have some amazing instructions for a person who has never really used a mill/lathe and needs allot of guidance. I have accumulated most of the tools and options needed for the kits other than the boring bar setup that unfortunately isn't well described other than to say there are many options. That was surprising because for ever other step they assume you don't know where the on switch is. The task is to drill up to 1/2in then bore the cylinder to a step under 9/16 and then ream/sand to finished size of .5625

1. If last drill used is .500 why can't you just ream to .562 (9/16) followed by the sanding with #400, is 1/16 too much of a step for a reamer to reasonably cut?

2. If a boring bar is needed for that last step I would like to buy a holder/bar set that will do this job as well as be generally useful but what would be a sensible choice for my G0516 mill/lathe?

Jaakko Fagerlund
01-15-2014, 11:48 PM
1/16" is a way too much for a reamer that small. Also a drilled hole is not straight nor round, so the reamer would tend to make something non-straight and over sized hole.

Can't give a suggestion for such a small boring bar, but I would look at a solid carbide bar that uses CCMT inserts with very small nose radius and meant for fine finishing.

v860rich
01-16-2014, 12:44 AM
With a small reamer like that you will need to get your hole to within 1/64 of the finished size.
I'm not familiar with your mill so I can't answer you boring bar question.

THANX RICH

RussZHC
01-16-2014, 01:15 AM
How deep/long is this hole?

Asking as I was thinking of suggesting a brazed tip version from someone like Micro 100 BUT you might run into issues with the depth you need to get to...Micro, as example, offers many bars that will fit into that half inch drilled hole but one begins to become limited as to how deep before there is more and more flex in the bar, solid carbide would help but cost will certainly go up. Ultradex makes some really nice carbide insert bars in 3/8" diameter...not sure how deep they suggest you can go to though...

Subarubrat
01-16-2014, 01:30 AM
The drawing shows the cylinder to be 1.38 in long with the bore running full length.

dan s
01-16-2014, 02:08 AM
Personally, I would just buy a drill bit or two to bridge the gap between the 1/2" bit and 1/64th under the finished dimension. The I would just ream it to final dimension.

If you want bore the hole do it in late mode, as you will have a lot more control on the diameter of the hole depending on what angle you have your cross slide set at.

for a machine the size of yours, Id go with the old school broached bar holders. they use normal hss blanks that you can grind to any profile. They are cheap and easy to work with.
http://www.use-enco.com/CGI/INSRIT?PARTPG=INLMKD&PMPXNO=949565&PMAKA=378-4000

the next step up in quality and price are Everede bars like this that take little triangular hss bits that you grind your self.
http://www.use-enco.com/CGI/INSRIT?PARTPG=INLMKD&PMPXNO=948646&PMAKA=376-6010
http://www.use-enco.com/CGI/INSRIT?PARTPG=INLMKD&PMPXNO=949571&PMAKA=376-7010

above the Everede bars are modern indexable insert bars made of either steel or carbide.

the cheap brazed boring bars are ok in a pinch but I would generally advise against them, as you can't adjust stick-out with them.

RussZHC
01-16-2014, 07:38 AM
With that depth of hole, there are "many options" as the instructions stated.

Micro 100 for one has quite a few that will work given min hole size, and that depth (brazed on tip), Everede has some in almost every series they make (several different type of inserts so something you may already have might be available) alloy, carbide or heavy metal shank, though choice does lessen a bit if you use their triangular shaped tool bit versions...most manufacturers you don't even need to go to their "midget" boring bars.
Sorry to say but it looks almost like how much money do you want to spend? Because they appear to be fairly common, you may find something very good and quite cheap going the eBay route

J Tiers
01-16-2014, 08:49 AM
A half inch hole is pretty big, really, even the cheap chinese/indian "sheepfoot" boring bar sets have bars that will do that size easily.

Drilling to a reasonably close size, followed by boring to a reamer-suitable size is one approach. Boring to final size is another, but the reamer probably will give a better finish and parallelism than boring with a non-rigid bar, considering that this is apparently an engine cylinder.

Most cheap boring bar sets have sharp pointed cutting edges, and will give a "ridgy" finish even with good care taken. The ridges are a bad surface for a cylinder, since they occur in rings, not lengthwise grooves, plus they make the true size of the cylinder larger than the measured size once the ridges wear down. The reamer ensures finishing to size, and reaming as a final step can ensure a better finish.

I would suggest buying a fairly cheap boring bar set, and using it. You will develop some idea of how things go with the process of boring, learning more about what you will really want in the long run. And if one of them breaks, it is no big loss.

They will certainly do the job you need done to ready the parts for reaming.

One note about boring... it is common for the hole to be smaller at the deepest part, and larger at the mouth. The mouth may even get to be over-sized. You need to measure, and work longer on the deep area to counteract this tendency.

One reason for the tendency is boring bar deflection under the cutting forces. As you bore deeper and deeper, the pressure of the cut tends to bend the bar inwards, more and more. That allows a tapered hole. The hole may work-harden a bit and resist the bars cutting action also.

The tendency is to keep moving the bar outwards to increase the hole size, but you really need to spend more time cutting the deeper parts, and/or to cut on the withdrawal as well instead of only on the entry movement into the hole.

At some point, the bar may be bent (sprung, really, the bend isn't permanent) sufficiently that the side force allows it to cut better, and it may cut down to closer to full depth again... If you have moved it outward too much, that may cause a crash or a stall as it suddenly cuts much deeper than you expect. Can break the bar, or stall the machine, depending.

Keep an eye on the hole size and taper , and spend more time on "spring cuts" deeper in the hole. A "spring cut" is a second or third cutting pass without adjusting the cut depth. It allows the "spring" of the tool to work itself out, as the tool cuts until it is straight again with no remaining "spring" that provides a side force. You dont adjust the tool position until it no longer cuts at any point in the bore.

With the small cut they suggest, taper may not be a big issue, but it would certainly cause more effort and worse finish when reaming, or especially sanding/"lapping" to size.

tylernt
01-16-2014, 10:37 AM
One note about boring... it is common for the hole to be smaller at the deepest part, and larger at the mouth.
...
One reason for the tendency is boring bar deflection under the cutting forces. As you bore deeper and deeper, the pressure of the cut tends to bend the bar inwards, more and more.

I'll readily admit I'm no expert, but I'm not sure I agree. If your boring bar is stuck out 1.5" to bore a 1.38" deep hole, the bar has the same amount of stickout, tool pressure, and deflection at the beginning of the bore as it does in the end of the bore. So I don't see why the setup would be inherently prone to wide-mouth taper (unless there was more wear in the ways closer to the headstock). If anything, I would expect work deflection in long or thin stock to cause the opposite taper to occur (smaller at the beginning with less work deflection deeper in the bore).

Anyway, if I needed to bore out a 1/2" starter hole, I'd grab a round 1/2" HSS blank toolbit, grind a little side relief, grind a cutting edge at the end of it, and bam -- I'd have a boring bar that can reach in 1.5" to maybe 2" no problem. It's worked for me before.

And if I didn't want to go to all that grinding effort, I'd instead grab a 2-flute endmill, cock it counterclockwise in the toolpost a tiny bit (to provide side relief so the side of the endmill doesn't cut a taper), and use one of the flutes as a pre-made boring bar. I've successfully done this before too, before I had a "proper" boring bar.

Toolguy
01-16-2014, 01:01 PM
All good points above. I would just add - to set the cutting edge of a boring bar slightly above center so when it is bent down by the forces pushing against it, it will go to a point of less contact with the part. If on center when it bends down, it will dig in deeper and cause chatter and gouges.

Boucher
01-16-2014, 01:46 PM
There are times that a end mill will make a better starting hole than a drill. Old carbide end mills can be ground to make excellent boring bars.

J Tiers
01-16-2014, 07:42 PM
I'll readily admit I'm no expert, but I'm not sure I agree. If your boring bar is stuck out 1.5" to bore a 1.38" deep hole, the bar has the same amount of stickout, tool pressure, and deflection at the beginning of the bore as it does in the end of the bore. So I don't see why the setup would be inherently prone to wide-mouth taper (unless there was more wear in the ways closer to the headstock).


You'd THINK so, but it seems not to happen that way. I thought that as well, but then I saw the way the bores ended up....

And there is a reason......

Once the bar deflects a little, that gives a new starting point, so now it deflects a little more due to the same forces that caused it to deflect in the first place. The amount of "rubbing" instead of cutting also can work harden the bore, so now it has even less ability to cut those places on the next pass, unless you take a deeper cut to get past the work hardened surface.

That goes on until the force due to the deflection overcomes the forces that deflect the bar, and suddenly it cuts again. Often that leads to an uneven bore if some of the areas are workhardened.

Cutting as you move the bar OUT of the bore can allow it to get under the workhardened areas, and also provides a different set of forces, as well as sometimes a fresh, sharper edge. That can help to overcome the taper issue.

wierdscience
01-16-2014, 08:42 PM
If your going to ream the hole anyway,then there is no reason to bore it full depth.Drills walk off center and make holes that are out of round.Boring the mouth of a hole trues it to the spindle axis and makes it round again making a place to start a reamer.
What I would do normally is drill the hole 17/32 and bore just the first 1/4" or so to .540-.550" then ream.Doing this you only need a short boring tool which can be freehand ground out of a square HSS toolbit.

I also prefer lefthand sprial,righthand cut reamers.They make more accurate holes and push the cuttings ahead of the reamer instead of letting them pile up in the flutes.
http://www.ebay.com/itm/NEW-CHUCKING-REAMER-LH-SPIRAL-RH-CUT-9-16-5625-HSS-R04-/310783647043

dian
01-17-2014, 04:26 AM
why not just use an endmill? i have 3 flute endmills, that produce very good finish and a hole exactly matching a hole reamed to h7 size.

J Tiers
01-17-2014, 08:29 AM
If your going to ream the hole anyway,then there is no reason to bore it full depth.

There kinda IS, depending on the way you will ream it... Reamers walk off-center also, for similar reasons to drills. But they tend to be stiffer than drills, at least that jobber length drills.

If the hole is not on-center, the reamer will be forced off center also, it likes to follow the hole, although it *will* be straightER than the original hole. Boring gives a good symmetrical hole, and the reamer can size it without being pushed around by an irregular hole.

That said, it depends on *how straight* it needs to be, and how long and flexible the machine reamer is. Hand reamers can be started off-line and obviously hand reaming is not a great choice for straight holes square to the part.

Subarubrat
01-18-2014, 04:11 AM
Ok, so all this brings up another question. For project #1 and 2 that I am doing, which are the elderberry launch and mill steam engines which are intended to be tutorials for people just like me, the bore is fairly small and they suggest drill - bore - ream. The third project I want to try is a hit - miss engine, has a much larger bore and while I am sure you can get a reamer in that size it doesn't seem like the way a home machinist on a mini mill would go. How would one get an engine cyliner quality finish following a bore without using a reamer?

I am saving the hit n miss until I get some skills from the elderberry steam projects but these are questions that come to mind as I learn.

mattthemuppet
01-18-2014, 10:48 AM
I'm no machinist, but I'd finish the bore slightly under size using a lot of high speed cut s with a very sharp HSS boring bar taking very light cuts, then finish off with a cylinder home (brake c cylinder home should fit)

J Tiers
01-18-2014, 10:59 AM
I'm no machinist, but I'd finish the bore slightly under size using a lot of high speed cut s with a very sharp HSS boring bar taking very light cuts, then finish off with a cylinder home (brake c cylinder home should fit)

What? You mean do it the way folks who MAKE engines commercially do?

Of course they do use a bit better equipment, but boring followed by abrasives is my understanding of the commercial approach. They do it so well that the traditional "break-in" time is less important than it used to be.

Jaakko Fagerlund
01-18-2014, 11:30 AM
why not just use an endmill? i have 3 flute endmills, that produce very good finish and a hole exactly matching a hole reamed to h7 size.
Because they are sidecutting, and if anything goes wrong at any point (stuck chip or anything), it will bite the hole oversized. End mills also have no lead-in chamfer, so they don't center at all and thus require extremely rigid mounting and movement to provide on-size hole. And end mills geerally don't have back-taper like reamers do, so they rub their whole length in the hole, thus going way past your H7 tolerances with even the slightest misalignment or movement.

Do a hole with an end mill and check it with a H7 tolerance gauge and you'll see what I mean.