Boring – best practice?

[Mike HurleyParticipant @mikehurley60381]

In one form or another (from what I see searching previous posts) this topic has aired many times. Even after reviewing these, I'm still not 100% clear.

Boring in steels, either via the lathe or on the mill, using carbide tipped tools I get results I'm never totally happy with. If I use sharp HSS bits in a boring bar, I make slow progress but usually get a reasonable job, but this can prove tedious at times.

My general understanding on tips for (for example) external turning is they perform best with a higher speed and much heavier cut than HSS – which I find to be true. When boring though applying the same parameters doesn't work well for me as I seem to get to much (apparent) flexing in the bar and it always sounds as if the tip is rubbing rather than cutting although it does cut, but I find it difficult to get accuracy. I have to assume the geometry at the tip end is correct as this is pre-set by the design of the unit as a whole.

Before anyone asks – I'm using bars substantial enough for the dia of each hole attempted, the mounting is as solid as possible, gibs tight , slidey bits locked where approriate etc and the correct type of tip for the bar ( as detailed by the suppier). Am I missing something glaringly obvious?

Any comments appreciated. Regards Mike

[Mike HurleyParticipant @mikehurley60381]

[Ady1Participant @ady1]

Ady system

Biggest drill possible to start

Heavy inaccurate lower speed hogging to 98%

Finish boring with sharp fine feed cutting to 100%, high speed seems to help too

——

I also did a big 45mm hole in 12mm steel plate by putting the boring bar in the chuck and whirring it through with the job mounted on the saddle. It made a damn nice job of it with the swarf floating off as it went through

I've never done a full bore with the tool revolving between headstock/tailstock and the job feeding through but with a nicely ground tooltip it's definitely got good potential for a hobbyist

edit: I always use hss for boring because it's nice and sharp

Edited By Ady1 on 20/08/2023 10:00:52

[bernard towersParticipant @bernardtowers37738]

.Not trying to upset anyone but I find the heavy cuts and feed rates for carbide not always true, I use ccmt060204 and dcmt and rcmt inserts both standard and polished and find fine cuts just as successful as deep ones. On the question of boring in the mill it’s possible to rotate the boring bar in the head where on the lathe the boring bar has a flat on it giving positive location could that be part of the problem?

[JasonBModerator @jasonb]

Swap to a **GT insert for the finishing cuts or all for that matter being "sharper" than **MT they will not cause the bar to flex away from the work and can take light finishing cuts to take out any spring where a **MT will just ride up on the surface.

[SillyOldDufferModerator @sillyoldduffer]

Posted by bernard towers on 20/08/2023 09:46:56:

Not trying to upset anyone but I find the heavy cuts and feed rates for carbide not always true, …

A sensible observation. My workshop rarely allows the fast heavy cuts typically needed to optimise carbide. I mostly work on fist sized objects using not particularly fast, powerful or rigid hobby machines. Difficult to get high surface speeds on small diameter work, so sharper carbide inserts often cut better than blunt efficient ones.

Boring is on my list of difficult operations. The biggest problem I think is boring bars tend to flex and chatter because they have so much overhang.

For convenience I prefer carbide boring to HSS, but getting good results can be fiddly, maybe swapping inserts, and often having to try different combinations of RPM, Feed Rate, and Depth of Cut. Fast and light cuts generally, but much depends on the material and the depth and diameter of the hole. I find it easier to get good results on larger diameters and deep holes are harder than shallow.

Dave

[Howard LewisParticipant @howardlewis46836]

CCMT0604 tips in a 6mm boring bar is the method used most of the time, once the hole has been roughed out with a drill. So shallow cuts , 0.005" (0.127mm ) or less

Often stop putting on the cut before finished size, and take spring cuts to creep up on redqauired size.

Can take several spring cuts before ik stops cutting.

Speed is about 500 rpm, with a 0.0025"/rev feed (0.0635mm /rev)

It can make a noise, but the finish is good.

All the above defies the usual advice for carbide tips, but ikt works for me.

If I have a reaner, I use that instead, rather than spending time on spring cuts.

Howard

[not done it yetParticipant @notdoneityet]

Boring on the lathe, with a boring bar in the compound slide on a small (not very rigid) machine is never going to be straight-forward. Problems are further increased with increased depth of bore, not diameter. I would never countenance using the compound slide as a means of extending the boring bar.

Mounting the part on the carriage and using a boring bar (supported at the chuck and tailstock) can clearly reduce the number of flexing joints in the process. So far better for deeper (longer) bores, but a pain to set up, of course. I’ve never yet needed to make a boring bar of that form.

Boring on the mill allows shorter cutter extension, so is inherently better than on the lathe – the only real mounting problems being for awkward shaped items. Knee raising is, IMO, better than quill extension when boring (both my mills have knees, but a fair amount of head-space is needed, so I haven’t used the smaller one for boring).

On the lathe I first drill, then bore (if a larger size) – followed by a reamer, if I have one . So much less hassle for most holes.🙂 Much like Howard’s post above.

[Mike HurleyParticipant @mikehurley60381]

The question reared its head this time with a job opening a 13mm hole (biggest drill I've got) to about 28mm. The worpiece was about 55mm round so fitted in the lathe chuck (outside jaws) OK, started with my insert-based bars until I realised I could only 'rough ' bore through to about 20mm without hitting the lowest steps in the chuck jaws. Managed to get it set up on the Mill and used the boring head (which I've had many years but hardly used) with the brazed carbide tipped tools that came with it ( ! )

I think I cold have got a better finish and nore accurately sized hole if I tried chopping through with a stone axe and flint chisel.

I've taken a mental note of all your useful observations guys, and will definately try out one or two ideas the next time a task comes up. So appreciate the time taken – thanks

Regards, Mike

[Kiwi BlokeParticipant @kiwibloke62605]

Mike, sorry to hear of your difficulties. Are you 'missing something glaringly obvious?' Well, I can't tell, but you've left the door open for folk to risk insulting you with the basics…

it's nothing like as easy to set a boring bar's position with respect to the work as it is to set a lathe tool for external cutting. For a start, it's difficult to see what you're doing. A major risk is that there's interference between the bore and the bottom of the tool tip – obviously worse as the bore diameter decreases. We always try to stuff our thickest bar into the workpiece, so that's increasing the risk. It's often necessary to gain clearance by setting the tool at what looks like a horrible negative rake. Raising the point of contact so that it's a tad above centre height is also a good idea. I find it much harder to set a tool correctly in a boring head, but the geometry is the same.

I recently bored several bits of an unfriendly stainless steel (dunno what exactly) using an Emco Compact 5 and Arc Euro's no-name **MT and **GT inserts. Bore dimensions similar to your job. To be honest, I didn't expect much from such low-priced inserts, of unknown provenance, and used them as an experiment, reasoning that there wasn't much to be lost. They did the job splendidly! The Compact 5 is not the world's most rigid lathe, but the resulting bird's nests of stringy swarf were witness to the fairly serious cuts and feeds used (sorry, I can't quote any figures…). I can only think that success was due to the lathe being in good condition, and the careful setting of the tools.

[JasonBModerator @jasonb]

Posted by not done it yet on 21/08/2023 08:20:44:

………………….

Boring on the mill allows shorter cutter extension, so is inherently better than on the lathe

Can you explain why you need less tool extension on the mill?

To me if I'm boring say a 30mm deep hole I need just over 30mm of tool sticking out the toolpost so it won't hit the work and likewise if Using a boring head I need just over 30mm of tool sticking out to avoid the boring head hitting the work.

In practice I would say the lathe allows for minimal stick out a sit is easy to adjust the position of the bar in the toolpost but you might have to cut the boring bar shorter to adjust it's stick out from a boring head.

I do use a between ctrs bar quite often but that only really works for through holes, blind need to be approached from one end only.

[JasonBModerator @jasonb]

Mike, investing in a couple of "blacksmiths" drills (reduced shank) would be worthwhile as at 13mm the largest insert bar you could usefully start with would be around 8mm shank and at 55mm deep you are close to 7xD sticking out of the toolpost which is going to flex and chatter.

I really only use something like a 6mm bar mentioned above for small holes say taking a hole drilled 11mm out to 12mm finished size as the diameter of the job goes up I just used a larger dia tool and would only be using 5 thou cuts to finish things off 20-30thou to hog out the majority of the waste on the Chinese hobby machine.

[HOWARDTParticipant @howardt]

Use a tip with the larger radius. Surface finish is a function of the tip radius, feed rate and depth of cut. Getting the speed and feeds right for the material being cut can be a challenge sometimes with unknown materials, you cannot be sure that the steel is tough or free cutting, brass and soft materials cut better with different edge geometries. There is a lot of science in machining.

[noel shelleyParticipant @noelshelley55608]

If the finish REALLY matters, rough out, leaving slightly undersize and finish with a cylinder hone ! Noel.

[Chris MateParticipant @chrismate31303]

After I received a new boring head and boring bar with inserts, and sort of solved my problems initially by comparing it to better bars etc, I shortened the bar and it seems ok., I was however offered assistance should I need further assistance by a different company that sell Walter tools in the form of they will find me inserts for that bar that wil cur freely and correctly. They know what I got, so I assume if everything is ok, your last resort will be insert types for that bar etc which in my case these people has the science behind it, and stuff I bought from them before were all excellent, however their top boring heads and bars are too expensive for me, but they still saw a good selution not overly expensive.

[Mike HurleyParticipant @mikehurley60381]

Posted by Kiwi Bloke on 21/08/2023 11:14:36:

Mike, sorry to hear of your difficulties. Are you 'missing something glaringly obvious?' Well, I can't tell, but you've left the door open for folk to risk insulting you with the basics…

Doesn't bother me at all, I genuinely believe you're never too old to learn something new, or occasionally unlearn something you've been doing poorly for years. A proportion of guys on this forum (like me) never had formal training in industry/ apprenticeship so are self taught,- and a lot of the learning was pre-internet / YouTube days, so you read what books you could get hold of, had a go and often got it right, sometimes not. But bad techniques could also be picked up.

If you aren't open to helpful suggestions from others you are missing a trick.

I prefer to be open minded & more than happy to take others ideas on board.

Thanks again for all the useful info guys!

Regards Mike

[Tim StevensParticipant @timstevens64731]

I would argue with Ady1 that the best start might be with a short (inflexible) drill, rather than a 'big' one. Get the hole properly central throughout and there is less chance of further eccentricity.

And just so you know, I think there is a generous selection of eccentricity in many of the postings, and a good thing too.

Cheers, Tim

[Howard LewisParticipant @howardlewis46836]

Tim,

Almost certainly, we each have a stable containing at least one hobby horse that we ride from time to time.

I certainly have!

Howard

[Mike HurleyParticipant @mikehurley60381]

Posted by JasonB on 21/08/2023 11:32:59:

Mike, investing in a couple of "blacksmiths" drills (reduced shank) would be worthwhile as at 13mm the largest insert bar you could usefully start with would be around 8mm shank and at 55mm deep you are close to 7xD sticking out of the toolpost which is going to flex and chatter……..

I know of these drills, but have never owned or used one. I'd be looking at very occasional use in the lathe (Bench drill a bit too lightweight) which is a Chinese BV20 3/4hp geared head with VFD. So what practically would be the largest size something like this might cope with do you think? I've seen quite modestly priced sets online ranging 14 – 25mm but (OK quality might not be too good , but for once-in-a-blue moon use ? ) or might consider, as you said, a couple of odd better quality ones say 15, 18, 22 ?

I appreciate it's a bit of a 'how long is a piece of string' type question, and wouldn't hold anything against you if it don't work well, but your thoughts would be appreciated.

regards Mike

[JasonBModerator @jasonb]

You would be unlikely to be able to go straight in with a big one but working up in 3mm or 1/8" steps it should cope with at least 20mm.

I have the 1/8 "increments upto 1" and not any special quality and just work my way up in size which is generally quicker than trying to force a big one in from the start. Good enough to quickly remove metal so you can get a half decent sized boring bar into the hole. This was drilled to 7/8" (22mm) and then bored to the final 24mm.

[Mike HurleyParticipant @mikehurley60381]

Much appreciated Jason.

Regards Mike

[Author]

Posts