Boring a cylinder - need advice please

[te5745]

I need to bore a cylinder in gray cast iron. The finish bore is to be one inch. The largest drill bit I have is 1/2". Do I drill to 1/2" (in how many steps?) and use a boring bar to get to reamer step; or, do I buy the additional drills to get to reamer step? I do not have a one inch reamer. Do I buy a fixed or adjustable? I admit I'm scared to try using a boring bar - my previous experience didn't end well. thanks in advance!

 

[portlandron]

If you want to keep the cost down drill it 1/2" with the drill you have then use the boring bar you have to get it just under the 1" finish bore. I would then purchase a 1" ream to use in finishing the bore. I would not get a adjustable ream but a straight flute one, it's a size you would probable use again if you build engines.

To drill the cylinder there is no need to do it in steps. Start first with a good center drill to center the 1/2" drill and just drill it in one step. Even if it gets a little off center the boring will bring it back to center.

The main problem you may have with boring is chatter marks which will clean up when you ream the bore.

 

[purpleknif]

I would add that if you ream to finish you really should give the reamer some back clearance . You can do this by stoning the reamer while running it backwards.

 

[bazmak]

For any cylinders over 3/4" i always use a boring bar in the lathe if poss
using the faceplt or 4 jaw.Reamers are too expensive.I also bought a cheap set of reduced shank drills for about $40 12 to 25 dia for step drilling.If you use a reamer you have to make the cylinder to fit the bore (usual practice) but for my latest 8 cylinder i used brass 3/4" stock polished lightly and the made the cylinder to fit.Little bit more difficult but i found it easy with 8 out of 8
regards Barry

 

[Blogwitch]

This seems to be a post about buying your way out of a problem.

Invariably, it never works.

It seems a little hard and unfriendly, but if you take this advice, you will never regret it.

Persevere and get your boring sorted and you should hardly ever need to buy a very expensive reamer.

You are working with cast iron, and that is one of the easiest materials to machine, if you can't bore that, you won't be able to bore hardly anything.

Rigidity and tool tip alignment is the secret to boring, get those right and you are 90% there, the rest is just finding a good speed for the job and getting your feed right, if in doubt, slow down both the lathe and feed and take small cuts.

Drill your job out to 1/2" then you have loads to practice on before you get anywhere near the size you need.

BTW, on a cylinder, usually near enough is good enough, as you make the piston later to match the bore, so if it is a couple of thou over or under on your bore, you should have no problems. Also, if you are boring right the way through, don't tighten up your chuck jaws too much otherwise you will end up with a triangular or square shaped bore where it has been held in the chuck, in fact the same will happen if you use a reamer or not. I always try to bore critical dimensions on the material outside the jaws and then part off.

Sorry to be so hard, and have a look at my signature line.


John

 

[gus]

John,
Well said and good advice backed by years' of turning experience. Incidentally I been boring C.I. Cylinders same way with good results. Tin Falcon gave me a good lead on Warner Boring Bars which gave me good boring for the 1/2 dozen I C engines built.The ''Cobalt'' HSS Bits stood up very well. Cylinders are very forgiving. A thou to two doesn't matter as you could make up with a OD matching Piston.
Gus had a good but wet weekend fishing. Nellie is happy with the two Snappers.
Take Care.

 

[toolznthings]

A word of caution. If you are going to step up in drill sizes make sure you " dub off " the next drill cutting edge. The drill will grab like brass in the cast iron.

As above posts. If you can bore to under size with good results, finish bore to size. Why ream ? Reamers are great in the right situation, but if I want a true hole I always bore where possible. Once you learn this operation you will be quite pleased with the new skill set.

Brian

 

[Hopper]

Another traditional way of finishing a model cylinder bore is to bore it to about .001" undersize, then make your own lapping tool and lap the final finish with some fine abrasive paste.
I think there is a whole book in the Workshop Practice series (or similar) on grinding and lapping in the lathe.

 

[petertha]

Here is my experience on cast iron.
http://www.homemodelenginemachinist.com/showthread.php?t=25163

I'd say skip the reamer & re-invest on some decent boring bar tooling. I found lapping to be slow going but no doubt on the finish & dimensional control you can achieve. It depends if you have to hit your 1" bore exact to fit existing piston/rings (example 1.000 +0.0005 -0.0000) or "about 1 inch with appropriate finish" knowing you will make piston/ring to suit whatever the diameter works out as. If its the first case and this is your first go, I'd aim for 0.002" under with boring bar. That should leave enough to remove all traces of tooling marks and/or hole irregularity & still not too much to lap off.

Another tip on drilling. The first big diameter bit will tend to push laterally pretty hard on the material back into chuck. That can risk having the blank move in the jaws unless you have lots of material to grip on &/or crank it down. Alternatively, pre-machine the end so the stub has a slight diameter reduction & the resultant edge now sits against the chuck jaws to prevent any movement. Good luck!

 

[Swifty]

There has been plenty of good advice regarding boring it to size, the main thing is to make sure that the bore is parallel. A few thou here or there on final bore diameter is of no consequence since you will be making the piston to match. Once you become proficient in machining you will become more at ease with minor changes to sizes.

Paul.

 

[Billitmotors]

G'day te5745
The main thing with setting up your boring bar, (preferably a boring bar with aproperly sharpened High speed steel tool bit), is to set it up with the minimum amount of overhang, make sure that the cutting edge is above centre, for a 1" bore use about .020" to .030" . Stone a small radius on the cutting point of the toolbit to smoothe the surface finish. Make sure that the boring bar is securely clamped preferably with at least 2 to 3 clamping screws, and use a slow speed and a slow feed. Because you are taking . 250" per side you have plenty of material to practise to find the optimum speed and feed. Don't bother with the reamer and take Hopper's advice and make a brass lap to get to final size.
Rob.

 

[goldstar31]

My advice is different as there is always the element of vibration with a single point tool and consequently cutting taper or barrel or worse.
The simplest and safest method is to do your boring between centres which ensures( if your lathe's Number one shear is Straight that your bore will be completely parallel despite the tailstock or whatever being a bit 'out'. It is geometrically accurate whilst the others are 'iffy'. Making an in line boring bar is as simple as complicated as you wish but Sparey - who is responsible for lots of bored cylinders- describes a simple tool in his Amateurs Lathe book. This is what every newcomer should have as an alternative to going into a store and buying a tool which will have a head scratching when the tool inevitably gets blunt. Years ago when I was making a Quorn tool and cutter grinder I had to bore 4 holes of 1" dead parallel but 3 had to be spot on 1.000" whilst the 4th had to be 1.003". Damned sight more complicated that a cylinder bore and I make up a George Thomas one which would have a controlled cutter advance of the thous and a half to do the final hole. Basically, it was a bit of 7/8th round with a 40 tpi advance. Still have it- rusting somewhere- along with the Quorn which is doing the same.

Be like all self respecting craftsmen( not machine minders) and make your own tools.

Regards


Norman

 

[Jasonb]

I'd usually drill to 7/8 in approx. 1/8" steps starting with 1/4" and then bore the last 1/8" to finish size and lap/hone as required but you can drill to 1/2" and bore out from there to finish size. I never ream a cylinder bore.

This is a 24mm one I did a couple of days ago and shows the drill sizes and the 3/4" dia homemade boring bar

PS John Bogs, if you are following the thread do you still have that photo of the Jowitt poppet valve engine you once posted as I cannot get it now as you have altered your PB setting. J

 

[kettrinboy]

If you go down the boring bar route , use as big a bar as you can fit in the bore for finishing like in Jasons photo, a smaller one is ok for roughing to within say 0.5 mm of the final size but will probably chatter a bit , and then sharpen the tool in the finishing bar before the final few cuts are taken , with the finest feed and assuming the bore is parallel to around 0.02 mm it shouldnt take much work to hone to the required surface finish from there, but dont overdo honing and polishing as you can lose the trueness of the bore or bellmouth it , ive never reamed a cylinder yet of this sort of size because i think boring is a better method , thats just my opinion though.