Reaming - depth of cut

I want to ream out a 12mm x 50mm deep through hole in EN1A to H7 tolerance. I have little experience with reaming and looking on the internet I've seen recommendations for initial drill size varying between 1-2 thou and 10-20 thou below finished diameter. So I'm confused!

My plan is to use a machine reamer mounted in the lathe tailstock.

Any advice?

Robin.

10-20 thou is fine.

I only have a standard set of drills and for 12mm reamer use a 11.5mm drill (20 thou = 0.508mm) which will produce a hole slightly bigger 11.5mm.

Paul

If its the first time you have reamed this sort of material, take the advice above, but try it out on a bit of scrap EN1A first. Its a shame to spoil a piece that you have invested time into.

Use your 11.5 drill to remove most of the material, but before you ream it take a very light cut down the drilled hole with a small boring bar, making sure you do not remove too much. This will ensure that any runout of the drilled hole is corrected before you ream it.

I did a 10mm hole 1½" deep last night using this method, and used a 3/8" drilled hole as the starting point, it is surprising how much your drill will wander off course by the time it reaches full depth and your reamer will just follow the drilled hole and the finished bore will not be concentric to the outside of your part.

I know not many people will advise you to do this boring operation, but it is a really important step if you want accurate results.

As Speedy said above, have a practice on some scrap to get the hang of it first.

Phil

Edited By Phil P on 05/11/2019 07:02:57

If it can fit in the lathe I would bore to 11.7mm as 50mm long a hole gives a drill the chance to wander and the reamer will just follow the hole.

Infact if it is a one off then I'd actually just carry on and bore to the finished size to give the fit I wanted on the mating part rather than ream.

If using a brand new reamer do as said above and try in some scrap. New reamers tend to cut big on the first pass or two.

New reamers tend to cut big on the first pass or two.

. . . . . or 10 or 100 passes. Don't just assume that the hole will be the size printed on the 'tin' particularly if you are using a machine reamer without a floating holder. Tailstocks are never bang on, neither are tailstock chucks. By all means ream the hole but measure afterwards. Reamers are handy to produce a number of holes to near identical dimensions but best practice is make the holes first and then turn the bits to fit in them afterwards.

regards Martin

Just to add to the confusion the more material the reamer has to remove the bigger the reamed hole will be. Also the speed of the reamer/work will have an effect on overall size. Fast surface speeds will produce a hole bigger than slower speeds. As my old mentor used to say if you have a surface finish/size issue then check your roughing tool first.

To add to the above, for imperial holes I generally use a drill 1/64" smaller (~16 thou), unless very small (1/8" or less when reaming gets closer to broaching anyway). My biggest reamer is 3/4", above that I would allow a bit more.

Neil

An important fact that has caught me out more than once. If you cut so much that the chips pack the flute of the reamer, the hole is going to be over-size. I've even caused a reamer to cut over-size deliberately by packing one flute with blue paper towel. Turned a tight fit into a free-sliding fit.

On stuff I’ve done the reamer cuts slightly larger under power on the lathe rather than by hand. With the reamer in the tail stock I run the reamer in manually first and check for size. If it’s too tight then I run it in again under power.

I was always taught the "1/64" (0.015" ) undersize technique.

I made up holders, using ER collets, so that the reamer can float.

If the reamer is off centre, for any reason, it is likely to behave like a boring bar, and cut oversize.

There is something to be said for locating with a centre in the Tailstock, rather than holding on the Morse taper, or in a drill chuck.

Howard

Thanks . The job is for someone who asked me to make a custom machine hand wheel to fit on a 12mm spindle - I haven't the spindle in hand, so I have to work to spec. Not my fault if it doesn't fit! If I were doing it for myself I would bore the hole then turn the spindle to fit, but I don't have that option.

I have an 11.5mm drill so will try with that on some scrap before going on. I read on the Sandvik site that reamers need to 'work', but they don't give any numbers. They don't want to commit themselves - too many variables I suspect!

Robin

Reaming is a tricky business, such that even my Machinery's Handbook declines to give any advice on this subject! It does, however, suggest that finish is improved by a low feedrate and reamer life maximised by using the highest possible (without saying what that is...)

Tubal Cain's workshop handbook avoids the subject too!

Neil

Robin, no one has mentioned using coolant when reaming steel, I always do, it helps to wash the chips away, and helps the reamer cut.

Chris Gunn

Remember reading somewhere that reaming with or without lubricant also makes a difference to the finished size, can't remember for certain which way round but have never tried it as I always use lubricant, except of course on CI.

Emgee

Yes good point Howard, I will try to remember that. Thanks.

I use the rule:

Up to 8mm diameter hole, drill 0.2mm undersize.

Above 8mm drill 0.3mm undersize.

Dormer recommend the following allowances:

Below 4mm: 0.1mm

Over 4 to 11mm: 0.2mm

Over 11 to 39: 0.3mm

Over 39 to 50: 0.4mm (Good luck with a reamer as large as 50mm)

The larger the drill, the larger the allowance, and I have seen charts suggesting between 2% and 3% undersize.

I agree it is best to drill smaller then bore to the undersized size, then ream, but I seldom bother under 8mm.

I also agree that a floating reamer holder is best. I use one made from the Hemingway kit. Works well.

Lots of neat cutting oil too.

Don't let the flutes get packed, so retract and clean at intervals.

Marcus