Drilling of 34CrNiMo6 4340 817M40 En24?

[PekkaNFParticipant @pekkanf]

I bought 4-6 metres of 16/20/25 mm tempering steel. It’s 34CrNiMo6 to me, these are other names for same stuff (or close)

4340

817M40

En24

 

Some of the bars are rolled some bright, but all are in tempered state. That is: free machining it aint. Swarf is closer to 2 metres than to well behaved chips. I’l manage pretty well external turning, pilot holes etc.

 

I’m trying to make axles/shafts/spindles out of this material and most of it I’m not heat treating after. Plan is to rough it on tempered state, age, finish to dimensions and use it happily.

 

I fail miserably on long pilot holes. I would like to make a pilot hole of 5 to 12 mm diameter and 60 – 120 mm long. This is pretty long by any standard I know.

 

This has stumped me totaly. I have Dormer and such drills, I use emulsion and pecker drill and hunt for right speed but I get snatches and blunt drill corners. If the drill squeals and produces black/violet swarf I go down with the speed and then I’ll get chatter and work hardening.

 

I would like to think slowing down to 640 rpm and increasing feed over 0.2 mm from 8mm HSS co5 drill and flooding it might be an official answer, but I have no power feed on tail stock and suds is not actually automatic and I bluntted and jammed one dormer bit trying it allready.

 

Advice on method and maching parameters are mostly wellcome.

 

PekkaNF

Edited By PekkaNF on 10/11/2010 10:48:49

[PekkaNFParticipant @pekkanf]

Drilling of a long pilot hole on Tempering steel?

[adyParticipant @ady]

Some of my engineering offcuts were pretty hard, tempered/semi-tempered.

 

Carbide was the only material happy to chomp through the tough bits, and good lathe stiffness is essential whenever possible.

 

I would try a boring bar with a carbide tip fitted like a flat drill bit.

You’ll probably have to modify an old boring bar or make your own.

 

It also sounds to me like you’re using too high a speed, so all you will do is heat harden an already hard material.

High torque, low speed, mounted on a good stiff toolpost and shove it in there, don’t be shy.

Curiously, I find that  “blunt” carbide can work well with negative rake on the really tuff bits.

it’s amazing stuff if your machine is stiff enough.

 

Whatever solution you find, carbide tooling will make life miles easier.

 

And don’t go buying expensive gear until you get a feel for the job, unless yer rich.

 

 

Edited By ady on 10/11/2010 11:23:04

[Anonymous]

Sounds like you’re way too fast on speed. Recommended speed for 4340 normalised, quenched and tempered, is around 30-40 feet per minute for HSS. For a 12mm drill that’s around 280rpm. Feed rate about 0.15mm/rev. A HSS speed drill should be fine, but you must keep the feedrate going. By hook or crook you’ll also need to get coolant to the drill tip. I’ve has no trouble drilling EN24T with HSS drills.

 

As ‘ady’ says, low speed, high torque (geared or belt drive head, no VFDs) and keep the feed on.

 

Regards,

 

Andrew

[Richard ParsonsParticipant @richardparsons61721]

 

The only way to drill such a hole is a G*N (I must not mention the name) drill. You can still buy these or you can make them yourself. They consist of a ‘D’ shaped hollow tube into which you pump oil and with a ‘Vee’ groove to take away the swaff an have a ‘Diamond (shaped) ‘flat’ bit fitted to the end. There s a very good book on the subject by W.F. Vickery called ‘Advanced xxxsmithing’ ISBN 1 873066 06 X, I think I bought my copy from Camden Miniature Steam (usual disclaimer) who regularly advertise in M.E.  I had another book which was confiscated which detailed everything including the oil pressures to use, speeds and feeds.  It came from the same source.  From memory with a 6mm hole the oil pressure will be quite high (about 600 psi)
My oil pump i got from a scrap yard for two pints of beer.  The rest of it  I made up from what eveer was to hand.  The tube I think I got from ‘Accles and Pollok’ in the U.K.

 Good luck and keep it under ‘their radar’

Edited By Richard Parsons on 10/11/2010 11:47:57

[Martin WParticipant @martinw]

Hi

 

I looked up GNU Drills on the web and there are several references including illustrations of the bits and systems used but mainly on U.S. sites. Another option is to search for ‘Deep Hole’ drilling which while the same is for the UK a more PC (not desktop) version.

 

Perhaps the ‘Government’ should give us back our guns and ban the car; logic is that drivers of cars in the UK alone kill 1000s per year and maim 1000s more but guns only ever kill a few at most; the saying ‘Licensed to Kill’ takes on a new meaning with driving.

 

Sorry about the rant .

 

Martin

 

PS

 

Late thought:-

 

Is there any mileage in regrinding the tip of a longish masonry drill and using that. I know that its been done for drilling very hard metals so may work for deep holes in tough metals.

 

 

PPS

 

The moderator will probably remove/edit this post as offensive/

Edited By Martin W on 10/11/2010 12:21:21

[PekkaNFParticipant @pekkanf]

Thank you all for insight. I’ll try to go slower and sacrify some drills and dignity.

 

I have read and paged of catalogs of the trough cooled drilI bits, but price is steep for few good holes. Dx12 seems to be achievable i.e 12*8mm = 96mm, that would be fine, but at price….and it would break my heart if that new expensive shiny drill would snap on my flimcy chinamade lathe.

 

I am aware of the mentioned technology, but it would seriously sidetrack me from building a spindle and would find very little use at my garage.

 

I have GHT:s book  “MODEL ENGINEERS WORKSHOP MANUAL” and there is a shor section on D-bits. I have never had success with these and I’m not yet desperate enough to jump on it first, but maybe I should check it just in case.

 

I wonder if tuned SDS masonry bit would work. Should I grind to D-bit aproximation or more of normal spiral drill? Any link/diagram etc?

 

Thanks,

Pekka

[Richard ParsonsParticipant @richardparsons61721]

 

PekkaNF –  try a ‘redesign’ Does the hole have to go right through? How about thick walled tube? There are many ways to kill a cat apart from drowning it in cream.

[GoCreateParticipant @gocreate]

Hi

I have done allot of drilling of En24T and found that cobalt HSS cuts very well and lasts but with rpm very low and highish feed rate by hand.

Dormer 135 deg split point about 10mm tin coated cut extreamly well with out a pilot.

Plenty of coolant applied.

For small holes <2mm ordanary hss was useless but cobalt hss no problem.

 

There are plenty cobolt hss or even better carbide drills at reasonable prices on ebay.

 

Nigel

[Richard ParsonsParticipant @richardparsons61721]

Get a squeezy bottle (wash up soap) add a length of plastic pipe say 4-6mm diam after drilling the width of the drill as a ‘peck’ Flush out by pushing the plastic pipe down the hole to its bottom and squeezing the bottle.  Catch the washings in a old tin and re-cycle.

Edited By Richard Parsons on 10/11/2010 17:35:42

[PekkaNFParticipant @pekkanf]

Thanks all,

 

Your advice will keep me busy some time….

 

I had an partial success with 10 mm Dormer  HSS A002 and Alpen HSS-Co drills. Not deep enough hole though. Dormer chompped away happily with 200 rpm and quite a large feed. Used some “manual dwell” on pecker it seemed to prevent jam-ups.

 

Maybe  I’ll invest to a slighty longer HSS-Co drill and try it out with the proposed plastic pipe trugh coolant. I have my reservations, I feel that chips will push it away, but it just might work.

 

I’m scared of solid carbide, not liking at all steep learning curve with it. Still always surpriced when I’ll chip off busines end of carbide insert lathe tool – mostly because too slow cutting speed.

 

There probably is no relatively cheap drill that would have trough cooling?

 

I tried one SDS+ mansory drill 8 mm and 100mm long (purrfect!). Despite it’s looks it cuts as long it has a pilot hole! Very tempted to try sharpening it, but I don’t have a foggiest idea to what form.

 

PekkaNF

[Tony Pratt 1Participant @tonypratt1]

As has been said decent HSS will do the job no problem but coolant and plenty of it is a must, you can get fairly cheap coolant pumps and tanks from the usual suppliers. Will a 12mm dia. x 60mm deep pilot hole be ok as you seem a little bit vague on exactly what you need?

Tony

[IanHParticipant @ianh]

I have recently had a bit of fun recovering a job which involved drilling into hardened EN 36B – my normal Dormer HSS drills wouldn’t touch it, it was like drilling glass. I bought a cheap solid carbide drill off Ebay (harryuk123 store) for just under £5.00 and it was a piece of cake. Don’t be scared of solid carbide.

 

Ian 

[BogstandardParticipant @bogstandard]

Maybe you could try these. I use them for anything that is a little bit hard or tough that tends to flatten off the ends of normal HSS bits.

 

The place is also very good for normal ground drills, and where I buy all mine in bulk.

 

Hardplate drills 

 

As you can see, in some of the larger ones, they do up to 300mm long.

 

Bogs

[PekkaNFParticipant @pekkanf]

Thank you, you have been most couraging.

 

I’m aware that there is quite a noticeable difference in machining this type of steel, some of the steels seem to easier to machine than the others. This tempered and pretty tough. I suppose same material could be bought soft too, but then still better would be free machining steel if it would do the job.

I believe these  bars are this one:
http://www.bohler-uddeholm.co.za/english/files/V155DE.pdf

I have this stock 4-6 meters of 16/20/25 mm and I’m trying to develop a feel how to use it. First thing I would like to make some small spindles out of it. Other parts would be made of very much easier material.

Ady, Andrew &all, you were correct about the speed. Normal HSS seems to be happier way below often quoted table values. Dormer A002 (HSS/Tin) drilled fine 10 mm dia hole with 200 rpm (Vc = 6,3 m/min). Only snag is that this is a standard drill and it will not make deep enough hole. Also delivering cutting emulsion and clearing the swarf is getting harder deeper it gets.

I have few short solid carbide twist drills and spot drills and they seem to work charm around 20 m/min Vc. So this material is good for work. But I have a flimsy lathe and I’m a little phobic of solid carbon. Also, I’m not sure of availability of longer drills and if it has trough cooling it would get pretty expensive.

* Immediate reaction for me is to find HSS-Co long drill and try if it will solve the problem.

* Ady, Richard Parsons and Martin got me interested on this idea of some sort of carbide tipped D-bit. I’m completely glueless on this one, but I’ll google it and shift trough some information, maybe there is something applicable. This probably would be good idea to try even if HSS-Co will get the work done.

All I need is pilot hole length of 10xdia and D is 5 to 12 mm, mostly I’m anticipating 8 mm and 10 mm pilot holes.

PekkaNF

[John OlsenParticipant @johnolsen79199]

You know you can extend an ordinary drill if you need to. The shank of the drill is not usually hardened, so you chuck it in the lathe (preferably a collett) and turn down a short length to make a spigot. Then you drill a matching hole in a length of stock of the same size or just under, and then silver braze the drill into place. This will not spoil the temper of HSS, and if you are concerned you can keep the cutting end of the drill cool by wrapping it in damp rag while you braze the other end.

 

Having got the hole as deep as you can with a normal drill, you then swap to the extended one.  The flutes do not go the full length, and must not be allowed to jam up with swarf, so you have to take a cut, withdraw, take another cut….A rack operated tailstock is a great thing. With this material the withdrawing would also be a great chance to squirt in some more cutting oil.

 

regards

John

[Author]

Posts