[ncttech]

Making some parts that call out D2 tool steel, heat-treated to 58-62 Rc. Two holes are .2362" +.0005"/-0, and one is .3740 +.0006"/-0. There are also two threaded holes. The hole spread is held +/-.0008". What's the best way to do this. Machine in soft state then use carbide drills and reamers? What about the tapped holes?
Thanks

[DareBee]

Tap the holes when soft and jig grind the other holes after HT

[handlewanker]

What's the job worth?

It might not be worth doing for all the fuss and bother.

If the job is already hardened steel, someone stuffed up or it's an add on, re-work, whatever.

You could get them spark eroded and wire cut if it's that hard, and the holes honed to size.
Ian.

[underthetire]

Is that true position of .0008"? Material will move after heat treat, so holes will need to be finished after hardening. Grinding or edm.

[handlewanker]

If you are going to make the job from "soft" tool steel and then harden it, you will have to grind the holes out to get a positional tolerance of .0008"........you can't hone them out as the hone will just follow the bore wherever it is after hardening.

With tolerances like that you must have quoted a high price to get it, otherwise you'll end up paying the customer so you can do the job.
Ian.

[juergenwt]

D-2 does not move in Heat Treating.

[Geof]

D-2 does not move in Heat Treating.

Actually while most most tool steels will grow between about 0.0005" and 0.002" per inch of original length during heat treatment, due to the changes in microstructure, D2 is a bit anomalous and under some circumstances can shrink. This occurs when the austenite to martensite transition does not go to completion during the (air) quenching, possibly because the steel was held either too long or at to high a temperature. The martensite transition can be pushed to completion by cryogenic treatment followed by tempering.

[zero_divide]

Using a carbide tialn coated drill you can drill 60rc hardened D2
I used Ultratool slow spiral stub drills.

Going around 1500 rpm and 1.5 ipm
Then follow up with a reamer. Best if coated as well.

The tapped holes should be done before HT. I dont think i ve ever seen tight tolerance on position of tapped holes.

If position is important you may be able to threadmill the holes if they are shallow.

I have tapped 50-55rc steel before using a powdered metal tialn coated tap from osg i think.
Not sure if you can do it to a 60rc steel. Carbide tap may be your best shot.

And yeah D2 may warp and twist during HT

[handlewanker]

Hmmmm, going back to post # 1, the tolerance on the "hole spread" is almost +/- one thou.....that's pretty generous in general toolmaking terms, but drilling and reaming will not give you the required end product.......drills will wander a smidgeon and reamers will just follow, and honing to size after hardening will not work.

The option to make before heat treatment means you can work in the soft state, first drilling and tapping, so....... you would drill and tap first, then drill undersize for the tolerance holes.

After heat treatment the holes must be repositioned relative to the block edge dimensions due to having acquired distortion from the heating process.

In this case no dimensions are given, which means they MUST have a general tolerance on the drawing for all untoleranced dimensions, and that could be as much as +/- .010"for dimensions to one decimal place...IE edge to centre of the holes 2.1"......or 2.10".....or 2.100"....the tolerance would alter accordingly unless specifically noted, as in the hole spread of +.0008"/-.0000".

The problem now is how do you open up a fairly rough hole firstly in 2 planes and secondly relative to one another?

You could set up the block in a vice on the mill and attempt to grind the hole out with a diamond point in a boring head, but as you would be working at relativel low revs ......max about 7,000 rpm, this would not get you to scratch much off the inside diams without wearing the diamond point away.....it breaks down more from pressure than wear.

You could mount a high speed die grinder in an adaptor in the spindle of the mill, ( spindle in the locked position), mount your job on a rotary table or dividing head in the vertical position, and by rotating the job against the high speed grinder diamond point, progressively grind the hole out....very slow and extremely labour intensive, and needs experience.

The big question is HOW DO YOU LOCATE THE CENTRE OF EACH HOLE RELATIVE TO THE BLOCK AND EACH OTHER?

That answer is by using toolmakers buttons.

Toolmakers buttons are small accurately hardened and ground on diam and ends steel bushes, about 1/2"diam X 1/2"long with a 3/8" hole through the centre, and they come with a socket head cap screw and a washer.....in sets of three.

The method is to attach the "buttons" one to each hole with the cap screw and washer so that they can be moved around on the hole.

That's it.......you attach the buttons to the block on each hole, but with a longer cap screw and a washer and nut on the back of the job, and by using whatever method you have, either a height vernier, gauge blocks etc, on a marking off table, surface plate or similar accurate flat surface to set up the distance from the edge of the block to the face of the button in two planes to give you a pseudo hypothetical hole in space, represented by the centrality of the buttons.

When you set the block on the rotary table, (or in the 4 jaw chuck in the lathe if that's your preference, but exceedingly difficult to maintain squareness in that many planes), you use a dial indicator to set the spindle concentric to each button in turn.

The job must rotate on each hole position.

The buttons will give you the positions to whatever accuracy is required, and the die grinder with diamond point will give you the hole diam.

No mention has been made of the thickness of the block, so assuming it is 1"thick for example.

As the holes are only approx 1/4" and 3/8" diam, the diamond point will not go very far into the job, maybe only 3/8"at most, but it will give you a pilot hole position and diam accurately that you can then hone out the holes to size.

If the material is only 3/8" thick at most, the grinding point will do the job.

In my opinion, no matter how thick the material, the job should be EDM'ed for the toleranced holes only, as this would give you the required accuracy and tolerance in one go.

What puzzles me is why this job was taken on in the first place if the method of production was unknown.

Looking at the CNC aspect for a solution, once you have the block fixed in your vice or on the table, you could grind the bores out with the die grinder held vertically in a bracket attached to the spindle (which does not rotate)......but the material has to be thin or further honing to size would be required to get the full depth.

The X and Y axes do all the circular work and the Z just plunges the point in and out......backlash in the X or Y axes is not an option to tolerate.

Hard machining also comes to mind, but as I have never done anything of that nature I can't comment.
Ian.

[juergenwt]

Wow handlewanker - you are taking me back some years. Tool buttons work.
However, we have been using D-2 on many of our dies and hardly ever did we need to rework Dimensions after HT. Granted, it does happen, but very seldom and than very little. A good Heat-treater can bring it back for you. If we had a die block with holes spaced out over several inches with a very tight tolerance between holes and no clearance required (line to line) condition between punch and die, than we would leave .002 to .003 grinding allowance. Not more because hardened D-2 is not easy to grind. Next station - Jig Grinder.
If the holes in the die block were still within the required tolerance than we would just adjust the dimensions on the punch holder to achieve a line to line condition.

Check here: http://buffaloprecision.com/data_sheets/DSD2TSbpp.pdf

I would no recommend drilling holes into 62Rc D-2. It can be done with carbide but I don't know how precise. Reaming???? Tapping -NO.

[handlewanker]

Hi, anyone who designs the job to be drilled and tapped after hardening had better go back home and take up another profession.

The only case would be if you had EDM and wirecutting equipment, which work better with steel in the hardended state, but given the choice, soft toolsteel is the way to go.

BTW Juergen, did you ever use a "sticky pin" for picking up your co-ordinates when milling or drilling?
Ian.

[RICHARD ZASTROW]

I both agree and disagree with juergenwt. We made semi-finished rotary dies to size in the bores. They were then hardened, quenched and crio-treated to -300 deg.f to stabilize them. The bores would shrink a few tenths. The bores were then finish ground to size. So they did shrink in the bores and grow on the O.D.'s, but very slightly.

The best answer above for hole sizing: Juergens jig grinder recommendation. We use that method/process for spindle bearing bores with tolerance total envelopes of .00018" and alignment of "dead nuts".LOL

BTW, nice to see somebody still remembers tooling balls!!!

Dick Z

[handlewanker]

Hi Dick, the fact that, as you stated, the bores were ground after hardening means they can be "relocated" due to any shift that might occur.......this is similar to boring after drilling, (in soft materials), which will give you the exact hole position no matter if the drill wanders.

In all cases I have experienced, any subsequent process that is affected by hardening is corrected by grinding to position or size.

I don't think my foreman would have smiled on me if I had made a part to size and stated that after hardening it would "probably" not vary in the dimensions...much.

There is a very real problem in this job as the holes are so small.....almost 1/4" and 3/8" diam, depth unknown, and using mounted diamond points also can lead to bellmouthing of the bores at the entry point.

About the only process that can produce a position and size when hardening has occurred is an EDM or a wirecutter as they can work without being affected by the hardness of the material.

In my previous job I worked in the metrology dept and we had key profile gauges made by the wire cutting process, completely from the hardened blocks of steel and with no further rework.

The keys were for pin tumbler type door locks and were for gauging the profile of the key blank, looking end on.

Previous to this the gauges were made by hand in soft tool steel, in two halves, and the profile of the keys was formed in each half before being hardened and further reworked to achieve the profile tolerance using a projection chart for contour comparison.....the gauges being fastened together with dowels and cap screws....very labour intensive.

Wire cutting not only gave us the gauges more accurately, but also subsequently caused a down sizing of the tool room as practically all tools were bought in from firms who had the EDM and wirecutting equipment and people who knew how to use them.

Our firm in their infinite wisdom, initially invested in an EDM and trained one man to work it, and as a Wire cutter was in the region of $150,000 decided to downsize the toolroom and outsource all further tooling.
Ian.

[Sho409s]

We would run that in a mill and leave the holes something like .003 small per side. I've not heard of tapping hardened A2/D2 we would scrap that part, and never heard of it being required as the bolt will have a clearance hole on the other side anyway. Finish it off (likely grind it) and send it out to heat treat. (Likely grind it again then) Put it back in the mill and mill the holes until you get what you want, and that tolerance will not be easy. Hard cut is not very nice to carbide end mills but we do it often in cases like this. If the holes were through then of course we would just do start holes and wire burn them. A2/D2 does move in heat treat but not a lot, most issues are plates that vary by .005 in say 10" when they were ground flat before treatment. Something more square and thick moves less. I doubt hole placement or size under 1" is going to change much, but when you talk tenths then it can be an issue. You can machine hard steel but its a pain, and lots of pain on the cutters. We save used inserts for projects like that, really bad inserts. Usually we only have to hard cut new stuff when there is a stepped or blind hole you can't wire burn. There are special end mills that work better for some hard cuts, but we seem to only bother with those for 3D cuts. We use full liquid cooling and all carbide EMs for something that small. But taking a few thou off is not that bad, taking .100 resharp is a lot more work. There are places that do other EDM and can do blind holes, this place only does wire. The problem with milling the hole is likely the precision of milling the hole and not burning it. CNC mills are great but getting under .001 tolerance is not something we try to do with them very often, or at least the ones we have. Most things are heat treated so its pointless anyway.

[juergenwt]

Handlewanker - I know exactly where how you feel. We went from 38 Tool and Die makers when I was the Foreman down to a total of three plus one Wire EDM Operator. But the rest of the plant was down sourced by the same ratio. Glad I retired and now work as a consultant for the same company.
Sorry I have never heard of a STICKPIN. We always had Jigbores and Jiggrinders. Pls. explain.
As far as Wire EDM goes - I can tell from my experience in Die work. We were one of the first companies to use the AGIE Wire EDM. It was a long learning process.
One thing should be mentioned here: after cutting a Die from A-2 or O-1 or D-2 or any other tool steel from a hardened block there is one thing you need to do: send the die block for a double draw. Most people do not know that during EDM a very hard surface about .0002 deep forms on the cut and if you don't double draw there is a good chance your die will crack in any sharp corner.

[handlewanker]

Hi Juergen.....a stickypin is a small piece of Plasticine, (which is a form of modelling clay used by the children etc), with a pin sticking out of it.

It is the equivalent of a set of Wigglers or edge finder set, where you have an edge finder, per se, and also a number of other items, one of them being a short pointed rod that fits in a small collet holder and is used to locate a marked off centre point before drilling etc in the mill and also a drilling machine.

The method is to attach the Plasticene to the end of the end mill, slot drill or centre drill, and with the spindle running use the edge of a ruler (or your thumb nail) to "true" the point of the pin, as it is running eccentrically when first attached to the tool point.

NEVER attempt to set the pointer of a Wiggler true with your thumb nail.......use the edge of a ruler.

The reason is this, when the Wiggler point centralises it only requires a further bit of pressure for the point to flick out sideways and whirl in an arc about 75 mm diam and if you've used you thumb nail to true the point the whirling disk of the pointer will lacerate the back of your hand like a razor......seen it happen, be warned.

The pin in the Plasticine will centralise with a bit of side pressure from the ruler, same as the pointer in a Wiggler set, but unlike a Wiggler pointer will not flick out sideways if you put too much pressure on it to centralise it, so the thumb nail truer upper is OK.

My father showed me that trick when I was apprentice and worked with him on the mills learning the tricks etc.

I still have the same ball of Plasticine with a pin that my father gave me in 1960, and it was a common piece of "equipment" for many machinists, and if you looked in their toolboxes you'd often find one stuck to the inside of a drawer.

When you have a drill set up in a machine you can just attach the "stickypin" to the end of the drill, true it up, and locate the exact centre of the cross lines for the hole you want to drill in a few seconds without removing the drill and setting up the Wiggler.

Mostly, you'd be locating your co-ordinates from the zeroed face of your machine vice on a mill or with an edge finder for side location, but when a job has been marked off, like for a rough casting, the hole locations or centre lines are frequently pre marked with crosslines and a circle, (with 4 dots)

BTW, when they down sized the tool room, part of the grand plan, I also got put out to grass permanently at age 60......never worked full time again, and was in the position to obtain a Bridgeport mill, one of six which were being sold off, and used it to carry on with other pursuits.
Ian.

[Sho409s]

We have used tooling balls to locate things, last time we made an angled jig to mount a piece on and got a zero with the balls.

Our shop will not touch something without CAD, so locating a marked point is not something we do. It better be in a program unless its something simple plus if its made to CAD there is no question about if its right or not. We do make our own CAD off prints for a few things, but manual stuff is so slow I don't like doing it lol...but never said I was speedy at it either.

[handlewanker]

Hi, there are many ways to get from A to Z........if you forget any of them you limit your options.

One of the many reasons so many CNC dominant "machinists" have problems with set-ups.....they just don't know.

In the present day CNC atmosphere, if you haven't familiarised yourself with current technology, all the old way experience will not benefit you.

Having been retired for 10 years now, I realise that engineering marches forward at such a rapid pace, just knowing what the new methods are is a full time job.

I read somewhere here that the current CNC method, where metal is removed from a larger piece of metal, is already being overtaken by 3D printing which will make cutting metal obsolete as opposed to adding metal to build a part that can't even be made using normal procedures, like casting, forming or hacking out of a block of material.

This does put pressure on the workforce to adapt to new ways or simply join the job queue for that old fashioned job nobody pays good money for anymore.

We are wrestling with the problem of producing a tool that requires heat treatment to produce a production part, whereas when 3D printing becomes the prime producer of the production, the tool making industry will disappear altogether.

It becomes very hard to imagine that a technique can be so completely overtaken by another technique within the lifespan of the average person.

Eventually 3D printing will become obsolete when Nano technology and artificial intelligence combine to enable particles to be given a unique identity and have them align themselves within a structure as required for a particular part.......similar to how the Human body is made from cell structure alignment and combinations........I'm going to go back to the Bible to find out how it was done originally.....LOL.

It won't happen today, and it won't happen tomorrow, but it will happen.......parts are already being made as a normal process with 3D printing, it's just another evolutionary step.
Ian.

[victorofga]

threads can be made before hardening and positioned holes can be recut with wire edm.. thats the ""normal"" way with dme ...

it sounds weird making thread in hardened steel... not because it would be impossible, but because it makes unnecessary cost..
but we dont know the whole story..

[handlewanker]

Hi Vic, I don't think the original question mentioned the material state, just the need to have two tolerance holes and a tapped one, and the need to harden it.

The question was a regular toolmaking one, so I expect the poster has decided on a method fuelled up with all the expertise we've supplied.

A lot depends on the availability of the solutions posted previously, and while wire cutting is one, if it's not available the next method opens another can of worms.

I doubt very much that anyone would want to work on a hardened block of tool steel, no matter what the equipment, when the soft approach is not stretching the envelope.

It's a different matter when a tool rework is needed and you cannot anneal the whole block just to rework a hole or two.
Ian.