66 Rockwell (HELP!)

[Slick]

Alrighty then, I gotta pick you pro's brain:

 

Heat treated High Speed Steel, it's testing at 66 Rc. Anybody have any good suggesttions for Surface feet and chipload? I'm drilling, plunging, and pocket/contouring, trying that is, to machine out some wheel cutter blades around 0.110 thick. I have carbide insert drills, carbide and HSS end mills available. The largest I can go is 0.375 in diameter. Any good tips would be apprecited! (Oh boy)

[Tony]

I read your post 5 times

with my Jaw agape!

66 rc!what? It Must be T-15 or Cpm 10 v.

I would Wire cut or grind it.

[Guest CNC Apps Guy 1]

Here's a tip, buy some Kobelco(sp?), OSG FX Series, Sumitomo ZX Series or RobbJack Die Mold cutting tools. Done even mess around with any other $#!+!!!!! You'll save yourself tons of time and wasted energy.

 

RPM???? How much you got? Chip load? about .0005 to .0015 depending on conditions. Use Airblast NOT coolant.

 

There's my .02¢ from my experience cuting 60 Rc.

 

HTH

[Nicholas Anachasian]

I would start over... rought it all out before heat treating it

[TheePres]

Many years ago, an outfit had me take a pre-employment quiz.

One of the questions:

Give feeds and speeds on cutting 55 rockwell(steel), using a .500 HSS endmill.

Supervisor told me afterward that i was 1st person to not give some numbers. My answer being "Good Luck".

[Greg Williams]

Slick,

 

I have machinied loads of this stuff. We use Prototyp and OSG Ultra FX coated carbide for roughing and CBN for finishing. Don't even bother with anything else as you will be wasting your cash.

 

[CNCme]

DuuuuuDE,

 

Nick is right, rough it out, leave grind stock

.003 to.01 ( even if you dont grind )

Harden it, draw it down to temper it

(otherwise it will be very brittle)

and then grind or attempt to machine to

finsh.

 

I've got to say, coming from the "old school "

The basics need to be resurrected...FAST...

OH BOY

 

By the way, tool steel Should be drawn to 63Rc

max...any reason for 66rc...oil or air hard...??

 

HTHeals

 

Tonyg

[mold100]

alrighty, the world hasnt ended,I cut D2 at 62-68

Rc.O.k. tooling is your biggest issue.Also what kind of rpms and feed can you run.I dont rough to much of anything before heat treat any more I can cut most of just as fast after.OSG is your best bet dont use anything with a sharp corner and stay away from any sudden moves youll want everything (tool paths) to flow nicely with no corner bangin.A good example is I cut last week

M2 at 64 RC a stamping cavity with an OSG maxcarb 1/4 ball,I found it to cut best using surf pock rough morph spiral with a helix entry 14,000 rpms

105 ipm at .013 step down and .024 stepover.cutter

roughed for about 40 minutes removing quite a bit of steel.No Coolant,In the hard world coatings

can make or break a delivery.Just a semi educated

$.02 There are other tool manufacturers than osg,they will tax the hell out of for cutters.

[Jack Mitchell]

Slick,

 

You are out there, in the grey area of Machinery’s handbook (ever notice how incredibly generalized feeds and speeds have become in the last six issues?)

 

James – I’m really impressed!

Greg – Ditto.

 

This man is attacking the hardness approaching that of a file, the ones we use to deburr our parts! Some would say that experience is a good lesson or education. – Slick, you’re about to enter this realm.

 

Greg has got an ultra valid point with CBN – your going to balk at the cost of these tools, you really need to ask your supervisor the following – do you want me to do this job or do you want me to dick around with it! – Drop the cash, lose your xxxx, and try to smile when you say – I just machined an impossible situation.

 

James approach is quite valid. You’re going to consume some expensive tools here, no matter what the attack. (Sometimes we really don’t have any choice when it comes to machining a virtually impossible task) but hey, this builds character.

 

I have deliberately consumed tooling (1/32 destroyed through light cut layered passes) – of course, the tools become reground after the abuse and live a happy and healthy life as stubby cutting tools (my personal fav, as these will soon become yours).

 

Please let us know your attack, your result, and your general demeanor after completing the challenge.

 

Hey Corey – just caught your reply the moment that I posted – looking good!

 

Good luck and good grief, Regards, Jack

[Jack Mitchell]

Corey,

 

The .013 depth of cut looks a little aggressive, but hey, who am I to question a professional?

 

Slick, please heed the advice from Mold100 – he is an expert at EDM and a pretty good toolmaker besides. (Still owes me some beers, I might add).

 

I still disagree with the depth of cut, yet, I am in total agreement with the avoidance of the sharp cutting edge.

 

Slick, it’s really your call on this one – for we could all eat crow, theoretically that is. - You’re the one that’s going to perform this miracle (please do not disappoint your supervisor, or worse, the rest of us in this fun-time forum.

 

As Emeril says, let’s kick it up a notch - BAM!

 

Regards, Jack

[Guest CNC Apps Guy 1]

I'd machine that sucker at full hardness too! Roughing it before heat treat is for wussies! It's a very delicious cut when using the proper tooling. Just use a foxtail to sweep off the chips, DON'T use your hands, it's like grabbing hold of a porcupine!

 

Greg, so CBN is the ticket eh? I've only used it for Hard Turning not milling and it worked awesome cutting 4130 Rc 52 ( I think, it was a while back). Looked like there was a fire in the machine, you could just see this orangish glow out of the window. It was a beeeeeeuuuuuteeeeeful sight!

[savtav]

James,

 

Your Qoute is

 

I'd machine that sucker at full hardness too! Roughing it before heat treat is for wussies!

 

just a curious Qestion James. How to you tap a 5mm blind hole and drill 1mm holes at 66 rockwell without breaking the tap and drill

 

i know what i will be doing first.

[Guest CNC Apps Guy 1]

Well..... I've never encountered that situation but if I had to take a guess, I'd probably use ceramic drills and a threadmill.

 

But, if the sizes I needed to drill and tap were not available, then I'd probably look at EDM.

 

HTH

 

[ 12-06-2002, 02:55 AM: Message edited by: James Meyette ]

[Greg Williams]

Slick,

 

I little CBN advive,

 

Cutters:

In the past we have used Sumitomo CBN Ballnose cutters with great success, However recently we have changed to a local supplier as his product is a little better for our current applications. Start at around 100mmin cutting speed (Remember to work out this cutting speed from the efective diameter not the actual diameter for ballnose cutters). Feed at 0.025mm per tooth per rev and take no deeper than 0.1 cuts for finishing.

 

Machines:

To have any real success at this you need to have a machine tool with at least 15K spindle, There needs to be less than 0.005mm runout at the cutter. The machine will need to have a control with good look ahead and feed control functions so that there is no dwelling at any point in the toolpath, If dwelling happens the cutter will not last (ouch that costs). The toolpath should have no sharp corners or plunging and of course use air not coolant.

Good luck and let us know how you go.

 

[chris m]

This sounds like a tough situation and as this is not my area of expertise I will bow before the gentlemen who obviously have good experience; I just had to say that this line:

quote:

---

My answer being "Good Luck".

---

will definitely make it to my one-liners list... that is just beautiful!

C

[mold100]

Jack, .013 is just just over 5% of diameter, It can handle 10 to 12% in 58-60 so I cut it in half for a tougher mtl,.We will someday settle the beer issue,Hows the sausage industry these days.

 

About drilling and tapping call OSG and they will help you out on this.I have seen them demo 10-32

tap in 62 Rc d-2.Hardest I have done is 56-58,and not alot of it,I still prefer to burn threads if there

isnt alot of them.

[Tony]

I machine S-7 around 54/56 rc range

and 0-1 at 60 rc "Hard milling" is away of life

these days.

Here is a tip that an old timer told me:

Keep the cut Dry Use only Air (Like everyone else said)

Don't even touch the Surface with your hand

The oil on your skin will get on it (You can see

it). And your carbide will Deflect up over it.

 

I tried diamond tools they work well.

(The mfg. let me try them....when I was done

He took them back!There that Expensive!)

 

[ 12-06-2002, 09:39 AM: Message edited by: Tony ]

[Slick]

Alrighty! To start, my floor supervisor and I (Roomates, and old friends) are totally pumped to try this. We have been told there are other options, but as I can tell by all of your statements, it's all about doing the things they say can't be done, and it sounds like most of you were told that, and proved 'em wrong!

So I want to sort out some facts really quick, before I get the ball rolling.

1. For sure OSG cutters (I'll spend the cash).

2. No coolant, just air. (Air mist, or just air?)

3. Surface pocket morph spiral out the material, 0.013 depth, 0.024 stepover as a base to start, all smooth moves. (Imagine a 0.110 thick solid wheel. I need to cut it out to look like a "Mag wheel". Use surface pocket to finish the walls as well? There is no taper to the walls)

4. Am I calculating my diameter correctly at 0.013 depth of cut: 0.110 diameter?

*5. This one is the clincher... I'm dealing with either 10,000 RPM on machine that isn't very rigid. Or 8000 RPM on a rigid machine. Or should I bag it. (I'm thinking if the Surface feed and chip load match, it shouldn't matter should it?)

All in all, I really want to cut this, let me know what you guys think.

When it's all said and done, I'll be buying cold beers for everyone.

[Jim Whipple]

quote:

---

2. No coolant, just air. (Air mist, or just air?)

---

No mist....just air!!

Jim

[mold100]

Slick,

technically for your application your not going to get the rpms you should really be at.Stick with air only

high pressure.Other than the rigidity factor how well does your machine handle fast feeding?What are the machine types.Gouging without suffient look ahead decel and accel is a factor.

 

I learned something awhile ago that I find holds pretty true for real hard cutting

things to look at without any one of them your missing a link, you can get by but it isnt safe.

 

1) Machine tool-speed, rigidity, CONTROLLER

2)software-Mastercam you covered there

3)Employee-You,ve got us,besides trying new stuff is the key to moving forward

4)Tooling-Very important it is used correctly,especially at its cost.

 

You said something else that I didnt like vertical walls-YUK.

[Jack Mitchell]

Slick,

 

Give it your best shot.

Do not entertain the feed hold button under any circumstances.

If this is a solid, then ramp into the workpiece - the dull orange glow will warm your hands quite nicely (please avoid the touch as suggested).

If your going with a .110" dia then order at least six cutting tools; do not forget to grind a .01" ~ .02" radius on these tools.

Stay pumped, especially if the going gets tough.

 

Regards, Jack

[Mick]

I few months ago, I cut through a block of 60HRC steel, with a 6mm endmill, 10mm wide, at 12mm depth, in one cut. The block was 60mm wide, and I did it with using a "trochoidal" cutting motion. Unforunately, Mastercam didn't have the right motion, so I had to draw the centreline of the cutter path, and switch compensation off. Worked a treat though.

If anybody is interested, I'll put a sample file up on the FTP.

[Jack Mitchell]

Slick,

 

I’m sorry, but this application is still haunting me.

 

The economics of this task reeks of producing the male electrode and boiling it through the rough with graphite and finishing with copper perhaps.

 

The time & effort spent on the electrode method will justify the cost; the opposing argument of hard milling is highly speculative and certainly cost prohibitive. ~ The gain is the education or personal satisfaction.

 

Basically, this job may take 3 hours, may take 20 hours of fighting the laws of physics, or may never occur for all the time invested.

 

Nobody here will judge or consider this a failure – please reconsider the attack, for nobody would argue that EDM is a solid solution given the 66Rc that you are presented.

 

Basically, it all comes down to cost – what is the quickest, most efficient method to make this part, Etc!

 

Regards, Jack

[Guest CNC Apps Guy 1]

quote:

---

Basically, it all comes down to cost – what is the quickest, most efficient method to make this part, Etc!

---

That would be machining it out. EDM is a HUGE expense and not necessarrily warrented from the limited information we know about the part.

 

JM2C

[Jack Mitchell]

James,

 

No offense, for I beg to differ, EDM costs are very much affordable as well as commonplace around the area slightly north of the 42nd parallel.

 

If given the choice of milling your name into a fine tooth flat xxxx file (.01” below the tooth form) or burning this in via carbon and copper electrodes, would you still argue this point?

 

My observation is based upon 66Rc, this is virtually impossible to machine when the tools recommended top out at about 50~58 Rc, there is an outside chance that CBN & diamond could effectively render a satisfactory result – economics would prevail if the cutting tool costs exceeded $1000.00 .

 

Please don’t get me wrong, I am not challenging you or anyone else for that matter.

From a shear economics viewpoint, I couldn’t expect a reasonable cost/result solution with this unusual application.

 

Hard milling 48Rc, 55Rc, and even 58Rc is nothing new to many of us; 66Rc is not as common a hardness to deal with and quite honestly I have never personally machined anything at this hardness without a grinding wheel.

 

Regards, Jack