Face Milling Cobalt HSS @65 HRc

ADFToolmaker · Jan 10, 2017

We have a repeat job we normally complete by surface grinding. We are looking at ways of improving our output and are trying milling but would appreciate pointers from anyone who has been doing it already.

We are using a mitsubishi ARX round insert tool, using MP8010 grade carbide. It cuts it but insert life is short. Seems to be chipping rather than flank wear suggesting our DOC is too deep? We have tried DOC from 0.010"-0.020", around 0.002" feed per tooth and 320-480 fpm surface speed. We are making incremental gains as we change parameters but are going through the inserts too quick to be able to justify carrying on. Any suggestions welcome...

ManualEd · Jan 10, 2017

Seems like a good application for a whisker re-enforced ceramic inserts?
Or maybe a ceramic or carbide end mill?

ADFToolmaker · Jan 10, 2017

Have not tried ceramics, I kind of figured they were more for fine finishing, we have to remove 0.060"-0.080" of some faces.

ManualEd · Jan 10, 2017

ADFToolmaker said:
Have not tried ceramics, I kind of figured they were more for fine finishing, we have to remove 0.060"-0.080" of some faces.

Theres tons of milling Inconel blisks with ceramic end mills on you tube so I imagine it should work. If you can run twice as fast, half as deep, and get better tool life it might be worth a call to a few tool suppliers.

Orange Vise · Jan 11, 2017

What's the size and shape of the workpiece?

Ox · Jan 11, 2017

Never done it, but that SFM seems awfully high for hardened material eh?

Greenfield may have some ceramic inserts that will fit in there.
Especially if round.

-------------------

Think Snow Eh!
Ox

Rstewart · Jan 11, 2017

Why are you not using CBN tipped inserts? This is what they're made for....

ADFToolmaker · Jan 11, 2017

Ox said:
Never done it, but that SFM seems awfully high for hardened material eh?

Greenfield may have some ceramic inserts that will fit in there.
Especially if round.

-------------------

Think Snow Eh!
Ox

ThanksOx, I don't think Greenfield are represented in this country but maybe I can contact them direct.

Agreed the SFM sounds high but we are not experiencing flank wear, the edge holds well for a time then chips without warning. Also, since we are taking small DOC with a toroidal cutter the effective cutting diameter is smaller than the cutter OD, so we may not be that far out.

ADFToolmaker · Jan 11, 2017

Orange Vise said:
What's the size and shape of the workpiece?

The work is actually a series 9 of 1/4" thick parts stacked in a vise so all the edges get milled in the same setup. Come to think of it, maybe that's part of the problem, the cutting edge is crossing a boundary between two parts. I have had problems with this before drilling and reaming hardened H13. If I could get more inserts (only half the suppliers are open this time of year here) I would try machining them one at a time.

Monarchist · Jan 11, 2017

ADFToolmaker said:
The work is actually a series 9 of 1/4" thick parts stacked in a vise so all the edges get milled in the same setup. Come to think of it, maybe that's part of the problem, the cutting edge is crossing a boundary between two parts. I have had problems with this before drilling and reaming hardened H13. If I could get more inserts (only half the suppliers are open this time of year here) I would try machining them one at a time.

You might have a better setup than you realize. That 'boundary' is also a source of support, one disk to the next - HSS Cobalt being prone to nano-fracturing at sharpish places when unsupported.

Wonder what would happen if there was a thin sheet of steel between each member of the stack?

Meanwhile 'wet' or coolant-supplied grinding has been the proven low-damage way to shape HSS-Cobalt since powder-metallurgy big-bang.

Is there room for useful gain in throughput of your abrasives techniques?

Bill

mjk · Jan 11, 2017

add a sacrificial piece of softer material on each side?

Monarchist · Jan 11, 2017

mjk said:
add a sacrificial piece of softer material on each side?

As said - steel. Not sure I'd consider copper, brass, aluminium, or the plastics.

ADFToolmaker · Jan 11, 2017

Monarchist said:
You might have a better setup than you realize. That 'boundary' is also a source of support, one disk to the next - HSS Cobalt being prone to nano-fracturing at sharpish places when unsupported.

Wonder what would happen if there was a thin sheet of steel between each member of the stack?

Meanwhile 'wet' or coolant-supplied grinding has been the proven low-damage way to shape HSS-Cobalt since powder-metallurgy big-bang.

Is there room for useful gain in throughput of your abrasives techniques?

Bill

Thanks Bill, There certainly is room for gains in our abrasive technique. We are only using aluminium oxide wheels at the moment. An SG wheel would surely make a difference but 350 dia wheel is a step up in cost and has a long lead time here. We are a long way from having large enough orders to justify a CBN Wheel.

mjk · Jan 11, 2017

to clarify my comment
At each side of vice jaws

Monarchist · Jan 11, 2017

mjk said:
to clarify my comment
At each side of vice jaws

Counterintuitive - so long as the vise is not contributing to damage, you don't want to introduce ANY movement on this sort of material.

I suspect milling - no matter how well done - is not even assured of being good enough for no-rejects final-final, vs 'best current practice' grinding.

That the OP reports the amount of work cannot easily support uber-grinding methods or experimentation, tells ME there isn't a whole lot of time, money, and rejects to play with sorting out which milling techniques work best, either.

Rough mill, finish grind might justify the double handling, keep rejects down, quality up and enjoy higher throughput. But only if there is a lot of stock to be removed.

Bill

Jashley73 · Jan 11, 2017

I work for Seco, but this is what I would consider, at least by your posts thus far...

If there's any volume to this at all, I'd be looking into CBN milling tools. They will come with fall-out-of-your-chair pricing, but you should get good tool life, and productivity. One technical tip with CBN milling, is that we recommend conventional-milling, rather than climb-milling. Conventional milling will create more heat as the cutter rubs it's way into the cut, which is actually preferred in the case of CBN. The thought is that the extra heat helps the chips become more "plastic" and translates into less flank-wear on the inserts.

If CBN isn't an option, we have a "MH1000" carbide grade that is specifically for hard-milling. I would try this in a high-feed style insert, even though you might not have the need for true high-feed rates. The high-feed toroidal geometry will help protect cutting edge, and give you security. (Your round insert does this too...) We have a "High-Feed 4" insert with 4 cutting edges, available in this grade.

I would also look for the highest flute-count possible for the cutter body. The thought is, that when feeding the tool based on teeth/revolution as you should, the cutter will complete the linear cut, with fewer revolutions. This means that each insert has to enter & pass thru the material less. For example - If you switched from a 6-flute cutter, to a 9-flute, then each insert only has to cut 2/3 of the material, which gives each insert 50% better life. That translates into 50% more parts before having to change the inserts, not to mention the extra productivity.

yardbird · Jan 11, 2017

Monarchist said:
Meanwhile 'wet' or coolant-supplied grinding has been the proven low-damage way to shape HSS-Cobalt since powder-metallurgy big-bang.

Is there room for useful gain in throughput of your abrasives techniques?

Bill

That's what I've been thinking all along. That's pretty hard! How good of tool life/wear could one hope for machining that stuff? Seems there a trade off and this may be it?

Brent

ADFToolmaker · Jan 11, 2017

Monarchist said:
Counterintuitive - so long as the vise is not contributing to damage, you don't want to introduce ANY movement on this sort of material.

I suspect milling - no matter how well done - is not even assured of being good enough for no-rejects final-final, vs 'best current practice' grinding.

That the OP reports the amount of work cannot easily support uber-grinding methods or experimentation, tells ME there isn't a whole lot of time, money, and rejects to play with sorting out which milling techniques work best, either.

Rough mill, finish grind might justify the double handling, keep rejects down, quality up and enjoy higher throughput. But only if there is a lot of stock to be removed.

Bill

You are pretty close to the mark Bill. The job is worth thousands, but not tens of thousands, but is growing. We would always finish grind, some of the tolerances are 0.002", and it is that that our competitors have struggled with.

I am looking at milling as a material removal process only. By most folks reckoning we are outside the realm of milling, and that could be true, but during my career milling H13 @52-54 HRc was unthinkable, at best experimental, yet today we do it daily without a second thought. If what we want to do is feasible, someone on this forum will likely have the info about it.

Monarchist · Jan 11, 2017

ADFToolmaker said:
You are pretty close to the mark Bill. The job is worth thousands, but not tens of thousands, but is growing. We would always finish grind, some of the tolerances are 0.002", and it is that that our competitors have struggled with.

I am looking at milling as a material removal process only. By most folks reckoning we are outside the realm of milling, and that could be true, but during my career milling H13 @52-54 HRc was unthinkable, at best experimental, yet today we do it daily without a second thought. If what we want to do is feasible, someone on this forum will likely have the info about it.

Been mentioned, has it not?

Inco and Hastel uber-critters where ya practically has to keep a ration of Kryptonite under the sump to make the buggers cooperative...

Mind - some folk are also working VERY high cost goods, and have different economics by perhaps a full order of magnitude than you might enjoy.

All the best with it!

Bill

onecut · Jan 11, 2017

Im only guessing but have m/cd some very tough materials in the past,My first thought was that will be very tough so if I was using a 4ins face mill,I would attempt about 50revs and 1.5ins feed using a cast iron insert with coolant.The speed and feed may be tweaked as all machines are different but if anything I would estimate the speed would go down not up otherwise you will be forever changing inserts and if your lucky you probably will not exceed 6loads per corner use an insert with no radius corner.Because of the shape of this job as a second choice may even consider clamping a stack to table and use a solid carbide e/mill with coolant

Face Milling Cobalt HSS @65 HRc

Cast Iron

Stainless

Cast Iron

Stainless

Titanium

Diamond

Stainless

Cast Iron

Cast Iron

Diamond

Titanium

Diamond

Cast Iron

Titanium

Diamond

Titanium

Titanium

Cast Iron

Diamond

Hot Rolled

Similar threads