Machining Cronidur 30

[Buckshott00]

Hello All,

I was wondering if anyone has actual experience with machining Cronidur 30. We are having a hard time and blowing through tooling trying to machine this stuff, and we were wondering if anyone else has had experience or tips they could share.

Thanks!

 

[TVP]

Is the material in the annealed or hardened condition? Cronidur® 30 should be heated uniformly to a temperature of 780 to 820 °C. The holding time after complete soaking is around 8 h. After this heat treatment the level of hardness will be 200 to 240 HB. Rough machining should be followed by stress relief annealing at around 600 to 650 °C. After thorough heating, the work piece should be held at temperature for about 2 hours and subsequently cooled down in the furnace to approximately 350 °C. This should be followed by cooling in still air.

 

[mfgenggear]

I uploaded a data sheet.
In addition to the very good advice I recommend this
I have never worked with this stuff. so when that is the case I experiment.
I will run sample of parts to experiment with machining, document dimensions before & after heat treating.
look at the stability after heat treat. does it expand , does it contract, or is it unstable.

I document it very closely. use the recommended feed & speeds, and work closely with you tooling supplier.
contact them & ask for assistance. ask for free sample of carbide or ceramics turning & milling inserts.
Make sure all setups are rigid as hell, keep all the tool holders short & large as possible.
I have worked with High Temperature alloys & these are the key points.

Rigid machines with generous horse power.
rigid set ups
the right inserts & tool holder.
the correct feeds & speeds.
any work hardening material requires a minimum depth of cut.
do not try to skim or it will work harden. .010-.015 min last finishing depth of cut.
use the the proper coolant & generous amount.
have plenty of m stops to remove chips.

Mfgenggear

 

[Buckshott00]

@TVP in the hardened condition we're machining it @ about 40HRc

@mfgenggear we've had lots of different tool guys here saying "try this, try that" and most none of it works and we're still under the gun for production. Thank you for your tips, but we're really looking for someone who has actual experience cutting it

 

[mfgenggear]

BuckShot

It can't be any tougher than stellite or Inconel 718.
It would help if you explained what difficulty you are encountering.
what tools have you tried, why & what is wearing out.
have you tried ceramics, do the machines have enough horsepower?
I seen exotics with metal flying off with 1/4" depth of cuts. if you have the horsepower & rigidity.

You said this
"mfgenggear we've had lots of different tool guys here saying "try this, try that" and most none of it works and we're still under the gun for production"

Try what? which tool guys? what feeds & speeds.
what country ?

Mfgenggear

 

[Buckshott00]

@mfggnggear

We're not wearing out tools, we're blowing through them. Trust me Cronidur is in a class of its own. We successfully machine stellite and Inconel 718 here frequently with help from ISCAR and Kennametal, but the corrosion and abrasion resistance coupled with the thermal conductivity properties make this ridiculous to nail down. We've got 40hp machines with as much rigidity as we can put into the setup. This is really one of those "you have to see it to believe it" type materials.

 

[Buckshott00]

Oh and I forgot to mention a lot of times it's at 58-60HRc when full hard with interrupted cuts. So we know it can be done well, because can do it, we're just doing it poorly.

 

[mfgenggear]

Buckshot

Then it is was it is.
No magic wand is going to make it faster or easier.
Like TVP said rough machine the stuff in the annealed condition.
then heat treat , & then do the finishing.
if you are blowing through the inserts then your going to fast.
or wrong geometry.
especially for interrupted cuts.
here are so more tips I left out
Insert seated properly
use the largest possible nose radius
use the largest possible positive lead angle
use the strongest insert geometry
round is the strongest
100 deg corner of the 80 deg diamond is the next strongest

Machining
roughing 550 SFM minimumum-1700
finishing 800 minimum -2000
flood coolant on insert
feed rate IPR
.005-.014 depending on depth of cut
if chip is curling & not breaking up increase feed rate or depth of cut

CNC program the feed to enter into the work with .003-.005 feed then full feed rate
reverse on exit

DOC
depth must be great enough to keep the nose buried.
lead angle should be 15-45 deg

If your sales engineer at either of the tool suppliers mention above are worth they weight
he or she should be able to nail down the right inserts.

Mfgenggear

 

[BillPSU]

If you are breaking the insert first try reduced depth of cut but feed at higher IPR. You may be work hardening. If the lighter cuts don't stop the insert breakage then you need to go to a tougher grade of carbide. One job in the distant past we were machining 17-4PH with multiple interruption. We ended up using a die grade of carbide. This material sounds like machining EDT150. Slower surface feet and higher feeds.

Good Luck

Bill

 

[Buckshott00]

Thanks for the suggestions guys but if you try to slow it down the chips will weld to the insert. It does not dissipate heat well it is super tough so it doesn't break chips well. Trying different inserts and chip breakers only meets with marginally better results. The best results were using our methods with different coolants with higher lubricity, but for various reasons we can switch over to that lube.

That's why I was really hoping that people who really do have experience with this Super-Stainless.

 

[mfgenggear]

Buckshot

The reason for catastrophic failure is the the inserts are wearing out. IE the edge is no longer cutting so heat build up is causing it to destroy it self.
I have had very very good success with ceramics. which are harder then carbide.
suggest this for interrupted cuts use C-5 carbide slow the hell down on surface speed to eliminate burning up inserts
or take very light cuts (.010 min DOC) with high SFM. the heat will dissipate with the chip.
for high stock removal & roughing then suggest using ceramics, then crank the sfm high as hell & use the tool geometry as suggested above.
if the machinist is using carbide with high SFM, it will not take the heat like ceramics. so it will fail. especially with abrasive material.

Ah brain starting to work, if the composition of tool & the part are similar there can or will be metal transfer to the tool which also ruins the tool.
the trick is to use grades of inserts that can handle the composition of the parent material. metal transfer to the tool, means this using the wrong grade
of carbide or ceramic. Thats why on start up ask the tool supplier for free samples of what should work & then what recommended feeds & speeds, depth of cut.
keep experimenting until you have it nailed down. sorry there is no easy way to do this, & those who are doing it probably will not give out that info.

Mfgenggear