[elite1]

Forgive me on my mill knowledge as i am a extreme novice.(nuts)

I have some Chromium Cobalt that i need to mill with no manufacture guidance. I ran a test today using a "Titanium Nitride" coating. Mill environment is as follows,

Tool diameter was 3.17mm/2 flute
0.2mm depth of cut at a feed rate of 200.
Spindle speed at 35,000rpm

I feel that the spindle speed is to high and my feed rate is to low as the tool life wore extremely fast. I knew the tool meet its life when i started seeing some sparks. Smearing of material was also present.

A sample of test run below. I can take better photos later.

Thank you for your time.

[christinandavid]

Never touched chromium cobalt (it doesn't sound very soft) and that kind of cutting speed is most suited to aluminium alloys, according to the literature I have available...

Also, you are taking .002mm cuts using that combination of speed and feed, which is not really ideal - you should be taking at least 10 times that amount if you want your tool to last.

I would start off at S2000 F60-F100. Increase feed until cutter sounds like it will break/does break, then back off a little. Rough out component and use fresh cutter for finishing (increase speed if finishing floor only). Exchange cutters often by disposing of rougher, relegating finisher to rougher status and loading new finisher. Use copius amounts of coolant/cutting oil.

If this method proves too time-consuming or cutters are breaking/pushing-off, you need to rough out using a larger tool. That cutter in the photo doesn't look coated (TiN is yellow, TiCN is purple, TiAlN is black)

DP

[beege]

Chromium cobalt is tough and abrasive.

try 2400 RPM, 40 mm/min.

Tools will not last very long, no matter what you do. Lots of luck to you. (chromium cobalt - is this Biodur?)

[Buntron]

Use Carbide Tools and a lot of coolant if you haven't already. Failing that, try using cutters that are designed to cope with cobalt chrome.

[Superman]

If doing a thru hole, drill it first

chrome, nickel/chrome are in the same machinablity zone ( bloody hard )

- Max. Cutting Speed with carbide tooling - less than 45m/min, feed about 0.03 /tooth
- stiff as possible part setup
- tooling as short as possible
- flood coolant

your 1/8" tooling may work better with 1/4" shank
don't use sharp cornered tools, use chamfered or radiused ( sharp corners do not have good strength, once corner goes-it goes quick )

Roughing may be better using 4 flute cutters ( bullnose or ballnose ), even look at "feedmill" type cutters
These run about the same RPM, <0.5 feed / tooth, 0.3-0.7 DOC

[BKGUY]

You should definitely to with a 3 or 4 flute cutter in this material. Also, use TiAln coating. You are going way to fast! Slow down.

[elite1]

Thanks Guys. I have integrated flood coolant and tipped radius endmills. Chrome cobalt is soft but smears. I have aquired feeds and speed from a titanium template which have got me much closer. I feel (being a novice) that chrome has a simular property as aluminum but a hardness simular to titanum (to some digree)


I am looking into purchasing a MiniMill from Haas but i am not sure until i produce parts well at a maxiumun spindle speed of 10,000RPM at a 0.6mm tool.

Thanks for your input!!

[Buntron]

CoCr is NOTHING like Aluminium or Titanium. If machine CoCr like either of these two materials your going to go through cutter's like there's no tomorrow!

You definitely need Cobalt TiAln coatings but you surface speed should not exceed 40 m/min!

With the information you've given 35,000rpm (Bloody fast!) and a feed of 200 means to have a feed per tooth of 0.003. This, together with the 0.2mm DoC means that your rubbing the tip of the tool away quicker than your removing the material.

Try these settings:
Spindle speed 2500rpm
Feed rate 50mmpm

Use TiALN for your first choice, then TiCN and TiN as you final choice. Also, make sure your engages are correct and use DO NOT have sharp angles when changing direction in cut. Use arc moves.

I spend a lot of time machining CoCr to tight tolerances and I've TiALN cutters to be the best.

[elite1]

Thanks Buntron!

For the suggested spindle speed and feedrates is that for a 1mm tool?

What kind of tool life are you getting using the TiALN coating?

Thanks for your help

[Buntron]

Those speeds and feeds are for the 3.17mm tool you said you was using.

I generally get very god tool life from my cutters. You can't take massive cuts at high speeds, but you can't take small cuts at low speeds and feeds either.

The smallest DoC I'll take is 0.1mm. Any less and the tools wears away.



The picture (if it worked) is of a CoCr part I have machined. The finish is a machined finish and it took about an hour and a half to machine (48mm in length). the cutters I used to machine this part were still being used 7 parts later.

[elite1]

Wow Buntron the finish on that chrome piece is amazing. i don’t need that type of finish on the part i am milling. I am milling dental copings. I have milled it successfully with that following but i think tool life is limited at these speeds. What do you think?

Roughing
3mm ball nose DOC 0.18mm / step over 0.75mm 20,000rpm / 2,000mmpm Flood
2mm Ball nose DOC 0.1mm / step over 0.5mm 22,0000rpm / 2,000mmpm Flood
Finishing
1mm Ball Nose DOC 0mm / Step over 0.05 32,000RPM / 1300mmpm Flood

Some are rather using air inside of flood. Do you use coolant or air.

I have successfully milled at these specs but haven’t milled quantity to know what the tool life is.

I will try to integrate a tighter step over for a finishing tool path on one side and create a further step over on to the external surface (tolerance non-important)

Thanks for your feedback and information. I need to produce parts at a much faster speed thus the feeds and speed. Any help in creating this is very much appreciated.

[Buntron]

I use thru coolant & flood coolant. I'll use high pressure coolant if I can as it helps to break the chip. I have been told that the way to machine CoCr is to use air blow systems.

This makes sense as your not putting the cutter through massive heat cycles. I had similar trouble with a 40mm face mill on 17-4ph stainless. The tips lasted twice as long when I switched off the coolant.

I use a M.A. Ford 3mm ball nose on cobalt chrome. This has 4 flutes and tapers onto a 6mm shank so it is very rigid and I very rarely have to change it. I can run it at 3500rpm and 300mmpm.

[TechGuy5002]

What about EDM instead of milling, if this is a medium to high production?