Tool steel milling questions

[thunderskunk]

Hey!

Some silly questions about milling tool steels like 1060, 1045, A6, and S7:

• Generally, what’s the benefit of going to a larger diameter endmill?
  • Scenario is: we mill an outside profile with a 1/2” endmill on a BT40 Fadal that has the clearance to accommodate 1-1/2”. Tool life is 32 parts. Would increasing diameter increase life? Chip clearance? Cycle time?
• What’s the intent of coolant when machining steel? Are we trying to cool the tool, the chip, or the workpiece? How important is having the right oil/water mixture?
• How do folks machine steel without coolant?
  • Is dry machining steel sensitive to bad runout?
• We grind all surfaces by hand just for a surface finish with super loose tolerances. What’s out there for mill tooling with grinding/polishing faces?
• What’s the benefit of using roughing endmill with serrations? I’ve used them before, but I’m trying to convince someone else to try it.

 

[plastikdreams]

Endmills with corner radius 5 or more flutes with atleast TiAlN coating, airblast to clear chips, for the harder stuff I run 5000 rpm or less and around 20 or so ipm...gotta fool with it though to get it dialed in.

You want the chips to come off hot. You want to run the endmill hard. Liquid coolant is a no no.

 

[crossthread82]

When running an AlTiN coated carbide endmill hard in steel the edge heats up very hot and if you are flooding the cut with coolant it will shock the endmill leaving micro cracks on the edge leading to premature failure. So people just run an airblast to get the chips out of the way. Modern carbide and coatings can take the heat.

Generally no, increasing diameter isn't going to increase tool life, unless of course the smaller endmill was chattering and by moving up in size it quiets down. Chip load and SFM are the two biggest factors effecting tool life, too low or too high on either will drastically affect how long a tool will last. In your case moving up to a 3/4" endmill could be beneficial but I'd need to know more details in order to really say for sure. The main benefit of the bigger tool is you can run it harder so you're cylce time will be lower. Toolholder also plays a part in tool life too, b/c yes holder runout has a greater effect when you start machining harder materials compared to say aluminum. Every tool rep I've heard says every 0.0001"tir reduces tool life by 10% , now I'm not sure if it's that drastic but for the most part I believe it. If one flute is cutting 15-20% more material than the others then it's obviously going to wear out and chip before the rest.

Are you machining these alloys in their hard state or annealed? Because that changes your machining strategy pretty dramatically

The serrated endmills are most beneficial when taking deep axial cuts b/c the chips come of as nice little piece that can get washed or blown away very easily and they take up less room in the pan; straight (non-serrated) make those long horse hair chips that cling to themselves and everything. Plus as an added benefit, by breaking the flute edge up it acts like multiple smaller flutes which if you do the math on actually take a little less torque to drive through the cut than compared to one big flute.

As far as grinding or polishing in the machine. You could look into a burnishing tool to smooth the top face of the piece. And for the sides you'd really benefit from a having a dedicated roughing and finishing endmill so you're getting the best finishes you can.

 

[Milland]

I'd also pay attention to the condition of the machine. If your Fadal has a loose spindle, or more seriously is a box way with worn Turcite, I'd be concerned about larger endmills and heavier cuts causing too much excess free-play movement, leading to early tool failure. A larger tool would exaggerate this.

If the machine is in good shape, then perhaps going to a larger multi-flute (7 or so) with faster, lighter full-depth passes would speed up MMR. Air blast if you can get reliable coverage and chip clearing, rich coolant with lower RPM to lessen heat at the cutting edge if chips are sticking to the tool (which might be a sign to speed up with AB).

If the material is hardened beyond ~55RC perhaps you'll have to consult with the tooling MFG to come up with workable strategies. As for grinding, maybe plated CBN if hard and you can get the RPM you need. If softer CBN might not work as well. Set up filtering in the coolant path (even if not used during this work) to minimize steel dust being recirculated through the machine.

 

[Blaser Swisslube]

To answer your questions about coolant, generally you'd like some form of coolant, even a "mister," which uses minimum quantity lubricant (MQL) to cool the tools a little and help with chip load - a little coolant can go a long way. Running coolant reduces friction which improves tool life, and cools tool and work piece.

 

[camhead420]

If you choose coolant it is all or none. If you cannot flood it constantly then go to no coolant.
All the heat should come off with the chip when speeds and feeds are right.

 

[Comatose]

https://hsmadvisor.com/ is pretty good for this sort of "what if' speculation. You can play with geometry, coating, speeds, feeds, etc and see what it thinks it will do to tool life. It's not perfect, but I find it to be a lot more reliable starting point than the TLAR method.

If you can't get air onto the tool and you have to run coolant to get the chips away, AlCrN coating will last a lot longer than AlTiN. We use a lot of the 3/8" version of these:

1/2 Variable 5 Flute End Mill with Chip Breaker 1.25 LOC .030 Radius MariTool

www.maritool.com

 

[RC Mech]

What model Fadal? Linear guides vs box way Fadals have a significant influence on how well they can cut hardened tool steels.

TIR of tooling also has a profound effect on tool life. More to your point, generally a larger diameter tool will accommodate a higher feed per tooth (just like twist drills). And no, you don’t care about cooling the chip. Ideally the heat goes with the chip and it turns colour while the part stays cool.