Some basic suggestions for machining grey cast iron

Hey all,
I'm currently nut deep in a rather sizeable job that includes several castings. From what I understand these castings are made of grey cast iron. I'm a relatively inexperienced machinist, and am open to any recommendations regarding tooling choice, feed and speed, and any other handy tips for tackling this particular material thanks! I'm running a DMG Mori DMU95 Monoblock 5 axis milling center.

Get ready for stinky dust.

Grey iron is abrasive, but it cuts easily. It will cut well, but it will wear tools a little quicker than mild steel.

Run slower SFM on solid round tools, and more feed-per-rev.

If you have a trusted tooling vendor, give them a call. If not, it may be time to look for one. Luckily, you're in Michigan, so there should be many to choose from.




Perhaps provide us with a little more detailed explanation of what kind of machining, and therefore what type of cutting tools you'll be needing.

I have gerat luck with a TNMA inserts. I had them forever and an not sure the grade.

Jashley,

Great information to start with. I'm currently dealing with only certain parts of these castings needing to be machined. The areas in question seem to have a pretty consistent .375" of stock cast in, so in the interest of mitigating guesswork, I have been toying with trochoidal HEM toolpaths that I can use to remove all of the extra material save for .010" or so for finish. I'm using predominantly reground tooling that has been shortened as well. So far, I've gotten relatively surprising tool life through the roughing sections this way. Hope this helps clarify what it is I'm attempting. Feel more than free to ask any other questions, or comment as necessary. Thanks a bunch!

I wouldn't bother trochoidal milling in grey iron. It's too easy to cut.

Here's the secret with abrasive materials.

Each time an endmill's tooth enters the cut, it accrues "mileage" - It has to travel a specified distance each time it enters the cut. Mileage = wear. If your part is 1" long, and your hypothetical 1-flute endmill is fed at .005" per rev, then that means it will take 200 revolutions - or cuts - for the endmill to feed all the way across your 1" long part, and remove all that material.

If you increase your feed to .007" per tooth, then it only takes 143 revolutions of the endmill. You just saved 67 revolutions/miles of wear on your tool, meaning you gained 33% tool life.

So, there's the lesson on feed...

Now, let's look at cutting width.

If you can do with with only 1 width pass, then good. If you choose a trochoidal-milling strategy, then let's say you have to take 5 width passes, instead of 1.

What's going to happen to those cutting edges? They accrue 5 times the wear....









HSM / Trochoidal milling works well, when you want longer cutting lengths to eliminate Z-depth passes. It works well when the material is tough, hard, or whatever, when a wider width-pass would prevent cutting of your profile at full depth. If your material is fairly easy to cut, then all HSM will do is add cycle time.



My advise - Buy a good endmill designed for bulk material removal, and cut it all away in one width pass. Leaving stock for finishing is a good idea.

I used to sell Niagara, but these would be good tools for your job, as well as a good resource for learning.

Roughing Endmills - Niagara Stabilizer 2.0
https://niagaracutter.com/search?listings=1&page=1&category=End Mill>High Performance>Stabilizer 2.0

HSM / Finishing Endmills - I would suggest a 7 flute for strictly finishing
Niagara Cutter

Jashley,

This was massively helpful. I have full intentions of gaining a better understanding of programming feedrate via feed per tooth as opposed to IPM, which I'm understanding is a relatively archaic way of thinking about feed. Your explanation does a great job of putting it in a format that makes sense, while spelling out what is happening while the cutter is engaged. I assume this concept of accruement of "mileage" as you put it, applies to any material just at varying rates based on the properties of the material? The sections to be machined are quite a bit larger than 1" haha, though I've strayed from the HEM path in favor of Z-level roughing with a high feed shell mill, though wear seems to rear its head as well here. I've taken to using the cutter mfg's recommended feed per rev and am having good results. Must say I'm ready to be through with this job either way.

Thanks for your wisdom, best regards

KevintheCrawdad said:

Jashley,

This was massively helpful. I have full intentions of gaining a better understanding of programming feedrate via feed per tooth as opposed to IPM, which I'm understanding is a relatively archaic way of thinking about feed.

Click to expand...

Whatever works. FPT may be easier, as most CAM systems can use this as an input. But whatever works really.

KevintheCrawdad said:

Your explanation does a great job of putting it in a format that makes sense, while spelling out what is happening while the cutter is engaged. I assume this concept of accruement of "mileage" as you put it, applies to any material just at varying rates based on the properties of the material?

Click to expand...

Yes.

KevintheCrawdad said:

The sections to be machined are quite a bit larger than 1" haha, though I've strayed from the HEM path in favor of Z-level roughing with a high feed shell mill, though wear seems to rear its head as well here. I've taken to using the cutter mfg's recommended feed per rev and am having good results. Must say I'm ready to be through with this job either way.

Click to expand...

High Feed Mills work great, especially as the material gets tougher. Wouldn't be my first choice for roughing grey iron though. The ends of the high-feed mill will accrue mileage, just as the periphery of the endmill will. A bunch of Z-level passes = more mileage accrued.

That said, If it cuts the material away, predictably, then just index the inserts as needed, and roll on.

I said that high feed milling wouldn't be my first choice. It works though. And if I could see your part to be cut, I may agree that it's the best choice. (Or not...)


I'm glad all that helped. Stick around, and best of luck.