Machining cast iron vs 1018, not as expected.

I've been making a part from 1018 for a couple years, for this recent order the 1018 was unavailable, so we are allowed to switch to class 40 grey cast iron.

I've never done any real cast iron milling, aside from small simple stuff. This part takes about hour, tons of roughing, flat and perpendicular within .002.

For my first part I decided to run my normal 1018 program as a baseline. I was expecting the program to be slow. My expectations would.be 650 sfm would be about right, and chatter would be non existent. I expected to be able to feed faster.

This part is held upright in a lang vise, most of the roughing is 5" away from the vise with the table at 90 degrees. Not a rigid setup, but excellent for those perpendicularity call outs.

Roughing 5 flute end,
650 sfm
.090 radial
1.25 axial
.004 per tooth.
This is the sweet spot for this setup in 1018. Chatter like crazy in cast, the whole system was humming, from end mill to concrete.

Face milling 2" facemill (don't remember the exact parameters)
1500rpm
.005 chip perhaps.
.035 stock depth finish,

I ended up having to take the end mill down to 12 percent for the cast before the chatter went away, and the facemill to .010 stock remaining, and even that wasn't great.

My question I suppose is, what is the typical things to look out for, or adjust from 1018 to cast. Thanks

Cast iron is more abrasive, denser, and has more surface tension. When machining cast, a rigid set up is a must and your D.O.C. is critical.

DouglasJRizzo said:

Cast iron is more abrasive, denser, and has more surface tension. When machining cast, a rigid set up is a must and your D.O.C. is critical.

Click to expand...

Seems like based on what I'm seeing a lighter step over with faster feed is the way to go. I can't do anything about the rigidity given the shape of the part. Would you say that's the correct direction to go?
Thanks

BRIAN.T said:

Seems like based on what I'm seeing a lighter step over with faster feed is the way to go. I can't do anything about the rigidity given the shape of the part. Would you say that's the correct direction to go?
Thanks

Click to expand...

Yes, absolutely. You would be reducing the amount of torsional force on the tool.

At the big shop, carbide worked best for CI. 1018 flows along the tool cutting edge while CI takes more pressure and fractures ahead on the cutting edge. Carbide always proved best for CI and a small negative land at the cutting edge proved good. . Higher heat was a factor so a thicker insert was good so to absorb some of the heat.. dry was often better than using a coolant. When a coolant was used it had to be flooding, not a mist.

The negative land perhaps 5* and .003 to .020 wide allows the cratering common with CI to have a more cutting edge body to crater away before it affects the optimum cutting action, the wear seems to be/begin a tad away and behind the actual top face of the cutting edge.

It was not uncommon that the negative land proved better than the whole top cutter face being negative.

CI really beats up HSS cutting tools from the very start.

I can't see your set-up but if it might bump onto a solid heavy block high at the part's away side so reducing vibrations and chatter might make tool life increase and part quality better, rock-solid is best for CI.

The old Valenite value mills are good because you can set each insert under an indicator to a few tenths quickly on a plate. Having all the teeth engaged from the start is good.

That's weird. I had a job once machining a planetary carrier out of a 12" diameter chunk of Durabar. I thought as I was cutting it 'wow, no wonder they made entire machines out of this stuff, it's the nicest machining shit possible' I only ran with carbide.

Durabar is not even close to #40 cast iron.

Gray iron has about 2/3 the rigidity of steel but roughly the same machinability as 1018.

The net result in your case is the need to dial back the parameters.

The vibration damping characteristics of gray iron don't really apply to small workpieces.

BRIAN.T said:

so we are allowed to switch to class 40 grey cast iron.

Click to expand...

Oh lucky you


Sent from my iPhone using Tapatalk

adh2000 said:

Oh lucky you


Sent from my iPhone using Tapatalk

Click to expand...

Haha yeah, there is a reason they listed it as the alternative. It's not great.

Orange Vise said:

Gray iron has about 2/3 the rigidity of steel but roughly the same machinability as 1018.

The net result in your case is the need to dial back the parameters.

The vibration damping characteristics of gray iron don't really apply to small workpieces.

Click to expand...

I was hoping I'd hear from you! This is interesting information, and seems to be on par with what I saw today really getting into it. I was only able to get through about 5 parts before I left for the day, but it was running well.

Interesting side note, 8 percent increase in sfm cleared up all the chatter.. hopefully 700sfm isn't too hot. What do you think?

michiganbuck said:

At the big shop, carbide worked best for CI. 1018 flows along the tool cutting edge while CI takes more pressure and fractures ahead on the cutting edge. Carbide always proved best for CI and a small negative land at the cutting edge proved good. . Higher heat was a factor so a thicker insert was good so to absorb some of the heat.. dry was often better than using a coolant. When a coolant was used it had to be flooding, not a mist.

The negative land perhaps 5* and .003 to .020 wide allows the cratering common with CI to have a more cutting edge body to crater away before it affects the optimum cutting action, the wear seems to be/begin a tad away and behind the actual top face of the cutting edge.

It was not uncommon that the negative land proved better than the whole top cutter face being negative.

CI really beats up HSS cutting tools from the very start.

I can't see your set-up but if it might bump onto a solid heavy block high at the part's away side so reducing vibrations and chatter might make tool life increase and part quality better, rock-solid is best for CI.

The old Valenite value mills are good because you can set each insert under an indicator to a few tenths quickly on a plate. Having all the teeth engaged from the start is good.

Click to expand...

Great info! Thanks, I'm definitely not using HSS anything, I probably haven't used a hss end mill in 2 years. For the setup, I can't (don't want to change it) it's a 5 axis setup, work on all sides, most faces are perpendicular to one another .002. splitting up the ops would be problematic I think.

So far with the info you and other provided my ends mills are doing great. Thanks

BRIAN.T said:

I was hoping I'd hear from you! This is interesting information, and seems to be on par with what I saw today really getting into it. I was only able to get through about 5 parts before I left for the day, but it was running well.

Interesting side note, 8 percent increase in sfm cleared up all the chatter.. hopefully 700sfm isn't too hot. What do you think?

Click to expand...

700 sfm should be perfectly fine. Full slotting endmills run the slowest at 500 SFM. Everything else runs faster. We run our facemills between 800 and 1000 sfm. Dry of course.

What a contradiction, cast iron and a lot to rough!
Cast parts are there to reduce the amount of machining.
We seem to have lost one great idea of industrialisation.

If you have to rough cast iron, reduce V[SUB]c[/SUB] by a third to half compared to mild steel.

Mechanola said:

What a contradiction, cast iron and a lot to rough!
Cast parts are there to reduce the amount of machining.
We seem to have lost one great idea of industrialisation.

If you have to rough cast iron, reduce V[SUB]c[/SUB] by a third to half compared to mild steel.

Click to expand...

While I understand what you're implying, the part is not cast, it's cast iron bar stock. Perhaps I could look into having them cast. I wonder what that would cost.. interesting.

At the big shop we decided to make a part of nodular cast iron so we had the Detroit Testing Lab run a machining test on that material. I should have kept a copy of the results but did not.