What's new
What's new

turning hardened cast iron

EnderDRM

Aluminum
Joined
Nov 13, 2012
Location
WI USA
hi,
We are trying to turn cast iron that is heat treated to 50RC
have tried everything from hard carbide inserts to ceramics but nothing seems to work.
Various feeds and speeds and doc but they all fail on the first part.
Any advice would be greatly appreciated.
 
If this is white iron then the only thing I found that worked was a CBN cutoff wheel. It are diamond and carbide... You should get results with a CBN tool also.

Sent from my SM-G892A using Tapatalk
 
Greenleaf WG300 SiC reinforced ceramic will cut it. If you have a rough surface to cut off first, use round inserts as these can be indexed several times. In many cases, the insert will fracture on the top and still present a sharp edge to cut with. Use an aggressive feed rate to help prevent chatter resonance. Run at about 1000sfm. You might need an umbrella as this will make a cast iron rain in the shop :D

While CBN is good, you don't get as many sharp edges per dollar spent. And if the work has a rough surface to remove, you need sharp edges frequently.
 
T-land? Unsure of tool failure mode so anything a wild guess..
In volume production for sure I'd be in CBN. Maybe you could get a freebie from the local tool source to try?
Ceramics the in between but come in so many flavors some of which will not like this material.
Bob
 
Greenleaf WG300 SiC reinforced ceramic will cut it. If you have a rough surface to cut off first, use round inserts as these can be indexed several times. In many cases, the insert will fracture on the top and still present a sharp edge to cut with. Use an aggressive feed rate to help prevent chatter resonance. Run at about 1000sfm. You might need an umbrella as this will make a cast iron rain in the shop :D

While CBN is good, you don't get as many sharp edges per dollar spent. And if the work has a rough surface to remove, you need sharp edges frequently.

1000 sfm? And what do you mean about aggressive feedrate? DOC?
 
1000 sfm? And what do you mean about aggressive feedrate? DOC?

Feedrate of about .050" or so. Depth of cut about the same or whatever it takes to get below the skin and to get a continuous surface. A 1/2" round insert will want to chatter if you baby the feed.

We had a set of chilled iron roller mill feed rolls to do. They had the remnants of a shallow groove pattern all over the surface, although it was worn in the center (which was the reason to resurface them). Absolutely could not make any headway unless we took a cut deep enough to get below the roughness. These were 12" diameter by 30" long rolls. It was pretty tense to take the cut, it turned out to be slightly tapered on the surface, so it was getting deeper as it went, and we could hear the load going up on the motor. It finally tripped the breaker, more than the full 25 hp required :D But after we had the roughness off, then we could take lighter cuts.

A 1/2" round insert doesn't really leave all that much of a scallop at a heavy feed rate, like .050" so you can come in with something like your CBN with a modest tip radius of 1/16 or 3/32" for a finish cut without too much grief.

I liked the WG300 a lot and still use it whenever I have to rough something ugly, like a hard surface buildup, or a flywheel with hardspots. It is the only ceramic I have experimented with that has a decently 'sharp' edge and will cut without putting extreme pressure on the toolslide. For a skinny finish cut, you'd swear the material comes off like its not even hard, but a file can't make a mark on it.
 
Just an update:
First of all, thanks for all the replies. Your help is greatly appreciated.
@huflungdung, a round insert will not be practical for our application, but thanks.
Maybe a larger rad cnmg (.0468) could be used? Perhaps we can use a separate tool to get through the scale then go from there.
This a part that we have run hundreds of in the past, but the castings came in much harder than spec this time. The foundry has admitted their mistake but what happens with that is above my pay grade so it looks like we are stuck running them.
We are using a mix of ceramic and cbn inserts right now with mixed results.
Again, thanks everyone for your input. I read this forum regularly and have a great deal of respect for the people here.
 
I have used Ceramics in the past on large rock crushers. The advantage was in that day it was a very strong, large, and rigid manual lathe.

CNC’s often are not made the same way using a lot of electric power to do the cutting. I have found unless a CNC is geared out and with substantial ways that they often have troubles.

That is for general CNC machines. Oil field and mining use a lot of Mazaks which have some very good rigidity and ease of use. There are several which would do well and they are not cheap.

Finding the right tooling to use and the best setup and range of speeds and feeds often work as long as the machine is good how the setup is everything it can be. Usually when people discover they can not cut it they find someone who can or explain to the customer that someone better equipped would do better.

First I would exhaust every possible fix before giving up which would include subbing it out to someone who can handle it better. There should never be any disgrace taking care of the customer.
 
Just a thought... not as familiar with HT CI, but can you temper them back down to spec so you don't have to struggle with the machining?
 
From what I understand, cast iron cannot be annealed.

Maybe not annealing as the annealing temperatures are typically much higher. Tempering is done at significantly lower temperatures to relieve stress and lower hardness, which subsequently increases toughness and ductility.

I'd wager if it can be hardened, so too can it be softened.

What grade of CI are you machining?
 








 
Back
Top