What's new
What's new

Hard Milling

emt2688

Cast Iron
Joined
Mar 6, 2006
Location
NE Nebaska
I have to machine some 1/8" chamfers around the perimeter of some hardened A-2 parts (56-58 RC). I will be doing this in a 20 hp. VMC with 10,000 RPM.

What would you use if these were your available cutters:
1. 90 deg carbide countersink.
2. 90 deg carbide Iscar multimaster insert cutter (looks like a 2 flute countersink or an end of a drill mill).
3. 1.25" dia Iscar octomill (uses 8 sided insert, results in a 45 degree lead angle).

What about speeds, feeds, and depth of cut?
 
I'd use the 90 deg countersink if it's the single insert kind. Cheaper to wear out 1 insert than 8 inserts.

I'd start speed out at 200-300 sfm, .005 chipload, and 1/32 depth. Observe and adjust speed accordinly based on insert wear.
 
Which tool is more rigid? That's the way I'd go. It also depends on the amount of parts. Then you really have to worry about tooling costs. Remember that rigidity is a major factor with all cutting, especially with hard milling. You don't want it bouncing off the side of the part. Even with a light cut, it's still 58 rc. That's some really hard stuff you got there.

Yet, I think all those tools would work in the short run.

I'd shy away from smaller tools and higher Rpm because that material will melt standard inserts in high heat conditions.

Just my 2 cents.
 
EMT,
I have had great success doing this with four flute carbide ball mills and bullmills. I cut hardened a2 at 500-650 sfm. I would try a .25 or .3125 ballmill and .001"-.0015" chipload. Sounds crazy but it works. Plus it makes a really cool sound when it cuts.

You have to think of it like this: the cutting edge of the tool is only going to pass through the hardened material a certain number of times before it begins to fail, so you have to make a chip and not wear down the edges feeding too slow.

I used a z-level finish 3d toolpath, .005-.015 depth of cut. If your cam will do it, start at the lowest point and step up in z, this keeps the cutting on the side of the ball (500-650 sfm) and not the center/tip (0 sfm). If your cam will not finish from bottom to top, then I would use a bullnose endmill. If you don't have 3d cam you can try draft/ taper toolpath in most 2.5d cam softwares.

Make sure if you use coolant that it is blasting as high as it will go and is aimed exactly at the cutting zone, if it is intermittent you cutter will be toast in a matter of seconds. If you can't get a constant blast of coolant you are better off cutting dry.

Also it is better to use tialn or altin coated cutters in the hard stuff. There are other coatings out there but I haven't tried them. You can get by with uncoated carbide for a few parts if you need to.

Hope I've helped, good luck.

Chris
 
I agree with Champion's previous post use a ball endmill and step it uphill,, my second option would be the multimaster by iscar.. I use those all the time on hard material with very good results.
 
I just did a similar job. I had to mill chamfers on some inserts that were 5 x 12, H-13, 53-54 Rockwell. I just split some 1/2 carbide blanks (two). Ground them to 45 degrees on the deckel, with 25 rake/relief. One for rounging, one for finishing. I ran them at 6000 Rpm (fastest macine will go, if I had ten I would have used most of it), I roughed at 21 IPM, and finished at 30 IPM......And cut them dry. Total time per insert....bout five minutes.

Don't over think the job, it's pretty elementary.
 








 
Back
Top