Milling a pocket in A36 Steel

[stang5197]

Need some help getting the feeds and speeds for cutting large pockets in A36 H.R.S.

Biggest problem is plunging into the material. Right now we are ramping in and that does not work very well at all.

We mostly run A.L. and this is the first time running steel. Right now I am using Promax Pro-4 3/8" Diameter 4 Flute Carbide ALTin E.M. with a 0.020 corner radius.

I was going to try drilling a clearance hole for the E.M. to keep from having to plunge but still get the feeds and speeds right in the pocket.

Total pocket depth is 1.125"

Any suggestions?

[DSL PWR]

What machine are you doing this on?
What feeds and speeds are you using?
What is the angle of the ramp?
Are you using a center cutting endmill?

[stang5197]

The machine is a Haas VF2 (40 taper)

Currently running at 3500 @ 25 ipm with a doc of 0.1"

The E.M. is center cutting, but is chipping during the ramp down process.

[HuFlungDung]

You did not mention what type of ramp: boundary ramp, zigzag ramp or helical ramp.

I prefer helical ramp because it makes a more open-sided entry which helps get the chips out of the way, minimizing the recutting which breaks the tool tips. I usually use about a 3 degree ramp angle, whether the tool is center cutting or not, many tools will still open a cavity at a shallow angle.

Use an air blast to move the chips out of the way. I avoid using coolant with carbide if there is significant heat generation due to heavy chip cutting. Coolant is fine with a finish cut, but it may actually cause your tool to fail prematurely if it is working hot in the cut zone.

[stang5197]

It is a zig zag ramp down, not sure of the angle yet, I will have to check the program.

Cutting dry concerns me, but I will give it a try. Only have flood coolant so I will have to keep an eye on chip control.

Do the feeds and speeds look close? This is the 1st time cutting this stuff, we cut 99% A.L. and very little of 304/303 S.S.

[HuFlungDung]

Yes, I'd say your speeds and feeds are workable. If you ramp in steeply, it would probably be advisable to reduce the feed rate to 50% until the tool is at depth.

Because you are already using radius tip flutes, and still getting chipping, I think the problem is either thermal shock or chip recutting. It does not take a huge amount of air to keep the chips flying. I use the tiniest loc-line nozzle (about a .055 diameter hole) and maybe 30 psi for an 'air blast'. It is barely audible air flow but it moves the chips.

It does not hurt the carbide endmill to warm up and stay warm while cutting. The occasional spark coming off is about right, you could maybe slow down the rpm a bit if that bothers you. On break through, you'll see lots of sparks, but that is normal.

[Andre' B]

Aluminum based coatings like AlTiN and even TiAlN need to run somewhat hot to get the most out of them.

The speeds and feeds you have are a good starting point, you can fine tune as you run.

You said a large pocket but you are using a 3/8 end mill. If you are doing a lot of these parts you may want to look at getting an insertable tool designed for pocketing and then use the smaller EM to clean out the corners if needed. Give your tool rep. a call and see what he suggests, is good to make them guys earn their keep.

If it is just a few parts as suggested you are likly ramping in too hard and/or recutting chips.

If you can drill a hole to start in an insert drill that makes an almost flat bottom is good, then you only have to helial ramp in on the last past, saves some time.