blue chips using 6" face mill???

[max90272]

Hello,

I've been getting some SERIOUS blue chips while face milling 4340 non-hardened steel using a 6" indexable face mill with 10 carbide positive inserts. Is this a bad thing? I certainly know it is not a good thing, but I am unsure as to if it is a big no-no... I usually mill aluminum so I am used to cutting fast and never had that problem. My rpm is 225 and my feed is 6ipm doing about .060" depth of cut... I know the formula dictates about 100 SFM*3.82/ diamaeter of cutter for the spindle speed but if i lower the rpm that much, the spindle meter load goes really high so when i put it back to 225 or higher, it goes back to about 30%. So i'd like to hear from experienced steel millers. What feed and speed would you use in this case. Are blue chips REALLY that bad? Thanks

[tony978]

I would say worie is you start having the insert worn back in the shape of the stock hitting it on the first pass . depending on the grade of carbide you can get a little dark blue and be fine . you could run coolant and make a mess.

[ntcnc]

Without knowing what grade/style insert you are using it is hard to get a good number. from what I see on your numbers your feed seems way to slow. My calculations show you running at 235 SFM and feeding .0027 per tooth. I do not know what kind of machine you are running but 30% spindle load is nothing. I do not have a lot of experience with 4340. But I would think you should be running about 400 SFM and .005 per tooth. (My math 382rpms and 19 ipm) but again your machine/insert/facemill and set up are all unknown factors to me.

Blue chips are not bad as you want the heat leaving with the chip. I would not run coolant as you will get thermal cracking on your inserts and your tool life will tank.

[little bubba]

100sfm??? Carbide inserts, annealed 4340????

Blue chips, thats what you need, that's what you want.

Right now you are at about 355sfm and .002 per tooth, you need more.

Ran out some 4340, lots of facing, this past summer. 3" 45 degree lead facemill, 5 flute. Low dollar TMX inserts. .070 depth of cut, 2" or so step over. 870sfm, .013 per tooth or 1100rpm, 70ipm. Ran great, just a run of the mill Fadal. Moved 180lbs or so and the inserts were good for the next job.

Dark blue chips are not a problem, running a carbon steel, thats what I want to see in the chip pan. If the chips are coming off shiny, you're leaving money and productivity on the table.

[neilw20]

Crank up the feed to 0.002" per tooth, and even a bit more speed.
A lot of noisy air so you don't recycle the chips, as the inserts won't like it much.
I have found on that size about 4-5mm DOC works well, and keeps the cleaner very busy. Add coolant, HP rockets as hot chip work hardens before breaking off, and it is not good. Do it dry.
Some experimentation with the insert so you get good chip breaking.
If you use 90% power, who cares, as long as it goes into the chips.
When it is running sweet, it has a different sound, albeit awful.
A good swarf conveyor is a bonus.
If you have intermittent cuts approaching the start of a cutting pass seriously consider reduced feed rate on approach.

[DareBee]

Push it harder.
Feed should be .006 (or more) per tooth

[gmfoster]

They say if the chips aren't blue your going to slow!

[eorourke]

There are two factors to look at: HorsePower curve and spindle taper. If the taper is a Cat 40, then you are straining the limits of the spindle. Also you should peg your rpms to the high end of the torque and horsepower curve. This should give you plenty of power depending on your available HP and then you should push your feed rate -.004-.008" per tooth would be an excellent area to go for. Also you don't say how dark blue the chips are. If they are almost purple then up you feed rate. Your desired chip should look bluish grey. Over

[PixMan]

The cutting speed should be determined as a match between the carbide grade and coating to the material being cut. The feed rate used should be a factor of the the insert's chipbreaker (top form geometry), depth-of-cut required, width of cut, and approach angle. Once the best cutting parameters are established, you calculate the horsepower requirement and back off on depth of cut or width of cut if the HP required exceeds what's available.

In most cases, an annealed 4340 and most carbide for steels would start at a minmum of 350sfm. I cut it at upwards of 800sfm with the right cutter and inserts.

No matter what, a blue chip is OK and desired. That means you're getting the heat of the process into the chip rather than the tool or the workpiece.

[Geof]

I am surprised nobody commented on this;10 carbide positive inserts.

You should be using negative inserts on steel as well as running a faster speed, much faster feed, with a strong airblast and NO coolant.

It is possible you had already burnt the tips off the positive inserts and where getting a lot of rubbing. It is also likely that running positive inserts at the speed and feed used for negative inserts will, very quickly, either burn or chip the cutting edge off with nasty results.

[PixMan]

Nobody brought that up because it's not a big problem. Some the best cutters I've used in steels have a positive rake insert. Negative rake cutters can remove more metal and do so faster than positive rake cutters, but they do require a lot more power @ the spindle and axis servos.

[littlerob]

Originally Posted by PixMan Nobody brought that up because it's not a big problem.

Eating popcorn and waiting