Machining Hard steels at 1400 SFM? Also, plunging question.

[facegarden]

So i was looking on SurfCAM's site, and i found some videos of them machining steel at well above the speeds i'm used to seeing for that kind of material...

This video in particular shows them machining 4140 steel ar about 30 Rc hardness at over 1400SFM! I'm relatively new to machining, and all the charts i find online recommend feed rates that are less than a quarter of that for steels... What is going on? Is it really safe to machine through 4140 steel at 11,000 RPM with a half inch tool? Or are they just destroying the tool to show off how fast they can machine? The surface finish looks nice...

I'm just really confused because our tools tend to complain if i turn up the spindle speed past about 2200 RPM in material like that, but i'm also machining at much slower feeds...

My last question is: I noticed that they're plunging into the material with a helical spiral - my boss, who has been doing manual machining for years, but has never touched the cnc, says i should always pre-drill as much as possible, rather than do any kind of plunging, even a helical spiral... Do you think that is really true? Pre-drilling requires an extra tool and more work... so if it's not worth it i'd love to not have to do it!

Everything but the softest steel has been the bain of my existence and i'd love to learn how to better machine harder materials, so any advice is appreciated! Thanks,
-Taylor

[facegarden]

Hey Mods, i meant to post this in the "General Machining" section, not the general engineering section, could you move it?
-Taylor

[Caprirs]

Like many things, it is the combination of the components involved.

The machine has to be rigid. At least one of the videos states the part is being run on a Makino. Rarely are these types of demo videos performed on Haas or Fadal style machines.

The tool must be designed for this sort of machining. It has to have the proper reliefs to allow high feed-per-tooth. Notice also how short the endmills are compared to their diameters. Stubby and rigid. None are mounted in collets either. It looks like some of the toolholders are the hydraulic type.

There is no flood coolant being used which can cause the tool to experience thermal shock. This occurs when the cutting edge of the tool gets hot while making a chip and then is hit with the coolant. Many of the carbide insert style endmills and facemills are designed to run dry or with an air blast to blow the chips clear of the cutting area.

It takes serious horsepower in the spindle motor and the axis servos. The spindle cannot dip in speed from the sudden load as the tool engages in the cut. The axes must feed smoothly and precisely even with high tool pressure.

The final part is what Surfcam is trying to advertise which is the programmed tool path. Typically, when pocketing, the tool will experience spikes in load when it enters a corner. While moving in a straight line, the tool is only engaged along one edge. When it gets to an inside corner, the "front" of the tool gets buried into the workpiece. Surfcam is advertising a programmed toolpath that avoids sharp inside corners allowing the tool to run close to its maximum performance all the time.

As for the ramping, it can be faster to ramp than to predrill. Endmills loathe straight plunges but will go sideways with much gusto. Predrilling can be preferred if there are enough plunge points or there isn't enough room to allow the endmill room to ramp.

[John3]

Originally Posted by facegarden So.... My last question is: I noticed that they're plunging into the material with a helical spiral - my boss, who has been doing manual machining for years, but has never touched the cnc, says i should always pre-drill as much as possible, rather than do any kind of plunging, even a helical spiral... Do you think that is really true? Pre-drilling requires an extra tool and more work... so if it's not worth it i'd love to not have to do it! -Taylor

Over the years I've come to the conclusion that "The most efficient and effective way to remove material is with a drill (PERIOD)."

I'd agree 100% with your boss.

We've played games drilling holes with endmills when we have to (which is a lot). But if there is a tool changer slot available for a drill bit, use it to rough the hole out. Nothing will work better/faster/cheaper/longer.

John

[Geof]

Originally Posted by facegarden ...machining steel at well above the speeds i'm used to seeing for that kind of material..... machining 4140 steel ar about 30 Rc hardness at over 1400SFM! I'm relatively new to machining, and.... i find online recommend feed rates that are less than a quarter of that for steels... What is going on? Is it really safe to machine through 4140 steel at 11,000 RPM with a half inch tool?... I'm just really confused because our tools tend to complain if i turn up the spindle speed past about 2200 RPM in material like that, but i'm also machining at much slower feeds...

Caprirs points out what is required for this type of machining; power, rigidity, smooth motion and emphatically no coolant. The reason it works, or I should say my interpretation of why it works based on long past experience, is that the heat generated in the chip takes it to a high enough temperature that even though it is a hardened alloy steel it becomes soft in the cutting zone.

The alternative method of machining these steels is to go much slower as many of the charts recommend. At the two ends of the speed spectrum tool life can be very good although you have to make sure the correct measure is being used. At the low speed the tool lasts a long time but doesn't remove as much material as the high speed does in a much shorter time. As you have found if you move into the mid-range the tools do not like it.

I first encountered this type of mind boggling metal removal many years ago using face mills on big manual machines but back then it was limited in application because most machines lacked the rigidity and smooth motion required. In addition the coatings used on the carbides were not as advanced so the cutting tip would get severely cratered from the extremely high temperature high pressure contact with the chip and could fracture off. Things would go downhill very quickly from there.

[toastydeath]

The absolute largest factor, beyond absolutely anything else in what you're seeing, is the tool itself. They're using whisker reinforced ceramic inserts. Other options are diamond and CBN, though diamond won't work on steel. Be prepared to spend 70-150 dollars per insert when you price these out.

Carbide, even the hardest grades, do not survive this kind of use, whereas ceramic won't survive without it. Ceramic inserts want the fastest spindle speed you can obtain, with a relatively gentle feed and depth of cut. That translates to a very fast cut in RPM and IPM, but comparatively little material removed per tooth.

As has been said, the ceramic, being somewhat a refractory and abrasive material, heats the metal up to the point of being molten, and just squeegees it off the part. The horsepower requirement for this kind of cutting is reduced, so high speed machining centers do not have the very large spindle motors that people would expect for that kind of material removal.

In addition, this kind of milling is hard on the machines and the folks that do it spend a lot of time and money keeping them running and certified - aerospace. The cost per part doing this when you don't NEED to be doing it increases.

[BluegrassPicker]

We machine with high feed mills (Iscar & Mitsubishi) on 40 and 50 taper machines at speeds up to 418IPM in 1018 mild steel. The DOC is up to.095The trick is to use air blast not coolant to clear the chips.
We also helical ramp to do pockets. I never predrill, even using inserted drills to predrill and 2.5 secs chipto chip toolchangers, it is still faster to helical ramp.

[Geof]

Originally Posted by BluegrassPicker ..... speeds up to 418IPM in 1018 mild steel. The DOC is up to.095The trick is to use air blast not coolant to clear the chips....

What SFM are you using? It has to be high to get a high rpm otherwise you must be using a very large feed per tooth.

[Caprirs]

There is also an element of getting the hot chip away from the tool so quickly that the hot chip cannot transfer its heat back to the tool. Thus, the air blast instead of liquid coolant which would more readily convect the heat back to the tool at the microscopic point of contact.

Also notice the software tends to program the tool path so the tool doesn't dwell in any one area for long. This is what Surfcam is specifically pimping in these videos. For example, instead of slotting the conventional way, the tool path is a series of "loops" clearing a path larger than the tool diameter. This prevents the tool from being engaged 180* as in conventional slotting.

The video cutting 4140 cited using an Iscar solid carbide endmill. In fact, none of those videos used insert tools, only solid carbide.

Here's Makino's general info regarding high speed machining: http://www.moldmakermag.com/techframeset.html

[dertsap]

first thing to remember when looking at advertise videos is they are trying to sell you something and the best way to sell is to impress by pushing everything beyond the max

with running high speeds there are many factors ,material type, insert grade ,depth of cut and engagement ,
on 1018 i 've run a 3/4 insert 3flt at 7200 + @ 120ipm +
right now we're drilling some mild steel parts 2 1/2" dp with carb drills 4300 rpm @42 ipm , etc
under the proper circumstances tools can perform incredibly well , most times tools are being under utilized ,people tend to be think that running tools slower with less heavy of a cut will preserve tool life ,this can t be any further from the truth , the days of burning hss are over , tools are of far better quality as well as the machines they are being used on

[Geof]

Originally Posted by Caprirs .....Also notice the software tends to program the tool path so the tool doesn't dwell in any one area for long. This is what Surfcam is specifically pimping in these videos. For example, instead of slotting the conventional way, the tool path is a series of "loops" clearing a path larger than the tool diameter. This prevents the tool from being engaged 180* as in conventional slotting....

That is an important part to this technique. Don't ever try to do something like this with a lathe tool that is buried in the cut zone 100% of the time.

[MDLang]

Geof,

http://www.youtube.com/watch?v=RVttPttIQZ0

In the above video I was running at 312 IPM with a new Hitachi feedmill.

The tool lasted about 50 pieces then we broke a pocket off. It was a trial tool that Hitachi gave us so the rep came by and replaced the tool and suggested a higher SFPM, from 650 to 750, a lighter DOC, from .035 to .025, and DOUBLE the feed from .12 FPR to .24.

At the new values the machine, a Mazak, was a bit unhappy with the feed so I settled on .22 FPR. Do the math and you'll get 660 IPM with a 1" tool at .055 feed per tooth. Finished off 100 more pieces with no more problems and a shorter run time.

High feeds are what feed mills are all about. DOC rarely exceeds .06 for the larger diameters.

418 is no problem really.

Mike