I am writing several speeds and feeds calculators at
formatting link
I want to write a calculator to figure out the best speeds and feeds given machine limitations (RPM and HP).
What I ran into is lack of quality references as to what feeds and speeds are acceptable. Some books (like _Machining Fundamentals_) or websites list pretty lame tables such as "recommended feed per tooth", without taking cutter diameter into account.
So, would anyone suggest a website (preferred) or book that gives good formulas for various combinations of cutter material, diameter, and material to be cut.
I did look and did not find anything suitable.
Also websites disagree pretty wildly on recommended SFM speeds.
Cutter diameter does not factor into "feed per tooth" a.k.a. chip load, but the number of cutting edges / flutes does. Cutter diameter factors into surface feet per minute for determining RPM. Your top RPM determines how fast your axis feed can be to maintain a given chip load.
Material and tool type will determine acceptable chip load and SFM, from there you look at the number of cutting edges and diameter to figure out what RPM and axis feed rate will put you in the acceptable chip load and SFM range.
Iggy, Even the best references are a starting point. Not only does the best speed and feed depend on your listed parameters, but the answer also involves the stability and stiffness of the work piece and machine itself. The horsepower of the machine is rarely a concern. Of course, the use, type, temperature and quantity of coolant also plays a major factor. No table can give you the definitive answer. The theoretical best is when the cutter causes the chip to rise to, but not beyond, the plastic state of the material being cut. That is where the least amount of stress is afforded the tool edge, but at the same time the tool edge must be kept at its most durable temperature for longevity. Unfortunately, every situation is different. Let experience be your guide. Steve
IMHO, you won't come up with a calculator that helps much. HSMs use too many different situations and aren't after that last 10% in productivity.
I just start on the low side and turn feeds and speeds up till it "looks about right". I'm after tool life first, top end speed second.
of course this is something you get the feel for with experience. I've been mangling metal for thirty years now. My son tells me I'm still just a hack.
Pete, are you saying that a 1/8" cutter should have the same feed per tooth as a 1" cutter? That seems counterintuitive, as the 1/8" cutter would break more easily, no?>
I will let Pete and others continue this, but feed per tooth is related to how much chip room there is in the flutes of a cutter, and to the force that a given cutter shank can tolerate. Unlike surface speeds, it has almost nothing to do with generating heat.
That's one of the things that makes milling a lot more complex to plan than turning is, for example. You really need to accumulate some experience to plan feeds and speeds for multi-tooth milling cutters. There's no simple way around it. You'll get a sense of how much chip volume a given feedrate will produce, and you'll eyeball your cutter, and make a reasonable judgment based on those factors. There are some formulas around for cutter diameter, number of flutes and feedrate, but the flute depths in small-diameter cutters vary quite a bit, and you'll have to temper it with experience.
The sound of a cutter that's chip-bound is distinctive, and it occurs for just a split second before you break the cutter. d8-)
No, it's more complex than that. Material to be cut, cutter material, cutter flute count, cutter diameter, RPM, axis feed rate, part and machine rigidity, available HP, depth of cut, coolant / lube, and the phase of the moon all are part of the equation. You simply aren't going to find one good formula to calculate your settings from.
Section 17.8 in Machining Fundamentals gives you recommendations for SFM range and chip load for various cutters and materials. Since your 3,000 RPM spindle top speed isn't likely to exceed the SFM of any modern end mill, you need to work from that RPM as your limiting factor and ignore cutter diameter and SFM for the most part.
For an end mill in aluminum, figure 17-71 shows 0.009-0.022 chip load.
Shooting for 0.012" chip load as a mid point, and using a .5" dia two flute end mill: (2*0.012)*3000=72 so 72 IPM at 3,000 RPM would give the desired chip load. Using the formula in figure 17-72 for SFM: ((3.1415*.5)*3000)/12=392.6875 so we're only at 393 SFM which is below the range specified in figure 17-70 for aluminum i.e. spindle RPM is the limiting factor.
Recalculating with a .5" four flute end mill: (4*0.012)*3000=144 so we can now go 144 IPM at 3,000 RPM to get the chip load we want. Since we didn't change the end mill diameter the SFM didn't change.
Recalculating with a 1" four flute end mill we haven't changed the number of flutes, so the chip load remains the same and we have the same
144 IPM feed rate for our 0.012" chip load. The SFM in this case does change: ((3.1415*1)*3000)/12=785.375 which puts us in the middle of the figure 17-70 SFM range for a HSS cutter in AL.
Yep, even more complexity. That chip clearance will relate to the depth of cut as the area swept by the cutting tooth and generating the chip along with the chip load determining the thickness of the chip. The depth of cut vertically on the end mill isn't the same, and mostly affects the HP required.
These are all things that don't matter a lot for manual milling since you will more-or-less instinctively find acceptable feeds and depths of cut by watching what's happening. In CNC milling you have to figure out what will work up front since you don't have the same interactivity beyond the feed rate override and spindle speed override controls.
A good argument for becoming proficient at manual milling before getting into CNC. I've never been proficient at milling, and I would be at a complete loss planning a CNC job. But I had some years of running a manual lathe before we got our Sheldon 1710H NC lathe in the mid-'70s, and it really paid off.
Exactly. And to those people who say "for hobbyists it does not matter how much it takes to complete a task", I would say it is not exactly true. More time means more wear on spindle bearings. I do not care for the "last 10%" but I do care to "remove unnecessary 50%".
This is why I am going towards a high speed spindle (read a Bosch router) as a spindle add-on, by the way.
I may be proficient with manual milling (well, not much, but for example sake), but with a manual mill I just turn handles, I do not really know what my feedrate it.
The high speed spindle will be of use for some things, such as engraving text and markings on signs and control panels, but you'll still be using your main spindle for most stuff. You're pretty much going to be operating the main spindle at it's top RPM for most things and calculating your feeds based on that RPM. Not very many tasks will take you below top RPM.
I'm pretty sure that's correct. The feed rate to maintain the desired chip load varies with RPM and number of cutting edges, the end mill diameter isn't part of the equation for the feed rate. The end mill diameter affects SFM as well as chip clearance and end mill rigidity.
4 flutes taking 0.012" cuts each and turning at 3,000 RPM is 144 inches per minute. 4 flutes * 0.012" chip load = 0.048" material removal per revolution * 3,000 RPM = 144 Inches per minute.
2 flutes at the same RPM is half the feed rate (but has more chip clearance), 1 flute would be 36 IPM. 0.012" chip load is mid range for aluminum and as the book notes can go much higher with machine HP and rigidity.
Note that they indicate (like all the other charts) that the figures are a starting point and may be increased or decreased based on other factors. They just appear to have a more conservative starting point.
I would also note that you should be avoiding using carbide tools while you are learning since they are a lot easier to break, and you can't turn the spindle fast enough to really benefit from carbide anyway.
My handy Mcdonnell-Douglas feed and speed calculator (slide-rule type) has a figure for feed per tooth for different workpiece materials. then you multiply this figure by cutter diameter. So, divide by 4 for a 1/4" end mill. I've just taken this pretty much at face value and it has worked pretty well for me.
For aluminum alloy, it gives .020" per tooth for face mills, .013 for "arbor" mills, which I guess means horizontal milling cutters, and .010 for end mills.
SFPM for "aluminum alloys" they recommend 600 up for HSS and "Max" for carbide. For Inconel, they recommend 10-20 for HSS and 50-70 for carbide. There are a bunch of values in between. The machines they use there are quite a bit bigger than your (or my) machine. I went to some auctions, and they had ROOMS full of 2" and 3" diameter end mills. Not much use on a Bridgeport.
PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here.
All logos and trade names are the property of their respective owners.