CNCCookbook: Be a Better CNC'er

 

Chiploads, Surface Speed and Other Concepts

CNC Milling Feeds and Speeds Cookbook

 

Before we get into calculating the best feeds and speeds for your goals, there are a few more concepts we need to understand.

Chipload: Chip Thickness per Tooth

While feedrates are specified in length units per minute, the more important measurement is something called "Chipload". Think of a chip as looking something like a comma in cross section, or perhaps an apostrophe. One starts big and gets smaller at the end. The other starts small and gets bigger at the end. We'll ignore that difference for a moment, though it is important as we shall see later.

Chipload is a measurement that is independent of spindle rpm, feedrate, or number of flutes that tells how hard the tool is working. That's a very useful thing, as you could imagine. Hence, manufacturers and machinists typically like to talk about chipload for a particular tool.

You can see that a tool with more flutes (cutting edges) has to be fed faster to maintain a particular chipload. Since each tooth is going to take a cut every rotation, a tooth has only a fraction of a rotation in which to cut a chip that reaches the chipload thickness. During the time it takes to rotate the next tooth to start cutting, the tool has to have moved far enough to shave off a chip that is thick enough. Hence, tools with more flutes can be fed faster. A 4 flute endmill can be feed twice as fast as a 2 flute, all other things being equal.

Why do Tools Break from Too Much Chipload?

You can imagine that forces simply become too great if a tool tries to take too much "bite" by having too much workload. This can chip or break the cutter.

But there is a second issue that comes from too much chipload--the chips get bigger and eventually can't get out of the cutter's way. Beginning machinists probably break more tools because they don't get the chips out of the way fast enough than because the force of the feed is breaking the tool. If the cutter is down in a deep slot, the chips have a particularly hard time getting out of the way. We use air blasts, mists, and flood coolant to try to clear the chips out of the way, but if they're way down a hole or slot, it makes it that much harder, and we have to reduce speed.

Making matters worse, chips always take more room once they're chips than the equivalent weight of material takes as a solid. The only place they have to go is gaps between the flutes of the cutter. Of course, the more flutes we have, the less space there is in the gaps. Can you see the point of diminishing returns coming? In fact, some materials have a tendency to throw off such big chips that we prefer 2 or 3 flute cutters instead of 4 flutes. Aluminum is a good example.

Performance Recipe: Cheating on the 2 Flute Rule for Aluminum and Going to More Flutes Elsewhere

Many beginners are taught to use a 2 flute in aluminum for chip clearance, but must we always use 2 (or perhaps 3 flutes) for Aluminum and never 4? Now that we know why fewer flutes must be used (chip clearance), we can think effectively about when we might not be restricted to fewer flutes. In general, when you have plenty of room for the chips to escape, you can use a 4 flute cutter, and you'll get a better surface finish.

How much is "plenty" of chip clearance?

Forget slots and plunging. Those are the worst cases. Try to avoid tight inside corners or interpolated holes whose diameter is at all close to the tool's diameter, those are nearly as tough. But what if we are profiling around the outside of a part and there's no concave curves, only convex? Tons of chip clearance there, so have at it. If you have a sufficiently roomy pocket, you may also get away with a 4 flute, especially if you can open up a big hole in the middle of the pocket to get started in.

The best case for more flutes is when you have a finishing pass, particularly if you're already committed to changing tools to get the best possible surface finish from a newer sharper tool that hasn't been roughing. The finishing pass will be very shallow and the rougher will have opened up plenty of room for chip clearance. Consider using 2 or 3 flutes for roughing followed by 4 flutes for finishing in materials like aluminum. In harder materials that don't need so much chip clearance, tools with as many as 10 flutes may be used.

This doesn't just apply to aluminum either. More exotic tools are available with 5, 6, 10 or more flutes. Experienced hands will tell you that if you're profiling (where there's lots of chip clearance) steel and aren't using 5 or 6 flutes, you're leaving money on the table. Let's run the numbers in G-Wizard. Suppose we're profiling some mild steel--1020 or some such. We're going to profile the outside of a part, so there's plenty of clearance. Cut depth will be 1/2", cut width 0.100", and we'll use a 1/2" TiAlN Endmill. Here are the numbers:

- 4 Flute: 3158 rpm, 29.8 IPM. MRR is 1.492 cubic inches/minute. A little over 1 HP.

- 5 Flute: Same rpms, now 37.3 IPM. MRR = 1.865. 1.3 HP. That's 30% faster cutting.

- 6 Flute: Now 44.8 IPM. MRR = 2.238. 1.6 HP. 60% faster than the 4 flute case.

How much more profitable are your jobs if you could run them 60% faster? The cost to do so is a more expensive endmill and a tool change for profiling. Harder materials can benefit particularly well because they're already up against surface speed limits. More flutes is the only way to get faster feeds.

Sometimes we have to go the other way too. If you've got some really sticky stainless steel that's giving you fits in tight chip clearances, try a 3 flute instead of a 4.

Rubbing: When You're Feeding too Slowly (aka I'm a Beginner, How About if I Just Run the Machine Super Slow?)

I've mentioned several times now that feeding too slowly causes "rubbing". How does that work?

Consider a magnified view of your cutting edge versus the material:

Rubbing from too little chipload

Two chiploads: Top one has chip thickness > tool edge radius. Bottom one has chip thickness < tool edge radius and will rub...

In the diagram, the cutter edge radius centerline travels along the yellow lines. If the radius is too large relative to the depth of cut (bottom), all the force goes to pushing the chip under the edge. This is the "rubbing" effect you'll hear talked about when feedrate and hence chipload are too low.

Tool manufacturers will tell you that too little feed is just as bad for tool life as too much feed (or too much spindle rpm). But how little is too little? That part is seemingly hard to find out. I went fishing around with Google to try to find what speeds and feeds result in a "burnishing" effect with tools. Here is what I found:

- Article on hard milling: 0.0008" per tooth is definitely burnishing because it is "less than the edge hone typically applied to the insert."

- De-Classified 1961 Batelle Institute report on aerospace machining of super-alloys says an IPR less than 0.0035 will result in burnishing and likely work hardening of these alloys. Interesting how well this number agrees with the one above for a 4 flute cutter. 8 tenths times four would be 32 tenths.

- Kennametal says the "highest possible feed per tooth will usually provide longer tool life. However, excessive feeds may overload the tool and cause the cutting edges to chip or break." So feed as fast as you can until you start to chip or break edges. They reiterate this under work hardening. One wonders whether rubbing leading to work hardening isn't the principal risk of cutting with too-low chiploads with respect to tool life in susceptible materials.

- Another reference, like the first, to keeping chiploads higher than tool edge radius. In this case, IPT should be greater than 0.001". This is once again an article on hard machining where work hardening may be a factor.

- Minimum chip thickness is 5-20% of the cutting edge radius. Below that level, chips will not form and the cutter will "plow" across the workpiece causing plastic deformation and considerable heat.

- Ingersoll says that as a general rule carbide chiploads should not be less than 0.004" or you run the risk of rubbing which reduces tool life and causes chatter.

- Chip Formation and Minimum Chip Thickness in Micromilling uses a figure of 20 micrometers for edge radius on micromills, which is about 0.00079". They go on to show that the rake angle becomes extremely negative as the chipload falls below the edge radius and conclude that there is a minimum chipload below which the cutter will not cut. It varies from about 0.2 to 0.35 times the radius for various kinds of steel.

- The Rutgers research paper, "Micromilling Process Planning and Modelling for Mold Making" uses a figure of 1 to 5 micrometers for micromill edge radius, which is 0.000039" to 0.0002".

I take away two things:

1. If you cut too little, you run the risk of work hardening if your material is susceptible to it. That will wreck your tool life if you are over-stimulating work hardening. Imagine tossing a handful of hardened chips into the path of our cutter--that can't be good!

2. Aside from work hardening, if you're cutting much less than the cutting edge radius, you're rubbing and not making clean chips. That will heat the tool and material and drastically reduce tool life.

Figuring out the work hardening part is easy. If your material is susceptible, keep the chipload up at manufacturer's recommendations and don't fool around. Figuring out the whole cutting radius issue is harder. Most of the time we don't know what the cutting radius is. I'm not talking about tip radius on a lathe tool, for example. I'm talking about the actual radius of the sharp edge. In other words, the smaller the radius, the sharper the tool. A lot of carbide inserts are pretty blunt. A chipload of less than 0.001" may very well be too little. Modern tools for aluminum are often much sharper, and can take less chipload. In general, indexable tools are usually less sharp than endmills, so they need higher chiploads.

It's ironic that just when you think you are taking it easy on a cutter with a very light cut, you may be doing the most damage of all due to rubbing.

Why chance it though? Use a calculator like G-Wizard to figure out how to deliver the manufacturer's recommended chipload by increasing the feedrates. Not only will the job go faster but your tooling will last longer.

Radial Chip Thinning (aka I'm an Expert and I ran the Machine too slowly without even knowing it)

Would you believe that especially for light cuts, the basic math combined with SFM and chipload tables often gives results that are wrong and radically increase the wear on your tools?

The reason is that there is more going on here than meets the eye. For example, if I poke around various endmill manufacturer's literature in search of speeds and feeds for steel, I can get to a page like this one from Niagara cutter. First thing to note is that the recommended chiploads and SFM vary depending on the exact operation being performed, and in particular, the depths of cuts. If you're just using the basic shop math around SFM and chipload, no such compensation is available. I have built compensation like this into my G-Wizard Machinist's Calculator, but trust me, it isn't so easy just to do it by hand. You'll be constantly referring to pages and tables, or to Excel spreadsheets.

Let's try an example based on doing some peripheral (edge) milling to profile a part made out of mild steel using a 1/2" uncoated HSS 4 flute endmill. We plan to take fairly shallow finishing quality cuts of 5% of the cutter diameter. Further, let's do a pretty deep cut axially, a full cutter diameter of 1/2". So if I am profiling a 1" high part, I can make a full pass by going around twice and cutting 1/2" each time.

What feeds and speeds should we use?

The Niagara page says for cuts less than 1/16 of a diameter (5% is 1/20), we want 210 SFM and a chipload of 0.0035. If I plug all that into G-Wizard, but ignore the chip thinning, I get the following results:

Radial Depth Ratio of 5% = 0.015" depth of cut

210 SFM and 0.0035 chipload gives us 22.46 IPM feedrate and a 1600 rpm spindle speed.

Is that the right speeds and feeds?

Yes and no. It's certainly what the majority of folks would use. In fact, they might even be less aggressive than that if they're trying to be conservative.

Let's see what G-Wizard would suggest by default and why:

For the same depth of cut and cutter, G-Wizard wants a little slower SFM of 160, and a little less aggressive chipload at 0.003.

The spindle speed works out to be 1200 rpm due to the lower SFM, but the feedrate is now 84.69 IPM--nearly 4x the original values.

How can we go so fast?!??

Unfortunately, avoiding the rubbing problem gets harder, even for experts, because of a phenomenon known as "Radial Chip Thinning." With chip thinning, you can be making a cut and following all the recommended chiploads, and still be rubbing. The cut above, 1600 rpm at 22.46 IPM will almost certainly wind up rubbing. The reason is that due to the geometry, when your radial engagement, the cut width looking down the axis of the tool, is less than half the diameter, the chips that come off are actually thinner than the basic formulas everyone learns in machinist's school predict.

A picture is worth a thousand words when understanding why:

Radial chip thinning

The blue chip is a shallower cut. Note how thin it is at its widest compared to the red chip from a deeper cut...

The blue chip represents a very shallow cut, and the red chip a deeper cut. Note how thin the blue chip is at its widest compared to the red chip from a deeper cut. You can see that the chip gets thicker all the way up to the point where we've buried the cutter to 1/2 its diameter. That's the thickest point.

Chip thinning simply answers the question, "How much faster do we have to go so the maximum width of the blue chip is the recommended chipload?" Because we're just trying to get back to the recommended chipload, chip thinning isn't about going faster in the sense of higher MRR's. You will see your machine going faster, sometimes a LOT faster, but chip thinning is about avoiding rubbing that will dramatically shorten your tool life.

Many manufacturers publish tables that suggest how much faster to feed based on the % of cutter diameter you are cutting. A good machinist's calculator, like G-Wizard, will factor in chip thinning automatically. Unless you never cut less than 1/2 the diameter of your tool, you need to make sure you're adjusting your cuts for chip thinning or you're probably wearing out tools prematurely as well as not taking full advantage of the material removal rates the tool is capable of.

Surface Speed: How Fast the Tool Slides Against the Workpiece While Cutting

When specifying the operation of a tool, surface speed goes hand in hand with chipload. Just as chipload is a better way to talk about feedrate because it is independent of so many factors, surface speed is a better way to talk about spindle rpm. Imagine that instead of a rotating cylinder with cutting edges, your tool was a flat piece of metal slid against the workpiece. The recommended speed to slide when cutting is the surface speed. Here's the visual:

Definition of Surface Speed

Visualizing Surface Speed...

Surface speed is measured in linear units per minute: feet per minute (SFM) for Imperial, and meters per minute in Metric.

You can't really cheat on Surface Speed. It is what it is and exceeding the manufacturer's recommendations is sure to reduce tool life fairly drastically except for some very special HSM cases you should only worry about when you've mastered the beginner and intermediate speeds and feeds concepts.

The Interaction of Surface Speed and Spindle RPM

Consider this table which shows tool diameter versus surface speed at 10,000 rpm:

Surface Speed vs Diameter at 10,000 rpm...

If we keep rpms constant, Surface Speed is directly proportional to diameter. The 1/16" endmill at the bottom is travelling 1/8 as fast in terms of Surface Speed as the 1/2" endmill at top. Hence, to achieve a given Surface Speed, small tools will have to spin faster and large diameter tools will have to spin slower.

 

Next Article: Calculating Feeds and Speeds

 

Try the Free Trial Version of G-Wizard Speeds and Feeds Calculator...

 

No credit card required--just your name and email.

CNC Milling Feeds and SpeedsContents

 

Featured Articles

Step-By-Step Guide to Making CNC Parts

CNC Router Cutter Types

Why Use a Single Flute Endmill?

Step and Servo Motor Sizing

The Truth About Tool Deflection

10 TIps for Router Aluminum Cutting

2 Tools for Calculating Cut Depth and Stepover

CNC Machine Hourly Rate Calculator

Special Purpose CNC Calculators

Feeds and Speeds Guide

CNC Cutter Guide

Feeds and Speeds By Material

G-Code Tutorial

Sales, and Special Deals

 

Feeds and Speeds:
Made Easy.

Try G-Wizard

 

GCode is complicated.
G-Wizard Editor
makes it easy.

Try It!

 

 

Do you want to be a better CNC'er?

Get Better Tool Life, Surface Finish, and Material Removal Rates.

 

Start Now, It's Free!