Origin/consistency of chipload recommendations

Just as a comparison, since I am trying to test this open-source cutting calculator @WillAdams found and pointed out (Bryan Turner’s Feeds and Speeds Calculator). Here is what it comes up with:

Julien’s 6061 T6 Aluminum
Link to Calculation
Chipload = 0.00075 (set by Julien)
Power (HP) = 0.00891
Tangential Cutting Force (lbf) = 0.12
Axial Cutting Force (lbf) = 0.63
Unit cutting power (HP/in^3) = 0.33

So the tangential cutting force seems low compared to the other calculators. Otherwise fairly in line. Also, it might be due to the unit power being off (which you can define yourself as a custom material.)

1 Like

Try 0.22 for unit power. Update: Just noticed that those Axial and Tangential cutting forces labels are apparently swapped (transposed)!

Unit power is the key and the hardest thing to get “right” - apparently even for metals, which have been published for years in machinists’ handbooks. Likely because those values are dependent on the cutter and how its used as well as the material. Take a look at Sandvik’s website if you dare. IMO Kennmetal does the best job of making its calculation user friendly and accurate. They make cutters and provide useful/reasonable speeds and feeds recommendations for their use.

That’s why it makes more sense to monitor cutting forces and/or sound as shown in this video or spindle input power as shown in this video.. Measuring forces is hard/expensive, sound is easy if the spindle is quiet enough, measuring input power is easy and inexpensive (adequate Chinese versions are available inexpensively from Amazon).

1 Like

@gmack, well thank you sir for pushing me further down the rabbit hole, just when I thought I started to get a hang of this chipload thing, now I have a whole other aspect (power) to take into account :slight_smile:

Seriously though, do you mind dumbing it down for me and explaining how these power-centric estimations should be taken into account in the overall process of determining optimal feeds and speeds ?

My earlier approach was (obviously) chipload-centric, and “just” aimed at making chips that are thick enough to manage heat, while still being compatible with the Shapeoko capabilities (once depth of cut etc are added in the mix). I have not even considered optimising MRR or pushing power to the limits of what the machine can do, and I would be very interested in complementing my somewhat naive approach with these power considerations…and what to do with these values.

Your insights will be much appreciated (and sorry if you did explain that earlier and I missed it!)

p.s. : the aluminium I used for the test cut mentionned above was in fact 2017A T451. It is surprisingly hard to find affordable 6061 over here.


Look for 6082, it’s very similar to 6061 and should be way more readily available in the EU. If you’re looking for 6061 (USA), go for 6082 (EU), if going for 2024 (USA), then 2017 (EU) is what you’ll find. In my day job I work for a European company that sources parts made in both the US and Europe. I spend good chunks of my day making sure that materials (alternates) are compatible with designs that come from different engineering groups around the globe. Those grades of aluminum are what I deal with most.

Edit/note: 2000 series and 6000 series aluminums are very different animals.



Thank you Dan, that is quite helpful. The reason I went for 2017 is

a) because this local French site sells cheap 2017 scrap cuttings, so I can experiment without thinking twice about wasting material

they also have 7075T6 and 5083h111

b) the wiki has these statements:
" AU4G (2017) is really good at machining : you can take deep passes (~0.3 to 0.5mm) at something around 500 to 800mm/min (20 to 23 ipm). This aluminium will resist to the heat and won’t melt."

“7075 also gives good results when milling, but is difficult to cut on a Shapeoko”

“5083: Tough, strong alloy with excellent corrosion resistance, however not easy to machine”

Can you elaborate on the pro’s and con’s of 2000 vs 6000 series ?
What about 7075 & 5083, do you agree with the wiki ?

7075 T651 (plate form of T6 sheet) is strong tough stuff, usually a bit more expensive than the others, but if you need high strength that’s the stuff. 5000 series is easily formed, but not super strong, and “gummy” to cut. 5000 series is work hardened (H designation, H32 for example) rather than tempered (T6 for example), so I suspect part of the reason it gums is the work hardening that’s caused by machining. I’ve never machined it to be honest, I’ve only ever used the sheet variety for making tv stands and drip pans when I was in the Navy, it’s not really used in aerospace as far as I know. 2017 is probably going to be more expensive on average than the 6000 series alloys from my experience, but if you’re getting usable drops for cheap then it’s a good choice. So to sum it up 7075 strong, a little tough to work with, expensive. 2017 a little cheaper, fairly strong, nice to work with. 6061/6082 not as strong, cheaper, easier to work with. 5052 great if you’re using sheet goods and making non-structural parts(I wanna say it’s popular for small watercraft, from memory), not fun to machine, work hardens. Even after doing this for many years it’s still strange to me that availability of these isn’t worldwide, but they aren’t. Like 2017 stopped being widely used in the US when 2024 came around (1930’s I think, again from memory), but the rest of the World kept using 2017?

Here’s a couple links with some decent info if you’re bored:

This is my favorite for understanding aluminum tempers


And this website has a database that will allow you to compare up to 3 materials with free membership (just requires an email address and they won’t send you a ton of junk mail):


The engineersedge website has so much info you could really find your rabbit hole there, I use it all the time;)



Great info, thank you. I’ll stick with 2017 then, and look for 6061 drops when they are in stock

1 Like

Plugging data for 2017-T451 Aluminum into the Kennametal calculator for your cut gives 0.682 lbf cutting force and 0.0081 HP (6 Watts) cutting power and 0.30 HP/cuin/min unit power. I need to think a little more about how best to answer your other questions. But, this stuff is all new to me, so I’m certainly no expert (not a “sir” either). I’m just a retired engineer trying to understand this stuff.

1 Like

Here’s another calculator that requires user entry of material unit power. It doesn’t show bit deflection or tangential cutting force (which equals its “Spindle Torque (in-lb)” / cutter diameter (in) / 2). But, since it shows the formulas and steps through them in a straightforward manner as information is entered, it might help demystify the calculations involved. (No “high level math” or “artificial intelligence” is needed). Controlling bit deflection is important to keep from breaking cutters. Lower cutting forces, larger diameters, less stickout, and stiffer cutter materials (like carbide) reduce deflection. No “high level math” is required to calculate it either.

@Julien and @Everyone
Here’s my thinking on chip-load and speeds and feeds issues. But, likely most - all of you folks have lot more experience than I do - so please don’t hesitate to ask questions or voice your disagreement (or agreement). Lets all talk about it! You won’t hurt my feelings and I apologize in advance if I unintentionally hurt yours.

  1. I don’t understand how large chip-loads are required to remove heat when cutting - especially when cutting thermal insulators (non -metals). Even with metals, cutting larger chip-loads takes more power and likely generates more heat to be removed by the chip. So, that may well be counterproductive.

  2. I also don’t understand the implied argument that larger chip-loads are required to prevent rubbing if the cutter is too dull for reasonably sized chip-loads (apparently - 0.001" for starters). Using dull cutters is wrong for so many reasons especially if they’re pushed harder in an attempt to compensate!

  3. Ideally all cutter manufactures would be as contentious as Kennametal apparently is with their cutter and speeds and feeds recommendations,, but?

  4. Due to power and/or rigidity limitations, some CNC routers may not be capable of satisfactorily realizing the cutter manufacturer’s speeds and feeds. To compensate, either depth of cut (DOC), width of cut (WOC), or feed rate can be reduced. Reducing feed rate (or increasing spindle speed if not power limited) reduces chip-load, which likely increases cutter life because it maintains the manufacturer’s recommended cutter wear and heat distribution while reducing heat generation. Decreasing WOC would have similar effects. In contrast, only decreasing DOC likely decreases cutter life because it has the opposite effect.

  5. I found this informative.

There - I feel better now :slightly_smiling_face:

For 1 and 2 please see: https://www.cnccookbook.com/chip-thinning-rubbing-lesson-3-fs-email/

1 Like

think of it this way, you’re keeping in mind how much time the edge is in contact with the material. flute goes in then spins out and cools off while it circles around to make another cut. less time in material = less heat. usually you have low radial engagement but increased sfm/rpm to maintain or sometimes increase chipload. @WillAdams link goes into more detail about chip thinning as well

dull cutters are always bad. not sure how that pertains to chipload but you def want to keep from rubbing. if your cutter isn’t cutting big enough chips it is generating excessive heat. dull or not.

1 Like

Your linked response for 2. says " 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 chip load of less than 0.001″ may very well be too little. Modern tools for aluminum are often much sharper, and can take less chip load. In general, indexable tools are less sharp than endmills, so they need higher chip loads." and " – 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″. There seems to be a consensus among experienced users that 0.001 inch (or less for smaller endmills) is a good starting point.

I didn’t see anything in the link about thermal insulators (point 1.)

Thanks for the feedback!

Please see the chart at:

(which I thought was included in the link I cited)

Doesn’t the linked “Rubbing: When You’re Feeding too Slowly” argument imply that duller cutters require higher chip-loads?

That link says “Feeds and Speeds Calculator for Wood and CNC Routers
For CNC Woodworking applications, a good Feeds and Speeds Calculator needs the following features:
– A detailed wood database to fine tune Feeds and Speeds by wood species.” Where can we find that?
There is still no explanation of me point 1.

Each chip carries away heat — smaller chips have less ability to carry away heat.

the image in the link @WillAdams attached expresses it well?

if you’re not making a (large enough) chip because the cutter is dull then you want to increase the chipload and get a full scoop of mass that can carry some of that heat away. otherwise your cutter is getting carpet burn on the material - just rubbing and adding heat. it’s still spinning along into the material but heat is no longer being carried away by a chip.

same reason why most people burn out drills prematurely - they want to make a hole through a material fast so they crank up the speed and have it burn up rubbing and not creating a chip. feeds and rigidity play factor in this but it’s the heat that kills the bit

1 Like

How can the thermal insulators “carry away heat”? Doesn’t making bigger chips generate more heat since it requires more cutting power?

“if you’re not making a (large enough) chip because the cutter is dull then you want to increase the chipload and get a full scoop of mass that can carry some of that heat away.” So, push harder?

“same reason why most people burn out drills prematurely - they want to make a hole through a material fast so they crank up the speed and have it burn up rubbing and not creating a chip”. Harder materials certainly require lower speeds, feeds, and procedures. I’ve ruined both HSS and Cobalt (M42) drill bits (they turn purple - not black!) by not using cutting oil when drilling stainless and hardened steels. But, I’ve never ruined a drill bit, table saw blade, bandsaw blade, router bit or endmill cutting wood, plastic, or Aluminum. Have you/others?