Speeds and feeds thoughts

I found this site quite interesting:


There are others like it, of course. What struck me is that to have optimal chip load on our machines, it is difficult to use a 1/4" bit. It would appear we would be better served to drop down to 1/8" bits for everything as we can’t achieve a high enough feed rate to hit the optimal zone for two flute cutters.

While we can and do scale down the calculations to adjust for our machines, it doesn’t mean that the equation scales down really. Has anyone done deeper chip load calculations?

Also interesting to note that the site recommends the lowest RPM possiblel, which also helps reduce the required feed rate. But even at 10,000 RPM (bottom for the Makita), with a 2 flute 1/4" bit the recommended feed rate range is in the 5500 mm/s (220 ipm) to 6600 mm/s (260 ipm) range.

If you drop down to a 1/8" bit at 10K RPM then you get a range of 2032 mm/s (80 ipm) to 3048 mm/s (120ipm) for approximate optimal chip loading.

It appears a lot of us may be running our RPMs too fast for the feed rates of the machine and the size of the bits we are using. The site doesn’t mention depth of cut, but I think it’s fair to assume the fairly standard practice of 1 x cutting diameter, as you normally apply a reduction factor for deeper cuts from the starting calculation.

Has anyone else gone down the detailed calculation hole to get a sense of what the sweet spots might be using industry standard calculations on the Longmill? The challenge with the 1/8" bits is we can’t get enough length to cut through thicker material, like 1" BB.

Amana does have a OD 2 1/2" bit with a 7/8" cut height in a compression configuration: https://www.toolstoday.com/v-13354-46170-k.html so I’m wondering if that may not be the sweet spot (the insane almost US$60 price tag aside).


@jwoody18 An interesting and confusing subject to be sure, Jeff; at least for me.

Looking at that calculator, it does not take into account pass depth. It just talks of “material thickness of average size for cutting edge length of the tool”. That tells me that they may be saying that a 1/4" bit, with a flute length of 1" would cut 3/4" material in one pass if their calculations were followed. Am I reading that correctly? (The Biesse at the shop does that all day.)

I would not attempt that with the LongMill. Also, I am obviously using much too high a speed on the Makita for the feed that I am setting. That said, I get good finishes on all sorts of materials, including corian, acrylic, mdf, and all sorts of hard woods. I am very conservative, though in my pass depths.

Here is another chip load calculator and it takes into account cut depth. Using it and running the Makita at its minimum, I get calcs well within their recommended loads.


With all this said, I am still confused. :grinning:

Thanks for the additional info and load calculator. You’re not the only confused one. There is a lot of information, and a lot of bad information, out there about feeds and speeds. In the year and a half I’ve been delving in to this I’ve rarely gotten the same answer twice about the topic.

One of the more knowledgeable people I spoke with at length mentioned that the hobbyist temptation is to go really shallow and think you’re saving your bits from wear, when in fact that often accelerates wear. Being designed to operate at a certain cutting load, putting all the work on the first few mm for eample may not be the correct approach for the endmills - especially those at 1/4" and above. It’s all about flute engagement, apparently. But I’ve not been able to find tools and references that make sense to me yet.

There is a lot of conflicting information and it’s hard to know whether these can be “scaled down” to non-industrial machines like ours or the only correct path is to scale down the bit diameter so the formulas still work correctly. That’s something I’m going to try and dig in to over the weekend.


Grant, what inputs are you using? Maybe I’m doing something wrong.

I need to go to 6 Meter/second at 10K RPM with a 2 flute to get a chip load in the correct rante (.012) for a 1/4" bit in Softwood/Plywood (Their range is .011-.013). Am I misunderstanding?


{Edit: I see Amana does have a single flute 1/4" Compression option, and with a single flute 3000 mm/s gives a good chip load. Maybe that is the ideal tooling? https://www.amanatool.com/46140-cnc-solid-carbide-compression-spiral-single-flute-1-4-dia-x-7-8-x-1-4-inch-shank.html)

@jwoody18 If I enter 200 ipm at 10000 rpm with a 2 flute bit, I get a chip load of .010. That is pretty much in the range of a 1/4" bit in the materials that they list. If I take that up to 300ipm, I get a load of .015, which is still in the range for mdf and not far out for any of the other materials other than plastic.

I never looked at the metric inputs.

I put in your 6 metres, but remember, it is metres per minutes, not metres per second. So, your 6 metres per minute is 236 inches per minute - very close to my example of 200 ipm.

Doh, that is likely my issue, I’m failing to accounting for the time adjustment. Off to do more math. :slight_smile: thanks for pointing that out to me, I just translated 6000 M/s in to 6000 mm/s without thinking. D’oh.

@jwoody18 If you can get your Mill to move at 6 metres per second, Jeff, I’ll assume that you bought the optional turbo for it and I’ll be so jealous. :grinning:

1 Like

Apparently I have a turbo, a magic carpet and a token for a free sundae too…

PS - At 6 M/s aren’t we likely supposed to use KM/H to measure it? :slight_smile:

1 Like

Wait, I’m going around in circles. Material typo aside, the question still stands. If we can’t run a Longmill at 200 IPM / 5,000 mm/s then we can’t really use a 2 flue 1/4" bit, since even at 10K RPM we can’t feed it fast enough. I think that’s right?


[EDIT: Found a feeds and speeds chart specifically for the Amana compression bits on their site, which assumes a spindle RPM of 18,000 and shows feeds that may be a bit more within reach. Check it out here: https://www.toolstoday.com/media/wysiwyg/attachments/feed_and_speed/Solid-Carbide-Compression-Spirals-v4.pdf)

So with their 1/4| compression they are saying 110 ipm / 2,800 mm/minute in plywood at 1x tool diameter. So a little less if the mortising end is taller than 1/4" which it is usually just a bit bigger.

1 Like

@jwoody18 Jeff: I must admit that I have likely spent more time looking into feeds and speeds as part of our conversation here than I have doing actual projects since I got the Mill. That is not in any way to be critical of your concerns. So far, I have looked at this differently. I use 1/4" shank bits when the project paths let me since I figure that they are more rigid and less prone to breaking than 1/8" bits. (In my router table, I use 1/2" shank bits when I can, instead of 1/4" for the same reason.) Before getting the mill, I don’t remember even knowing the term “chip load”.

I set my feeds in the tool database in VCarvePro. I tend to be conservative. Then, when running the job, I generally increase them on the fly in UGS. I listen to the bit cutting and, based on my incredible hearing and knowledge of metallurgy, I reduce or increase the speed as the job continues. :grinning:

So far, that plan is working out pretty well. The finish on my cuts is acceptable and I am not breaking or burning bits. Nor am I burning the wood.

I can understand the argument that deeper cuts may be better for the bit since the cutting is not always concentrated on the end 1/4" of the bit. That makes a lot of sense. However, we must also take into account the stress on the Mill of cutting deep in one pass. I don’t pretend to know or to be able to measure that. However, when I look at the shear bulk of the components of the Biesse at the shop, compared to our hobby machines, it seems logical to me that my Mill cannot plow through 3/4" material in one pass all day, day after day, like the Biesse can.The same holds true for the Makita router’s capabilities compared to the humongous spindle on the Biesse. So, if I dull bits somewhat faster than necessary because I take shallow passes, I’ll accept the consequences and costs of that decision compared to the possible costs of pushing the capabilities of the Mill or the Makita.

I had better get down from my soap box now before someone pushes me off.


Just about all of the places to look up feeds and speeds give you a starting point, not an exact measurement. Even the tool I use (purchased) does that, but gives me a very good starting point.

It all boils down to the ideal chip load for the material; everything else is calculated from that with restrictions place on the power available from the spindle, the stiffness of the machine, the strength of and chip load capabilities of the bit being used, the maximum allowable deflection of the bit, and quite a few other factors. With that many variables, one table just isn’t going to give you other than a range of feeds and speeds. Most experienced CNC folk use whatever they have to get close and then tune it by ear.

I’m not that experienced that I can tune it by ear, so depend on the software (GWizard Calculator) to give me the best I can get. If it still sounds off to me after using that, I’ll make adjustments.

To the depth of cut, that depends greatly on the bit being used. Obviously, a 1/8" bit will not be able to tolerate the forces that a 1/4" bit can and it’s not a linear relationship. The real limiting factor is the deflection of the bit; too much and you risk breaking the bit and, even if you don’t, a far less than ideal surface.

There is a “sweet spot” in feeds and speeds where you get the best finish and speed of work. This differs based on the material. Typically, the harder the material, the smaller the sweet spot and the need to be closer to the “ideal”. Other factors come into place with some materials, such as aluminum. If you aren’t near the sweet spot, you risk the aluminum chips welding themselves to the bit and a broken bit as a result.

The actual chip load for each bit depends a great deal on its geometry, so two 1/8" two-flute carbide bits may differ quite a bit in their capability just from that fact. Most manufacturers will give a table of the chip load for each of their bits.


1 Like

I hear you on that, my question was more one of the math and science of it all. It does seem like the Longmill would hit the more optimal range for many bits, especially compression bits, if they were only 1/8" in diameter. However, the trade offs in likely breakage and even handling may make that unappealing.

I was more broadly asking the question whether there is an science of math reason that you can scale the the speeds and feeds from industrial machines down substantially, as we are doing, or whether it results in falling outside optimal cutting ranges and using smaller bits would be more optimal. I’ve not actually found anything so far that says you can materially scale down the optimal feeds and speeds ranges to the point where you run at half the speed and half the cut and should expect similar results. I think it may simply not apply.

Agree, my point was more that there seems to be a range of even 1/4" end mills that are probably not appropriate in any optimal way for our smaller machines. I hadn’t considered that before really digging in to this and I can’t seem to find too much information on the topic. I really like my compression bit but if I end up running it at half of it’s optimal settings, what does that do to it’s life span and quality of cut? That’s the key question I’m trying to get my head around. Conversely, would I be better off with a 1/8" compression bit running at optimal speeds and just being careful handling it?


If you want read up on some of the intricacies of how feeds and speeds are calculated, I’ve mentioned G-Wizard before. The author has a tutorial that can be found at https://www.cnccookbook.com/feeds-speeds

He’ll have several plugs in it for his own software, but does a reasonable job of describing how the many factors go into getting the correct feed and speed.

I hope it’s OK for me to post that URL, but I’ve found it educational.

One of the take-aways I got from it is that smaller machines that aren’t as rigid as the commercial milling systems actually do better with 1/8" bits because either the spindle cannot be slowed down enough or the feed cannot get high enough to get into the sweet spot unless a smaller bit is used (1/8", for example, instead of a 1/4" bit).


1 Like

@jwoody18 As I’ve said before, Jeff, I find the whole question very interesting, but somewhat frustrating, too. I could, I suppose, use only 1/8" bits in order to get my tool paths creating the optimal feed rate. For profile cuts, that would work well, I think. However, for the mouldings that I am doing, or for pockets, not only would it take forever at 10% step overs, but I wonder if the finish would be as good. I don’t know the answer to that, of course. Maybe, I’ll do some experimenting. When I do 3D models, I typically use a 1/4" ball nose bit with a 10% step over for the finishing pass. That’s a very small step over - .025" - but it yields a very smooth finish. A very quick sanding with 220 grit and I can apply finish.

Thinking as I type, I guess using a 1/8" ball nose with the same 10% step over - .0125" - should yield the same quality finish. It will just take twice as long. I can accept the time penalty, as long as I get something out of it - like a better finish.