Chip Load and Tool Diameter
Experts and operators discuss the relationship between bit size, chip load, RPMs, and feed speed when machining various materials on a CNC router. August 29, 2006
Question
All the chip load formulas given in the Knowledge Base reference number of flutes, spindle speed, and feed rate; shouldn't it reference tool diameter as well? I am trying to compare two tools of different diameter. Does a difference in tool size matter?
Forum Responses
(CNC Forum)
From contributor J:
I believe the short version is "no." The RPM is the same regardless of the tool diameter. For a given spindle speed (RPM) and time, a 1/2" 2 flute tool makes the same number of cuts that a 1/8" 2 flute tool makes.
As for the second question, I would use the smallest diameter that will work without breaking the tool, because a smaller tool has to remove less material than a larger tool. I would think that for a given feed speed, a larger diameter tool requires more power than a smaller one.
From contributor M:
Spindle speed for a cutter is derived from the cutter manufacturer. Commonly the term "surface footage" or SFM ("surface feet per minute" is used. Surface footage is more commonly used in the metal industry where tooling rpm's are more critical (and significantly slower) for machining various different materials. Essentially, it is based on all things being equal (material used to make bit, material to be machined, proportional depths of cut - ratio or percentage of the diameter deep) *except* the diameter. This is the reason if you buy a form cutter to machine a molding style feature that the cutter has inserted cutting inserts and the diameter of the cutter is 4.5" inches, usually there will be a recommended speed somewhere on the cutter. (I will almost guarantee you will be significantly less than the 18k-20k that most people run their .5" carbide compression bits.)
Another way of looking at this is say you have two different bits, both same substrate carbide, both with same edge and flute geometry, and the depths of cut remain proportional to the diameter, etc. But one is a .5" inch and the other is a .25" inch diameter. To over-dramatize this, I will apply a very low surface footage as if I were machining aluminum on a machine with marginal coolant supply.
Let's say the manufacturer told me that under my machining conditions, I could machine with each of the cutters at 1200 sfm. The formula used to determine RPM for a cutter using manufacturer's recommended surface feet per minute is:
RPM = SFM x 3.82 / tool diameter
My rpm for each cutter would be as follows-
1/2 bit
1200 x 3.82 / .5 = 9168 rpm
1/4 bit
1200 x 3.82 / .25 = 18336 rpm
The intent is to maintain a constant material removal rate. Therefore, all else being equal, smaller diameter cutters will run at a higher rpm than larger diameter cutters. And this is not the only consideration. Machine, setup and tool rigidity are huge factors in this. And the smaller diameter tooling usually can not handle the chip load of a larger diameter cutter due to the inherent rigidity.
Unfortunately, the problem that CNC routers face is that, and this is significantly different than working with CNC Mills (metal working), the majority of materials you will machine stay within a bandwidth that you can usually comfortably run the same rpm for the same cutter types in MDF, LDF, some composites. Then you usually only have to worry about RPM's when your material changes rather dramatically (hardwoods, aluminum, etc). Routers also tend to be much more forgiving of errors in consistent surface footage. In actuality, someone could be running an "off" speed and feed, yet they think they are doing okay because the tool wear is relative to what they have always gotten.
I know this is a hard concept to grasp, and because the majority of people only machining wood fall within the forgiveness zone, it really is never a consideration. However, if you start talking to your tooling supplier in terms of "what is the rated surface footage" of a particular tool, you may be able to determine a little more how this effects tool life, consistent tool wear, etc.
From contributor M:
P.S. I am not a tooling expert. But... even though a 1/2 diameter cutter and a 1/8 diameter cutter both turning at the same rpm will take the same number of cuts, the furthest most edge of the 1/2 diameter tool will have traveled peripherally 4 times farther than the 1/8 diameter tool. It is cutting on a .25 arc or swing while the 1/8th diameter cutter is only cutting on 1/16th (.0625) arc or swing. This is the basis of constant surface footage.
From the original questioner:
Wow! Thanks. But you'll have to bear with me. So I am cutting 0.25" thick paper phenolic, I have a 3/8" roughing bit recommended to me by my tooling supplier. Where do I find the recommended SFM? The tool is cutting okay now. I am running it at 18000rpm at a 472.5 ipm feed rate (I know it's a slow feed rate, but the machine is from 1997). Phenolic is definitely a harder material than any wood products, so am I still in the safe zone or should I try something else?
From contributor M:
You would need to contact the manufacturer or tooling distributor and say "I have a 3/8 (.375) diameter carbide (or material cutter is made of), number of flutes (2,3,etc.), model number (if known) of yours. I am cutting phenolic (grade and type if known) and want to know what the recommended surface footage is to run this tool at a 1/4"(.25) depth." They should be able to give you a response like "1100 surface feet."
At that time you would ask, "What is your recommended chip load for this tool, in this material, under these conditions?" They should respond with some value, say .0045 per flute. Then you plug the surface footage into the formula. Take the answer and multiply it by the number of flutes multiplied by the chip load they recommend. Remember it is a starting point, but should be a very good ballpark.
From contributor J:
I am curious as to applicability of the "constant surface footage" concept to cutting wood and wood products (and phenolic) with a router bit. As you mentioned, "surface footage is more commonly used in the metal industry." Isn't the mechanical action of cutting metal entirely different than that of cutting wood and wood products? Also, isn't the tool diameter already allowed for by the manufacturer's recommended chip load? For example, if you examine the Onsrud chip load per tooth chart for cutting MDF, you will find that for the same tool, the chip load varies by the diameter. Thanks for your insight.
From contributor G:
Formula to determine chip load:
(feed speed IPM divide by RPM)/ (# of cutting edges).
Diameters on the tooling will effect the feed speeds (surface feet), formula:
(SFM)=RPM x dia. x .262
Contributor J, a smaller diameter tool will not last as long as a larger diameter. As you go up by .125 diameter, the tool is 50% stronger; smaller is not always better.
Contributor M made some excellent points.
To the original questioner: you are using the correct tool, a 3 flute ruffer. I know ours can achieve quicker speeds, but without knowing part size, I am assuming you are in the ballpark. As I do not know the brand of tool and the substrate they use, we could not recommend the tool you are using to the fullest.
As a tool manufacturer (Courmatt), we always suggest the feed speeds to our customers. Otherwise the tool you purchased will not work to its max performance and tool life.
From contributor E:
Consider one other factor, and that is not all spindles are designed to handle phenolics. Even spindles from the same manufacturer rate differently. I cut some phenolics using a Columbo spindle, which is not rated to cut phenolic material, thus I need to be more careful with the feed speeds. These slower feeds tend to burn up cutters quicker.
From contributor J:
"Contributor J, a smaller diameter tool will not last as long as a larger diameter. As you go up by an .125 diameter the tool is 50% stronger; smaller is not always better."
That's why I posted "smallest diameter that will work without breaking." I agree that one shouldn't simply use the smallest tool available. But are you saying the smaller tool won't last as long because it isn't as strong and it will break sooner? Or did you mean that the cutting edge will last longer because of the larger diameter?
From contributor G:
The smaller diameter has less of a gullet to remove the chips from the cut. On a larger diameter tool, we increase the size of the gullet to allow for more chip removal. 80% of the tools we manufacture are .500 or under. Sometimes you have to use a smaller diameter tool based on what you are going to machine. The #1 reason a tool breaks, regardless of diameter, is due to improper feed speeds vs. rpm's.
From contributor H:
In regard to the tool diameter, I know when I am looking at the Onsrud catalog, the chip load is referenced by the tool series. If you look in the back, they will call out the material and the series used for that material. So say I am using their 2 flute compression #62-123mw, then I find the material that I am cutting listed, and look for the series number of the tool I am using. I follow the lines across and it will give me the recommended chip load for that tool and diameter. Based on that number, I will then crunch the number for the feed rate. (# of flutes)(rpm)(chip load), then I usually drop it by 5%. So number of flutes on my tool, 2, recommended chip load for my tool is .016, and I run my CNC at 18,000 rpm with my 5% reduction, looks something like, (2)(18,000)(.016)(.95) = 547.2 ipm.
From contributor K:
Is the formula for surface feet a minute in the woodworking industry applicable? I ask because it seems like the woodworking CNC world is just based on opinion. I know there are formulas out there for chip load to find rpm's and feed rates, but you still have to guess on a number. I have researched the metal working field and it just seems like they have a system in place. If they know the tool and metal, they can find the sfm and then use that to find rpm, then use the chip load and rpm to find the feed rate. This has been an ongoing discussion among vendors and employers since I started in this field.
I am really not looking to start any fights, just looking for information so I can gain a better understanding of how all this works, so I can set up standard libraries for cutting hardwoods, plywood, MDF and plastics. We are a high end millworking company in New England that makes custom windows, doors, radius moldings, and casework. There is no limit to the millwork we do here, so the machine is constantly cutting new materials.
From contributor G:
Surface feet in metal is standard. As we market to the metal industry, COURMATT uses this standard. In the CNC wood, plastics, etc, we rely on chip load and the size of the chips. See info for the size of chip on our web site. The type of products that firms machine in this industry are in the hundreds, from exotic woods to different manufacturing of PB, different densities, species, moisture content, humidity in different parts of the country, etc. In the metal industry, there is no moisture content and metal is by far a more consistent product than wood.
We have a database, based on 25+ years in this business, on the types of tools and cutting edges used to machine these parts. We receive new material parts to be machined on CNC's every week. Based on the material, density and composition, we try (I say try) to assist our customers on the correct tools, along with feed speeds vs. rpm's, to machine the material.
My fellow competitors use a chip load for this industry as well. They may have come up with a different formula since we last spoke, but I would hope they share any new info, as we all can make this industry better.
