Feed rates and spindle speeds
I have recently come under fire for the feed rates I program our machines at. I cut everything from 1/4" thick 5 ply back panels to 5" thick ash, oak, maple, etc. crown rails. I cut a lot of 7/8" thick parts, which are mostly 5 ply and lumber banded. These parts have a chipcore center with poplar lumber bands all the way around and are then laid up with veneer face, lebanite, core, lebanite and poplar veneer back. I usually rough cut these parts out in one depth pass with a 3/4" serrate cutter at 18k rpms / 175 ipm. Then I finish cut them (take 1/16" more) with a 3/4" 2-flute finish cutter at 18k rpms / 150 ipm. I have obtained feeds as high as 600 ipm with 3/4" serrate cutters while relief cutting profiles and at times, I have had to cut the same cutter to 75 ipm when trimming cross grain thick hardwoods.
I would like some feed and speed recommendations for solids for different cutters in different diameters, to see where we stand. I know the tool sales reps will give you this, but they are salesmen. I want to hear from people who are actually cutting wood. Here are some of the standard cutters we stock and the feeds and speeds that I have Mastercam set up to post out.
1/8" sc - 18k / 50ipm - .25" mdoc
Is there a formula for speeds and feeds for various types of materials depending upon tool diameter, number of flutes, chip load, tool material, climb cutting vs. conventional, tool geometry, etc.? We have good vacuum and I want to maximize the performance of these machines. I do not, however, have time to stand out at the machines and optimize each program as we currently have over 10k of them. I need to be able to do this during the programming phase.
You and I can tell more from watching the chips and listening to the machine than a salesman can from his formulas. I tend to run most 1/4"-1" cutters at 15,000 rpm and range from 100-300 ipm. My operators are very used to using the % dial and will make program adjustments as necessary.
We very seldom dull a cutter because of run time. We usually run a cutter from wood to MDF, then resharpen it before we have to use it for wood again. We have a handful of diamond cutters that we conserve as much as possible.
Don't get me wrong - we don't waste money on cutters. But when the main concern is quality, I will sacrifice a cutter to get it.
Bottom line is your feeds and speeds sound in the ballpark to me. Formulas may give you a place to start experimenting.
From the original questioner:
I found out last night that one of our driver cads is fading in and out on us. I am having a new one shipped here tomorrow - maybe this will help some. One other note - I am using Bobcad to design and code write. My controller is made by Microsystems, and my router is made by CNC Router Corporation out of Florida. I cannot always change the direction of the cut. Some things it will only cut clockwise and others only counter clockwise (sometimes it will cut any direction). It likes to turn an arch into a circle. Tooling guys tell me to practice.
The short answer is chip load. RPM x #flutes x chipload=feedrate.
Rpm depends on material, tool diameter, and tool geometry. #flutes depends on material, tool and material thickness. Chip load depends on tool geometry, desired finish, material, and sometimes, available power.
Higher rpms means more heat. Higher chip load means better heat sink effects. Higher chip loads may degrade finish, but too low a chipload leads to burning and short tool life.
From the original questioner:
I would like to hear more on the chip load formula. Do you not take depth and width of cut into the formula? I would say 85% of the parts I run come to me at 1" over finish length x width. I will size and trim these parts to ensure that they are square.
We went from 6 tennon machines to 2 in the past couple of years. Tennon machines just can't cut as square as a CNC router. We are a very high quality furniture manufacturer and we sell our product on quality.
I have around 3000 custom profiled router bits that I use - how would one determine feeds and speeds for these? I have some background in a metal working job shop, and speeds and feeds mean everything on a lathe or milling machine, and I know the formulas will get you real close, but even then you have to do some fine tuning. I would be happy to get that close to max feeds and speeds with a formula on a router, because there is a much greater margin of error.
From contributor M:
We don't run many hardwoods, but I cut 1.5 pb laminated 2 sides with 1/2" cutter at max feed (472 ipm) and 17,000 rpm with no problems in one pass. The only tool I've broken in over 1 year since we bought the machine was a 1/2" diamond about a week ago. I was cutting some trespa (like solid surface/epoxy resin) 1" thick. I was cutting 5/16" deep 1/2" wide at 100 ipm/18k rpm. It was an already used and abused tool before I did that. It had no problem at 80 ipm. I'm never afraid to push the limit and lose a part or a tool. Then you know your limits and can learn from them. Push them today, learn and make more money tomorrow!
From contributor S:
Contributor M, I don't agree with your "push them today, learn and make more money tomorrow" philosophy.
Remember, pushing the tool also pushes the collet, which pushes the toolholder, which pushes the spindle. Which can cost big money to rebuild. I hope you save the money you make in increased production so you can pay for rebuild service. There's something to be said for being cautious and slowly finding your limits. We have a 6 year old and a 2 year old and have not had a single spindle problem. I'll stick with my "steady productivity and low down time" philosophy.
From contributor M:
I don't live by the rule, but I do push things to the limit. I know some people down the road with the same machine. They had to rebuild their spindle in less than a year because they always went straight down into the material (when you should ramp in) with $5 cutters that had no cutting edges on the bottom. I'm aware of some of the stresses caused by cutting. We run mostly 3/4" material and I don't have a problem running max through that. I do take some time to find my limits at first - I just try to make that time as short as possible. Trust me - I don't want to rebuild anything any sooner than I have to.
From contributor G:
First, save some money on your tools by reducing the diameter to 1/2" on the rough cut. The formula for chip load that was provided is what this is all about. I am not sure why you are doing 2 passes, as one will do the trick. Your .125 cutter feed and rpm are okay.
.250 feed to slow go 250 imp
If you are going in the serrated, use a rougher 3 flute - much quieter and lasts longer.
From the original questioner:
No one has said anything about depth of cut. I never go deeper in one pass than the diameter of the cutter. Does anyone else have any depth of cut standards?
Contributor G, if the chip load formula is the answer, and if all the cutters you mentioned above were all 2 flutes, would not the feed speed be the same on all the cutters? Why are you giving me different feeds for different diameters? I really want to know. Does the chip load ability go up with an increase in cutter diameter? If so, why is that not a part of the formula?
I feel that the chip load formula, by itself, is not sufficient. Through all this I see myself creating my own feed rate and spindle speed formula. After I compile some information and add my 13 years of "sawdust-making experience" to it, I hope to come up with something like this, and these are just a few of the factors that come to mind.
(part finish factor) x (material hardness factor) x ( depth x width of cut ) x ( direction of cut factor, conventional or climb ) = chip load
(cutter dia) x ( # flutes ) x ( cutter geometery rating ) = spindle speed
feed rate = (spindle speed) x (chip load) x ( # flutes )
From contributor G:
Diameters make a difference. A small diameter tool does not have rigidity (.125 vs. a .750). So, on a smaller diameter you require a higher rpm, so as not to put undue force on the tool, or breakage occurs. The chip load assists in chip removal. If you create fine dust in cutting, this means your chips are being cut not once but 2 or 3 times. The chips dissipate the heat away from the cutting, resulting in a better edge finish and longer tool life. Again, this depends on tool design. What may work in your facility may not work down the street, due to collet/spindle run out, moisture/humidity in material vacuum, and so on. As for depth of cut, you are removing more cubic inches of material, so you may be required to slow down the feed speed and rpm's. The diameter, the style and whether it is an up or down shear tool determines if you can do your machining in one pass. The key here is to have the cutting length of the tool close to the thickness of material being machined. There are really a lot of variables when selecting the correct tools.
The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).
In order to determine the right feedrate it is necessary to know the max chip load diameter of the tooling and the physics of the material. Regardless if you drill, saw or router material it comes all back to splitting the material with a wedge. Whenever you drive the wedge (sawtooth) into the material you apply pressure and cause the material to split in advance of the tooling. In order to acheive a good cutting result you need to be faster with your tool. Most hardwoods (oak, maple and so on) split with a speed of 40m/s to 60m/s. That means your cutting speed needs to be faster than that in order to get a good result, therefore your cutting diameter and the specific wood physics determine your cutting speed. You also need to consider the geometry of your tooling, especially profile bits, since your chipload gets smaller toward the center of the tooling. Your feedrate is dependant on the max chipload and the number of cutters your tool has. Assuming you have two fluted 1/2" low kick back tooling (max depth of single cut is 1.1 mm) and you want to machine a groove into solid oak, I would start out as follows. 12'000 rpm, 20 meters/minute feedrate, that way I cut faster than the wood splits (76 m/s) and the max depth of each single cut would be 0,75 mm.
In metal machining, and from what I read it is much the same in wood, we concern ourselves with the SFM of the cutter (furface feet per minute) that is calculated (RPM X Cutter Diameter X Pi)/12 because the answer will be in inches, and you want surface feet. You get the same result with (RPM X Cutter Dia. X .262). The problem as I see it is your material is not as predictable as steel, cast iron, etc. Chip load is the key. If your chip is too light, you are just rubbing the material off. You need to cut the material. So the chip load must be sufficient to keep the heat down. Heat kills the cutting edge in any material. If you are getting a burnt edge anywhere, kick up the feed rate (IPM). Some machines slow down on radius cuts due to the calculation speed of the processor. You may need to increase the feed in the radius cuts. Or slow down the RPM to match the speed loss - this will help tool life.
Also, it is important in metal machining to make sure you are climb milling so the thickest part of the chip is at the entry point of the tooth. This will keep the heat down and help chip formation. We normally machine steel in the 500 to 700 SFM range, so with a 1" cutter that would be around 1900 to 2000 rpm using a 4 flute cutter at a .005 chip load. We move at around .02 per rev or 38 to 40 inches per minute, so you can see we run a lot slower but create a lot more heat. In aluminum we too use diamond cutters and reach speeds on lathes up to 10,000 SFM in milling we usually run out of RPM but machines are getting faster every day.
I am a carbide tooling saleman and I usually suggest starting on the low end of reccommended speeds and feeds because we want to be succesful. Once we see how the material and cutter are doing along with the work holding, we speed up from there. But it's all about tool life in metal cutting. SFM and chip load determine that in metal cutting. All our carbides are rated for a certain SFM and we have a different carbide for every material from non-ferrous to cobalt chrome (nasty stuff to machine).
Would you like to add information to this article?
Interested in writing or submitting an article?
Have a question about this article?
Have you reviewed the related Knowledge Base areas below?