Question
I am a CNC programmer for a furniture manufacturer. I have been with the company since '89 and have been programming for them since '93. We currently have 4 CMSs, 2 Heians, 2 Biesses, 1 Cambell, 1 Weeke and a CNC laser cutter. We use Mastercam Mill 8 Level 3 for the routers and laser. We program our Biesses on the floor and use Woodwop 4.5 on the Weeke.
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
1/4" sc - 18k / 75imp - .50" mdoc
3/8" sc - 18k / 100imp - .50" mdoc
1/2" sc - 18k / 125imp - .50" mdoc
3/4" sc - 18k / 150ipm - .88" mdoc
3/4" se - 18k / 175imp - .88" 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.
Forum Responses
From contributor S:
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.
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.
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.
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.
.250 feed to slow go 250 imp
.375 " " 500 "
.500 " " 750
.750 " 1000
If you are going in the serrated, use a rougher 3 flute - much quieter and lasts longer.
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 )
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.
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).
