Determining CNC feeds and speeds
I recently began to really ponder the chip load equation and am asking the same question as the originator of that post. Why doesn't the depth of cut and diameter of the cutter figure into the chip load equation? (I read that the larger diameters relate to a larger chip load and lower spindle RPM - to understate this, that is not very specific!) Also, according to the tables I'm looking at for plywood, the chip load can be anywhere from .015-.030" with the RPM anywhere from 9,000-16,000. This puts the feed rate anywhere from 562 IPM to 1440 IPM. That is one heck of a range... Where is a guy supposed to start? Especially a brand new programmer like myself. I don't have any experience with CNC routers but I'm in charge of setting this up. The best information says to start at "safe" speeds and rates and gradually creep up until the finish suffers or the bit breaks. Like I have time for that (or the experience and judgment to go with it). I need to set this up tomorrow! What the heck do these tooling companies do with all these studies everyone has already done? Surely there is better information than "try it til it breaks." Please tell me I don't have to experiment to find out about something I'm sure thousands of people have already been through.
I can accept generalities of feed rates and spindle speeds for certain materials, diameters, etc. but the answers given in the post are not generalities - they are windows - and very large ones at that. Surely someone can point to a table that puts all this together?
That's right, it's pretty much trial and error while you're learning. I used to reference the Onsrud website because they have quite a bit of information on chipload and feeds and speeds, but it still all comes down to experience from learning, breaking bits, and edge quality.
From the original questioner:
This sounds like the old saw I heard when I first started looking for a job years ago. "Ya can't get a job without experience and ya can't get experience without a job."
I'm not looking for tight specs here. (Although that would be nice.) I would like to get in the ballpark. Can someone tell me where to find whether (given the above example) inputting the midrange values for a 3/8 inch three flute compression cutter will work for 3/4 birch ply, say 12,500 RPMs and feed rate of 562 IPM? I've got to start somewhere...
From contributor E:
I understand your frustration; been there, done that.
To provide starting points, I will make some assumptions.
You are using a production sized router, and 12 hp or better. You are using a flow through vacuum system, and are using prudent vacuum management techniques. You are using industrial tooling, *not* Menards Clearance specials.
Bear in mind that desired finish, tool brand/geometry, etc will heavily influence feeds and speeds.
Will your example of 3/4 birch ply, 3/8 compression tool, 12500 rpm and 562 ipm work? I would say yes, but a 0.015 chip load in a cut twice as deep as wide will pack pretty tight. If you are looking for a fine finish, I would say no, chip load is too high, and birch is prone to fuzzing under even good conditions. If all you need to do is bust up work, then yes, *if, if, if* the machine is rigid, the tool holding system (collet, tool holder, spindle, spindle slides, etc) are clean, tight, rigid, and accurate. If you are using a Porter Cable 3 1/2 hp hand router, forget it. The better the machine and tool holding system and the work holding system is, the harder you can push the tools.
Your best bet for specific recommendations for specific applications is to specify the project parameters, just like your example. Then, whoever has run that material and thickness can say what their personal experience is. That will be your best starting point.
I do not run your example parameters, but I do run 1” thick marine grade plywood (untreated) on a regular basis. I use a 1/2” compression tool at 16500 rpms and 885 ipm as my starting point. With a fresh, new tool, I may go to 1100 ipm, same rpms, full parting cuts. Sometimes I use a 3 flute slow helix tool in this product, and will run the feeds up a little more, but get a lot better finish. If I am running light periphery cuts, 1/8 to 1/4 wide, 3 flute cutter, 20000 rpm and around 1300 to 1500 ipm. When I run aluminum, 1/4” plate, I rarely get over 200 ipm even at 20000 rpm.
You will find that some products require very specific tooling, and very specific feeds and speeds that will be specific to your machine. It sucks, but that is the way it is. Aluminum, acrylic, and many plastics fall in this category.
Here are some of my considerations:
Larger tools have less peak-to-valley variation in the mill marks, so larger chip loads provide approximately comparable finish quality to smaller tools with lower chiploads. Larger tools generally have more gullet space per flute, and it is not linear. A 1” tool will have more than twice the gullet space of a similar design 1/2” tool (this is my observation, not a statement of fact).
Deeper cuts (thicker materials) cause more tool deflection, require more horsepower, generate more heat, and generally pack the chips behind the tool more, which can be merely annoying in oak, to catastrophic in acrylic.
Deep cuts on small parts may result in part vibration, so chip load is no longer the determining factor, but rather cutting force imparted to the part, and possible vibration and / or movement of the part will degrade the finish or eject the part.
Choosing feeds and speeds for a given material will be dictated to a fair degree on tool selection.
Tool selection considerations and guidelines:
Number of flutes:
Down shear: Left hand spiral, right hand cut (lhs-lhc). This is a popular geometry used in our industry to help keep the parts on the table, as a part of the cutting forces imparted to the material being cut are directed *down*. This geometry has the same shearing advantages of an up spiral, but is very prone to pack the chips into the cut. A down shear tool will also erode the spoilboard quickly as the chips are literally ground against it. This may or not be a big deal. Your situation will dictate.
Compression geometry: The tip of the tool (usually about 1 diameter) is up shear (rhc-rhs) to provide good surface finish for the bottom of the part in both NBM spoilboard environments as well as P2P or elevated work environments. The rest of the tool is down shear (rhc-lhs) which provides a clean top surface cut, and promotes work holding. This tool packs the chips about as bad as a down spiral, but is much friendlier to the spoilboard.
No shear: This is what most brazed tooling (carbide tipped) is. These are usually more economical to buy, and may come in any variety of profiles.
Brazed tooling is often designed with 5 to 15 degrees of shear, comes in many profiles, can be custom ordered for special profiles, is (usually) easier/cheaper to buy and to sharpen.
This has been rather long winded, so I hope that you found at least some directly useful information, but the subject you address is just not easy to put into a simple formula. Each wood species has certain characteristics which influence several of the principle parameters, which affect the final solution. Nonferrous materials like aluminum or acrylic are more predictable, but also more finicky about each parameter.
As you have probably noticed, several machine tool manufacturers and tool manufacturers/vendors visit this site. I do not make or sell CNC routers; I use them in my CNC router job shop. I do sell router tooling, and I use what I sell, so I do have some direct experience, and advantages over some vendors of tooling.
One thing to consider. Depending on the spindle (not a hand router), if you drop the RPM's below 12,000 you are behind the power curve and you can't maintain RPM. Some of the newer 4 pole motors are rated at 9,000 RPM so this is not a problem, but on the older units, this is a problem. Also on the smaller units running single phase inputs, as you overload the motor and the inverter is putting out max power, you will blow that 20 amp breaker. Just my experience.
From contributor E:
I should have added this tidbit of advice to my previous post. When you are machining, you can discern a lot about the cut by the sound the tool is making in the cut. The most basic fundamental rule is this: The quieter the tool is in the cut, the better. Some other guides, which you will have to develop an ear for, are: If the tool squeals, you are either spinning too fast or going too slow (or a combination). If you hear the tool growling at you, then either the rpms are too low, or the feed is too fast.
This is not so easy as it sounds (pun intended), because up spirals sound different in the same situation than down spirals, so expect to have to learn to interpret the sound by more than just these three basic guides.
I have found that trying to teach this technique to others is very challenging., which surprises me as my hearing is not the best to begin with. Some people are very adept at sound differentiation, and others must rely on other methods.
I noticed a typo in my first (long-winded) post in the paragraph regarding down spiral tools. I used "(lhs-lhc)" which would mean Left Hand Spiral-Left Hand Cut, which is actually a valid upspiral tool, you just spin it left handed. I should have used "(lhs-rhc)" as I did while describing compression tooling. My apologies.
As a tool manufacturer, I tend to agree with the above explanation. At COURMATT, when a customer has a new product to machine, we provide them with a starting point, usually within 10% of optimum running speeds. Always remember you want a chip to take the heat away from the cutting edge, longer tool life. A chip load between .015-20 is usually what we recommend. With a shorter up shear (.200) for dado cuts you will actually be loading up the chips on the perimeter, because of the longer down shear. I am amazed that a lot of the newer pieces of CNC equipment want to go faster and faster. But take the parts that you are cutting out - if it's a cabinet (nesting) you are not going to machine on average 1600 IPM, as it takes time to accel and decel. I have seen the fastest machine travel at 900IPM even though it's programmed at 2000IPM.
I'm going of the subject… With your 3 fluted tool, run it at 800 IPM at 16000RPMs. As mentioned, this will get you in the 10% range and you will not break the tool.
In New Zealand we run the CNC machine between 18000rpm and 24000rpm depending on diameter. Try running a 3 fluted 1/2" at 24000rpm with a feed rate of 20 meters per minute.
I have two suggestions for you. First off, I would call the CNC router manufacturer. Most router builders would be more than happy to try and help their customers. I would assume that the company that built your router has an in-house applications engineer who can give you tooling and programming assistance. That's a good place to start.
Then I would try to find a list of customers who have the same brand of router as you. Oftentimes they have taken some bumps and bruises that they can help you avoid with your machine. You can also ask them about their success with their own tooling and spindles.
We cut a lot of Baltic birch and hardwood going with the grain. We can run 1200-1500 ipm and get good finish but across the grain we will use a small scoring bit, slowly, about 400 ipm, 18000 rpm and then hog it with a 1/2". This works well for me.
The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).
Comment from contributor A:
To find rpm: RPM = CS/Dia.*3.82
CS is cutting speed, Dia. is diameter of tool and 3.82 is a constant. Then you can calculate feed rate using the recommended chip load. Your example was .015-.030. I usually start at the mean.
To find feed rate: FEED= RPM* Chip load* number of teeth.
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?