I just read an article/post about feed rates/spindle speeds/chiploads. Unbelievable! You mean the woodworking industry hasn't figured this out yet? Every time someone buys a CNC router they have to reinvent the wheel?
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?
Sorry to be the bearer of bad news but the referenced article is right. I can also speak from experience as to the learning curve you're facing. There is no way you should expect to set up a machine and then start production the next day unless you have plenty of experience. Different machines have different quirks. The same machines are equipped with different hold down systems of varying abilities. Different spindles have their own performance limits. There are the varying qualities of different manufacturers' tooling. Then there is such a wide range of materials, each with their own cutting properties ( all plywood does not cut the same, etc ). Now the end user has to determine the balance between all of these and the cut quality / speed / tooling cost / equation. The issue of chip loading is just about keeping your tooling properly cooled more than anything else and this means longer tooling life. Manufacturers of some plastics will tell you the best results they have achieved by calling their tech departments, but for most wood products it's all about experience.
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...
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:
More flutes = less gullet = lower chip load.
More flutes = better finish (usually, but not always)
Small chips mean less heat dissipation = hotter tool.
Up shear: Right hand spiral, right hand cut (rhs-rhc). This is the standard configuration of the common endmills used in the metal industry, and is very common in ours as well. Provides good chip evacuation and promotes a cool running tool and better dust collection. However, under marginal work holding conditions, such as high feeds on small parts, you run the risk of “jacking” the part up, which will cause loss of holding power > movement of part > lost parts and maybe a broken tool. Also, the upshear may cause chipping or fuzzing of the top surface.
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.
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.
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.
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.
Comment from contributor A:
The proper start point would be to follow pre-established cutting speed and feed fate guidelines recommended for wood. Usually these can be obtained from the tooling manufacturers. Cutting speed is usually given in surface feet per minute.
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.