Feeds and Speeds, Cutting Tools & Surface Finish for the Mill
CNC Cookbook Milling Feeds and Speeds Cookbook
This page is being replaced by the Milling Feeds and Speeds Cookbook which is greatly enhanced and expanded with new material. It has the most comprehensive and up-to-date information on feeds and speeds, surface finish, tool life, and material removal rates for milling operations.
Getting the best possible surface finish on the milling machine covers a lot of ground. We'll start with a checklist and then expand on some of the areas:
Feeds and Speeds: Appropriate feeds and speeds for the material, cutting conditions, and tooling are paramount.
Chip Clearing: Recutting chips contributes to poor surface finish and increased wear on the tooling.
Workholding: Achieving maximum rigidity is key to the best surface finish.
Tooling: Different tooling yields different surface finish results in many cases.
Toolpath Considertions: There are a variety of toolpath considerations such as climb versus conventional milling that will make a difference to surface finish.
In this article, we'll go through some CNC Cookbook recipes from each of those categories for selecting
the right cutting tool and achieving a decent surface finish with it.
Feeds and Speeds
Getting the appropriate feeds and speeds for your workpiece material, tooling, and cutting conditions is the most important first step. Consistent speeds and feeds will make a huge difference in your surface finish as anyone who has switched from hand cranking to power feed will attest. Getting the right speeds and feeds is just as important. Speeds and feeds are complex to calculate if you want to get values as close to optimal as possible.
There are lots of feeds and speeds tables available from tooling manufacturers, and they often show ranges. The ranges are because they can't account for all the variables in tables. Better information sources will provide multiple tables for different conditions. For example, the tables provided by Niagara Cutter take into account slot versus peripheral machining (which goes to cutter engagement), coating type, and depths of cut relative to cutter diameter. That's better than many other manufacturers in terms of helping account for the variables involved, but there are even more variables to consider. For example, peripheral versus slot machining only assumes two conditions. It would be nice to smoothly interpolate a full range of radial and axial depths of cut. There are many other considerations such as chip thinning, and each different tooling type has its own peculiar considerations. For twist drills, there is a whole series of rules about when peck drilling is needed, when the hole is deep enough that a parabolic drill should be considered, and so on.
Here is a quick video course in feeds and speeds for machinists (I hesitate to say a "crash" course!):
It's a 10 minute video that covers things like chip thinning, relationship of cutter edge radius to chip thickness for best tool life, ballnose cutter compensation, and a number of other topics associated with feeds and speeds.
There is a tendency to assume that if one is simply conservative, it's suddenly okay to just ignore all those considerations and cutter life will be extended as well. This is based on the idea that manufacturers are there to sell more tooling and want you to run it within an inch of its life using their published speeds and feeds. This is true to an extent, but is a drastic over simplification. No doubt some manufacturers are playing the game of one upsmanship by quoting speeds and feeds that are the highest possible, perhaps too high for their tools. But others know that machinists value tool life as well and will state their numbers more conservatively so that the actual experience of using the tooling is a good one for the machinist.
When compiling the cutting data for the G-Wizard Machinist's Calculator, I accounted for these differences by analyzing no less than 3 manufacturer's recommendations for each tool type, and in more common cases such as twist drills and end mills, I analyzed 6 to 9 tables. I then took the ranges called out by these tables, put the numbers in order, and went with numbers 40% of the way from most conservative to most optimistic. In other words, I erred on the side of conservatism. This results in good numbers that undo most of the over aggressive tendencies yet still yield good machining rates (faster than what most customers had seen before without breaking tools).
Radial Chip Thinning: When Babying a Tool Kills It
Chip thinning makes chipload vary more than expected as depth of cut changes...
Another issue to consider when dialing back feedrates to try to improve surface finish or cutter life is chip thinning. Radial chip thinning is a geometric effect (see the diagram below or read the article) that causes chips to be thinner than the simple feeds and speeds equations predict whenever your width of cut is less than half the diameter of the cutting tool. The differences can be quite astounding, and if you ignore chip thinning while running feedrates too slowly (sometimes even the predicted feed rate is too slow with a light enough cut) you will wind up reducing tool life because the tool will rub instead of cutting. This happens whenever the actual chip thickness is less than the radius of the cutting edge. We're talking about the sharp knife-like edge of an endmill flute, for example. If you visualize such a thin chip, and visualize the cutting edge as being round instead of infinitely sharp, you can see that such thin chips can get under the cutting edge which will tend to push them down into the workpiece. This is like a negative rake tool. Sometimes the effect will result in some burnishing, which can give improved surface finish, but it is usually at the expense of tool life. That burnishing or rubbing really heats up the tool and the workpiece.
Besides chip thinning, there are other geometric effects such as ballnose compensation and lead angle that one should consider to find the appropriate feeds and speeds. Because all these effects are complex to account for with simple tables or calculations, I use the G-Wizard Machinist's Calculator for feeds and speeds. G-Wizard can afford to take a lot more variables into account at the touch of a button.
Lastly, if you have chatter problems, the last thing you want to do is cut back the feedrate. Maintain pressure on the cutting surfaces to help dampen the vibrations. With chatter, try increasing the feedrate first, then reducing it. Chatter is a harmonic phenomenon, which means that the most important thing is simply to move outside the range of feeds and speeds that are exciting the harmonics. A move either higher or lower works, though our human intuition is always to slow down when we hear something scary. Increasing feedrate will increase the load on the endmill which is like pulling a vibrating string tighter to take out the vibrating slack. Likewise, you can try increasing spindle rpm first and then slowing it. If you're near the surface speed limits for your tooling material, you won't be able to go too far with rpm without overheating the tool though.
What About Optimal Feeds and Speeds? Try Cut Optimizer!
If you're machining for a business, you want optimal feeds and speeds. You need to go as fast as you can go without breaking anything and while still delivering adequate surface finish. You can get pretty close with G-Wizard's basic feeds and speeds calculations as described above, but "optimal" implies something a little more to me. For a long time I searched to find an approach to optimizing feeds and speeds. The trouble with optimizing, is you need something to optimize, some cost function. Eventually, I hit on the idea of optimizing against Tool Deflection.
Why Tool Deflection?
It's an ideal metric to optimize because it is something we can calculate (albeit with quite a bit of higher math!) that applies to any machine and that goes directly to the quality of the cut. It applies to any machine because it is largely influenced by your cutting conditions, and the part of your tool that sticks out of the tool holder. It applies to the quality of the cut because too much deflection kills your accuracy and that flexing of the tool is one (the other is flexing of the workpiece) of the engines that feeds the arch-enemy of optimal feeds and speeds--chatter. If your tool isn't flexing at all, then provided your workpiece isn't incredibly lightweight where you are cutting (thin walls on the mill or work sticking way out of the chuck unsupported on the lathe), you won't get chatter. Also, it makes sense that we can allow a "roughing" cut to have more tool deflection than a "finishing" cut and still be okay.
Thus, the Cut Optimizer was born. I won't say more about it here, because you really have to try it to understand just what a revolutionary approach to planning your speeds and feeds can be. Suffice it to say, all those old rules of thumb can't begin to capture the complexity of tool deflection, but G-Wizard can. See the Cut Optimizer documentation page for more information.
It's impossible to get good surface finish if chips are being recut over and over again, especially for softer materials like aluminum or brass. Good chip clearing is essential to both surface finish and tool life. In a slot, where chip clearance is minimal, clumped up chips can jam the cutter to the point where it breaks. When you look at the finish, you can actually see chip marks, which will be irregularly spaced gouges (be sure you don't have a nick on your tool causing them, but chip marks are usually parallel to the cutter flute). Chatter marks will be much more regularly spaced.
Flood coolant or an air blast should be used to clear the chips at all times. They won't clear of their own accord, although the tendency for gravity to help the process along is one reason horizontal mills can be more productive than vertical mills (or lathes too for that matter). The term Flood "Coolant" is in some ways a misnomer. Yes, there is a coolant action as well as a lubricating action that can reduce built up edge, but the primary purpose of the "coolant" is to clear chips. The cooling action itself can actually have a detrimental effect on carbide. Liquid coolant should either be used in copious amounts or not at all for carbide, and companies like Sandvik, in their metal cutting home study course, are starting to recommend it less and less because of the shock cooling effects on carbide inserts and endmills. Insufficient liquid coolant can turn instantly to steam when it hits the carbide, and thus produce little cooling effect while still shocking the tooling material. This leads to premature cracking and wear. Tooling materials like CBN are even more susceptible to thermal shock. The Sandvik recommendation is to either use lots of coolant or none at all for most materials.
It's worth noting that some tool coatings, especially TiAlN (titanium aluminum nitride) actually won't work right with coolant. They depend on high temperatures for their proper function.
For cuts that are set up for proper feeds and speeds, most of the heat should be carried away in the sheared off chip anyway.
If you can see chips piling up in the cut at all, you need more coolant or more air. Some rules of thumb for liquid coolant:
10 gallons/minute per inch of tool diameter
0.5 gallons/minute per HP on the spindle
If enough liquid can be applied, one advantage is that the mass of the liquid can carry away chips better than a simple air blast. Even organizations that are focused on minimizing their use of coolant (which can be as much as 15% of total machining costs for some operations according to Sandvik) may have to use it for certain operations that have poor chip evacuation such as internal boring and deep hole drilling benefit particularly from thru spindle coolant--the more pressure and volume, the better. Milling deep cavities with long-reach tools would be another example. If you don't have flood coolant or thru-spindle coolant, try to avoid large depths of cut. When dry machine, DOC stands for "Death of Cutter."
Aside from cooling the tool, the coolant cools the workpiece. Sometimes this is helpful to accuracy, as a workpiece that heats up is a workpiece that is moving due to thermal expansion. One alternative to liquid coolant is a cold air gun. They work well, but I'll warn you in advance they use a LOT of air, so make sure you have a good compressor that is quiet enough that it won't drive you batty if you use one.
Another advantage of coolant is that it lubricates the tool/workpiece interface. This can reduce built up edge tendencies for sticky materials (like some aluminums). If you're seeing BUE, consider cranking up the coolant. Slow surface speeds (for example, the tip of a ballnosed cutter is so small diameter it doesn't move fast) also benefit from the lubrication effects of coolant because the tool is more dragging across the surface than cutting it in these conditions. If you want the lubricating action but don't want the mess of full flood coolant, try a mist system.
Lastly, some materials, such as Titanium or the high temperature "super alloys", conduct heat very poorly and almost have to have flood coolant rather than an air blast for successful machining. Coolant can also help to reduce work hardening tendencies for some materials.
Assuming you've got the proper feeds and speeds, and you're doing a good job chip clearing, the next thing to look at is workholding. The primary impact of workholding on surface finish is vibration. In the worst case vibration will turn into chatter, which is a harmonic effect that will be very visible in your surface finish. Clearly, the more solid you can make your workholding, the less likelihood of vibration there will be. Make sure your workpiece is supported and clamped over as much area as possible surrounding the cut while still leaving room for the cutter to get in there and do its job. Remember that as you are removing material during the machining process, you are in some sense weakening the workpiece. You may weaken it to the extent that the vise or other workholding fixtures can start to deform the part.
For example, suppose you've firmly clamped a relatively thin piece of aluminum plate flat in the vise. You intend to machine away the middle so it's like a picture frame. The initial slotting pass may relieve enough material that the slot pinches against the cutter with poor results.
Plates are some of the most difficult pieces to machine because they often want to vibrate like gongs. The thinner and more poorly supported the plate, the greater the tendency. Here are some things to consider when machining plates:
- Glue the plate to a subplate with super glue. It releases with heat (careful, the fumes are toxic!) when done. You can also use double sided tape and various commercial products for machinists that are intended for the purpose. Jeweler's wax (sometimes called "Dop Wax") is also good for securing parts as is hot glue. For all of these adhesives, make sure they will stand up to your coolant!
- If you stand a plate on end in the vise or other fixture in order to machine the edge, support the plate as much as possible up to the edge. A pair of 2-4-6 blocks make a great strengthening sandwich around a plate standing on end:
Providing a little extra support for the plate with 2-4-6 blocks...
- Move the vise jaws to the outside so the plate is supported in the middle by the vise:
- In general, keep the unsupported workpiece overhang as little as possible for all machining operations.
Where tooling is concerned, the first order of business is to minimize deflection. The principles are not unlike those for workholding--we're trying to get to a more rigid tool and deflection is one way of looking at rigidity. A tool that is deflecting wants to act like a tuning fork. It will neither leave a good surface finish, nor be accurate. How much deflection is too much? Ingersoll's ballnose catalog talks about just one thousandth of an inch leading to a chatter-prone tool. It's surprising how easy it is to get that little bit of deflection with small diameter or long reach tooling. In fact, the ratio of diameter to length of the tool is a great place to start talking about reducing deflection.
Reducing length to diameter ratio by 25% makes the tool more than twice as stiff so it deflects less than half as much. Deflection is directly proportional to length to the third power (a tool twice as long will deflect 2*2*2 = 8 times as much, all other things being equal!) and inversely proportional to diameter to the fourth power (a tool half the diameter will deflect 2*2*2*2 or 16 times more, all other things being equal!). In other words, use the shortest, fattest tooling possible:
- Consider a toolchange between roughing and finishing. Instead of using the largest tool that fits the smallest radius of the tool path, use an even larger tool for roughing and let the finishing pass deal with the smaller radii. Roughing is where you're hogging the deep chatter-prone cuts anyway.
- Never use a longer tool than necessary. Any length more than 3x the tool's diameter starts to be chatter-prone and by 5x you're wishing for all the help you can get to control the chatter.
- Choke up the tool in the chuck as much as you can.
By the way, the part of the endmill that is fluted is weaker than the solid shank. Use the shortest possible endmills with the shortest possible fluted lengths for maximum rigidity.
Solid carbide cutters are much more rigid than HSS cutters. Hence, even if you're not running them at flat out carbide speeds, they may still produce a better finish. This will be especially true for longer reaches, smaller diameters, and so forth. Incidentally, carbide generally takes a smaller chipload than HSS, but it runs at so much higher rpm that it still comes out ahead.
Last point about deflection: G-Wizard's Cut Optimizer can determine the maximum width and depth of cut within a deflection allowance, such as 0.001" for roughing.
More tooling thoughts:
- Coarser pitch tooling reduces vibration frequency. Lower frequencies are often better damped by your machine tool. The lower limit is 2 inserts. With 2 inserts, you've only got one in the cut at a time. This behaves like a fly cutter and can hammer the work, tooling, and machine.
- When you must use longer reach tooling, heavier feeds at lower speeds reduce vibration frequency.
- Positive cutting geometries will typically require lower cutting forces (resulting in less deflection), and they will produce a finer surface finish. The positive geometry bites into the material's shear planes with less force.
- Prefer sharper inserts. These are often more expensive ground inserts rather than pressed or molded inserts.
Ground CCGT insert with sharp edges...
- High helix cutters leave a better finish. Variable helix cutters break up chatter vibrations because the varying helix keeps the vibration from settling on a single frequency.
- More flutes or inserts are equivalent to a higher rpm. Many older mills are limited on their spindle's rpm. Being able to employ more flutes or inserts can restore some of the advantage. Be sure to consider chip clearance. You shouldn't use a 4 flute cutter when slotting in aluminum (there isn't enough chip clearance), but you can use a 3 flute to slot and it is equivalent to 50% more rpm than the 2 flute. Even better, if you are milling around the outside profile (peripheral milling), there may be plenty of clearance for chips to fall away and you could use a 4 flute cutter on aluminum.
- A counter argument to using more flutes or inserts is that fewer flutes/inserts are less prone to chatter.
- You can sometimes break up chatter on a facemill or other indexable tooling by removing an insert. It is the regular striking of the inserts against the workpiece that feeds the vibration. Taking out an insert means that every so often that regular pattern is broken up.
- Optimize insert geometry: Round inserts are most prone to chatter (but if they are not chattering, the big radius leaves a great finish!), while those with a 45 degree lead angle are least prone to vibration and chatter.
- Read the note below on Climb Milling for Thin Walled Parts. There is a good discussion of the impact of your cutter radius versus the smallest radius on your part. You'll get a better finish if your tool radius is less than your minimum part radius.
Obviously the toolholder has a lot to contribute to the rigidity and vibration dampening of the system. A CAT40 holder is much stiffer than the Bridgeport's R8. Even an NMTB30 has a lot more mass to it than the R8:
- HSK toolholders are as much as 4x stiffer than equivalent sized CAT40 holders. This is mainly due to the dual-face contact of the HSK design.
- The thesis compared the performance of milling chucks, shrink fit, hydraulic chucks,and collet chucks. The most important characteristic for finishing operations is modal stiffness. In order of best to worst performance, here is how the different toolholders ranked:
Tool Holder Type
Surprising that the lowly collet chuck performed nearly as well as finicky shrink fit tooling and quite a bit better than more expensive hydraulic and power chuck-style holders!
However where roughing is concerned, the Dynamic Stiffness is important for suppressing chatter. For maximum material removal rates, we want to maximize Dynamic Stiffness. Here the Collet Chuck also performs pretty darned well, and it is in hogging out lots of material that the hydraulic and milling chuck style holders start to come into their own. The shrink-fit performs poorly because the shrink fit doesn't dampen the vibrations, it just holds the tool very very tightly. Makes you wonder if it doesn't make it more likely to ring like a bell when held so tight?
Other toolholder thoughts:
- Consider balancing your toolholders. It's a requirement for rpms over 10K, but it will smooth vibrations even at lower rpms. Obviously tools like flycutters are inherently unbalanced to start with, or must they be? Perhaps a design that is balanced will produce a smoother result.
- Consider runout. A holder with a lot of runout injects a lot of vibration that will ruin surface finish and ultimately break cutters. Smaller cutters are more sensitive to runout. A thousandth of an inch is a lot of runout for a 1/8" cutter to deal with as it is effectively jerking the cutter around in the cut as it rotates.
- Collets often have less runout than setscrew holders. Some complain they don't hold as well. A compromise would be to use set screw holders for larger shanked tooling (say anything over 1/2") and collets for smaller shanks. OTOH, for those that claim the collets don't hold (tools are getting sucked out), others are claiming the toolholder and collet aren't clean, or the nut isn't torqued down tightly enough. The specs for ER collet nut torque are pretty high, so be sure to give the spanner wrench a good tug. Alternatively, I have been using ball bearing nuts which take surprisingly less torque because they have a ball bearing interface with the ER collet instead of trying to spin against the collet as it tightens.
- Integral shanks are almost always stiffer than inserting a shanked tool into a toolholder.
- Various specialized holders are available such as flatback drives that seat the toolholder against a precision spindle face for more support than the taper alone could provide.
Facemills are a staple for most shops. They're great for squaring blocks and facing large areas. Here are some things to keep in mind when facemilling:
- The best efficiency occurs when 2/3's of the facemill engages the workpiece at a time (67% stepover). This also results in a better surface finish. Full engagement of the cutter keeps the forces on either side of the centerline fighting each other (leads to vibration) as well as starting chips out at zero thickness. Chip formation should start thick and end thin for best surface finish. See the note below on Entering the workpiece ("rolling in") for more on starting thick and ending thin.
- Climb mill with this 2/3's cut ratio. Conventional milling with a face mill causes the chip to start out thin, which sometimes leads to rubbing at the outset of chip formation that is bad for surface finish and can lead to BUE. The best finishes start the chip out fat and then thin it out before the chip releases.
- Take a light cut when finishing: 0.003 - 0.010"
- Keep an eye on the horsepower required for your cut. Facemilling uses a lot of it with surprisingly low depth of cut because the cutter is so wide. A wide cutter relative to the workpiece produces a more pleasing finish (fewer "mow" bands), but too much horsepower can be injected into the cut and will lead to vibration problems. Your horsepower used (or a load meter on your VMC) is telling you how much of this tendency there is.
- Roll into cuts with a face mill as described below under Toolpath Considerations.
- If you don't need a square shoulder, a 45 degree lead angle facemill will often leave a better finish than a 90 degree. Chips are also about 30 percent thinner versus a 90 degree facemill so faster feedrates are possible.
- Where surface finish is the major consideration, use the extra sharp finishing inserts, they make a big difference.
- Recutting or back cutting occurs when the surface that was already cut is cut again by the back edge of the facemill. A perfectly trammed machine cuts on the leading edge only, but perfection only occurs in theory. Slight tramming errors and deflection can make back cutting a reality, and it usually results in a poorer finish. Some machinists will put their machines very slightly out of tram so that the cut is always made on the leading edge of the path. This also helps to prevent chips being dragged around the circumference of the cut which further degrades the finish. Obviously you'd only want to cut travelling in one direction as well. The bias in tram needs to be very slight lest the angle cutter create scallops that are too pronounced. Larger diameter cutters will magnify the scalloping effect.
- "Wiper" inserts can be used to great effect for improved surface finish. A wiper is a flat ground on the insert. It cuts with the leading edge of the flat (which is parallel to the workpiece) and then the "wiper" burnishes the work as it passes underneath. The width of this wiper flat must be greater than the advance per revolution to allow the cutting edges to overlap. Spindle tilt such as was discussed around back cutting is critical when using wipers. Due to the sharp ends on the insert, excessive spindle tilt can cause dig-in.
A fly cutter will often produce
the best surface finish because they allow you to finish a very wide area
in one pass with no overlap marks and the cut has a constant depth. If your face mill has individually adjustable insert heights, you probably won't see a lot of benefit in a flycutter, but if not, you can easily convert a facemill to a flycutter by removing all but one insert, and it is interesting to experiment with the results. Reducing the number of inserts will necessitate a reduction in feedrate, but it may be worth it in terms of improved surface finish.
The biggest challenge with ball nosed end mills of various kinds is slow nose speed. As you get closer to the tip, the diameter on the ball gets smaller and smaller, finally going to zero. As a result, the cutter must perform over a wide range of surface speeds and chiploads at different depths in the cut. Be sure to keep this in mind when using one. If possible, use a feeds and speeds calculator or CAM program that properly accounts for these effects.
Balance the diameter of a ball end cutter versus the rigidity. Remember, the part of the ball near the axis moves slowly. A smaller ball interpolated exposes more of the surface to a faster moving cutter, leading to a better finish. But, the smaller cutter can flex more. Hence the need to balance these two factors.
If you have a 4th axis or 5-axis mill, you can try "Sturz" milling to combat the slow moving tip. See below for details.
Climb versus conventional milling
This has to do with the direction
of the cut and how it relates to the rotation of the cutter. Climb milling
is when the direction of cut and rotation of the cutter combine to try
to "suck" the mill up over (hence it's called "climb"
milling) or away from the work. It usually produces the best surface finish. Here
is a diagram showing climb versus conventional milling for a number of
Keep in mind that
for this illustration, it is the workpiece that moves, not the spindle.
On some machines, like a gantry router, the spindle moves, so the labels
would reverse. I keep it straight by thinking of the spindle as a pinch
roller that can either help move the workpiece in the direction it was
already going (climb milling), or that might fight that movement (standard
or conventional milling).
Most CNC progammers always specify Climb Milling, thinking it is the best approach for all problems. That's not the case. To understand where Climb Milling shines versus when Conventional Milling would be better, see our Climb Milling page in the Feeds and Speeds Cookbook. You'll be surprised at some of what you find there.
Entering and Exiting a Cut
Entering and exiting a cut and cutting in corners are some of the most challenging spots on the toolpath. The way a cutter enters and exits the material can really impact surface finish, vibration, and tool life. Here's a great tip on how to "roll into a cut", courtesy of Sandvik, with a hat tip to Don "Milacron" at the PM Boards. This Sandvik video explains the gist of it:
I'm fascinated by these geometric effects. Chip thinning is another. Isn't it interesting how Mother Nature tends to like circles better than straight lines? Chip thinning, rolling into a cut, and the trochoidal paths of high speed maching are all about the behavior of circles as we try to use them (in the form of rotating cutters) to cut the straight lines that we humans are more comfortable with. Circles are more gentle and natural in these applications. Here is another look at the geometry:
Not the chip shape to the right of the feed line (the red line is the path the cutter follows): thin chips on exit are better!
To execute an entry like this means starting the cutter out one radius to the right of the original starting location and then rolling it in along a path that is an arc with the same radius as the cutter. The folks on PM report that this works as well for endmills as it does for the face mills Sandvik shows in their video. In fact, they say it really helps improve cutter life on materials like Stainless Steel.
Cutting in Corners
Corners are points where cutter engagement goes way up. Consider this diagram, which shows the amount of material the cutter removes when travelling in a straight line versus in a corner:
Entering a corner doubles the cutter engagement...
There are families of high speed machining toolpaths such as Trochoidal milling that involve swinging the cutter through arcs to try to maintain constant cutter engagement. A corner can be processed as a series of arcs, for example:
Toolpath arcs to clean out a corner...
The alternative to these arc movements is to simply slow down the cutter on entry, exit, and in corners. Typically slowing to 50% of the normal feedrate is the right thing to do. Of course, imagine that all of the recommended feeds and speeds tables for cutters are created on the assumption that they have to work for entry, exit, and corners too. If you have sufficient control of the toolpath to slowdown, or cut with arcs to maintain constant engagement, it becomes obvious that much higher feedrates are possible.
Convert Slots to Pockets and Pockets to Profiles
Remember that old fitness saying, "Never sit when you can walk nor walk when you can run?" Here, the equivalent is never to machine a slot when you could do a pocket or pocket when you could profile. What does it mean?
Consider the slot. If the dimensions are right, you could be tempted to cut it in one pass with a cutter of the appropriate diameter. But, your surface finish and accuracy will come out better if you use a bit smaller diameter cutter to go down the middle and then climb mill the outline of the slot as a final finish pass. Surprise, we just converted the slot to a pocket! Why does this work better? Because cutting the whole slot in one go maximizes cutter deflection and also maximizes the number of chips that have to be cleared in one pass. Taking a couple passes allows the latter passes to be finishing passes with fewer chips and less deflection.
What about converting pockets to profiles? This is a relative thing. But, in general, its about considering when to remove more material or when to fixture the work so that what had been a pocket-like operation is more like profiling. In short, its about opening things up to make it easier to evacuate the chips.
Avoid Cutting Down the Centerline
Let's say you're face milling. Don't run your facemill so that each cutting edge goes right down the centerline of the face mill. Doing so means the inserts are hitting the material dead flat, which is the worst case from a shear standpoint. It puts maximum stress on the cutter and bangs around the workpiece. It maximizes the interrupted nature of the cut. bad for tool life, bad for surface finish. This rule is appropriate not just to face mills, but to any milling operation: don't make your cut width equal to your tool's radius. Either go bigger or smaller.
G-Wizard has a "Tips" area that will remind you to avoid the centerline if it comes up.
Plunge Milling and Drilling
For most milling machines, the spindle axis is by far the most rigid axis. In addition, material removal rates for drilling are often much higher than for milling. Hence, plunge milling, where a series of holes is used to rough out a cavity, can produce very high material removal rates.
- Start with a hole that is 15% larger than the plunge tool to provide some chip clearance.
- Use a stepover of 70% of the drill diameter on your plunge tool. If you are using an inserted tool for plunge milling, step over no more than 75% of the insert's diameter or cutting length.
- Don't try to plunge more than 6x the diameter of your plunge tool. 3x is more optimal unless using tooling specifically designed for plunge milling.
As has been discussed, the tool engagement angle goes way up in corners. Consider plunge milling or drilling the corners during roughing to eliminate this problem.
Other Toolpath Tricks
Got a 4th axis, or better yet, a 5-axis machine? Are you doing profiling with a ball nosed cutter? You have an advantage because you can use "Sturz" milling. This is the practice of tilting the cutter or workpiece so that the cutter is not perpendicular to the workpiece. The end of a ball nose is moving very slowly because its diameter is so small. Sometimes it is so slow that the end more rubs than cuts. By tilting the whole process, the workpiece is exposed to the faster moving side of the ball, which results in a faster machining operation and a better surface finish. I love it when a plan comes together.
Quick, what tool can you put into your mill that has both the highest rigidity and the highest material removal rates? If you hadn't guessed, it is the lowly twist drill. Consider chain drilling around a profile to rapidly clear material before going in with an endmill to finish. In fact, some CAM programs support a plunge milling toolpath that will clear an entire pocket in this manner before finishing with an endmill. Plunging a twist drill puts all the force into the Z-axis, which is the stiffest axis on most vertical mills.
In no particular order, a variety of quick tips that may be helpful:
- Tramming: Your mill's tram matters for quality of finish. Tram here is defined as whether the spindle moves up and down a Z-axis that is perpendicular to the table and whether the axis of the spindle is perpendicular. See the notes above on back cutting for some other tramming considerations.
- Drawbar Force: Are you running an older CNC mill? When was the last time you measured your drawbar force? If the Belleville springs that hold the drawbar are weakening, it can have an immediate effect on your surface finish. CAT40-style spindles need considerable first (on the order of 2400lbs) to make sure the toolholder is properly seated in the spindle taper.
- Spindle Bearings & Spindle Runout: While we're on the subject of older machines, consider the state of your spindle bearings and whether there is any spindle runout. Consider toolholder runout too. I had a problem with an ER32 collet chuck one time. It was breaking little 1/8" endmills right and left. I finally checked the runout and it was ridiculous--4 to 6 thousandths. It had been kind of a cheap chuck, so I was about to write it off when I got the bright idea to check the collet. Sure enough, other collets were fine in the chuck. I had one bad collet which was cheaper to replace than the whole chuck.
- Keep your finishing cutters separate from roughing cutters. When finish degrades, you may choose to demote the cutter to "roughing" status. Use made-for-the-purpose roughing cutters for hogging. These often have serrated flutes.
- Material choice matters. Cast aluminum is gummy, and won't finish as well as wrought aluminum. Harder materials often have a better surface finish as the chips shear more cleanly.
- Keep the gibs tighter for less chatter. Make sure the z gib is tight by lowering the spindle on an aluminum or wood block on the table to put a bit of upward pressure on the head and tighten the gibs with it resting there.
- Reduce the flex in deep holes on a 2 flute cutter by grinding down one flute. Now the cutter acts like a boring bar.
- If the finish is down a hole, relieve the upper cutting surface so it won't be in contact with the hole and just cut at the bottom. This will reduce chatter, and works well when profiling with ball nosed end mills as well.
- TiAl coatings should not be used to cut aluminum. The aluminum in the coating sticks to the workpiece aluminum. Uncoated won't last as long but give the best finish on aluminum. If you want to use a coating for longer cutter life, use ZrN or TiB. Micrograin C-3 (low cobalt) carbides will have the best life.
- Try to get the mill head as low on the column as possible to maximize rigidity.
- If your machine has a quill, extend it as little as possible to maximize rigidity.
The Truth About "Mirror" Finishes
Anyone who frequents the machining boards online has seen countless threads where someone is asking after how to get a "mirror" finish from their mill or lathe. While it is easier to come close on a lathe, the truth about mirror finishes is that they largely do not exist. Yes, there are machine tools capable of doing optical quality finishes. These are extremely rigid machines that largely use diamond tooling. But, those are not the machines most of us will have access to, and they are not the machines most people are talking about as they ask after a mirror finish.
Have you ever noticed how most photographs of a so-called mirror finish have the workpiece tilted at an extreme angle? Have you ever seen the highway mirage where it looks like there is a pool of water on the road far ahead of you that vanishes as you get closer? Same principle. Even asphalt will apparently have a "mirror" finish (that water you saw in the mirage was a reflection of the sky) if the angle of incidence is right. Ask to see the mirror finish looking straight down on the part and you'll see more clearly what these finishes are all about.
This is not to say that a fine milled finish cannot be extremely attractive, its just that it doesn't really look like a mirror when viewed straight on. The tooling marks will still be visible, but they will be extremely faint grooves. In the best case, you'll see rainbows created by diffraction effects acting on the grooves. It's a look that has been called "prismatic". The closest thing to it is the back of a CD where all the rainbows are, but the milled finish will be a more subtle effect.
That's what you're looking for to decide you have achieved a great finish. If you need to do better, it's time to go to some abrasives of some kind and either user vibratory polish or a buffing wheel.