CNCCookbook: Be a Better CNC'er

Enjoy CNC Micromachining & Micro-Cutter Success: Easy Guide

CNC Feeds and Speeds Cookbook

Introduction to Micromachining

Micro-mills look similar but operate in a different world than conventional cutters do...

Makino says micro-milling involves features smaller than about 0.001" (what they actually say is smaller than 0.00098"). Given that we typically want accuracies that are about 1/10 of the tolerances required, micro-machining requires accuracies in the 0.0001" or less range. Cutters smaller than 1/8" or about 3mm are used for micromachining. The world of micromachining is all about either very small features on normal-sized parts, or very tiny parts. Some of the work done with micromachining is truly beautiful and spectacular. Consider these tiny Turner's Cubes, for example:

micromachining for turner's cubes

Exquisite micromachined turner's cubes...

Micro-endmills live in a different world than most of our cutters are used to. The feeds and speeds formulas and calculations that work reasonably well for larger cutters need quite a bit of adjustment for smaller cutters to account for these changing conditions. For example, the geometry at these scales is such that the rake on the cutters is almost always negative. To understand why that is, consider our diagram that shows how rubbing occurs when chipload gets too low relative to the radius of the cutting edge:

Rubbing from too little chipload

Two chiploads: Top one has chip thickness > tool edge radius. Bottom one has chip thickness < tool edge radius and therefore is showing negative rake. It's also more likely to plough or rub at these scales.

There's a limit to how sharp micro-cutters can be made, and hence they're far more likely to run in the negative rake regime where ploughing and rubbing are the norm rather than cleanly shearing chips as is the case with regular machining. As a result, The Association for Manufacturing Technology says:

The principal distinction between Macro and Micro-Machining operations emerges and manifests itself as the dominance of ploughing and rubbing phenomena at the cutting edge over shearing and the necessity to take micro-structural effects into consideration. Once feed-per-tooth is on the order of the cutting edge radius of the tool, macroscale rake angle is irrelevant.

For really small cutters, the cutting force is twice what conventional calculations suggest it should be and chipload must be matched even more closely to manufacturer's recommendations to prevent rubbing. In fact, the cutting forces can be even worse, and research from The Association for Manufacturing Technology finds it as high as 10-20 times what conventional machining models would predict.

With micromachining there is a pronounced minimum chip thickness that must be observed if the machining operation is to be successful. Below that thickness, chips simply do not form. In fact, most micro-milling involves a relationship between chip thickness (chipload per tooth) and cutting edge radius that is marginal. Often, a chip is not formed by every revolution. In other words, chips are formed intermittently, and when they do form, they're larger than would be predicted by the calculated chiploads. The difference between the volume of chips formed by "normal" milling operations and micro-milling can be as high as 9x for micro-milling and is typically on the order of 2-3x.

Compounding the problem of higher cutting forces is that the micro-machining cutters themselves are small and less able to resist tool deflection. They're more delicate and more likely to break in the face of deflection, higher chiploads relative to their size, and higher cutting forces.

Our G-Wizard feeds and speeds software takes all this into account, and is well-suited to providing feeds and speeds for your tiny cutters. G-Wizard will automatically switch to appropriate micromachining algorithms as your cutter diameter drops. If you haven't tried G-Wizard, and especially if you plan to do any micro-milling, take a moment to join the free 30-day trial.

 

What's Required for Micro-Machining Success?

1. Accuracy: As described, micro-machining begins with features around 0.001" in size and this requires accuracies in the 0.0001" range.

2. Care for Deflection and Cutting Forces: Small tools deflect much more easily and the forces involved are 2-20 times greater than conventional machining models would predict. Always use the shortest possible tool to maximize rigidity. Toolpaths may need to combine roughing and finishing as the feature may be too thin for separate roughing and finishing paths.

Small tools deflect more easily...

3. Care for Chiploads and Feedrates: Once the cutting edge radius is the same as the chipload, the actual rake of the cutter is irrelevant and it behaves as a negative rake cutter. There is a very narrow range of acceptible chiploads before tool life and outright breakage become a problem.

4. High Spindle RPMS to allow reasonable feedrates within the limitations of the chiploads micro-cutters can tolerate. Given that chiploads are baked in by cutter geometry considerations at the micro-scale, the only way to increase machine speeds is to use high spindle rpms to allow reasonable feedrates within the chipload limitations micro-cutters can tolerate.

5. Software. You can't hear the cutter's health when micro-machining, so you'll have to get the feeds and speeds right the first time. Likewise, very little tool deflection at the wrong moment will snap your cutters instantly, so you need high quality toolpaths. Invest in software that can help you through these issues--micro-machining is not something you do by ear or "gut feel."

 

10 Tips for Minimizing Breakage of Micro-Mills and Other Tiny Cutters

Over time certain questions and queries start to stand out, and the most prevalent questions we hear a lot about is that machinists are breaking their delicate micro-mills and other tiny cutters too often, and they'd like some pointers on how to avoid it. Micro-mills are certainly more delicate than normal endmills, but as mentioned, they also operate under different conditions. There are three issues that lead to more breakage of micro-mills:

- Because of the relationship of chip thickness to cutter edge radius, micro-mills require more energy than normal endmills relative to their Material Removal Rate. It's as if the material is actually harder for the micro-mill than it would be for a regular mill. Cutting forces are larger, as much as 2X according to one source, and the little cutter can exceed its bending limit. This is a good reason to keep tool deflection within limits by using a calculator that does tool deflection calculations like G-Wizard.

- Micro-mills are much more susceptible to breakage due to chip clogging. The available space for chips between flutes is smaller, and the clogging tends to happen much more suddenly. For that reason, some machinists will prefer to use HSS cutters which can bend more than carbide without breaking. If the chips do clog, the cutter is likely to break within relatively few rotations. Machinists will also prefer 2 flute micro-mills, even in materials such as steel where they're used to having 4 or more flutes in conventional milling. The reason is that micro-milling produces a larger volume of chips than conventional milling.

- Built up edge (BUE) is much more likely on a micro-cutter. It too leads to more force being required, which leads to more deflection, which leads to breakage.

Given that set of concerns, let's take a look at how to minimize micro-mill breakage.

First thing is first, you need to have proper feeds and speeds for these cutters. As mentioned, our G-Wizard feeds and speeds software takes all this into account, and is well-suited to providing feeds and speeds for your tiny cutters.

For best results though, you have to go beyond the feeds and speeds. Here are a few thoughts of where to look for problems when you're breaking small cutters:

1. Never reduce the spindle rpms much without reducing feedrate first. Reducing the rpms balloons the chipload, and it is chipload that breaks cutters. Too much rpm merely dulls them sooner.

2. Inexpensive machines typically have more spindle runout than higher-end CNC's. Runout is a real problem when micro-milling because you should think of runout as a % of the cutter's diameter. Hence a small cutter tolerates very little runout, and the smaller the cutter, the less runout that can be tolerated. Even very expensive CNC machines can run into this problem over time as bearings start to fail. Runout can also be made worse by your tool holder. I had a brand new ER32 collet one time that turned out to be bad. It looked perfect, but I was breaking small cutters in it right and left. I was convinced my cheap collet chuck was at fault, but I eventually tracked it down to a brand new collet. Replacing it immediately improved my results. It's pretty hard to accurately measure your runout on tiny endmills, but it is important to keep this source of trouble in mind.

One last thought on runout. I mentioned it is too much chipload that breaks cutters. Runout places most of the work on just a few or even one flute depending on how the flute is oriented relative to the direction of the runout. Hence, a lot of runout, as a % of tool diameter, is increasing your chipload by that same %. If you're already close to the "edge", you'll break the cutter just as surely as dialing up more chipload by any other means would.

flood coolant

3. In micro-milling it's very important to keep the chips clear. I always cringe when I see a picture with a lot of chips piled around the cutter. Recutting the chips and trying to force the new chips past the pile of old ones is really hard work on your poor old cutter. Flood coolant is not necessarily a panacea. Too little flow or poorly aimed flow can sometimes allow chips to pile up even with a simple flood system. I prefer either a lot of flood (e.g. the carwash), or if I can't have that, a really strong jet of air augmented with a little mist for sticky materials like aluminum. If you train yourself to be paranoid about chips in the cutting area, you'll immediately see benefits in cutter life and surface finish.

Note that if your cutters are particularly small, you have reached the point of diminishing returns or even damage with flood coolant because the force of the flood can deflect the tools and workpiece. Try a mist system, and use as low a viscosity cooling fluid as you can with it. Some are even using alcohol for micro-machining coolant.

4. Be wary of tool deflection. G-Wizard lets you calculate your deflection and even optimize cuts to hold to deflection limits. Deflection is just like runout for small cutters, and it becomes easy to forget about having too much tool stickout because the darned things are so small it seems like only a small amount protrudes.

5. G-Wizard has some specific features for small machines that are particularly germane to small cutters. If you fill out the hardware profile under Setup completely, tell it to compensate for machine weight. Just click the "Adjust" button by spindle HP to turn on that option. What this does is to "de-rate" your spindle HP from a particularly light machine like a Sherline or a Taig so that the HP relative to the weight of the machine and its envelope (total travels) is commensurate with full size CNC mills. Like tool deflection, if the machine is flexing around, that isn't helping the little cutter.

Some additional tips from Micromanufacturing.com:

6. Keep your setup and workholding as rigid as possible.

7. Don't "baby" the cutter on chipload lest you be cutting so little that the cutter is rubbing instead of cutting.

8. Use tools with an odd number of teeth, such as a 3 flute endmill. They deliver less vibration and more chip clearance.

9. Try a serrated rougher if you have a lot of material to remove, though in most cases, you'll use a regular EM for both roughing and finishing.

10. Consider HSS tools instead of carbide--they're less brittle and can "flex" a little more.

 

Using G-Wizard's Cut Optimizer for Micromachining

The key thing to keep in mind is that tool stickout is measured from the top of the cutter-diameter section to the tip, and should not include the much larger tapered shank. From the standpoint of the micro-mill, that tapered shank is so much larger than the cutting portion that its rigidity is not in question. When you buy your micro-mills, look for stub lengths of this section. Keep it as short as possible. 3 x the cutting diameter is a good basis though much longer cutters are available. Resist the temptation to stock up on the longer cutters unless your job specifically calls for it because they're so much less rigid.

The G-Wizard Cut Optimizer will calculate the optimal Cut Width, Depth of Cut, or Feedrate to stay within tool deflection guidelines...

 

More Micromachining Tips

Conventional Milling is Preferred Over Climb Milling

There are a variety of arguments for this but the primary issue is one of which way the tool deflects. Since micro-mills are particularly susceptible to deflection, a conventional milling approach is preferred since deflection will be along the tool path and not into the workpiece. Deflection into the workpiece leads to inaccuracy as well as encouraging chatter if the workpiece is very thin.

For more, try our Climb vs Conventional Milling page.

Try Combining Roughing and Finishing Passes

Sometimes when micro-machining, the wall that's left after roughing will be so thin that it can't support itself for a further finishing pass. The result is workpiece chatter and very unsatisfactory results. Consider combining the roughing and finish operations in a single pass for these cases.

CADCAM Considerations for Micro-Milling

- Adjust the mesh size, accuracy, and resolution of your CAD and CAM to deal with the very small features found in micro-machining. CADCAM translation problems are a high risk due to these precision issues.

- Toolpath strategies that reduce the forces on your cutter, especially sudden shock forces are very helpful. HSM toolpaths control tool engagement angle to minimize corner shocks. Trochoidal paths are a common fixture of a lot of micro-machining and perform the same function. Even simple things, like avoiding sharp motions as the tool path direction changes are very helpful--use arcs and not connected line segments to smooth that transition.

- Cutter Entry and Exit are especially important to tool life. Be aware of strategies that allow your cutter to gracefully enter the material with minimum shock and stress.

- Rest Machining strategies are valuable as clean up toolpaths are often a requirement when micro-machining. Given the extreme taper of micro-milling tooling, the CAM package needs to use its Rest Machining to avoid collisions with the workpiece and the tool shank on successive passes. Make sure your CAM software's Rest Machining is computed to a sufficient degree of accuracy.

- There are a lot of similarities between high speed machining (HSM) and micro-machining. For example, the need to avoid sharp tool motions which is often accomplished by rounded entries to corners. However,  rounding  can  become  a  challenge  in  micro‐milling, which commonly features very small stepovers. Rounding smaller than the stepover will likely create a sharp motion, while rounded corners larger than the stepover could create ridges and gaps between sequential passes and generate excessive scallops.  Specialized toolpaths exist to ensure high surface quality and to prevent such gaps and ridges. These include CBP (Clean Between Passes), CBL (Clean Between Layers), and Ridge Machining.

- Effective rest machining at a resolution commensurate with micro-machining is critical. Rest machining allows clean up tool paths as well as a knowledge of exactly how much material is being removed at every point in the toolpath so that feeds and speeds can be optimally varied along the toolpath.

Machine Considerations for Micro-Milling

- Vibration is paramount. Look for machine characteristics that minimize vibrations. Polymer Concrete can provide up to 10x the damping of a cast iron machine frame.

- Linear ways beat box ways for micro-machining because the short distances travelled are more subject to sticktion in Box Way machines.

- The higher the spindle speed, the better.

- Accuracy is particularly critical for micro-machining.

 

Links

CAD/CAM Considerations for Micro-Milling: MMSOnline

Ultra-Cool: Coolant considerations when micro-machining.

Turning Tips for Micro-Machining

Building a Low-Cost Micro-Milling Machine: Interesting academic paper.

MicroManufacturing.com CNCCookbook Interview

 

Next Article: Advantages and Pitfalls of Rigid Tapping

 

Try the Free Trial Version of G-Wizard Speeds and Feeds Calculator...

 

No credit card required--just your name and email.

 

CNC Milling Feeds and SpeedsContents

 

Featured Articles

Step-By-Step Guide to Making CNC Parts

CNC Router Cutter Types

Why Use a Single Flute Endmill?

Step and Servo Motor Sizing

The Truth About Tool Deflection

10 TIps for Router Aluminum Cutting

2 Tools for Calculating Cut Depth and Stepover

CNC Machine Hourly Rate Calculator

Special Purpose CNC Calculators

Feeds and Speeds Guide

CNC Cutter Guide

Feeds and Speeds By Material

G-Code Tutorial

  Feed Rate Calculator

Sales, and Special Deals

 

GCode is complicated.
G-Wizard Editor
makes it easy.

Try It!

 

Feeds and Speeds:
Made Easy.

Try G-Wizard

 

 

Do you want to be a better CNC'er?

Get Better Tool Life, Surface Finish, and Material Removal Rates.

 

Start Now, It's Free!