This page is work-in-progress.
¶ Overview
CNC Milling (image credit: Greg Rosenke)
Machining is a process of removing material from a workpiece to create a desired shape. The workpiece is typically a piece of raw material, such as metal, plastic, or wood. The process is performed using a variety of tools, such as lathes, milling machines, and grinders. The workpiece is held in place by a fixture, and the cutting tool is moved across the workpiece to remove material. The cutting tool is typically a drill bit, end mill, or lathe tool. The process is controlled by a computer, which is programmed to move the cutting tool in a specific pattern to create the desired shape. This process is known as computer numerical control (CNC) machining.
¶ CAD/CAM Process
The general workflow to go from CAD model to machined CNC part is:
- Begin with CAD model.
- Establish Job parameters including CNC coordinate system and stock shape/size.
- Select CNC process.
- Select cutting tool and machining parameters.
- Select driving CAD geometry.
- Verify toolpath.
- Post Process.
- Transfer G-code program to CNC machine.
- Set up and operate CNC machine to make part.
¶ CNC Machining Safety Practices
Use these extra precautions when running a CNC program for the first time:
- Use machine Rapid and Feed override controls to slow the machine down.
- A major cause of crashes is setting the tool or fixture offset incorrectly. Pay particular attention to
moves at the start of program and immediately after a tool change as the tool moves towards the part. Use single-block mode to advance through the program one line at a time until the tool is at cutting depth. - Remain at the machine with a hand on or near the emergency stop button.
- Stop machine motion at the first sign of trouble.
¶ Tools
¶ Overview
A wide range of tool types and configurations are available for CNC milling machines. Discussing every type, variation and use is beyond the scope of this course. This chapter introduces the most commonly used tools for prototype and short run production machining. Any tool supply catalog will list many others.
- End mills (Flat, Ball, Bull and Chamfer)
- Face mill
- Corner Rounding tools
- Slot Tools
- Spot-Center Drill
- Twist Drill
- Tap
- Reamer
- Counterbore
¶ End Mills
Milling tools include flat, ball, bull nose and chamfer.
Mill Tool Nose Types
Flat nose mills are used for milling 2D contours and pockets. Ball nose mills are used for 3D milling. Bull nose end mills have a radius corner. They are used to create a fillet on the bottom of a wall. Because they are sturdier than an end mill they are also sometimes used for roughing operations. Chamfer mills have an angled nose used to create a chamfer or to de-burr parts.
¶ Number of Flutes
Milling tools usually have either two or four cutting flutes. Two flute cutters provide more chip clearance when milling in close areas. Four flute mills are more rigid, can be fed faster, and are preferred when greater chip clearance is not required, such as when milling an outside contour.
¶ Center-Cutting End Mills
Milling tools are either center cutting or non-center cutting. Center cutting mills can plunge straight down into material, while non-center cutting tools cannot. Figure 2 below shows the cutting end view of a center cutting and non-center cutting end mill. Notice that the cutting edges of the center cutting end mill continues to the center of the tool. The center of the other has a small hole at the center. Non-center cutting end mills require a pilot hole, ramping or helical motion to plunge into material.
End View of Center and Non-Center Cutting End Mill
¶ Face Mill
A face mill has cutting inserts that are replaced when worn. They are rigid, may have up to eight or more cutting edges, and can remove material quickly. They are often used for the first machining operation to quickly create a flat finished face on the part.
Face Mill
¶ Corner Radius Tool
Corner radius (also called Corner Round) tools are used to place a fillet on the outside corner of a part.
Corner Round Tool
¶ Slot Mill/Slotting Saw
Slot mills include side milling cutters, slitting saws, and Woodruff keyset cutters. Slitting saws and side milling cutters are installed on a special arbor. Woodruff cutters are single piece tools used for creating slots and undercuts that can be held in a standard tool holder.
Slot Tools
¶ Hole-Making Tools
¶ Center-Spot Drills
Center (spotting) drills are short and very rigid drills used to create a conic on the face of the part. Because they come to a sharp point and resist bending, they locate the hole precisely. The conic helps prevent the subsequent drill from wobbling and ensure the drill is located precisely and drills straight down. Countersink drills are used to create the conical face for a machine screw. Combined spotting-countersinks are used to create a screw clearance hole and countersink in one operation. There are many different sizes and tip angles of center, countersink, and combined drills. Be sure the tip angle of the countersink matches the included angle of the machine screw, and that the drill diameter is greater than the screw head diameter.
Countersink and Center Drill
¶ Twist Drill
Twist drills are available in many diameters and lengths. Usually made of high speed steel, carbide, or cobalt, they may also be coated with titanium nitride (TiN) for longer life. The tip angle of most twist drills is 118 degrees.
Twist Drill
¶ Taps
Cutting taps form threads by shearing material away. Form taps (roll taps) form the thread by forming the metal to shape. Form taps produce no chips and are used for soft materials including aluminum, copper, brass and plastics.
Taps
Bottoming taps are used to tap blind holes. Spiral point taps push the chip ahead and out the bottom of a through hole. Taps require a hole drilled to the correct size to ensure the thread is formed properly. For example, a ¼-20 cutting tap requires drilling a .201 (#7) hole. Refer to the drill chart in Appendix A to find the correct drill size for a specified thread size and fit. Most CNC Machines support rigid tapping, which means the tap can be held in a rigid holder. The tap is advanced at a feed rate that matches the thread lead into the hole. The spindle then stops, reverses, and backs out of the hole. Machines without rigid tapping require special tapping attachments. Always refer to the manufacturers’ instructions as the speed, feed, and other machining parameters for tapping attachments may be different that those for rigid tapping.
¶ Reamer
Use reamers to create holes of precise shape and excellent surface finish. Reamed holes are usually accurate within .0002 inches diameter. For example, a reamer is used for holes used for ground pins and bushings. Reamers require a specific size hole be drilled before use. Cutting speeds and feeds are also important. Remove too little or too much material and the hole will not be the correct size.
Reamer
¶ Counterbore
A counterbore looks similar to a end mill with a pilot in the center. It is used to spot face holes, and the pilot ensures the spot face is centered on the hole. Counterboring is not necessary when using a CNC machine. Rather, create a spot face using a pocket or circle mill tool path. This saves having to buy and stock counterbore tools and pilots, and the time required to load and set up the counterbore.
¶ Cutting Tool Fundamentals
¶ Rotation Direction
All tools (except left-handed taps) rotate clockwise (M3) when viewed from the machine spindle looking down at the part.
Clockwise Tool Rotation
¶ Chip Formation
Cutting tools remove metal by shearing action as illustrated in Figure 11 below. As the tool advances into the material it causes a small amount of the material to shear away, forming a chip.
Chip Formation Diagram
¶ Chip Load
The thickness of material sheared away by each cutting tooth is called the feed per tooth, or chip load. As the chip is ejected from the work area it carries with it some of the heat generated by the shearing process.
Chip Load
A methodology for calculating cutting speeds and feeds is presented later in this chapter. One of the best ways to validate cutting speeds and feeds is to observe the chips created by the machining process. Chips should be curled and may change color due to heating. After gaining some experience machinists are able to adjust cutting speeds and feeds based in part on the size, shape, and color of chips and on the sound produced by the cutting process
¶ Climb vs. Conventional Milling
Milling tools can advance through the material so that the cutting flutes engage the material at maximum thickness and then decreases to zero. This is called Climb Milling. Cutting in the opposite direction causes the tool to scoop up the material, starting at zero thickness and increasing to maximum. This is called Conventional Milling. Conventional milling is used often on manual machines because backlash in the machine lead screws causes the tool to lurch when climb cutting. This is not a problem on CNC machines because they use ball screws. Conventional milling causes the tool to rub against the cutting surface, work hardening the material, generating heat, and increasing tool wear. Raking chips across the finished surface also produces a poorer surface finish. Unless specifically recommended by the tool manufacturer for the material being milled, always use climb milling on a CNC. Climb milling produces far less cutting pressure and heat, leaves a better surface finish, and results in longer tool life.
Climb vs. Conventional Milling
¶ Cutting Speeds and Feeds Formulas
The tool moves through the material at a specified rotational speed, defined in revolutions per minute (RPM), and feed rate, defined in inches per minute (IPM). Probably the most vexing problem for the beginning CNC machinist is selecting proper cutting speeds and feeds. This selection is actually more difficult on a CNC than a manual mill because, with a manual mill, the operator can feel the cutting pressure and alter the feed based in part on the cutting force.
CNC mills require calculating speeds and feeds in advance. These speeds and feeds can, and often are, adjusted at the machine based on chip shape and color, cutting sound, and machine horsepower meter readings.
The best source of data about cutting speeds and feeds for a specific tool, application, and material is the tool supplier. Much of this data is found on manufacturer’s web sites or printed tooling catalogs. Tool sales representatives can be a valuable resource, so if you do a lot of machining, develop a good relationship with a knowledgeable representative.
Another source of speeds and feeds data is CAD/CAM software. These have become increasingly sophisticated and often provide good cutting data.
Yet even the best speed and feed data is just a starting point. Speeds and feeds require adjustment due to many factors including the maximum spindle speed or horsepower of the machine, rigidity of work holding, and the quality and condition of the machine tool itself. The following pages provide cutting data for the most commonly machined materials and a methodology for calculating speeds and feeds. As always, use common sense. If the part is held by double sided tape, feeds based on vise work holding are probably too high. If the tool is very long and thin, speeds and feeds will likely require reduction.
¶ Speed Formula
Milling machine cutting speeds are derived from the following formula:
is the rotational frequency of the tool (Spindle Speed) in revolutions per minute (RPM).
(Surface Feet per Minute) is the speed at which the material moves past the cutting edge (outside diameter) of the tool in feet per minute. SFM values depend on the tool type, tool material, and material being machined.
is the circumference of the cutting tool in feet.
¶ How Speed Formula is Derived
Because cutting tools are defined by their diameter in inches, this formula is rewritten and simplified as follows:
is the tool diameter in inches.
is a constant derived from 12/𝜋 which converts the tool circumference in feet to diameter in inches.
¶ Feed Formula
Cutting feeds are in (IPM) and use the following formula:
is the linear feed of the tool through the material in inches per minute.
is the result of the speed formula (Figure 15) in revolutions per minute.
is the chip load, or how much material each cutting edge of the tool removes per revolution. Chip load is sometimes referred to as feed per tooth (FPT) or inches per rev (IPR).
is the number of cutting flutes. (For a twist drill, this value is one.)
¶ Tap Feed Formula
For tapping operations, feed rate is based on the number of threads per inch and feed rate:
is the linear feed of the tool through the material in inches per minute.
is the result of the previous formula in revolutions per minute.
the threads per inch of the tap. For example, the TPI of a ¼-‐20 tap is 20.
¶ Speed/Feed Example
¶ Milling Speed/Feed Example
Problem: Calculate the cutting speed and feed for a milling operation given the following values:
| Parameter | Value |
|---|---|
| Tool | .500in |
| NumFlutes | 4 |
| SFM | 600ft/min |
| IPR | .005in |
Solution
Step 1: Calculate RPM
Step 2: Calculate IPM
Note: Round off milling speeds and feeds to the nearest integer.
¶ Drill Speed/Feed Example
Problem: Calculate the cutting speed and feed for a drill operation given the following values:
| Parameter | Value |
|---|---|
| Tool Diameter | .201in |
| SFM | 250ft/min |
| IPR | .002in |
Solution:
Step 1: Caculate RPM
Step 2: Calculate IPM
Note: Round off drilling feeds to the first decimal point.
¶ Tap Speed/Feed Example
Problem: Calculate the cutting speed and feed for a ¼-‐24 tap operation given the following values:
| Parameter | Value |
|---|---|
| Tool Diameter | .25in |
| SFM | 100ft/min |
| IPR | 24 |
Solution:
Step 1: Caculate RPM
Step 2: Calculate IPM
Note: Round off tapping feeds to three decimal points or the maximum number the machine allows.
¶ Maximum Spindle Speed Example
In cases where the calculated spindle speed exceeds the machine capabilities, program the maximum spindle speed of the machine and use this value in the feed calculation.
Problem: Calculate the cutting speed and feed for a milling operation given the following values:
| Parameter | Value |
|---|---|
| Tool Diameter | .125in |
| NumFlutes | 2 |
| SFM | 300ft/min |
| IPR | .003in/rev |
| Maximum RPM | 7,500rev/min |
Solution:
Step 1: Caculate RPM
Step 2: Calculate IPM
¶ Cutting Data
Tables on the following pages provide basic speed, feed and cutting data for some of the materials commonly used for prototypes. Use the tool manufacturer’s data instead whenever it is available.
¶ Mill Cutting Speed
SFM surface mm/min
| Material | HSS | Carbide |
|---|---|---|
| Aluminum | 180 | 240 |
| Brass | 50 | 50 |
| Delrin | 120 | 240 |
| Polycarbonate | 90 | 150 |
| Stainless Steel (303) | 25 | 100 |
| Steel (4140) | 20 | 100 |
SFM surface ft/min
| Material | HSS | Carbide |
|---|---|---|
| Aluminum | 600 | 800 |
| Brass | 175 | 175 |
| Delrin | 400 | 800 |
| Polycarbonate | 300 | 500 |
| Stainless Steel (303) | 80 | 300 |
| Steel (4140) | 70 | 350 |
¶ Drill Cutting Speeds (SFM)
surface ft/min
| Material | Drilling | C-Sink | Reamer | Tap |
|---|---|---|---|---|
| Aluminum | 300 | 200 | 150 | 100 |
| Brass | 120 | 90 | 66 | 100 |
| Delrin | 150 | 100 | 75 | 100 |
| Polycarbonate | 240 | 160 | 120 | 100 |
| Stainless Steel (303) | 50 | 35 | 25 | 35 |
| Steel (4140) | 90 | 60 | 45 | 35 |
Tip: Never use tools that have been used to machine metal to cut plastic. The sharp edge of the tool will be compromised and cutting performance and finish will suffer. A good practice is to keep two sets of tools: one for plastic and one for metal.
Tip: High speed steel cutters work best for plastics. Carbide cutters work better for aluminum and other metals.
Cutting Feed (IPR) in/rev
| Material | Tool Diameter Range (in) | ||||
|---|---|---|---|---|---|
| Milling | |||||
| Aluminum | .002 | .002 | .005 | .006 | .007 |
| Brass | .001 | .002 | .002 | .004 | .005 |
| Delrin | .002 | .002 | .005 | .006 | .007 |
| Polycarbonate | .001 | .003 | .006 | .008 | .009 |
| Stainless Steel (303) | .0005 | .001 | .002 | .003 | .004 |
| Steel (4140) | .0005 | .0005 | .001 | .002 | .003 |
| Drilling | .002 | .004 | .005 | .010 | .015 |
| Reaming | .005 | .007 | .009 | .012 | .015 |
¶ Best Practice Machining Parameters
Best practice machining parameters for prototype and short-production milling are different than for mass production. Production machining is obsessed with minimizing run time and maximizing tool life because even small improvements per part can result in significant cost savings. Prototype and short run production seeks to maximize reliability. Obviously, it does not make sense to risk breaking a tool or scrapping a part trying to save a few seconds if only making a few parts. Tables 8 and 9 on the following pages list recommended machining parameters for prototypes. The values are relatively conservative and work well for materials and tool types listed on the previous pages. For materials or tools not listed, consult cutting data from the tool manufacturer.
Recommended Machining Parameters
| Operation | Parameter | Value |
|---|---|---|
| All | Clearance Height | 1.0 inches |
| All | Rapid Height | As need to clear clamps and fixtures |
| Mill (Roughing) | Stepover (XY) | 50-80% of tool dia. |
| Mill (Roughing) | Stepover (Z) | 25-50% of tool dia. |
| Dill | Peck Increment | .05 inches |
| Stop Drill | Dwell | .5 seconds |
Stock Finish Allowance
| Operation | Tool Diameter Range (in) | ||||
|---|---|---|---|---|---|
| <.125 | .125-.25 | .25-.5 | .5-.1 | >1. | |
| Milling (XY) | .001 | .005 | .015 | .020 | .020 |
| Milling (Z) | .001 | .002 | .005 | .005 | .005 |
| Reaming | .005 | .010 | .012 | .020 | .030 |
¶ Troubleshooting Speed/Feed Problems
Do not make the mistake of thinking that the only option when encountering a machining problem is to reduce feed rate. Sometimes that is the worst thing to do and decreasing speed and increasing feed may be a better option. Be methodical. When a problem occurs, stop. Analyze what is happening, draw on all available resources, and then devise a solution to correct the problem. The Machinery’s Handbook (Industrial Press Inc, 2008, New York, NY, ISBN: 978‐8311‐2800‐5) contains extensive information about diagnosing and correcting cutting tool problems. This book is an essential reference for anyone using machine tools.
¶ CAM
¶ Machine Operation
¶ Tooling Guide
¶ CNC Tooling
This tooling guide has been put together to help both newcomers and even the more experienced to the CNC machining industry. The purpose is to assist with the selection of cutting tools and clamping systems. The ability to maximize tool life and achieve best possible surface finish is a prerequisite to obtaining the highest return on investment made in a CNC machine. Its efficiency and productivity is only as good as the tooling paired with it, so understanding the most critical aspects of both tooling and accessories is essential.
¶ Introduction
Precision cutting tools and clamping systems offer a high degree of technical sophistication. There are important characteristics they must possess, which provide the basis for safe, smooth and efficient operation of a CNC machine. Beginning with design, construction, engineering expertise, to the balancing and inspection of the finished product, the selection of tool and clamping system made can have a profound impact on performance and production cost and can have an even greater impact on your bottom line. With the many options and suppliers to chose from, it does require a bit of homework to make the right tooling decisions. Surprisingly, cutting tools are often the last thing thought about when buying a CNC machine…...but consider this: without the cutting tool, your machine won’t produce a single thing!
¶ A Synergy at Work
Cutting tool performance, i.e. tool life and surface finish, is the result of a synergy between cutting tool, clamping system, machine spindle, material hold-down, efficiency of dust extraction, correct machining parameters (i.e. spindle speed and feed rate) and the composition of the material being machined. For best performance, all facets need to be right.
¶ A Good Analogy
Keeping in mind that a high class, high performance automobile requires high quality, precision-balanced tires to run smooth, the same applies to cutting tools and tool holders used on a CNC machine.
Remember:
…. a CNC machine cannot cut a single panel without the tool. Good tires provide a smooth and safe ride and similarly, high quality, precision balanced tooling is needed to deliver the promise of productivity that comes with a CNC machine.
¶ CUTTING TOOL OPTIONS
This presentation will familiarize the CNC novice with the variety of tooling solutions that are available to meet specific cutting, profiling, drilling, grooving and sawing tasks. Furthermore, proper tool selection, material hold down and dust extraction will increase the frequency of the following desirable CNC characteristics:
- Accuracy
- Waste Reduction
- Repeatability
- Spindle Bearings upkeep
- Finish Quality
- Bottom Line Tooling Cost
Using tools within appropriate machining parameters, in particular, correct “chip load”, is important. Simply put, chip load is the size/thickness of the chip being removed per flute/cutting edge with every revolution of the tool. So, going from a 2 flute bit to a 3 flute bit, the size of the chip is reduced by 33% if the feed rate or spindle speed (rpm) is not adjusted accordingly. A smaller chip will increase heat during the cut as the chips cannot be extracted fast enough and are re-cut into yet smaller particles. The resulting heat generated is very detrimental to tool life!
Remember:
Too big a chip load will decrease the finish.Too small a chip will decrease the life.
¶ Safety First
every field of technology. For the wood/composites industry, it has developed very extensive criteria/norms for the safe and effective operation of manufacturing machinery, cutting tools, clamping systems and many other accessories. It’s closest U.S. counterpart, ANSI (American National Standards Institute), does not have a detailed norm for cutting tools and accessories. When it comes to very specific tool design DIN NORM – abbreviation for Deutsches Institut für Normung (often just referred to as Deutsche Industrienorm) is the German national institute for standardization of almost criteria with details such as minimum acceptable shank diameter based on the mass of the respective tool body being made, maximum knife protrusion beyond tool body (on insert tools) and countless other details that serve to protect both machine operators and the machine itself, in absence of such established norms in the U.S, we look to Germany’s stringent DIN standards to dictate what we do. While today’s CNC machining centers are equipped with state-of-the-art safety features such as curtain guards, contact mats, guard fencing and more, a cutting tool spinning at 16,000+ rpm still poses a risk if sub-standard tools and clamping systems are employed and safety warnings not followed.
Partner with someone who meets the standard!
¶ Clamping Systems Overview
From left – clockwise
- Drill Bit Adapter
- IS0/SK30/BT/HSK-F & E collet chucks
- Arbor Adapters for cutters/blades with bore
- Saw Blade Adapters
¶ Most Common Clamping System
Developed in Germany, the HSK tool holder is the most widely used collet chuck on CNC routers and machining centers in the wood/composite industry today as it provides the highest degree of accuracy for high speed machining. A precision machined interface between spindle and tool, it is balanced to G2.5 spec for 25,000 rpm. Manufactured in accordance with DIN 69893, it is designed for use with automatic tool changers. HSK (Hohl-Schaft-Kegel), translated from the German language means hollow shank taper which is the part of an HSK tool holder that connects to the machine. This taper is machined to the highest precision, both radially and axially, of 0.0001” per DIN Norm. It’s important to purchase only the highest quality tool holders from reputable manufacturers to protect the machine spindle from potential damage.
¶ HSK Interface Anatomy (DIN 69 893)
Understanding the inner workings!
.png)
¶ Overview of Most Common HSK-F 63 Tool Holder Styles for Router Tooling
¶ Accuracy of the Differnent Tool Holder Styles
Tool holder styles are interchangeable on any machine that has the HSK-F 63 tool interface.
¶ Collet Style and Range Tolerance
RDO / SYOZ Style
ER Style
¶ Collets - Noteworthy Info
Collets wear out! Over time, the spring steel loses elasticity due to wear and heat. Collets that are not replaced will eventually fail. Collets are inexpensive…. Failure to replace them regularly will increase tool cost due to unnecessary vibration and runout, tool chattering and breakage. They can do considerable damage to a spindle, so adhering to a collet maintenance schedule is preferable to costly repairs.
• Clean collets and collet nuts when changing tools!
• Use proper torque! Investment in a torque wrench to tighten the collet nut is a prerequisite to extending tool life and reducing breakage!
• Pay attention to clamp tool correctly! (see below) With proper tool setup, the collet should be filled to 80% with the tool shank. Shorter will allow deflection.
• Replace collets every 500 machine hours for optimum tool life! Prevent costly spindle repairs!
¶ Collet Nuts
The collet nut, and accuracy thereof, is an important component of collet tool holder setup. A high precision collet nut will have a ball bearing located at its base which reduces the overall runout and improves clamping force (pictured in photo below on the right). It also prevents tool slippage. The static nut (pictured on the left) does not clamp as accurately as the bearing version. The bearing in the collet nut also facilitates the ability to run either CW or CCW tools in the same tool holder. With a static nut this is not possible….a lefthand toolholder would be needed.
¶ Which Style Tool Holder to Use?
For routine machining of wood and composite materials, the standard collet chuck style
tool holder is an excellent choice. It has an accuracy of .006-0.01mm depending on which
collet style is used. For the more discriminate user and critical machining applications, the
option of a Preziso® Precision Chuck, Hydro Chuck or Heat Shrink chuck is a good option.
STANDARD CHUCK
• Excellent general use choice. This version is supplied with most new machines and adequate for general machining tasks.
PREZISO® CHUCK
• Excellent choice to reduce vibration when cutting very hard materials
• Improved efficiencies over standard tool holders, optimizes tool life.
• Good choice to increase tool life with solid carbide spiral bits.
• No additional equipment needed.
HYDRO CHUCK
• Rigid tool stability
• Extremely high clamping force
• Saves expense of replacing collets regularly.
• Initial higher cost.
HEAT SHRINK CHUCK
• Best for the Spoil Board (Fly) Cutter, all Insert Tools and Diamond Tools.
• Improved efficiencies over standard tool holders, increases tool life and improves finish.
• Not suitable for solid carbide tools and tools requiring frequent change since an additional investment in a heat induction unit is required.
• Saves expense of replacing collets regularly.
• Order Insert tools and diamond tools mounted on heat shrink chucks!
¶ Cyclone Dust Nut
A dust nut can be especially useful if too much dust is remaining on the table. More importantly, it’s a safer and healthier work environment to reduce airborne exposure to dust particles. The Cyclone Dust Nut takes the place of the regular bearing collet nut on the tool holder. Through its geometry, it creates a whirl-wind type effect that sucks the chips out of the cut and into the dust extraction system. The Cyclone must be kept close to the shroud / table to function properly, so best to have shortest possible cut length on the router bit to allow the nut to be positioned as close to the table as possible. Below are photos of the same cut made with a regular collet nut (on the left) and the other, with a cyclone dust nut (on the right). Our company offers a demo/test nut to try so customer knows if it will work in his application before buying.
¶ Demonstration on Collet Replacement
First, click the collet into position by pressing only one side
Then, pushing down on the other side to lock it in.
To release the collet, use the ball of your hand to push out sideways.
¶ Proper Tool Assembly
- Snap the collet into the collet nut or cyclone nut.
- Place the tool into the collet paying close attention to the proper tool depth in the collet. Tighten the collet nut manually onto the tool holder.
- Position and secure the tool holder in a tool setup fixture as shown below.
- Tighten the collet nut with a torque wrench to the correct torque based on the collet style used.
Setup Ffixture with gauge.
Setup Fixture (no gauge) and torque wrench.
| Collet Style | Recommended Torque |
|---|---|
| RDO 35 (SYOZ25) | 59 ft/lbs |
| ER 20 | 100 ft/lbs |
| ER 32 | 130 ft/lbs |
| ER 40 | 90 ft/lbs |
¶ Proper Torque
Incorrect torque when tightening the collet nut will result in poor cutting performance, premature collet wear, tool slippage during the cutting process and over-torqueing can often result in tool breakage and chattering. Investment in a torque wrench has paid for itself after the first few bits broken due to over torqueing. Use the torque wrench only for tightening the collet nut. Use a standard wrench to remove it. Otherwise, the torque wrench can lose calibration accuracy.
¶ Tool Setup Fixture
A setup fixture and torque wrench are a necessary investment to achieve optimum tool life These are necessary to avoid tool breakage, inferior finish, premature wear and a high tooling cost. After spending over six figures on a CNC machine, this is not the time to pinch pennies.
¶ Drill Bits and Adapters
¶ Using Drill Bits on a CNC
Using typical 10mm shank drill bits with a set-screw flat area on the shank in a collet-style tool holder can result in oval holes. The drill bit shank cannot be clamped evenly around its circumference due to the flat on the tool shank present for set screw tightening. The gap that remains between the collet wall and tool shank in the flat area can cause the bit to deflect, possibly wobble and not provide a good finish. The solution is to get a small and inexpensive drill bit adapter that has a 10mm cylindrical shank (without flat) to go into the collet, and the
female end of the adapter accepts the 10mm drill shank with flat and is tightened in with a set screw. For CNC use, the 70mm drill bit length should be chosen over the 57mm length
¶ Drill Bit Selection
From left to right:
-
For holes that will go through the material, use V-Point Bits (ThruHole Bits) that prevent surface tear-out on the bottom of the cut.
-
For blind holes, a brad point/dowel bit is required. It has a center point and outside spurs to cut a clean hole. For pilot holes, this bit is available in solid carbide in 1/8” diameter
-
For hinge pockets, the hinge boring bit is the best option. The center point and outside spurs provide a clean edge hole and prevent the bit from “walking”.
¶ CNC Drill Adapter
This Universal Drill Adapter is the best and only option if drilling many different cylindrical drill bit sizes for which collets are not always available.
RPM and Feed rate:
When drilling or boring holes on a CNC machine, your spindle
speed and feed rate must be adjusted to within the proper
parameters for drill/boring bits.
Recommended Feed / Speed for Drilling on CNC:
| -- | -- | -- | -- | -- |
| RPM | Feedrate (m/min) |
|3000| 1 - 2 |
|4500| 1.5 - 2.5 |
|6000| 2 - 3.5 |
|9000| 2.5 - 5.5 |
¶ Sizing, Jointing, Rebates, Dado Cuts, and Grooving
¶ Straight Router Bits - Tool Materials
• The best options for CNC machining are either solid carbide bit or PCD
(polycrystalline diamond).
• PCD tooling achieves the best return on investment when it is dedicated to cutting homogeneous material and not interchanged between, for instance, composite and wood. Use dedicated tools per material!
• The only time a carbide-tipped tool is an economical solution for use on a CNC is for cutting a small profiled proto-type (i.e. one-off).
¶ Router Bits
Depending on product and volume being machined, the selection of the most suitable cutting tool requires a bit of homework if best performance and finish relative to investment is desired.
In the following slides we present the most common and cost effective router bit options based on application.
For straight cuts such as sizing, jointing, rebating, grooving and dados, the options available are solid carbide, carbide insert or PCD (polycrystalline diamond).
For profile routing applications, options are either carbide insert or PCD and for proto-type or “one-off” needs, a corrugated head provides a cost-effective solution.
In addition to the many standard tool designs, it is often necessary to customize a tool for a particular requirement in order to provide a more economical option over time.
Many tools styles can effortlessly produce the same cut, so researching cost, time and yield based on tool choice can have a substantial impact on a tooling budget.
¶ Solid Carbide Bits
Solid carbide router bits come in a variety of tool geometries, number of flutes, and edge grind to include the most popular ones below and described in more detail on the following pages.
• O-Flute, Straight (Soft Wood/Soft Plastic)
• O-Flute, Up Cut (Plastics, Aluminum)
• Up Cut
• Ball Nose Up cut
• Down Cut
• Compression (Mortise Compression)
• Compression Chip Breaker
• Up Cut Chip Breaker
• Down Cut Chip Breaker
• Up Cut Rougher
• Down Cut Rougher
• Single, Two and Three Flutes
Remember: More flutes does not equal better finish! More flutes means you have faster feed rate capability! Refer to the chip load information later in this presentation to calculate your needs.
¶ O-Flute Bit (Solid Carbide)
This image shows a solid carbide, straight O-Flute. The flute shape is ground into what looks like a half-circle. This particular geometry is used for cutting flexible plastics. The flute is straight and helps keep a light weight flexible plastic from moving orlifting on the router table during machining.
.png)
Use this tool on materials such as:
- Polycarbonate
- ABS
- Polystyrene
- PVC
- and other flexible plastics
-materials.png)
¶ O-Flute Upcut
The O-Flute upcut bit features the same O-Flute geometry needed for efficient chip removal when routing plastic, and also has an upward shearing angle to bring the chips out of the cut and provide cleanest possible edge finish.
This tool is the preferred router bit for hard and rigid plastic materials, such as:
- Acrylics
- Nylons
- Plexiglass
- and other rigid plastics
¶ Upcut Spiral
The up cut spiral bit is used when getting the chips out of the cut is critically important, or when the material is laminated or coated on one side only, and is being machined face down. This tool geometry does present a risk that the top of the material being cut can chip or fray.
This tool is a good choice for mortise and tenon cutting needs and also provides an excellent option for short runs on Corian or phenolic. (longer runs should consider a PCD diamond bit as it is more cost-effective). Upcut bits provide the ability to feed faster than down cut bits as the chips are pulled out of the cut by the upward shearing action and keep the tool running cooler.
¶ Ballnose Upcut Bit
A ball nose tool is a great choice for cove and fluting operations, but is also the tool of choice when complex shapes have to be surfaced. A flat bottom bit would leave lines and a poor finish, but a ball nose bit, due to its rounded shape, provides seamless passes.
Another option for this tool is a carbide insert version (pictured below), which is always much more cost effective if the project is ongoing with a continuous tooling need.
¶ Down Cut Bit
The down cut spiral bit provides a superb top surface finish, but it does run the risk, depending on application, of pushing the chips into the cut and bogging down the bit. With good dust extraction and proper chip load, this should not be a problem. It is often selected for doing grooves, dados and rebate cuts . Important to remember, always use the shortest possible cut length for dados, grooves and rebates, as the longer tools will have more deflection and can break more easily or provide poor finish due to deflection when cut length is excessive.
If there is an ongoing dado or rebate cut requirement, an insert bit will decrease cost considerably within a short period of time if the tool is available in the diameter needed. (Image below)
¶ Compression Bit
The compression bit is designed to cut materials that have a laminate, melamine, HPL, paint, paper etc. on both top and bottom surface. The cutting flutes have opposite shear angle geometry and cut toward the center of the material, thus providing clean surface top and bottom. This is the most popular style bit used in composite panel processing and is available in many different executions….ranging from a variety of carbide
grades defined for wood, composite material and melamine, and also coated versions. These bits come in multiple carbide grades! Pick the right one for the job!
If using 3/4” or larger compression bits, an insert or a PCD diamond tool offer the lower cost option for any ongoing need.
Insert Bit for >3/4” diameter
PCD bit compression bit
¶ Compression Chip Breaker Bit
The compression chip breaker is the best choice for cutting plywood and OSB panels where a good surface finish both sides is expected. The chip breakers, which are notches machined in an offset pattern into the flutes, facilitate faster feed rate and breaking up the larger chips created by these materials. While the chip breaker is essentially more of a hogging tool, it does provide excellent machining characteristics as well as a good finish in the compression style.
Below is an insert tool option for high feed speed requirements on plywood panels and other composite materials.
¶ Upcut or Downcut Chipbreaker Bit
The up or down cut chip breaker is a great choice for cutting composite panels and plywood where a good surface finish on one side is needed. (down cut for best finish on top, and up cut for machining face-down).
The insert option pictured below, features a selection of insert knives that are either straight, up- or down shear or even compression style and can be arranged as needed on the tool body as shown below.. This allows them to be positioned for best possible finish results.
¶ Upcut or Downcut Roughing Bit
A roughing bit is designed to remove a lot of material quickly, but, as the name implies, it does leave a rough edge which must be cleaned up with a finishing pass using another tool. Typical feed rate for these 3 flute tools is 800”/min and up.
A very cost effective option is an insert roughing tool (pictured below) which is available with either carbide or diamond (PCD) inserts and provides a tremendous cost saving for high volume operations.
¶ Diamond-Tipped Router Bits
Whether diamond tooling should be a consideration for a particular application is discussed in the next few pages. Diamond router bits come in a variety of styles such as high shear, single flute, two flute or three flute disposable, single segment opposite shear etc. Diamond tools are not all equal. Some are designed to be disposable, others can be sharpened one or more times and these factors should be considered when shopping for PCD tooling.
¶ Nesting Tips to Remember
• Always adapt the cutting length of the router tool to the panel thickness, i.e. cutting length should be minimally longer than the panel thickness.
• Always chose the stronger tool, i.e. cut length not too long and diameter not too small.
• Material hold-down must fit the tool. That means, select small diameter tools for parts that are prone to moving.
• Chip clearance is better on larger diameter tools, therefore when running high feed rates and thicker panels, use a diameter of 5/8” or greater.
• Select highest accuracy clamping tools. (Heat shrink, Hydro Chuck or Preziso)
• If using collet chucks, replace collets regularly. (every 500 machine hours!)
¶ For MDF / Particleboard Carbide or Diamond
There is no debate that PCD (polycrystalline diamond) will outperform solid carbide tooling in wood and composite material by many multiples and be the more economical choice over time. Until recently, there was a good argument to stay away from diamond router bits, because most companies promoting them only offered single flute on diameters of ½” or less. This did not facilitate high feed rates. That has changed with the introduction of 3/8” and ½” PCD bits that are 2-flute!
If you want to achieve the best possible tool life and save substantial amounts of money in the process, you would be remiss to not investigate the cost of running a diamond tool for your biggest projects! Whether sizing or profiling,diamond tooling should always be used on homogeneous material and same panel thickness to maximize the tool life and performance. Most diamond tools can be sharpened a few times and will last longest when paired with a heat shrink tool holder for highest accuracy.
¶ When not to use Diamond Tools
These are circumstances under which solid carbide bits would be the better choice:
• When materials and material thickness varies and having a diamond tool for each operation isn’t feasible.
• If initial cost outlay is critical and a higher upfront tool price isn’t tolerated for cash flow reasons even though it will save much over time.
• If material is prone to inclusion of staples, nails etc. (diamond tools are susceptible to impact damage).
• If the machine is older and has excessive spindle runout, or parts tend to move on the table....stick with carbide.
• If machine operators are poorly disciplined and wouldn’t handle a diamond tool with the gentle respect it deserves.
• If customer is not prepared to invest in a complete setup to insure the diamond tool is capable of performing to expectations, i.e. doesn’t want to replace the collet or invest in a heat shrink tool holder.
• Customer is cutting parts that require plunging straight down into the material (this creates a lot of heat that will cause the PCD tool to wear prematurely.
¶ A Typical Cost Comparison of A Carbide Compression vs Diamond Tool
The below comparison is based on both tools being sharpened twice and does not include setup cost or machine downtime, nor does it factor in that after sharpening a carbide spiral, clearance is lost and thus lower tool life cycle is achieved. Life Cycle estimate 24:1 - a conservative value!
| -- | -- | -- | -- | -- |
| Comparison Data | Carbide | Diamond |
| Initial Tool Cost | $65.00 | $388.00 |
| Sharpening Cost | $16.50 (x2) | $125.00 (x2) |
| Tool Life | 85 panels | 2000 panels |
The next two pages contain information that is critically important to preventing tool breakage and maximizing tool life. Please take the time to review.
¶ Chip Loads / RPM / Feed Speed
Correct chip load is an important factor to extend tool life and avoid premature tool wear! The chip load is the size of the chip the tool makes during the cutting cycle and it is calculated based on the number of flutes on the tool, the spindle speed and the feed progression. The below chart is a starting point reference range only! The below range is based on cutting depth being equal to cutting diameter. For deeper cuts, adjust the chip load as follows: for 2x diameter, reduce by 25%, 3x diameter reduce by 50%.
| -- | -- | -- | -- | -- |
| Tool Diameter | Hardwood | Plywood | MDF / Particleboard | Soft Plastic | Hard Plastic | Acrylic | Solid Surface |
| 1/8" | .003" - .005" | .004" - .006" | .004" - .007" | .003" - .006" | .002" - .004" | .003" - .005" | .002" - .004" |
| 1/4" | .009" - .012" | .011" - .013" | .013" - .016" | .007" - .010" | .006" - .008" | .008" - .009" | .006" - .009" |
| 3/8" | .014" - .018" | .017" - .020" | .020" - .023" | .010" - .012" | .008" - .010" | .010" - .012" | .008" - .010" |
| 1/2" | .019" - .021" | .021" - .023" | .025" - .027" | .012" - .016" | .010" - .012" | .012" - .015" | .010" - .012" |
Calculating Chip Load:
Calculator available here: www.guhdo.com/chipload-calculator
The formula is:
Chip Load = Feed Rate (inches per minute) / (RPM x number of flutes)
Example:
Feed rate of 500” per min / (16,000 rpm x 2 flutes) = 500/32000 = Chip Load is .015”
To calculate feed rate on the fly:
Example: Using a 2 flute 3/8” compression bit cutting MDF, and rpm of 16,000
Your formula is:
(16,000x2) x .023 (chip load per schedule above) = 736”/minute (adjust based on cut depth)
If your machine displays feed rate in metric values, take the metric value, example, 8 meters, and multiply by 39.37 to obtain the inch equivalent for your calculation.
¶ Finding Your Optimum Chip Load
When the chip is too small, the cutting action will generate heat in the cut and will cause the cutting edges of the tool to deteriorate prematurely. A larger generated chip within the reference range for a particular material will achieve the longest tool life.
You can find your optimum chip load, which will allow you to maximize productivity and get the best tool life and lowest cost per panel, if you follow the steps below:
Start using the recommended chip load and slowly increase your feed rate until the finish quality becomes unacceptable. Then slowly decrease feed rate again until desired finish is restored. Make note of your feed rate. Next, decrease the machine RPM's until the finish deteriorates. Once that occurs, increase RPM's until finish is once again restored. At this point, you have found the “sweet spot”
¶ Other Common CNC Tooling Solutions
¶ Spoil Board / Fly Cutter
A clean and level spoil board is prerequisite to good vacuum hold-down and machining accuracy. When setting up machining program, the routing tool should extend beyond the work piece and penetrate the spoil board by 0.3 – 0.6mm. Periodic resurfacing of the spoil board to maintain a flat, even surface is most efficiently performed with a large diameter fly cutter. (available in 40mm, 80mm or 100mm diameter).
For best performance these cutters should all be mounted in an HSK heat shrink tool holder
¶ High Quality Surface Planing Tool
An insert tool with special insert knives and edge radius provides a superb surface finish for applications such as MDF shaker style cabinet door cut outs. Using two additional tools (a 1/2” solid carbide bit and a 1/16” solid carbide bit provide the ability to produce a square corner cutout in MDF doors. For optimum results, this tool should be used on an HSK heat shrink tool holder.
¶ Insert Rebate Cutter
For rebate or deeper surface planing cuts, these insert tools provide a very economic solution as the replacement insert knives, when the tool is dull, usually cost under $6.00/cycle. The solid carbide inserts are available in different carbide grades to facilitate efficient cuts in either wood or composites.
¶ Deep Pocket Mortise Cuts
The further the cutting edge of a tool gets away from its clamping source, the more deflection is created and the bigger the risk of tool breakage. Considering the rule of thumb is that cut length shouldn’t exceed three times the cut diameter, that means that cutting a deep mortise pocket can represent a challenge. Special deep pocket mortise bits solve that problem as they are made from a very special high density alloy that prevents deflection and tool breakage despite the depth of cut.
Recommended RPM: 12,000-18,000
Gradual Plunge Feed: 12m/minute (up/down)
Max. Cut Progression: 8-10mm solid wood, 15mm composites
¶ V-Groove and Angle Cuts
For mitre folds, insert V-Groove Bits are available as standards for 45, 60 and 90 degree (included angle) cuts. Other angles can be produced as custom tools. The insert knives are double sided and provide two life cycles each. Insert V-Groove bits are also a great solution for lettering, engraving and decorative cuts as well as beveling the inside edges of shaker doors and square corner cut-outs.
The following slides show some examples of tooling options for specific materials. A solid carbide tool is often selected for most cutting challenges on a CNC machine. However, this is definitely not always the most cost effective solution. As you will see in the following frames, there are many options to choose from. Therefore, we recommend to look for the most economical option for the job at hand that doesn’t compromise end result. Carbide insert tools or diamond tools offer a lower cost alternative. These options are often overlooked by short-sighted decisions based on initial cost which can be deceptive. In the following slides, we present some examples for slotting, grooving, edging, drilling and profiling in a variety of materials, such as -
¶ Machining Multiplex, Veneered Composite Panels
- Insert Bit (22025)
- 3 Flute PCD Bit (13750)
- Solid Carbide Through Hole Bit (6028SC)
- Carbide-tipped Dowel Bit (6024)
- PCD Round over Bit
- PCD Jointing Bit*
- PCD Bevel Bit*
Similar Applications: Plywood and layered wood panels of different wood species, laminated with HPL.
¶ Machining Phenolic (left) Cement Fiber Board (Right)
- PCD 6815 2 Flute bit
- PCD Dowel Drill Bit
- PCD Dowel Drill Bit
- PCD Engraving/Grooving Bit (4389)
- PCD Radius Bit
Similar Applications: Cement Fiber containing wall panels, Swiss Pearl and particleboard panels with cement fiber content.
¶ Machining Aspen Plywood with Paper Laminate
- Z3 Compression Bit
- Gigaspeed PCD Milling Cutter 15700 (or for smaller diameter 6814)
- Solid Carbide Dowel Drill
- Carbide-tipped Dowel Drill
Similar Applications: Birch plywood veneer coated, other paper coated plywood panels.
¶ Machining Solid Wood (Oak)
- Insert Edge Profile (22530-97) 4) Carbide Insert Boring Bit
- Roughing Cutter Z3 on Heat Shrink Holder 5) Carbide-tipped Dowel Drill Bit
- Carbide Roundover Bit
¶ Machining Lightweight Veneered Honeycomb Panels
- Fourcut 3+3 Cutter set for Lightweight panels (custom)
- Z3 PCD Router Bit (15551)
- Z2+V2 Boring Bit w/custom grind
- Carbide-tipped dowel bits
Similar Applications: Plywood and layered wood panels of different wood species, laminated with HPL.
¶ Machining MDF/Veneer (left) and Cement Fiber (right)
- PCD Engraving/Grooving Bit (4389)
- PCD Slotting Cutter
- Insert Router Bit Z2
- Solid Carbide Dowel Drill
- PCD Cove (Ball nose) Bit
Similar Applications: MDF and HDF panels, gypsum board panels
¶ Machining Carbon Fiber Composite Material
- PCD Dowel Bit Z2
- PCD Router Bit Z2
- PCD Dual Cut Router Bit (Custom)
- PCD Z4 Opposite Shear Router Bit
Similar Applications: Fiber-glass reinforced panels
¶ Machining Particleboard with Wood Veneer and Particleboard with Stainless Steel Laminate
- Insert Router Bit 6243
- Solid Carbide Compression Bit
- Carbide Tipped Through Hole Bit
- Carbide Tipped Dowel Bit
- Megaspeed PCD Jointing Cutter Z4+2+4
- Insert Trim Bit (for portable router)
Similar Applications: Particleboard panels with other laminates
¶ Machining Polyurethane Foam (PU) with Aluminum Laminate
- Insert Plunge Router Bit (Custom)
- PCD Dowel Bit Z1
- PCD Router Bit Z2
- PCD Fourcut Roughing Bit
Similar Applications: PU panels with other laminate coatings top and bottom.
¶ Profile and Custom Tooling Doors, Cabinets and More
¶ Cope/Stick Tongue & Groove Raised Panel Tooling
Larger profiles and tool assemblies that can provide flexibility such as the ability to machine various door thicknesses or tongue width, are manufactured on arbor adapters as sets with replaceable insert knives.
Caution: Some manufacturers have patented insert tool systems (unique
insert blank) that restricts sourcing and can impact competitive pricing!
¶ Made-to-Spec Tooling
Most CNC profile tooling is made-to-order. The process is very simple. A profile drawing or material sample is supplied in order to obtain a firm price quote. Once an order is placed, a dimensioned drawing is submitted for review and revision. Once the drawing is completed to satisfaction a last approval is needed to proceed. Larger profile tools are usually made of an aluminum tool body mounted on an HSK arbor adapter in order to adhere to typical CNC machine spindle weight restrictions.
¶ Short Run Profile Tool Flexibility
A corrugated knife adapter fitted with a heat shrink tool holder provides flexibility needed for proto-type production and ”one-off” projects that won’t break the bank. This tool body is made of steel and is available to accept either 8mm , 5/16” ,¼” x 60 degree corrugated knives. This tool is designed to accept knives of length 40, 60 and 80mm corrugated knives. Similar cutters are seen in the market with an aluminum body but we strongly suggest you stay clear of such cutters as the aluminum corrugations in the head will eventually wear out and the tool can become a real danger to operate!
¶ Helical Planing Cutter for Large Rebates, Jointing, Trimming in Millwork Operations
Advantages:
Excellent finish with solid carbide, 4-sided insert knives resulting in considerable savings compared to solid carbide tool. Excellent chip removal and very quiet running due to helical design. Perfect solution for many millwork tasks such as arches and window production. This cutter features scoring (spur) insert knives on the bottom to cut clean corners in a rebate cut.
¶ Saw Blade and Groover Adapters for a CNC
¶ Saw Blades Adapters for CNC's
Depending on blade diameter needed, there are several options for use of sawblades on a CNC machine. The shank style adapter, (on the left), is designed for blades up to 8” (200mm) diameter. Below left is a design with saw collars, which provides blade stability for up to 16” (400mm) diameter blades and the assembly below (right) is for blades up to 14” (350mm) and available in several ”A” dimension lengths.
¶ Saw Blade Flange on HSK-F63 Arbor Adapter for Blades up to 14" in Diameter
¶ Saw/Grooving Blade Adapter for Blades up to 8" Diameter
¶ Aggregate Heads
An aggregate head can provide 5-axis capability with boring/sawing outputs that facilitate horizontal boring and vertical sawing/grooving. Single, double and even four outputs on the same head. Torque arm connections are machine specific and must be verified at the time an
aggregate head is ordered. GDP aggregate heads are manufactured in Germany and adhere to the highest standards of quality and accuracy!
¶ Tool Presetters and Setup Fixtures
Tool setup fixtures are available in a variety of executions, from the very simple version of a setup tool holder fixture to more expensive and elaborate tool presetters. Regardless of choice, accurate tool setup will save much time and material waste and insure repetitive accuracy of the final product!
¶ Spindle Calibration Bar
A high precision Spindle Calibration Test Bar (pictured left) allows measurement of spindle accuracy which is an important maintenance item of CNC ownership. Indispensable to test runout and alignment after initial machine installation or relocation, after an unexpected ”crash” or simply as a periodic performance test. This will identify spindle issues long before they become bigger and more costly repair items.
¶ Spindle Dust Plugs
Spindle plugs, (pictured below) serve to protect the spindle motor from dust intrusion when the machine is either being moved or the machine is performing a saw/grooving operation or horizontal drilling application. Preventing dust from getting into the spindle motor will insure best maintenance practices and reduction of repair cost.
¶ Trouble Shooting
Tell-tale signs on these photos show us some corrective measures are needed to extend tool life. On the top photo, collet marks are visible on the tool shank. This is an indication that vibration is occurring during the cutting cycle, and it contributes to poor tool life, poor finish quality and can also cause the tool to break at its weakest point, which is right below the shank. Tool breakage is usually the result of one or a combination of: bad/worn collet, poor quality tool holder or collet nut, incorrect torque, vibration during the cut, clamping the tool too high on the shank, too shallow a cut in relation to cut length of the tool, running the tool when it’s dull!
¶ Evidence of Heat in the Cut
When you see the residue of heat, either black/burned material buildup or a blue discoloration of the carbide or tool body itself, it is time to go over the machining parameters to obtain the correct chip load. This will require one or a combination of:
- Increasing Feed Speed
- Reducing RPM
- Changing to a tool with less flutes.
This photo shows too much heat generated during the cutting cycle which impacts tool life quite dramatically. When this pattern is seen on a used tool, the chip load is incorrect and the feed rate most likely needs to be increased which will increase the chip size. This can also occur from slowing down too much in corners and depending on the application and feasibility, could be corrected by programming to loop. (see image below).
¶ Tool Breakage
| -- | -- | -- | -- | -- |
| Possible Cause | Remedy |
| Deflection – cutting edge too long | Select a tool with cutting edge not more than ¼” longer than material thickness. |
| Bad or worn collet | Check tool shank for evidence of chatter marks. When visible, replace collets. |
| Over-torqueing | If tool breaks in the shank area, tightening the collet nut to incorrect torque can cause tool breakage. Invest in a setup-fixture and torque wrench. |
| Overheating | If signs of heat buildup are in the tool flute, check chip load and adjust feed/speed. |
| Part Movement | Improve vacuum hold-down. |
| Too much pressure on the tool tip | For rebates, grooves, slots, use the shortest length to avoid tool breakage. |
| Tool slippage in the collet | Replace static collet nut with a bearing nut. |
