CNC Tooling

Cutting Tool Geometry:
The tool geometry influences cut quality, cutting speed, chip removal, and the life expectancy of the tool in a specific material. Choosing the right tool for the specific material being routed can be critical. There are several different geometries to choose from such as upcut / downcut helix, straight flute, and ball nose, to name a few. The cutter selection of this catalog defines in more detail the ideal geometry for specific materials. Illustrations on the next page shows basic terms used to define a tool's geometry.

Router Bit Materials:
There are four basic materials to choose from when selecting a router bit for a specific application: High-speed steel, carbide tipped, solid carbide and PCD diamond. The choice of a specific tool depends on the material being routed. High-speed steel and carbide tipped tools tend to be used more with handheld routers vs. CNC routers. The steel body of the tools tend to withstand the vibration caused by the inconsistencies of handfeeding the router. Another reason they are used with hand routers is that they are available in many geometries for low cost, and available at most home centers. The ideal choice for a CNC router is solid carbide or PCD Diamond. Solid carbide is the most common router bit used on CNC's. It provides long life due to the tougher body construction (carbide), delivers the best edge finish, largest variety of geometry profiles available, can achieve greater feed rates, is the best tool for plunging into the workpiece and has relatively low cost. PCD Diamond tools are ideal for very abrasive materials. These type of tools, however, are not cheap, perform very poorly on nonabrasive materials, cannot plunge, and are limited to how fast they can route.

































Heat:
Heat generation in cutting tools should be avoided. Heat can change the properties of the tool and melt or burn the material being routed. This can lead to very poor surface finish, causing the tool to fail/break, or material melting and wrapping onto the tool. There are many causes of heat buildup such as improper tool selection, incorrect machine feeds, incorrect spindle rpm and/or rotation, and improper toolpath programming. In order to minimize or eliminate the heat buildup, you must avoid the above causes. To determine if you have programmed the feeds and speeds correctly, you can follow these simple formulas:

Formula 1: Chipload = chipload % x cutter diameter
Formula 2: Feed Rate = [chipload] x [# of flutes] x [rpm]

A good starting point for determining chipload (thickness of the chip) is 2% of the cutter diameter (example 1/4" cutter = .005). For softer materials, it is recommended to take 4% of the cutter diameter.

2% Hard material:
Brass, hardwood, cast acrylic, solid surface

4% Soft material: Aluminum, MDF, particle board, extruded acrylic, sintra, polycarbonate

Chipload = [2% or 4%] x [cutter dia]
Feed Rate = [chipload] x [# of flutes] x [rpm]

Example 1:
1/4" 2-flute endmill (Hard Material)
Chipload = .02 x .25 = .005
Feed Rate = .005 x 2 x 18000 = 180
Feed Rate = .005 x 2 x 12000 = 120
Feed Rate = .005 x 2 x 6000 = 60

Example 2:
1/4" 4-flute endmill (Hard Material)
Chipload = .02 x .25 = .005
Feed Rate = .005 x 4 x 18000 = 360
Feed Rate = .005 x 4 x 12000 = 240
Feed Rate = .005 x 4 x 6000 = 120

Note that for each cutter, there is a feed rate range that corresponds to the rpm range. The number of flutes determines the range at which a cutter should be fed. The number of flutes should be taken into consideration when cutting material. 3- and 4-flute cutters are best for high feed rates, while 1- and 2-flute cutters are best at lower feed rates. Also, keep in mind that spindles have peak power at higher rpm. It is better to use a 2-flute cutter at 18000 rpm than a 4-flute at 9000 rpm.

When dealing with material that melts, a thicker chip will reduce melting. When cutting deep into these materials, it becomes important to remove the chips from the cut. Cutters with fewer flutes are better capable of removing these chips. Also, larger cutters are better for dealing with melting.

Collets:
There are two basic types of collets, half-grip and full-grip (see below). Half-grip collets are identified by slits running from the bottom (or “mouth”) of the collet toward the top for about 80% of the collet length. This type of collet grips the router bit at the mouth of the collet. Half-grip collet is the simpler of the two collet types, and is ideally used with shorter shank tools where the shank would not fill the entire length of the collet. Full-grip collets have slits running up from the bottom and down from the top, again for about 80% of the collet length. This type of collet grips the tool evenly over the entire length of the collet and tends to have more flexibility, which results in "ranged" or "universal" collet sizes. This means that a specific collet size can hold a range of tool sizes (typically inch and close metric sizes). Collets are made from spring steel, and regular usage causes loss of elasticity and the need to replace them more often. It is recommended to use collets designed for specific size tools, as requiring the collet to expand for too-large tools or compress for too-small tools will shorten the life expectancy of the collet.



Proper Tool Colleting:
Installation of the tool in the collet and collet nut is equally important. To prevent unnecessary strain on the collet and to ensure a proper fit, only use a collet designed to fit your tool shank diameter. In addition, the tool's flute should not extend into the collet; doing so can score the inside of the surface, as well as force debris into the collet, putting the entire assembly off-balance and potentially damaging the spindle. The graphic below illustrates the correct and incorrect installation. Please note that these illustrations are designed to show proper insertion of the tool into the collet, and do not show the collet nut.



Collet Maintenance:
Tool geometry, cutting material, and machine feeds and speeds are all important to the machine's performance. Basic tooling maintenance should be at the top of this list. Proper colleting and collet maintenance are essential, and directly affects the cut quality and longevity of the spindle. A clean collet, tool holder, router bit, and spindle taper allows for a firm grip of the tool, preventing tool runout. "Runout" occurs when the tool and spindle do not share the same center of rotation (they are not concentric). This runout puts enormous strain on the spindle bearings and can cause the spindle to fail prematurely. In addition, a tool that is not perfectly concentric will result in an uneven, wavy cut. It is recommended that the collet, tool holder, router bit, and spindle taper be cleaned each and every time you change a tool. When the machine is running, dust and debris collects in all crevices of the spindle, while resins can build up on the tooling. These resins will usually build up around the mouth of the collet. Because of this buildup, the tool may not be properly gripped, and a loss of concentricity ("runout") of the tool results. Proper cleaning and maintenance easily solves this problem.



Spindle Taper:
Proper maintenance for optimal performance does not stop at the tool or the tooling accessories. Care should be taken to extend cleaning to the spindle as well. For instance, regular cleaning of the inside of the spindle taper should be part of your maintenance regimen. In addition, always leave a tool holder in the spindle, even when the machine is not in operation. This will greatly reduce the amount of dust and debris that can enter the spindle's interior, subsequently causing premature spindle failure.

Accessories: CNC Tooling