ME 23/123

There are times when you won’t be able to avoid a jobber length drill because the hole is too deep for a screw machine drill. In that case, you could spot drill to start the twist drill, or you could drill the shallow part of the hole with a screw machine length and then switch to the longer drill bit. Either way you’re facing a tool change, so it’s six of one and half a dozen of the other.

NC spot drills due not have body clearance and are not designed to drill greater than the depth of the point angle. The 90º and 120º spot drills are primarily used to create an initial spot for 118º and 135º secondary drills respectively. The 142º point NC Spot drill, is designed to help center carbide drills with an angle of 140º.

Note for Carbide Drills: The center of the carbide drill bit must make contact with the center of the spot drilled hole, if the outer edges make contact first, it will chip the drill bit!

For additional information regarding CNC Drilling, please click here. 

Please click here for more information on machining deep pockets.

Please click here for more information on plunge milling.

End Mill Selector: 

End Mill Selection Synopsis:

• A ¼″(6mm) end mill is much stronger than an 1/8″(3mm) end mill, this a 4th order equation, so unless absolutely necessary, try to select the largest tool that will do the job. The law of diminishing returns applies here, as once end mills reach ½″(13mm) in diameter, they are typically strong enough to cut anything we need to, and at that point larger tools just cost more money without much gain in strength or stiffness. Execution of this point often arises when deep pocking is needed, if this is indeed the case try to design the parts with sufficiently large radii.

• Select the shortest tool that will do the job. Almost every cutting tool used on a milling machine is essentially a cantilevered beam whose stiffness is inversely proportional to the cube of the length sticking out of the collet. So always select the smallest L:D (length-to-diameter) ratio possible for increased productivity, tool life, and surface finish.

• Flute Count: as simple as it seems, a tool’s flute count has a direct and notable impact on its performance and running parameters. A tool with a low flute count (2 to 3) has larger flute valleys and a smaller core. As with LOC, the less substrate remaining on a cutting tool, the weaker and less rigid it is. A tool with a high flute count (5 or higher) naturally has a larger core. However, high flute counts are not always better. Lower flute counts are typically used in aluminum and non-ferrous materials, partly because the softness of these materials allows more flexibility for increased metal removal rates, but also because of the properties of their chips. Non-ferrous materials usually produce longer, stringier chips and a lower flute count helps reduce chip recutting. Higher flute count tools are usually necessary for harder ferrous materials, both for their increased strength and because chip recutting is less of a concern since these materials often produce much smaller chips.

Do not use more than 3 flutes when full slotting in non-ferrous materials like aluminum.

• Chattering Issues: try using a variable helix, or variable pitch, geometry is a subtle alteration to standard end mill geometry. This geometrical feature ensures that the time intervals between cutting edge contact with the workpiece are varied, rather than simultaneous with each tool rotation. This variation minimizes chatter by reducing harmonics, which increases tool life and produces superior results.

• Use roughing tools for roughing and save finishing tools for finishing. Roughing tools are much stronger than finishing tools because they have generous fillets or chamfers on their cutting tips and serrated edges to break up chips into smaller pieces for improved evacuation and less chance of re-cutting.

• Roughing End Mill Types:

  • Coarse Pitch: For deep slotting and deep profile applications in softer steels and non-ferrous materials, with heavy material removal.

  • Fine Pitch: For smaller and lighter cuts in hard materials, leaving a better surface finish.

  • Sinusoidal: For titanium alloys, with higher metal-removal rates at increased feeds.

• Roughing End Mill Benefits:

  • Ease chip evacuation in deeper pockets, with the unique chip-breaking qualities of these roughers.

  • You can be more aggressive with feedrates, while using less horsepower than comparable standard tools.

  • The “tooth” design of these endmills virtually eliminates chatter during roughing operations, by creating a constantly interrupted cut.

• Understand the benefits of WC (tungsten carbide) tools (aka the 2.5 rules). WC tools can withstand approximately 2.5X more heat than HSS tool alloys (or more in the right application!). Coincidentally, WC is also about 2.5X stiffer than steel, which means it will deflect significantly less during heavy cutting. The downsides are that WC is approximately 2.5X more expensive and much more brittle (less tough) than HSS, which is why both tool materials remain popular in modern manufacturing.

• Use the right tool coating for the job (or none at all). The only tool coatings that work well when cutting aluminum are ZrN (zirconium nitride) or TiB2 (titanium diboride). TiN (titanium nitride), TiAlN (titanium aluminum nitride), TiCN (titanium carbo nitride) are intended for cutting ferrous metals and tend to gall when cutting aluminum.

• Shallower helix angles provide stronger cutter edges for hardened materials, decreased axial forces and cutting aggressiveness, less potential for tool pull-out, less flute engagement and therefore less potential for chatter. Higher helix angles provide a greater shearing action and therefore lower power requirements, increased axial forces and cutting aggressiveness, higher potential for tool pull-out, and more flute engagement and therefore more potential for chatter.

• Use multiple tools when cutting deep features. A standard length end mill may have flutes that measure 2×D in length, where D is the tool diameter. For example, a standard ½″ end mill may have 1″ of usable flute length. If cutting a feature that requires a longer end mill, always use a normal length tool first and only then switch to the longer tool(s) as necessary. In cases where the finish is important, longer end mills are also available with radially relieved shanks so they don’t gall the portion of the part previously cut.

• Not all end mills are center-cutting, meaning not all can be used to plunge mill (like a drill bit).

• End mills do not like to plunge cut, as they have serious trouble with chip evacuation, which leads to chip recutting, and damaged cutting edges. Predrill a hole before plunge cutting into the part, there are also ramping and spiral entry techniques that can be utilized in most CNC software packages that address these issues.

• Feeding an end mill too slowly is as bad for it as feeling it too quickly. When the chip thickness becomes too small, each cutting edge is smearing rather than cutting, which produces significantly more heat and quickly dulls the cutting edge. The general rule of thumb is to not feed an end mill slower than 25% of its recommended feed per tooth. So if the suggested chip load for a ½″ end mill is 0.004″/tooth, bad things will start happening when you drop the feedrate lower than about 0.001″/tooth.

Depth of Cut -vs- Radial Depth of Cut:

5-15% steep over is a good starting point for High Efficiency and Trochoidal Toolpaths
See pages 27 through 36 of the Helical Machining Guidebook for more details.

Implement these calculations once the hole size becomes smaller than 4 to 5 times the end mill diameter… 

"O" Flutes For Mechanical Plastics by LMT∙ONSRUD:

Mechanical plastics are steadily becoming the material of choice for the job shops and machine shops throughout the country. These plastics have proven to demonstrate excellent performance in gears, bearings, material-handling parts, and other machine components such as spacers and positioning mounts where reduction of vibration is essential. A few common mechanical plastics include: (ABS), Acetal, Delrin, Hydex, UHMW, nylon, polycarbonate, polyurethane, and polyethylene terephtalate (PTE). These plastics have consistently demonstrated predictable performance because of durability, machinability, and exceptional mechanical and electrical properties and are replacing metal for parts manufactured to resist wear.

In terms of machining mechanicals, they can be classified as a soft plastic. Soft plastic utilizes "O" flute router type tooling that tends to curl a chip during the machining process. (Figure 1-"O" Flute Chip Action) This tooling has been designed to attack soft plastics with a high rake and low clearance geometry that actually carves the material. This tooling, when properly applied within a narrow range of chipload, typically 0.004 to 0.012, will provide an excellent finish in mechanical plastics. The consequence of improperly curled chips is visible knife marks that adversely affect the finish, which remains the most important consideration in plastic fabrication. (Figure 2-Formation of Edge Finish)

"O" flute tools are manufactured from micro grain solid carbide tool material in straight and spiral configuration. The upcut, or right hand spiral is most readily utilized because of the need to evacuate chip in an upward direction in flat sheet or block applications. Upward movement of chips avoids welding, which is a common problem in the machining of plastic. The tools are available in either single or double edge cutting diameters. A single edge tool is an excellent choice for most machining applications and can accommodate those situations requiring smaller diameters. The only caution with single edge tooling is to avoid using diameters over 3/8’s because of balance issues associated with the tooling. If larger diameters are needed, the double edge alleviates the balance problem while providing a much improved bottom finish for slotting application, which are prevalent in the machining of mechanical plastics. The double edge tools additionally provide longer cutting edges for deeper cuts of two to four times the cutting edge diameter at aggressive feedrates.

In shops with high feed and speed CNC routers the use of router bits is common practice. The benefits of the tooling are understood, but this is not always the case in shops with CNC mills. In these environments, the tool of choice has traditionally been the end mill. These tools are intended for metal removal and do not possess the proper geometry to effectively machine mechanical plastics. End mills have minimal rake and low clearance and were designed as robust cutting tools for heavy loads. Also, minimal flute area on these multi-edged tools interfere with the process of clearing chips, and this along with inappropriate geometry, can easily aggravate melting and rewelding problems common in mechanical plastic applications. Besides the end mill dilemma, machining methodology in many shops remains constant because of past practices associated with milling metal. The feedrates and spindle speeds tend to be slow relative to the capability of today’s CNC machining centers and climb cutting with multiple passes are commonly utilized to enhance finish. These practices adversely affect productivity, profitability, and are the antithesis of the meaning of high speed machining.

The first step towards actual high speed machining is selecting an "O" flute router bit to machine mechanical plastics. The tool selection process is simplified by contacting a legitimate manufacturer of "O" flute router tooling with technical support capabilities. Once the proper tool is chosen, the user will be able to increase spindle speed and feedrate and boost productivity by 40 to 50 percent. In order to accommodate this process the direction of cut in almost all cases will be conventional in nature. Conventional cutting will provide a better finish by eliminating burrs associated with climb cutting and inefficient finish passes are avoided in the process. Also, the geometry associated with the "O" flute router tooling allows the user to cut without the use of coolant. This becomes particularly important in industries associated with medical devices where contamination of the mechanical plastic can become an issue. The increased feed rates associated with the heavier chiploads increases productivity and dissipates heat thus eliminating the need for coolant.

Climb Cutting VS Conventional Cutting in Plastics:

While Climb Cutting is the most prevalent method in metalworking and Conventional Cutting is the dominant method in woodworking, plastics routing is somewhere in between the two. There are usually significant differences between the finish on a Climb Cut part and a Conventional Cut part and the degree of difference can vary by plastic and cutter geometry.

The only rule of thumb that can be offered is that most soft plastics (HDPE, UHMW, Polypropylene, etc.) respond best to Conventional Cutting, while some harder materials (Acrylic, Polycarbonate, Nylon) can occasionally respond better to Climb Cutting. Typically Climb Cutting will only show an improved performance in the smaller diameters (less than 3/8"), but of course there are always exceptions.
The other factors when considering Climb or Conventional Cutting is the aggressiveness of the cutter and part hold down. Climb Cutting is a much more aggressive means of cutting and can chatter or move small parts that are not fixtured well. In most cases soft chips that are difficult to extract from the cut are also more likely to weld to the climb cut side rather than the conventional cut side. The best method of approach for most new materials is to run sample parts with both methods of cutting at the same feeds and speeds and make the determination from there.

Programming Parameters for Plastics:

Many CNC operators and/or programmers have previous experience in the metal working industry and that can be a detriment when attempting to use similar cutting parameters in acrylic. A typical finish pass in ferrous and non-ferrous metals can be as little as .004”-.005”. When this amount of material is remove in acrylic, it frequently will compress and cause the cutter to actually skip across the surface. This is due mainly to the high rake angles employed in plastic tooling and the aggressiveness of their cutting action. Without at least .015”-.030” of material to remove, most acrylic router bits will not have enough material to bite into and will actually show a deteriorated finished edge over the initial roughing cut.

Entry points can also be a troublesome issue during programming. While most acrylics do not exhibit the chip wrap problem prevalent in other softer plastics, their tendency to craze can sometimes inhibit their ability to be machined at high speeds during cutter entry. The most common method is to slow the feed rates down to compensate for this problem, but a ramped entry can work equally well and will not show the entry melt that is associated with direct plunging by router bits. Another issue on cutter entry is that because router bits do not have a centering point similar to drills (this is to allow flat bottom cutting), they will have a tendency to “walk” during the plunge. The visible result is a larger entry point then the routed channel that will follow. The result is somewhat similar to what a keyhole slot looks like with a large diameter hole followed by a smaller slot width. Once again ramped entry can reduce this effect, but it is easier to enter the cut by plunging into a scrap area and moving to the final cut path in a lateral direction.

As a final parameter to be considered, depths of cut are critical to ensuring consistent edge finishes and non-broken tooling. A good rule of thumb is a maximum of twice the cutter diameter per depth of cut. A favorite programming method is to use multiple depths of cut when cutter breakage is an issue and the to take a final clean-up pass of .015” for the entire material thickness. (see Figure 8) This gives a premium edge finish while preventing broken tools in the smaller diameters. It is a common concern that taking finish passes in small parts will cause the parts to move once they have been cut away from the scrap, particularly in intricate parts like letters. The best solution is to use the multiple depth pass/single finish pass method described above, but to not cut through the paper masking on the bottom side of parts. This allows the vacuum to continue holding the parts, while the .015” finish pass will not typically tear the parts off of the masking.

For additional information on machining plastics, please click here, some more info can be found here as well.

Tap Selection Synopsis:

Power Taps for CNC applications:

• Spiral Point Taps: these taps have a spiral cut with relief grooves, the spiral angle on the front cutting edges helps eject the chips and the angled edge also gives superior cutting performance. The primary disadvantage of these is they push the chips ahead of the tap–down into the hole in other words, this is not a big deal for through holes but is a bad idea for blind holes.

• Spiral Flute Taps: Spiral Flute Taps have an open spiral just like a drill bit, their primary advantage is they eject chips up and out of the hole. They are the preferable choice over spiral point taps for blind holes, click here for additional information on Spiral Flute Taps.

• Form or Roll Taps: Thread Forming taps don’t cut threads at all, instead they cold form the material.

  • With this process, the metal is pushed out of the way and compressed into position rather than being cut, there are no chips to remove. As a result, the taps themselves are less likely to break and the threads they form are stronger.

  • Form Taps do require different feeds and speeds and they require a different starting hole size, so be aware of that before using one. Click here for a Tap Drill Chart for Form Threading.

  • It is often believed they are only good for soft materials like aluminum but they can actually be used on materials up to a hardness of 36 HRC/(340 BHN).

  • One issue with quite a few of the roll forming taps is that unless they have a groove that allows cutting oil to escape, the oil will build up back pressure as the tap goes in, this will create a hydraulic lock and break the tap.

• Punch Taps: The Emuge Punch Tap – technology, also called helical cold-forming of threads, constitutes the fourth method for the production of internal threads besides tapping, cold-forming of threads and thread milling. This patented method was developed in cooperation between Audi AG and EMUGE-FRANKEN and presented for the first time to the public in 2014. Thanks to entirely new kinematics with a significantly shorter tool path, the Punch Tap allows for time savings of up to 75% compared to conventional cold-forming of taps, click here for more information on these taps.

Tapping Essentials:

For each toolholder type, there are multiple rows with scores from 1 to 4, where a higher score is better. 4 is the best score and 1 is the worst. 

Note: A Milling Chuck/Power Chuck is not the same as a Drill Chuck…

Best Application:

• For your absolute highest Material Removal Rates (MRR) milling and drilling applications, consider a Side Lock or Weldon Shank-style toolholder. We’re talking big indexable tooling for the most part, not solid endmills.

• For mid-sized milling and drilling, consider a Milling Chuck. This is your largest solid endmills and twist drills, say 3/4 to 1″ and up. Also consider these when you have chatter problems on your big tooling using a Side Lock holder.

• For lighter milling and drilling, consider an ER collet chuck. Anything 3/4″ or under makes sense.

• For high rpm applications, consider shrink fit toolholders.

Obviously there is some gray area of overlap in each of these cases, but this should serve as a good starting point for toolholder selection.

Tool Holder Essentials by HAAS Tip of the Day:

Keep all collets and their holders clean & dry… 

Radial Depth of Cut (RDOC): The distance a tool is stepping over into a workpiece. Also referred to as Stepover, Cut Width, or XY.

Axial Depth of Cut (ADOC): The distance a tool engages a workpiece along its centerline. Also referred to as Stepdown, or Cut Depth.

Do not exceed a ADOC of more then 1.5 times the cutter diameter! 

Please click on the drawing that you want: TRAK Lathe Part or TRAK Mill Part

Please click here for part fabrication instructions.

Please click here for the SolidWorks, DXF, STL, and G-Code files.

Please click here for the Wankel Rotary Engine drawings.

Please click here for the Wankel Rotary Engine setup sheets.