Technology Why mould makers can’t treat cutting tool choice in isolation
They say only a poor workman blames his tools, but selecting the proper ones isn’t always that easy. Cutting tool suppler Seco Tools (UK) Ltd offers a few tips for die and mould shops.
Advancements in milling techniques and tooling have enabled UK mould makers to reduce part cycle times and lead times, increase accuracies and repeatability, achieve superior surface finishes and control manufacturing costs.
A range of factors goes into cutting tool selection
A direct result of these improvements in performance and increases in productivity has seen shops become better able to compete against, and win back mould making contracts from, lower cost economies. An important element in improving machining performance for mould makers is the correct identification and selection of the optimum cutting tools. But, essential as this is, it is only part of the equation and cannot be treated in isolation because of other factors to consider. Machine tool type and capability, intended milling techniques, programming, work-holding and tool-holding are all important and have a direct influence on cutting tool selection.
Equally critical remains the ability to analyse worn cutting inserts in an effort to both maximise tool life and predict tool usage in tool and mould machining applications.
First up: Machine tools and milling techniques
Fast and powerful machine tools with increased programming capabilities are essential when it comes to taking full advantage of the latest cutting tools and to get the most (and best) from highly-effective milling techniques. High-feed milling and high-speed milling are two popular milling techniques that require certain types of cutters for operational success.
High-speed milling is becoming increasingly popular. It is also particularly effective when using solid carbide cutting tools. This milling method employs an optimised roughing approach that combines large cutting depths with relatively small radial engagements when cutting steel. This technique is also effective when machining materials 60 HRC and harder.
For high-feed milling, specially-designed large indexable insert cutters are recommended to remove the majority of material. Essentially, the process starts with relatively large indexable insert cutters for roughing, and works down to smaller-diameter indexable ball nose cutters and solid carbide cutters as the mould approaches its near complete shape.
Size and geometry play a role, too.
The selection of the most effective cutter diameters is determined by mould features – such as corner radii. High-feed indexable insert cutter diameters are usually 15 mm and larger. If smaller cutters are needed, solid carbide end mills are used.
Inserts for high-feed indexable cutters can vary depending on work-piece material, but most applications will dictate that a PVD-coated or CBN-coated insert is used.
As for insert geometry, Trigon-style inserts provide the lowest possible lead angle over round or square inserts. Low lead angles produce a much thinner chip, which in turn requires higher feed rates to maintain proper chip thickness for the insert geometry. The lower lead angle also directs the cutting forces in the axial direction, pushing up into the spindle, which is more stable and easier on the machine. Higher lead angles create thicker chips requiring fewer adjustments to feed rates. In addition, they also produce more radial force, causing vibration and stress on the spindle bearings. Solid-carbide cutters used for high-speed milling are typically four-flute shoulder end mills with long cutting edges and built-in chip splitters. The chip splitters break up chips into small, manageable sizes – resulting in improved evacuation from the cutting zone, as well as from the machine. Additionally, full cutting lengths and chip splitters - when combined with high-speed milling - generate increased levels of productivity and significantly higher tool life due to consistent loads.
Settings important for best milling results
During high-feed operations, cutters should be run at full diameter engagement, but no less than half their insert width. Full diameter engagement is possible because high-feed cutters effectively direct cutting forces at the machine spindle in the axial direction to create balance. Cutters engaged at less than half their insert width will experience push and increased vibrations because the cut is unbalanced. For high-speed milling, the same types of tools (indexable insert cutters and solid-carbide end mills) used for high-feed milling are applicable as long as they have geometries conducive to using high spindle speeds and feed rates.
While high-feed end mills with long overhangs are effective in high-speed operations they cannot be run as fast as tools with shorter overhangs (unless specialised vibration dampening tool holders are used or cutting speeds are reduced significantly). When a tool with long overhang operates faster than recommended, excessive vibration can be the result, causing insert chipping and premature insert failure.
Insert wear analysis points out problems of the process
Maximum tool life and predictable tool usage are critical in optimising mould machining operations. Mould makers must understand the various insert failure modes and examine used inserts to determine the root cause of failure. To assist in the examination of inserts, a stereoscope - with good optics, adequate lighting and a magnification of at least 20 times - can help identify failure modes that contribute to premature insert wear.
There are eight common insert failure modes. Of these, flank wear, thermal cracking and chipping are the ones to watch out for when machining moulds. However, using unsuitable inserts during the process can cause the other five modes to occur.
- Flank wear occurs uniformly and happens over time due to the insert’s cutting edge becoming dull or worn. With normal flank wear, a relatively uniform wear scar will form along the insert’s cutting edge. Occasionally, metal from the work-piece smears over the cutting edge and exaggerates the apparent size of the wear scar on the insert. To slow down normal flank wear it is important to employ the hardest insert grades as well as using the positive cutting edge to reduce cutting forces and friction. On the other hand, rapid flank wear often occurs when cutting abrasive materials such as ductile irons, silicon-aluminium alloys, high temperature alloys, heat-treated PH stainless steels, beryllium copper alloy and tungsten carbide alloys. The signs of rapid flank wear look the same as normal wear, and avoiding rapid flank wear requires a more wear-resistant, harder or coated carbide insert grade be used.
- Cratering is caused by a combination of diffusion and abrasive wear in inserts. Heat build-up in the workpiece chip causes elements used in the cemented carbide to dissolve and diffuse into the chip, creating a crater on the top of the insert. The crater will eventually grow large enough to cause the insert flank to chip and deform, or possibly result in rapid flank wear. While common coatings will provide crater resistance, an aluminium oxide type is recommended.
- Built-up edges occur when fragments of the workpiece are pressure-welded to the insert cutting edge. Eventually, the built-up edge breaks off and sometimes takes pieces of the insert with it, leading to chipping and rapid flank wear. Built-up edges are identifiable by erratic changes in part accuracies or finish, as well as by shiny material appearing on the top or the flank of the insert edge. Built-up edges are controlled by increasing cutting speeds and feeds, using nitride (TiN)-coated inserts, and selecting inserts with force-reducing geometries and/or smoother surfaces.
- Chipping of insert cutting edges originates from mechanical instability often created by non-rigid setups, bearing wear, worn spindles, hard spots in work materials, or interrupted cutting operations. Ensuring proper machine tool setup, minimising deflection, using honed inserts, controlling the creation of built-up edges, and employing tougher insert grades and/or stronger cutting-edge geometries will reduce chipping.
- Thermal mechanical insert failure is a combination of rapid temperature fluctuations and mechanical shock. Stress cracks form along the insert edge, eventually causing sections of the insert’s carbide to pull out and appear to be chipping. A sign of thermal mechanical failure is multiple cracks occurring perpendicular to the cutting edge. Thermal mechanical failure can be addressed through the correct use of coolant or to remove its incidence completely, by employing a more shock-resistant grade and using a heat-reducing geometry.
- Edge deformation arises from excessive heat combined with mechanical loading, as is often the case with mould machining. High temperatures can occur when machining with high speeds and feeds or when machining hard steels, work-hardened surfaces and high-temperature alloys. This causes the carbide binder or cobalt in the insert to soften. Edge deformation can be controlled by using a more wear-resistant insert grade with lower binder content, as well as by reducing speeds and feeds and employing a force-reducing insert geometry. Notching becomes noticeable when chips (or notches) appear in the depth-of-cut area on an insert. To prevent notching the following should assist: vary the depth-of-cut when using multiple passes; use a tool with a larger lead angle; increase cutting speeds when machining high-temperature alloys; reduce feed rates; carefully increase the hone in the depth-of-cut area; and, prevent build-up, especially in stainless steel and high-temperature alloys.
- Mechanical fracturing of an insert occurs when the imposed force overcomes the inherent strength of the insert cutting edge. Any of the seven previously mentioned failure modes can contribute to fracturing and this phenomenon can be avoided by using a more shock-resistant grade, selecting a stronger insert geometry, using a thicker insert, reducing feed rates and/or depth-of- cut, verifying setup rigidity and checking the work-piece for hard inclusions as well as difficult entry.
Cutter grades, geometries, materials and sizes
Many cutting tool manufacturers develop cutting tool grades and geometries for specific materials. In mould machining, those materials are typically P20 steels, CPMV 10 and powdered metals. It is therefore critical to select the grades and geometries best-suited to the particular material being machined to avoid premature tool failure. Additionally, matching cutting tool to material increases performance and predictability, resulting in fewer tool changes, fewer rejects and reduced re-working.
If the material used is 52 HRC or softer, general-purpose solid carbide tools work well. For materials harder than that, solid carbide end mills with different geometries and coatings such as aluminium titanium nitrate (designed for extremely hard materials) should be used. It is worthwhile remembering that for solid carbide tooling there are special blends of coatings, unique to individual tooling manufacturers, available. For indexable insert cutters, insert geometries and coatings for hard milling will work for extremely hard powder metals. And the different insert grades and chip grooves available on today’s indexable insert cutters make it possible for machining harder mould materials.
Once cutter types are determined, proper cutter radii sizes must be selected. Cutter radii must be smaller than inside mould corner radii. If the radius of a tool matches the radii of a mould’s corner, a hard stop will occur. For the finishing process, smaller diameter solid carbide cutters are recommended.
The same radii principle is true for roughing operations, i.e., using cutter radii smaller than those of the work-piece and, while this leaves more material in corners, it helps maintain consistent and better evenly distributed cutter load for all subsequent semi-finishing and finishing operations.
Just as critical as cutter radii is cutter rigidity where cutter draft angles/tapers play a key role. Most cutters have either relief neck or tapered neck styles. Relief neck tools have a smaller diameter than the flute size above the flutes and below the cutter’s shank diameter. With tapered neck style tools, there is the cutting diameter and above that a smaller relief area and a taper up to the shank diameter. Most long-reach cutters incorporate tapered neck designs.
Less draft angle means more rigidity in the tool. But, draft is needed to avoid rubbing against mould cavity sidewalls. To select the most rigid cutter, mould cavity drafts need to also be taken into consideration.
Cutting tool drafts should never match or exceed mould drafts. For instance, if a mould cavity has a 3-degree draft on all its sidewalls, tools with drafts up to 2.5 degrees on their relief can be used.
The roles of coolants and tool holders
As far as the use of coolant is concerned in mould machining, most of today’s advanced cutter designs and geometries perform at their optimum when run dry. The exception is running with oil mist, but doing so at all times. For hard milling, the rule is absolutely no coolant use at all, unless oil mist is available.
Most cutting tool companies recommend vibration-dampening holders for mould machining and for use with today’s advanced cutters. The best tool in a below-par holder will fail to achieve optimum performance and tool life will be impaired whereas, with advanced high-performance holders, tool life can potentially be doubled.
Vibration control is critical, especially with long tool gauge lengths and in high-feed roughing operations. The key is that any vibration-dampening holder has been designed to reduce harmonics and any vibration generated by the cutting process.
Using the best possible toolpaths
Mould machining cutter paths should be optimised by correct programming to avoid placing unrealistic demands on cutting tools. For example, when machining a mould and the toolpath encounters a corner, a smooth transition must be programmed to allow for the change in direction in order to prevent a large angle of engagement which could overload the cutting tool. A good rule of thumb is to program an arc that is larger than the cutting tool’s radii. So, if a 50 mm diameter cutter is used, the program should not encounter 25 mm radii, but instead use a smoothing radius that is larger.
Programming proper arcs can be a challenge and, if not done properly, can lead to erratic toolpaths. Several current software packages can help accurate programming and an experienced programmer with an understanding of the arc of contact principle is obviously a bonus. The key is to avoid machine stop and start scenarios within the toolpath because any amount of machine hesitation when changing directions generates heat that transfers to the tool. Heat can destroy a tool’s cutting edge and coating, and must be evacuated from the cutting zone through and with the chips.
By gaining a better understanding of today’s milling techniques and tooling technologies as well as the various failure modes and failure analysis skills, mould manufacturers can experience increased productivity, reduced cycle times, better tool life and tool life consistency, improved part tolerances and appearance, superior mould surface finishes, and less wear and tear on equipment.