Hard millingrequires the utmost attention to detail to achieve maximum performance and tool life and tight tolerances down to 0.0001 inch. These tips help machinists get the most from hard milling.
Maintain a constant chip load and feed rate. Machine tools rapidly fluctuate feed rates when machining complex surfaces and cutter paths, which drastically reduces tool life. Machinists must understand that when machining complex surfaces, machine tools do not reduce rpm in conjunction with feed-rate reductions. So, if the machine cannot maintain programmed feed rates 80 percent of the time, operators should record the average feed rates and then reduce the feed rates and rpm accordingly. For example, if an operator programs a 30,000 rpm and a 150-ipm feed rate, but the machine can only maintain an average feed rate of 75 ipm, the operator should reduce the rpm to 15,000. The subsequent reduction in rpm will increase tool life by 50 percent and impact cycle time negligibly.
Do not leave extra stock for finishing. When machinists are machining tool steels above 48 HRC, extra finish stock will reduce output and wreak havoc on surface finish and tool life. A general rule for finish-stock allowance is 1 to 2 percent of the finish-cutter diameter. Most cutting-tool manufacturers base their finishing cutting data on 1 to 2 percent of the tooling diameter engagement, so leaving more than that decreases productivity. For example, when using a tool with a 0.5-inch diameter, leave no more than 0.005 to 0.010 inch of finish stock.
Leave consistent stock on all surfaces. After a machinist roughs a complex surface, he or she should run a rest-rough and semi-finish tool path to ensure consistent finish stock on all surfaces. For example, when a machinist roughs out a complex 3D surface using a 12-millimeter ball-nose end mill, and the intended finishing cutter diameter is 8 millimeters, a safe practice for ensuring 0.003 to 0.006 inch of stock on all surfaces is to rest-rough with a 10-millimeter ball-nose end mill and then semi-finish with an 8-millimeter ball-nose end mill. Then the machinist should finish mill with a new 8-millimeter ball-nose end mill to ensure all surfaces have a consistent surface finish. This practice also extends finishing cutter life and enables the machinist to use the finishing ball-nose end mill as a semi-finishing tool when the life of the finishing tool ends.
Use strong, precise toolholders. High-precision holders are crucial when hard milling to achieve maximum tool life. Run-out must be limited to less than 0.0004-inch to maximize tool life. Machinists can achieve this level of precision with most shrink-fit holders, milling chucks, high-precision collet chucks and select end-mill holders. A precise holder ensures process accuracy, whereas a less secure holder can cause unpredictable tool life and produce out-of-tolerance surfaces.
Follow recommended cutting parameters. Cutting data is optimized according to the tool’s design and for specific material groups, as some common hardened tools steels present unique challenges, so machinists should use recommendations as a starting point. The machinist can make modifications depending on the application.
Tips for Successful Hard Milling
Use a strong insert geometry, like a button (round) insert
Use a strong cutting edge – a T-land or K-land insert can better hold up to the stress of the hard milling
Use a very hard grade of carbide that can handle the heat without deformation
Use a high-temp. coating designed for hard milling or high-temp. alloys
Use a light width of cut, typically between 25-40%
Use a light depth of cut, usually between .005″-.015″
Use a light feed per tooth, usually less than the T-land width (.003″-.006″)
Good air blast should be used – no coolant (thermal shock)!
Employ a dynamic tool path to maintain cutter engagement with workpiece
Even common hardened tool steels in the Mold and Die industry present unique challenges. Take for example D2 tool steel that can be heat treated to 60-62 HRc. Because of the added Chromium content, this tool steel is not only hard but also tough, making it machine similar to tool steel that is 62-65 HRc.
420 stainless steel is also very common in the mold industry because it is wear-resistant and can be polished to a mirror finish. Although this material is typically heat-treated to 48-52 HRc, it still retains its sticky stainless-steel properties and is prone to causing Built-Up Edge (BUE) making running the proper surface feet per minute crucial.
To achieve maximum tool life, high-precision holders are crucial to hard milling. For ultimate success, your run-out needs to be kept to less than 0.0004”. This type of precision can be achieved by most shrink fit holders, milling chucks, high precision collet chucks and select manufacturers’ end mill holders. A precise holder also ensures the accuracy of the process, whereas a less secure holder may cause unpredictable tool life and produce surfaces that are out of tolerance.
In today’s shops machinists encounter endless materials with properties that vary greatly. These materials are grouped into categories that are based on how they typically react to a cutting tool during machining.
Ferrous metals that are hardened to 45 HRC or greater usually are classified as hard materials. A common example of their use is in the die and mould industry where die steels, high-speed tool steels, and alloy steels often are found.
In the past components produced from hardened steels were roughed in the soft state, heat-treated, and then finished by an EDM or grinding process. However, advancements in tool geometries and coatings, increasingly accurate toolholders, and continually evolving machines and CAM toolpaths have enabled these materials to be cut in their hardened state with high accuracy and productivity.
The Challenges
Hard materials are challenging to machine for several reasons.
First, hardened steels typically have much higher springback than their annealed counterparts. This results in much higher cutting forces during machining. High cutting forces can increase a tool’s susceptibility to deflection and vibration, which results in poor part accuracy and surface finish.
Because these materials produce high cutting forces, milling tools for hard materials typically have negative rake angles, which makes the cutting edge dull to prevent chipping. This dull cutting edge results in increased friction during the cut, which in turn generates more heat at the cutting edge.
To offset the cutting forces, slower feed rates may be required, resulting in the tool dwelling in one area and subsequently creating even more heat over a longer period of time. This increased heat can cause the cutting tool coating to break down rapidly followed by the tool substrate.
This rapid wear of the tooling is another reason that hard milling is often thought of as challenging.
Larger-scale components in the mould and die industry often require a single tool to finish a large surface area. Because the tool breaks down rapidly when machining hardened materials, it may become too worn to produce a satisfactory surface roughness as it progresses through the part. This often results in the need for a second finishing process, increasing part cycle times and, in turn, manufacturing costs.
Choosing the correct tool, holder, and toolpath is crucial to the success of milling hard materials accurately and efficiently.