by Kip Hanson
Still doing the three step mouldmaking dance? It might be time for a change.
Although plastic injection moulding is a complex endeavor, the steps taken to produce moulds is a fairly standard, three step process that’s been defined for decades: rough machine the mould cavity together with all of its various inserts, cores and attendant components while still in a soft state, harden the heck out of everything, and then finish grind or EDM each piece to size.
That’s admittedly a gross oversimplification, but shops have been making moulds in much this manner for as long as there’s been EDM. With the advent of faster, more rigid CNC machine tools, however, along with CAM software able to generate highly efficient toolpaths and advanced cutting tools designed specifically for high feed, high speed machining of hardened tool steel, many shops have begun to jettison their traditional ways in favour of faster, more flexible mouldmaking processes.
It’s not that hard
As these same shops began doing more with their machining centres and less with their EDM equipment, a few brave souls said, “well, if I can finish the darned thing on my machining centre when it’s hard, why not rough it, too?” Just think: no more waiting days or weeks for the heat treater to harden a semi-finished mould. No more truing up that same mould to remove heat induced warpage. No more electrodes (or at least not as many). The number of machine setups is reduced, lead times to the customer are shorter, and if scrap does occur, it’s not quite as catastrophic as scrapping a tool that took weeks to produce.
Machining moulds from a hardened block of steel should be every mouldmaker’s dream. So why aren’t more of them doing it? “Probably half of the shops I work with are still using the traditional process of roughing soft, heat treating, and then finish hard milling their moulds,” says Jay Ball, North America product manager for solid milling at Seco Tools LLC. “Because of the improvements in CAM software, however, and also because of the advanced carbide, coatings, and cutting tool geometries that are now available, it is now more economical to rough and finish from the hardened state, often completing the mould in one operation.”
What is this magic bullet? It’s called high feed milling. Unlike high speed trochoidal toolpaths, which engage a significant portion of the cutter length and use shallow stepovers, high feed milling uses low axial depths of cut and relatively wide radial tool engagement, directing cutting forces up into the spindle. As the term implies, this makes for extremely high feedrates, even on lighter duty machines or those without a dual contact interface.
Despite its obvious advantages, Ball says many shops remain reluctant to travel down this now well established road, thinking that because they’ve had problems with tool life in the past when semi-finishing and finishing hardened mould cavities, that roughing would therefore be impossible, a perception that is simply not accurate. Need proof? Ball offers the following starting parameters, which are typical of a high feed milling strategy:
- Material: 48-56 HRc hardened tool steel
- Cutter: 12 mm (0.500 in.) torical bull nose high feed end mill
- Cutting speed: 137 surface m/min (450 sfm), or 3,600 rpm
- Feedrate: 0.36 mm (0.012 in.) feed per tooth, or 4.3 m/min (170 ipm)
- DOC: 0.56 mm (0.022 in.) axial depth of cut, and up to full-width stepovers
- Using that same cutter in 56-62 HRc material, Ball says the cutting speed and axial depth of cut were reduced by approximately half, but stepover amounts remained the same. In either case, the tools lasted a surprisingly long time. “These values may need to be adjusted based on the machine tool being used, the rigidity of the setup and toolholders, etc., but I have personally seen more than six hours of tool life when roughing hardened tool steels up to 56 HRc, and two to four hours in tool steel at a hardness of 56-62 HRc,” Ball says. “In the majority of cases, hard milling is a very stable, predictable, and productive machining process.”
The one exception is tool steel that’s high in chromium. Together with aerospace alloys such as Inconel, titanium, and other metals that “don’t like to be cut,” these materials are among the biggest thorns in any machine operator’s side. Even here though, thanks in large part to the chip thinning effect that comes with high feed machining, this modern metal removal strategy performs quite well, Ball explains.
Mix it up
Feed milling aside, don’t discount the trochoidal, high speed toolpaths common in the aerospace industry, especially if you’re machining one of Ball’s “don’t like to be cut” materials. Steve Avers, application support team leader at IMCO Carbide Tool Inc., describes a job he helped a customer with recently, one that required 50 mm deep (2 in.) insert pockets be cut in P20 die steel and used a similar machining approach known as high efficiency milling, or HEM.
“We were able to drive a 12 mm (0.500 in.) diameter IPC-7 two flute end mill at just over 2700 rpm using a 2.61 m/min (103 ipm) feedrate, an axial engagement of 41 mm (1.625 in.), and a 0.95 mm (0.038 in.) stepover, giving us a metal removal rate (MRR) of 6.28 in.3/min.,” he says. “This was a big advantage for the customer, as it was a long reach situation and we were able to achieve much higher MRR using HEM than we would have with traditional toolpaths and conventional end mills.”
Whether your machining strategy relies on low axial engagement and large stepovers (good for roughing most hardened steels), high axial engagement and small stepovers (good for roughing most everything else), or a combination of these programming approaches (perhaps the most common approach), it’s important to work with a supplier that has knowledgeable people who understand your materials, your machine tool’s capabilities, and your unique requirements.
IMCO, Seco Tools, and a number of other cutting tool suppliers have such people, as well as premium grade cutting tools designed to excel in mouldmaking and other demanding applications. Whichever path you take, however, be aware that specialty cutting tools like these aren’t inexpensive, at least compared to their generic counterparts; the message is clear—don’t let a little sticker shock scare you away from the possibility of greater mouldmaking success.
“The shops that are most progressive and wish to improve their metal cutting capabilities—whatever they are producing—are those that pay special attention to their tooling, their processes, and ways to maximize each,” says Perry Osburn, IMCO’s owner and president. “When I was a sales representative and ran into people that only cared about tooling costs, I knew that I should probably move on to the next shop, because the ones that buy everything based on price rather than performance often won’t be around long enough to worry about.”
Putting it all together
That might seem like a harsh statement, but the fact remains that you get what you pay for, and nowhere is this truer than in manufacturing; whether it’s the machine tool, the toolholders, or the cutting tools, no one should expect high performance from a less than optimal solution.
The same goes for CAM software. Ben Mund, senior market analyst at CNC Software Inc., developer of Mastercam, says that when it comes to the high speed and high feed machining strategies, increasingly common among mouldmakers, only an upscale programming solution will do.
“For example, we offer programming functions that are specific to the geometries found on newly emerging cutters, where you have these large sculpted surfaces being machined with a specially shaped tool,” Mund says. “If done properly, you can achieve much better finishes in a far shorter time than is possible with a traditional ball end mill. For mouldmakers, it doesn’t get any better.”
Aside from these industry specific functions, Mastercam is well known for its Dynamic milling, which generates the radial chip thinning-inspired toolpaths that, as IMCO’s Avers points out, also have a place in mouldmaking. When used with a high performance cutting tool, Dynamic milling can remove large amounts of material very quickly. “Fewer cutting tools are needed, it’s easier on your machine, and the parts come off in less time,” says Mund. “That’s a pretty good machining wish list for a mouldmaker—or any machinist, for that matter.”
The third leg
We’ve discussed a few of the cutting tools used for mouldmaking and touched on some of the programming techniques, but where would the industry be without the top notch, highly capable CNC machine tools available today. Unfortunately, there’s no space left to discuss this third and very important leg of the mouldmaking stool. As an example, a company using fifteen Röders brand machining centres is achieving three dimensional form accuracy of five microns (0.0002 in.) on its mould cavities, many of which are machined from solid blocks of hardened tool steel. SMT