So much has been said and written about high speed machining in the past few years, you'd think everybody would know a lot about it by now. Unfortunately, too much of that information has been conflicting, or simply wrong. So if you're uncertain about whether this process is right for your shop, join the club. A lot of your peers are also currently trying to separate the fact from the fiction on high speed machining. Others are a little farther down the trail, having already made an investment in more capable machine tools, and now they'd just like to see the machines live up to their billing.
We can't say for certain whether any given die or mold shop should make the move to high speed machining -- only a shop's managers can make that call. What we can say, however, is that just about any shop can benefit from this process if they are willing rethink the way they go about machining cores and cavities, and commit themselves to changing the overall tool-making process to which they are accustomed.
Contrary to what you may have heard, executing high speed machining is not all that difficult, it's just different. You're still dealing with all the same components of the machining process -- feeds, speeds, depths of cut, tools and toolholders, part programs and so on -- but the strategies of how to apply them change. To make that transition a little easier, here are some thoughts about the process, and some common-sense suggestions on how to make it work.
What's It For?
What's so different about high speed machining? In the simplest terms, not all that much. You're replacing a process of fewer, slower, heavier cuts with a process of more, faster, lighter cuts. The sound and feel of the cut are different. That familiar low rumble of a hogging cut gives way to the high pitched buzz of a smaller tool flying back and forth (or other ways) across the surface of the workpiece. The chips, though narrower, are similar, but they come a whole lot faster.
There a number of benefits to this methodology. Even though the cuts are considerably lighter, average metal removal rates are generally higher overall. But a more important benefit comes after the machining. Smaller cuts taken closer together and at higher speed result in an inherently smoother and more accurate surface. Benchwork -- from cusp grinding, to polishing, to spotting -- is drastically reduced, and sometimes eliminated outright. Indeed, for molds of average complexity, we typically see total tool-building cycle time reductions of 30 percent or more.
It also becomes practical to machine smaller tools entirely from hardened stock -- as hard as 72 Rc. Taking the heat treating process "off-line" in this manner can cut days from the time it takes to make a die or mold.
By our measure, truly high speed machining begins at about 1200 surface feet per minute (sfm), which is going to require a minimum of 8,000 rpm from the spindle. That's not to say, however, that some measure of the benefits of high speed machining can't be achieved on more modestly appointed equipment. In fact, we see very few existing machining processes that can't be speeded up. But with basic equipment, you will be rather limited as to how much you can achieve.
A good test of a machine is to take some trial cuts at 1200 sfm, and then adjust the process up or down, depending on the results. For example, instead of driving a 2-inch end mill at 500 to 600 sfm, try to run it up to 1200 sfm, and see what happens. You should have about the same chip load, but significantlylower horsepower consumption. If the machine doesn't have the rpm capability, you obviously have to adjust downward from the outset, but you get the point.
You'll have to get used to the idea that a smaller tool is going to do more work in the same amount of time, and that includes both roughing and finishing. Many times it is more efficient to rough with a smaller tool to get closer to net shape, and then proceed directly to the finish process. Most people would think this inefficient, but considering that roughing and finishing can both be done at high feed rates, and on the same machine in a single setup, the efficiencies start adding up. So, that 6-inch slab mill you used to rough with will give way to a 2-inch face mill running much faster and removing more material.
Most speeds and feeds charts that tooling manufacturers publish are conservative, designed to work on just about any machine. And if your machine tool is near the bottom of the capability curve, it's best to stay within those recommendations. But if you have a more capable machine, you likely will find yourself pushing the published limits. Never go beyond the maximum recommended rpm for a tool, as that's an important safety measure. Surface footage is a different matter, however, and many of the better tools are capable of moving beyond what is published in their sfm charts. Many tooling manufacturers also publish recommended surface speeds for cutting wood, and those numbers are sometimes quite appropriate for high speed metal cutting. That's no joke -- try it.
Depending on the hardness of the material, the tooling that is required to properly cut metals in a high speed environment is not much different than the tooling needed for traditional machining. Cermet or TiCN coated insert tooling, or solid carbide with TiN or TiCN coatings, are best at higher surface speeds for steels under 40 Rc. When materials get harder, solid carbide with TiAlN coating, or CBN, are the tools of choice.
A particularly good benefit of this process is that the type of material is not necessarily a limiting factor. For example, P-20 steel in its normal state of 28 to 32 Rc can be roughed or finished quite well with either Cermet or TiCN coated inserts. And some materials that are really difficult to machine, such as D2 steel hardened to 50 Rc, actually machine better at high speeds than with conventional techniques.
When cutting the harder materials, through-spindle liquid or air must be used to dissipate the intense heat created and to maintain an adequate temperature at the cutting edge as well as to ensure proper chip evacuation. For materials that are under 40 Rc, flood coolant is sufficient.
A Little Balance
Toolholders that worked fine at 3,000 rpm probably won't get the job done at 8,000. So when considering toolholder choices it is very important to make sure the holder is sufficiently balanced for the speeds at which your spindle will be turning. Rather than the simple maximum speed rating for a toolholder, look for the "G2.5" specification, which deals with both balance and speed. Anything less can result in excessive vibration, which in turn can lead to tool runout problems that can have a devastating impact on tool life, as well as surface finish and accuracy. Longer term, it will diminish spindle life as well.
For all of these reasons, most sidelock tooling grows increasingly precarious as spindle speed increases. The best toolholder of all is a shrink fit; the tool will always bottom and the balance is as near to perfect as it can be. But that will require some special equipment and more time on the front end to prepare tooling for a job.
A more practical choice for many shops is a hydraulic tool-holding chuck, which centers the tool extremely well, and is much more versatile in the sense that tools can be changed easily. A hydraulic chuck does suffer some loss in grip force in comparison to conventional toolholders, but that loss is not much of a factor in high speed machining, and the gains in reduced runout and vibration are substantial.
In any case, you're going to pay more for balanced or balanceable toolholders, but the benefits in surface quality and tool life are more than worth the price.
Don't Sweat The Programming
One of the misconceptions that most shops have about high speed machining is that the programming is more difficult than with conventional machining. Not true. The programmer only has to utilize the features that many 3D CAM systems have as standard packages. Most programmers are already using the techniques in one form or another. Constant Z-level machining, for example, has already proven to be one of the best ways to generate a high quality surface.
For roughing, programming a smaller depth of cut with a faster feed rate, and using positive rake cutters, will help in the machining process. This method is not only better for tool life, it also puts less heat stress into the metal and helps to bring the part closer to the final shape. Often by roughing in this manner, the semi-finish pass may be eliminated, saving more machine time and tool wear.
Finishing may be done by using Z-level machining or raster cutting (that is, to climb cut, pick over, then conventional cut). While raster cutting is faster, Z-level machining will produce a better surface finish because each successive pass is cut in precisely the same way and the profile of cutter contact is much more consistent from pass to pass. On most parts, both techniques are used to optimize the machining process.
When the machine tool is able to travel faster and more accurately, a much finer surface finish can and should be achieved. The movement per block can be much shorter to obtain the best dimensional accuracy. Cusp heights should be programmed as low as 0.00005 inch (yes, that's 50 millionths) and chordal tolerances (the maximum allowable distance the tool path can deviate from the base geometry) should be set under 0.0005 inch and possibly as low as 0.00005 inch. Note, however, that these kinds of tolerances will substantially increase the size of the NC program by laying in many more cutter passes (due to reduced stepover distances) and many more point-to-point moves. This will require high speed capabilities for both transmitting the part program from your CAM system or file server to the machine tool and for processing the program in the CNC. (Both are discussed below.)
There's a lot of talk these days about how to manage tool deflection. Many people are beginning to recognize the need to keep cutting conditions as constant as possible so the tool is seeing minimal variance in cutting forces as it traverses the part. (This technique pays dividends in surface finish as well.) The idea is that if the tool deflects, at least it will deflect consistently, which in theory offsets the negative effects.
But you should realize that completely maintaining constant cutting conditions is next to impossible with today's technology. A better approach for now is to manage feed, speed and depth of cut so that the tool is far less inclined to deflect to begin with. There are limits to the depth of cut per diameter of tool for various materials that, if observed, should head off trouble with deflection.
Fast In The Curves
If you hope to cut accurate contoured surfaces at high feed rates, you must have a powerful control. And for many machine tools, the CNC will prove to be the limiting factor on feed rates. If the feed is proceeding in fits and starts, that's probably because the control is not capable of processing the blocks of the program fast enough to keep up with the feed rate. In that case, you'll have little choice but to slow the feed or to program with a larger chordal tolerance so the points in the part program are not so close together.
If the tool is consistently gouging the part, that's an indication that the machine axes are over-shooting the commanded path. Here, about all you can do is slow down.
Newer high performance controls have the block processing speed to handle just about any cutter path you can program. Moreover, they also have a feature called look-ahead that that scans ahead in the NC program, searching for abrupt changes in tool path direction, and then automatically adjusts the feed rate, allowing the servos enough time to accelerate or decelerate to stay on path. This allows the straight-aways and gentle curves to be cut at the maximum feed rate, and to only slow down where the tight curvatures demand it. Without look-ahead, practically speaking, you'll have to set the feed for the worst case tool path geometry (if accuracy matters). In typical mold work, that's going to limit the feed to a maximum of somewhere between 40 to 80 ipm.
You'll also have to worry about how fast the program can get into the control.
If you are drip feeding the program via a DNC link, the speed of transmission may also be too slow to keep up with the feed. That may be due to an insufficient baud rate in the DNC system, or in the CNC's limited ability to process the incoming data.
The ideal situation is to have a network card in the control, and a hard drive with a direct link to the high speed bus. That way transmission speed from a file server down to the CNC is incredibly quick, the entire program will be able to fit on the hard drive, and the speed at which the program data is made available to the tool path processor is not ever a limiting factor. Short of that, you'll have little choice to work with a DNC system, so make sure it's fast. For die and mold machining, the baud rate should exceed 38,400 KB. We've worked with DNC systems with published baud rates as high as 76,800, and have gone as high as 115,000 on some machines with conventional DNC. However, remember that just because your DNC system can deliver data at high speed, doesn't mean your CNC can accept it that fast. So, you'll have to adjust your expectations for data transmission speed to the slowest component in the system.
The Big Picture
When it comes right down to it, what's required more than anything to achieve success in high speed machining is a change in attitude. You have to think differently about how a cut is supposed to look and feel, and you have to be committed to moving away from the old tried and true methods.
Sooner or later, everyone will recognize that high speed machining of dies and molds has arrived, and it's here to stay. It's a practical option that should be investigated by shops of all sizes. The advantages in lead time, accuracy and surface quality are exciting to say the least. With the proper machine tool and transfer of technology, the benefits of high speed machining can be yours.blog comments powered by Disqus