Much high speed machining is done on conventional machining centers. It's more about how you cut than what you cut with. If you need higher speed performance from your existing machines, here are some things you can do.
The high speed machining question for many shops is not whether to get started but how to get started- without blindly investing in very expensive equipment and experimenting in totally new processes. Is there an incremental approach?
There are ways to better utilize a shop's existing stable of machine tools in order to increase machining speeds and begin to take advantage of the benefits of high speed machining. Some involve how you process work, which means a change in your metalcutting approach.
Other steps involve your machine, including its spindle, cutting tools, servo system, CNC and CAM package. Here, smaller improvements to components can add up to very significant performance increases.
Here are some incremental improvements that can help your shop do higher speed machining using your current tools. We'll also look at some auxiliary equipment that can help you get older machines cutting faster.
Try It - You'll Like It
High speed machining (specifically milling) is not very different from conventional milling. It involves all the same process components as conventional machining- feeds, speeds, depths of cut, cutting tools, and programs. The difference is in the application of these components.
In high speed machining practice, you're basically replacing a few slower, heavy cuts with more, faster, lighter cuts. The goal for each cutting method is identical- produce an accurate workpiece.
It may seem counter-intuitive that lots of shallow passes can result in faster machining than a few heavy cuts. Actually, the metal removal rates, cubic inches per minute, are higher using high speed milling techniques. Shops need to get used to the high pitch whine of a high speed cut-ter as it makes lots of little chips instead of the low rumble of a hogging cut making lots of big chips.
To get started, Ron Field, an application engineer at Makino (Mason, Ohio), suggests experimenting a little. Take some trial cuts in tool steel at 1200 sfm, and then adjust the process parameters up or down depending on your results.
For example, instead of driving a 2-inch end mill at 500 to 600 sfm, try running it up to 1200 sfm to see what happens. With the increased feed and speed, you should have about the same chip load. If your machine doesn't have the rpm capability, adjust downward- start at 1,000 sfm.
A fixed, center spindle delivers spindle speeds from 15,000 to 50,000 rpm. It is held by the machining center spindle so programming adjustments are minimal, requiring only a Z-axis offset.
In general, 8,000 rpm is considered a minimum ante for the rotational aspect of high speed machining. That's not to say some high speed machining benefits can't be derived at slower speeds. But, very basic equipment will limit the incremental improvements that can be made.
If your machine is on the spindle speed cusp, or just too slow, auxiliary spindles may be your ticket to high rotational speed. These come in different configurations and can give a machining center spindle high speed capability.
Many shops looking at high speed applications to go along with their general purpose work would prefer to hedge their bets when it comes to committing to a high speed-only spindle on a machining center. According to spindle maker Precise Corporation (Racine, Wisconsin), the spindle diameter and bearing requirements for lower rpm machining are opposite the requirements for high speed spindles.
For a reasonable amount of money, installing an auxiliary high speed spindle on an existing machine might be an answer. The idea here is to keep the original machine tool spindle and simply bolt-on high rpm capacity.
One secondary spindle option is a fixed center line spindle. Speeds for these units go up to 50,000 rpm, and up to 17 hp is available on some models. The unit mounts in the machine tool spindle but has its own power source and control.
Because it operates off the same center line as the main spindle, programming is transferable with only the need to adjust Z-axis depths to compensate for the addition of the unit in the main spindle.
An auxiliary spindle can be mounted to the side of the main spindle, which allows the shop to switch between the two as needed. Auxiliary spindles are a less expensive "bolt on" way to boost the rpm capacity of existing machine tools.
Another spindle option is to mount an independently powered high speed spindle to the side of the main spindle. This auxiliary spindle setup allows the use of the main spindle for cutting with large diameter tools. Thus, the auxiliary spindle is ready to use small diameter tools to cut at high speed.
Auxiliary spindles can be used as part of a phase-in program for high speed machining. As the shop becomes proficient with high speed, it may choose to install a high speed spindle on the machining center main spindle and move the auxiliary spindle to another machine. As more applications are converted to high speed, the conversion process repeats from one machine to the next.
Add A Flute
Reducing the depth of cut and increasing feed rates is the core process change for high speed machining. The goal is to get more metal removed in less time.
One advantage of shallower depth of cut is that the cutter takes less power to get through the material. Chip load is created by feeding a rotating cutter into the workpiece. If your machine tool has limited speed, you may use the reduced depth of cut to your advantage. Using cutters with more teeth is a method to get increased higher speed machining with a limited rpm spindle. Calculating the chip load on a given cutter edge is simple:
The correlation is that four flutes permit twice the feed rate of two flutes at the same rpm. This does impose additional cutting forces that can impact available horsepower. This can be offset by the reduced depth of cut. It takes some balancing to get it working, but the potential increase in metal removal and throughput is worth the effort.
High speed impacts machining in ways other than the mechanical delivery of a cutter to a workpiece. A machine is a controlled device. Commands come from a flow of data that begins with the tool path generated in a CAM terminal.
In many shops, data flows from the CAM terminal to a program management buffer through a serial connection. This buffer is a direct numerical control (DNC) computer which stores programs for direct loading into a machine's CNC when a specific part program is called for.
However, for very long programs, chances are that resident memory in the machine's CNC is insufficient to hold all of the program. In these cases the DNC pulls double duty as a program drip feed unit. In some die mold applications, a million lines of code can be generated for one program.
Each step in this data flow represents a potential bottleneck for high speed machining. On the other hand, each step can also represent an opportunity to streamline the data flow and reap the benefits of faster throughput. There are some relatively simple things you can do.
Check Your CNC And DNC
Using arcs fit to a point-to-point tool path, data density can be reduced allowing the CNC to process the program more quickly. These arcs are set to a specified tolerance, fit end to end, and outputas circular interpolation commands to the CNC.
There are some simple tests to determine if your CNC and DNC have sufficient speed for the kinds of feeds you want to run at higher speeds. For your CNC, Todd Schuett, president of Creative Technology (Arlington Heights, Illinois), suggests you try this approach.
Load a dense data program into the memory of your CNC. Don't put the program through the DNC as this may not indicate what the CNC is really doing.
An example of the data density recommended for this test is a set of 1,000 points in a row 0.010 inch apart. This totals a 10-inch move. In a perfect system, this test run at 200 ipm should take just over 3 seconds to execute, including acceleration and deceleration at the beginning and end of the program.
This should give you a processing speed benchmark for your CNC. Likewise the DNC execution can be a bottleneck for data flow as well. Mr. Schuett suggests you test that unit for relative speed too.
For testing the DNC, use the same program as for the CNC, a 10-inch linear move in 0.010-inch point segments. The DNC program should not be much slower than the CNC. Otherwise, the DNC is a bottleneck.
These two computers, the CNC and DNC, need to support the processing rates that your high speed machining needs to have. A fast DNC is no good if the CNC can't process the data fast enough to keep up. The fastest method of program data transfer is using a direct feed from a network file server into the CNC. This allows a full flow of data with no bottleneck between the program storage device and the CNC.
In the beginning of NC, each block of data was executed in order, one at a time. Speeds were sufficiently slow that this was a workable arrangement, especially for drilling and 2D linear milling operations.
It was when the machine needed to execute a curve or contour that the need arose for seeing what kind of data was ahead in the program. Otherwise machine momentum would cause the cutter to overshoot or undershoot a programmed change in cutter direction, wreaking havoc on the workpiece.
That need lead to the development of look-ahead, which is requisite for high speed machining of any geometry except for linear, single-axis moves. If your CNC doesn't have a look-ahead feature, it needs to be upgraded for high speed machining.
More From Less
There are programming techniques to help shops condense data so that a CNC can process smaller blocks of information faster. In some cases, this may be just enough additional processing speed to keep an older control viable for higher speed machining.
One technique is to use circular interpolation to replace traditional, data-dense point-to-point contouring. The idea is to use a series of arcs rather than line segments to construct curving paths. Then the control executes those arcs using circular interpolation.
It's a 2D process, so cuts can occur only in one of the machine's primary axis zones (XY, XZ, YZ). According to Bill Elliot, whose company, Northwoods Designs (Antwerp, New York), markets a software product called NWD SuperCut, one arc can replace ten points or more, reducing the program density to a fraction of its original size, which increases block processing speed.
Speed- It's Relative
Relatively speaking, most shops are cutting faster today than they did ten years ago. Albert Einstein said it first and best, "All motion is relative."
From that perspective, incremental improvements in "rate" mean that a shop is machining at high speed relative to what it did previously. Increasing the feed rate of a ballnose end mill in tool steel from 12 to 24 ipm and spindle speed from 4,000 to 8,000 rpm is a 100 percent increase in cutting speed and well within the capability generally found on most CNC machining centers.
In spite of all the talk about cutting fast, high speed machining is not an end in itself. Rather it's a means to an end. Cutting faster is not very helpful if quality, surface finish, or tool life go to the wrong end of the spectrum.
We know that the benefits of HSM are real. Shops using high speed machining techniques see increases in machine tool productivity, delivery response, accuracy, and tool life.
But, there is no "book" on high speed machining. It's a process in progress and everyone involved in applying the technique is learning on the job. It can be done incrementally, and it's worth the effort.
Source : Gardner Publications