July 5, 2011
Heavy plate fabricators drill and mill plate to achieve tight tolerances. But these metal cutting tools exert significant forces on the workpiece vibration, particularly in large workpieces such as plate. When machining in general and especially in large plate, three major factors work together: cutting tool selection, milling strategy, and workpiece setup.
Machining large plate often can be a challenge, but if certain areas are controlled, the challenge is replaced with success. Heavy fabricators drill and mill such plate to attain high accuracy. But unlike oxyfuel or plasma cutting, drilling and milling exert significant forces that can cause workpiece vibration—especially in large plate. All this makes for inaccurately cut parts and poor tool life, which lead to higher production costs caused by lost machining time and broken tools or inserts.
When machining in general and especially in large plate, three major factors work together: cutting tool selection, milling strategy, and workpiece setup.
Many conventional cutting tools are made of carbide, others are high-speed steel (HSS). Compared to carbide, HSS is relatively soft, flexes, and withstands impacts, so it is a little more forgiving than carbide in less rigid setups. The tradeoff is that HSS offers relatively slow feeds and speeds and a shortened cutting-edge life overall.
Speeds, feeds, and productivity can be greatly increased with carbide tooling, but using such tools requires careful preparation. Carbide tools tend to chip or crack from excessive vibration, damaging the tool or at least dramatically shortening the tool’s life. This is almost always directly related to the three main areas previously mentioned: cutting tool selection, milling strategy, and workpiece setup.
Pay special attention to the cutter pitch. The mill cutter’s pitch refers to the number of inserts in a cutter. Cutters come in coarse, medium, and fine pitch, and which to use depends on how much material the cutter is designed to remove, both in depth of cut and feed per tooth (see Figure 1).
A coarse-pitch cutter removes more square inches of material while in the cut. It also allows maximum chip clearance. These cutters are best-suited for general-purpose milling in which adequate horsepower is available and maximum depth of cut is required. Generally, though, tools with fewer inserts also have limitations when it comes to feed per revolution, so the overall feed rate usually is lower.
A medium-pitch cutter has slightly more inserts and, because of the smaller space between inserts, less chip clearance. These cutters work best with a moderate depth of cut and feeds per tooth. More inserts also help maintain a high feed rate, as there are more inserts removing material per revolution.
A fine-pitch cutter has more inserts and even less chip clearance than a medium-pitch cutter. Such tools can maintain a high feed rate but experience high cutting forces because of the number of inserts engaged in the cut at one time. Large depths of cuts usually are more difficult, but the finish produced by each milling pass usually is much finer compared to that of a coarse-pitch mill.
Cutters with even pitches have inserts or flutes spaced evenly along the circumference, while those with differential or variable pitches have inserts or flutes that are spaced unequally around the circumference. In some applications, cutters with variable pitches can help overcome workpiece vibration. In short, this is related to the harmonics frequencies in the spindle and the workpiece; the variable pitch interrupts these harmonics, improving the milling operation greatly.
Also note the geometry and position of the cutter’s inserts—including the lead angle, or the position of the insert cutting edge in relation to the workpiece (see Figure 2). Some inserts have cutting edges positioned vertically. This occurs when using a tool with inserts having a 0-degree lead angle (see Figure 3). This means the programmed feed rate is equal to the actual chip thickness.
Now picture the same square insert but rotated 45 degrees (Figure 2). In a face milling operation (in which the workpiece surface is perpendicular to the spindle axis), this would mean only the corner and a portion of the insert’s edge would contact the workpiece.
Generally, as the lead angle increases, chip thickness decreases. Inserts are designed for specific chip loads. To maintain an average chip thickness (say, 0.008 inch) when using a face mill with inserts having a 45-degree lead angle, the feed would need to be increased to accommodate for chip thinning.
In certain circumstances the 0-degree insert may be appropriate, such as when machining a 90-degree shoulder with a square-shoulder cutter. But when face milling, try to use a milling cutter with inserts having a lead angle whenever possible.
The cutter rotation and milling direction determine how exactly those inserts contact the metal, which in turn affects the shape of the chip, the life of the cutting edge, the surface finish produced, and the efficiency of the operation. When milling with a CNC machine, make sure the inserts contact the metal so that they produce so-called “thick-to-thin” chips (see Figure 4). This means the insert engagement is at its greatest when it first contacts the metal, producing that thick chip at the cut entrance; as it rotates, the insert engagement reduces to produce a thin chip at the cut exit. This is called climb milling or down milling.
Consider the consequences of the reverse—a thin chip on insert entry and a thick chip on exit. If the insert enters the cut with only a small level of engagement, it actually rubs against the surface before actually cutting the material. That rubbing action causes friction, increases heat, increases the chance of work hardening, tends to pick up and recut chips, and may lead to vibration and other issues.
Whenever possible, try positioning the cutter so that about 70 to 80 percent of the tool diameter is engaged in the cut. This overlap allows the inserts to cut and evacuate that thick-to-thin chip. More insert engagement entering the cut avoids the rubbing action, while less insert engagement at the end avoids the shock of forcing a thick chip out the cut exit.
The shape of the toolpath also plays a role. Cutting tools are a bit like car engines; they last a long time when consistently engaged (think highway driving), but don’t last when that engagement is continually interrupted (city driving). Dramatic changes in cutter engagement—either by entering into a cut head-on or by turning at a hard angle within a cut—make for some serious city driving and, hence, poor tool life.
When entering a cut, you may reduce the feed to avoid that screech as the cutter slams into the workpiece. In plate milling, this can apply to starting from the edge of a hole, plate perimeter, or open profile in the plate interior. But reducing feed may cause other problems and possibly hinder productivity.
Alternatively, you can use a lead-in technique in which the cutter eases into the cut, following a curved toolpath (see Figure 5). Similar logic applies within the cut. Whenever possible, avoid sharp angles and instead program a toolpath with rounded turns, which helps keep the cutter consistently engaged and at a much steadier axial load.
Workpiece support is one of the key components of a successful machining operation. If the part is not set up properly, it limits the tool’s ability to machine optimally. As much thought and knowledge must go into a part setup as choosing the right tool and process.
Part support, fixturing, and clamping often are overlooked and said to be wasted time. But carbide tooling imposes huge forces during operation. There is no harm in oversupporting your parts. When cutting plate with carbide tooling, the more workpiece support, the better. Carbide is very hard but brittle, and when vibration occurs it can chip or crack. This will damage or drastically shorten the life of the tool. If you have a solid setup, you will be able to optimize the process and tooling, and produce accurate, consistent parts time after time.
Many heavy fabricators have experience with conventional machining, which is far more hands-on than CNC work. The traditional knee mill survives because it doesn’t make sense to tie up a CNC milling center for one or two parts that may not require extreme accuracy.
When conventional machining, you can react in the middle of an operation and adjust feeds and speeds to suit the situation. This is much more difficult with CNC machines, which is why knowing the fundamentals of good milling practice is so important.
For any CNC—be it a vertical or horizontal machining center or bridge-type machine that mills heavy plate—you must ensure the setup, tools, and process work together to produce an accurate part efficiently. Once an operation starts, there’s no turning back.
The FABRICATOR® is North America's leading magazine for the metal forming and fabricating industry. The magazine delivers the news, technical articles, and case histories that enable fabricators to do their jobs more efficiently. The FABRICATOR has served the industry since 1971. Print subscriptions are free to qualified persons in North America involved in metal forming and fabricating.