How fast should you drill?

Modern Machine Shop, June, 1990 by Ken Gettelman

The story is as old as creative selling. The salesman comes in with the exciting news that the new TiN (titanium nitride) coated twist drill, on a single sharpening, will produce an average of 128 quarter-inch holes a half inch deep in that tough 4340 steel at your accustomed drilling speed of 100 sfpm. Your old, uncoated high-speed steel drills produce somewhere around 23 holes under these conditions. The coated drills will deliver a beautiful 456 percent increase in tool life.

Or let's turn the conditions around. You have 100 holes in the job and you don't want to change drills during the run. With the standard twist drills, you had to cut the speed back to 64 sfpm. With the new coated drills you can jump the speed to 116 sfpm and still get your 100 holes. With this approach, the productivity increase is still an impressive 81 percent. The coated drills cost only 1 1/2 times the price of the uncoated variety. Any way you look at it, the figures are impressive. The salesman has scored his point and you make the switch.

Did you do wrong? Of course not. Your decision to switch was good. However, with a little additional information, you not only could improve productivity or tool life on a particular job, but you also could build a database that will help your shop develop the best manufacturing process plan for all the jobs going across your plant floor. While floor-to-floor time on any job is an important consideration, it is the door-to-door time that is the ultimate measure of competitiveness, productivity, and profitability. Good process planning is a key in arriving at the best door-to-door times, where the raw material comes in and the quality finished product goes out in the shortest possible time.

This is the point made by Dr. William Zdeblick, Director of Advanced Process Technology, Metcut Research Associates, Cincinnati, Ohio. Metcut has been developing specific machinability data for decades. Such data will give suggested feeds, speeds, and depths of cut for specific cutting tool and workpiece material combinations for machining operations including drilling, milling, turning, boring, sawing, and so on. Many numerical control programmers use this data bank as a starting point in choosing feeds and speeds in their development of part programs.

However, as Dr. Zdeblick points out, the thinking has matured over the years to the point where such data now can be used to help generate optimum process plans. Dr. Zdeblick uses drilling in an example demonstrating how such a plan can be developed. Speed And Tool Life

Around the turn of the century, Frederick W. Taylor demonstrated, with his famous formula T = [CV.sup.-n], that the greater the speed of machining, the shorter the tool life. The formula simply states that tool life, in terms of time (T), is equal to a constant (C) multiplied by the velocity (V) to an inverse exponent -n). The constant is based on the cutting tool and workpiece material combination. The velocity is the speed of machining based on either surface feet per minute or meters per minute. The -n exponent is the log slope of the line, which goes down as speed goes up.

The printout in Figure I is an example of tool life in relation to cutting speed. As the drilling speed goes up, the tool life quickly falls. If maximizing tool life was the only consideration, all holes would be drilled at the lowest possible speed.

The twist drill is not the only cost in drilling a hole. Direct labor, machine amortization, general administration and overhead, and similar costs must be considered. At the left-hand side of the graphs, where tool costs are low, the other costs are high because the output rate is low.

Thus, feeds and speeds of most machining operations traditionally have been selected to give the lowest total cost per unit of work. These selections have been made in an attempt to compromise the right mix of cutting speeds with all the other costs that go into the equation. Only in this manner can a shop achieve the lowest machining cost. This process has been used for generations, and it has been formalized in precise mathematical equations for at least 25 years. Some shops use a computer to generate data that produces the optimum cutting speed.

For a computer to generate this data, the shop must have a good idea of the labor, overhead, amortization, and other indirect costs. If accurate and precise numbers go into the equations, sound machining practices can be achieved. If people use inaccurate data to figure their overhead or other costs, they will get inaccurate data about the optimum machining rates.

Figure 2 shows a typical set of curves for drilling. These curves combine the tool cost with the category of labor, machine, and overhead costs. The total cost is the sum of the two, and there is always a point on the combination curve where a given machining speed will provide the lowest cost for producing a drilled hole. Best Economics

World manufacturing competition has taught us that the true lowest cost of overall manufacturing may not be the same as the lowest cost of floor-to-floor machining time. Many shops today are looking toward JIT (just-in-time) production (organizing production in a kit form, complete with a set of tools, so that no tool changes take place on the job) synchronous manufacturing, WIP (work-in-process) reduction, and so on. The lowest overall cost per hole in the drilling operation may have to be revised to meet the other, more strategic goals. All the other machining operations may require these revisions as well.