If you’re going to drill a hole, it stands to reason that you want the hole to be straight and accurate. There are many ways to accomplish this, but all involve getting the hole started properly.
The main obstacle standing between you and drilling a straight hole is drill walk—the amount the tool deflects from a straight path. Avoiding this usually involves starting a hole with the shortest drill possible followed by successively longer drills until the desired hole depth is attained.
The hole is started by “spotting” the workpiece, which involves making a dimple in the face of the part with a very stubby and rigid drill known as a spot drill. This dimple minimizes drill walk by capturing the point of the subsequent drill as it enters the cut.
To Spot or Not
Quite often, spotting is unnecessary. A solid-carbide drill usually doesn’t need to be spotted because it’s very rigid and resists walking. The same holds true for indexable carbide drills. In fact, spotting the workpiece before using this type of drill will usually cause the inserts to chip or break.
Another drill that typically needs no spotting is the screw-machine-length drill, also known as the stub-length drill. It is so short that spotting is unnecessary, assuming that the hole to be drilled is shallow and part tolerance permits.
One reason shops avoid spotting is because the process is time consuming. Assume that you have an order for 5,000 parts made of 303 stainless steel. Two 3/8″-dia. holes 1½” deep need to be drilled in each part. A solid-carbide drill would perform admirably in this situation, but you may have a tough time convincing your boss to spend $30 for one when you could buy a dozen HSS drills for the same price. This will force you to use a jobbers-length (medium-length) drill, which requires spotting.
Let’s also assume that the hole to be created requires a 0.050″x45° chamfer. You decide to use a 90° spot drill so you can chamfer the hole at the same time. This means you will need to spot to a programmed depth of 0.240″. You’ll need to position the spot drill 0.050″ or so away from the part, giving a total cutting distance of 0.290″ per hole.
At 800 rpm and 0.003 ipr, this equals 14.5 seconds of drilling time per part. The machine positioning time for each part averages two seconds. If you have three vises set up with two parts per vise, your tool-change time is 12 seconds. Twelve seconds divided by the six parts adds two seconds to the operation, meaning a total of 18.5 seconds is needed to spot each part.
Multiplying 18.5 seconds by 5,000 parts equals about 26 hours of machine time. At a shop rate of $75 per hour, the decision to save $30 by using a HSS jobber-length drill ends up costing the company over $1,900. And that figure doesn’t take into account maintenance costs, which tend to be higher for HSS tools than carbide ones.
This example clearly illustrates that, whenever possible, it’s best to eliminate spotting altogether. But sometimes it can’t be avoided.
For instance, spotting is necessary when using a jobbers-length or longer drill. But starting a hole with one of these tools is dangerous and leads to unpredictable hole quality. Long drills deflect when they make initial contact with a flat surface. If they deflect enough they break, which can send shrapnel in all directions. Another potential problem is that even if you manage to start a hole with a long drill, chances are good that the tool will not go in the intended direction.
Then there’s the matter of cumulative error. On a lathe equipped with a bar feeder, the operator often drills through the workpiece, past the point where the part is cut off, and into the next workpiece. If any drill walk occurred when machining the first workpiece, the negative effects will carry over to subsequent parts. The tool eventually will poke through the side of a part. A spot drill will straighten out any drill walk that occurred during the machining of earlier workpieces.
On any machine, drilling holes more than 2 or 3 diameters deep requires spotting if carbide drills are unavailable or impractical. For very deep holes, this means starting the hole with a spot drill followed by a screw-machine-length drill then progressively longer drills until the required depth is reached.
Center vs. Spot Drills
If you do need to spot a workpiece before drilling, you have just two choices: the center drill or the NC spotting drill.
Many shops choose center drills,which are also called combined drill/countersinks. Center drills are cheap, readily available and come in sizes from No. 00000 to No. 10. The 00000 has a 1/8″-dia. body and a drill point that’s only 0.010″ in diameter. (How do they make those things anyway?) The No. 10 is a big monster, boasting a 1″-dia. body and a 3/8″ drill point.
Center drills come in two shapes. The most common is the plain type, which drills a hole with a 60° countersink. The second is known as the bell type. It has a curve-shaped countersink. Center drills are roughly one-fifth the price of comparably sized NC spot drills, which may account for their popularity.
Despite their popularity, center drills are not designed for starting holes. Their purpose is to drill holes with 60° angles in the ends of parts. These holes are used to secure parts in the tailstock of a lathe or to mount a workpiece between centers for a grinding operation.
The center drill is inefficient. Its thick web puts a great deal of pressure on the tool. Pressure leads to heat, and heat leads to premature drill failure. The tip of the center drill is also prone to breaking, as anybody who has ever used one to drill stainless steel can attest.
The best tool for starting a hole is an NC spot drill, which is also referred to as a spotting/centering drill. NC spot drills come in several styles, but they all share similar characteristics. All are short and rigid and can handle much higher feed rates than comparably sized center drills.
Unlike a conventional drill, an NC spot drill has zero back taper and no clearance behind its drill lip. Spot drills are made of HSS or carbide, but it is difficult to attain surface speeds high enough for carbide to work properly.
The web on a spot drill is very thin, giving it a chisel point with an efficient cutting action. Spot drills come in fractional and metric sizes and are offered with 90°, 118° and 120° points. The most popular points are 90° and 120°.
The point angle of the spot drill plays an important role in hole accuracy. A spot drill with a 90° point is convenient because most holes require a 45° chamfer, which means you can spot and chamfer simultaneously. However, this point angle may not be the best choice.
Jobbers-length drills usually have a 118° point. Using a spot drill with a 90° point causes the 118° jobbers drill to initially contact the workpiece at its outer margins (Figure 1a). If the jobbers drill is not sharpened perfectly, one of it flutes will touch the workpiece first. The drill will deflect away from this flute and could eventually begin to walk. This improper contact can also cause the drill to flutter back and forth slightly until it is fully engaged in the workpiece. Fluttering may cause chipping of the drill point when cutting extremely hard or tough materials.
It’s usually better to spot the workpiece with a drill that has a 120° point. Since a spot drill has a thin web, using one with a wider angle will force the 118° jobbers drill to make contact at the outer part of its chisel edge (Figure 1b). This will minimize the chance of an inaccurate hole being drilled. Additionally, choosing a spot drill with a 120° point instead of a 90° point allows you to drill a shallower hole and attain a given diameter more quickly.
Figure 1: Spotting with a drill that has a 90° point can cause the flutes of the 118° jobbers-length drill to contact the workpiece (left). This can lead to drill walk. When using a 118° jobbers drill, it’s best to spot with a 120° drill.
Hitting the Spot
On machining centers with Fanuc or Fanuc-compatible controls, spotting operations are usually programmed with the G81 command.
Sometimes it is desirable to allow the spot drill to dwell slightly at the final depth. This allows it to leave a clean surface for secondary drills. To do this you must use a G82 command.
It is important to mount spot drills correctly. Since they’re used at the beginning of the drilling process, any inaccuracies introduced here will negatively impact subsequent operations.
Spotting drills—indeed all drills—are best held by a clean, well-maintained collet chuck whose size is as near the tool’s diameter as possible. The use of a backing screw is recommended to prevent the tool from pushing back in the collet and to simplify tool replacement.
An endmill holder should never hold a spot drill. If you must use an endmill holder, grind a small flat on the shank of the tool. The set screw on the toolholder should be tightened against this flat to prevent the drill from spinning.
Following these procedures—along with choosing the correct NC spot drill—will help ensure the success of your spotting operations.
Read the rest: https://www.ctemag.com/news/articles/get-it-straight