U Drill for Hole Processing: How It Cuts, and Where It Stops Working

• 1
  What makes a U drill for hole processing different
• 2
  How the U drill for hole processing removes material
• 3
  L/D ratio and diameter range as design limits
• 4
  What tolerance and finish to expect from a U drill for hole processing
• 5
  Running the U drill for hole processing on mill and lathe
• 6
  Symptoms that point back to the process, not the insert
• 7
  U drill vs twist drill vs helical milling vs solid carbide

A U drill is a drill body with two indexable inserts seated at the tip. One insert sits near the centerline and cuts from zero to roughly half the radius. The other sits on the outer edge and cuts the remaining material out to the full diameter. Neither insert overlaps the other's path much, so each one sees a different cutting speed as it travels around the hole.

That split is the whole idea. The center insert runs at low surface speed because it sits near the axis, so it is ground with a stronger edge and a different rake than the outer insert. The outer insert runs faster and takes the finished wall. Because the two inserts are separate, the drill body can be a simple steel shank with a coolant channel instead of a solid carbide twist drill.

Compared with a conventional twist drill, a U drill does not need a pilot hole in most cases. It plunges straight into solid material and produces a hole close enough to final size that a boring bar only has to clean up. That removes one operation from the routing, which is usually the reason it gets specified.

The trade-off is stiffness. A U drill body is hollow for coolant and cannot be necked down the way a solid carbide drill can, so the length-to-diameter ratio is limited. Push past that limit and the body deflects, the hole walks, and the outer insert chips.

A U drill does not shear material the way a twist drill does. It cuts with a negative or neutral rake at relatively high feed per revolution, which produces a short, broken chip instead of a long stringy one. Feed rates typically run two to four times higher than a comparable HSS twist drill, and the chip leaves the hole through the flute rather than wrapping around the body.

Chip evacuation is the real constraint. The hole is being cut at the same time the drill is trying to push chips back up the flute, and the deeper the hole, the longer that path. Coolant pressure does most of the work. A U drill generally wants through-coolant at 20–70 bar depending on diameter, delivered through the internal channel and aimed at the cutting edge.

Without enough pressure the chips recut. Recutting shows up as a rough wall, a rise in spindle load, and insert edge chipping on the outer corner. If you hear the load climbing on a hole you have drilled a hundred times before, stop the cycle and check the coolant filter before you blame the insert grade.

Heat leaves with the chip, so a U drill runs cooler than its cutting speed suggests. That is why the same body can cut aluminum at 200 m/min and 4140 at 120 m/min with only an insert change. The body does not care. The insert grade and coating do.

The standard U drill body is available in 3×D and 5×D lengths, with longer bodies made for specific jobs. The 3×D body is rigid and behaves well. The 5×D body is where most shops start seeing taper and drift, especially in stainless and titanium where cutting forces are higher and the material springs back against the body.

Diameter drives the coolant requirement more than any other variable. A Ø20 mm U drill needs less flow but more pressure to reach the cutting edge than a Ø50 mm body, because the internal channel is smaller. Below roughly Ø12 mm the coolant channel gets tight enough that pressure requirements climb sharply, and solid carbide becomes the better choice.

Above roughly Ø60 mm the insert loads get large, the body gets heavy, and a different strategy usually wins: drill undersize with a smaller U drill, then open the hole with a boring head or a helical milling path. Helical milling also lets you correct position error partway down, which a U drill cannot do.

As a rule, if the hole is deeper than 5×D, or if the diameter is outside Ø12–60 mm, look at the alternatives before you commit the process. A U drill used inside its window is fast and repeatable. Used outside it, it generates scrap quietly.

A U drill does not produce a precision bore. Diameter typically lands within IT9 to IT11, and the wall carries visible feed marks. On a Ø20 mm hole that is roughly ±0.05 mm on diameter, which is fine for a clearance hole or a tapped hole but not for a bearing seat or a dowel pin fit.

Position is better than diameter. Because the drill enters in one plunge with no pilot, the entry position tracks the toolpath closely. A rigid setup on a 5-axis machining center can hold position within a few hundredths of a millimeter, which is often tighter than the diameter tolerance.

Straightness depends on the L/D ratio and the material. At 3×D in aluminum, a U drill can hold straightness well enough that a reamer finishes the hole in one pass. At 5×D in 316 stainless, expect a slight drift and plan a boring pass to correct it.

If the print calls for ±0.005 mm on diameter or Ra 0.8 μm or better, plan the U drill as a roughing step and leave 0.2–0.5 mm on the wall for a boring bar or reamer. Trying to hit those numbers with the drill alone leads to rework, because insert wear changes the diameter over the run.

On a machining center, hold a U drill in a side-lock or hydraulic holder, not a collet chuck. The drill needs to resist torque and side load, and a collet can slip under a heavy feed. Keep the holder as short as the work allows. Every millimeter of overhang adds deflection at the cutting edge.

Rigid tapping and spot drilling are not needed for most U drill work. Skip the spot if the surface is flat and the tool is on center. A spot drill can actually cause the U drill to rub at entry if the spot is smaller than the drill's center insert, which dulls the inner insert before the hole is a millimeter deep.

On a lathe, the U drill mounts in the turret and cuts on center. Alignment matters more here than on a mill, because a drill running off center will cut on one insert more than the other and wear them unevenly. Check center height whenever you change holders.

Peck drilling usually hurts more than it helps with a U drill. Each retract lets the chips settle back into the hole, and the re-entry shock loads the outer corner. If you need to clear chips, use a shorter body or raise the coolant pressure instead of pecking.

An outer insert that chips at the corner usually means the drill is deflecting at entry, not that the insert grade is wrong. Check holder runout and overhang before you switch grades. Runout over about 0.02 mm at the drill tip will wear one insert faster than the other every time.

A hole that comes out oversize by more than 0.1 mm usually points to the same deflection, or to a feed rate that is too low. Running a U drill too slowly lets it rub instead of cut, which pushes the body off center and opens the hole. Increase feed before you increase speed.

A chirping or squealing sound at the bottom of the hole is often the drill hitting a cross hole or an interrupted cut. Reduce feed through that zone. A U drill does not like interrupted cuts, and forcing it through is how you break a body.

Short insert life on the inner insert only usually means the coolant is not reaching the center. That insert sits in the hottest, most confined part of the cut. If the inner insert wears first, check that the coolant holes are clear and aimed, not just that the pump is running.