U-Farling Tools for Holes: How Indexable Insert Drills Cut
U-Farling tools for holes use two indexable inserts, one central and one peripheral, instead of a ground solid tip. This page explains how the cutting edges share the load, which hole sizes and materials suit them, and when a solid carbide drill is still the better call.
What U-Farling Tools for Holes Actually Are
A U-Farling drill, often shortened to U drill, is a replaceable-tip drill. Two indexable carbide inserts sit in the drill head: an inner insert that reaches the centerline and an outer insert that cuts the full diameter. The body is a short steel shank with two helical or straight flutes. There is no brazed tip and no regrinding.
The geometry is what gives U-Farling tools for holes their name in shop talk. The outer insert leaves a characteristic cone or U-shaped bottom when a through hole is not finished through. On a blind hole you see a small center pip plus a conical seat. If your drawing calls for a flat bottom, this drill does not produce it in one pass.
Because both inserts are clamped, not welded, the effective cutting diameter is set by the insert position, not by a hand-ground edge. Change the insert, and the diameter returns to nominal without touching the body. That is the whole economic argument for the tool.
Body length is short by design. A typical 2:1 to 3:1 length-to-diameter ratio keeps deflection low, which is why U-Farling tools for holes hold size better than a long twist drill at the same feed. Longer versions exist up to roughly 5:1, and they trade that stiffness away.
How the Two Inserts Share the Cut
The inner insert cuts from the center out to about one third of the radius. Its cutting speed is low near the axis, so it runs on a tougher grade and a stronger edge geometry. The outer insert cuts the remaining two thirds at the full surface speed, so it carries a sharper, more wear-resistant grade.
This split is the reason U-Farling tools for holes survive higher surface speeds than a comparable HSS drill. Each insert only sees the speed range it was designed for. On a Ø30 mm hole at 200 m/min the outer edge is moving fast while the inner edge is still in a comfortable range.
Chip formation differs at each edge too. The inner insert produces a short, thick chip that breaks easily. The outer insert makes a longer, thinner chip that needs enough feed per revolution to break cleanly. Feed too light and the outer chip strings out and wraps the body.
Both inserts cut simultaneously, so the axial thrust is balanced on the drill axis. That balance is why the tool does not walk on entry the way a poorly sharpened two-flute twist drill can.
When U-Farling Tools for Holes Beat Solid Carbide
Pick a U drill when the hole is large and the batch is not. A Ø40 mm hole in 4140 steel is slow work for a solid carbide drill, and the drill itself is expensive. A U-Farling body in that size costs a fraction, and you replace only the inserts.
Pick it when the material changes often. One body covers aluminium, 304 stainless, 4130 and cast iron as long as you match the insert grade and geometry. Solid carbide drills are bought for a narrower window and do not move between material families well.
Pick it when the machine has enough thrust but not enough spindle speed. U-Farling tools for holes run well at moderate rpm and high feed per revolution. On an older 3-axis mill with 6,000 rpm available, that combination is easier to hit than the high rpm a small solid drill wants.
Pick it when you need a shallow, accurate start. The short body resists bending, so hole position stays close to nominal on entry. That matters on a part where the hole is a dowel or bearing seat and the entry point is the datum.
Where the Tool Stops Being the Right Choice
Small holes below about Ø12 mm are not its territory. Insert geometry needs room for two clamping pockets, and below that size the body walls get too thin to carry the torque. Use solid carbide down there.
Thin-wall and deep holes also fight the tool. Past roughly 4:1 depth-to-diameter the body flexes, hole straightness drifts, and chip evacuation gets unreliable. A gun drill or a solid carbide drill with through-coolant is a better fit.
A flat-bottomed blind hole is a poor match. The insert leaves a cone and a center pip, so you either add a flat-bottom end mill to clean it or choose a different drill. On a hydraulic manifold with a sealing seat at the bottom, that extra operation kills the cycle time advantage.
Finally, U-Farling tools for holes need a rigid setup. If the part rings or the vise is loose, the outer insert chips on entry. Fix the workholding before you blame the insert grade.
U-Farling Drill vs Solid Carbide Drill
Same hole size, same machine, different trade-offs
| Factor | U-Farling drill | Solid carbide drill |
|---|---|---|
| Typical diameter | Ø12–60 mm | Ø1–20 mm |
| Cost of a worn edge | Insert swap, low cost | Regrind or replace the drill |
| Material changeover | Same body, new insert grade | Dedicated drill per material |
| Hole size control | Set by insert seat, repeatable | Set by grind quality |
| Bottom of blind hole | Cone plus center pip | Flatter, closer to flat |
| Rigidity at depth | Good to about 4:1 | Good to 8:1 and beyond |
| Best batch size | One-off to mid volume | Mid to high volume |
| Chip control | Needs firm feed per rev | Tolerant of light feed |
Which One to Put in the Spindle
For a Ø20 mm or larger hole in mixed materials and short runs, use U-Farling tools for holes and keep the inserts on the shelf. For holes under Ø12 mm, deep holes past 4:1, or a flat-bottom seat, use solid carbide and accept the higher tool cost.
Common Questions on U-Farling Drilling
What coolant pressure does a U-Farling drill need?
Through-coolant at 20–40 bar is typical for holes deeper than 2:1. The coolant clears chips from the inner insert, which is the pocket most likely to pack.
Below 2:1 depth you can get away with flood coolant on aluminium and cast iron, but steel still wants through-spindle delivery.
How do I know an insert is worn?
Watch the outer insert corner first. A small flank wear land, roughly 0.2–0.3 mm, is the normal end of life.
Hole size drifting up is the other signal. If the diameter grows past your tolerance band, the corner is rounded and the tool is pushing rather than cutting.
Can I drill stainless or titanium with the same body?
The body is fine. The insert grade and geometry are not. 304 and 316 work-harden, so a light feed skates on the surface and dulls the corner fast. Keep the feed firm per revolution.
TC4 (Ti-6Al-4V) runs hot and needs lower surface speed plus high-pressure coolant. Expect shorter insert life than on 4140.
Why does the drill squeal on entry?
Squeal usually means the outer insert is rubbing instead of cutting, often from too low a feed per revolution or a slightly off-center start.
Check the feed first, then verify the part is clamped flat. A shim under one corner is enough to change entry angle and set up a vibration.
Does the drill need a pilot hole?
No. The inner insert cuts to the centerline, so the tool can start on a solid face.
A pilot is only useful on cast or forged surfaces with scale, where a spot face gives the inserts a clean entry.
What tolerance can I hold straight off the drill?
On a rigid setup, expect roughly IT9 to IT10 for diameter and 0.05–0.10 mm for position.
If the hole is a bearing seat or a dowel fit, plan a reaming or boring pass. Drilling is the roughing operation, not the finish.
Send Us the Hole and We Will Pick the Tool
Upload your drawing and we return a quote plus a free DFM note on hole size, depth and tolerance within 12 hours.
12-hour quote±0.005 mm tolerance100% inspection
More CNC Machining Notes
We publish setup notes, tooling trials and inspection data from the factory floor.
