CNC machining bottom cutting: how a tool actually reaches the floor

• 1
  What CNC machining bottom cutting actually removes
• 2
  Tool geometry limits in CNC machining bottom cutting
• 3
  How five-axis motion changes bottom cutting reach
• 4
  Symptom, cause and fix on a bottom face
• 5
  When a design should change instead of the toolpath
• 6
  What floor tolerance costs in practice
• 7
  Step by step: planning a floor cut
• 8
  Choosing a tool for a bottom face

Every pocket has a floor. Bottom cutting is the pass that creates that floor, feeding the end of the cutter sideways or in a spiral so the edges on the bottom of the tool sweep the material away. A slot drill cuts with its end teeth. A ball nose cutter leaves a scalloped floor that needs a second pass.

The floor is not free geometry. The tool has to sit at the bottom of the cavity with enough shank left above the part to clear the walls. Deep floors force long tools, and long tools deflect. On a 12 mm carbide end mill hanging 60 mm out of the holder, a 0.3 mm radial load can push the tip off line by several hundredths before the cut stabilizes.

Finish on the floor depends on feed per tooth and the corner radius of the tool. A square-corner cutter leaves a sharp internal corner that no rotating tool can copy exactly; the floor meets the wall with a radius equal to the tool corner. Draw the radius you want, or accept the one the tool leaves.

Flatness across a floor is a separate number from surface roughness. A floor can be Ra 0.8 μm and still dish 0.05 mm over 80 mm if the part springs or the fixture lifts. Check both on the drawing before the first cut. One without the other rarely holds in production.

• 1
  Floor flatnessControlled by rigidity and fixturing, not by spindle speed.
• 2
  Floor finishSet by feed per tooth, corner radius and tool runout.
• 3
  Internal cornerCannot be sharper than the cutter corner radius.

A cutter has three numbers that decide how deep a floor can go: diameter, flute length and overall reach. Flute length is the cutting portion. Reach is everything from the holder face to the tip. The gap between flute length and reach is dead shank, and it is where chatter starts.

Rough rule from the shop floor: a carbide end mill holds size when its reach is no more than three times its diameter for aluminum, and two times for stainless or titanium. Go past that and you are trading depth for taper and chatter. A 6 mm cutter at 18 mm reach is a normal job in 6061. At 30 mm reach it needs a stub pass and light depths.

Coating matters less than people expect at the bottom of a pocket. The failure mode is usually deflection or chip packing, not abrasion. Aluminum builds up on uncoated flutes; use polished or ZrN-coated tools and keep air blast on the floor. Stainless work-hardens, so keep the chip load up and never dwell at the bottom.

Ball nose cutters handle curved floors and fillets. Stepover decides the scallop height. For a 10 mm ball nose at 0.5 mm stepover in aluminum, scallops land near Ra 1.6 μm. Drop stepover to 0.2 mm and the same tool reaches Ra 0.8 μm in one direction. The trade is cycle time, roughly 2.5 times longer.

• 1
  AluminumReach up to 3× diameter; polished flutes, air blast.
• 2
  StainlessReach up to 2× diameter; high chip load, no dwell.
• 3
  TitaniumReach up to 2× diameter; flood coolant, reduce radial engagement.

Three-axis machines drive the tool straight down Z. The whole length of the tool has to fit inside the pocket walls. Tilt the tool and the geometry changes; the shank can clear the wall while the tip still reaches the floor corner. That is the main reason five-axis work exists for deep floors.

A 30-degree tilt on a 10 mm cutter effectively shortens the vertical reach needed by roughly 13 percent on the wall side. Small gain, but it is often the difference between a 3× diameter tool and a 2× diameter tool. Tilting also moves the cutting load off the tip and spreads it along the flute.

Tilt has limits. Past about 45 degrees, the bottom edge stops cutting and starts rubbing. Floor finish drops, heat climbs, and the tip wears on one side. For flat floors in aluminum, 15 to 30 degrees is the useful window. For contoured floors, the tool axis should stay near normal to the surface.

Contouring with a ball nose on a five-axis machine lets the tool lead or lag along the path. Leading by 10 to 20 degrees keeps the contact point off the tool tip, where surface speed is near zero. That single change often moves a floor from Ra 1.6 μm to Ra 0.8 μm without touching feed or speed.

• 1
  Tilt window15–30 degrees for flat floors in aluminum.
• 2
  Past 45 degreesBottom edge rubs instead of cutting.
• 3
  Tool lead angle10–20 degrees pulls contact off the tip.

Chatter marks across a floor, evenly spaced, mean the tool is vibrating at its natural frequency. Shorten the reach, reduce radial engagement, or change spindle speed by 10 percent. Adding a coating will not help. The vibration comes from the setup, not the cutting edge.

A floor that tapers from one wall to the other usually means the part moved. Thin floors deflect under clamp pressure and spring back after unclamping. Support the floor from underneath with a jack or a sacrificial pad, and rough with the clamps loosened to a light touch.

Burn marks or a discolored floor point to rubbing, not cutting. The tool is dull, the chip load is too low, or the bottom edge is tilted past its working angle. Raise feed per tooth, replace the tool, or reduce tilt. Do not slow the spindle down; that makes rubbing worse.

A floor that measures flat but fails on roughness has a different cause. Runout at the tool tip, a worn corner radius, or a stepover that is too wide. Measure runout at the tip with a dial indicator. Anything above 0.01 mm TIR will show on the floor finish.

• 1
  Even chatter marksToo much reach or radial load. Shorten the tool.
• 2
  Tapered floorPart deflection under clamping. Support the floor.
• 3
  Burn marksRubbing, not cutting. Raise chip load or change tool.
• 4
  Flat but roughTip runout or wide stepover. Check TIR first.

Some floors cannot be cut from above at any reasonable cost. A closed pocket with a 3 mm corner radius and a 40 mm depth in 17-4PH is one. The tool that fits the corner is too long to hold tolerance; the tool that holds tolerance cannot reach the corner. Redesign moves faster than heroics.

The cheapest fix is often a larger corner radius. Going from R3 to R5 raises the maximum tool diameter from Ø6 mm to Ø10 mm, which nearly doubles stiffness at the same reach. If the radius is not functional, open it up. Nobody pays extra for a sharp corner that does nothing.

A second option is to split the part. Machine the pocket floor on one half, then join. This adds a joint and a fixture, so it only pays when the floor has a real function such as a sealing face or a bearing seat.

The last option is electrical discharge machining for the corner after milling. It adds a setup and a separate process, but it reaches geometry that no rotating tool can touch. Use it for the corner only, not for the whole floor.

• 1
  Raise the corner radiusR3 to R5 nearly doubles tool stiffness.
• 2
  Split the partPays off for sealing faces and bearing seats.
• 3
  EDM the cornerReaches geometry milling cannot. Extra setup.

Bottom cutting tolerance is not one number. Depth of a floor, flatness of a floor, and position of a floor relative to a datum are three different measurements with three different cost curves. Ask for the one that matters and leave the others at general tolerance.

Depth is the easiest to hold. On a rigid setup we hold ±0.005 mm on floor depth in aluminum and steel. Flatness is harder because it depends on the part, not the machine; a thin floor will move no matter how good the spindle is.

Position matters when the floor carries a mating surface. If the floor sits 0.02 mm off from the bolt pattern, an assembly will rock. That is a fixture and probing problem, not a cutting problem, and it usually needs in-process measurement.

Finish and flatness interact. A floor ground to Ra 0.2–0.8 μm usually comes off a fine finishing pass with a small stepover. Push the same floor to Ra 0.4 μm across a 200 mm span and the cycle time climbs fast. Check whether the seal or bearing actually needs the finer number.

• 1
  Depth±0.005 mm is routine on a rigid setup.
• 2
  FlatnessSet by part stiffness, not spindle accuracy.
• 3
  PositionNeeds probing or in-process measurement.