Basic Knowledge of CNC Router Processing

• 1
  What Basic Knowledge of CNC Router Processing Actually Covers
• 2
  Spindle, Gantry, and Bed: Where the Accuracy Comes From
• 3
  Tool Geometry Changes What a Router Can Hold
• 4
  Feed, Speed, and Depth of Cut on a Router
• 5
  Which Materials Belong on a Router
• 6
  Router vs. Machining Center: Which Fits the Part

A CNC router holds the workpiece on a fixed bed and moves a spinning cutter over it on a gantry. That one sentence separates routing from milling. On a machining center the tool stays roughly in place and the table carries the part into it. On a router the part sits still and the gantry carries the spindle. The distinction sounds academic until you look at accuracy.

The moving mass on a router is large. A gantry spanning 2 m or more has to accelerate and stop thousands of times per program. Inertia limits how fast the machine can reverse direction without ringing. That is why router positioning tolerance is usually stated in tenths of a millimeter, not microns, and why deep pockets with tight corner radii are a poor fit.

What routers do well is cover area. A 4,000 mm bed with a 24,000 rpm spindle can profile a full sheet of 18 mm plywood, trim a composite panel, or cut a batch of acrylic faces in a single setup. The value is in throughput and work envelope, not in holding ±0.005 mm.

The rest of this page walks through spindle types, gantry geometry, tooling, and the cut parameters that decide whether a router job succeeds. Read it before you commit a drawing to routing.

The spindle is the first thing to check. Router spindles run 18,000 to 24,000 rpm and use ER collets or HSK holders. High rpm suits small-diameter tools and soft material. A 6 mm cutter at 20,000 rpm gives a sane surface speed in aluminum and MDF alike. Drop the rpm and the same cutter rubs instead of cutting.

Spindle power matters more than rpm for hard material. A 3 kW spindle can take a 6 mm depth of cut in plywood at a healthy feed. Push the same tool into 6061 aluminum at that depth and the spindle stalls or the tool snaps. Aluminum on a router works best with light radial engagement, high feed, and good chip evacuation.

The gantry carries the Z axis and spindle across the X travel. A dual-drive gantry with a servo on each side resists racking better than a single screw, which matters when you cut near the table edges. Ball screws or helical racks set backlash. Any backlash shows up as chatter on climb-cut walls.

The bed is usually a vacuum table, a T-slot extrusion, or a sacrificial MDF spoilboard. Vacuum holds flat sheet well. It does not hold a 200 mm tall block, and it will not resist side load from a large face mill. If the part needs strong clamping in Z, it may not belong on a router.

• 1
  Spindle speed18,000–24,000 rpm suits small cutters in wood, plastic, and light aluminum work.
• 2
  Gantry driveDual servo drive on both sides cuts racking and keeps corners square.
• 3
  WorkholdingVacuum is fast for sheet; T-slot or fixtures are needed for thick stock.

Router tooling falls into three families: upcut and downcut spirals, compression bits, and straight or V-groove tools. An upcut spiral lifts chips out of the kerf and gives the cleanest edge on the bottom face. A downcut pushes chips down and protects the top veneer, which is why it is used on laminated panels. A compression bit combines both and produces clean edges on both faces in one pass.

Tool diameter sets the minimum internal radius. A 6 mm cutter leaves a 3 mm corner radius at best. If the drawing calls for a 0.5 mm radius, the router will need a 1 mm cutter, which then limits depth of cut and feed. That is a real constraint, not a preference. Design for the tool you can actually run.

Coating choice follows the material. Solid carbide works for wood, MDF, and most plastics. Diamond coating is the right call for fiberglass, carbon fiber, and other abrasive composites, where an uncoated tool dulls in minutes. For aluminum, a polished or ZrN-coated cutter with a high helix clears chips and reduces built-up edge.

Tool length is the hidden variable. A long tool reaches deep pockets but deflects. Deflection shows up as taper on the wall and a poor finish at the bottom of a pocket. Keep the gauge length as short as the part allows and take the depth in two or three passes instead of one.

Chip load is the number that ties feed and speed together. It is the thickness of material each cutting edge removes per revolution. Too low and the tool rubs, heats, and dulls. Too high and the tool breaks or the gantry loses position. For a 6 mm two-flute carbide cutter in MDF at 18,000 rpm, a feed around 4,000 to 6,000 mm/min gives a workable chip load.

Aluminum behaves differently. The same 6 mm cutter in 6061 wants a lower surface speed and a shallower radial engagement. A common starting point is 12,000 rpm, 1,500 to 2,500 mm/min, and a 0.5 mm radial stepover with a 3 mm axial depth. Mist coolant or an air blast keeps chips from re-cutting, which is the usual cause of a rough finish.

Depth of cut should be taken in passes. A full-depth cut in hardwood or acrylic loads the tool and the gantry at once. Two or three passes at a third of the total depth each hold size better and leave a cleaner wall. The time penalty is small compared with scrapping a part.

Ramp or helical entry beats straight plunge. Plunging a flat-bottom cutter into the material spikes the load and can push the gantry off position. A 3° to 5° ramp spreads the entry load and keeps the tool on the programmed path. On hard plastics, a helical entry into a pocket is even gentler.

• 1
  Chip load firstSet feed from chip load, then adjust rpm to match the material.
• 2
  Multiple passesTwo or three passes hold size better than one deep cut.
• 3
  Ramp inA 3°–5° ramp avoids the load spike of a straight plunge.

Wood and wood composites are the native material. MDF, plywood, hardwood, and particle board all cut cleanly at high rpm. Sheet goods are the sweet spot because the vacuum bed holds them flat and the gantry can run the full sheet without repositioning.

Plastics route well with the right tool and chip clearance. ABS, PC, PMMA, POM, and HDPE all machine on a router. Acrylic is prone to melting and cracking if the feed is too low or the tool is dull. POM cuts cleanly but needs sharp tools because it grabs. Keep the rpm moderate and the feed high enough to throw chips clear.

Aluminum is possible but limited. Thin plate, brackets, and panel work are fine. Deep pockets, tight tolerances, and thick sections are not. If the part needs ±0.005 mm or a mirror finish, a machining center with a flood-coolant spindle is the right machine. Routing aluminum is a compromise between work envelope and accuracy.

Composites are a router specialty. Carbon fiber and fiberglass cut on a router with diamond-coated tooling and dust extraction. The dust is a health hazard, so the machine needs enclosed extraction. Cut edges are usually trimmed or sanded afterward because the tool leaves a slight fray.