CNC Machining Accuracy on the Surface: How It Is Controlled
This page explains what actually sets the finish on a machined face: tool geometry, chip load, spindle and fixture rigidity, and the finishing pass you leave for last. It is written for design engineers and buyers who need to judge whether a drawing callout of Ra 0.8-1.6 μm is realistic, and what it costs in cycle time.
Key takeaways
What Actually Creates the Surface
Every machined face is a set of overlapping arcs left by the cutting edge. The height of those arcs is the theoretical surface roughness, and it comes from two numbers: the corner radius of the insert or the ball nose, and the feed per tooth. Raise the feed and the scallops get taller. Raise the corner radius and they get shorter. That relationship is the whole foundation of cnc machining accuracy on the surface, and it holds for milling, turning, and drilling alike.
In practice the theoretical number is not what you measure. A sharp tool cutting 6061 aluminium at 0.08 mm per tooth can produce a near-mirror face on paper, yet the part leaves the machine at Ra 1.6 μm because the tool chattered, the chips were recut, or the coolant stopped reaching the edge. Real Ra is the theoretical value plus everything the process adds on top.
The added roughness has names. Built-up edge welds workpiece material onto the cutting edge, then breaks off and leaves a torn patch. Chatter marks appear as a periodic pattern with a pitch you can measure and trace back to a spindle speed, a tool overhang, or a natural frequency in the fixture. Smearing happens when the cutting edge rubs instead of shears, which is common on soft stainless and on any material cut with a worn edge.
So the honest answer to what controls surface finish is that the tool path sets the target and the machine dynamics decide whether you hit it. Machines with high static stiffness and well-damped spindles give you a wider window of cutting data that still works. Machines that flex force you into conservative feeds, which costs cycle time.
- 1Theoretical RaSet by corner radius and feed per tooth. Predictable and easy to calculate.
- 2Dynamic RaSet by vibration, chip evacuation, edge condition, and thermal movement.
- 3Measured RaTaken on the real part after the real fixture. This is the only number that counts.
Cutting Parameters That Move Ra
Feed per tooth is the single most direct lever. Doubling the feed per tooth roughly quadruples the scallop height on a radiused cutter, so a small change has a large effect on the measured number. On aluminium we commonly finish at 0.03-0.08 mm per tooth with a 2-flute or 3-flute cutter, and on stainless we drop to 0.02-0.05 mm per tooth because the material work hardens if the edge rubs.
Cutting speed controls where the heat goes. Running a carbide tool too slowly in steel pushes heat into the workpiece and the tool edge, which promotes built-up edge. Running too fast burns the coating. The practical window for finishing 6061 aluminium is 200-400 m/min surface speed; for 304 stainless it is 80-150 m/min with generous coolant.
Radial and axial depth of cut do less for Ra than people expect, but they do control tool load and therefore deflection. A finishing pass at 0.2-0.5 mm radial width keeps the radial cutting force low, which keeps the tool from pushing away from the wall. If you take a full-width finishing pass, the tool bends and the wall comes out tapered or rippled.
Coolant is not optional on finishing. Flood coolant clears chips before they are recut, which is the main source of random scratches. Through-spindle coolant helps most in deep pockets and bores, where a flood nozzle never reaches the cutting zone.
- 1Feed per tooth0.03-0.08 mm/tooth finishing in aluminium; 0.02-0.05 mm/tooth in stainless.
- 2Surface speed200-400 m/min in 6061; 80-150 m/min in 304 with flood coolant.
- 3Finishing pass width0.2-0.5 mm radial keeps deflection low and the wall straight.
Rigidity, Tool Holders, and the Floor You Cannot Beat
Vibration sets a floor on surface finish. You can see it on the part as a regular pattern, and you can feel it as a tone change during the cut. The usual sources are long tool overhangs, thin walls that deflect under cutting force, and fixture points that allow the part to ring. Shortening the tool assembly by 20 mm often does more for Ra than any change to the cutting data.
Tool holders matter more than most drawings admit. A shrink-fit or hydraulic holder runs with less than 0.003 mm runout, while a worn collet chuck can run at 0.02 mm or worse. Runout makes one flute cut deeper than the others, so the effective feed per tooth is uneven and the surface carries a once-per-revolution mark. On finishing operations we check runout before the pass, not after.
Thermal growth is the slow variable. A spindle that has been running for two hours is not the same machine that started cold. On tight-tolerance finishing we let the machine warm up and take a light skim cut before the final pass. For long parts, cutting fluid temperature stability matters as much as the spindle.
Our own machines cover a range here. We run 16 simultaneous 5-axis machining centers, 12 four-axis mills, 27 three-axis machines, and 16 mill-turn centers, with a maximum processing size of 4,000 mm and travels from 500 × 500 × 450 mm up to 4,000 × 400 × 150 mm. Five-axis work helps surface finish because the tool can stay normal to a curved surface, which keeps the effective contact geometry constant across the whole face.
- 1Shorten the toolLess overhang means less bending and a higher chatter threshold.
- 2Check runoutUnder 0.003 mm on finishing holders. Uneven flute load shows as a periodic mark.
- 3Warm up firstA cold spindle finishes differently from a warm one on tight tolerances.
Where Surface Accuracy Gets Hard
Deep slots are the classic problem. A slot 6 mm wide and 40 mm deep forces a small-diameter cutter on a long shank, and the length-to-diameter ratio climbs past 6:1. At that ratio the tool deflects under normal cutting force and the wall finish degrades. There is no feed rate that fixes it. The options are a smaller depth of cut with more passes, a larger corner radius on the slot floor, or accepting a coarser Ra and a separate finishing operation.
Internal corners are the second limit. A 90° corner can only be reached by a tool whose radius is smaller than the corner radius, so a sharp internal corner is impossible with a rotating cutter. The corner always carries a radius equal to the tool radius. If the drawing calls for a sharp corner and a fine finish, one of the two has to move.
Thin walls behave differently again. A 1 mm wall in aluminium will deflect away from the cutter and spring back, leaving a tapered surface and a chatter mark near the top edge. We usually leave material on both sides, finish one side, then flip and finish the other with light passes.
Material choice closes the loop. Free-machining grades like 6061-T6, 303 stainless, and C36000 brass finish cleanly with standard parameters. Titanium Ti-6Al-4V, Inconel, and 17-4PH stainless need lower surface speed, more coolant, and a fresh edge, and even then the achievable Ra is typically one grade coarser than the same geometry in aluminium.
- 1Deep slotsAbove 6:1 length-to-diameter, expect a coarser finish on the walls.
- 2Sharp internal cornersThe cutter radius becomes the corner radius. Design for it.
- 3Thin wallsDeflection and spring-back. Finish both sides with light passes.
- 4Hard materialsTitanium and Inconel run one Ra grade coarser than aluminium at the same geometry.
Ra Targets and What They Require
Typical capability at GreatLight. Values depend on geometry and material.
| Ra target | Typical process | Where it fits | Main constraint |
|---|---|---|---|
| Ra 3.2 μm | Roughing or single-pass milling | Brackets, non-sealing faces | Nothing special; fast cycle |
| Ra 1.6-3.2 μm | Standard finishing pass | General machined surfaces | Tool wear if the edge is dull |
| Ra 0.8-1.6 μm | Dedicated finishing pass | Sealing faces, bearing seats | Rigid setup and sharp edge |
| Ra 0.2-0.8 μm | Fine finishing or light polishing | Optical and sealing surfaces | Cycle time and inspection cost |
| Below Ra 0.2 μm | Lapping or polishing after machining | Mirror surfaces, some optics | Not a milling operation |
| Sharp internal corner plus fine Ra | Not feasible as drawn | Redesign the corner | Cutter radius sets the corner |
The Trade You Are Actually Making
If the face seals or carries a bearing, spend the cycle time on a separate finishing pass and a rigid setup. If it is a bracket or a cover, call out Ra 3.2 μm and put the money into tolerance instead.
Questions Engineers Ask
Can you hold Ra 0.8 μm on a deep bore?
It depends on the depth-to-diameter ratio. Up to about 4:1 we can bore and finish with a rigid bar and get into the Ra 0.8-1.6 μm band. Beyond that the bar deflects and the finish degrades, so we would either interpolate with a smaller tool at a lower feed or plan a separate honing step.
Send the drawing and we will tell you which side of that line your part falls on before you commit to a finish callout.
Does a smoother finish always cost more?
Yes, almost always, because the finishing pass is a separate operation at a low material removal rate. Going from Ra 1.6 μm to Ra 0.8 μm on a simple face might add a few minutes. Going to Ra 0.2 μm adds polishing, which is manual and hard to automate.
The cost curve is not linear. The last step is the expensive one.
How do you inspect surface finish?
We inspect 100% of parts before shipment, with raw material checks, in-process monitoring, and final inspection. Surface finish is checked with a portable profilometer on the specified face, and reports are available on request.
If your drawing names a specific cutoff length or a specific measurement direction, put it on the drawing. Ra measured across the lay is not the same number as Ra measured along it.
Can anodizing change the measured Ra?
Yes. Anodizing grows an oxide layer that follows the original profile, so a light clear anodize usually reads close to the pre-plate value. Hardcoat anodizing builds a thicker and rougher layer, and a bead blast before anodizing will dominate the final number.
If the finish matters, specify the surface treatment before you specify Ra, not after.
What tolerance can you hold alongside a fine finish?
We hold ±0.005 mm (±0.0002 in) on tight features, with a 99.99% qualification rate across production. Fine finish and tight tolerance usually go together because both depend on a rigid setup and a sharp edge.
The exception is thin walls, where deflection limits both at once.
Do you work from a 3D model or a drawing?
Both. We return a quotation and a free DFM analysis within 12 hours, and production can start within 24 hours. For finish-critical faces, mark them on the model or the drawing so we can plan the tool path around them.
There is no minimum order quantity. One prototype and a 10,000-part run go through the same DFM step.
Send the Face You Care About
Upload your model or drawing and mark the surfaces that need a finish callout. We will return a quotation with a free DFM analysis within 12 hours and tell you which Ra values are realistic for your geometry.
12-hour quote100% inspectionNDA on request
More From the Shop Floor
We publish setup notes, tooling trials and inspection data from the factory floor.
