CNC Router Bit Selection Is Three Decisions: Helix, Chipload and Tool Material

The rain comes off the Sound most of the winter and the shop smells like wet cedar even when I'm cutting maple. Ten feet from the hand planes sits a router spindle that will turn an expensive compression bit into scrap in about four seconds if I feed it wrong. Clients don't pay me for either machine. They pay for an edge that doesn't need sanding and a delivery date I can hit.

So when someone new to CNC asks which bit to use, they want one answer, and there isn't one. There are three, and they're independent.

Bit Selection Is Three Decisions, Not One

The manufacturer literature never treats "which bit" as a single question. It answers three:

1. Helix geometry — upcut, downcut, compression, straight. Decided by which face has to come out clean and how the part is held to the table.
2. Chipload — the bite each cutting edge takes. Decided by material and bit diameter, and published in tables you can look up.
3. Tool material and coating — HSS, carbide-tipped, solid carbide, PCD. Decided by how abrasive the material is and how many parts you're making.

Most people I watch pick a bit by name and then guess at feeds. Reverse it: geometry first, chipload from the chart for that exact tool, then decide what you're willing to spend.

Helix Geometry Answers a Hold-Down Question Before a Finish Question

The Leitz Metalworking Technology Group's CNC Production Routing Guide, authored by Onsrud Cutter, states the trade-off plainly: an upcut helix gives the best finishes and good chip extraction but sometimes lifts parts; a downcut helix helps hold parts down but sometimes rewelds chips and chatters on unsupported parts. Whiteside describes its RU2100 up-cut spiral as bringing "chips up and out of the cut" and its RD2100 down-cut as excelling at "clean, top edges."

The rest of the hold-down argument is less known. The same guide says that in flow-through vacuum work, downcut spirals are chosen to intentionally pack the chips into the cut and minimize vacuum loss through the open table the cutting creates — and it's explicit that this "sustains more heat in the tool." That's a deliberate trade of tool life for hold-down, not a finish decision at all. Pod systems, it adds, almost always require downcut or neutral tools so parts don't get pushed off the pod.

Onsrud publishes a good/better/best matrix on each per-material cutting-data sheet. For single-pass hardwood, "good" is the 52-200 or 57-200 wood rout — the PCT-19 catalog identifies these as a solid carbide 2-flute upcut and downcut spiral respectively — "better" is the 60-300/60-350, and "best" is the 60-100C compression. Softwood reads identically. The laminated chipboard sheet is the interesting one: every option in its good/better/best row is a compression tool, from 60-100MW at "good" through 60-100MC to 60-100PLR at "best." No straight or single-helix entry is offered in that row at all.

Onsrud also rates a compression as "best" for single-pass solid hardwood and softwood, so the shorthand that compression bits are only for plywood isn't what the charts say. All of this is vendor guidance, though: I found no independent test comparing upcut, downcut and compression edge quality on the same material.

Chipload Is the Number That Decides Everything Downstream

Every source publishes the same arithmetic. Chipload equals feed rate in IPM divided by RPM times the number of cutting edges; rearranged, feed rate equals RPM × cutting edges × chipload. ShopBot Tools explains the stakes in its Feeds and Speeds charts: too small a chipload and "bits will get too hot and dull quicker"; too high and "the tool will deflect creating a bad surface finish and, in extreme cases, chip or break the bit."

Two things in the tables surprise people.

First, tool construction moves the number on its own. In Freud's own charts, a 1/4" solid carbide bit in hardwood takes .008"–.011" per tooth. A 1/4" carbide-tipped bit, same diameter, same hardwood, takes .005"–.007". Roughly 60% more bite from the solid carbide tool. Freud also warns that carbide-tipped bits should not be used to drill directly into the workpiece.

Second, geometry moves it further. On Onsrud's hardwood sheet a 1/2" 52-200/57-200 wood rout is listed at .007"–.009", while a 1/2" 60-100MW compression is listed at .018"–.020" and the 60-100C at .021"–.023". Run Onsrud's own formula on those midpoints — my calculation, not a feed rate Onsrud prints — and at 18,000 RPM the two-flute wood rout gives 288 IPM against the two-flute compression's 684. Same diameter, same flute count, same species, same spindle speed, 2.4× the feed. The Leitz/Onsrud guide corroborates the shape of that gap: at 1/2" cutting edge diameter and 18,000 RPM it lists wood routs at 200–400 IPM and compression spirals at 400–1500. Chipload is per tooth, though, and Onsrud's series differ in flute count, so don't compare feeds across series until you've confirmed that in the catalog.

Every chart here assumes depth of cut equals bit diameter. Freud publishes the correction: at 2× diameter, reduce chipload by at least 25%; at 3×, by at least 50%. Onsrud's hardwood sheet prints the same rule. Freud's worked example takes a .019" chart value for a 1/2" bit cutting 1" deep down to .014".

Then stop trusting the chart and tune. ShopBot publishes the procedure it credits to Onsrud: raise feed until finish degrades or the part moves in the hold-downs, back off 10%, then reduce RPM until finish deteriorates and bring it back up until acceptable. The Leitz guide gives the same loop in its own words. Date these charts when you cite them — ShopBot's is from 2016, Freud's and the hosted Leitz guide from 2017, the Onsrud hardwood sheet's file metadata from 2018.

The Leitz feeds-and-speeds page ends with an instruction I'd put on a sticker: "Always remember make chips not dust!" ToolsToday's argument that slowing the feed without also dropping RPM makes scorching worse follows straight from it, though as a vendor claim with no measured burn data behind it.

The Expensive Bit

The argument I've come to believe matters most for anyone taking commissions is one Onsrud published in full. Its value analysis covers 500 high-pressure-laminate chipcore desk tops at $100/hour machine cost: an Onsrud 60-170 compression at $84.85 against a competitive carbide-tipped straight at $15.00. The compression runs 600 IPM to the straight bit's 200, cutting machine time from 460 minutes to 155. Tooling cost comes out higher for the compression, $243.20 against $93.00 — and total job cost still lands at $501.53 against $859.67. A bit costing 5.7× more to buy finishes the job $358.14 cheaper. Those are historic figures from an undated guide hosted since 2017, but the structure doesn't age: machine time dominates.

Coatings are a smaller version of the same bet. At ToolsToday, Amana's retail arm, the uncoated 46170 quarter-inch compression listed at $76.80 on 3 August 2026 and the Spektra-coated 46170-K at $87.38, a 13.8% premium. Amana claims the nACo coating runs about 4,500 Vickers and delivers "up to 2.5 times" the durability of uncoated — a manufacturer claim with no independent verification I could find. One oddity I'll report rather than explain: the DLC-coated 46170-DLC listed at $55.73 the same day at the same retailer, below the uncoated version. The 1/2" 46188-DLC at $139.39 checks out on its own product page, so the DLC pricing is real. I don't know why the quarter-inch lists under the uncoated tool.

On tool material, Leitz/Onsrud draws the line at the machine: HSS and carbide-tipped for manually fed work, solid carbide and PCD for CNC — solid carbide buying high feed rates at the cost of increased breakage, PCD buying long tool life at very high initial cost and slow feed rates.

Species

The machinability table The Wood Database reproduces from Davis's 1962 USDA bulletin belongs above every CNC machine, because shaping is the operation closest to what a router bit does, and it's the column that collapses. Red oak planes at 91% defect-free but shapes at 28%. Basswood, the default carving stock because it's soft and cheap, shapes at 10%. Hard maple runs the other way: worst planing in the group at 54%, but 72% shaping, second only to cherry at 80%.

Peer-reviewed work sharpens this. Lungu, Gurău and Coșereanu, in BioResources in 2023, routed maple and oak with a CMT 715.095.11 90° V-bit at 15,000 RPM and feeds of 3 and 6 m/min across grain angles from 0° to 90°. Oak's core roughness climbed from Rk 11–13 µm along the grain to 28–30 µm at a 60° milling angle. Maple showed no significant change from 0° to 60° and only worsened at 75° and 90°. On edge quality — the ruptures you actually see — the worst angle for both species was 60°, not 90°. That isn't what shop intuition predicts, and it makes nesting orientation a real variable.

Two findings deserve to be held loosely, because they cut against the marketing. Pelit, Korkmaz and Budakçı, in BioResources in 2021, measured lower roughness from straight end mills than from spiral end mills in thermally treated pine, beech and linden — thermal treatment is a real confound, but it's a peer-reviewed result against a uniform vendor position. And Sütçü's 2013 BioResources study of edge-glued panels found the dominant roughness parameter differs by species: cutting direction for pine, cutting depth and feed rate for spruce.

Where I'd Start

Pick geometry from the hold-down, not the catalog photo. Look up the chipload for the exact series and diameter in your hand, correct it for depth of cut, then run the feed up until the finish or the part tells you to stop and back off 10%. Check the collet before you blame the bit: Leitz/Onsrud attributes almost 80% of breakage problems to worn equipment and improper tooling and fixturing, and wants the shank filling at least 80% of a full-grip collet's depth.

Most of all, price the machine hour before you price the bit. Onsrud's own numbers say the tool costing five times more can still be the cheap way to cut the job. In a shop where the spindle is the bottleneck, that isn't a preference. It's arithmetic.