Why buyers mix up reaming and boring on CNC hole RFQs
Hole size control on CNC parts is where quotes stall and first articles surprise. Drawings say “ream,” “bore,” or simply give a tight diameter with no process note. Estimators hear different cost and capability stories in those words: a reamer finishes a drilled hole to a size band; boring with a boring bar or fine-boring head can correct position and produce a true round diameter on a different workholding setup. Treating the adjectives as interchangeable is how aluminum housings get quoted for the wrong operation and how steel fixtures miss position while meeting size.
This guide helps buyers and RFQ teams specify CNC hole size without inventing a shop’s default process. It compares typical roles of reaming and boring, what to put on the print and an RFQ checklist. Numbers are orientation only; your OEM fit tables and the supplier’s process plan own the final method. Related reading includes designing threads and tapped holes, press-fit pins and bushings for CNC housings, GD&T basics for buyers, and deep hole drilling and gun drilling when L/D grows.
What each process is trying to do
Reaming (typical intent)
Reaming usually follows drilling (and sometimes semi-finish boring or helical milling). A multi-flute reamer removes a small amount of stock to improve size, roundness and surface finish relative to the drill. It does not reliably “move” a hole that was drilled off location—the reamer largely follows the existing center. Buyers should think: size and finish refinement of an already-located hole.
Boring (typical intent)
Boring uses a single-point tool (boring bar) or a fine-boring head to enlarge and true a hole. On a mill or lathe, boring can correct position within the machine’s capability, create stepped bores and hold diameter with in-process adjustment. Buyers should think: diameter plus the ability to locate or clean up a bore relative to datums when the process plan supports it.
Other size-control cousins
Helical interpolation / circle milling, honing and grinding also produce precise holes. This article stays on reaming vs boring language because those two words dominate RFQ email threads. If you need a specific lay or very tight cylindricity, say the geometric requirement rather than naming a process you may not need. Illustration 1 compares typical capabilities buyers assume versus what drawings should purchase.
Size, position and finish: buy geometry, not tool names
Diameter tolerance
Both reaming and boring can hold common precision bands (for example H7-class language as an illustration of fit naming—not a claim of any shop’s default). What matters on the print is the diameter limits or fit class tied to the mating pin, bearing or bushing. See press-fit pins and bushings when interference or transition fits drive the hole.
Position and pattern
If two holes must locate a dowel pattern, position tolerance and datum scheme dominate cost more than whether the email said “ream.” Boring or mill interpolation may be chosen so the machine can pick up datums and place the pattern; a reamer after a wandering drill will not rescue true position. State TP (or equivalent) explicitly—see GD&T basics for buyers and flatness parallelism perpendicularity for related frame control.
Roundness, taper and surface
Long holes taper; thin walls spring. Call out cylindricity or separate diameter checks at depths when function needs it. Surface roughness for bearing or seal bores belongs as Ra (or equivalent), not as “bore nice.” See surface roughness Ra for machined parts.
Blind vs through
Blind reamed holes need chip clearance and sometimes a undercut or relief at the bottom; boring bars need stick-out room. Note blind depth, any relief and whether the bottom face is functional.
Material and stock-removal practical notes
Aluminum
Reaming aluminum is common for pin holes and bushing bores when position comes from a quality drill or interpolation pass. Built-up edge and smear can hurt finish—coolant and reamer condition matter, but that is the shop’s problem unless you mandate a finish that forces a method.
Steels and stainless
Higher cutting forces; boring may be preferred for larger diameters or interrupted cuts. Stainless work-hardening rewards sharp tools and adequate stock removal per pass—again, specify size and geometry, not spindle brand.
Hardened materials
After heat treat, grinding or hard boring/reaming families appear. If holes must be finished after heat treat, say so; see heat treating steel after CNC machining so estimators do not assume soft machining sizes survive harden and temper movement.
Depth and L/D
As L/D grows, drill wander and reamer follow error grow; boring setups and gun-drill approaches enter the conversation. Point to deep hole drilling and gun drilling when depth is the real risk, not the word “ream.”
Drawing language that reduces churn
Prefer:
- Diameter limits or hole basis fit + mating part P/N
- Position / datum scheme for patterns
- Blind depth, through condition, relief
- Ra on functional bores
- Coat sequence if anodize or plate changes size (chem film vs Type II anodize; anodizing Type II vs Type III)
Avoid relying on:
- “Ream all holes” with no size
- “Bore for bearing” without bearing P/N and housing limits
- Process-only notes that conflict with a tolerance the shop would hold another way
Illustration 2 routes common RFQ intents to callout priorities.
Process choice vs RFQ responsibility
Shops choose tools to meet the print at quoted cost. Mandating “must ream” or “must bore” is appropriate when you have a validated process, a customer print that freezes method or a surface/lay requirement that truly forces it. Otherwise purchase the diameter, position and finish. If you are comparing quotes, ask how they will hold TP on the pattern and how they will verify diameter—not which catalog reamer number they stock.
Inspection notes that match:
- Pin / plug gauges for go/no-go size bands
- Bore micrometers or air gauges for size and taper
- CMM for position of patterns; see CMM vs optical measurement for method choice
- First article inspection reports listing each critical bore separately
RFQ checklist for hole size control
1. Every precision hole has diameter limits (or fit + reference shaft/bearing).
2. Patterns have position tolerances and datums—not only “reamed.”
3. Blind/through, depth and any relief are clear.
4. Functional Ra or seal/bearing notes are present where needed.
5. Finish sequence vs final size is stated for coated parts.
6. Process mandates appear only when truly required; otherwise geometry leads.
7. Quantity of precision holes and any customer-supplied gauges are noted.
8. Link CNC machining service and request a quote when ready to price.
Side-by-side buyer language
| Intent | Prefer writing | Avoid |
|---|---|---|
| Pin locate size | Hole limits + pin P/N | “Ream for dowel” alone |
| Bearing housing | Bore limits + bearing P/N + TP | “Bore nice” |
| Pattern location | Position to datums | Hoping reamer fixes drill walk |
| After coat size | Machine → coat → optional size | Ignoring anodize build |
| Deep small hole | Depth, L/D, breakout notes | Only “ream Ø3 through” |
Common scrap modes and quote traps
- Size OK, pattern fails: reamed holes followed a drilled location error.
- Size fails after anodize: limits were for bare metal; coat build ignored.
- Taper in deep bore: no mid-depth check; only one plug gauge used at the mouth.
- Mandated ream on a large interrupted bore: wrong process family for the feature.
- Over-specified process note blocked a cheaper interpolation strategy that met the same tolerances.
How this fits a CNC hole RFQ package
Send PDF/PMI plus STEP, list critical bores in a balloon table and include mating pin or bearing datasheets. Separate press-fit holes, tapped holes and clearance holes so estimators do not apply one H7 note globally. When fixture plates also need flatness, face milling vs peripheral milling for flatness and step heights keeps plane control distinct from hole size control.
Summary for estimators and buyers
Reaming and boring are tools for different combinations of size, position and access—not synonyms. Put diameter, position, depth and finish on the drawing; reserve process mandates for locked methods. That package compares quotes on geometry, machines with fewer method arguments and inspects against the same characteristics the part needs in assembly.