A drilled hole and a reamed hole can have the same nominal diameter in CAD and still represent very different manufacturing requirements.
Drilling is usually the efficient way to create an ordinary clearance or preparation hole. Reaming is a finishing operation used when the final bore size and surface condition need tighter control.
The useful design question is not "is reaming better?" It is whether the assembly function actually needs the extra precision.
Start with the fit, not the process name
Ask what the hole does:
- clear a bolt;
- locate a dowel pin;
- guide a shaft;
- accept a bushing;
- locate two parts repeatedly;
- provide a bearing or sealing surface;
- act only as a pilot for tapping.
A clearance bolt hole normally does not need the same diameter control as a dowel locating hole.
If the function only needs clearance, specifying a tight reamed fit can add machining and inspection cost without improving the product.
Reaming is a finishing operation
A common sequence is to create a pre-hole slightly undersize and then ream to final size.
The reamer removes a relatively small amount of material and improves size or finish. Tool makers' instructions make the pre-hole part of the process: it must leave the correct stock allowance, and if too little stock is left the reamer rubs, wears quickly and loses diameter. Sandvik Coromant reaming instructions. It is not a magic tool that turns a badly located or crooked pre-hole into perfect geometry.
The University of Florida Design Lab's DFMA guidance makes this point directly: do not rely on reaming to correct position or alignment errors. See UF Design Lab reaming guidance.
If true position is critical, the whole process including setup, pre-hole location and inspection has to support it.
Diameter tolerance and position tolerance are different questions
A drawing can require a tightly sized hole that is allowed to move substantially in position, or a more ordinary diameter with a very tight positional tolerance.
Do not replace one requirement with the other. The ISO fit system itself draws this line: ISO 286-1 defines tolerance classes for sizes and the terminology for fits between two features of size, without constraints of orientation and location. Position has to be specified separately. ISO 286-1:2010.
For a pin-locating feature, review final diameter and fit system, true position or coordinate tolerance, perpendicularity or axis requirement, depth, mating pin tolerance, and surface finish if functionally important.
A STEP cylinder shows nominal geometry. It does not automatically tell the shop which tolerance band governs the finished bore unless the PMI or drawing handoff preserves that information.
The STEP tolerance guide explains that distinction.
A reamer tends to follow the hole it is given
If the pre-drilled hole wanders, is tapered badly or begins on an unstable surface, the reamer may improve diameter without fully correcting the axis.
That is why feature location should be created with an appropriate upstream process and setup.
For large or difficult bores, boring or another finishing operation may be more appropriate because process choice depends on diameter, depth, location accuracy, material and machine capability.
Do not specify "REAM" as a substitute for defining the functional requirement.
Blind holes need extra process room
A blind reamed hole creates another depth question.
The pre-drilled hole often needs extra depth for drill point, reamer lead, chip space and tool clearance. The UF Design Lab's reaming tips say so directly: if a blind hole requires reaming, drill extra depth to provide room for chips. UF Design Lab reaming tips.
If the design requires a precision cylindrical depth of 20 mm, a 20 mm-deep blind cavity in CAD may not give the process enough room.
Review the full-diameter precision length separately from total drilled depth and bottom geometry. If depth-to-diameter ratio is high, also review tool reach with the deep-hole guide.
Do not put a tight fit on every important-looking hole
Standard fit systems are useful when a standardized fit is actually part of the design. They should not be used as decoration to signal "this hole matters."
A tolerance should come from required clearance or interference, assembly repeatability, locating strategy, load and wear, mating-part tolerance and inspection capability.
If a supplier can meet the functional fit with precision drilling, boring, interpolation, reaming or grinding, the engineering drawing usually should control the result rather than dictate one process unless the process itself is required.
Use CAD to inspect geometry, drawing or PMI to define precision
CADProps can inspect supported STEP geometry and measure nominal analytic features such as readable circular or cylindrical geometry in supported cases.
It does not determine whether a hole should be drilled, reamed or bored, and it does not certify fits from nominal geometry alone.
Before quoting:
- verify units;
- identify fit-critical holes;
- record nominal diameter and depth;
- check nearby wall thickness and access;
- attach the tolerance or fit requirement;
- distinguish diameter tolerance from positional tolerance;
- let the supplier propose the process where appropriate.
A useful RFQ distinction
Instead of sending only "diameter 10 hole," communicate whether the hole is ordinary clearance or a controlled locating feature with a specific fit and position requirement.
That difference gives the shop permission to use an efficient process for ordinary holes while spending precision machining and inspection effort only where the assembly benefits.
The CNC quote preparation guide covers the rest of the RFQ package.
The design principle is straightforward: use drilling for ordinary geometry, call for precision only when the fit requires it, and define the result rather than assuming one machining operation guarantees it.
Separate two acceptance checks on a locating bore
For a locating bore, create separate checks for finished diameter and axis location relative to the specified datums. A hole can pass a size gauge while its center is in the wrong place; a correctly located hole can still have an unsuitable size or finish.
A nominal Ø10 cylinder in the model supplies neither the permitted fit band nor the positional tolerance. Read both from the controlling definition and confirm how the supplier will inspect them. If reaming is proposed, discuss pre-hole location and accessible finishing depth. CADProps can help inspect nominal geometry, but it does not turn a measured cylinder into an H7 designation or approve the measurement method.
Original article: CADProps · https://www.cadprops.com/guides/reamed-hole-vs-drilled-hole/