Guide
How do you write a hole callout for drilled, reamed and bored holes?
A hole callout is the leader note that defines a hole completely in one place: how many, what size and tolerance, how deep or THRU, and any counterbore, countersink or thread stacked on top. Write it to describe the finished hole, not the tool: the tolerance, not the word DRILL or REAM, is what tells the shop whether the hole is drilled, reamed or bored.
By Saola Manufacturing engineering team · Published · Updated
On this page
What goes into a complete hole callout, and in what order?
Write the quantity first, then the diameter with its tolerance, then the depth or THRU, then each secondary feature in the order it is machined, and finish with any note that applies to the whole hole. A callout is complete when every diameter has a depth, an angle or THRU, and every size has a tolerance from the note or the title block.
A typical complete callout reads 4X Ø8.0–8.1 THRU for a clearance pattern, or 2X Ø6 H7 ↧12 for a pair of blind dowel holes. The symbols and how to read them are covered in our engineering drawing symbols guide, and the screw-head recesses in the counterbore vs countersink guide; this guide is about writing the note so the hole comes back right.
Drawings made to ISO conventions follow the same logic with a compact designation defined in ISO 15786, the standard for simplified representation and dimensioning of holes. If your supplier mostly reads one convention, do not mix the two on one sheet.
Keep the location separate. The callout defines the hole itself; where it sits comes from basic dimensions and a position tolerance in a feature control frame placed under the callout, or from toleranced coordinate dimensions. A callout with a perfect size and no location control is still an incomplete hole.
Should the callout say DRILL, REAM or BORE?
Generally no. Among the fundamental rules of ASME Y14.5 is that a drawing should define a part without specifying manufacturing methods, so the hole is given by its size and tolerance, and the shop picks the process that meets it.
The rule, as summarized by this ASME Y14.5 study guide, gives a hole diameter as the example: the drawing states the size without saying whether the hole is drilled, reamed, punched or made another way. Information that is essential to the engineering requirement may still be specified. The standard itself is ASME Y14.5-2018.
Old drawings are full of notes like “DRILL .257 THRU” or “REAM Ø.250”. They cause two problems. A shop that reams a hole because the note says so may still miss the intended size, because “ream” carries no tolerance. And a shop that can meet the size more cheaply by boring or interpolating is technically out of compliance with the note. Replace the verb with a size and a tolerance. If a process really is functional, for example a hole that must be free of helical tool marks, say that as a requirement, such as a surface texture or a form tolerance, or as a note like “NO SPIRAL TOOL MARKS”. If you want to share a suggested process without making it mandatory, Y14.5 provides a NONMANDATORY (MFG DATA) note for that purpose.
How do you call out a plain drilled hole?
Give the diameter with a tolerance that a drill can hold, and prefer sizes that match standard drills. For clearance holes, take the size from a clearance-hole standard and keep the tolerance generous.
A clearance hole callout such as 4X Ø6.6 THRU takes its size from a standard like ISO 273 for metric screws; our clearance hole chart lists the sizes. A drilled hole typically comes out slightly oversize and not perfectly round, so a tight tolerance on a drilled hole simply forces the shop to ream or bore it. If the hole is for clearance, let the title-block tolerance or a plus-only tolerance govern it. The reamed vs drilled hole guide covers what each process typically holds.
For a through hole, write THRU, not a depth equal to the part thickness: a depth invites the question of what happens when the stock thickness varies. For a hole that breaks into a cross hole or an internal cavity, say so on the drawing, because the exit burr is then inside the part and needs its own deburr requirement.
How do you call out a reamed or bored precision hole?
Give the size with a fit class or explicit limits, add any form, orientation or surface texture requirement that the function needs, and state how deep the full-size portion must go. The tolerance will lead the shop to ream or bore; the drawing does not need to say which.
Dowel and bearing holes are usually called out with an ISO tolerance class, such as Ø6 H7, per the system in ISO 286-1, or with explicit upper and lower limits. Many drawings show both the class and the limits so nobody has to look up the table. If the hole must stay straight and round along its length, add a cylindricity or straightness tolerance rather than relying on size alone; size limits by themselves allow some taper and lobing within the envelope.
On a blind precision hole, the critical value is the depth of full size, not the total depth. Reamers and boring bars cannot finish all the way to the bottom of a drilled hole, so a blind H7 hole needs a drilled depth that runs deeper than the reamed depth. Give the reamed depth as the requirement and let the drill depth be a result, or show both, for example Ø6 H7 ↧12 with the drilled hole beyond it, if the material under the hole is thin. Large holes, holes that must be on position tightly, and holes in castings where the cored hole wanders are typically bored rather than reamed, because boring corrects location and reaming follows the existing hole.
| Callout on the drawing | What it requires | Process the shop will usually choose |
|---|---|---|
4X Ø6.6 THRU (title-block tolerance) | Clearance hole, generous size tolerance | Drill |
2X Ø6 H7 THRU | Fit-class hole for a dowel | Drill, then ream (or bore) |
Ø6 H7 ↧12 | Blind fit hole, full size for 12 deep | Drill deeper, ream to depth |
Ø32 H7 THRU with tight position | Large fit bore on location | Rough, then bore |
Ø10 ↧8 FLAT BTM | Blind hole with a flat floor | Drill, then end mill or flat-bottom drill |
DRILL Ø.257 THRU (legacy) | A process, no tolerance stated | Ask: replace with size and tolerance |
REAM Ø.250 (legacy) | A process; size limits and depth missing | Ask: replace with limits or fit class |
How do you call out the bottom of a blind hole?
Say what the bottom must be: a drill point is the default and needs no note, a flat bottom needs a note such as FLAT BTM, and any limit on the remaining wall needs a dimension. The depth symbol always means the depth of the full diameter, not the tip of the drill point.
A standard twist drill leaves a conical bottom with a typical 118° point angle. If that is acceptable, the callout needs only the diameter and depth. If a pin, a spring or a sensor must sit flat on the floor, write FLAT BTM and, if it matters, a maximum corner radius. A flat-bottom hole costs an extra tool, so do not ask for one out of habit.
Thin floors are the other risk. If a blind hole sits close to the opposite face, the drill point can break through even when the full-diameter depth is in tolerance. Either dimension the remaining wall thickness as a minimum or give a maximum drill-point depth. For tapped blind holes, the blind tapped hole guide shows how to separate thread depth from drill depth.
How do you call out stepped and multi-feature holes?
Use one stacked callout per hole, listing features in the order they are cut from the entry face, and use FAR SIDE when a feature is on the opposite face. Splitting one hole into unrelated dimensions invites features that are not on the same axis.
A stepped bore for a bearing and a seal might read Ø22 H7 ↧10 above Ø15 THRU, both in one note from the same leader. That tells the shop and the inspector that the two diameters share an axis. If coaxiality matters beyond what one setup naturally produces, add a runout or position control between them; one callout implies a common axis, but it does not put a number on how common.
When a hole pattern repeats with different features, use separate callouts with their own quantities rather than one callout with exceptions. “6X … EXCEPT 2X …” notes are easy to misread and hard to inspect. If the part is a casting with cored holes, say which holes are machined from solid and which are finished from the cored hole, because that decides the stock and the process.
What should the drawing and RFQ say about holes?
Every hole should have a complete callout with a tolerance, a location control and, for blind holes, a bottom definition. The RFQ should flag the holes that matter for function so the supplier can plan gauging for them.
- No process verbs. Replace DRILL, REAM and BORE notes with sizes and tolerances.
- Fit holes flagged. Mark dowel, bearing and seal holes as critical characteristics.
- Blind holes. Full-size depth, bottom form, and minimum remaining wall where thin.
- Finish allowance. If the part is anodized, plated or coated, say whether hole sizes apply before or after finishing, or mask the holes.
- Inspection. For fit holes, say whether a go/no-go plug gauge is acceptable or a measured value is required.
How does Saola handle hole callouts at drawing review?
Hole callouts are checked at drawing review, and legacy process notes or incomplete callouts come back as written questions on a marked-up copy of the drawing. Reamed and bored holes in castings are a large part of the work on the CNC milling line.
The CNC milling page describes second-operation machining of castings, including bores bored and reamed to print and tapped holes, and states that simultaneous five-axis machining is not offered, so compound-angle holes should be raised early. On a new part, the first-article inspection report covers every toleranced dimension on the drawing, as described on the quality page. Send the drawing set through the quote form.
Frequently asked
Is it wrong to write DRILL on a drawing?
It is not forbidden, but it is discouraged by ASME Y14.5 practice because it names a process instead of a requirement. If the size and tolerance are there, the word adds nothing; if they are missing, the word does not replace them.
What does the depth symbol mean on a drilled hole?
The depth of the full diameter, measured from the surface where the hole starts. The drill point below it is not included.
Should I give a fit class like H7 or explicit limits?
Either is valid. Many drawings show both, which saves the shop and the inspector a table lookup and removes any doubt about the standard edition.
How do I call out a hole that must be reamed for surface finish?
State the surface texture and any form tolerance the function needs. If the shop can meet them by another method, the part still works.
Do I need a separate callout for each hole?
No. Use a quantity such as 4X for identical holes. Use separate callouts when holes differ in any feature, rather than one callout with exceptions.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018
- Fundamental Rules of ASME Y14.5 (study guide summary), Open Exam Prep, accessed November 2026
- ISO 286-1:2010, ISO code system for tolerances on linear sizes, Part 1, ISO, 2010
- ISO 273:1979, Fasteners: Clearance holes for bolts and screws, ISO, 1979
- ISO 15786:2008, Technical drawings: Simplified representation and dimensioning of holes, ISO, 2008