Guide
Full radius callout: when do you write R, CR, R MAX or a radius with no value?
A full radius callout is a radius shown with the letter R and no value, used where an end or edge is fully rounded so that the radius is set by the width or thickness of the feature it closes, such as the ends of a slot or a rounded tab. Use it only when the round must blend tangent into both sides; when the radius size itself matters, give R with a tolerance, a MAX or MIN limit, or CR when the shape of the curve also has to be smooth.
By Saola Manufacturing engineering team · Published · Updated
The radius looks like the simplest dimension on a drawing, yet five different callouts are in common use and each lets the machinist make something different. This guide sets them side by side, explains what each permits and how it is checked, and lists the mistakes that cause arguments at incoming inspection. Choosing between a fillet and a chamfer in the first place is covered in fillet vs chamfer on machined parts.
On this page
What are the different ways to call out a radius?
Five: a toleranced radius (R), a controlled radius (CR), a single-limit radius (R MAX or R MIN), a full radius shown with R and no value, and a basic radius controlled by profile of a line.
All five rest on the radius rules of ASME Y14.5-2018, the current US dimensioning standard. A recent euspen conference paper on radius inspection summarizes the three main approaches the standard offers: the standard radius, which lets the profile take essentially any shape inside a crescent-shaped zone when the center is not located; the controlled radius, which also excludes flats, reversals and local irregularities; and profile of a line around a basic radius (Szczepański and Magdziak, euspen 2026).
| Callout | Example | What it allows | Typical use | How it is checked |
|---|---|---|---|---|
| Toleranced radius | R 1.8–2.2 (limits) | Any shape, including flats and reversals, inside the zone between the two limit arcs | Most fillets and edge rounds | Radius gauge, optical comparison, vision system |
| Controlled radius | CR 1.8–2.2 | Same zone, but a fair curve with no flats or reversals | Fatigue-loaded shoulders, sealing and flow surfaces | Size as for R, plus a separate check for defects in the curve |
| Single limit | R0.5 MAX / R1 MIN | Anything from zero up to the MAX, or from the MIN upward | Inside corners for mating clearance (MAX); stress relief (MIN) | Go or no-go radius gauge on the one limit |
| Full radius | 2X R (no value) | A round tangent to both sides; size follows the feature width | Slot ends, rounded tabs and lugs | Width and length of the feature, plus visual tangency |
| Profile of a line | Basic R2 with a profile frame | A uniform band around the true arc, optionally located to datums | Radii that must also be located, or curves checked by scanning | Vision system or CMM scan against the nominal curve |
What does a full radius with no value actually require?
It requires the end to be fully rounded and tangent to both sides, so its size is whatever the width of the feature makes it, within the width tolerance.
On a slot dimensioned by width and overall length, the ends are shown with 2X R and no number. Adding a radius value would create a double dimension, because the radius is already half the width. If the width is toleranced, the radius follows it; a separate radius tolerance can only conflict with the width tolerance. Current Y14.5 practice does not use the word FULL, although many shops still read “R FULL” on legacy drawings to mean the same thing.
The full radius is the wrong callout when the end is only partly rounded, for example a pocket wider than the corner radius, or a tab whose round does not meet both faces. Then the radius has a size of its own and must be dimensioned. It is also the wrong callout when the round must hold a size independent of the width, such as a slot that a pin must bear against at a known radius.
For milled slots, full-radius ends match the cutter: an end mill of the slot width leaves full-radius ends automatically, so the full radius also tells the shop which cutter size the slot assumes.
When is a plain R not enough, so the drawing needs CR?
When a flat or a dip inside the tolerance zone would hurt the part, for example a stress concentration on a fatigue shoulder or a step in a sealing or flow surface; otherwise R is enough and cheaper to inspect.
Under a plain radius, a profile that is mostly flat with two sharp corners can still pass if it stays inside the crescent. The controlled radius was introduced to limit such distortions and keep stress uniform along the transition, and it is common on aerodynamic and rotating parts. The same euspen paper notes that the standard defines CR but gives no detailed inspection method, so how large an imperfection breaks a CR callout is best set in a company standard or internal document (euspen 2026).
That is the practical point for buyers: CR adds an inspection step, a check of the curve for flats and reversals on top of the size check, and the result depends on the scanning data quality. The authors found that, for the radii they tested, the quality of the scanned data influenced the result more than the evaluation method. If you use CR, say how the curve will be judged: a vision system overlay with a defect limit, a scan with a stated filter, or a profile tolerance.
What does R MAX or R MIN let the machinist do?
A MAX radius permits any radius up to the limit, including a sharp corner, and a MIN radius permits any radius from the limit upward, so each controls only the side of the size that matters.
R MAX is the right callout for an inside corner where a mating part with a sharp or chamfered edge must seat: the shop can use any cutter up to that radius, and a smaller one is never a defect. It is the wrong callout for a fatigue shoulder, because it allows a sharp corner. There, R MIN is the safer limit, or a toleranced R or CR if the mating part also needs clearance.
A general note is the efficient way to cover the many internal corners on a milled part, for example “inside corners R MAX unless otherwise specified” with a value chosen for the mating parts. It tells the shop how large a cutter it may use without dimensioning every corner.
What are the most common radius callout mistakes?
Double-dimensioning a full radius, using R MAX where a minimum matters, specifying CR without saying how it is inspected, and leaving tangency unstated on partial rounds.
- A value on a full radius. A slot dimensioned by width and also by an end radius has two dimensions for one size. Remove the value, or remove the width.
- MAX on a stress radius. R MAX on a shaft shoulder permits a sharp undercut. Use a MIN limit or a toleranced radius.
- CR everywhere. Applying CR to every edge round adds inspection cost for no benefit. Keep it to the few curves where shape matters.
- Radius on a model only. A model-based definition with an untoleranced CAD fillet leaves the general profile or block tolerance in control; say which applies.
- No inspection method on tiny radii. Radii well under a millimeter are hard to gauge by hand. Agree whether an optical check is acceptable.
How should the RFQ state radii, and how are they checked on a Saola order?
Put every radius that matters on the drawing with its callout type and limits, flag any CR features, and say which inspection method you accept.
Parts are machined at our lead CNC plant in Vietnam on CNC milling and CNC turning. The plant’s inspection equipment includes a 2D optical (vision) measuring instrument, which suits checking radii and their tangency in profile, and a height gauge; there is no CMM, so a CR or profile callout that you expect to be scanned should be discussed at drawing review. New parts get a first-article inspection report and every lot a dimensional inspection record. Send the drawing for a quote.
Frequently asked
Is “R FULL” still a valid callout?
Current ASME practice shows a full radius as R with no value; FULL is not needed. Shops still understand it on older drawings, but on a new drawing use the plain R and let the width set the size.
What does SR mean on a drawing?
SR is a spherical radius, used for a ball end or a domed face. It follows the same tolerance logic as R, applied to a sphere rather than a cylinder or arc.
Can a turned part have a controlled radius?
Yes. A turned shoulder with a CR is cut with a form tool or a programmed arc, and the curve is then checked in profile, typically on an optical or vision system. Say on the drawing whether a tool-change blend or a small step is acceptable.
What is the default radius if none is given?
There is none in the dimensioning standard. Without a callout or a general edge note, the machinist will use whatever the tool leaves, so cover undimensioned edges and inside corners with a general note.
Sources
- Evaluation of radii in machined components, A. Szczepański and M. Magdziak, euspen 26th International Conference & Exhibition, Krakow, June 2026
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018