Guide
Profile of a surface vs profile of a line: which should a machined contour get?
Profile of a surface is the GD&T control that puts one three-dimensional tolerance zone around the whole true surface, so every point of the machined surface must lie inside it, while profile of a line puts a two-dimensional zone around each cross-section separately. Use profile of a surface when the contour as a whole has to fit, seal or mate, and profile of a line when only the shape of each section matters and the length direction is controlled some other way.
By Saola Manufacturing engineering team · Published · Updated
Profile callouts are the most flexible tools in ASME Y14.5 and ISO 1101, and also the ones most often written by habit. A designer picks the arc symbol the CAD template offers, leaves the datum boxes empty, and the supplier has to guess whether the contour may float, whether the zone is meant to be equal on both sides, and whether a cam lobe is inspected as a whole surface or one slice at a time. This guide is for the engineer who draws the part and the buyer who sends it out for machining. It covers what each symbol controls, what datums add, how the zone can be shifted to one side, what the all-around and between symbols do, how a CMM reports each control, and a decision table you can use on the next drawing. Castings have their own considerations, covered in the casting profile guide; this page stays on machined contours.
On this page
What is the difference between profile of a line and profile of a surface?
Profile of a line controls each cross-section of a feature as an independent two-dimensional curve, while profile of a surface controls the entire surface at once inside a single three-dimensional zone. A surface can pass profile of a line in every section and still be twisted or bowed along its length, which profile of a surface would reject.
Both controls start from the same idea: a true profile, the exact nominal shape, defined by basic dimensions on the drawing or by the CAD model, and a uniform boundary on either side of it. In ASME Y14.5-2018 the profile of a line symbol is an open arc and the profile of a surface symbol is the same arc closed with a straight base line. ISO 1101:2017 uses the same two symbols and calls them line profile and surface profile, and ISO 1660:2017 sets out the detailed rules for both.
The difference is in where the zone lives. For profile of a line, the inspector takes cross-sections in the direction the drawing view shows, and each section has its own pair of boundary curves. Nothing ties one section to the next, so the sections can shift or rotate relative to each other unless datums or other tolerances stop them. For profile of a surface, the two boundaries are offset surfaces that wrap the whole feature, so form, twist along the length and, with datums, location are all judged together. That is why profile of a line almost never appears alone: it is usually paired with a size tolerance, a profile of a surface, or a straightness or parallelism control that governs the direction the sections do not.
Does a profile tolerance control form only, or location as well?
Without datum references, a profile tolerance controls only form, and for a closed or irregular feature its size, so the zone may float and rotate to fit the part. With datum references, the zone is fixed to the datum reference frame, and the same callout controls form, orientation, location and size together.
This is what makes profile one of the most versatile controls in GD&T, and also one of the easiest to misuse. A profile of a surface with no datums on a flat face acts like a flatness callout, because the zone is two parallel planes allowed to settle wherever the surface is. Add a single primary datum and the same zone must also stay parallel to that datum, and if a basic dimension ties the face to the datum, it is held at that distance as well. Add a full datum reference frame and the zone is locked in place by the basic dimensions that connect the contour to the datums, so the callout also does the job a position or a plus-and-minus location tolerance would do. The datum reference frame guide explains how to choose those datums.
A common refinement is to state two requirements in one frame. A composite or two-segment profile, per ASME Y14.5, can give a larger zone for location relative to the full datum frame and a tighter zone for form and orientation relative to fewer datums or none. That lets a cam lobe or pocket wall keep a precise shape without forcing the supplier to hold an equally precise location, which is usually not what the function needs. The 2018 edition also added a dynamic profile modifier, a small triangle after the tolerance value, which lets the form refinement apply while the feature size is controlled separately.
| Callout | Zone shape | What it controls |
|---|---|---|
| Profile of a line, no datums | Two curves around each cross-section, free to float section by section | Form of each section only |
| Profile of a line, with datums | Two curves per section, fixed to the datum frame | Form, orientation and location of each section; not twist between sections unless constrained |
| Profile of a surface, no datums | Two offset surfaces, free to float as one body | Form of the whole surface, plus size of a closed feature |
| Profile of a surface, primary datum only | Two offset surfaces, orientation fixed | Form and orientation, plus location from that datum where a basic dimension ties the surface to it |
| Profile of a surface, full datum frame | Two offset surfaces, fully located by basic dimensions | Form, orientation, location and size |
| Composite profile of a surface | Larger located zone plus smaller floating or oriented zone | Location loosely, form and orientation tightly |
How do bilateral, unilateral and U-modifier profile zones work?
By default the profile zone is bilateral and split equally on both sides of the true profile. The circled U modifier in ASME, or the UZ modifier in ISO, shifts the zone so that more of it, or all of it, sits on one side.
An equal bilateral zone suits most machined contours, because the cutter can drift either way and the function does not care which. Per ASME Y14.5, the value after the circled U is the portion of the total zone that lies in the direction that adds material; the rest lies inside the material. A U value equal to the full tolerance puts the whole zone outside the true profile, and a U value of zero puts it all inside. ISO 1101 reaches the same result differently: the UZ modifier is followed by a signed offset of the zone's center from the true profile, with a positive sign meaning toward the outside of the material, so the frame looks different even when the intent is identical.
Choose a unilateral zone when the function only fails in one direction. A clearance pocket that receives a mating boss can grow but must not shrink, so its zone should sit on the side that removes material from the wall. A blended outer surface that must leave stock for a later grinding operation should sit on the side that adds material, so no point of the surface ends up below the finished shape. Older drawings show the unequal zone with a phantom line and a short tolerance segment drawn on one side of the profile; that method still reads correctly, but the U modifier is clearer for a supplier reading a translated or scanned print. For the plus-and-minus equivalent of the same idea, see the unilateral vs bilateral tolerance guide.
| Feature control frame value | Zone outside the material | Zone inside the material | ISO 1101 notation |
|---|---|---|---|
| 0.4 (no modifier) | 0.2 mm | 0.2 mm | 0.4 |
| 0.4 U 0.1 | 0.1 mm | 0.3 mm | 0.4 UZ−0.1 |
| 0.4 U 0.4 | 0.4 mm | 0 mm | 0.4 UZ+0.2 |
| 0.4 U 0 | 0 mm | 0.4 mm | 0.4 UZ−0.2 |
What do the all-around, all-over and between symbols do on a profile callout?
The all-around symbol, a small circle at the leader bend, extends the profile callout to every surface around the outline shown in that view. The between symbol, a double-headed arrow between two lettered points, limits the callout to the stretch of the contour from one point to the other.
Without one of these, a profile callout applies only to the single surface the leader touches, and a supplier reading the drawing literally will treat every other face of the contour as uncontrolled. All-around is the usual choice for the perimeter of a milled pocket or the outside of a plate cut to a nominal shape. Note that it covers the outline in the view, not every surface on the part: the floor and the top face of a pocket are not included. ASME Y14.5 also provides an all-over symbol, two concentric circles at the leader bend, which applies the callout to every surface of the part; it suits a fully modeled part where the CAD model is the definition and one general profile replaces many local tolerances.
The between symbol is the right tool when a contour changes function partway around. A cam might need a tight zone across the lift section and a looser one on the base circle, which is written as two callouts, each limited by its own pair of letters. Make sure the lettered points are clearly placed at tangency or transition points the inspector can find on the part, because a point that floats on a smooth blend leaves the extent of the tolerance open to argument. ISO 1101:2017 has its own all-around and all-over indicators and its own way of limiting a tolerance to part of a feature, and the notation differs in detail, so a drawing should say which standard it follows.
Should a machined contour get profile of a line or profile of a surface?
Use profile of a surface for any contour where the whole surface has to mate, seal, clear or locate, which covers most machined contours. Use profile of a line only for constant-section features, or for sections whose shape matters while the length direction is governed by another tolerance.
The test is to ask what happens if the part passes every individual section but the sections do not line up. If that part would still assemble and work, profile of a line is enough. If it would leak, bind or sit crooked, the drawing needs profile of a surface, possibly with profile of a line added as a tighter refinement on the sections that matter most. The table below applies that test to the contours that show up most often on drawings sent for machining.
| Feature | Recommended control | Datums | Why |
|---|---|---|---|
| Plate cam or cam lobe | Profile of a surface, often split with between symbols | Bore axis and a clocking feature | Follower contact runs across the full face width, and the lift has to be timed to the bore |
| Constant-section bar stock or extruded section, machined to length | Profile of a line for the section, plus straightness or twist control along the length | Often none for form; a datum face if the section must locate | The section shape matters, and the length direction is governed separately |
| Blended pocket wall or 3D-milled cavity | Profile of a surface, all around or all over | Full datum frame | The cavity has to receive a mating part at a known location |
| O-ring or gasket sealing face | Profile of a surface, or flatness if the face is planar | None for form; primary datum if it must also be parallel | A seal fails on waviness across the whole face, not on one section |
| Turned radius or ogive on a shaft | Profile of a surface (sections alone miss lobing) | Shaft axis and a shoulder | The form must be consistent around the axis and located along it |
| Airfoil, blade or guide vane section | Profile of a line at stated sections, inside an overall profile of a surface | Full datum frame for the surface; fewer for the section refinement | Section shape drives flow, the surface keeps sections aligned |
For milled contours, the zone the supplier can hold depends on the cutter path, the stepover on 3D surfaces and how the part is fixtured, which is why the profile value and its datum scheme should be on the drawing before the quote, not settled after first articles. The CNC milling page lists the machines and the part sizes run, and turned contours such as radii and ogives are covered on the CNC turning page.
How does a CMM inspect profile of a surface and profile of a line?
A CMM measures points on the contour, compares each point to the CAD nominal along the surface normal, and checks that every deviation falls inside the zone. With datums the part is aligned to the datum reference frame before comparison; without datums the software is allowed to best-fit the points to the nominal first.
That alignment step is where most profile disputes start. If the drawing calls datums but the inspection program best-fits the whole contour, the report will look better than the part, because best-fitting removes the location error the callout was written to catch. If the drawing has no datums and the program aligns to datums anyway, a good part can fail. A first-article report should therefore state which alignment was used. NIST publishes free CAD test models annotated with GD&T to the ASME Y14 standards, which are a useful public set for checking how CAD and inspection software carry tolerance callouts from the model.
For profile of a surface, the result is usually reported as the largest deviation on each side and as a profile value: for an equal bilateral zone, twice the largest absolute deviation, which must not exceed the tolerance. For a U-modified zone, the two sides have to be checked against their own limits, because a single profile number cannot show whether the error fell on the side with more room. For profile of a line, the program scans or probes the part at a series of section planes and evaluates each one on its own, so the report should list the section locations and a result per section. Point density matters for both: a sparse grid can miss a gouge or a step at a tool change, so dense scanning is the normal method on blended and cam surfaces. Without a CMM, a profile of a line can be checked with an optical comparator against an overlay chart, and a located profile of a surface with a dial indicator on a fixture that holds the datums, though both give less information than a full point cloud.
How should a profile callout be written on a drawing sent for an RFQ?
Give the true profile with basic dimensions or a referenced CAD model, state the datums the zone is tied to, add a U modifier if the zone is not centered, and mark its extent with all-around, all-over or between symbols. Send the STEP file with the PDF, because a supplier cannot inspect a profile against a shape it does not have.
When we review a drawing for quoting, profile callouts get the most questions. The usual gaps are a contour dimensioned with plus-and-minus values plus a profile frame, which gives two conflicting definitions of the same surface; a profile with no datums where the function clearly needs location; and a model referenced by name without a revision, so the nominal shape is uncertain. Each of these is cheap to fix on the drawing and expensive to argue about after parts ship. The basic dimensions guide covers how to make the true profile unambiguous.
In the RFQ, say which standard and edition the drawing follows, ASME Y14.5-2018 or ISO 1101:2017, because the modifiers and default rules differ. Name the profile callouts you consider critical, so they can be ballooned and reported individually on the first article, and say whether you need a CMM point report or a pass/fail summary is enough. When the drawing and model are ready, send them for a quote; our reply will list any profile callout we would read differently from you before machining starts.
Frequently asked
What is the difference between profile of a surface and flatness?
On a flat face with no datums, profile of a surface gives the same two-parallel-plane zone as flatness. The difference appears when datums are added: profile can then control orientation and location as well, while flatness only ever controls form. Use flatness when form is all that matters, because it is simpler to read and inspect.
Can profile of a surface be used without a datum?
Yes. Without datums it controls form, and size for a closed feature, and the zone may float to fit the part. That is correct for a sealing face or a form-only requirement, but wrong for a contour that has to sit at a known place relative to holes or mounting faces.
Does Rule #1 apply to profile tolerances?
Not in the usual sense. Rule #1 ties form to the limits of a size tolerance, while a profile-controlled feature is defined by basic dimensions and the profile zone itself sets the boundary. That is why plus-and-minus dimensions on a profiled contour are a conflict rather than a backup.
How do you calculate a profile of a surface result?
Measure the deviation of each point from the nominal along the surface normal, after the alignment the callout requires. For an equal bilateral zone, the reported profile value is twice the largest absolute deviation, and the part conforms when that value does not exceed the tolerance. For a U-modified zone, check each side against its own limit.
Is the circled U the same as ISO UZ?
They achieve the same result but are written differently. The ASME circled U is followed by the amount of zone on the material-adding side; the ISO UZ is followed by a signed offset of the zone's center. Converting a drawing between the two systems means recalculating the number, not just swapping the symbol.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018 (reaffirmed 2024)
- ISO 1101:2017, Geometrical product specifications (GPS) — Geometrical tolerancing — Tolerances of form, orientation, location and run-out, ISO, 2017 (confirmed 2022)
- ISO 1660:2017, Geometrical product specifications (GPS) — Geometrical tolerancing — Profile tolerancing, ISO, 2017 (confirmed 2022)
- Download Free CAD Models, STEP Files, and Test Results (MBE PMI Validation and Conformance Testing Project), NIST; project concluded 2015, simplified test cases 2023