MAKENEXAForm - 4 characteristics
Straightness, flatness, circularity and cylindricity constrain a feature against its own perfect counterpart. They never reference a datum. If you see a datum letter in a form frame, the frame is wrong.
Engineering design resource
GD&T symbols chart
Twelve geometric characteristic symbols are in current use, in five categories. Form controls never take a datum, orientation and location and runout always do, and profile depends on how it is referenced. The chart is first on this page because that is what the question usually is.
- CAD nowSTEP or native model under one revision
- DrawingCritical dimensions, finish and notes
- QuantityFirst order and any repeat context
- MaterialGrade, condition or open alternatives
- TimingTarget date or priority window
Ready to quote this part?Upload CAD for a reviewed quote across MakeNexa’s supplier network.
Get a QuoteFeature control frame
GD&T symbols chart: all 12 geometric characteristics under ASME Y14.5-2018
ASME Y14.5-2009 carried 14 geometric characteristic symbols. The 2018 edition withdrew two of them and carries 12: four form, two profile, three orientation, one location and two runout. Both withdrawn symbols are listed below rather than dropped, because ISO 1101 still carries them, drawings in circulation still use them, and the replacement matters more than the removal. Form controls never reference a datum; orientation, location and runout always reference at least one. Six of these characteristics have a Unicode codepoint assigned to them by name; the rest borrow a technical glyph.
| Symbol | What it controls | Category | Datum | Status in ASME Y14.5-2018 | Status in ISO 1101 |
|---|---|---|---|---|---|
| ⏤ Straightness | How far a line element or an axis may depart from a straight line | Form | No | In use | In use |
| ⏥ Flatness | How far a surface may depart from a single plane | Form | No | In use | In use |
| ○ Circularity | How far one cross-section may depart from a perfect circle | Form | No | In use | In use |
| ⌭ Cylindricity | How far a whole cylindrical surface may depart from a perfect cylinder | Form | No | In use | In use |
| ⌒ Profile of a line | Deviation of a cross-sectional outline from its true profile | Profile | Conditional | In use | In use |
| ⌓ Profile of a surface | Deviation of a whole surface from its true profile | Profile | Conditional | In use | In use |
| ∠ Angularity | Orientation of a feature at a specified angle to a datum | Orientation | Yes | In use | In use |
| ⟂ Perpendicularity | Orientation of a feature at 90 degrees to a datum | Orientation | Yes | In use | In use |
| ∥ Parallelism | Orientation of a feature parallel to a datum | Orientation | Yes | In use | In use |
| ⌖ Position | Location of an axis, centre plane or centre point against basic dimensions and datums | Location | Yes | In use | In use |
| ↗ Circular runout | Variation of one rotating cross-section relative to a datum axis | Runout | Yes | In use | In use |
| ⌰ Total runout | Variation of a whole rotating surface relative to a datum axis | Runout | Yes | In use | In use |
| ◎ Concentricity | Opposing median points of a feature relative to a datum axis | Location | Yes | Withdrawn in 2018 - use position for axis-to-axis location, or runout on a rotating feature | In use |
| ⌯ Symmetry | Opposing median points of a feature relative to a datum centre plane | Location | Yes | Withdrawn in 2018 - use position applied to the centre plane | In use |
Concentricity and symmetry were withdrawn from ASME Y14.5 because they controlled opposing median points rather than an axis or centre plane. That is rarely the functional requirement, it is routinely confused with what position already controls, and verifying it takes extensive CMM work. Both remain active in ISO 1101, so a drawing produced to ISO can legitimately carry either one and is not out of date. If either appears on a drawing you are quoting, check which standard the drawing cites before assuming a replacement, then ask what the feature actually has to do.
Use this guide
Read a feature control frame in three parts
A feature control frame reads left to right in three parts: the geometric characteristic symbol, the tolerance value with any material condition modifier, and the datum references in order of precedence. The symbol names what is controlled, the value says how much departure is allowed, and the datum letters say what the feature is measured against. A frame with no datum letters is controlling the feature against itself, which is only valid for the form characteristics.
Datum order is not decorative. The primary datum constrains the most degrees of freedom, the secondary constrains what remains, and the tertiary fixes the rest. Reordering the letters describes a different fixture and a different measurement, so a frame that names the same three datums in a different sequence is a different requirement. MakeNexa reviews the datum scheme against the drawing and the model before quoting.
Design priorities
What each category controls
Five categories, twelve characteristics in current use. The category decides whether a datum is required, so identifying it is usually the fastest way to check a frame.
Profile - 2 characteristics
Profile of a line and profile of a surface control deviation from a true profile defined by basic dimensions. Referenced to datums they control form and location together; used with no datum they control form alone. This is the only conditional case.
Orientation - 3 characteristics
Angularity, perpendicularity and parallelism control the angle a feature holds to a datum. Perpendicularity is the 90 degree case and parallelism the zero degree case; angularity covers every other specified angle. All three require at least one datum.
Location - 1 characteristic
Position locates an axis, centre plane or centre point against basic dimensions and datums. It is the most used control in the system, and it absorbed both characteristics the 2018 edition withdrew. A cylindrical zone stated as 0.25 mm diameter covers about 57 percent more area than a square zone of the same across-flats size, which is why position is written with a diameter symbol for round features.
Runout - 2 characteristics
Circular runout checks one rotating cross-section against a datum axis; total runout checks the whole rotating surface. Both require a datum axis, and both are measured with the part turning rather than static.
Common review gaps
Where a feature control frame gets misread
Most quoting delays on a GD&T drawing come from four recurring ambiguities rather than from tight tolerances.
A chart drawn from the wrong edition
Many symbol charts still in circulation show 14 characteristics with no note that 2 of them were withdrawn. A drawing carrying one of those two is not automatically out of date - it may be drawn to ISO, where both remain active. Check the standard the drawing cites before assuming a replacement.
Datum letters in a form frame
A flatness or circularity frame with a datum reference cannot be measured as written, because a form control has no external reference by definition. It usually means orientation or profile was intended.
Datums named but not identified on the part
A frame can reference datum A, B and C while the drawing never attaches those letters to actual features. The control is then unmeasurable and the fixture cannot be designed from the drawing alone.
A tolerance tighter than the function needs
Position at 0.05 mm on a clearance hole that would function at 0.25 mm adds CMM time without changing whether the bolt fits. Cylindricity at 0.01 mm on a feature that only has to slide is the same mistake. State what the feature has to do and the review can suggest the control and the value that gets there.
Practical choices
Choose the control that matches the function
Several characteristics can constrain the same feature. The one to specify is the one that describes what the part actually has to do.
The feature has to assemble
Position against a datum reference frame, with basic dimensions, is normally the right control for holes, slots and bosses that mate. It is the control most shops are set up to inspect. Applied at maximum material condition it also releases a bonus tolerance as the hole grows: a 6.0 mm hole toleranced to 6.2 mm carries 0.2 mm of extra positional freedom at its largest size.
The feature has to seal or seat
Flatness or profile of a surface controls the condition the seal or seat depends on. Flatness of 0.05 mm across a 100 mm face is a common gasket requirement. Add surface texture separately - a face held flat to 0.05 mm can still be Ra 6.3 and leak, because flatness and roughness are different requirements and one does not imply the other.
The feature has to rotate
Circular or total runout against the datum axis states the requirement directly and is measured with the part spinning. Total runout of 0.02 mm on a bearing journal is a routine callout, and it is usually cheaper to verify than an equivalent stack of form and orientation controls.
Design decision table
Datum requirement by category
The fastest check on any feature control frame: find the category, then confirm the datum references match what the category allows.
| Category | Characteristics | Datum reference and what it measures against |
|---|---|---|
| Form | Straightness, flatness, circularity, cylindricity | Never. The feature is measured against its own perfect counterpart, so a datum letter in a form frame is an error |
| Profile | Profile of a line, profile of a surface | Conditional. Referenced to datums it controls form and location together; with no datum it controls form alone |
| Orientation | Angularity, perpendicularity, parallelism | Always at least one. The feature is measured at its specified angle to that datum |
| Location | Position | Always. The axis, centre plane or centre point is measured against basic dimensions from a datum reference frame |
| Runout | Circular runout, total runout | Always a datum axis. The surface is measured with the part rotating rather than static |
Turn the guide into an RFQ
Before sending a GD&T drawing for quote
Open the drawing beside the model and confirm each geometric control can be measured as written.
Complete packages move faster: revision-matched CAD, critical dimensions, quantity and material notes are enough to open engineering review across the network.
Get a Quote- 01
Every datum letter referenced in a frame is attached to a real feature on the drawing
- 02
Datum precedence order matches the way the part is located in its assembly
- 03
No form control carries a datum reference
- 04
Basic dimensions are present wherever position or profile is used, and general block tolerances such as plus or minus 0.13 mm do not silently apply to them
- 05
Material condition modifiers are intentional, not carried over from a template
- 06
The drawing states which geometric tolerancing standard and edition it was drawn to
- 07
Critical characteristics that need documented inspection are marked as such
Questions before routing
Questions when applying this guide
These answers prepare the request; the reviewed quote controls project-specific commitments.
How many GD&T symbols are there, and did any change recently?
ASME Y14.5-2009 defined 14 geometric characteristic symbols. ASME Y14.5-2018 withdrew concentricity and symmetry, leaving 12: straightness, flatness, circularity and cylindricity for form; profile of a line and profile of a surface; angularity, perpendicularity and parallelism for orientation; position for location; and circular and total runout. Many symbol charts still published online show all 14 without noting that two are no longer supported, so check which edition a chart is drawn from before relying on it.
Which GD&T controls need a datum reference?
Form controls never take a datum, because they constrain a feature against itself: straightness, flatness, circularity and cylindricity. Orientation, location and runout always take at least one datum, because they constrain a feature against something else: angularity, perpendicularity, parallelism, position, circular runout and total runout. Profile is the conditional case. Referenced to datums it controls both form and location; used without them it controls form alone.
What do the parts of a feature control frame mean?
The frame reads in three parts. First the geometric characteristic symbol, which names what is controlled. Then the tolerance value, optionally with a diameter symbol for a cylindrical tolerance zone and a material condition modifier. Then the datum references, listed in order of precedence: primary, secondary, tertiary. Changing the order of the datum letters changes the requirement, because it changes which datum constrains the part first.
Does a GD&T callout replace a plus-minus tolerance?
Not always. Size is still controlled by a plus-minus tolerance or a limit dimension; the geometric control constrains form, orientation, location or runout on top of that size. Position and profile use basic dimensions, which carry no tolerance of their own - the tolerance lives in the feature control frame instead. A drawing normally carries both kinds of control, and the two answer different questions.
Do I need GD&T on every drawing?
No. Block tolerances are enough for features whose fit is not critical, and adding geometric controls to everything raises inspection cost without improving the part. Apply geometric tolerancing where a functional interface depends on it - mating holes, seating faces, rotating features, sealing surfaces - and let the default tolerance block cover the rest.
Can MakeNexa quote a part with tight geometric tolerances?
Yes. Precision-class work to plus or minus 0.025 mm and ground work to plus or minus 0.005 mm is routed routinely across the supplier network, and suppliers holding ISO 9001, ISO 13485, AS9100 and IATF 16949 certification are part of it. Whether a specific geometric tolerance is achievable on a specific feature, in a specific material and section, with a specific measurement method, is confirmed on the reviewed quote rather than assumed from the callout.
Next step
Send the package and get a reviewed quote
Apply the guide to a real drawing and RFQ package. MakeNexa routes capable suppliers from a global network covering competitor-class process categories, then returns a prepared quote or focused clarification for your revision.