Technical Drawing Symbols and Abbreviations: What 38 Marks Mean
6 August 2026
Mentor CNC Editorial Team
You have a drawing in front of you and there is a symbol on it you do not recognize. This page is for exactly that. 38 sembol, each with three things: what it is, what it means, and what it means for you at the machine. Type the name of the symbol, or any word you remember, into the search box.
Geometrical Tolerances (GD&T)
These state how far the geometry of a part may deviate. To ISO 1101:2017 (TS 1304). There are fourteen basic symbols in all.
Straightness —
Form / no datum
How much an edge or an axis may bow. If Ø precedes the tolerance value the zone becomes a cylinder.
At the machine: This decides whether a long shaft needs center or steady support when turned.
Flatness ⏥
Form / no datum
The surface must lie between two parallel planes separated by the tolerance value.
At the machine: Critical on clamping and sealing faces. On a milled face it puts the table run-out in question.
Roundness / Circularity ○
Form / no datum
The cross-section must be a true circle. Each section is assessed separately.
At the machine: Chuck centering error and chatter on the lathe show up directly here.
Cylindricity ⌭
Form / no datum
Roundness + straightness + taper all at once. The whole cylinder must lie between two coaxial cylinders.
At the machine: The hardest form tolerance to hold; it may require grinding.
Profile of a line ⌒
Profile / datum optional
Deviation of a curve in one section from the theoretical profile.
At the machine: On die and cam profiles it sets the CAM tolerance setting.
Profile of a surface ⌓
Profile / datum optional
Deviation of a whole surface from the theoretical surface. Used on free-form surfaces.
At the machine: In 3D die machining it is the upper limit for the high-speed tolerance setting.
Parallelism ∥
Orientation / datum required
Parallelism of a surface or axis relative to the datum.
At the machine: The part should be located on whichever face is the datum — this drives the setup order.
Perpendicularity ⊥
Orientation / datum required
A surface or axis must be at 90° to the datum.
At the machine: Squareness of a bore axis to a face; it puts the vise and fixture squareness in question.
Angularity ∠
Orientation / datum required
Being at a stated angle other than 90° to the datum.
At the machine: On angled faces it indicates the need for a sine table or a fourth axis.
Position ⊕
Location / datum required
Deviation of a hole or feature from its theoretical position. Usually given as a cylindrical zone with Ø.
At the machine: The most common symbol on a hole pattern. Ø0,1 A B C sets the X-Y positioning accuracy.
Concentricity / Coaxiality ◎
Location / datum required
Two diameters sharing the same axis.
At the machine: On stepped shafts it calls for machining in a single setting.
Symmetry ≡
Location / datum required
A feature must be symmetrical about the datum plane.
At the machine: Used to center keyways and slots.
Circular run-out ↗
Run-out / datum required
The total deviation shown by a dial gauge in one section as the part is rotated about the datum axis.
At the machine: Directly measurable — set a dial gauge against it and turn the part. The most practical shop-floor check.
Total run-out ↗↗
Run-out / datum required
The total deviation seen as the gauge is traversed along the surface. It covers the whole surface.
At the machine: The stricter form of run-out; it limits wobble and taper or bow together.
Tolerance Frame Modifiers
Symbols added next to the value or the datum in a tolerance frame that change its meaning.
MMC — Maximum Material Condition Ⓜ
Modifier
The tolerance applies when the part contains the most material (hole at its smallest, shaft at its largest). As the part departs from that condition, bonus tolerance is gained.
At the machine: It exists to guarantee assembly. With Ⓜ the feature can be checked with a functional gauge, and bonus tolerance equal to the size tolerance becomes available.
LMC — Least Material Condition Ⓛ
Modifier
The tolerance applies when the part contains the least material.
At the machine: Used where wall thickness and edge distance must be maintained.
TED / Basic Dimension 30 (in a box)
Modifier
A boxed dimension carries no tolerance of its own — its deviation is given by the position tolerance.
At the machine: General tolerances such as ±0,1 do NOT apply to a boxed dimension. This is a frequent misreading.
Ø in tolerance zone Ø0,1
Modifier
A Ø in front of the tolerance value states that the zone is a cylinder, not a square.
At the machine: Ø0,1 and a ±0,05 square zone are not the same; at the corners of the square zone the deviation can reach 0,071 mm, while a Ø0,1 cylindrical zone limits it to 0,05 mm in every direction. The cylindrical zone that covers the corners of a ±0,05 square is Ø0,14; it gives 41% more tolerance along X and Y and 57% more area.
Surface Texture Symbols
These state how smooth a surface must be and how that is to be achieved. Textbooks cite ISO 1302; that standard was withdrawn in December 2021 and replaced by ISO 21920-1:2021. Most drawings in circulation still use the older notation.
Basic symbol √
Basic
Two arms at 60° to the surface, the short arm half the length of the long one — at least 3 mm and 6 mm. It has no meaning on its own.
At the machine: If you see it alone the drawing is incomplete — a value or an additional symbol must follow.
Material removal required √ (bar added)
Basic
A bar closes the top. Machining — turning, milling, grinding, drilling — is mandatory.
At the machine: This surface is your job. It may not be left as raw stock.
Material removal prohibited √ (circle added)
Basic
A circle closes the top. The surface stays as cast or rolled and must not be machined.
At the machine: Put a tool on this face and you scrap the part. It is not used as a clamping reference either.
All surfaces √ + circle
Basic
A circle added to the symbol means every surface of the part is to be finished to that value.
At the machine: One symbol covers the whole part; you do not have to look for a mark on every face.
Parallel =
Lay direction
The lay is parallel to the projection plane of the view carrying the symbol.
At the machine: Longitudinal on the lathe, single-direction passes on the mill.
Perpendicular ⊥
Lay direction
The lay is perpendicular to the projection plane.
At the machine: Facing on the lathe, or transverse passes.
Crossed X
Lay direction
The lay crosses in two oblique directions.
At the machine: The honing and cross-grinding pattern. Required on cylinder bores that must retain oil.
Multidirectional M
Lay direction
The lay has no particular direction.
At the machine: Processes such as abrasive finishing, polishing and blasting.
Circular C
Lay direction
The lay is approximately circular about the center of the surface.
At the machine: Face milling or circular grinding pattern.
Radial R
Lay direction
The lay radiates outward from the center of the surface.
At the machine: Face machining that sweeps outward from the center.
Dimensioning Symbols
Placed before or beside a dimension figure to state what the dimension describes.
Diameter Ø
Dimension
The diameter of a circular feature. Ø20 means 20 mm diameter.
At the machine: On a lathe the X axis usually works in diameter values — do not confuse it with radius.
Radius R
Dimension
The radius of an arc or corner fillet. R3 means a 3 mm radius.
At the machine: An internal corner radius sets the largest tool you can use: tool radius must be ≤ R.
Sphere SØ / SR
Dimension
The diameter (SØ) or radius (SR) of a spherical surface.
At the machine: A spherical surface usually needs a ball-nose tool and a 3D toolpath.
Square □
Dimension
States that the section is square. □20 means a 20×20 square section.
At the machine: One dimension describes both sides, so no second view is needed.
Chamfer 2x45°
Dimension
Edge break. At 45° it is written on one line as depth × angle. At other angles the depth and angle are dimensioned separately.
At the machine: Used directly in a lathe chamfer cycle; a C2 chamfer means 2×45°.
Slope ▱
Dimension
The slope of a surface relative to the horizontal, given as a ratio such as 1:10.
At the machine: Found on keys and guideways; you have to convert it into an angle.
Taper ◁
Dimension
The ratio of a conical surface, calculated as (D−d)/L.
At the machine: Critical on Morse tapers and taper fits. The angle for the lathe taper cycle comes from here.
Arc length ⌒
Dimension
States that the dimension follows the arc, not the chord.
At the machine: Confusing chord and arc length creates errors in a contour program.
First angle projection ⊏⊙
Projection
The view from the left is drawn on the right. Standard in Europe and Türkiye.
At the machine: Do not start interpreting views before you find this symbol in the title block — confuse it with third angle and you machine the part mirrored.
Third angle projection ⊙⊐
Projection
The view from the left is drawn on the left. Standard in the USA and Japan.
At the machine: Common on drawings from the USA and the Far East. The symbol is in the title block.
Ra Values and N Surface Grades
The N grade numbers came from ISO 1302:1978 and were formally withdrawn with ISO 21920 — but they still appear on older drawings and in machine catalogs. 1 µm = 0,001 mm.
