The short answer
An engineering drawing defines a part for manufacture and inspection: geometry in orthographic views, plus the material, tolerances, finish, threads and notes a 3D model does not carry. To quote and build, a shop needs a complete title block (part number, revision, material, finish, units, general tolerances, projection angle), toleranced dimensions from datums, complete thread and hole callouts, and clear notes. Send it as a PDF with a matching STEP file.
What an engineering drawing is for
An engineering drawing is the controlled, dimensioned definition of a part or assembly: what it is made of, what size it has to be, how much each size may vary, how its surfaces must be finished and how it will be inspected. A 3D model shows the nominal shape. The drawing adds the requirements, and on many purchase orders it is the document the part is accepted against.
This guide covers the structure of a formal drawing, the conventions a shop reads it by, and the omissions that turn a quote into a list of questions. For a shorter, practical take on what to include when you are not producing formal drawings, see creating a shop drawing.
Two standards families govern most drawings. In North America, the ASME Y14 series: ASME Y14.5 for dimensioning and tolerancing, ASME Y14.3 for views, ASME Y14.100 for drawing practices. Elsewhere, ISO standards such as ISO 128 for presentation and ISO 1101 for geometric tolerancing. Shops read both, but a drawing should say which one it follows.
The title block: the fields a shop reads first
Before a machinist looks at a single dimension, an estimator reads the title block. It answers the questions that set the price and the process.
| Field | What to write | What happens if it is missing |
|---|---|---|
| Part number and title | A unique part number and a plain description | Parts get confused across revisions and reorders |
| Revision | A letter or number that matches the CAD file name | The shop cannot tell which file governs |
| Material | Alloy and temper or grade, for example 6061-T6 or 304 stainless, and a material spec if required | "Aluminum" gets quoted as the shop's default alloy, which may not be what you need |
| Finish | The process by specification, for example anodize per MIL-A-8625 Type II, Class 2, black | Finish is quoted as an assumption or left off entirely |
| Units | Inch or millimeter, stated once | Dimensions get misread by a factor of 25.4 |
| General tolerance block | Default tolerances for untoleranced dimensions, by decimal places or by ISO 2768 class | The shop applies its own default, or quotes tight to be safe |
| Projection symbol | First angle or third angle | Views can be read mirrored |
| Standard | ASME Y14.5-2018, ISO 1101 or similar | Ambiguity about how GD&T is interpreted |
| Scale and sheet | For example 1:2, sheet 1 of 3 | Missing sheets go unnoticed |
| Drawn and approved by, date | Names or initials and dates | Nobody knows who can answer a question or approve a change |
Quantity usually belongs on the RFQ or purchase order, not on the drawing, because the same drawing is reordered at different quantities.
Views and projection: first angle versus third angle
A drawing shows the part in orthographic views: front, top, side and so on, each looking straight at one face. The projection method decides where those views sit relative to each other.
- Third angle projection is standard in the United States and Canada (ASME Y14.3). The top view sits above the front view and the right side view sits to its right, as if you unfolded a glass box around the part.
- First angle projection is standard in much of Europe and Asia (ISO 5456-2 allows both, and many ISO users default to first angle). The top view sits below the front view and the right side view sits to its left.
The two layouts are mirror images of each other, which is exactly why the projection symbol, a truncated cone in two views, belongs in the title block. A part read in the wrong projection can be made with a feature on the wrong side.
Beyond the principal views, a good drawing adds:
- Section views to show internal features such as bores, counterbores and wall thickness
- Detail views at a larger scale for small features such as grooves, thread reliefs and fillets
- Auxiliary views looking square to an angled face, so features on it can be dimensioned true size
- An isometric view, not dimensioned, to help a reader understand the shape at a glance
Use the fewest views that fully define the part. Extra views add more places for dimensions to disagree.
Dimensions, tolerances and GD&T
Every dimension on a production drawing has a tolerance, either directly or from the general tolerance block. How you express it matters.
Dimension from datums, not from each other. Choose the surfaces that locate the part in its assembly as datums and dimension features from them. Chains of dimensions, each from the last feature, accumulate tolerance; see tolerance stack-up for how that adds up.
Do not double dimension. If a length is defined by three other dimensions, giving it again creates a conflict. Mark any repeated dimension as reference by putting it in parentheses, and reference dimensions are not inspected.
Tolerance only what matters, and tolerate the rest generally. Put explicit tolerances on fits, locating features and anything that controls function. Leave the rest to the general tolerance block. Typical machining capability by feature is in the CNC machining tolerance chart, and how to specify tolerances covers choosing them.
Use GD&T where plus/minus cannot say what you mean. Plus/minus dimensions control size well but location and orientation poorly. Geometric dimensioning and tolerancing controls form, orientation, location and runout relative to datums, using feature control frames. A hole pattern that has to line up with a mating part is the classic case for position tolerance. Basic dimensions, shown in a box, are theoretically exact values whose allowed variation comes from the feature control frame. The GD&T symbols reference lists all 14 characteristics.
Typical general tolerance block (inch drawings):
- X.X: plus or minus 0.030 in
- X.XX: plus or minus 0.010 in
- X.XXX: plus or minus 0.005 in
- Angles: plus or minus 0.5 degree
Metric drawings more often cite ISO 2768-m (medium) or ISO 2768-f (fine) for linear and angular dimensions, and ISO 2768-2 classes for general geometric tolerances.
Threads, holes and surface finish callouts
Some features are defined almost entirely by their callout, so the callout has to be complete.
Threads. A thread callout gives size, pitch or threads per inch, series, class and depth. Examples:
- 1/4-20 UNC-2B, 0.50 DEEP (internal thread, class 2B)
- M6 x 1.0-6H, 12 DEEP
- 1/8-27 NPT (tapered pipe thread)
Say whether a depth is full thread depth or drill depth; they differ. The thread callout guide shows the full format, and the tap drill chart covers the drill sizes.
Holes. Use hole callouts for drilled, reamed, counterbored and countersunk features: diameter and tolerance, depth, and the counterbore or countersink size and angle. A hole that has to take a dowel needs a reamed tolerance, not a drilled one.
Surface finish. Specify roughness, usually Ra in micrometers or microinches, with the surface texture symbol (ASME Y14.36 or ISO 21920-1). Set a general value in the notes, for example Ra 3.2 µm (125 µin) unless otherwise specified, and call out tighter values only on sealing faces, bearing bores and sliding surfaces. Typical Ra by process is in the surface roughness chart.
Edges. "Break sharp edges 0.2 to 0.5 mm" or "0.005 to 0.015 in" is a clear note. "Deburr" on its own is not, because it does not say how much.
Notes: the part of the drawing that most often causes a re-quote
General notes carry requirements that do not fit on a dimension: finish, heat treatment, marking, inspection, cleanliness. They are also where most quoting problems start. These are the notes shops most often have to come back about:
| Note as written | Why it causes a re-quote | Clearer version |
|---|---|---|
| Tolerance on all dimensions plus or minus 0.001 in | Every feature priced as precision work, often with CMM inspection | A normal general tolerance block, with tight tolerances only on the features that need them |
| Anodize black | No type, class or seal, so the shop has to guess between decorative and hard coat | Anodize per MIL-A-8625 Type II, Class 2, black, sealed |
| Heat treat to 40 HRC | No range, no specification, no point in the process | Heat treat to 38-42 HRC after machining, verify hardness on one sample per lot |
| Polish | No roughness value or surfaces listed | Ra 0.8 µm max on surfaces marked A |
| Model governs, or drawing governs, with no revision match | If the model and drawing disagree, nobody knows which is right | Drawing governs for tolerances; model rev C governs for untoleranced geometry |
| Match existing part | The shop has never seen the existing part | Dimensions and tolerances on the drawing, or a sample part sent with the RFQ |
| Material: steel | Hundreds of grades with very different cost and machinability | 1018 CRS, or 4140 pre-hardened 28-32 HRC |
| Inspect 100 percent | Inspection scope and report format undefined | Inspect dimensions marked with balloons; first article report per AS9102 if required |
Put certification requirements, such as material certs, a certificate of conformance or a first article report, in the notes or the RFQ. Added after the quote, they change the price.
Detail drawings versus assembly drawings
A detail drawing defines one part completely, everything needed to make and inspect it. Shops quote and build from detail drawings.
An assembly drawing shows how parts fit together. It identifies each component with a balloon, a numbered circle with a leader pointing at the part, and lists the components in a bill of materials (BOM) or parts list (ASME Y14.34 covers parts lists). A typical BOM has an item number that matches the balloon, a part number, a description, the material or source, and the quantity per assembly. Assembly drawings also carry assembly-level requirements: torque values, adhesive or sealant, orientation of parts, and overall dimensions that must be held after assembly.
For quoting, the distinction matters:
- Send a detail drawing for every part you want made. An assembly drawing alone does not give a shop the tolerances or finish of each part.
- Send the assembly drawing too when the shop is assembling, when it helps explain which features are functional, or when the part is a weldment. A weldment is drawn as an assembly of its cut pieces, with weld symbols, and it is manufactured as one item.
- Mark purchased parts in the BOM (screws, inserts, bearings) as purchased, with the manufacturer part number, so the shop knows whether to supply them.
Send STEP and PDF together
Most shops program from the 3D model and inspect against the drawing. Sending both, with matching revisions, gets the fastest and most accurate quote:
- STEP (or the native CAD file if the shop asks for it) for geometry, so the shop can program and estimate machine time without redrawing anything
- PDF drawing for the requirements the model does not carry: tolerances, finish, threads, material, notes and inspection
- The same revision on both, in the file names and in the title block
- A note on precedence, so the shop knows what governs when the two disagree
CAD files for quoting covers file formats in more detail. If you have only a model, a STEP is enough to quote simple parts at standard tolerances. As soon as a part has fits, threads, cosmetic faces or critical dimensions, add a drawing.
Upload both at openspindle.com/quote. The matched shop reviews the drawing as part of the quote and sends one price, usually in about 24 hours.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing
- ASME Y14.3, Orthographic and Pictorial Views
- ASME Y14.100, Engineering Drawing Practices
- ASME Y14.34, Associated Lists
- ISO 128, Technical product documentation: general principles of representation
- ISO 5456-2, Technical drawings: projection methods, orthographic representations
- ISO 2768-1 and ISO 2768-2, General tolerances
Last reviewed by Tom Petrini