The Drawing Is the Contract

When a part comes back wrong, the argument is always the same. You say it is obviously not what you wanted. The shop says they built exactly what the drawing specified, and the shop is usually right: a machinist is obligated to make what is dimensioned and free to do anything reasonable with what is not.

A 3D model is geometry. A drawing is a commercial document stating which of that geometry matters, how much variation is acceptable, and what the part is made of. Sending a STEP file with "make this" attached hands every judgment call to someone who has never seen your assembly. The file-format side of that decision is covered in STL vs STEP, but the file never replaces the drawing.

Views and Dimensions: Enough, Not Everything

Show the minimum set of views that fully describes the part: front, top, right, plus a section through anything internal and a detail for small features. Add an isometric in a corner; it takes thirty seconds and prevents a whole category of misreading. Mark the projection convention explicitly. US practice is third-angle, much of Asia and Europe uses first-angle, and a drawing read in the wrong convention produces a mirrored part.

On dimensioning, the rule that separates a usable drawing from a bad one: dimension what is functionally critical, and let the model define the rest. Over-dimensioning is worse than under-dimensioning because it creates conflicting requirements the shop cannot satisfy simultaneously.

  • Dimension from datum faces, not chained feature to feature. Chained dimensions accumulate error across the part, which is exactly the problem examined in tolerance stack-up analysis.
  • Never double-dimension the same feature. If overall length is 4.000 in and two segments are 1.500 and 2.500, one of the three is redundant. Mark it as reference in parentheses.
  • Dimension mating features explicitly: bore diameters, bolt patterns, mounting hole positions, sealing surfaces, and anything that touches another part.
  • Give hole callouts fully: diameter, depth, thread specification with class, counterbore or countersink, and quantity. "4X 1/4-20 UNC-2B THRU" answers every question at once.
  • Note where dimensions apply to a coated or plated part, since finishes add thickness.

Tolerances: A Default Block Plus Deliberate Exceptions

Every drawing needs a general tolerance block, because otherwise the shop invents one. A conventional US block reads: two-place decimals plus or minus 0.010 in, three-place plus or minus 0.005 in, four-place plus or minus 0.0005 in, angles plus or minus 0.5 degrees, unless otherwise specified.

Then override individually where function demands it, and only there. This is the largest cost lever on the whole document. Tightening a bore from plus or minus 0.005 to plus or minus 0.001 can add 30 to 50 percent to the price of a machined part because it forces a finishing pass, in-process gauging, and a higher scrap rate. A drawing with every dimension at plus or minus 0.001 signals an inexperienced designer and gets quoted defensively high.

Two habits help. Write the tolerance you can justify from the fit, not the one that feels safe. And use asymmetric tolerances where the function is one-sided: a clearance hole that must never be undersized is better as plus 0.010 minus 0.000 than as a symmetric band.

GD&T Where Plus-or-Minus Cannot Say It

Linear tolerances cannot express "this face must be flat," "this bore must be perpendicular to that surface," or "this pattern must be located as a group." Geometric dimensioning and tolerancing, per ASME Y14.5, exists for exactly those statements, and used sparingly it both clarifies intent and widens the manufacturing window through bonus tolerance at maximum material condition.

Start with a defined datum reference frame chosen to match how the part is located in the assembly and, ideally, how it is held in the fixture. Then apply position tolerance to hole patterns, perpendicularity or parallelism to mating faces, flatness to sealing surfaces, and profile where a contour matters. Do not sprinkle symbols decoratively; a misapplied feature control frame is worse than none, because it is unambiguous and wrong. The working introduction is in GD&T basics.

The Lines Everyone Forgets: Material, Finish, and Treatment

These belong in the notes block and they are omitted more often than any dimension.

  • Material, fully specified. Not "aluminum" but "6061-T6 per ASTM B221." Not "stainless" but "304 or 316" with the condition. Alloy and temper change strength, machinability, and corrosion behavior.
  • Surface finish. A default such as 125 microinch Ra with tighter callouts on sealing or sliding surfaces. Without it you get whatever the tool left.
  • Coating or plating. Type, thickness, color, and standard: "Type II clear anodize per MIL-A-8625" is a specification; "anodized" is a wish. Cost implications are in anodizing aluminum.
  • Heat treatment with the target hardness range and the sequence relative to machining.
  • Edge condition. "Break all sharp edges 0.010 to 0.020 in" prevents both injuries and a callback.
  • Marking. Part number and revision on the part, with location and method, if traceability matters.
  • Cosmetic requirements. If a face is visible in the product, say so and define the acceptance criteria; otherwise a witness mark is fair game.

The Title Block

The title block is the part's identity card and it settles disputes. It must carry the part number, the part name, the revision letter, the units of measurement, the scale, the projection symbol, the drawing sheet number, the material, the general tolerance block, the approving engineer, and the company name. Revision control is the piece startups skip: without a revision letter that increments through a controlled engineering change order, a shop will happily build to the version they were emailed four weeks ago, and neither of you will be able to prove which was current.

The Drawing Is Part of a Package

Before sending, assemble the rest of what a shop needs to quote without a single question: the STEP file, the drawing as PDF, the quantity and whether it is a one-off or a first article for a repeating order, the required delivery date, any inspection requirements, and the assembly context so the shop understands what the part mates to. Requesting a first article inspection report against the ballooned drawing turns your tolerances from aspirations into something measured and signed.

For a full product, the drawing sits inside a larger deliverable carrying the bill of materials, assembly instructions, and test specs, described in the manufacturing data package. The cheapest final check: hand the drawing to an engineer who has not seen the project and ask them to describe the part. Every question they ask is a hole a shop would have filled with a guess.

Getting Drawings a Shop Can Quote

Projects House produces production drawing packages for US clients: datum schemes, justified tolerances, GD&T only where it earns its place, complete material and finish callouts, and revision control that survives contact with a factory. Send your CAD and target process through our contact form.