technical-drawing

Technical drawings

Drawings are generated, not drawn by hand: a parametric build123d model (or a STEP file) is the single source of truth, scripts/drawlib.py derives the views from it (hidden-line removal, sections, hatching) and adds the annotations a workshop needs. Every save runs an automatic sheet check. The result is a vector PDF per sheet (optionally DXF/SVG) plus a PNG preview that you look at before you call anything finished.

Why this route: views can never disagree with the model, a changed parameter regenerates every sheet, and the same model gives STEP files and an interference check for free.

What a good drawing has to achieve

A drawing is a contract with the person who makes and inspects the part. Someone who has never seen the project must be able to manufacture it from the sheet alone. That decides everything below: dimension what the function needs, tolerate only what matters, and say how each functional surface has to look. A sheet with every edge dimensioned but no fits, roughness or geometrical tolerances is not manufacturable in the sense examiners and workshops mean.

Choose the route

• The user has a STEP file and wants a drawing quickly: run python scripts/step2drawing.py part.step [--section] [--lang en --projection third] [--units in] [--material ...] [--density ...] [--dxf]. It gives views, hidden lines, centre lines, overall dimensions, title block and the check. Then say clearly that functional dimensions, fits, tolerances and surface texture still have to be added - and offer to add them: auto_drawing() in the same module returns (sheet, views, issues) with out=None, so you can keep annotating the sheet in Python (--up y for Y-up exports).
• Anything that has to be manufactured from: model the part(s) and write the sheet in Python (workflow below). STEP input can still be the model: D.load_step(path).

Workflow

1. Clarify the function first. For each part ask: which surfaces mate with what, what must be coaxial/perpendicular/flat for the machine to work, which dimensions come from purchased parts (bearings, pins, screws). These become datums, fits and tolerances. If the user has a report, BOM or older drawing, read it and keep its numbers; mark every value you invent as your assumption and tell the user. Ask which language and projection method the drawing is for (default: German, first-angle; North America: English, third-angle) and whether there is a company title block.
2. Model the parts in one module, each part in its manufacturing position, all dimensions as named parameters. Turned parts: revolve a half-profile (x, r); prismatic parts: boxes minus bore solids, or extrude one profile (no fused seams). Model threads as core holes only. Put purchased/standard parts in as simple solids so the assembly and the interference check are complete.
3. Check the assembly before drawing: pairwise (a & b).volume over all parts; every overlap must be either zero or deliberate (thread engagement, press fit). Fix the model, not the drawing.
4. Write one function per sheet, copying the closest example in examples/: flanged_bush.py (turned part, the basic template), bearing_bracket.py (assembly, parts list), stepped_shaft.py (broken view, detail, removed section, thread), flange.py (half section, pitch circle, position tolerance), spur_gear.py (gear data table), weldment.py (weld symbols), milled_block.py (English, third-angle, company title block). Start with geometry only, render, look, then add annotations in layers: centre lines -> dimensions -> datums and tolerances -> surface texture -> notes, tables -> title block.
5. Render, read the check, look at every sheet. Sheet.save(pdf, png=...) prints the check report and writes <png>_check.png with each finding framed. Fix every error and warning (move the annotation, change offsets, tshift, tpos, knees of leaders). Then read the PNG yourself - the check finds collisions and inconsistencies, not a wrong dimensioning concept or an arrow pointing at the wrong edge. Crop dense regions to zoom. Never report a sheet as done that you have not seen.
6. Deliver: one PDF per sheet named by drawing number, a merged set (pypdf PdfWriter.append), DXF if the user edits in CAD, STEP per part and for the assembly (export_step). State plainly what is not drawn yet and which values are assumptions.

Setup once per machine: pip install -r requirements.txt. The ISO 3098 font osifont is not bundled; it is found in $DRAWLIB_FONT, scripts/fonts/, ~/.drawlib/fonts/ or the system fonts (see scripts/fonts/README.md). Without it the library uses DejaVu Sans - same geometry, lettering not ISO 3098; the check measures whichever font is active.

Using drawlib

Read references/drawlib_api.md before writing the first sheet - every call with its coordinate conventions, recipes and pitfalls. The essentials:

• S = D.Sheet("A4"|"A3"|"A2"|"A1"|"A0", lang="de"|"en", projection="first"|"third"). A4 is portrait, the others landscape (landscape= overrides). Sheet coordinates are mm from the lower left corner. Numbers the library writes follow the language's decimal marker, and decimals inside dimension texts are converted ("0.02" -> 0,02 on a German sheet).
• V = D.View(S, origin, scale, *D.VIEWS["front"]) - VIEWS has front, top, bottom, left, right, rear, iso. V.p(u, v) turns view coordinates (model mm) into sheet mm - use it for every annotation. Wrong vectors raise a clear error; non-ISO scales and upside-down views warn.
• Views: V.draw(solids, hidden=), V.section([(V.cut(solid), angle, spacing), ...], background=[uncut parts]), V.half_section(...), V.removed_section(...), V.detail(centre, r, at, scale, "Z"), D.BrokenView(...), V.thread(...), D.views_layout(...) for placement by projection method.
• Dimensions: S.hdim, S.vdim, S.dim, S.dim_angle, S.rdim, S.ddim; options tol=, box=True, outside=True, half=True, tshift=.
• Fits: write them in the text ("Ø20 H7", "Ø20 H7/s6"); S.fit_table, S.fit_pair_table print ISO 286 values; iso_tolerances gives deviations, limits, fits, ISO 2768.
• GD&T: S.datum, S.fcf(x, y, kind, "0.02", ["A", "B"]), S.fcf_leader.
• Surfaces: S.rough, S.rough_leader, S.general_surface.
• S.notes, S.leader_text, S.posnum, S.cutting_plane, S.bom, S.table, S.weld, S.pitch_circle, S.title_block(values, layout=json_or_dict, logo=png).

Rules that make the difference

These are the points examiners and workshops check; references/normen.md has the tables (line types, ISO 2768 values, common fits, typical Ra values, which geometrical tolerance for which function) and should be read when choosing values.

• Projection and views: state the method (symbol in the title block). Fewest views that define the part; a turned part needs one section along its axis. Prefer sections over hidden lines. Scales from ISO 5455 only; small parts are drawn enlarged so dimensions have room; long parts are broken; small details get a detail view.
• Dimension from the functional datum, not in chains, never twice. Auxiliary dimensions in parentheses. Dimensions outside the contour where possible; hole patterns in the view that shows them as circles; smaller dimensions closer to the part.
• Fits and tolerances: every mating diameter gets an ISO 286 fit (bearing seats as the bearing maker recommends). Everything untoleranced falls under the general tolerance in the title block (ISO 2768-mK by default; ISO 13920 for weldments).
• Geometrical tolerances only where function needs them, always with a datum that is itself a functional, measurable feature. Datum on an axis: in line with that diameter's dimension line. The leader meets the surface square on. Hole patterns: theoretically exact dimensions plus position tolerance.
• Surface texture on every functional surface, the general value once beside the title block. Symbols must read from below or from the right - use a leader for faces pointing down.
• Sections: shafts, pins, screws, keys, rolling elements and ribs are not cut in a longitudinal section. Neighbouring parts get different hatching; thin cut faces are blackened (angle="solid"); hatching is interrupted around text automatically.
• Threads (ISO 6410), welds (ISO 2553), gears (ISO 2203): drawn simplified, with the callout or data table carrying the information.
• Assembly drawings: item numbers in a row, leaders ending in a dot; parts list above the title block, item 1 at the bottom; standard parts with their standard designation; only functional and mounting dimensions; notes say how it is assembled and adjusted.
• Title block: title, drawing number, material with standard designation, mass (solid.volume × density), scale, general tolerance, date, sheet n/m, document type, revision. Never leave material or scale empty - the check flags it.

Honesty about limits

• Output is PDF/SVG/PNG/DXF plus STEP, not a native SolidWorks/Inventor drawing. For further editing in CAD give the DXF and STEP and say so.
• The sheet check finds collisions and inconsistencies; it does not judge whether the dimensioning, tolerancing or the choice of views is right. That is your review of the PNG against the checklist in references/normen.md.
• Tolerance values you choose are engineering proposals. Say which come from the user's documents and which are yours, so they can defend them.