Engineering drawing

An engineering drawing is a DOCUMENT derived from a part. cad.eng_drawing projects views from the part's geometry, places dimensions between points ON that geometry, finds centre marks on it, and lays the result out on an ISO sheet with a frame and a title block. Change the model, rerun the drawing script, and the views, hidden lines and measured values move with it. Nothing on the sheet is drawn by hand, and nothing on it is a number you typed unless you chose to override a value.

The output is one PDF. That is what a shop receives and what every operating system opens. No DXF is written, nothing is paired or linked, and there is no CLI: the script is the interface. Cut layouts and flat patterns are toolpaths, not documents, and a different job.

Setup

Run the cad command (~/.local/bin/cad where ~/.local/bin is not on your PATH, or where a project's environment puts its own cad first; cad.cmd on Windows). If cad is not found and the CAD app was only just added, its server may still be starting: wait five seconds and run the command again, for up to a minute, before anything else. Otherwise install text-to-cad, outside a sandbox or with its permission:

curl -fsSL https://texttocad.dev/install.sh | sh

On Windows, in PowerShell: irm https://www.texttocad.dev/install.ps1 | iex. Any other failure says what to do, and cad doctor explains the installation.

Workflow

1. Get the part. Call the model: enclosure(), imported from the model's script, is built by text-to-cad's server (a replay when the server already holds it), and its .shape is the part. For a part with no model, read its file: read_step for a STEP, read_xbf for an xbf, anchored on Path(__file__).parent. Any build123d shape works. The drawing documents geometry, it does not build it.

2. Write <name>_drawing.py beside the model, from the template. Import the model facts the dimensions reference (hole pitch, overall size, wall) from the model module rather than retyping them, so moving a feature moves its dimension.

3. Place views with sheet.three_views(part, iso=True), which returns FOUR views: top, front and right in third angle with room for two rows of dimensions, plus an isometric in the free corner. sheet.three_views(part) returns three. Use sheet.view(part, name, at=(x, y)) (sheet millimetres from the bottom-left corner; A3 is 420 × 297, A4 is 297 × 210) only for a custom layout.

4. Dimension what a maker needs, in MODEL coordinates: overall size per view (view.overall()), feature positions and sizes (view.dim, with tol= or fit= where the design requires one), holes as callouts (view.hole: thru, depth, counterbore, countersink, thread), and notes with leaders (view.note). Leave text unset so the dimension is measured; give a value only where the model does not define it. Leave offset unset too and the dimension takes the next free row outside the view; pass one only to place a dimension deliberately, and remember it is measured from the dimension's own points, not the view's edge. Keep notes few and short; one wider than the sheet's note column is refused, and notes= takes a LIST (notes="BREAK EDGES" is a sequence of eleven characters, so it is refused too).

5. Run cad run <name>_drawing.py. It prints the PDF it wrote, and anything it noticed while drawing — read those first:

   • "measures blank paper": the dimension's model points do not land on the view's geometry. Almost always the part was built from a corner and the script assumed it was centred. Check the part's bounding box.
   • "annotation overlaps": two callouts print on top of each other, usually one view's outermost dimension against the label of the view above it. Pass a bigger three_views(gap=...) or place one with offset=. The text is measured as the renderer draws it, glyph by glyph, so this fires on ink and not on markup: a chain of toleranced dimensions is silent when the values clear each other.

   Steps 3 and 5 stand on their own: a sheet of views with no dimensions on it yet is a drawing, and writes its PDF.

   When running unattended, set MPLCONFIGDIR to a writable directory so matplotlib's font cache does not warn.

6. Read the PDF and fix what collides. Check that no dimension text sits on a view, that hidden lines appear where features are behind faces, that every hole has a centre mark, and that no leader crosses the part. Very small dimensions (a few mm) put their value on their own extension line; dimension the larger feature instead. Move at= or offset= and rerun.

What the sheet contains

• Layers with meaning: VISIBLE (heavy outline), HIDDEN (dashed), CENTER (centre marks), DIM, NOTES, TITLE, SHEET (frame), each printed at its own weight — 0.5 mm down to 0.18 mm, so thick reads against thin on paper. An edge is drawn once: a silhouette that the kernel returns as both visible and hidden stays on VISIBLE. Hidden TANGENT transitions are not drawn at all — a fillet running into a face, or the seam where a cylinder closes on itself, marks nothing a shop can see, and drawn dashed it reads as a hidden edge that is not there (on a bore, as a line down the hole's own axis).
• Dimensions measured from the geometry, with filled arrowheads and witness lines, and true-size values at any drawing scale.
• A title block with title, part number, material, author, scale, units, projection, revision, SHEET n OF m and the drawing function's name; numbered notes above it (the general tolerance, when given, is note 1); a revision table top-right when revisions= is given. Text longer than its cell is set smaller, and cut with an ellipsis rather than overrun.
• PDF bytes that are a function of the content: no creation date is stamped, so an unchanged drawing rebuilds to an identical file.

What fails loudly

The script raises rather than writing a wrong or missing document:

• Views that run off the frame, naming a scale that has been laid out and verified to fit, or saying that no standard scale does.
• A part argument the vocabulary does not define: an unknown view name, sheet size or projection, orientation= other than "h"/"v", a negative or zero diameter, a counterbore that is not a (diameter, depth) pair, a tol that is not a number or a pair, a hole that is both thru and given a depth, notes= or revisions= given a bare string, a note wider than the sheet, angle() legs that are collinear or zero-length, a non-finite at= or offset=.
• A missing renderer. The PDF is the drawing, so no matplotlib is a failure, not a skipped half. A failed render leaves no file it wrote; an earlier PDF stays byte for byte.
• out= missing or not naming a .pdf, at import time.

Limits to state in the handoff

• Tolerances come only from tol=, fit= and general_tolerance= that you write; get the values from the design requirements or the user, never invented. A dimension without one is nominal.
• Views are orthographic projections with hidden lines from the kernel; no sections, details, or auxiliary views yet. Say what a view does not show.
• The sheet keeps callouts clear of the views it knows about, and reports annotation that still prints over other annotation, but it does not check annotation against line work. Read the PDF.