fdm-design-rules

name	fdm-design-rules
description	Design rules for FDM/FFF 3D printing — wall and feature minimums, 45 deg overhangs, bridging, teardrop holes, elephant foot, warping, orientation, tolerances.
triggers	["fdm","3d print","3d-print","printed","printing","overhang","bridge","support","layer","nozzle","teardrop","warp"]
version	1.0.0
license	Apache-2.0
author	AgentCAD core
requires	[]

FDM/FFF parts fail for geometric reasons a kernel can see long before a slicer runs: a wall thinner than two extrusions, a face leaning past 45°, a round hole lying on its side, a corner that peels off the bed. This skill is the rule set for a part that prints right the first time with no support, plus the checks to run before you ship an STL. Use it when the process is fused filament. Do not use it for SLA/DLP (no overhang rule; drain holes and cure shrinkage instead), SLS/MJF (no support at all, different minimums), or any subtractive process. See fits-and-clearances for mating clearances, snap-fits for latches, enclosures for housing walls, and selectors-and-occt-failures for fillet failures.

Rules at a glance

Everything derives from the extrusion line width w ≈ 1.0–1.2 × nozzle (0.42 mm on a 0.4 mm nozzle). Values below assume 0.4 mm and 0.2 mm layers.

Rule	Value	Limit / why
Minimum wall	0.8–1.2 mm (2–3 × w)	under 2 perimeters the slicer drops it
Load-bearing wall	≥ 1.6 mm (4 × w)	2 perimeters is a skin, not structure
Emboss / engrave	≥ 0.8 mm wide, 0.6 mm deep	narrower than 2 × w is skipped
Pin, peg, rib	≥ 2 mm dia (3 loaded), L/D ≤ 8	thin towers wobble, delaminate
Vertical hole	≥ 2 mm dia	smaller and the perimeter closes over
Overhang	≥ 45° from the bed plane	shallower needs support or a redesign
Unsupported bridge	≤ 10 mm clean, ≤ 25 mm sagging	anchored at both ends
Hole compensation	+0.2 mm on the diameter	printed holes come out small
Elephant-foot chamfer	0.3–0.5 mm at 45°, bed edges	the first layer spreads
Bed-corner fillet	R ≥ 3 mm	sharp corners lift first
Tolerance	±0.2 mm, ±0.1 mm calibrated	add ±0.2 % above 100 mm
Layer height	0.1–0.3 mm (≤ 0.75 × nozzle)	quantises every Z dimension

Derive them — a 0.6 mm nozzle moves every row:

PARAMS = {
    "nozzle": {"default": 0.4, "min": 0.2, "max": 1.0, "unit": "mm",
               "description": "Nozzle diameter"},
}

def build(p):
    line_w = p.nozzle * 1.05     # slicer extrusion width
    min_wall = 2.0 * line_w      # two perimeters, the floor
    ...

Walls, features and the nozzle

Keep a wall an integer multiple of w (0.84, 1.26, 1.68 …). A 1.0 mm wall at 0.42 line width prints as two lines plus a 0.16 mm gap the slicer either leaves hollow or fills by over-extruding — a ridge, and weak either way. Step thicknesses by a whole line width.

Engrave rather than emboss: raised text under two lines wide disappears, while engraved text 0.6 mm deep with a 0.8 mm stroke and ≥ 4 mm cap height survives. Never put text on the bed face — the first-layer squish fills it.

Overhangs, bridging, support avoidance

Self-supporting means the downward-facing surface makes ≥ 45° with the bed plane, so each layer overlaps the one beneath by at least half a line width. Below 45°, in order of preference: reorient the part; replace the overhang with a 45° chamfer; add a self-supporting gusset; add a sacrificial bridge (a 1–2 layer web across the gap, cut off after printing); only then accept support.

Chamfer, do not fillet, where material meets the bed or an overhang. A fillet's tangent leaves horizontal at 0°, so its first millimetre is an unprintable overhang that droops; a 45° chamfer prints exactly as modelled. Fillets stay welcome on vertical (Z-parallel) and upward-facing edges. Author the 45° transitions into the profile rather than adding them afterwards — run equals rise:

def side_profile(x_face, x_pad, plate_t, gusset, z_ramp):
    pad = x_pad - x_face
    return [
        (x_face + gusset, plate_t),   # gusset toe on the plate
        (x_face, plate_t + gusset),   # run == rise -> 45 deg
        (x_face, z_ramp - pad),       # foot of the pad ramp
        (x_pad, z_ramp),              # run == rise -> 45 deg
    ]

Bridging: a span anchored on solid material at both ends prints to ~10 mm with no visible sag, 10–25 mm with 0.1–0.5 mm of droop, and ropes beyond. A bridge needs one direction and two anchors — exactly what a round horizontal hole lacks at its widest point.

Holes

Printed holes come out small. The perimeter over-extrudes at inner corners and the arc is approximated from inside, so a bore measures 0.1–0.3 mm under nominal. The error is near-constant in absolute terms, so it dominates small holes — a 3.4 mm M3 clearance can measure 3.15 mm. Compensate +0.2 mm on the diameter as a parameter you can recalibrate, never a constant in a radius.

Horizontal holes need a teardrop or polygon top. The roof of a bore whose axis is parallel to the bed is a bridge over nothing. A teardrop — the circle plus a 45° apex — keeps the bore round where a shaft or bearing touches and prints support-free; a hexagonal top suits a captive nut.

from math import sqrt

r = (bore_d + 0.2) / 2.0
t = r / sqrt(2.0)                       # where the 45 deg roof meets the bore
with BuildSketch(Plane.YZ) as teardrop:
    Circle(radius=r)
    with BuildLine():
        Polyline((-t, t), (0.0, r * sqrt(2.0)), (t, t), close=True)
    make_face()

Do not model FDM threads below M6 — use a heat-set insert boss or a self-tapping pilot (≈ 0.8 × major dia in PLA/PETG); see threads-and-fasteners. Counterbores print fine (their floor is a bridge no wider than the head), and a 90° countersink is a 45° cone either way.

First layer and warping

The first layer is squashed into the bed and spreads 0.1–0.4 mm past nominal — the elephant foot. Slicers can compensate, but the setting is printer-specific and invisible to your model; put the chamfer in the geometry and the part sits flat and mates correctly on any machine.

foot = min(p.foot_ch, plate_t * 0.3)          # 0.3-0.5 mm typical
if foot > 0.01:
    chamfer(part.edges().group_by(Axis.Z)[0], length=foot)

Warping is a cooling part's shrinkage concentrated at its corners. Geometric fixes: fillet the footprint corners (R ≥ 3 mm — a sharp corner is the stress concentration and lifts first); break a large flat base into ribs or a grid rather than one slab; keep unbroken flat runs under ~100 mm in ABS/ASA/PA; avoid abrupt cross-section changes along Z; add mouse-ears (sacrificial 8–12 mm discs, 2 layers, at each corner) when the footprint cannot change.

The two rules look contradictory and are not — they act on different edges: fillet the vertical corner edges (edges().filter_by(Axis.Z)), chamfer the horizontal bed edges (edges().group_by(Axis.Z)[0]).

Orientation for strength

The layer interface is the weak axis. Inter-layer (Z) tensile strength is typically 30–70 % of in-plane, and Z is also the impact and fatigue weak direction; Ahn et al. measured FDM ABS at 10–65 % of the injection-moulded value depending on raster orientation. So:

• Put bending and tensile loads in the layer plane. An L-bracket printed standing up loads its corner straight across the layers and snaps there; laid flat — the whole L in one plane, load in XY — it is several times stronger and needs no support. That is the snippet's orientation.
• A screw pulling out of a boss loads layers apart: prefer a heat-set insert, a through-bolt, or a boss whose axis lies in the layer plane.
• Pick the largest flat face for the bed, then break ties by load direction, support-free, surface finish.
• Anisotropy is not a safety factor. If the load has to cross layers, size the part against the Z strength, not the datasheet tensile value.

Tolerance envelope

Well-tuned desktop FDM holds ±0.2 mm under 100 mm, ±0.1 mm once flow and shrinkage are calibrated, plus ±0.2 % of the dimension above 100 mm. Industrial FDM is published at ±0.127 mm or ±0.0015 mm/mm, whichever is greater. XY repeats better than Z, and Z is quantised by layer height — make critical heights an integer multiple of it.

Design the clearance; do not rely on the tolerance. Per side: 0.2–0.3 mm sliding, 0.4–0.5 mm loose or rotating, 0.05–0.1 mm interference for a press fit. Anything tighter than ±0.1 mm gets machined or reamed after printing. See fits-and-clearances.

Materials at a glance

Material	Nozzle °C	Bed °C	Shrink	Stiffness	Warp	Use for
PLA	200–220	55–60	~0.3 %	high, E ≈ 3.0–3.6 GPa, brittle	low	jigs, fit checks, indoor non-structural (Tg ≈ 60 °C)
PETG	230–250	70–85	~0.4 %	medium, E ≈ 1.7–2.1 GPa, tough	low	functional brackets, outdoors, chemicals
ABS	240–260	90–110	0.8–1.5 %	medium, E ≈ 1.8–2.3 GPa	high	heat and impact, vapour finishing (Tg ≈ 105 °C)
ASA	240–260	90–110	~0.8 %	medium	high	UV-stable outdoor ABS
PA (nylon)	250–290	80–110	0.8–2.0 %	medium-low, very tough	high	gears, living hinges, wear parts — dry it first
TPU 95A	220–240	30–60	0.5–1.2 %	flexible	low	gaskets, bumpers, seals — slow, direct drive

Class-typical; the filament's own datasheet wins. Shrink is cooling shrinkage compensated on long dimensions — a different effect from the hole compensation above, which is dominated by the extrusion path.

Pre-print checklist

Run these before declaring a part printable; each is a real call on the part.

1. Wall — analyze_part(kind="wall", min_required=2*line_w) returns min_thickness_mm and its location. It is a sampled ray cast, so it also finds chamfer runouts: read the location before believing a red.
2. Build volume — metrics.bbox against the printer envelope.
3. Footprint — analyze_part(kind="projected_area", axis="Z") versus the real bed-contact area; a part standing on a knife edge will not stick.
4. Overhangs — analyze_part(kind="section", plane="XZ") for the silhouette; walk it for downward faces under 45°. Still manual today.
5. One solid — metrics.solids should be 1, or match SOLID_LABELS; a stray extra solid is material floating in mid-air.
6. Extremes — rebuild at every parameter's min and max (robust-parametrics).

Pin the checkable ones as intent so every rebuild re-runs them:

from agentcad.toolkit.specs import check_bbox, check_wall

SPECS = [
    check_wall(min_mm=0.84, grid=12, requirement="FDM-min-wall"),
    check_bbox([250.0, 210.0, 210.0], name="fits_build_volume"),
]

PRD-021 will ship these rules as an FDM process profile — check_dfm {process: "fdm"} returning located violations for overhang angle, bridge span and minimum feature — so a rule written as a SPECS entry today becomes a pack rule then, with the same read-fix-recheck loop.

snippets/printable_bracket.py puts it together: an L-bracket that prints flat with no support, its side profile one closed polyline whose gusset and bore-pad transitions are authored at 45°, a teardrop bore sized bore_d + hole_comp, an elephant-foot chamfer on the bed edges, minimum wall clamped to two line widths off nozzle, and fixing holes through holes.clearance.

Sources

• ISO/ASTM 52910:2018, Additive manufacturing — Design — Requirements, guidelines and recommendations; ISO/ASTM 52900:2021 (terminology).
• Gibson, Rosen & Stucker, Additive Manufacturing Technologies, 3rd ed., Springer, 2021 — design for AM, anisotropy, shrinkage.
• Redwood, Schöffer & Garret, The 3D Printing Handbook, 3D Hubs, 2017 — FDM feature minimums, overhang and bridging limits, tolerance bands.
• Ahn, Montero, Odell, Roundy & Wright, "Anisotropic material properties of fused deposition modeling ABS", Rapid Prototyping Journal 8(4), 2002.
• Stratasys, FDM Best Practice: Designing for FDM, and its accuracy statement (±0.127 mm or ±0.0015 mm/mm).
• UltiMaker, Design for FDM 3D printing; Prusa Research Knowledge Base — bridging, elephant-foot compensation, warping.
• Filament datasheets for the property table (UltiMaker PLA/PETG/ABS/Nylon/ TPU 95A; Prusament PLA/PETG/ASA).