Three-dimensional FEM#

A transverse slice cannot show how a helical tooth twists across its width or how stress varies near a free face. The package can build and solve 3D models for these questions. That capability must be separated from validation: this chapter documents the implemented 3D workflow, not a validated 3D design result.

What changes from 2D?#

Aspect	2D	3D
Domain	Transverse section in plane strain	Finite-width volume
Mesh	Quadrilaterals	Extruded or twisted hexahedra
Displacements	In-plane	Three components
Applied force	Normalized per unit width	Total force over the modelled width
Reported torque	Per unit width	Total N·mm
Face effects	Not resolved	Can vary across width
Cost	Usually manageable for a sweep	Can grow rapidly with flank and width refinement

For spur gears, extrusion preserves the section orientation. For helicals, the twist over width \(b\) is

\[\Delta\theta=\frac{b\tan\beta}{r},\]

with reference radius \(r=d/2\). The pair generator gives the two members opposite hands. This geometric extrusion is not a model of every possible manufacturing modification.

Hexahedral mesh of a helical gear sector

Three-dimensional gear pair

Mesh the volume first#

Continue Quick start. This example controls the axial count explicitly; it is a mesh inspection example, not a converged contact mesh:

from dataclasses import replace
from gearbox.fem import ToothMeshSettings, mesh_pair

helical = replace(transmission,
    pinion=replace(transmission.pinion, helix_angle=15.0),
    wheel=replace(transmission.wheel, helix_angle=15.0))
settings_3d = ToothMeshSettings(
    flank_size=0.08, fillet_size=0.05,
    tooth_elements=10, width_elements=8, order=1,
)
volume_mesh = mesh_pair(helical, "out/3d_mesh", "helical_pair", "3D",
                       settings=settings_3d, teeth=(3, 4), formats=("msh",))
print(volume_mesh.node_count, volume_mesh.element_count, volume_mesh.min_quality)

The solver reader maps linear hexahedra to C3D8I and quadratic serendipity hexahedra to C3D20R. Quadratic order adds degrees of freedom and does not remove the need to resolve the contact band. Physical groups become surfaces (FLANK, FILLET, BORE) or volumes (GEAR), with end faces FACE_Z0 and FACE_ZB; pair prefixes remain unchanged.

Inspect the mesh in 3D: excessive twist per layer, slender elements, distorted fillets and too few axial layers can all matter even when the minimum scaled Jacobian is positive.

Three-dimensional bending#

solve_bending defaults to 3D, but state the dimension explicitly for reproducible scripts. The bore translations are fixed and a pressure band loads one flank. The total normal force is \(F_t/(\cos\alpha_t\cos\beta_b)\).

from gearbox.fem import ElasticMaterial, solve_bending

# Illustrative solver invocation: not executed to produce a published 3D result here.
root_3d = solve_bending(
    helical, "out/3d_bending", dimension="3D", settings=settings_3d,
    material=ElasticMaterial(
        youngs_modulus=helical.pinion.material.elastic_modulus,
        poisson_ratio=helical.pinion.material.poissons_ratio,
    ),
)

The loaded band is at approximately constant radius across the width. It does not follow the actual inclined instantaneous contact line of a helical pair. This is useful as a defined load case, but it is not equivalent to a 3D tooth-contact analysis. Compare the reaction torque with applied torque, inspect the tensile root field across the width and perform mesh and sector-size studies before interpreting its maximum.

Three-dimensional contact#

The wheel bore is fixed in three translations. The pinion bore has prescribed in-plane rigid rotation and fixed axial displacement. Those axial restraints can react helical thrust; they do not model shaft or bearing compliance. Flank contact remains frictionless surface-to-surface penalty contact.

from gearbox.fem import CONTACT_SETTINGS, solve_contact

# Illustrative only: a full fine-width model may be computationally expensive.
contact_mesh_3d = replace(CONTACT_SETTINGS, width_elements=24, order=1)
contact_3d = solve_contact(
    helical, "out/3d_contact", dimension="3D", settings=contact_mesh_3d,
    teeth=(3, 4), tolerance=0.05,
)

The chosen 24 layers are an explicit example, not a validated convergence prescription. The default contact flank size is 0.015 modules. If axial layers are chosen automatically from that size, a 34 mm width at module 2.5 implies roughly 907 layers: multiplying a fine transverse mesh by hundreds of layers quickly becomes expensive. Reducing width_elements makes a run cheaper but may make the contact representation inaccurate.

The contact result exposes pressure, root stresses, displacement arrays, mesh and last-run files. The same target-torque iteration and summary rescaling described in Contact analysis apply. Successful torque matching proves equilibrium under the selected model; it does not prove pressure convergence.

A defensible convergence programme#

Establish a small 2D spur reference at the same nominal line load and compare with Hertz.
Build the 3D mesh and inspect geometry, groups and constraints before solving.
Refine the flank and fillet independently from axial layers. Record all counts and material data.
Compare torque, contact area, peak pressure and root stress—not just one scalar peak.
Test penalty sensitivity and the number of teeth in each sector.
Check whether maxima occur at free edges or sharp tips, where local singular behaviour can prevent peak-stress convergence.
Only then extend the model to a sweep of mesh positions.

Do not assume a 3D solver run is more accurate than a well-resolved 2D reference simply because it has more dimensions. Accuracy follows the model assumptions and convergence evidence.

Scope and available evidence#

External rack-generated gears, linear-elastic materials and frictionless contact are the current basis. The full double-helical geometry, shaft/bearing system, measured manufacturing deviations, flank relief, friction and plasticity are not supplied by these examples.

The published 2D checks do not establish a validated 3D error bound. No new 3D pressure result or 3D convergence study is asserted here; the expensive solver snippets above are documented for users who can carry out that study. Existing 3D mesh images demonstrate geometry, not validation of stress or contact pressure.