Meshing
A part is meshed from its geometry with one call, part.mesh(settings, section, ...). What the geometry is decides
what you get: a line gives beams or bars, a surface shells, a STEP solid tetrahedra. The meshing is done by Gmsh,
installed with xfea-mcp and with pip install "xfea[all]".
Lines into beams
Section titled “Lines into beams”Give the part its geometry, then mesh it with a section. For a line, element_cls says what the elements are, and
orientation is the beams’ local y axis.
from xfea.geometry import Linefrom xfea.meshing import MeshingSettingsfrom xfea.model import BeamElement, ElasticIsotropic, Model, Part, RectangularSection
model = Model(name="meshing")steel = ElasticIsotropic(E=210_000, v=0.3, density=7.85e-9) # N, mm, t
beam = model.add_part(Part(name="beam"))beam.base_geometry = Line((0, 0, 0), (2000, 0, 0))beam.mesh( settings=MeshingSettings(max=100), # elements of 100 mm at most section=RectangularSection(w=50, h=100, material=steel), element_cls=BeamElement, orientation=[0, 1, 0],)print(len(beam.nodes), len(beam.elements)) # 21 nodes, 20 elementsMeshingSettings(divisions=8) cuts each line into exactly 8 elements instead. base_geometry also takes a polyline,
or a list of lines or polylines. TrussElement, TieElement and StrutElement are meshed the same way, with their
sections.
Surfaces into shells
Section titled “Surfaces into shells”A surface is given as a mesh of its faces. There are two ways to mesh it:
from xfea.geometry import Meshfrom xfea.model import ShellSection
concrete = ElasticIsotropic(E=30_000, v=0.2, density=2.4e-9)
slab = model.add_part(Part(name="slab"))slab.base_geometry = Mesh.from_meshgrid(4000, 8, 2000, 4) # 4 m by 2 m in the xy plane, 8 x 4 quads
# Keep the faces: each quad becomes 2 x 2 quadratic quadsslab.mesh(settings=MeshingSettings(divisions=2, element_order=2), section=ShellSection(t=200, material=concrete))
# Or mesh the surface again in triangles of the size asked forslab.mesh(settings=MeshingSettings(max=250, element_order=2), section=ShellSection(t=200, material=concrete))divisions keeps the faces you gave, each cut into divisions x divisions elements, quads staying quads:
divisions=1 means the mesh given is the mesh. Without it, the surface is remeshed. Mesh(vertices, faces) takes any
vertices and faces of your own.
Solids from a STEP file
Section titled “Solids from a STEP file”from xfea.model import SolidSection
block = model.add_part(Part(name="block"))block.base_geometry = "bracket.step" # the path of a STEP fileblock.mesh( settings=MeshingSettings(max=10, element_order=2), section=SolidSection(material=steel),)Naming parts of the geometry
Section titled “Naming parts of the geometry”A STEP part has solids, faces, edges and points, each with properties: a face is a plane with a normal, or a cylinder
with an axis and a radius; an edge is a straight line with a direction, or a circle. Select picks them by those
properties, and groups turns each selection into a group of the meshed part’s nodes, to put supports and loads on:
from xfea.meshing import Select
block.mesh( settings=MeshingSettings(max=10, element_order=2), section=SolidSection(material=steel), groups={ "base": Select.faces(normal="-z"), # the faces facing down "bolt_holes": Select.holes(radius_max=9), # the walls of holes up to 18 mm across "front_edge": Select.edges(near=(50, 0, 20)), # the edge nearest that point },)model.add_fix_bc(nodes=block.find_group_by_name("base"))What a selection can say:
| Selection | Picks |
|---|---|
Select.faces(normal="+z") |
Plane faces whose outward normal is +z ("z": either way). |
Select.faces(on_plane=((0, 0, 20), "z")) |
Faces lying in the plane z = 20. |
Select.faces(type="cylinder", along="x", radius_max=12) |
Cylinders along x, of radius 12 at most. |
Select.holes() |
Holes’ walls: round faces with their material away from the axis, going at least half way round. Not pins, not fillets. |
Select.edges(near=(x, y, z)) |
The edge nearest a point (count=3: the 3 nearest; within=5: all within 5). |
Select.edges(type="line", along="z") |
Every straight vertical edge. |
Select.edges(type="circle", touching=Select.holes()) |
The holes’ rims: edges of what another selection picks (a hole’s wall also has a straight seam). |
Select.points(near=(x, y, z)) |
The geometry’s corner nearest a point. |
Select.solids(named="BasePlate") |
A solid by its name in the STEP file (a CAD tool’s body label). |
Every condition given must hold, and selections pick by properties, never by numbers, which change when the CAD file
does. A surface mesh and lines have faces, edges and points too: Select.points(near=...) names a beam’s end.
Seeing what is there
Section titled “Seeing what is there”describe lists a STEP part’s entities with their properties, or only what a selection picks: the way to check a
selection before meshing with it.
from xfea.meshing import describe
for face in describe("bracket.step", what="faces"): print(face)# face 3, plane, area 5485, normal (0, 0, 1), centre (50.2, 30, 20)# face 7, cylinder, area 1257, radius 10, axis (0, 0, 1), hole wall, centre (30, 30, 10)# face 8, cylinder, area 754, radius 8, axis (0, 0, 1), outer, centre (75, 30, 27.5)
print(describe("bracket.step", select=Select.holes()))Your AI assistant does the same with its describe_geometry tool: ask it to “refine along the top front edge” and it
lists the candidates, shows them to you, and writes the selection into the script.
Finer where it matters
Section titled “Finer where it matters”refine makes the mesh finer on what a selection picks, in a box or in a ball, growing back to the part’s size over
reach (4 x size by default). The rest stays coarse.
from xfea.meshing import Refine
block.mesh( settings=MeshingSettings(max=10, element_order=2, refine=[ Refine(Select.holes(), size=1.5, reach=8), # around the holes Refine(Select.edges(near=(50, 0, 20)), size=2), # along one edge Refine.in_box((0, 0, 0), (100, 60, 5), size=4), # a slice near the base Refine.around((30, 30, 20), radius=15, size=2), # a ball round a point ]), section=SolidSection(material=steel),)The same works on lines (Refine.around(tip, radius=50, size=5) shortens a beam’s elements near its tip) and on
surfaces that are remeshed. To refine everywhere, lower max; there is no splitting of an existing mesh: mesh again
with the new settings, and compare the results to see that they have converged.
Sizes and order
Section titled “Sizes and order”| Setting | What it is |
|---|---|
min, max |
The smallest and the largest element size, in the model’s length unit. |
element_order |
1 for linear elements, 2 for quadratic ones, with midside nodes. |
refine |
Where the mesh is finer: a list of Refine. |
divisions |
For a surface mesh or lines: keep the faces (segments), each cut into this many. |
optimize |
Gmsh’s mesh optimisation setting. |
Gmsh’s own options go through its settings class, which MeshingSettings would drop:
from xfea_gmsh import GmshMeshingSettings
block.mesh(settings=GmshMeshingSettings(max=10, element_order=2, algorithm_3d=1), section=SolidSection(material=steel))Assemblies and meshes made elsewhere
Section titled “Assemblies and meshes made elsewhere”model.add_parts_from_step(path, parts=[...], refine=[...])meshes the solids of a STEP assembly, each into a part of its own;refineworks across the parts as above.model.add_parts_from_mesh(path, parts=[...])reads a mesh made elsewhere: Gmsh.msh, Abaqus.inp, VTK, Salome.med.
Both are in the API reference. Parts meshed apart are joined by interfaces, found with
model.detect_interfaces(...).
Finding nodes on the mesh
Section titled “Finding nodes on the mesh”Besides the groups a mesh is given, nodes can be found by where they are:
from xfea.geometry import Plane
start = beam.find_closest_nodes_to_point((0, 0, 0)) # the node nearest a pointedge = slab.find_nodes_on_plane(Plane((0, 0, 0), (1, 0, 0))) # the nodes on the plane x = 0top = block.nodes.subgroup(lambda n: n.z > 19.9) # any rule of your ownWithout a mesher
Section titled “Without a mesher”Nodes and elements can also be made one by one, with part.add_node(Node(xyz=...)) and
part.add_element(BeamElement(nodes=[a, b], section=section)): the model on the Analysis
page is built that way.
When meshing goes wrong
Section titled “When meshing goes wrong”- “A refinement selects nothing” or “The group … selects nothing”: check the selection with
describe(path, select=...). - To see Gmsh’s own output, set
settings.MESH_VERBOSE = True(fromxfea import settings). xfea.meshing.failed_algorithms()gives the meshing plugins that failed to load, each with its error.
© 2026 Francesco Ranaudo · Text and pictures CC BY 4.0 · Code Elastic License 2.0 · how to reuse them