Converting GMSH to OpenSeesPy

This GMSH case is derived from t1: Geometry basics, elementary entities, physical groups.

First, we need to understand a few important concepts: dim, entity, and physical groups.

Dimensions, Entities, and Physical Groups in GMSH

Dimensions (dim)

GMSH supports the following geometric dimensions:

• 0D: Points, used to define vertices or key geometric features. (dim=0)

• 1D: Lines, formed by connecting points, used for boundaries or linear structures. (dim=1)

• 2D: Surfaces, enclosed areas formed by lines. (dim=2)

• 3D: Volumes, closed regions formed by surfaces. (dim=3)

Entities

Entities are the basic building blocks of the geometry:

• Point entities: Define key points or boundary features.

• Line entities: Represent boundaries or divisions of surfaces.

• Surface entities: Define areas for 2D mesh generation.

• Volume entities: Represent regions for 3D mesh generation.

Physical Groups

Physical groups group entities to assign material properties, boundary conditions, or loads in simulations:

• Purpose: To label geometric features for simulation (e.g., load regions or boundary conditions).

• Examples:

  • A physical group can include multiple points, lines, surfaces, or volumes.

  • Simulations work with physical groups rather than individual entities.

Important

In the GMSH-to-OpenSeesPy conversion implemented by opstool, the names of the physical groups are crucial. Physical group names are used to identify different nodes and elements. Therefore, if you want to use physical groups, make sure to assign a unique name to each desired group!

An example

In the examples above, we have two ways to identify geometry:

(dim, entity_tag):

• For points: [(0, 1), [0, 2], [0, 3], [0, 4]]

• For lines: [(1, 1), [1, 2], [1, 3], [1, 4]]

• For surfaces:[(2, 1)]

Physical group:

• name: “Boundary”, include 4 lines and 4 points

• name: “Surface”, include 1 surface.

Note

In GMSH, geometries are mutually exclusive. For example, Surface 1 does not include its boundary lines (1–4), and Line 1–4 does not include its boundary points (1–4). This is a crucial point to note!

GMSH model

Here, we use Python code to create a GMSH model. If you already have a generated .msh file, you can skip this section. opstool provides two methods to obtain GMSH data: one is directly from memory, and the other is by reading a ``.msh`` file. Both methods are equivalent.

import gmsh
import sys

gmsh.initialize()
gmsh.model.add("t1")

# points
# (dim, entity_tag) = [(0, 1), [0, 2], [0, 3], [0, 4]]
lc = 1e-2
gmsh.model.geo.addPoint(0, 0, 0, lc, tag=1)
gmsh.model.geo.addPoint(0.1, 0, 0, lc, tag=2)
gmsh.model.geo.addPoint(0.1, 0.3, 0, lc, tag=3)
gmsh.model.geo.addPoint(0, 0.3, 0, lc, tag=4)

# Lines
# (dim, entity_tag) = [(1, 1), [1, 2], [1, 3], [1, 4]]
gmsh.model.geo.addLine(1, 2, tag=1)
gmsh.model.geo.addLine(3, 2, tag=2)
gmsh.model.geo.addLine(3, 4, tag=3)
gmsh.model.geo.addLine(4, 1, tag=4)

gmsh.model.geo.addCurveLoop([4, 1, -2, 3], tag=1)

# Surface
# (dim, entity_tag) = [(2, 1)]
gmsh.model.geo.addPlaneSurface([1], tag=1)

gmsh.model.geo.synchronize()

# Important:
# Note that we use names to distinguish groups, so please do not overlook this!
# We use the "Boundary" group to include 4 lines and 4 corner points, which will later be used to specify the boundary conditions.
# The "Surface" group includes 1 surface, which will be used later to generate triangular elements!
gmsh.model.addPhysicalGroup(dim=0, tags=[1, 2, 3, 4], tag=1, name="Boundary")
gmsh.model.addPhysicalGroup(dim=1, tags=[1, 2, 3, 4], tag=2, name="Boundary")
gmsh.model.addPhysicalGroup(dim=2, tags=[1], tag=3, name="Surface")

# We can then generate a 2D mesh...
gmsh.model.mesh.generate(2)

# ... and save it to disk
# gmsh.write("t1.msh")


# if "-nopopup" not in sys.argv:
#     gmsh.fltk.run()

# This should be called when you are done using the Gmsh Python API:
# However, we still need to read data from GMSH, so we will keep it open for now and close
# it later after all the data has been read.
# gmsh.finalize()  # !!!!!!!!!!!!!!!!!!!!!!!

GMSH to OpenSeesPy

API: opstool.pre.Gmsh2OPS

import opstool as opst
import openseespy.opensees as ops

# Initialize GMSH to OpenSeesPy converter with 3D model and 6 degrees of freedom per node
GMSH2OPS = opst.pre.Gmsh2OPS(ndm=3, ndf=6)

# Read the saved .msh file generated by GMSH
# GMSH2OPS.read_gmsh_file("t1.msh")
GMSH2OPS.read_gmsh_data()
# Finalize and close, must after GMSH2OPS.read_gmsh_data()
gmsh.finalize()

Info:: Geometry Information >>>
9 Entities: 4 Point; 4 Curves; 1 Surfaces; 0 Volumes.

Info:: Physical Groups Information >>>
2 Physical Groups.
Physical Group names: ['Boundary', 'Surface']

Info:: Mesh Information >>>
404 Nodes; MaxNodeTag 404; MinNodeTag 1.
810 Elements; MaxEleTag 810; MinEleTag 1.

By physical group

Here, we use physical groups to identify nodes and elements.

ops.wipe()
# Initialize a basic 3D model with 6 degrees of freedom per node
ops.model("basic", "-ndm", 3, "-ndf", 6)

# Define an elastic isotropic material
# Material ID: 1
# Elastic modulus: 2e8
# Poisson's ratio: 0.3
# Density: 7.85
ops.nDMaterial("ElasticIsotropic", 1, 2e8, 0.3, 7.85)

# Define a section using PlateFiber
# Section tag: 1
# Material tag: 1 (linked to the material defined above)
# Thickness: 0.005
secTag = 1
ops.section("PlateFiber", secTag, 1, 0.002)

GMSH2OPS.get_physical_groups()

{'Boundary': [(0, 1), (0, 2), (0, 3), (0, 4), (1, 1), (1, 2), (1, 3), (1, 4)],
 'Surface': [(2, 1)]}

Since we will read nodes and elements from GMSH, element tags and node tags are not needed. You only need to input element parameters other than the element tags and node tags.

# Create OpenSeesPy node commands based on all nodes
GMSH2OPS.create_node_cmds()

# Create OpenSeesPy element commands for specific entities
# ASDShellT3 elements (3-node shell elements)
#
ele_tags = GMSH2OPS.create_element_cmds(
    ops_ele_type="ASDShellT3",  # OpenSeesPy element type
    ops_ele_args=[secTag],  # Additional arguments for the element (e.g., section tag)
    # Dimension-entity tags to specify which elements to create
    physical_group_names=["Surface"],
)

Using ASDShellT3 - Developed by: Massimo Petracca, Guido Camata, ASDEA Software Technology

Boundary conditions are specified using the “Boundary” physical group.

# fix_node_tags = GMSH2OPS.create_fix_cmds(
#     physical_group_names=["Boundary"], dofs=[1] * 6
# )

fix_node_tags = GMSH2OPS.get_node_tags(physical_group_names=["Boundary"])
for tag in fix_node_tags:
    ops.fix(tag, *[1] * 6)

# If there are too many geometries on the boundary, you can iterate through and extract
# all lines and points on a geometry using the following commands:

# This will extract all the boundaries on face with name Surface.
boundary_dim_tags = GMSH2OPS.get_boundary_dim_tags(physical_group_names="Surface", include_self=False)
print(boundary_dim_tags)
print(GMSH2OPS.get_physical_groups()["Boundary"])
# # Create fix commands for the boundary with constraints applied to all 6 degrees of freedom (DOFs)
# fix_node_tags = GMSH2OPS.create_fix_cmds(
#     dim_entity_tags=boundary_dim_tags, dofs=[1] * 3
# )

[(0, 1), (0, 2), (0, 3), (0, 4), (1, 1), (1, 2), (1, 3), (1, 4)]
[(0, 1), (0, 2), (0, 3), (0, 4), (1, 1), (1, 2), (1, 3), (1, 4)]

opst.vis.pyvista.set_plot_props(
    point_size=0,
    notebook=True,
    mesh_opacity=0.75,
)
plotter = opst.vis.pyvista.plot_model()
plotter.show(jupyter_backend="jupyterlab")
# plotter.show()

It can also be saved to a file.

# GMSH2OPS.set_output_file("t1_ops.py")
# # GMSH2OPS.set_output_file("t1_ops.tcl")
# GMSH2OPS.write_node_file()
# GMSH2OPS.write_element_file(
#     ops_ele_type="ASDShellT3",  # OpenSeesPy element type
#     ops_ele_args=[secTag],  # Additional arguments for the element (e.g., section tag)
#     # Dimension-entity tags to specify which elements to create
#     physical_group_names=["Surface"],
# )
# GMSH2OPS.write_fix_file(physical_group_names=["Boundary"], dofs=[1] * 6)

By (dim, entity_tag)

Here, we use dimensions and entity tags to identify nodes and elements.

ops.wipe()
# Initialize a basic 3D model with 6 degrees of freedom per node
ops.model("basic", "-ndm", 3, "-ndf", 6)

# Define an elastic isotropic material
# Material ID: 1
# Elastic modulus: 2e8
# Poisson's ratio: 0.3
# Density: 7.85
ops.nDMaterial("ElasticIsotropic", 1, 2e8, 0.3, 7.85)

# Define a section using PlateFiber
# Section tag: 1
# Material tag: 1 (linked to the material defined above)
# Thickness: 0.005
secTag = 1
ops.section("PlateFiber", secTag, 1, 0.002)

Since we will read nodes and elements from GMSH, element tags and node tags are not needed. You only need to input element parameters other than the element tags and node tags.

# Create OpenSeesPy node commands based on all nodes
GMSH2OPS.create_node_cmds()

# Create OpenSeesPy element commands for specific entities
# ASDShellT3 elements (3-node shell elements)
#
ele_tags = GMSH2OPS.create_element_cmds(
    ops_ele_type="ASDShellT3",  # OpenSeesPy element type
    ops_ele_args=[secTag],  # Additional arguments for the element (e.g., section tag)
    # Dimension-entity tags to specify which elements to create
    dim_entity_tags=[(2, 1)],
)

# Define boundary conditions
# Get the boundary dimension tags for the surface
boundary_dim_tags = GMSH2OPS.get_boundary_dim_tags([(2, 1)])
print("Boundary dim_tags:", boundary_dim_tags)
# Create fix commands for the boundary with constraints applied to all 6 degrees of freedom (DOFs)
fix_node_tags = GMSH2OPS.create_fix_cmds(dim_entity_tags=boundary_dim_tags, dofs=[1] * 6)

Boundary dim_tags: [(0, 1), (0, 2), (0, 3), (0, 4), (1, 1), (1, 2), (1, 3), (1, 4)]

plotter = opst.vis.pyvista.plot_eigen([1, 9], subplots=True)
plotter.show(jupyter_backend="jupyterlab")
# plotter.show()

Using DomainModalProperties - Developed by: Massimo Petracca, Guido Camata, ASDEA Software Technology

OPSTOOL ::  Eigen data has been saved to .opstool.output/EigenData-Auto.nc!