Gmsh example

Objective

This example demonstrate the interoperability of PyAnsys with Gmsh, a very well known open source Python meshing library. For more information, visit the Gmsh website: Gmsh.

Description

Gmsh is used to import an external geometry file in STL format. The pymapdl-reader library is then used to import the geometry into PyMAPDL.

This example makes use of these files:

• gmsh_converter.py: Loads a STEP file, meshes it, and saves it as a Gmsh file.

• mesh_converter: Converts the MSH file into an Ansys CDB database format file (archive file).

• modal_analysis.py: Imports the CDB database, sets up the modal analysis, and runs it. It also shows an animation of the first mode and saves it to a GIF file named animation.gif.

Requirements

You must have Gmsh installed. You can install it using pip:

pip install gmsh

Source code

gmsh_generator.py file

"""Using ``gmsh``, read the STEP file, mesh it, and save it as a MSH file."""
import gmsh

gmsh.initialize()
gmsh.option.setNumber("General.Terminal", 1)

gmsh.model.add("t20")

# Load a STEP file (using `importShapes' instead of `merge' allows to directly
# retrieve the tags of the highest dimensional imported entities):
filename = "pf_coil_case_1.stp"
v = gmsh.model.occ.importShapes(filename)


# Get the bounding box of the volume:
gmsh.model.occ.synchronize()

# Specify a global mesh size and mesh the partitioned model:
gmsh.option.setNumber("Mesh.CharacteristicLengthMin", 10)
gmsh.option.setNumber("Mesh.CharacteristicLengthMax", 10)
gmsh.model.mesh.generate(3)
gmsh.write("from_gmsh.msh")

gmsh.finalize()

mesh_converter.py file

"""
This script convert the file in `gmsh` format to ANSYS `CDB` format.
"""

from ansys.mapdl.reader import save_as_archive
import pyvista as pv

filename = "from_gmsh.msh"
mesh = pv.read_meshio(filename)
# mesh.plot()  # optionally plot the mesh
mesh.points /= 1000
save_as_archive("archive.cdb", mesh)

modal_analysis.py file

"""Import the CDB database, setup modal analysis and run it."""


from ansys.mapdl.core import launch_mapdl

mapdl = launch_mapdl(override=True, additional_switches="-smp")
filename = "archive.cdb"
mapdl.cdread("db", filename)
mapdl.save()

# verify cells are valid
mapdl.prep7()
mapdl.shpp("SUMM")

# specify material properties
# using aprox values for AISI 5000 Series Steel
mapdl.units("SI")
mapdl.mp("EX", 1, 200e9)  # Elastic moduli in Pa (kg/(m*s**2))
mapdl.mp("DENS", 1, 7700)  # Density in kg/m3
mapdl.mp("NUXY", 1, 0.3)  # Poissons Ratio
mapdl.et(1, 181)  # ! ET,1,SHELL181 ! SHELL181
mapdl.keyopt(
    1, 3, 2
)  # ! Option for the shell. Integration option: 'Full integration with incompatible modes'
mapdl.sectype(1, "SHELL")
mapdl.secdata(1, 1, 0, 3)  # ! which means: SECDATA,TK, MAT, THETA, NUMPT, LayerName
mapdl.emodif("ALL", "MAT", 1)  # ! Setting material id
mapdl.emodif("ALL", "REAL", 1)  # ! Setting real constant

# By setting the section type (`SECTYPE`) the model will run and solve.

# The model has solid and shell elements.
# We don't need both, hence I'm going to delete the shell elements.
mapdl.esel("S", "type", "", 4)  # selecting elements with type 4 = shell181
mapdl.edele("all")
mapdl.allsel()

# Run an unconstrained modal analysis
mapdl.run("/SOLU")
mapdl.outres("all")
mapdl.antype("MODAL")  # default NEW
mapdl.modopt("LANB", 20, 1)
mapdl.solve(verbose=False)
mapdl.save("solved")

mapdl.post1()
mapdl.set("FIRST")

result = mapdl.result

result.animate_nodal_displacement(
    4,
    show_edges=False,
    lighting=True,
    loop=True,
    add_text=False,
    nangles=30,
    # displacement_factor=50,
    n_frames=100,
    movie_filename="animation.gif",
)

mapdl.exit()

Notes

You should copy all the files in a separate directory to make running the example easier.