Example 01: Gmsh Example

Objective

Demonstrate the interoperability of PyAnsys with gmsh, a very well known open source Python meshing library.

For more information about gmsh please visit its website: Gmsh.

Description

In this example the interoperability of PyAnsys with the open source mesher gmsh is demonstrated. Using gmsh we import an external geometry file in STL format and then the geometry is imported into PyMAPDL using the pymapdl-reader library.

This example is composed of several files.

• gmsh_converter.py: Load a STEP file, mesh it, and save it as a gmsh file.

• mesh_converter: Convert the *.msh file into an Ansys CDB database format file (archive file).

• modal_analysis.py: Import CDB database, setup the modal analysis and run it. It also shows an animation of the first mode and save it to a gif file named animation.gif.

Requirements

You need to have gmsh installed. You can install it using pip:

pip install gmsh

Source code

gmsh_generator.py

"""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

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

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

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

"""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

It is recommended that you copy all the files in a separate directory to make it easier to run the example.