Thermal stress example

This example shows how to create a thermal stress model with the PyDYNA pre service. The executable file for LS-DYNA is ls-dyna_smp_s_R13.0_365-gf8a97bda2a_winx64_ifort190.exe.

Perform required imports

Peform the required imports.

import os
import sys


from ansys.dyna.core.pre import launch_dynapre
from ansys.dyna.core.pre.dynamech import (
    DynaMech,
    ThermalAnalysis,
    ThermalAnalysisType,
    SolidPart,
    SolidFormulation,
    NodeSet,
    AnalysisType
)
from ansys.dyna.core.pre.dynamaterial import MatElasticPlasticThermal
from ansys.dyna.core.pre import examples
from ansys.dyna.core.pre.misc import check_valid_ip

Start the pre service

Before starting the pre service, you must ensure that the Docker container for this service has been started. For more information, see “Start the Docker container for the pre service” in https://dyna.docs.pyansys.com/version/stable/index.html.

The pre service can also be started locally, please download the latest version of ansys-pydyna-pre-server.zip package from ansys/pydyna and start it refering to the README.rst file in this server package.

Once the pre servic is running, you can connect a client to it using the hostname and the port. This example uses the default local host and port ("localhost" and "50051" respectively).

hostname = "localhost"
if len(sys.argv) > 1 and check_valid_ip(sys.argv[1]):
    hostname = sys.argv[1]
solution = launch_dynapre(ip = hostname)

Start the solution workflow

NODES and ELEMENTS are read in from the thermal_stress.k file. This file also has the PART defined in it, but the section and material fields are empty to begin with.

fns = []
path = examples.thermal_stress + os.sep
fns.append(path + "thermal_stress.k")
solution.open_files(fns)

ret: true

Set simulation termination time

Set the simulation termination time.

solution.set_termination(3.0)

To invoke the transient thermal solver, set the thermal analysis type for CONTROL_SOLUTION to 2 by ThermalAnalysisType.TRANSIENT.

ts = DynaMech(analysis=AnalysisType.EXPLICIT)
solution.add(ts)

tanalysis = ThermalAnalysis()
tanalysis.set_timestep(initial_timestep=0.1)
tanalysis.set_solver(analysis_type=ThermalAnalysisType.TRANSIENT)
ts.add(tanalysis)

ts.set_timestep(timestep_size_for_mass_scaled=0.01)

Define material and section properties

Define the MAT_4 material, which can have temperature-dependent properties. For the MAT_THERMAL_ISOTROPIC property, which is associated with the same part, define the specific heat, thermal conductivity, and thermal generation rate.

mat = MatElasticPlasticThermal(
    mass_density=1.0,
    temperatures=(0,10,20,30,40,50),
    young_modulus=(1e10,1e10,1e10,1e10,1e10,1e10),
    poisson_ratio=(0.3,0.3,0.3,0.3,0.3,0.3),
    thermal_expansion=(0,2e-6,4e-6,6e-6,8e-6,1e-5),
    yield_stress = (1e20,1e20,1e20,1e20,1e20,1e20)
)
mat.set_thermal_isotropic(density=1,generation_rate_multiplier=10,specific_heat=1,conductivity=1)

slab = SolidPart(1)
slab.set_material(mat)
slab.set_element_formulation(SolidFormulation.CONSTANT_STRESS_SOLID_ELEMENT)
ts.parts.add(slab)

Set initial conditions

Initialize nodes 1 through 8 with a temperature of 10 degrees.

for i in range(1,9):
    ts.initialconditions.create_temperature(NodeSet([i]),temperature=10)

Define output frequencies and save input file

Define output frequencies and save the input file to disk.

solution.set_output_database(glstat=0.03)
solution.create_database_binary(dt=0.01)
solution.save_file()

'/server/output'