The next few sections show how to preprocessing, solve, and postprocessing a ball plate example.

Preprocessing

The following code processes a ball plate example. In the repository, you can get the input file from src/ansys/dyna/core/pre/examples/explicit/ball_plate/ball_plate.k and the Python file from examples/Explicit/ball_plate.py.

import os
import sys
from ansys.dyna.core.pre import launch_dynapre
from ansys.dyna.core.pre.dynamech import (
    DynaMech,
    Velocity,
    PartSet,
    ShellPart,
    SolidPart,
    NodeSet,
    Contact,
    ContactSurface,
    ShellFormulation,
    SolidFormulation,
    ContactType,
    AnalysisType
)
from ansys.dyna.core.pre.dynamaterial import (
    MatRigid,
    MatPiecewiseLinearPlasticity,
)
from ansys.dyna.core.pre import examples

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

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

solution.set_termination(termination_time=10)

ballplate = DynaMech(AnalysisType.NONE)
solution.add(ballplate)

matrigid = MatRigid(mass_density=7.83e-6, young_modulus=207, poisson_ratio=0.3)
matplastic = MatPiecewiseLinearPlasticity(mass_density=7.83e-6, young_modulus=207, yield_stress=0.2, tangent_modulus=2)

plate = ShellPart(1)
plate.set_element_formulation(ShellFormulation.BELYTSCHKO_TSAY)
plate.set_material(matplastic)
plate.set_thickness(1)
plate.set_integration_points(5)
ballplate.parts.add(plate)

ball = SolidPart(2)
ball.set_material(matrigid)
ball.set_element_formulation(SolidFormulation.CONSTANT_STRESS_SOLID_ELEMENT)
ballplate.parts.add(ball)

selfcontact = Contact(type=ContactType.AUTOMATIC)
surf1 = ContactSurface(PartSet([1, 2]))
selfcontact.set_slave_surface(surf1)
ballplate.contacts.add(selfcontact)

spc = [34,35,51,52,68,69,85,86,102,103,119,120,136,137,153,154,170,171,187,188,204,205,221,222,238,239,255,256]
for i in range(1,19):
    spc.append(i)
for i in range(272,290):
    spc.append(i)
ballplate.boundaryconditions.create_spc(NodeSet(spc),rx=False,ry=False,rz=False)

for i in range(1,1652):
    ballplate.initialconditions.create_velocity_node(i,trans=Velocity(0, 0, -10))

solution.set_output_database(glstat=0.1, matsum=0.1, sleout=0.1)
solution.create_database_binary(dt=1)
serverpath = solution.save_file()

serveroutfile = '/'.join((serverpath,"ball_plate.k"))
downloadpath = os.path.join(os.getcwd(), "output")
if not os.path.exists(downloadpath):
    os.makedirs(downloadpath)
downloadfile = os.path.join(downloadpath,"ball_plate.k")
solution.download(serveroutfile,downloadfile)

Solve

The following code solves this basic ball plate example. In the repository, you can get the Python file from examples/solver/ball_plate_solver.py.

import ansys.dyna.core.solver as solver

hostname = "localhost"
port = "5000"
dyna=launch_dyna(ip = hostname,port = port)            # connect to the container
dyna.push("./output/ball_plate.k")                            # push an input file
dyna.start(4)                                   # start 4 ranks of mppdyna
dyna.run("i=ball_plate.k memory=10m ncycle=20000")   # begin execution

Post processing

The following code processes results from the solve of this basic ball plate example:

from ansys.dpf import core as dpf
import os

ds = dpf.DataSources()
data_path = os.path.join(os.getcwd(), 'd3plot')
ds.set_result_file_path(data_path, 'd3plot')

model = dpf.Model(ds)
# Extract displacements for all time steps from d3plot
D = model.results.displacement.on_all_time_freqs().eval()
D.animate()

stress = dpf.operators.result.stress()
stress.inputs.data_sources(ds)
stress.inputs.time_scoping([12])
stress.connect(25, [1])
stress.inputs.requested_location.connect("Nodal")
fields = stress.outputs.fields_container()

shell_layer_extract = dpf.operators.utility.change_shell_layers()
shell_layer_extract.inputs.fields_container.connect(fields)
print(shell_layer_extract.inputs.e_shell_layer)
shell_layer_extract.inputs.e_shell_layer.connect(0)
fields_top = shell_layer_extract.outputs.fields_container_as_fields_container()
print(fields_top)
fields_top.animate()

For more examples, see Examples in the PyDYNA documentation.