Keyword and run example

The next few sections show how to generate, preview, solve, and review a Taylor bar impact problem. An example of a sweep over impact velocities for this problem can be found in this repository at examples/Taylor_Bar/plot_taylor_bar_example.py.

Preprocessing

The following code describes an LS-DYNA Model for a Taylor bar impact problem. It assumes that the mesh file taylor_bar_mesh.k exists in the working directory. This mesh file can be found in this repository at examples/Taylor_Bar/taylor_bar_mesh.k.

import pandas as pd

from ansys.dyna.core import Deck, keywords as kwd

# construct a new Deck
deck = Deck()

# Define material
mat_1 = kwd.Mat003(mid=1)
mat_1.ro = 7.85000e-9
mat_1.e = 150000.0
mat_1.pr = 0.34
mat_1.sigy = 390.0
mat_1.etan = 90.0

# Define section
sec_1 = kwd.SectionSolid(secid=1)
sec_1.elform = 1

# Define part
part_1 = kwd.Part()
part_1.parts = pd.DataFrame({"pid": [1], "mid": [mat_1.mid], "secid": [sec_1.secid]})

# Define coordinate system
cs_1 = kwd.DefineCoordinateSystem(cid=1)
cs_1.xl = 1.0
cs_1.yp = 1.0

 # Define initial velocity
init_vel = kwd.InitialVelocityGeneration()
init_vel.id = part_1.parts["pid"][0]
init_vel.styp = 2
init_vel.vy = 300.0e3 # mm/s
init_vel.icid = cs_1.cid

# Define box for node set
box_1 = kwd.DefineBox(boxid=1, xmn=-500, xmx=500, ymn=39.0, ymx=40.1, zmn=-500, zmx=500)

# Create node set
set_node_1 = kwd.SetNodeGeneral()
set_node_1.sid = 1
set_node_1.option = "BOX"
set_node_1.e1 = box_1.boxid

# Define rigid wall
rw = kwd.RigidwallPlanar(id=1)
rw.nsid = set_node_1.sid
rw.yt = box_1.ymx
rw.yh = box_1.ymn

# Define control termination
control_term = kwd.ControlTermination(endtim=8.00000e-5, dtmin=0.001)

# Define database cards
deck_dt_out = 8.00000e-8
deck_glstat = kwd.DatabaseGlstat(dt=deck_dt_out, binary=3)
deck_matsum = kwd.DatabaseMatsum(dt=deck_dt_out, binary=3)
deck_nodout = kwd.DatabaseNodout(dt=deck_dt_out, binary=3)
deck_elout = kwd.DatabaseElout(dt=deck_dt_out, binary=3)
deck_rwforc = kwd.DatabaseRwforc(dt=deck_dt_out, binary=3)
deck_d3plot = kwd.DatabaseBinaryD3Plot(dt=4.00000e-6)

# Define deck history node
deck_hist_node_1 = kwd.DatabaseHistoryNodeSet(id1=set_node_1.sid)

# Insert all these cards into the Deck
deck.extend(
    [
        deck_glstat,
        deck_matsum,
        deck_nodout,
        deck_elout,
        deck_rwforc,
        deck_d3plot,
        set_node_1,
        control_term,
        rw,
        box_1,
        init_vel,
        cs_1,
        part_1,
        mat_1,
        sec_1,
        deck_hist_node_1,
    ]
)

# Add keyword that imports the mesh
deck.append(kwd.Include(filename="taylor_bar_mesh.k"))

Preview

The following code opens a 3D graphics window to preview the mesh for the LS-DYNA Model

# Preview the model
deck.plot()

Write to file

The following code writes the LS-DYNA model to an input.k keyword file in the working directory.

# Convert deck to string
deck_string = deck.write()

# Create LS-DYNA input deck
with open("input.k", "w") as file_handle:
    file_handle.write(deck_string)

Solve

The following code runs LS-DYNA using the input.k file.

import os

from ansys.dyna.core.run import run_dyna

# Run LS-DYNA
run_dyna("input.k")

# Confirm that the results exist
assert os.path.isfile("d3plot")
assert os.path.isfile("lsrun.out.txt")

Post processing

The following code processes results and generates a line chart of Time vs. Energy from the impact. This requires an installation of a matplotlib backend.

import matplotlib.pyplot as plt
import ansys.dpf.core as dpf

ds = dpf.DataSources()
ds.set_result_file_path("d3plot", "d3plot")
model = dpf.Model(ds)

gke_op = dpf.operators.result.global_kinetic_energy()
gke_op.inputs.data_sources.connect(ds)
gke = gke_op.eval()
field = gke.get_field(0)
ke_data = field.data

time_data = model.metadata.time_freq_support.time_frequencies.data_as_list

plt.plot(time_data, ke_data, "b", label="Kinetic Energy")
plt.xlabel("Time (s)")
plt.ylabel("Energy (mJ)")
plt.show()

Pre and solver example

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.