Pressure Vessel

This example demonstrates how to create a basic pressure vessel and apply a pressure to it.

Also shown here: - Various ways of accessing stress results from MAPDL. - Comparison between PRNSOL, VGET (efficient wrapping), and the legacy reader. - Notes regarding FULL vs. POWER graphics when using PRNSOL.

import numpy as np

from ansys.mapdl.core import launch_mapdl

# start mapdl, enter the preprocessor, and set the units
mapdl = launch_mapdl()

mapdl.clear()
mapdl.prep7()

# US Customary system using inches (in, lbf*s2/in, s, °F).
mapdl.units("BIN")

Set the materials and element type

mapdl.et(1, "SOLID285")
mapdl.mp("EX", 1, 10e6)
mapdl.mp("PRXY", 1, 0.3)
mapdl.mp("DENS", 1, 0.1)
print(mapdl.mplist())

Create the Geometry

# area generation
height = 10
inner_width = 2.5
outer_width = 3.5
mapdl.rectng(inner_width, outer_width, 0, height)
mapdl.cyl4(0, height, inner_width, 0, outer_width, 90)

# combine areas
a_comb = mapdl.aadd(1, 2)
mapdl.aplot(color="grey", background="w", show_area_numbering=True)

# Generate a cylindrical volume by rotating an area pattern about an axis
mapdl.vrotat(a_comb, pax1=6, arc=90)
mapdl.vplot(background="w")

Create the mesh

mapdl.smrtsize(1)
mapdl.esize(0.25, 0)
mapdl.mshape(1, "3D")
mapdl.mshkey(0)
mapdl.vmesh("ALL")
mapdl.eplot(color="grey", background="w")

Solve

# boundary condition selection
mapdl.geometry.area_select([3, 5, 7])
mapdl.da("ALL", "SYMM")
mapdl.allsel()

# apply pressure
mapdl.geometry.area_select([1, 6])
mapdl.sfa("ALL", 1, "PRES", 1000)
mapdl.allsel()

# solver
mapdl.run("/SOL")
mapdl.antype(0)
mapdl.outres("ALL", "ALL")
mapdl.run("/STATUS,SOLU")
sol_output = mapdl.solve()
mapdl.finish()

Post-Processing

Enter the MAPDL post-postprocessing routine (/POST1) and obtain the von-mises stress for the single static solution. Here, we use MAPDL directly to obtain the results using a wrapper around the VGET method to efficiently obtain results without outputting to disk.

# enter the postprocessing routine
mapdl.post1()
mapdl.set(1, 1)

# results directly from MAPDL's VGET command
# VGET, __VAR__, NODE, , S, EQV
nnum = mapdl.mesh.nnum
von_mises_mapdl = mapdl.post_processing.nodal_eqv_stress()

# we could print out the solution for each node with:

print(f"\nNode  Stress (psi)")
for node_num, stress_value in zip(nnum[:5], von_mises_mapdl[:5]):
    print(f"{node_num:<5d} {stress_value:.3f}")
print("...")

# or simply get the maximum stress value and corresponding node
idx = np.argmax(von_mises_mapdl)
node_num = nnum[idx]
stress_value = von_mises_mapdl[idx]
print(f"\nMaximum Stress")
print(f"Node  Stress (psi)")
print(f"{node_num:<5d} {stress_value:.3f}")

Plot the results

mapdl.post_processing.plot_nodal_eqv_stress(cpos="zy")

We could, alternatively, get the exact same results by directly accessing the result file using the legacy file reader ansys-mapdl-reader.

# access the result
result = mapdl.result

# Get the von Mises stress and show that this is equivalent to the
# stress obtained from MAPDL.
nnum, stress = result.principal_nodal_stress(0)
von_mises = stress[:, -1]  # von-Mises stress is the right most column
min_von_mises, max_von_mises = np.min(von_mises), np.max(von_mises)
print("All close:", np.allclose(von_mises, von_mises_mapdl))

That these results are equivalent to results from PRNSOL.

注釈

Enabling POWER GRAPHICS with mapdl.graphics('POWER') will change the averaging scheme.

mapdl.header("OFF", "OFF", "OFF", "OFF", "OFF", "OFF")
table = mapdl.prnsol("S", "PRIN").splitlines()[1:]
prnsol_eqv = np.genfromtxt(table)[:, -1]  # eqv is the last column

# show these are equivalent (RTOL due to rounding within PRNSOL)
print("All close:", np.allclose(von_mises, prnsol_eqv, rtol=1e-4))

print(f"LEGACY Reader and MAPDL VGET Min: {min_von_mises}")
print(f"PRNSOL MAPDL Min:                 {prnsol_eqv.min()}")
print()
print(f"LEGACY Reader and MAPDL VGET Min: {max_von_mises}")
print(f"PRNSOL MAPDL Min:                 {prnsol_eqv.max()}")

Stop mapdl

mapdl.exit()