Skip to content
Pythonic interface to ANSYS result, full, and archive files
Branch: master
Clone or download


This Python module allows you to:
  • Interactively control an instance of ANSYS v14.5 + using Python on Linux, >=17.0 on Windows.
  • Extract data directly from binary ANSYS v14.5+ files and to display or animate them.
  • Rapidly read in binary result (.rst), binary mass and stiffness (.full), and ASCII block archive (.cdb) files.

See the Documentation page for more details.


Installation through pip:

pip install pyansys

You can also visit GitHub to download the source.

Quick Examples

Many of the following examples are built in and can be run from the build-in examples module. For a quick demo, run:

from pyansys import examples

Controlling ANSYS

Create an instance of ANSYS and interactively send commands to it. This is a direct interface and does not rely on writing a temporary script file. You can also generate plots using matplotlib.

import os
import pyansys

path = os.getcwd()
ansys = pyansys.ANSYS(run_location=path, interactive_plotting=True)

# create a square area using keypoints
ansys.K(1, 0, 0, 0)
ansys.K(2, 1, 0, 0)
ansys.K(3, 1, 1, 0)
ansys.K(4, 0, 1, 0)
ansys.L(1, 2)
ansys.L(2, 3)
ansys.L(3, 4)
ansys.L(4, 1)
ansys.Al(1, 2, 3, 4)

Loading and Plotting an ANSYS Archive File

ANSYS archive files containing solid elements (both legacy and current), can be loaded using Archive and then converted to a vtk object.

import pyansys
from pyansys import examples

# Sample *.cdb
filename = examples.hexarchivefile

# Read ansys archive file
archive = pyansys.Archive(filename)

# Print raw data from cdb
for key in archive.raw:
   print("%s : %s" % (key, archive.raw[key]))

# Create a vtk unstructured grid from the raw data and plot it
grid = archive.parse_vtk()

# write this as a vtk xml file

You can then load this vtk file using pyvista or another program that uses VTK.

# Load this from vtk
import pyvista as pv
grid = pv.UnstructuredGrid('hex.vtu')

Loading the Result File

This example reads in binary results from a modal analysis of a beam from ANSYS.

# Load the reader from pyansys
import pyansys
from pyansys import examples

# Sample result file
rstfile = examples.rstfile

# Create result object by loading the result file
result = pyansys.open_result(rstfile)

# Beam natural frequencies
freqs = result.time_values
>>> print(freq)
[ 7366.49503969  7366.49503969 11504.89523664 17285.70459456
  17285.70459457 20137.19299035]

# Get the 1st bending mode shape.  Results are ordered based on the sorted
# node numbering.  Note that results are zero indexed
nnum, disp = result.nodal_solution(0)
>>> print(disp)
[[ 2.89623914e+01 -2.82480489e+01 -3.09226692e-01]
 [ 2.89489249e+01 -2.82342416e+01  2.47536161e+01]
 [ 2.89177130e+01 -2.82745126e+01  6.05151053e+00]
 [ 2.88715048e+01 -2.82764960e+01  1.22913304e+01]
 [ 2.89221536e+01 -2.82479511e+01  1.84965333e+01]
 [ 2.89623914e+01 -2.82480489e+01  3.09226692e-01]

Plotting Nodal Results

As the geometry of the model is contained within the result file, you can plot the result without having to load any additional geometry. Below, displacement for the first mode of the modal analysis beam is plotted using VTK.

# Plot the displacement of Mode 0 in the x direction
result.plot_nodal_solution(0, 'x', label='Displacement')

Results can be plotted non-interactively and screenshots saved by setting up the camera and saving the result. This can help with the visualization and post-processing of a batch result.

First, get the camera position from an interactive plot:

>>> cpos = result.plot_nodal_solution(0)
>>> print(cpos)
[(5.2722879880979345, 4.308737919176047, 10.467694436036483),
 (0.5, 0.5, 2.5),
 (-0.2565529433509593, 0.9227952809887077, -0.28745339908049733)]

Then generate the plot:

result.plot_nodal_solution(0, 'x', label='Displacement', cpos=cpos,
                         window_size=[800, 600], interactive=False)

Stress can be plotted as well using the below code. The nodal stress is computed in the same manner that ANSYS uses by to determine the stress at each node by averaging the stress evaluated at that node for all attached elements. For now, only component stresses can be displayed.

# Display node averaged stress in x direction for result 6
result.plot_nodal_stress(5, 'Sx')

Nodal stress can also be generated non-interactively with:

result.plot_nodal_stress(5, 'Sx', cpos=cpos, screenshot=beam_stress.png,
                       window_size=[800, 600], interactive=False)

Animating a Modal Solution

Mode shapes from a modal analsyis can be animated using animate_nodal_solution:


If you wish to save the animation to a file, specify the movie_filename and animate it with:

result.animate_nodal_solution(0, movie_filename='/tmp/movie.mp4', cpos=cpos)

Reading a Full File

This example reads in the mass and stiffness matrices associated with the above example.

# Load the reader from pyansys
import pyansys
from scipy import sparse

# load the full file
fobj = pyansys.FullReader('file.full')
dofref, k, m = fobj.load_km()  # returns upper triangle only

# make k, m full, symmetric matricies
k += sparse.triu(k, 1).T
m += sparse.triu(m, 1).T

If you have scipy installed, you can solve the eigensystem for its natural frequencies and mode shapes.

from scipy.sparse import linalg

# condition the k matrix
# to avoid getting the "Factor is exactly singular" error
k += sparse.diags(np.random.random(k.shape[0])/1E20, shape=k.shape)

# Solve
w, v = linalg.eigsh(k, k=20, M=m, sigma=10000)
# System natural frequencies
f = (np.real(w))**0.5/(2*np.pi)

print('First four natural frequencies')
for i in range(4):
    print '{:.3f} Hz'.format(f[i])
First four natural frequencies
1283.200 Hz
1283.200 Hz
5781.975 Hz
6919.399 Hz

License and Acknowledgments

pyansys is licensed under the MIT license.

ANSYS documentation and functions build from html provided by Sharcnet. Thanks!

This module, pyansys makes no commercial claim over ANSYS whatsoever. This tool extends the functionality of ANSYS by adding a python interface in both file interface as well as interactive scripting without changing the core behavior or license of the original software. The use of the interactive APDL control of pyansys requires a legally licensed local copy of ANSYS.

You can’t perform that action at this time.