APDL Math overview#

APDL Math provides the ability to access and manipulate the large sparse matrices and solve a variety of eigenproblems. PyMAPDL classes and bindings present APDL Math in a similar manner to the popular numpy and scipy libraries. The APDL Math command set is based on tools for manipulating large mathematical matrices and vectors that provide access to standard linear algebra operations, access to the powerful sparse linear solvers of ANSYS Mechanical APDL (MAPDL), and the ability to solve eigenproblems.

Python and MATLAB eigensolvers are based on the publicly available LAPACK libraries and provides reasonable solve time for relatively small degrees of freedom (dof) eigenproblems of perhaps 100,000. However, Ansys solvers are designed for the scale of 100 s of millions of dof, providing a variety of situations where you can directly leverage Ansys high-performance solvers on a variety of eigenproblems. Fortunately, you can leverage this without relearning an entirely new language because APDL Math has been written in a similar manner as the numpy and scipy libraries. For example, here is a comparison between the NumPy and SciPy linear algebra solvers and the Ansys MAPDL Math solver:

numpy vs PyMAPDL Math Implementation#

numpy and scipy


k_py = k + sparse.triu(k, 1).T
m_py = m + sparse.triu(m, 1).T
n = 10
ev = linalg.eigsh(k_py, k=neqv, M=m_py)
k = mm.matrix(k_py, triu=True)
m = mm.matrix(m_py, triu=True)
n = 10
ev = mm.eigs(n, k, m)

What follows is a basic example and a detailed description of the PyMAPDL Math API. For additional PyMAPDL Math examples, see PyMAPDL math examples.

MAPDL matrix example#

This example demonstrates how to send an MAPDL Math matrix from MAPDL to Python and then send it back to be solved. While this example runs the MapdlMath.eigs() method on mass and stiffness matrices generated from MAPDL, you could instead use mass and stiffness matrices generated from an external FEM tool or even modify the mass and stiffness matrices within Python.

First, solve the first 10 modes of a 1 x 1 x 1 steel meter cube in MAPDL.

import re

from ansys.mapdl.core import launch_mapdl

mapdl = launch_mapdl()

# setup the full file
mapdl.block(0, 1, 0, 1, 0, 1)
mapdl.et(1, 186)

# Define a material (nominal steel in SI)
mapdl.mp("EX", 1, 210e9)  # Elastic moduli in Pa (kg/(m*s**2))
mapdl.mp("DENS", 1, 7800)  # Density in kg/m3
mapdl.mp("NUXY", 1, 0.3)  # Poisson's Ratio

# solve first 10 non-trivial modes
out = mapdl.modal_analysis(nmode=10, freqb=1)

# store the first 10 natural frequencies
resp = mapdl.set("LIST")
w_n = np.array(re.findall(r"\s\d*\.\d\s", resp), np.float32)

You now have solved for the first 10 modes of the cube:

[1475.1 1475.1 2018.8 2018.8 2018.8 2024.8 2024.8 2024.8 2242.2 2274.8]

Next, load the mass and stiffness matrices that are stored by default in the <jobname>.full file. First, create an instance of the MapdlMath class as mm:

mm = mapdl.math

# load by default from file.full
k = mm.stiff()
m = mm.mass()

# convert to numpy
k_py = k.asarray()
m_py = m.asarray()

After running the Mapdl.clear() method, these matrices are stored solely within Python.

(0, 0)      37019230769.223404
(0, 1)      10283119658.117708
(0, 2)      10283119658.117706
:   :
(240, 241)  11217948717.943113
(241, 241)  50854700854.68495
(242, 242)  95726495726.47179

The final step is to send these matrices back to MAPDL to be solved. While you have cleared MAPDL, you could have shut down MAPDL or even transferred the matrices to a different MAPDL session to be solved:

my_stiff = mm.matrix(k_py, triu=True)
my_mass = mm.matrix(m_py, triu=True)

# solve for the first 10 modes above 1 Hz
nmode = 10
mapdl_vec = mm.eigs(nmode, my_stiff, my_mass, fmin=1)
eigval = mapdl_vec.asarray()

As expected, the natural frequencies obtained from the MapdlMath.eigs() method is identical to the result from the Mapdl.solve() method within MAPDL.

[1475.1333421  1475.1333426  2018.83737064 2018.83737109 2018.83737237
 2024.78684466 2024.78684561 2024.7868466  2242.21532585 2274.82997741]

If you want to obtain the eigenvectors as well as the eigenvalues, initialize a matrix eigvec and send that to the MapdlMath.eigs() method:

>>> nmode = 10
>>> eigvec = mm.zeros(my_stiff.nrow, nmode)  # for eigenvectors
>>> val = mm.eigs(nmode, my_stiff, my_mass, fmin=1)

The MAPDL Math matrix eigvec now contains the eigenvectors for the solution.

APDL Math reference#

For more information, see MapdlMath module.