How do I interpret .rst results file with python using pyansys library?

I am reading the binary files '.rst' using the ansys.mapdl library reader, and I want to understand those results. I have a beam simulated on ansys mechanical and I am evaluating total deformation, equivalent elastic strain and equivalent stress.

What nodes are associated with which values? How are all three results separated? Also, I tried printing random data just to try and make sense of it but some data are NAN, so I would like to know why that is the case.

Here is the simulation and some code

EDIT: Here is total deformation for the first 10 nodes exported from ansys mechanical to a .txt file

Node Number Total Deformation (m)
1   3,4011e-002
2   3,1337e-002
3   2,8684e-002
4   2,6064e-002
5   2,3489e-002
6   2,097e-002
7   1,8522e-002
8   1,6157e-002
9   1,389e-002
10  1,1736e-002

Here are my results after running this small script

rst_results = path + "file.rst"
model = pymapdl_reader.read_binary(rst_results)
nnum, data = model.nodal_solution(0, nodes=range(1, 10))
print(data)

output:

[[-1.30837114e-03 -5.18717535e-07 -3.39862333e-02]
 [-1.19035991e-03 -6.35982671e-07 -3.13144870e-02]
 [-1.07379301e-03 -8.05693695e-07 -2.86642968e-02]
 [-9.59576794e-04 -1.01205615e-06 -2.60467228e-02]
 [-8.48646606e-04 -1.24353973e-06 -2.34735376e-02]
 [-7.41942455e-04 -1.49284317e-06 -2.09571697e-02]
 [-6.40385662e-04 -1.75494961e-06 -1.85106729e-02]
 [-5.44855004e-04 -2.02586199e-06 -1.61477097e-02]
 [-4.56160962e-04 -2.30167900e-06 -1.38825364e-02]]

From the docs:

def principal_nodal_stress(self, rnum, nodes=None):
    """Computes the principal component stresses for each node in
    the solution.
    Parameters
    ----------
    rnum : int or list
        Cumulative result number with zero based indexing, or a
        list containing (step, substep) of the requested result.
    Returns
    -------
    nodenum : numpy.ndarray
        Node numbers of the result.
    pstress : numpy.ndarray
        Principal stresses, stress intensity, and equivalent stress.
        [sigma1, sigma2, sigma3, sint, seqv]
    Examples
    --------
    Load the principal nodal stress for the first solution.
    >>> from ansys.mapdl import reader as pymapdl_reader
    >>> rst = pymapdl_reader.read_binary('file.rst')
    >>> nnum, stress = rst.principal_nodal_stress(0)

So each number in your nodal number array nnum correspond to the stresses in stress.

Can you check which node numbers correspond to midside nodes? Nodal stress data for printout and postprocessing are available only for the corner nodes. So I would guess that's the reason for the nan.

For nodal displacements:

    >>> from ansys.mapdl import reader as pymapdl_reader
    >>> rst = pymapdl_reader.read_binary('file.rst')
    >>> nnum, data = rst.nodal_solution(0)

For elastic strain you need an element result:

    >>> enum, edata, enode = rst.element_solution_data(0, datatype='EEL')
    >>> enum[0]  # first element number
    >>> enode[0]  # nodes belonging to element 1
    >>> edata[0]  # data belonging to element 1

The available results are:

        EMS: misc. data
        ENF: nodal forces
        ENS: nodal stresses
        ENG: volume and energies
        EGR: nodal gradients
        EEL: elastic strains
        EPL: plastic strains
        ECR: creep strains
        ETH: thermal strains
        EUL: euler angles
        EFX: nodal fluxes
        ELF: local forces
        EMN: misc. non-sum values
        ECD: element current densities
        ENL: nodal nonlinear data
        EHC: calculated heat
        EPT: element temperatures
        ESF: element surface stresses
        EDI: diffusion strains
        ETB: ETABLE items (post1 only)
        ECT: contact data
        EXY: integration point locations
        EBA: back stresses
        ESV: state variables
        MNL: material nonlinear record