How to get the frequency response results of the acceleration of a NamedSelection node

[hrntsm]

I am using Mechanical for frequency response analysis. I am trying to get the results using dpf.
The code is as follows.

sim = post.load_simulation("my_result.rst")
print(sim)

The sim's DPF model returned the following
Does it not include acceleration results?
When I checked with WB, I get results that are included.

DPF Model
------------------------------
Harmonic analysis
Unit system: NMM: mm, ton, N, s, mA, degC
Physics Type: Mechanical
Available results:
     -  displacement: Nodal Displacement
     -  reaction_force: Nodal Force
     -  stress: ElementalNodal Stress
     -  elemental_volume: Elemental Volume
     -  stiffness_matrix_energy: Elemental Energy-stiffness matrix
     -  artificial_hourglass_energy: Elemental Hourglass Energy
     -  thermal_dissipation_energy: Elemental thermal dissipation energy
     -  kinetic_energy: Elemental Kinetic Energy
     -  co_energy: Elemental co-energy
     -  incremental_energy: Elemental incremental energy
     -  elastic_strain: ElementalNodal Strain
     -  structural_temperature: ElementalNodal Temperature
------------------------------

Acceleration is preferred, but if it is not included, the frequency response of the displacement of the nodes selected in Named Selection is also acceptable.
How should I get it after this?

[PProfizi]

Hi @hrntsm,

It seems that DPF did not find acceleration results in the RST file. The reason you see it available in Mechanical may be that it recomputes it. It is possible it is not stored in the RST file. @ayush-kumar-423 do you know if acceleration results are stored in RST for frequency response analyses?

Now to get the displacement fields for the nodes in a Named Selection, you should be able to follow this example despite it showcasing a modal analysis.

[ayush-kumar-423]

Hi,

@hrntsm acceleration results are not stored by default in the RST for a Harmonic Response Analysis. Mechanical calculates them as the second order derivative of displacement. For a Harmonic response, you can multiply the Displacement field with (-omega^2) to obtain acceleration. Where omega is Angular Velocity = 2*pi*f.
For multiplication you can use dpf.operators.math.scale()

[hrntsm]

Thanks @PProfizi @ayush-kumar-423 !

I was able to retrieve the results.
I see that I can output the result on the terminal when I run the following code, but how can I make a graph of the frequency response or get the value of each frequency?
Is it possible to convert the results to a numpy array or something similar?

sim = post.HarmonicMechanicalSimulation(r"my_result.rst")
disp = sim.displacement(all_sets=True, named_selections=["C_100001"])
print(disp)

             results           U                                                             ...
             set_ids           1                       2                       3             ...
             complex           0           1           0           1           0           1 ...
 node_ids components                                                                         ...
   100001          X -1.1033e-04  2.9118e-06  1.6701e-08 -6.3268e-07 -4.7175e-05  3.2532e-03 ...
                   Y  3.7236e-04 -6.4921e-06 -8.8455e-05  1.9681e-06  3.7314e-06  2.1758e-03 ...
                   Z  2.5355e-03 -6.5708e-06  1.4849e-05 -7.9472e-06 -1.3825e-04 -1.4386e-02 ...

[PProfizi]

Hi @hrntsm,
You can indeed convert a post.Dataframe to a np.array as shown in this example. The caveat is that since NumPy arrays do not have column or row labels, you must first select a column of interest before exporting it.
As for plotting graphs, we do not have yet this capability native for the post.Dataframe so for now the best way is to perform selections and filtering on the Dataframe, then query Dataframe.array, and then plot this data using Matplotlib or Plotly.

[hrntsm]

Hi @PProfizi

The results were retrieved and the process I was thinking about was done.
Thank you!