The DPF Model¶
The DPF model is the basic starting point for opening a file through DPF. From here you can connect various operators and display results and data from the result file.
To create a Model instance, import dpf and load a file. The
path provided must be an absolute path or a path relative to the DPF
server.
from ansys.dpf import core as dpf
from ansys.dpf.core import examples
path = examples.simple_bar
model = dpf.Model(path)
Printing the model (or any other instance) ca be useful to understand what is available in the result file
print(model)
Out:
DPF Model
------------------------------
DPF Result Info
Analysis: static
Physics Type: mecanic
Unit system: MKS: m, kg, N, s, V, A, degC
Available results:
U Displacement :nodal displacements
ENF Element nodal Forces :element nodal forces
ENG_VOL Volume :element volume
ENG_SE Energy-stiffness matrix :element energy associated with the stiffness matrix
ENG_AHO Hourglass Energy :artificial hourglass energy
ENG_TH thermal dissipation energy :thermal dissipation energy
ENG_KE Kinetic Energy :kinetic energy
ENG_CO co-energy :co-energy (magnetics)
ENG_INC incremental energy :incremental energy (magnetics)
BFE Temperature :element structural nodal temperatures
------------------------------
DPF Meshed Region:
3751 nodes
3000 elements
Unit: m
With solid (3D) elements
------------------------------
DPF Time/Freq Support:
Number of sets: 1
Cumulative Time (s) LoadStep Substep
1 1.000000 1 1
For a full example using the model, see Basic DPF-Core Usage.
For a full description of the Model object, see the APIs section Model.
Model Metadata¶
The metadata of the model can be used to access all the information about an analysis:
the type of analysis
the time or frequencies description
the mesh
the available results
For example, you can get the analysis type with:
model.metadata.result_info.analysis_type
Out:
'static'
You can get information about the mesh:
>>> model.metadata.meshed_region.nodes.n_nodes
>>> model.metadata.meshed_region.elements.n_elements
>>> print(model.metadata.meshed_region.elements.element_by_id(1))
Out:
3751
3000
DPF Element 1
Index: 1400
Nodes: 8
Type: element_types.Hex8
Shape: Solid
You can the time sets with:
time_freq_support = model.metadata.time_freq_support
print(time_freq_support.time_frequencies.data)
Out:
[1.]
For a full description of the Metadata object, see the APIs section Model.
Model Results¶
The model contains the results attribute, which you can use to
create operators to access certain results. To view the available
results, print them with:
print(model.results)
Out:
- DPF Result Info
Analysis: static Physics Type: mecanic Unit system: MKS: m, kg, N, s, V, A, degC Available results:
U Displacement :nodal displacements ENF Element nodal Forces :element nodal forces ENG_VOL Volume :element volume ENG_SE Energy-stiffness matrix :element energy associated with the stiffness matrix ENG_AHO Hourglass Energy :artificial hourglass energy ENG_TH thermal dissipation energy :thermal dissipation energy ENG_KE Kinetic Energy :kinetic energy ENG_CO co-energy :co-energy (magnetics) ENG_INC incremental energy :incremental energy (magnetics) BFE Temperature :element structural nodal temperatures
- Model.results
Available results of the model. Organize the results from DPF into accessible methods. All the available results are dynamically created depending on the model’s ‘ResultInfo’
- Returns
Available results of the model
- Return type
- all types of results
Result provider helper wrapping all types of provider available for a given result file
Examples
Create a stress result from the model and choose its time and mesh scopings
>>> from ansys.dpf import core as dpf >>> from ansys.dpf.core import examples >>> model = dpf.Model(examples.electric_therm) >>> v = model.results.electric_potential >>> rf = model.results.reaction_force >>> dissip = model.results.thermal_dissipation_energy
- Type
Examples
Extract the result object from a model.
>>> from ansys.dpf import core as dpf >>> from ansys.dpf.core import examples >>> model = dpf.Model(examples.simple_bar) >>> results = model.results # printable object
Access the displacement at all times
>>> from ansys.dpf.core import Model >>> from ansys.dpf.core import examples >>> transient = examples.download_transient_result() >>> model = Model(transient) >>> displacements = model.results.displacement.on_all_time_freqs.eval()
Choosing the time or frequencies or the spatial subset on which to get a given result
is straightforward with this results attribute:
disp_result = model.results.displacement
disp_at_all_times_on_node_1 = disp_result.on_all_time_freqs.on_mesh_scoping([1])
For a full example using the Result API, see Go Easily over Times Transient Analysis.
For a full description of the Model object, see the APIs section Results.