Access results

After a result file is loaded, you can access the results themselves. You can query results using dedicated methods.

This code shows how to instantiate the Simulation object and then get the displacement result for a loaded simulation:

Instantiate the simulation object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> simulation = post.load_simulation(examples.multishells_rst)

Extract the displacement data as a DataFrame object

>>> displacement = simulation.displacement()
>>> # stress, elastic_strain (...) can also be called.

See the following list for the results that can be
extracted.

You can use keyword arguments to specify additional options, including the components, scope, and time. For detailed examples, see Use keywords to get a more precise result.

PyDPF-Post supports two types of result files:

• Structural (RST)

• Thermal/electric (RTH) (with the legacy load_solution() method only)

It also supports some LS-DYNA result files and some Fluent and CFX result files as indicated in solver_result_files_support.

You should only request results available in the result file. To determine which results are available, see Browse result file metadata.

Structural result files

You can use the legacy Solution object to access structural results.

After loading a Solution object from a structural analysis result (RST) file, you can query these Result objects:

• displacement

• stress

• elastic_strain

• plastic_strain

• structural_temperature

Displacement

Displacement is the DOF solution for a structural analysis. The location argument for a DOF solution must be modal.

This code shows how to access the Displacement result object:

# Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the displacement result object

>>> displacement = solution.displacement()

The displacement Result object corresponds to a vector field. To obtain the scalar components (y-components) of this field, access the subresult with this code:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the displacement result object

>>> displacement = solution.displacement()

Get the y displacement result data

>>> u_y = displacement.y
>>> u_y.get_data_at_field()

For more information, see ResultData class.

Stress

This code shows to access the Stress result object:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

# Instantiate the stress result object

>>> stress = solution.stress()

A Stress result object corresponds to a tensor field. To obtain the scalar components of this field, such as the normal y-stresses, access the subresult:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the stress result object

>>> stress = solution.stress()

Get the yy stress result data

>>> s_yy = stress.yy
>>> s_yy.get_data_at_field()

You can query other components, as well as whole tensor data, accordingly. For more information, see ResultData class.

Elastic and plastic strain

This code shows how to access the ElasticStrain and PlasticStrain result objects:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the strain result objects

>>> elastic_strain = solution.elastic_strain()
>>> plastic_strain = solution.plastic_strain()

A Strain result object corresponds to a tensor field. To obtain the scalar components of this field, such as the shear xy-strains, access the subresult:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the elastic strain result object

>>> elastic_strain = solution.elastic_strain()

Get the xy elastic strain result data

>>> e_yy = elastic_strain.xy
>>> e_yy.get_data_at_field()

You can query other components, as well as whole tensor data, accordingly. For more information, see ResultData class.

Structural temperature

This code shows to access the StructuralTemperature result object:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the structural temperature result object

>>> structural_temperature = solution.structural_temperature()

To access the temperature scalar field, use this code:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the structural temperature result object

>>> structural_temperature = solution.structural_temperature()

Get the structural temperature result data

>>> temperature = structural_temperature.scalar
>>> temperature.get_data_at_field()

Miscellaneous results

The Solution object might contain other miscellaneous ansys.dpf.post.misc_results.MecanicMisc result objects that you can access. For example, this code shows how to access the nodal_acceleration result object:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Get the nodal acceleration result data

>>> acceleration = solution.misc.nodal_acceleration()

All keyword arguments are available for miscellaneous results, except location. For more information, see Use keywords to get a more precise result.

Some subresults might be available as keyword arguments, such as the scalar components of nodal acceleration:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Get the result data

>>> acceleration = solution.misc.nodal_acceleration(subresult="Y")

To determine available queries, you can browse the metadata in the result file. For more information, see Browse result file metadata.

Thermal/electric result files

You can access thermal/electric results using the legacy Solution object.

After loading a Solution object from a thermal/electric analysis result file (RTH), you can query these Result objects:

• temperature

• heat_flux

• electric_field

• electric_potential

Temperature

Temperature is the DOF solution for a thermal analysis.

This code shows how to access the Temperature result object:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.steady_therm)

Instantiate the temperature result object

>>> temperature = solution.temperature()

As inferred above, the location argument for a DOF solution must be nodal. This code shows how to access the scalar field directly:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the temperature result object

>>> temperature = solution.temperature()

Get the y temperature result data

>>> temp = temperature.scalar
>>> temp.get_data_at_field()

Heat flux

This code shows how to access the HeatFlux result object:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.steady_therm)

Instantiate the heat_flux result object

>>> heat_flux = solution.heat_flux()

The HeatFlux result object corresponds to a vector field. To obtain the scalar components (x-components) of this field, access the subresult:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the temperature result object

>>> heat_flux = solution.heat_flux()

Get the y heat_flux result data

>>> heat_flux_x = heat_flux.x
>>> heat_flux_x.get_data_at_field()

You can query other components accordingly. For more information, see ResultData class.

Electric field

This code shows how to access the ElectricField result object:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.electric_therm)

Instantiate the electric field result object

>>> electric_field = solution.electric_field()

The electric_field result object corresponds to a vector field. To obtain the scalar components of this field, such as the x-components, access the subresult:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the electric field result object

>>> electric_field = solution.electric_field()

Get the y electricfield result data

>>> electric_field_x = electric_field.x
>>> electric_field_x.get_data_at_field()

For more information, see ResultData class.

Electric potential

This code shows how to access the ElectricPotential result object:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.steady_therm)

Instantiate the electric potential result object

>>> electric_potential = solution.electric_potential()

The electric_potential result object corresponds to a scalar field. You can access its values with:

Instantiate the solution object

>>> from ansys.dpf import post
>>> from ansys.dpf.post import examples
>>> solution = post.load_solution(examples.multishells_rst)

Instantiate the electric potential result object

>>> electric_potential = solution.electric_potential()

Get the y electric potential result data

>>> ep = electric_potential.scalar
>>> ep.get_data_at_field()