Export results to VTK format

I am trying to export each time step of my analysis (available as rst file) into the VTK format using a python script and ansys.dpf.core. I don't want to save the whole model, but only a selection of elements, which I have as named_selection. This seems to work in general with my script (see below).

The problem I have is that the stress tensor is not written for some reason. It doesn't matter if I write it into fields1 or fields2. I would also like to export other results (e.g. total strain) but the operator only has two variables for fields. Is there a way to save more than two results?

Finally, I would like to assign a name to the results. At the moment the result of the displacement is called e.g. "3_displacement_1.s_()" in the first time step, "3_displacement_2.s_()" in the second time step and "3_displacement_3.s_() in the third time step. Can I rename the result so that the displacement in each time step is called "displacement" or "displ"?

Here is my code so far:

from ansys.dpf import core
from ansys.dpf.core import operators as ops

rst = "model.rst"
model = core.Model(rst)


mesh_scoping = core.mesh_scoping_factory.named_selection_scoping("myElements", model=model)
mesh_op = core.operators.mesh.from_scoping()
mesh_op.inputs.mesh.connect(model.metadata.meshed_region)
mesh_op.inputs.scoping.connect(mesh_scoping)


for time in range(1, model.metadata.time_freq_support.n_sets+1):
    results = model.results
    displacement = results.displacement(time_scoping = time)
    displ_vector = displacement.outputs.fields_container()
    stress = results.stress(time_scoping = time)
    stress_tensor = stress.outputs.fields_container()   # This is somehow not exported
    
    op_export = core.Operator("vtk_export")
    op_export.inputs.file_path.connect(f"export_{time}.vtk")
    op_export.inputs.mesh.connect(mesh_op)
    op_export.inputs.fields1.connect(displ_vector)
    op_export.inputs.fields2.connect(stress_tensor)
    op_export.run()

Speaking of which: Can i format the code in the post so that it looks pretty?

Find more posts tagged with

Python

PyAnsys

PyDPF

Accepted answers

Pernelle Marone-Hitz

Hi again @Sven Lohmann , to answer your other questions:

Can you please check that your result file indeed contains stress results ? You can print this to the console through print(model). On my side I see that the stress is saved to the .rst file:

2023-01-11 16_38_59-Spyder (Python 3.8).png

and I can check the stress data through:

stress = model.results.stress()
data = stress.outputs.fields_container.get_data()
print(data)

Here is an example of exporting to vtk:

from ansys.dpf import core as dpf 
my_file_path = r'D:/test/export/file.rst'
my_data_sources = dpf.DataSources(my_file_path)
my_model = dpf.Model(my_data_sources)
my_mesh = my_model.metadata.meshed_region 
u_op = my_model.results.displacement()
my_export = dpf.operators.serialization.vtk_export()
my_export.inputs.file_path.connect(r'D:/test/export/fileNew.vtk')
my_export.inputs.fields1.connect(u_op.outputs.fields_container)
my_export.inputs.mesh.connect(my_mesh)
my_export.run()

The vtk_export operator only allows two fields (https://dpf.docs.pyansys.com/api/ansys.dpf.core.operators.serialization.vtk_export.html?highlight=vtk#module-ansys.dpf.core.operators.serialization.vtk_export). The way to go here will be to export one vtk file per result that you want to export.

Pernelle Marone-Hitz

Hi @Sven Lohmann , after checking with the dev team they confirmed that vtk_export() does not support ElementalNodal results (as you have experienced). However you can look into vtu_export that should be able to do that.

All comments

Pernelle Marone-Hitz

Hi @Sven Lohmann , this post should help you for the last part of your question: https://discuss.ansys.com/discussion/1887/how-do-i-use-the-text-editor#latest

Please give us a little bit more time to address the technical question, we'll get back to you shortly!

Pernelle Marone-Hitz

Hi again @Sven Lohmann , to answer your other questions:

Can you please check that your result file indeed contains stress results ? You can print this to the console through print(model). On my side I see that the stress is saved to the .rst file:

and I can check the stress data through:

stress = model.results.stress()
data = stress.outputs.fields_container.get_data()
print(data)

Here is an example of exporting to vtk:

from ansys.dpf import core as dpf 
my_file_path = r'D:/test/export/file.rst'
my_data_sources = dpf.DataSources(my_file_path)
my_model = dpf.Model(my_data_sources)
my_mesh = my_model.metadata.meshed_region 
u_op = my_model.results.displacement()
my_export = dpf.operators.serialization.vtk_export()
my_export.inputs.file_path.connect(r'D:/test/export/fileNew.vtk')
my_export.inputs.fields1.connect(u_op.outputs.fields_container)
my_export.inputs.mesh.connect(my_mesh)
my_export.run()

James Derrick

Hi @Sven Lohmann, welcome to the forum! @Pernelle Marone-Hitz is correct concerning the code formatting. I've edited your post for now, to change the code to a code block, although I think you still need to fix the indentation to get the code highlighting to work properly.

Additionally, you should have a look at the posts in the "Miscellaneous" category as there is a lot of guidance there around how to get the most out of the forum. 😊

Sven Lohmann

Hi @James Derrick

Thanks for adjusting the code. I have tweaked the code block further, however, it seems that it is not formatted properly until the comments are removed completely. After a #, all lines that come after that seem to be interpreted as comments.

I will have a look in the misc section.

Hi @Pernelle Marone-Hitz

Thanks for the help. My rst file contains stress as ElementalNodal Stress:

DPF Model
------------------------------
Static analysis
Unit system: SI: m, kg, N, s, V, A, K
Physics Type: Mecanic
Available results:
     -  displacement: Nodal Displacement
     -  reaction_force: Nodal Force   
     -  element_nodal_forces: ElementalNodal Element nodal Forces
     -  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
     -  thermal_strain: ElementalNodal Thermal Strains
     -  thermal_strains_eqv: ElementalNodal Thermal Strains eqv
     -  swelling_strains: ElementalNodal Swelling Strains
     -  structural_temperature: ElementalNodal Temperature
------------------------------
DPF  Meshed Region: 
  3111730 nodes 
  868247 elements 
  Unit:  
  With solid (3D) elements, shell (2D) elements, shell (3D) elements, beam (1D) elements
------------------------------
DPF  Time/Freq Support: 
  Number of sets: 3 
Cumulative     Time (s)       LoadStep       Substep         
1              1.000000       1              1               
2              2.000000       2              1               
3              3.000000       3              1

And the output also says that data would be available:

>>> print(stress_tensor)
DPF stress(s)Fields Container
  with 1 field(s)
  defined on labels: time 


  with:
  - field 0 {time:  1} with ElementalNodal location, 6 components and 794853 entities.

The output differs only between that of displacement in the location (ElementalNodal instead of Nodal):

>>> print(displ_vector)
DPF displacement(s)Fields Container
  with 1 field(s)
  defined on labels: time 


  with:
  - field 0 {time:  1} with Nodal location, 3 components and 3111730 entities.

Is it possible that VTK cannot store ElementalNodal information? Do they have to be converted to Nodal first?

EDIT:

Indeed, it seems that ElementalNodal results are not written to VTK. I have converted the result to Nodal with:

stress = results.stress(time_scoping = time)
stress_tensor = stress.outputs.fields_container()
stress_tensor_nodal = core.operators.averaging.elemental_nodal_to_nodal(
    field = stress_tensor,
).eval()
op_export.inputs.fields2.connect(stress_tensor_nodal)

and now it works.

Pernelle Marone-Hitz

Sven Lohmann

Thank you very much, i will have a closer look.