Read Results at the Specific Locations

Gordon1998

Hi, there.

I am currently developing an ANSYS ACT automation tool to output deformations at specific locations. Note that these locations are different from the mesh nodes. The desired locations are described in XYZ coordinates via either a txt file or in-memory arrays (whichever is available in ANSYS).

Some say that I can load these coordinates as a name selection and set the scoping method to the name selection so that the solver can solve for the deformation of these specific locations. Or I can use the dpf module to map the deformation onto the given locations. I would appreciate it if anyone could shed light on the problem. Thanks ahead!

Rajesh Meena

@Gordon1998

The DPF way is easier here:

Refer to this example:

https://dpf.docs.pyansys.com/version/stable/examples/06-plotting/04-plot_on_path.html#sphx-glr-examples-06-plotting-04-plot-on-path-py

You can use the above example as reference and write a script either in PyDPF or mechanical DPF ( Since you are working on ACT).

Gordon1998

Rajesh, thanks for your reply.

I followed the steps in the example and applied them to my test project. My test project only has one object (sleeve) and I would like to get the Z_displacement at the target coordinates. The target coordinates are given from the txt file. However, I have problems retrieving the Z_displacement at the target coordinates: the mapped displacements have 0 fields. Would you please point out the mistakes I have in my codes? (Please change the path of the text file and solve for the model again). The text file, geometry, and model are provided in the attachment. Note that I test my codes in the 'Scripting' and use ANSYS 2024R2. The codes are shown below:

import os
import mech_dpf 
import Ans.DataProcessing as dpf

# Load the Model===========================================================
analysis=ExtAPI.DataModel.Project.Model.Analyses[0]
Data_source = dpf.DataSources(analysis.ResultFileName)

# Read the Target Coordinates==============================================
# Specify the Path of the Result File--------------------------------------
Path_script = os.path.join(os.getenv('TEMP'), "Target_Coordinates.txt")

# Initialize the Data List-------------------------------------------------
Target_Coordinates = []

# Read the File------------------------------------------------------------
with open(Path_script, 'r') as file:
    # Read Each Line in the File===========================================
    for line in file:
        # Split the Line into Two Parts based on the Comma Delimiter=======
        parts = line.split(',')

        # Convert the parts to float and append as a list to the data list=
        Target_Coordinates.append([float(parts[0]), 
                                   float(parts[1]),
                                   float(parts[2])])

Length = len(Target_Coordinates)
Target_field = dpf.FieldsFactory.Create3DVectorField(Length)
[Target_field.Add(i, Target_Coordinates[i - 1]) for i in range(1, Length + 1)]
# Result_field = Target_field.Data

# Load the Displacement in the Axial Direction============================
Axial_displacement = dpf.operators.result.displacement_Z(
                                               data_sources = Data_source)
Axial_displacement_fc = Axial_displacement.outputs.fields_container. \
                                                                 GetData()

# Map the Displacement to the Target Coordinates==========================
Mapped_displacement_fc = dpf.operators.mapping.on_coordinates(
                                  fields_container = Axial_displacement_fc, 
                                  coordinates = Target_field)
Mapped_displacement = Mapped_displacement_fc.outputs.fields_container. \
                                                          GetData()[0].Data

Rajesh Meena

@Gordon1998 Sorry. wbpj file does not have all the information. Please archive the project and share wbpz.

Gordon1998

@Rajesh Meena, thanks for your reminder. Please find the wbpz file attached.

Gordon1998

Hi, @Rajesh Meena.

My latest finding is that this problem only occurs in mapping the displacement results (displacement_X, displacement_Y, displacement_Z, displacement). However, the mapping operation can be performed properly in interpolating strain and stress results by simply replacing codes of

dpf.operators.result.displacement_Z(data_sources = Data_source)

to

dpf.operators.result.stress_von_mises(data_sources = Data_source)

or

dpf.operators.result.strain_eqv_as_mechanical(data_sources = Data_source).

I would appreciate it if you could provide some insights.

Rajesh Meena

@Gordon1998

The source field container should have MeshedRegionSupport.

You can connect mesh in the displacement_Z operator and it should work. Here is a bit of updated code.

import os
import mech_dpf 
import Ans.DataProcessing as dpf

# Load the Model===========================================================
analysis=ExtAPI.DataModel.Project.Model.Analyses[0]
Data_source = dpf.DataSources(analysis.ResultFileName)
model = dpf.Model(Data_source)
# Read the Target Coordinates==============================================
# Specify the Path of the Result File--------------------------------------
Path_script = r"D:\down\Target_Coordinates.txt"

# Initialize the Data List-------------------------------------------------
Target_Coordinates = []

# Read the File------------------------------------------------------------
with open(Path_script, 'r') as file:
    # Read Each Line in the File===========================================
    for line in file:
        # Split the Line into Two Parts based on the Comma Delimiter=======
        parts = line.split(',')

        # Convert the parts to float and append as a list to the data list=
        Target_Coordinates.append([float(parts[0]), 
                                   float(parts[1]),
                                   float(parts[2])])

Length = len(Target_Coordinates)
Target_field = dpf.FieldsFactory.Create3DVectorField(Length)
for i in range(1, Length + 1):
    Target_field.Add(i, Target_Coordinates[i - 1])
# Result_field = Target_field.Data

# Load the Displacement in the Axial Direction============================
Axial_displacement = dpf.operators.result.displacement_Z(
                                               data_sources = Data_source)
Axial_displacement.inputs.mesh.Connect(model.Mesh)
Axial_displacement_fc = Axial_displacement.outputs.fields_container. \
                                                                 GetData()

#Axial_displacement_fc[0].MeshedRegionSupport = model.Mesh
# Map the Displacement to the Target Coordinates==========================
Mapped_displacement_fc = dpf.operators.mapping.on_coordinates(fields_container = Axial_displacement_fc, 
                                  coordinates = Target_field)
Mapped_displacement = Mapped_displacement_fc.outputs.fields_container.GetData()[0].Data

Rajesh Meena

Also, make sure that you are coordinates are in the same unit as solver.

Gordon1998

Hi, Rajesh. Thank you so much. Your codes give the correct results.

I have also found that the format of codes matters. For example, if I build up the result field container as:

Axial_displacement = dpf.operators.result.displacement_Z()
Axial_displacement.inputs.mesh.connect(model.Mesh)
Axial_displacement.inputs.data_sources.connect(Data_source)

the code works fine. However, if I build up the field container in one line as:

Axial_displacement = dpf.operators.result.displacement_Z(mesh = model.Mesh, data_sources = Data_source)

an error will pop out and say the displacement_Z does not have the keyword 'mesh':

Rajesh Meena

@Gordon1998 , yes, I got the same issue and then ended up using additional line for connecting mesh pin.