Mechanical Python Code example - write nodal information to .csv file

Pernelle Marone-Hitz

I have a model where several nodal named selections are defined:

etc. These named selection are named with the format "nodalns_fvf_XX".

I also have a .csv file, saved in the user_files directory of the project. This .csv file will be used to define a 3D look-up table in ACP. The "XX" value in the named selection's name will define the fiber volume fraction to be used on that node ("XX" in the NS name defines a FVF of 0.XX, ie "nodalns_fvf_50" should define a fiber volume fraction of 0.50 for all nodes in this named selection).

I want a script that will:

• loop through all named selections
• identify the named selections with the specific names (in this case, that their name contains "nodalns_fvf"
• for each node in these named selection, write to the csv file the (X,Y,Z) position of the node, and the fiber volume fraction to be used on that node.

Pernelle Marone-Hitz

Below is an example script that will do exactly that:

# Import necessary modules
import os
from os.path import exists
import wbjn
import clr
clr.AddReference("Microsoft.Office.Interop.Excel") 
import Microsoft.Office.Interop.Excel as Excel
from System import Array


# Open Excel instance
excel = Excel.ApplicationClass()
excel.Visible = True


# Open pre-existing Excel file 
user_files = wbjn.ExecuteCommand(ExtAPI, "returnValue(GetUserFilesDirectory())")
filename = os.path.join(user_files,'LookUpTable3D.csv')
workbook = excel.Workbooks.Open(filename)
worksheet = workbook.Worksheets("LookUpTable3D")


# Clear existing data
worksheet.Range("A14:D10000").ClearContents()


# Get list of named selection which name contains "nodalns_fvf"
ns_fiberVolumeFraction = [ns for ns in ExtAPI.DataModel.GetObjectsByType(DataModelObjectCategory.NamedSelection) if 'nodalns_fvf' in ns.Name]


# Extract data (from ns name and nodes in ns) 
mesh_data = ExtAPI.DataModel.MeshDataByName('Global')
X_pos = []
Y_pos = []
Z_pos = []
fiber_vf = []
for ns in ns_fiberVolumeFraction:
    for node in ns.Location:
        X_pos.append(mesh_data.NodeById(node).X)
        Y_pos.append(mesh_data.NodeById(node).Y)
        Z_pos.append(mesh_data.NodeById(node).Z)
        fiber_vf.append("0."+ ns.Name.Split('_')[-1])


# Write data to Excel file
len_data = len(X_pos)
range_data = "A14:D"+str(len_data)
xlrange = worksheet.Range[range_data]
data = Array.CreateInstance(object,len_data, 4) 


for row in range(len_data): 
    for column in range(4): 
        data[row, 0] = X_pos[row] 
        data[row, 1] = Y_pos[row]
        data[row, 2] = Z_pos[row]
        data[row, 3] = fiber_vf[row]


xlrange.Value2 = data


# Save file and exit
workbook.Save()
workbook.Close(True)
excel.Quit()

For the script to be executed each time the mesh is generated, simply place it in a Python Code object and use the "After Mesh Generated" callback:

The returned .csv file is as follows:

Pernelle Marone-Hitz

See also this post for a way to do this in ACP: https://discuss.ansys.com/discussion/1999/acp-script-example-create-3d-lookuptable#latest