Load output of PyMechanical Script to PyDyna

I have a .mechdat file output from a previous sim in PyMechanical. How can I load it as an input mesh for subsequent simulation in PyDyna?

Thanks in advance

Find more posts tagged with

PyDyna

PyMechanical

Comments

Erik Kostson

Hello

One approach is in Pymechanical to generate the k file (also define all of the LS-Dyna loads/bc if one wants), which you can then import into pyDyna.

To generate the k file in pymechanical use:

analysis = Model.AddLSDynaAnalysis()


analysis.WriteInputFile('D:\\mypymechkfile.k')

Then import the k file into PyDyna

Thank you

Erik

cardiac.scripter

Hi Erik,

So construct a model from the mechdat file within PyMechanical with the deformed geometry. Then save that as .k file with the lines above.

Have I understood you correctly?

Cheers

cardiac.scripter

Just because I want to use the deformed geometry from the result of the PyMechanical script as the starting geometry for the PyDyna script.

cardiac.scripter

I realised an oversight on my part.

I need the .rst file.

However, I am struggling to load the .rst file with PyMechanical. Once in PyMechanical its easy to then follow your instructions.

Would you suggest opening in pyDPF? I was thinking to go down this route, but I can't find documentation of then saving in PyDyna format.

Ben

Landon Mitchell Kanner

I am struggling to load the .rst file with PyMechanical.

You might find this discussion useful:
https://discuss.ansys.com/discussion/3460/which-scripting-part-or-pyansys-modules-can-i-use-to-obtain-results-in-the-avz-format

cardiac.scripter

Hi Landon,

Thanks for this.

I have downloaded the library and tried the method.

It worked, thank you Erik and Landon.

```python
from ansys.mechanical.core import App
import sys
import os
from ansys.mechanical.core import global_variables

library = r"C:\Users\XXX\Scripts\ResultsFileMechReader"
result_file = r"C:\Users\XXX\StaticStructural\file.rst"

outfolder = os.path.split(result_file)[0]
app = App()
globals().update(global_variables(app))

sys.path.append(library)
sys.path.append(r'C:\Program Files\ANSYS Inc\v242\aisol\DesignSpace\DSPages\Python'.format(app.version))

import RunAPDL
RunAPDL.Initialize(ExtAPI, Ansys)
SI, CdbPath = RunAPDL.GetCdbFileFromResultFile(result_file)

import RunMech
RunMech.Initialize(ExtAPI, Ansys)
RunMech.ImportResultsToCurrentSession(CdbPath, result_file, library)

results =ExtAPI.DataModel.GetObjectsByType(Ansys.Mechanical.DataModel.Enums.DataModelObjectCategory.Result)

Set units

ExtAPI.Application.ActiveUnitSystem = MechanicalUnitSystem.StandardNMMdat

analysis = Model.AddLSDynaAnalysis()

dyna_file = r"C:\Users\XXX\stress_free_mesh.k"
analysis.WriteInputFile(dyna_file)

Erik Kostson

Hi @cardiac.scripter

That is great.

In this way do you export to the LS-Dyna k file a deformed geometry (as per rst file)?

Erik

cardiac.scripter

Hi Erik,

Yes I can. Works well.