How to create a custom material in Ansys Workbench programmatically ? By using APIs/ACT

surajsalvi

System Information

Application : Ansys Workbench
Version : 2022 R2

Problem Statement

To create a material manually user can add material name in below option

After entering name a blank material is created

From the left side pallet, user can add material properties manually, and material object will be created with some properties in it.

How this can be done programmatically or using using ACT/ APIs ?

Find more posts tagged with

AnsysACT

Python

Ansys Workbench

Accepted answers

Pernelle Marone-Hitz

Hi @surajsalvi , this is doable via scripting at the project schematic level. There are recording capabilities at the project schematic level which I encourage you to use when you are trying to find the appropriate commands to do something.

Go to File /Scripting and select "Record Journal":

Then take the actions manually, and finally go to the same place (File / Scripting) and select "Stop Recording". This will create a .wbjn file which can be opened in a text editor and gives you the commands related to whichever action you have just done.

To insert an engineering data component system and add a new material, the commands would be:

# encoding: utf-8
# 2023 R1
SetScriptVersion(Version="23.1.153")
template1 = GetTemplate(TemplateName="EngData")
system1 = template1.CreateSystem()
engineeringData1 = system1.GetContainer(ComponentName="Engineering Data")
matl1 = engineeringData1.CreateMaterial(Name="custom_mat")
matlProp1 = matl1.CreateProperty(
    Name="Elasticity",
    Behavior="Isotropic",
    Qualifiers={"Definition": "", "Behavior": "Isotropic"})
matlProp1.SetVariableProperty(
    VariableName="Young's Modulus",
    Property="Unit",
    Value="MPa")
matlProp1.SetData(
    Index=-1,
    Variables=["Young's Modulus"],
    Values=[["200000 [MPa]"]])
matlProp1.SetData(
    Variables=["Poisson's Ratio"],
    Values=[["0.3"]])

Pernelle Marone-Hitz

Hi @surajsalvi , this script is based on Python. You can replay it by going to File / Scripting / Run script file.

You could add to that script some Python code to open an Excel file and read the data from it, and execute this in batch mode. Please refer to second proposal of this post: https://discuss.ansys.com/discussion/2197/how-can-i-run-a-mechanical-script-in-batch-mode

All comments

Pernelle Marone-Hitz

Go to File /Scripting and select "Record Journal":

To insert an engineering data component system and add a new material, the commands would be:

# encoding: utf-8
# 2023 R1
SetScriptVersion(Version="23.1.153")
template1 = GetTemplate(TemplateName="EngData")
system1 = template1.CreateSystem()
engineeringData1 = system1.GetContainer(ComponentName="Engineering Data")
matl1 = engineeringData1.CreateMaterial(Name="custom_mat")
matlProp1 = matl1.CreateProperty(
    Name="Elasticity",
    Behavior="Isotropic",
    Qualifiers={"Definition": "", "Behavior": "Isotropic"})
matlProp1.SetVariableProperty(
    VariableName="Young's Modulus",
    Property="Unit",
    Value="MPa")
matlProp1.SetData(
    Index=-1,
    Variables=["Young's Modulus"],
    Values=[["200000 [MPa]"]])
matlProp1.SetData(
    Variables=["Poisson's Ratio"],
    Values=[["0.3"]])

surajsalvi

Hi Pernelle Marone-Hitz,

Your answer is really helpful this what I am looking for, but I am not sure how to run this programmatically.

How I can run these commands ? is it using MAPDL ? or any Python or Java code ?

I want to trigger material creation from external program using supported programming language by Ansys

Pernelle Marone-Hitz

Hi @surajsalvi , this script is based on Python. You can replay it by going to File / Scripting / Run script file.

surajsalvi

Hi Pernelle,

Thanks for your support I was able to create material using script file you suggested and using command.

I have one more doubt related to programmatic execution, as I was trying this on student version if I move to licensed enterprise version will there be any python or java APIs available to do the same action ?

surajsalvi

Hi Pernelle Marone-Hitz

From the post you shared I can able to add material over the existing project successfully. Below is the command which I used :

"C:\Program Files\ANSYS Inc\ANSYS Student\v222\Framework\bin\Win64\RunWB2.exe" -B -F "D:\Script\PROJECT_cust_matl.wbpj" -R "D:\Script\SCRIPT_create_matl.wbjn"

And below is the script which I generated from the File -> Scripting -> Record Journal option in Ansys Workbench

# encoding: utf-8
# 2022 R2
SetScriptVersion(Version="22.2.192")
system1 = GetSystem(Name="SYS")
engineeringData1 = system1.GetContainer(ComponentName="Engineering Data")
matl1 = engineeringData1.CreateMaterial(Name="MATL-04")
matlProp1 = matl1.CreateProperty(
  Name="Elasticity",
  Behavior="Isotropic",
  Qualifiers={"Definition": "", "Behavior": "Isotropic"})
matlProp1.SetData(
  Index=-1,
  Variables=["Young's Modulus"],
  Values=[["85 [Pa]"]])
matlProp1.SetData(
  Variables=["Poisson's Ratio"],
  Values=[["2"]])
matlProp1.SetData(
  Variables=["Poisson's Ratio"],
  Values=[["0.1"]])
matlProp1.SetData(
  SheetName="Elasticity",
  SheetQualifiers={"Definition": "", "Behavior": "Isotropic", "Derive from": "Young's Modulus and Poisson's Ratio"},
  Variables=["Temperature"],
  Values=[["35 [C]"]])
Save(
  FilePath="D:/Scrip/PROJECT_cust_matl.wbpj",
  Overwrite=True)