This example demonstrates scripting interaction with Engineering Data to access, create, and modify material property data. In this example, you have experimental total strain/stress data in a text file that you wish to use to define Multilinear Isotropic Hardening property data for a material. After you extract the ScriptingGuideExamples.zip file, you will find the files for this example in the Material_Tabular_Data directory.
As an additional consideration, Multilinear Isotropic Hardening property data in Engineering Data is defined in terms of plastic strain. The script must first convert the total strain data to plastic strain, using the relationship:
Plastic Strain = Total Strain – Stress/Young’s Modulus
The above consideration will be used to demonstrate calculations based on physical quantities and units.
To automate property creation, we will write a script that performs the operations described below:
Create a system for a Static Structural analysis, and access the data container for Engineering Data.
Load material data for Polyethylene. By default, this material does not include property data for Multilinear Isotropic Hardening.
Read experimental data from a text file, and generate lists of data for the necessary variables (converting Total Strain to Plastic Strain)
Create the Multilinear Isotropic Hardening property within Polyethylene and set its data table.
Sample Data File The sample data file to be used in this example follows:
# # Stress Stain Data for the Material Properties scripting example. # # The data is Total Strain (in m m^-1), Stress (in MPa) # 7.33E-02, 80.6 1.80E-01, 88.0 6.30E-01, 142.5 7.53E-01, 168.0 8.70E-01, 187.0
Workbench Script The script for this example follows. Each line is numbered for reference in the discussion that follows.
1 workDir = "ScriptingGuideExamples\Material_Tabular_Data/"
2
3 # Create an Engineering Data system and access its data container
4 template1 = GetTemplate(
5 TemplateName="Static Structural",
6 Solver="ANSYS")
7 system1 = template1.CreateSystem()
8 engineeringData1 = system1.GetContainer(ComponentName="Engineering Data")
9
10 # Import Polyethylene
11 poly = engineeringData1.ImportMaterial(
12 Name="Polyethylene",
13 Source="General_Materials.xml")
14
15 # Initialize lists for variable values
16 temperature = []
17 strain = []
18 stress = []
19
20 # Get the value of Young's Modulus for use in the Total/Plastic strain calculation.
21 # Material Property data is always returned as a Quantity.
22 elasticity = poly.GetProperty(Name="Elasticity")
23 E = elasticity.GetData(Variables="Young's Modulus")
24
25 # Read the data file and create lists for Temperature, Strain and Stress values
26 # We must convert Total Strain in the data file into Plastic Strain
27 fileName = AbsUserPathName(workDir + "StressStrainData.txt")
28 dataFile = open(fileName,"r")
29 for line in dataFile:
30 # Skip comment lines
31 if line.startswith("#"):
32 continue
33
34 # Split at the comma to get strain, stress
35 (thisStrain, thisStress) = line.split(",")
36
37 # Convert the data into Quantities with Units.
38 thisStrain = Quantity(float(thisStrain),"m m^-1")
39 thisStress = Quantity(float(thisStress),"MPa")
40
41 # Append data to the variable lists (converting total strain to plastic strain)
42 temperature.append(0)
43 calcStrain = thisStrain - thisStress/E
44 if calcStrain.Value < 1e-4:
45 calcStrain = Quantity(0.0,"m m^-1")
46 strain.append(calcStrain)
47 stress.append(thisStress)
48
49 # Create the Multilinear Isotropic Hardening property and set the data for it
50 miso = poly.CreateProperty(
51 Name="Isotropic Hardening",
52 Definition="Multilinear")
53 miso.SetData(
54 SheetName="Isotropic Hardening",
55 SheetQualifiers={"Definition Method": "Multilinear"},
56 Variables = ["Temperature","Plastic Strain","Stress"],
57 Values = [temperature, strain, stress])
58
59 # Save the project
60 Save(
61 FilePath=AbsUserPathName(workDir + "TabularData.wbpj"),
62 Overwrite=True)
Discussion This example demonstrates interaction with Engineering Data to get, create, and set material properties, as well as calculations involving quantities and units. The following discussion refers to the specified line numbers of the example script to illustrate some of these concepts and constructs. Discussion points from earlier examples will not be repeated here.
To set the project up to work with Polyethylene, we create a new Static Structural system, access its Engineering Data container, and load material data from the General Materials library.
Interaction with tabular data is done in terms of the variables that make up the data table. Each variable represents a column in the table, with a list of data for the variable. Here we initialize three lists for temperature, strain and stress data. Multilinear Isotropic Hardening property data can be temperature-dependent, and temperature is a required variable in the data table. Since our data is not temperature-dependent, we will use the same value of temperature (0 [C]) at each strain/stress point.
Since the calculation for plastic strain depends on Young's Modulus, we use the
GetData() method to get the Young’s Modulus value from
the elasticity property. Within Engineering Data, all property values are stored and
returned as quantities which include both a numeric value and a unit. See Lines 35-41
for further discussion on quantities and units.
Here we open our text data file and read each line one at a time. If the line begins with a comment character '#', we continue to the next line in the file.
The Python split() function is
used to break the comma delimited line and return the separate values
into variables for strain and stress.
In this example we are creating explicit unit-based quantities for stress and strain values, to ensure dimensional and unit consistency in later calculations.
Material property data (or any other quantity data) can be set either as a quantity (i.e., with value and units), or as a simple numeric value (see Specifying Quantities Without Units). If a numeric value is supplied, the units are assumed to be the same as the current project units for the variable (it is the script writer’s responsibility to ensure the numeric data and project units are consistent).
Since temperature is a simple constant value, we will specify temperature as a numeric value (without units), and the units will be taken from the current project unit system. We append 0 into the list of temperature data for this strain/stress pair.
Here we calculate plastic strain based on the available quantities and append it to the variable list. Mathematical operations involving quantities enforce dimensional consistency and automatically perform unit conversion as necessary to generate a consistent result.
Stress data is also appended to the appropriate list.
A new property for Multilinear Isotropic Hardening is created within Polyethylene.
The SetData() method is used
to set single value or tabular data for material properties. Some
properties can contain more than one data table, so the SheetName
and SheetQualifiers arguments are used to specify the exact data table
to be accessed. The Variables argument specifies one or more variables
in the table to be set. The Values argument specifies the values
that correspond to each variable.
Finally we save the project, overwriting if one already exists.