Defining Material Properties

To define material properties, select the Define subtab at the bottom of the Material tab in the Input dialog and specify a material ID in the ID: box.

First decide whether you wish to enter your own material properties, or select material properties from a standard list provided by StressCheck.

To use material properties from the standard list, click on the Browse… button located at the side of the material ID and when a list of material designations appears in the Material Library dialog, click on the material name and the property data will be entered automatically in the Material tab input fields. Finally, click on Accept to add the material ID record to the record listbox directly under the C/A/O/M combo-boxes. These steps are demonstrated in the below animation:

Standard Properties

The Material Library provides two tabs, one for materials defined in the “Standard” StressCheck material database file, the other for materials that may be defined in a “Company” material database. By default, the Standard material data is contained in a file called “material.dat” found in the /ui installation directory.

As discussed in Display Menu Overview under “Material Database File Format”, it is possible to edit the material.dat file to include additional material properties. For an example of expanding the material property database, refer to StressCheck Tutorial: Expanding the Material Property Database.

Note: The material properties on the Standard list of StressCheck are average values taken from various reference books. Actual material properties may vary substantially from these generally accepted average values. It is the users responsibility to ensure that the material data are properly defined for the specific application.

Material Specification & Units

In the Material Library dialog or in the Material tab, specify whether the material is Linear Elastic, Elastic-Plastic or Nonlinear Elastic material and whether you wish to use standard U.S. units (lbf, in, sec, degrees Fahrenheit), S.I. units (kg, m, sec, degrees Kelvin, force: MN, stress: MPa), or some other system of units. If you choose your own system of units then you must enter your own material properties.

If you have selected either standard U.S. units or S.I. units, and you wish to use a material from the Material Library, then click on the material name and the property data will be entered automatically in the Material tab input fields.

Material Type & Coefficients

Specify the material type: Linear, Elastic-Plastic or Nonlinear-Elastic (exponential isotropic).

• For linear materials the choices are Isotropic, Transversely Isotropic, Orthotropic, Anisotropic, Laminated Isotropic, Laminated Orthotropic or Stiffness (Link stiffness in force per unit length).
  • For isotropic, temperature-dependent material properties may be defined.
  • For transversely isotropic materials, the plane of isotropy is the yz-plane of the material axes.
• For elastic-plastic materials the choices are Elastoplastic, Bilinear, 5-Parameter and Ramberg-Osgood.

After you select the material type, the Material tab automatically adjusts to provide the appropriate number of input fields into which the material coefficients are to be entered. For Planar Elasticity specify whether the analysis is to be Plane Stress or Plane Strain, and provide the material coefficients if not using a standard material from the library.

All values of the material coefficients can be constant, parametric or formula-based. Entering a parameter name or expression in the input field is all it takes to make a coefficient parametric.

Temperature-Dependent Material Properties

To specify temperature-dependent material properties for a linear isotropic material (or for coefficients of thermal conductivity if solving a conduction heat transfer problem), check the “Temp Dep” toggle switch in the Define Material tab of the Input dialog.

• If the coefficients are specified by formula (as a function of temperature) then the formula name is entered into the input area. The results of the evaluation of the formula will be displayed in the Graph window.
• If the coefficients are specified by tabular data, enter the table name in the corresponding fields. The program will fit the tabular data using least square fitting and the results will be displayed in the Graph window.

Any combination of constant, parameter, formula or table can be used for the four material coefficients. Note: When temperature-dependent material properties are defined and assigned to elements, only Linear, Buckling and Modal analyses can be performed. Margin Check and Nonlinear analyses are not supported.

For an example of performing an linear elastic analysis with temperature-dependent material properties, refer to StressCheck Demo: Thermo-Mechanical Analysis with Temperature-Dependent Material Properties.

Input Checking

When you define material properties, StressCheck automatically computes the smallest and largest eigenvalues of the material stiffness matrix (λ_min and λ_max, respectively). When the condition number of the material stiffness matrix, that is, the ratio λ_max/λ_min , is greater than 20 then a warning message appears in the execution window. The reason for this is that the energy error and the root-mean-square error in stresses are close only when / is not large. For details see Section 5.3.1 in “Finite Element Analysis” by Szabó, B. A. and Babuska, I., John Wiley and Sons, Inc. New York, 1991. You may proceed with the analysis but exercise care when computing stresses from the finite element solution.

For more information on material types and coefficients, refer to Linear Elastic Materials and Elastic-Plastic Materials.

Adding a Material ID Record

Click on the Accept button to associate the material name (entered into the material ID field) with the specified material properties. The material ID will be added to the record listbox directly under the C/A/O/M combo-boxes.

Replacing/Deleting Material ID Records

If the user wishes to edit the data in an existing material ID record, or delete an existing material ID record, the user first selects the material ID record from the record listbox directly under the C/A/O/M combo-boxes. Once it is selected, the Status column will read “Selected”, signifying the record can be replaced (updated) or deleted.

Replacing a Material ID Record

Once a material ID record is selected, the user may update the data in the Define tab, and then click Replace to update the material ID record. After clicking Replace, the Accept button will become active and the Replace and Delete buttons will become inactive.

Deleting a Material ID Record

Once a material ID record is selected, the user may click Delete to delete the material ID record. After clicking Delete, the Accept button will become active and the Replace and Delete buttons will become inactive.

Removing All Material ID Records

To remove all material ID records, click the Purge button.

Assigning Material Properties

To assign a material ID name to an element or group of elements which are to have the specific properties, select the Assign subtab at the bottom of the Material tab, and the form will change to the assignment form. Then, select the material ID from the ID: dropdown.

You may then specify all elements in the model (All Elements), elements one-by-one or a group of elements (Any Element), one or more surfaces (Any Surface), a fully enclosed group of surfaces (Mesh Region) or geometric bodies (Any Body) for assignment of one or more material ID’s. Finally, click Accept to add the material assignment record to the record listbox directly under the C/A/O/M combo-boxes. These steps are demonstrated in the below animation:

Note: if the A/O/M is set to Select > All Elements > Selection, it is not necessary to perform any screen selection of elements; all elements in the mesh will receive the assignment of the selected material ID.

Selecting Objects for Assignment to a Material ID

If the assignment is to be based on the selection of objects, then in the Model View simply left-click on the objects to which the property is to be assigned.

• If the assignment is to a group of elements, for example, then left-lick and drag the cursor to enclose the desired group of elements in a marquee selection. The selected elements will be highlighted and ready for assignment. Note: it is important to disable the Wetted Faces toggle if internal elements are to be included in the marquee selection.
• If you wish to add one or more elements to the selected group, hold the Shift key down and left-click on the elements to be added to the group.
• If you wish to remove one or more elements from the selected group, hold the Ctrl key down and left-click on the elements to be removed from the group.
• If you wish to cancel the current selection of objects, simply right-click on the Model View.

The multi-layer toggle can be turned on if you want the program to select the elements that share the face of the opposite face selected in a given element. This cascade effect allows selection of “layers” of elements for the assignment of laminate properties.

As discussed, material assignments may also be made to geometric objects via Mesh Region, Any Surface or Any Body. Elements associated with these objects will automatically inherit the material assignment. For more information on assigning material properties to geometry/mesh objects, refer to Can I Assign Material Properties to Bodies/Parts Directly? and StressCheck Tutorial: Assigning Material Properties.

Specifying a Set for Assignment to a Material ID

Alternatively, if a there is a set definition containing a list of objects for assignment, the name of this set may be specified in the Set: combo-box instead of selecting the objects from the Model View. Simply select the name of the set, and the objects in the set list will automatically be selected in the Model View.

Note: automeshed element sets are automatically generated, and are identified by _AUTO_B_#, where # is the number of the automeshed body. For an example of using automesh sets to assign materials, refer to Helpful Hints and Tips: Using Automesh Sets to Assign Materials.

Specifying a Material System

If the material properties are orthotropic, laminate orthotropic or transversely isotropic and the orientation of the material axes is not coincident with the global coordinate system, you can enter the name of the local coordinate system in the System: field. To create a local coordinate system select Geometry > Create > System > Locate. Enter the location and orientation of the system.

• The material 1-axis will be aligned with the local x-axis of the system if the system is Cartesian.
• For Cylindrical systems the material 1-axis will be aligned with the circumferential direction and the material 2-axis with the radial direction.

Note: to display the name of a coordinate system select Display > Objects from the Main Menu Bar and turn the corresponding label on.

Specifying a Material Color

The color of the elements receiving the material property assignment can be specified from the Color dropdown as “Same As Solid” (default, elements will have the same color as the associated solid body), “Steel” (dark grey color), “Titanium” (teal blue color), “Fastener” (light yellow color), “Aluminum” (blue grey color), or “Beam” (dark blue color).

To define a custom color, click the “Color…” button to access the Assign Colors pane. From there, a custom color may be defined, and then specified from the Color dropdown during the material property assignment.

Adding a Material Assignment Record

Once an object or group of objects are selected, and a material ID is specified in the ID: dropdown, to add the new material assignment record to the record listbox simply click the Accept button.

Note: if an existing record has already been selected from the record listbox, you first must choose Set: “New set” or re-select the action, object, or method. Then, you are able to create the new material assignment record as usual.

Replacing/Deleting Material Assignment Records

If the user wishes to edit the data in an existing material assignment record, or delete an existing material assignment record, the user first selects the assignment record from the record listbox directly under the C/A/O/M combo-boxes. Once it is selected, the Status column will read “Selected”, signifying the record can be replaced (updated) or deleted.

Replacing a Material Assignment Record

Once a material assignment record is selected, the user may update the data in the Assign tab, and then click Replace to update the material assignment record. After clicking Replace, the Accept button will become active and the Replace and Delete buttons will become inactive.

Deleting a Material Assignment Record

Once a material assignment record is selected, the user may click Delete to delete the material assignment record. After clicking Delete, the Accept button will become active and the Replace and Delete buttons will become inactive.

Removing All Material Assignment Records

To remove all material assignment records, click the Purge button.

Checking Material Assignments

To check whether a material property was assigned to each element, select Action: Check, Object: All Elements, and then click on the Accept button. A confirmation report will appear on the screen.