Command reference help topics
Material dialog box
The following description of the Material dialog box lists the material properties in the dialog box. If the property is exported to Simcenter Nastran, click the link to the Simcenter Nastran Quick Reference Guide for more information. If a material property is not used by Simcenter Nastran, the description indicates where it is used.
Some material properties, such as Mass Density, may be used in Simcenter Nastran as well as by other solvers or applications.
General options
Anisotropic material properties
Compound Isotropic material properties
Creep material properties
Durability material properties
Electromagnetic material properties
Fluid material properties
Formability material properties
Hyperelastic material properties
Isotropic material properties
Miscellaneous material properties
Multiple fluid material properties
Orthotropic material properties
Porous material properties
User models material properties
Viscoelasticity material properties
Visual material properties
General options
| Option | Description |
|---|---|
| Property View | Lets you filter material properties by solver and analysis type. For more information, see Filtering specific material properties by solver and analysis type.For information about Samcef property views, see Material Property Views (Simcenter Samcef). |
| Name – Description | Lets you enter a name and description for the new material. |
| Label | Lets you enter an integer label as the material identification number. |
| Inherited Value | Appears when the material has been copied from another material definition.Indicates that this material property has the same value as the material property in the original material definition from which this material was copied.When a material is copied, a parent-child relationship is established. The copied (child) material inherits the property values from the original (parent) material definition. |
| Overridden Value | Appears when the material has been copied from another material definition.Indicates that this material property has been changed from the value in the original material definition from which this material was copied. The original property value has been overridden.To revert the value to the inherited value, click the Overridden Value button. |
| Read Only | Appears when the material is a custom library material.Indicates that the material property is non-configurable.For more information, see Editingand configuring material definition in a custom library. |
| Magnitude options | You can define the magnitude with a constant value, expression, or field. You can:Enter a constant value directly in the entry box. Enter an expression directly in the entry box. As you begin to type the expression, tooltips provide hints about valid parameter names. If you enter an invalid or incomplete expression, the warning icon appears next to the entry box.Click and select from these options: Expression opens the Expressions dialog box, where you can select an existing expression or create a new one.For more information about expressions, see Expressions.Select Existing Field opens the Fields dialog box, where you can select a field. A field can define a magnitude that varies with independent variables such as frequency, temperature, or time. For more information about fields, see Fields.New Field→Formula Constructor opens the Formula Field dialog box, where you can define a formula to construct a field.For more information, see Define a boundary condition using a formula field.New Field→Table Constructor opens the Table Field dialog box, where you can define tabular data to construct a field.For more information, see Define a boundary condition using a table field and Define a material property using a table field.New Field→Link Constructor opens the Linked Field dialog box, where you can construct a linked field from an existing spatial field. For more information, see Linked Field dialog box.Plot (XY) plots the field as an XY graph. For more information, see Graph overview.Overlay(XY) overlays a plot on an existing plot. You can overlay up to 50 plots. For more information, see Overlay plots.For more information about other options in the list, see Additional magnitude options. |
| Pedigree | |
| Appears only when you copy a material to create a new material. | |
| Parent Material | Lists the material definition from which the current material definition was copied. |
| Parent Library | Lists the XML file where the parent material is stored. |
| Parent Library Version | Lists the version of the material library in which the parent material definition is stored. |
| Configuration options | |
| Appear only when you edit a custom library material in the Material Library Manager dialog box.If a property is configurable, users can modify the configurable material properties in the Manage Materials dialog box.For more information, see Editingand configuring material definition in a custom library. | |
| Allow Configuration | Lets you make the material property configurable by users. |
| No Configuration Allowed | Lets you make the material property read-only so that users cannot change it. |
| Checking option | |
| Check Properties based on current Property View | Appears for some property views.When the Check Properties based on current Property View check box is selected and you close the dialog box with OK, the software validates the material properties. If the properties do not pass the check, the invalid properties appear in an Information window. |
| Categorization | |
| Alternate Name | Specifies a different name for the material property. This name could be used when your company refers to materials using informal names in addition to the standard names. |
| Category | Specifies a category for the material property. The category is often supplied with existing materials; you can also enter a category name when creating a new material. |
| Sub-Category | Specifies a secondary category for the material property. |
| Reset to Defaults | |
| Appears only when you copy a material to create a new material. | |
| Property | Lists the names of all material properties in the current library. |
| Inherited Value | Lists the value of the material property on the parent material definition. |
| Indicates that the material property in the current material definition contains a value that is different from the value of the material property in the parent material definition. | |
| Indicates that the material property in the current material definition has not been changed from its parent material definition. | |
| Current Value | Lists the new value of the material property in the current material definition, which overrides the value in the parent material definition. |
| Select All | Selects all rows in the table. |
| Override with inherited value | Locks the selected material property so that future changes to this material property in the parent library material will not change the override value. |
| Remove Override | For all selected records, restores the value of the material property to the value of the material property in the parent material definition. |
Isotropic material properties
| Properties | |
|---|---|
| Material Property Dependency | Appears when Property View is set to any but the following:Simcenter Nastran MAT1Simcenter Nastran MAT1/MATT1Simcenter Nastran MAT1/MATS1/MATSRSimcenter Nastran MAT1/MAT1FSimcenter Nastran MAT1/MPLASSimcenter Nastran MAT1/MATS1/MATSR/CREEPSimcenter Nastran MAT1/MATS1/MATSR/MATCRP****Simcenter Nastran MAT1/MPLAS (standalone plasticity)Simcenter Nastran MAT1/MVPLAS (standalone creep)Simcenter Nastran MAT1/MPLAS/MVPLAS (coupled plasticity and creep)Sets whether certain material properties on the Mechanical, Strength, and Thermal pages are constant, temperature dependent, frequency dependent, or both temperature dependent and frequency dependent.For more information on which material properties are temperature or frequency dependent, see the Mechanical, Strength, and Thermal pages.ConstantDependent material properties are not set, and a nominal value is used for each material property.TemperatureAllows material properties to vary with respect to temperature.In Nastran, temperature-dependent properties are written to a MATT1 bulk entry, which specifies temperature-dependent material properties for MAT1 entry fields via TABLEMi entries.FrequencyAllows material properties to vary with respect to frequency.In Nastran, frequency-dependent properties are written to a MAT1F bulk entry, which specifies frequency-dependent material properties for MAT1 entry fields via TABLEDi entries.Frequency and TemperatureAllows material properties to vary with respect to either frequency or temperature.In Nastran, temperature-dependent properties are written to a MATT1 bulk entry and frequency-dependent properties are written to a MAT1F bulk entry. |
| Reference Frequency | Appears when Property View is set to Simcenter Nastran MAT1/MAT1F, or when Material Property Dependency is set to Frequency or Frequency and Temperature.Sets the reference frequency.In Nastran, the reference frequency determines how the required nominal values are written to the MAT1 bulk entry when you define frequency dependent material properties.The reference frequency is used as follows:If you define a nominal value for a material property, the software writes the nominal value to the MAT1 bulk entry.For example, if you type 1 in the Young's Modulus (E) box, the MAT1 entry for E is 1.If the material property box is blank, then the frequency-dependent material property is evaluated at the reference frequency you specify.For example, if the Young's Modulus (E) box is empty, you define a field for Specify Frequency Dependent Young's Modulus (E) Field, and you type 2 Hz in the Reference Frequency box, the software writes the nominal value for Young's modulus as the value of Specify Frequency Dependent Young's Modulus (E) Field that corresponds to a frequency of 2 Hz.The default value is 0.0.Note: If Material Property Dependency is set to Frequency and Temperature, then the MAT1 bulk entries are defined using temperature-dependent fields that are evaluated at the reference temperature Temperature (TREF). |
| Mass Density (RHO) | Sets a nominal value for mass density.In Nastran, when you define frequency-dependent or temperature-dependent materials, this nominal value is always written to the MAT1 bulk entry instead of using the corresponding temperature dependent or frequency dependent mass density fields. |
| Specify Temperature Dependent Mass Density (RHO) Field | Appears when Property View is set to Simcenter Nastran MAT1/MATT1, or when Material Property Dependency is set to Temperature or Frequency and Temperature.Allows you to define a mass density that varies with respect to temperature.You can use temperature-dependent mass density to calculate the solid properties of your model at a specified temperature. For more information on how solid properties are calculated, see Solid Properties Check dialog box. |
| Specify Frequency Dependent Mass Density (RHO) Field | Appears when Property View is set to Simcenter Nastran MAT1/MAT1F, or when Material Property Dependency is set to Frequency or Frequency and Temperature.Allows you to define a mass density that varies with respect to frequency.Note: If Mass Density (RHO) is not defined or is 0.0 and Specify Temperature Dependent Mass Density (RHO) Field is not defined, solid properties are calculated using Specify Frequency Dependent Mass Density (RHO) Field evaluated at the Reference Frequency.For more information on how solid properties are calculated, see Solid Properties Check dialog box. |
Compound page, Isotropic properties
Appears only when you create or edit a Compound Isotropic material.
For more information, see Compound isotropic materials.
Mechanical page, Isotropic properties
| Elastic Constants | |
|---|---|
| **Young’s Modulus (E)****Poisson’s Ratio (NU)****Shear Modulus (G)**Structural Damping Coefficient (GE) | In Nastran structural solutions, these properties are written to the MAT1, MATT1, and MAT1F bulk entries.You can define either frequency or temperature dependency by specifying a field for these properties when:Property View is set to Simcenter Nastran MAT1/MATT1.Property View is set to Simcenter Nastran MAT1/MAT1F.Material Property Dependency is set to Temperature, Frequency, or Frequency and Temperature. |
| Stress-Strain Related Properties | |
| Type of Nonlinearity (TYPE) | Specifies the type of material nonlinearity.When writing out the solver input file, the software converts the stress-strain data depending on the solver, and for Simcenter Nastran, also depending on the type of solution and the setting of the Type of Nonlinearity option. The output stress-strain data will be in the same units as the input stress-strain data. The units of Young’s Modulus should be consistent with the input stress-strain data.**Nonlinear elastic: stress-strain (MATS1/NLELAST)**Note: This option does not apply to SOLs 401 or 402.**Elastoplastic: stress-total strain (MATS1/PLASTIC)****Elastoplastic: stress-plastic strain (MATS1/PLSTRN)****Elastoplastic: material (MPLAS)**For more information, see Specifying stress-strain data for nonlinear materials. |
| Yield Function Criterion (YF) | Specifies the yield function:von MisesTrescaMohr-CoulombDrucker-PragerRaghavaHillHill by Stress Ratios****Grey Cast IronNote: Certain yield functions may be not be compatible with your Type of Nonlinearity (TYPE) selection. To verify that your selection is valid, hover over the yield function from the list and view the tooltip. |
| Ratio of Compressive and Tensile Yield Stresses (S) | Appears when the Yield Function Criterion (YF) list is set to Raghava.Sets the ratio between the compressive and tensile stresses.For more information on elastoplastic yield function criterion, see Elastoplastic yield function criterion (Simcenter Samcef). |
| **Initial Tensile Yield Stress (XT2)**Initial Tensile Yield Stress (XT3) | Appears when the Yield Function Criterion (YF) list is set to Hill.Sets the tensile stress limits.The major Hill tensile stress limit value is computed from the value of the Stress-Strain (H) law at the origin and for the given Reference Temperature.For more information on elastoplastic yield function criterion, see Elastoplastic yield function criterion (Simcenter Samcef). |
| **Shear Yield Stress (RST)****Shear Yield Stress (RSTT2)**Shear Yield Stress (RST3) | Appears when the Yield Function Criterion (YF) list is set to Hill.Sets the shear yield stresses.For more information on elastoplastic yield function criterion, see Elastoplastic yield function criterion (Simcenter Samcef). |
| R11 = Y0,11 / Y0R22 = Y022 / Y0R33 = Y033 / Y0R12 = 3^0.5 * Y0,12 / Y0R23 = 3^0.5 * Y0,23 / Y0****R13 = 3^0.5 * Y0,13 / Y0 | Appears when Yield Function Criterion (YF) is set to Hill by Stress Ratios.Sets the stress ratios.These properties are written to the corresponding fields (Y-PAR1, Y-PAR2, etc.) in the MPLAS bulk entry. |
| Hardening Rule (HR) | Lets you select the hardening model:IsotropicKinematicMixed HardeningSublayer KinematicIsotropic + Chaboche Kinematic****Isotropic Saturated + Chaboche KinematicFor more information on elastoplastic hardening laws, see Elastoplastic hardening laws (Simcenter Samcef).Note: Certain hardening rules may be not be compatible with your Type of Nonlinearity (TYPE) and Yield Function Criterion (YF) selections. To verify that your selection is valid, hover over the hardening rule from the list and view the tooltip. |
| Hardening Ratio (Between Isotropic and Kinematic | Appears when the Hardening Rule (HR) list is set to Mixed Hardening.Lets you balance the hardening law between the standard Isotropic formulation and the full Kinematic one.For more information on elastoplastic hardening laws, see Elastoplastic hardening laws (Simcenter Samcef). |
| Kinematic Laws | Appears when the Hardening Rule (HR) list is set to Kinematic or Mixed Hardening.Lets you define either a Prager (KPRA) or Ziegler (KZIE) kinematic hardening law.For more information on elastoplastic hardening laws, see Elastoplastic hardening laws (Simcenter Samcef). |
| Non-Linear Hardening Coefficient (NLH) | Appears when the Hardening Rule (HR) list is set to Kinematic or Mixed Hardening.Lets you define the hardening coefficient.This coefficient can be temperature dependent.For more information on elastoplastic hardening laws, see Elastoplastic hardening laws (Simcenter Samcef). |
| Stress-Strain Input Data Type | Specifies the data type of the value in Stress-Strain (H).Engineering Stress-Strain (default)Engineering-Plastic StrainTrue Stress-Log StrainTrue Stress-Plastic Strain****Undefined (When migrated from earlier versions of this software, materials that contain stress-strain property data will be set to this option)Note: Certain stress-strain data types may be not be compatible with your Type of Nonlinearity (TYPE) selection. To verify that your selection is valid, hover over the stress-strain data type from the list and view the tooltip.When Stress-Strain Input Data Type is set to Undefined, the software writes out the stress-strain data directly as specified in the material data and does not perform a conversion.For more information, see Specifying stress-strain data for nonlinear materials. |
| Stress-Strain (H) | Sets value for stress-strain based on the specified Stress-Strain Input Data Type.For more information, see Elastoplastic hardening laws (Simcenter Samcef). |
| Initial Yield Point (LIMIT1) | Sets the initial yield point.For more information, see MATS1. |
| Initial Friction Angle (LIMIT2) | Sets the internal friction angle.For more information, see MATS1. |
| Strain Rate Dependency | Specifies how you want the strain rate to be calculated for plastic material.Symonds and CowperLets you define parameters for strain-rate hardening and transition strain rate using only two parameters.General DefinitionLets you specify a field, formula field, table field, or table of fields. Use this option when you have several curves, and you want to identify the stress at a given point. The general definition requires multiple stress/strain curves for various strain rates. This gives you more control but it is harder to identify. User-defined material properties are written to the Simcenter Nastran MATSR bulk entry. |
| Exponent (BVALUE) | Appears when Strain Rate Dependency is set to Symonds and Cowper.Sets the strain-rate hardening. |
| Strain Rate Level (TSRATE) | Appears when Strain Rate Dependency is set to Symonds and Cowper.Sets the transition strain rate. |
| Strain Rate****Specify Field | Appears when Strain Rate Dependency is set to General Definition.Sets the field, formula field, table field, or table of fields that you want to use to identify the stress at a given point. |
| Grey Cast Iron | |
| Appears when Yield Function Criterion (YF) is set to Grey Cast Iron. | |
| Compression Specify Stress-Strain Curve Field | Lets you specify a field to define the stress-strain relationship of grey cast iron in compression.For more information on cast iron plasticity, see Cast iron plasticity SOLs 401 and 402. |
| Traction Specify Stress-Strain Curve Field | Lets you specify a field to define the stress-strain relationship of grey cast iron in tension.For more information on cast iron plasticity, see Cast iron plasticity SOLs 401 and 402. |
| Tensile Plastic Poisson's Ratio (NUPL) | Sets the plastic Poisson's ratio in tension for the grey cast iron yield type.For more information on cast iron plasticity, see Cast iron plasticity SOLs 401 and 402. |
| Isotropic Portion | |
| Appears when Yield Function Criterion (YF) is set to von Mises or Hill by Stress Ratios. | |
| Specify Stress-Strain Curve Field | Specifies the stress-strain curve for the following hardening rules:IsotropicSublayer KinematicIsotropic + Chaboche Kinematic |
| Chaboche Kinematic Hardening Portion (True Stress and Plastic Strain) | |
| Appears when Hardening Rule (HR) is set to Isotropic + Chaboche Kinematic or Isotropic Saturated + Chaboche Kinematic. | |
| Isotropic Saturated Portion (True Stress and Plastic Strain) | |
| Appears when Hardening Rule (HR) is set to Isotropic Saturated + Chaboche Kinematic. | |
| Y0 Initial Stress | Appears when Hardening Rule (HR) is set to Isotropic Saturated + Chaboche Kinematic.Sets the initial yield stress. |
| Number of Rows [1 - 20] | Sets the number of rows (up to 20) in the table. Each row represents a Chaboche kinematic or isotropic saturated term. To increase or decrease the number of rows, type the number and press Enter, or click the up and down arrows.After you set up the table:To add rows, do one of the following:To add one row at a time, right-click a row and choose Add a Row at Bottom.To add multiple rows at one time, type the total new number of rows you want. For example, if you created the table with 10 rows and you now want 18 rows, type 18. The rows are added to the end of the table.To delete rows, do one of the following:To delete one row at a time starting with the bottom row, right-click the row and choose Delete a Last Row. You can delete only the last row in the table.To delete multiple rows at one time, type the total new number of rows you want. For example, if you created the table with 20 rows and you now want 16 rows, type 16. The last four rows of the table are removed.You cannot add or a delete a row that is in between two other rows. Rows are always added to the bottom of the table, or deleted from the bottom of the table. |
| Chaboche kinematic term C Stress (Linear Back-Stress) (n) G Factor (NL Back-Stress) (n) Isotropic saturated term Q Stress (n) B Factor (n) | Sets the values for the Chaboche kinematic or isotropic saturated term. To add or change a value:Click the row whose term you want to add or change.The label updates to indicate the row number.Type the value, or click to select a function or to select or create a field.The table updates with the value or the name of the function or field.For more information about other options in the list, see Additional magnitude options. |
Strength page, Isotropic properties
| Strength Properties | |
|---|---|
| Yield Strength | In Nastran, this property is written to the MATS1 bulk entry. For more information, see MATS1 bulk data entry export. |
| Ultimate Tensile Strength | This property is not exported to Simcenter Nastran. It is used by the Durability capability. |
| Tsai-Wu Interaction Coefficient (F12) | This property is not exported to Simcenter Nastran. It is used by Laminate Composites. |
| Stress Limits | |
| **Max Tension (ST)****Max Compression (SC)**Max Shear (SS) | In Nastran, structural solutions, these properties are written to the MAT1 and MATT1 bulk entries. You can define temperature dependency by specifying a field for these properties when:Property View is set to Simcenter Nastran MAT1/MATT1.Material Property Dependency is set to Temperature or Frequency and Temperature. |
| Strain Limits | |
| **Tension (XT)****Compression (XC)**Shear (XS) | These properties are not exported to Simcenter Nastran. They are used by Laminate Composites. |
Thermal page, Isotropic properties
| Thermal | |
|---|---|
| Temperature (TREF) | In Nastran thermal solutions, Temperature (TREF) is written to the MAT4 and MATT4 bulk entries. In Nastran, Temperature (TREF) also determines how the required nominal values are written to the MAT1 bulk entry when you define temperature-dependent material properties.Temperature-dependent material properties are available when:Property View is set to Simcenter Nastran MAT1/MATT1.Material Property Dependency is set to Temperature or Frequency and Temperature.When you define temperature-dependent material properties, the nominal values are written to the MAT1 bulk entry using Temperature (TREF) as follows:If you define a nominal value for a material property, the nominal value is written to the MAT1 bulk entry.For example, if you type 1 in the Young's Modulus (E) box, then the MAT1 entry for E is 1.If the material property box is blank, then the temperature-dependent material property is evaluated at the reference temperature you specify.For example, if the Young's Modulus (E) box is empty, you define a field for Specify Temperature Dependent Young's Modulus (E) Field, and you type 2 °C in the Temperature (TREF) box, the software writes the nominal value for Young's modulus as the value of Specify Temperature Dependent Young's Modulus (E) Field that corresponds to a temperature of 2 °C.The default value is 0.0. |
| *Thermal Expansion Coefficient Type***Thermal Expansion Coefficient (A)****Thermal Conductivity (k)**Specific Heat (CP) | In Nastran thermal solutions, these properties are written to the MAT4 and MATT4 bulk entries. Thermal Expansion Coefficient Type lets you select a Secant or Tangent type for the thermal expansion coefficient (CTE). For more information on CTE, see Understanding Coefficient of Thermal Expansion (CTE) in the Simcenter Nastran User’s Guide.You can define temperature dependency by specifying a field for Thermal Expansion Coefficient (A) when:Property View is set to Simcenter Nastran MAT1/MATT1.Material Property Dependency is set to Temperature or Frequency and Temperature.Note: When you open an existing material, where the Thermal Expansion Coefficient Type was not set, the software sets the Thermal Expansion Coefficient Type to the default value Undefined. The same applies when you read a material from your own material library file, where the CTE type for this material is not specified. |
| Thermal Phase Change | |
| Latent Heat****Phase Change Temperature Range | In Nastran thermal solutions, these properties are written to the MAT4 and MATT4 bulk entries. |
| Specific Heat above Phase Change | This property is not exported to Simcenter Nastran. It is used by the Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal solvers. |
| Infrared Coefficients | |
| Scattering****Extinction | These properties are not exported to Simcenter Nastran. They are used by the Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal solvers. |
Electromagnetic page, Isotropic properties
These properties are not exported to Simcenter Nastran. They are used by the electromagnetic environments.
For more information, see Electromagnetic isotropic material properties.
Other Physical Properties page, Isotropic properties
These properties are not exported to Simcenter Nastran. They are used by the electromagnetic environments and are available when the Property View is set to All Properties, Simcenter MAGNET Thermal Electromagnetic, or Simcenter MAGNET Thermal Electric.
| Dynamic Viscosity | |
|---|---|
| Dynamic Viscosity Control | Specifies how to control dynamic viscosity.Constant or TemperatureThe dynamic viscosity can be constant or temperature dependent.Temperature and PressureThe dynamic viscosity is defined with field values.Note: Available when Property View is set to All Properties. |
| Dynamic Viscosity | Appears when Dynamic Viscosity Control is set to Constant or Temperature.Lets you enter a constant dynamic viscosity value or when you click , you can define temperature-dependent dynamic viscosity values.For more information, see Magnitude options above. |
| Specify Dynamic Viscosity field | Available when Property View is set to All Properties.Lets you select an existing field, use a formula or table, or table of fields to define temperature and pressure-dependent dynamic viscosity values. |
Orthotropic material properties
Mechanical page, Orthotropic properties
| Young’s Modulus | |
|---|---|
| **Young’s Modulus (E1)****Young’s Modulus (E2)**Young’s Modulus (E3) | In Simcenter Nastran structural solutions, this property is written to the following bulk entries:Material properties for shell elements are written to MAT8 and MATT8 bulk entries.Material properties for axisymmetric elements are written to MAT3 and MATT3 bulk entries. |
| Poisson’s Ratio and Shear Modulus | |
| **Poisson’s Ratio (NU12, NU23, NU13)****Shear Modulus (G12, G13, G23)**Note: For Poisson’s Ratio, specify whether the values are for Major Poisson’s Ratio or Minor Poisson’s Ratio | In Simcenter Nastran structural solutions, these properties are written to the following bulk entries:Material properties for shell elements are written to MAT8 and MATT8 bulk entries.Material properties for axisymmetric elements are written to MAT3 and MATT3 bulk entries. |
| Stress-Strain Related Properties | |
| **Yield Function Criterion (YF)****Hardening Rule (HR)****Initial Yield Point (LIMIT1)****Initial Friction Angle (LIMIT2)**Stress-Strain (H) | See the description provided previously in the Isotropic material properties section. |
| Type of Nonlinearity (TYPE) | |
| Stress-Strain Input Data Type | |
| Strain Rate Dependency | |
| Exponent (BVALUE) | |
| Strain Rate Level (TSRATE) | |
| Strain Rate****Specify Field |
Strength page, Orthotropic properties
Allowable stress and strain for laminate failure analysis.
| Stress Limits | |
|---|---|
| Tension (ST1, ST2, ST3) | Material properties for shell elements are written to MAT8 and MATT8 bulk entries. |
| Compression (SC1, SC2, SC3) | |
| Shear (S12, S13, S23) | |
| Strain Limits | |
| Tension (XT1, XT2, XT3) | Material properties for shell elements are written to MAT8 and MATT8 bulk entries. |
| Compression (XC1, XC2, XC3) | |
| Shear (X12, X13, X23) | |
| Tsai-Wu Coefficient | |
| Tsai-Wu Interaction Coefficient (F12) | Material properties for shell elements are written to MAT8 and MATT8 bulk entries. |
| Tsai-Wu Interaction Coefficient (F13) | For solid composites that are defined with the PCOMPS bulk entry. Use them for composite ply failure theories. They are written to the MATFT bulk entry. |
| Tsai-Wu Interaction Coefficient (F23) |
Thermal page, Orthotropic properties
In Simcenter Nastran thermal solutions, the Mass Density property is written to the MAT5 and MATT5 bulk entries.
| Thermal | |
|---|---|
| Thermal Expansion Coefficient Type****Temperature (TREF) | In Simcenter Nastran structural solutions, these properties are written to the following bulk entries:Material properties for shell elements are written to MAT8 and MATT8 bulk entries.Material properties for solid elements are written to MAT9 and MATT9 bulk entries.Material properties for axisymmetric elements are written to MAT3 and MATT3 bulk entries.Thermal Expansion Coefficient Type lets you select a Secant or Tangent type for the thermal expansion coefficient (CTE). For more information on CTE, see Understanding Coefficient of Thermal Expansion (CTE) in the Simcenter Nastran User’s Guide.Note: When you open an existing material, where the Thermal Expansion Coefficient Type was not set, the software sets the Thermal Expansion Coefficient Type to the default value Undefined. The same applies when you read a material from your own material library file, where the CTE type for this material is not specified. |
| Specific Heat (CP) | In Simcenter Nastran structural solutions, this property is written to the MAT4 and MATT4 bulk entries. |
| Thermal Expansion | |
| Thermal Expansion (A1, A2, A3) | In Simcenter Nastran structural solutions, these properties are written to the following bulk entries:Material properties for shell elements are written to MAT8 and MATT8 bulk entries.Material properties for solid elements are written to MAT9 and MATT9 bulk entries.Material properties for axisymmetric elements are written to MAT3 and MATT3 bulk entries. |
| Thermal Conductivity | |
| Thermal Conductivity (K1, K2, K3) | In Simcenter Nastran thermal solutions, these properties are written to the MAT4 and MATT4 bulk entries. |
| Thermal Phase Change | |
| Latent Heat****Phase Change Temperature Range | In Simcenter Nastran thermal solutions, these properties are written to the MAT4 and MATT4 bulk entries. |
| Specific Heat above Phase Change | This property is not exported to Simcenter Nastran. It is used by the Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal solvers. |
| Infrared (IR) Coefficients | |
| Scattering****Extinction | These properties are not exported to Simcenter Nastran. They are used by the Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal solvers. |
| Solar Coefficients | |
| Scattering****Extinction | These properties are not exported to Simcenter Nastran. They are used by the Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal solvers. |
Electric page, Orthotropic properties
| Electrical Properties | |
|---|---|
| Resistivity | This property is not exported to Simcenter Nastran. It is used by the Thermal/Flow, Electronic Systems Cooling, Space Systems Thermal, and electromagnetic solvers. |
Damage page, Orthotropic properties
For the Samcef solver, damage properties predict fibers breaking, matrix cracking, and de-cohesion between fibers and the matrix. For more information, see Damage models for Orthotropic materials (Simcenter Samcef) and Damage Interface material (Simcenter Samcef).
Laminate page, Orthotropic properties
To activate the Laminate tab in the Orthotropic Material dialog box, follow these steps before starting NX or Simcenter 3D:
Create a folder named startup, preferably on your local drive as performance may suffer on a network drive.
Copy the Advanced_Woven.udmpx file from the**[software_installation_path]/nxcae_extras/laminate/LamPropsForOrthoMat** location to the startup folder.
Set the UGII_USER_DIR environment variable to point to the startup directory's parent folder.
| Default Ply Properties | |
|---|---|
| Ply Thickness | Sets the thickness of the ply. |
| Ply Color | Sets the ply color. Enter the color ID which is an integer between 1 and 216. You can see the color IDs in the Color dialog box. |
| Ply Failure Theory | Specifies the ply failure theory that the software uses. For more information, see Laminates failure analysis. |
| Interlaminar Failure Theory | Specifies the interlaminar failure theory. For more information, see Interlaminar failure analysis (2D and 3D). |
| Default Draping Parameters | |
| Draping Solver | Specifies the draping solver. For more information, see Draping solvers. |
| Lock Angle | Specifies the maximum amount of slippage that the fibers can withstand for a unidirectional ply.Specifies the maximum allowable shear angle for the woven ply. Buckling and bridging may occur beyond the maximum allowable shear angle.You can change the default lock angle value with the Lock Angle customer default. |
| Draping Path | Specifies how the primary direction is defined.GeodesicDefines the primary and secondary draping directions using the vector you select in the Draping Data dialog box.Seed CurveDefines the primary draping direction using the seed curve you define in the Draping Data dialog box. |
| Zone Angle Tolerance | Sets the change in yarn angle that the software uses to determine the anisotropic properties of the ply and the zones from which the ply properties are computed. The smaller the angle, the more properties are computed and the more zones are created. For more information, see Creating zones. |
| Account for Woven Fiber Shear | Activates the improved woven model for those global plies that point to this ply material and have the draping solver set to Woven or Imported.With the improved woven model, the software calculates the equivalent anisotropic properties for plies. |
| Ply Fibrous Influence Coefficient | |
| Ke | Appears when you select the Account for Woven Fiber Shear check box.Specifies the degree to which the ply elastic properties are fiber-driven. A value close to, but less than 1 indicates that the ply is significantly influenced by the properties of the fibers (for example carbon/epoxy system). Plies with less stiff fibers (for example glass) could have a value closer to 0.5. Ke is determined experimentally. |
Anisotropic material properties
Mechanical page, Anisotropic properties
| Material Property Matrix (Cij) | |||||||||||||||||||||||||||||
|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|---|
| Elements of the symmetric material property matrix in the material coordinate system. | In Simcenter Nastran structural solutions, these properties are written to the following bulk entries:The numbers of the matrices columns and rows correspond to the numbering used by Simcenter Nastran.Material properties for shell elements are written to the MAT2 and MATT2 bulk entries.Material properties for solid elements are written to the MAT9 and MATT9 bulk entries.The MAT9 bulk entry is used to define anisotropic material behavior for 3D elements. The constitutive relation is:Equation 47-1.where:σx σy σzNormal stressesτxy τyz τzxShear stressesεx εy εzNormal strainsγxy γyz γzxEngineering shear strainsCijElements of the 6 × 6 symmetric material property matrix in the material coordinate systemAiThermal Expansion coefficients (defined on Thermal page)(T − Tref)Temperature difference used to calculate thermal strainThe MAT2 bulk entry is used to define anisotropic material behavior for 2D elements. When using a MAT2 bulk entry, you define the in-plane material properties with respect to an element material coordinate system. The constitutive relation is given by:Equation 47-2.where:σ1 σ2Normal stressesτ12Shear stressε1 ε2Normal strainsγ12Engineering shear strainCijElements of the 3 × 3 symmetric material property matrix in the material coordinate systemA1 A2 A12Thermal Expansion coefficients (defined on Thermal page)(T − Tref)Temperature difference used to calculate thermal strainYou can also include material properties for transverse shear. When a MAT2 bulk entry is used for transverse shear, the transverse shear constitutive relation is:Equation 47-3. | σx σy σz | Normal stresses | τxy τyz τzx | Shear stresses | εx εy εz | Normal strains | γxy γyz γzx | Engineering shear strains | Cij | Elements of the 6 × 6 symmetric material property matrix in the material coordinate system | Ai | Thermal Expansion coefficients (defined on Thermal page) | (T − Tref) | Temperature difference used to calculate thermal strain | σ1 σ2 | Normal stresses | τ12 | Shear stress | ε1 ε2 | Normal strains | γ12 | Engineering shear strain | Cij | Elements of the 3 × 3 symmetric material property matrix in the material coordinate system | A1 A2 A12 | Thermal Expansion coefficients (defined on Thermal page) | (T − Tref) | Temperature difference used to calculate thermal strain |
| σx σy σz | Normal stresses | ||||||||||||||||||||||||||||
| τxy τyz τzx | Shear stresses | ||||||||||||||||||||||||||||
| εx εy εz | Normal strains | ||||||||||||||||||||||||||||
| γxy γyz γzx | Engineering shear strains | ||||||||||||||||||||||||||||
| Cij | Elements of the 6 × 6 symmetric material property matrix in the material coordinate system | ||||||||||||||||||||||||||||
| Ai | Thermal Expansion coefficients (defined on Thermal page) | ||||||||||||||||||||||||||||
| (T − Tref) | Temperature difference used to calculate thermal strain | ||||||||||||||||||||||||||||
| σ1 σ2 | Normal stresses | ||||||||||||||||||||||||||||
| τ12 | Shear stress | ||||||||||||||||||||||||||||
| ε1 ε2 | Normal strains | ||||||||||||||||||||||||||||
| γ12 | Engineering shear strain | ||||||||||||||||||||||||||||
| Cij | Elements of the 3 × 3 symmetric material property matrix in the material coordinate system | ||||||||||||||||||||||||||||
| A1 A2 A12 | Thermal Expansion coefficients (defined on Thermal page) | ||||||||||||||||||||||||||||
| (T − Tref) | Temperature difference used to calculate thermal strain | ||||||||||||||||||||||||||||
| Stress-Strain Related Properties | |||||||||||||||||||||||||||||
| **Yield Function Criterion (YF)****Hardening Rule (HR)****Initial Yield Point (LIMIT1)****Initial Friction Angle (LIMIT2)**Stress-Strain (H) | See the description provided previously in the Isotropic material properties section. | ||||||||||||||||||||||||||||
| Type of Nonlinearity (TYPE) | |||||||||||||||||||||||||||||
| Stress-Strain Input Data Type | |||||||||||||||||||||||||||||
| Strain Rate Dependency | |||||||||||||||||||||||||||||
| Exponent (BVALUE) | |||||||||||||||||||||||||||||
| Strain Rate Level (TSRATE) | |||||||||||||||||||||||||||||
| Strain Rate****Specify Field |
Thermal page, Anisotropic properties
| Properties | |
|---|---|
| Temperature (TREF) | Sets the reference temperature of the anisotropic material. |
| Specific Heat (CP) | Sets the specific heat of the anisotropic material.In Simcenter Nastran thermal solutions, these properties are written to the MAT5 and MATT5 bulk entries. The numbers of the matrix columns and rows correspond to the numbering used by Simcenter Nastran. |
| Thermal Expansion (Ai) | |
| Thermal Expansion Coefficient Type | Selects a Secant or Tangent type for the thermal expansion coefficient (CTE). For more information on CTE, see Understanding Coefficient of Thermal Expansion (CTE) in the Simcenter Nastran User’s Guide.Note: When you open an existing material, where the Thermal Expansion Coefficient Type was not set, the software sets the Thermal Expansion Coefficient Type to the default value Undefined. The same applies when you read a material from your own material library file, where the CTE type for this material is not specified. |
| Thermal Expansion Coefficient | See the information listed previously for the MAT2/MAT9 bulk entries. |
| Thermal Conductivity (Kij) | |
| Sets the values for the six unique terms of the symmetric thermal conductivity matrix.In Simcenter 3D Multiphysics, Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal environments, the magnitude of each off-diagonal term must be less than the magnitude of the smallest diagonal term. |
Electromagnetic page, Anisotropic properties
These properties are not exported to Simcenter Nastran. They are used by the electromagnetic environments.
For more information, see Electromagnetic anisotropic material properties.
Other Physical Properties page, Anisotropic properties
These properties are not exported to Simcenter Nastran. They are used by the electromagnetic environments and are available when the Property View is set to All Properties, Simcenter MAGNET Thermal Electromagnetic, or Simcenter MAGNET Thermal Electric.
| Dynamic Viscosity | |
|---|---|
| Dynamic Viscosity Control | Specifies how to control dynamic viscosity.Constant or TemperatureThe dynamic viscosity can be constant or temperature dependent.Temperature and PressureThe dynamic viscosity is defined with field values.Note: Available when Property View is set to All Properties. |
| Dynamic Viscosity | Appears when Dynamic Viscosity Control is set to Constant or Temperature.Lets you enter a constant dynamic viscosity value or when you click , you can define temperature-dependent dynamic viscosity values.For more information, see Magnitude options above. |
| Specify Dynamic Viscosity field | Available when Property View is set to All Properties.Lets you select an existing field, use a formula or table, or table of fields to define temperature and pressure-dependent dynamic viscosity values. |
Fluid material properties
For more information, see Fluid materialsfor heat transfer and flow analyses and Fluid materials for acoustic analyses.
| Properties | |
|---|---|
| Density Control | Available when Property View is set to All Properties.Specifies how to control density.Constant or Temperature or FrequencyThe density can be constant, or dependent on temperature or frequency.Direct ComplexThe density is defined with Real and Imaginary values.Temperature and PressureThe density can be dependent on both the temperature and the pressure.Note: This property is not exported to Simcenter Nastran. It is used by Simcenter 3D Multiphysics, Simcenter 3D Thermal/Flow, Simcenter 3D Space Systems Thermal, Simcenter 3D Electronic Systems Cooling, or Samcef. |
| **Mass Density (RHO)**Damping Coefficient (GE) | In Simcenter Nastran structural solutions: If Density Control is set to Constant or Temperature or Frequency, these properties are written to the MAT10 bulk entry.If Density Control is set to Direct Complex, and Mass Density (RHO) is set to Real/Imaginary or Magnitude/Phase, only Mass Density (RHO) is written to the MAT10C bulk entry.If Density Control is set to Direct Complex, and Mass Density (RHO) is set to Field, only Mass Density (RHO) is written to the MAT10C, MATF10C, and TABLED1 bulk entries. |
Mechanical page, Fluid properties
| Properties | |
|---|---|
| **Bulk Modulus (K)**Bulk Modulus Ratio (Gamma) | In Simcenter Nastran structural solutions, these properties are written to the MAT10 bulk entry. |
| Speed of Sound Control | Available when Property View is set to All Properties.Specifies how to control speed of sound.ConstantThe speed of sound can be constant.Complex and FrequencyThe speed of sound can be complex with frequency dependency. |
| Speed of Sound (C) | In Simcenter Nastran acoustic and vibro-acoustic, and Simcenter 3D Acoustics BEM solutions, the Speed of Sound (C) can be constant, or complex and frequency dependent. |
Thermal page, Fluid properties
| Properties | |
|---|---|
| **Thermal Expansion Coefficient (B)****Thermal Conductivity (K)**Specific Heat (CP) | These properties are not exported to Simcenter Nastran. They are used by the Simcenter 3D Multiphysics, Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal environments. |
Other Physical Properties page, Fluid properties
| General Properties | |
|---|---|
| Molar Mass****Gas Constant | These properties are not exported to Simcenter Nastran. They are used by the Simcenter 3D Multiphysics, Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal environments. |
| Dynamic Viscosity | |
| Dynamic Viscosity | This property is not exported to Simcenter Nastran. It is used by the Simcenter 3D Multiphysics, Simcenter 3D Thermal/Flow, Simcenter 3D Electronic Systems Cooling, and Simcenter 3D Space Systems Thermal, environments. |
Miscellaneous page, Fluid properties
See the description provided later in the Visual material properties section.
Material Conversion page, Fluid properties
To activate the Material Conversion page in the Fluid Material dialog box, copy the Material_Conversion.udmpx file from the %UGII_TMG_DIR%\customization directory location to the any UGOPEN_STARTUP_DIR folder, such as %UGII_USER_DIR%\startup, %UGII_SITE_DIR%\startup, or %UGII_VENDOR_DIR%\startup before starting NX or Simcenter 3D.
| Properties | |
|---|---|
| Specify Material Conversion Properties | Changes the original fluid material properties of a the fluid material specified in the Convert to Material box after the temperature of a 1D fluid element reaches the value specified in the Threshold Temperature box. |
Multiple Fluid material properties
These properties are not exported to Simcenter Nastran. They are used by the thermal solver in Simcenter 3D Multiphysics, Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal. For more information, see Multiple Fluid materials.
Durability material properties
These properties are not exported to Simcenter Nastran. They are used by the Durability capability. For more information, see Simcenter 3D Durability.
Formability material properties
These properties are not exported to Simcenter Nastran. They are used by the One-step Formability Analysis tool. See One-step Formability Analysis overview for more information.
Creep material properties
For information about creep properties, see:
Nastran creep material properties
Abaqus creep material properties
ANSYS creep material properties
The following options appear for SOLs 401 and 402 when Property View is set to Simcenter Nastran MAT1/MPLAS/MVPLAS. Some of the properties, such as Power Law Creep Coefficients, are available for other solvers and creep laws.
| Creep Law list | Specifies the creep law for SOLs 401 or 402 visco-plastic material.**Strain Hardening Creep (MVPLAS/Law STRNHARD)****Norton Creep (MVPLAS/Law NORTON)****Generalized Garofalo Creep (MVPLAS/Law GENGAROF)****Norton-Bailey in Time Hardening Creep (MVPLAS/Law TIMEHARD)**User Creep (MVPLAS/Law USER + MUCRP on Bulk Data user defined text) |
| Threshold Strain (THRESH) | Appears for all creep laws except User Creep (MVPLAS/Law USER + MUCRP on Bulk Data user defined text) |
| Anisotropy | Specifies how you want to set anisotropic plasticity and creep. To apply Von Mises stress to the creep laws, select None.To set anisotropic creep for visco-plastic materials only, select Hill and set the Hill yield criterion ratios (R11, R22, R33, R112, R23, R13) in the boxes that appear.To set anisotropic creep and plasticity for plastic and visco-plastic materials, select MPLAS and set the anisotropy on the plastic material.Note: To define both plasticity and anisotropic creep: On the Mechanical page, set Yield Function Criterion (TF) to Hill by Stress Ratios (associated with MPLAS bulk entry).On the Creep page, set Anisotropy to MPLAS. |
| Power Law Creep Coefficients | |
| Appears for all creep laws except for Generalized Garofalo Creep (MVPLAS/Law GENGAROF) and User Creep (MVPLAS/Law USER + MUCRP on Bulk Data user defined text). | |
| Check Unit System | Specifies whether to check for units when the material is exported to the solver. |
| Units(Force)(Length)(Mass) | Appears when Check Unit System is set to Yes.Specifies the unit system to use when the material is exported to the solver input file. This is useful to properties whose units are not designated in the dialog box. For example, the units for Rate Strain Factor (C1) [1/(Pressure^C2 * Time)] can vary depending on the value for C2, so the value is dimensionless in the dialog box. |
| Viscoplastic Creep Coefficients | |
| The options that appear change depending on the coefficients in the equation of the specified creep law. Each option name includes the coefficient that appears in the equation.Except for the absolute temperature options, the values you enter are temperature-dependent scalar fields.Note: C1 is 1/time, represented as Hz in this dialog box. Thus, if your main factor is 1/hours or 1/days, convert the value to seconds (Hz) before adding it.If the value for C1 is less than 1E-15, the value is filtered out and treated as zero when the simulation is exported. To avoid that, manually update the threshold to consider numbers as 0 in the Real Data Filter Value box on the Formatting Options tab in the Advanced Solver Options dialog box. For more information, see Export Simulation/Advanced Solver Options dialog box—Nastran. |
Viscoelasticity material properties
For information about viscoelasticity properties, see Abaqus viscoelastic material properties.
Hyperelastic and gasket material properties
For general information about hyperelastic and gasket material properties, see Hyperelastic, gasket, and shape memory alloy material models.
For information about Nastran hyperelastic material properties, see Hyperelastic materials for Nastran analyses.
For information about ANSYS gasket material properties, see Defining a gasket displacement material for ANSYS analyses.
Miscellaneous material properties page
| Visual Properties | |
|---|---|
| RGB Color, Studio Material, and Select Studio Material Name properties support functionality that will be included in a future release. | |
| Crosshatch Pattern | Applies a crosshatch pattern type to the material. This crosshatch pattern is displayed when the material is assigned to an object and that object is sectioned in a PMI lightweight section view. For more information, see Lightweight Section View in the PMI Help. Type the name of any supported crosshatch pattern. Valid pattern names are provided in crosshatch definition files included with this software. For more information about crosshatch patterns, see Crosshatch patterns in the Drafting Help.Note: Only crosshatch patterns are supported. You cannot use area fill patterns. |
| Coating Layer Attributes | |
| These properties support functionality that will be included in a future release. | |
| Shipbuilding Insulation Attributes | |
| Fixed Stock ThicknessDefault ThicknessAdhesive | Assign thickness and adhesive properties to materials used for insulation in a ship.We recommend that you use the Steel Insulation command to model the insulation in a ship and define the materials in the ship materials spreadsheet.For more information, see Steel Insulation in the Shipbuilding Help. |
| Pedestrian Protection | |
| Specifies the Offset distance of the impacted surface for the child head impact zone, adult head impact zone, and the leg impact zone in compliance with the various pedestrian protection regulations.The default values of the Offset distance are only for reference. You must assign the appropriate values for the Offset distance as per the applicable material, based on the industry standards or customer specific requirements.Only isotropic materials support this property.When you assign an isotropic material to the components of the hood system in a vehicle, the Pedestrian Protection command uses the offset value of the assigned isotropic material to generate the head impact and leg impact zones.For more information, see Pedestrian Protection in the Vehicle Design Help. |
User Models - Simcenter Nastran material properties
These properties are only available when user-defined material (also referred to as UMAT) models are defined in the current environment. The structural and coupled analyses in Simcenter 3D Multiphysics use these properties. For more information, see Simcenter Nastran user-defined material models.
| Model Type | |
|---|---|
| None(additional model types) | No user-defined material properties are written to a bulk entry.User-defined material properties are written to the Simcenter Nastran MUMAT bulk entry. |
Porous material properties
These properties are only available in an acoustic or vibro-acoustic analysis in Simcenter Nastran. Porous material properties are written to the Simcenter Nastran MATPOR bulk entry. For more information, see Porous materials.
| Acoustics tab, Properties group | |
|---|---|
| Porous Models | Lets you choose between Craggs, Delany-Bazley-Miki, and Johnson-Champoux-Allard material models. |
| Speed of Sound (C) | |
| Static Flow Resistivity | |
| Porosity****Tortuosity |
How do I
Assign a material using a mesh collector
Assign a material to a body
Use an inherited material in a physical property table
Override a material assignment in a Simulation file
Create a material
Define a material with stress-strain data
Create a new material by copying another material
Define a material property using a formula field
Define a material property using a table field
Revert material properties to their inherited values
Lock an inherited material property
Learn more
Materials
Defining materials for Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal
Isotropic materials
Orthotropic materials
Anisotropic materials
Defining materials for laminate plies
Specifying stress-strain data for nonlinear materials
Look up more details
Nastran creep material properties
Abaqus creep material properties
ANSYS creep material properties
Abaqus viscoelastic material properties
Material properties for durability analysis
Hyperelastic, gasket, and shape memory alloy material models
Hyperelastic materials for Nastran analyses
Abaqus keywords supported for import and export
ANSYS commands supported for import and export
Exporting Nastran data
LS-DYNA keywords supported for import and export
Quick links
Command reference
Pre/Post video examples
Bulk Entry Descriptions
Simcenter 3D tutorials
Browse Simcenter 3D help by product area
Related Topics
Electromagnetic material properties
Material dialog box, Simcenter 3D 2021.1 Series
© 2020 Siemens
window.mainLanguage="en_US"
window.delivId=""
window.projectId=""
MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });
Source: https://docs.sw.siemens.com/en-US/doc/289054037/PL20200601120302950.advanced/id636376 · retrieved 2026-07-17