Design Objective - Global dialog box

Modeling Object
Name	Sets a unique name for the design objective.
Label	Sets a unique integer for the modeling object.The dialog box automatically displays the next available modeling object number. However, you might want to change this if you use a particular series of numbers to identify certain types of modeling objects.
Properties
Description	Sets a description for the design objective.You can also click Description to open the Description dialog box. This lets you see more of the text that you type, as well as cut, copy, or paste text.This description appears only on this dialog box.
Response Definition	Definition MethodSpecifies the approach to use for completing this dialog box:Standard—Limits the Response Type list to the most common responses.Any weight response is assumed to be in the Z-direction, indicating that there is no directional mass.Advanced—Displays a complete list of responses in the Response Type list and enables you to specify the direction of the mass when Response Type is set to Total Model Weight (WEIGHT).Response LabelSets the design response identifier to write to the .f06 file when you solve the solution.This label must begin with an alphabetic character.Response TypeSpecifies the response that you want to minimize or maximize.This list displays only responses that are appropriate for a solution. In addition, if Definition Method is set to Standard, this list displays only the most common responses.For more information about response types, see DRESP1.Note: If you select Compliance, make sure that the Inertia Relief (INREL) check box is cleared in the Bulk Data page on the Solution dialog box for your topology optimization solution. If that check box is selected, the solve will fail.DirectionAppears when Definition Method is set to Advanced and Response Type is set to Total Model Weight (WEIGHT).Specifies the direction of the weight.Select Mx, My, or Mz to specify the direction of the mass using a specific axis of the absolute coordinate system, or select Ix, Iy, or Iz to specify the direction of inertia. Select Row/Column Entry to use the Simcenter Nastran grid point weight generator.Row Number/Column NumberAppear when Direction is set to Row/Column Entry.Set the row and column number to use in the Simcenter Nastran rigid body mass or weight matrix. Based on the value in this matrix, the Simcenter Nastran grid point weight generator computes the mass properties, centers of gravity, and inertias of the structure.The default values for Row Number and Column Number are 3, which specifies Wz (mass or weight in the Z-direction of the absolute coordinate system). This default value is appropriate for models that have no directional mass. If no directional mass is defined (for example, if no CONM1, CMASS, or DMI bulk entries exist), the Wx, Wy, and Wz values each equal the mass or weight of the structure.By default, the mass properties calculation is performed relative to the origin of the absolute coordinate system, which is the same as the Simcenter Nastran basic coordinate system. However, if you define the GRDPNT parameter, the calculation is performed relative to the reference node you specify.To define the GRDPNT parameter, in the Case Control page in the Solution dialog box, click Create Modeling Object next to Parameters (PARAM), and then click G-H in the list. If you type a different value in the GRDPNT box, the parameter is added to the solution. To add the parameter and retain the default value, click Add .For more information, see DRESP1, Overview of the Grid Point Weight Generator, and Weight Center of Gravity and Moment of Inertia Check.DOF1–DOF6Appear when Response Type is set to Displacement (DISP) or SPCForce (SPCFORCE).Specifies whether to apply the objective to translational (DOF1–DOF3) or rotational (DOF4–DOF6) degrees of freedom for the displacement coordinate system of the selected node.Lamina NumberAppears when Response Type is set to Composite Strain (CSTRAIN), Composite Stress (CSTRESS), or Composite Failure (CFAILURE).Sets the number of the ply layer whose response you want to minimize or maximize.Element Specification MethodAppears when Response Type is set to Strain (STRAIN), Strain Energy (ESE), Stress (STRESS), Force (FORCE), Composite Strain (CSTRAIN), Composite Stress (CSTRESS), Composite Failure (CFAILURE), Frequency Response Force (FRFORC), or Frequency Response Stress (FRSTRE).Specifies the method to use for selecting the elements to use for the response.Select Element Selection to select the elements using a group or the graphics window. Select Physical Property to select them using a physical property table.Element DimensionAppears when Response Type is set to Strain (STRAIN), Strain Energy (ESE), Stress (STRESS), Force (FORCE), Frequency Response Force (FRFORC), or Frequency Response Stress (FRSTRE), and when Element Specification Method is set to Element Selection.Specifies the dimension of the elements to use for the response, such as 3D for a tetrahedral mesh.The options that appear in this list vary, depending on your selection in the Response Type list.Element TypeAppears when Response Type is set to Strain (STRAIN), Strain Energy (ESE), Stress (STRESS), Force (FORCE), Frequency Response Force (FRFORC), or Frequency Response Stress (FRSTRE), and when Element Dimension is set to 0D or 1D.Specifies the type of element to use for the response.The options that appear in this list vary, depending on your selection in the Element Dimension list.TypeAppears when Element Specification Method is set to Physical Property.Specifies the type of physical property table to use for selecting the elements.The options that appear in this list vary, depending on your selection in the Response Type list.Physical Property Appears when Element Specification Method is set to Physical Property.Specifies the physical property table to use.If the list is extensive, click More Options to search for a particular physical property table or filter the list.You can also click Create Physical to create a new physical property table for the selected physical property type, or click Open Manager to edit an existing physical property table.Element ResultAppears when Response Type is set to Strain (STRAIN), Strain Energy (ESE), Stress (STRESS), Force (FORCE), Composite Strain (CSTRAIN), Composite Stress (CSTRESS), Composite Failure (CFAILURE), Frequency Response Force (FRFORC), or Frequency Response Stress (FRSTRE).Specifies the element result to use as the response.The options that appear in this list vary, depending on your selection in the Response Type list and other element specification options.If Item Code appears in the list, you can select that option and then set the appropriate Simcenter Nastran item code.Item CodeAppears when Element Result is set to Item Code.Sets the Simcenter Nastran item code to use as the response.Note: For some element types, the response value depends on the location setting for the structural output request. You can set this in the case control for the solution.For more information about item codes, see Item Codes.Normal Modes Mode NumberAppears when Response Type is set to Eigenvalue Modes (EIGN) or Normal Modes (FREQ).Sets the number of the normal mode whose response you want to minimize or maximize.Buckling Mode NumberAppears when Response Type is set to Buckling Modes (LAMA).Sets the number of the buckled mode whose response you want to minimize or maximize.Approximation CodeAppears when Response Type is set to Eigenvalue Modes (EIGN), Normal Modes (FREQ), or Buckling Modes (LAMA).Specifies whether to use direct or inverse linearization.Output FormatAppears when Response Type is set to Frequency Response Displacement (FRDISP), Frequency Response Velocity (FRVELO), Frequency Response Acceleration (FRACCL), Frequency Response Force (FRFORC), Frequency Response SPCForce (FRSPCF), or Frequency Response Stress (FRSTRE).When the dynamic response is complex, specifies whether the solution output uses real/imaginary or magnitude/phase values.This option should match the Data Format setting for the structural output request modeling object for your solution. For example, if Data Format is set to REAL or IMAG, set Output Format to Real/Imaginary. If Data Format is set to PHASE, set Output Format to Magnitude/Phase.ComponentAppears when Response Type is set to Frequency Response Displacement (FRDISP), Frequency Response Velocity (FRVELO), Frequency Response Acceleration (FRACCL), or Frequency Response SPCForce (FRSPCF).Specifies the translational (X, Y, or Z) or rotational (RX, RY, or RZ) component associated with the tensor value that you want to use (real, imaginary, magnitude, or phase).The components are relative to the displacement coordinate system for the selected node.For example, to use the phase angle from the Y-displacement output for your response, you would set Data Format to PHASE for Displacement in the structural output request modeling object for your solution. In this dialog box, you would set Response Type to Frequency Response Displacement (FRDISP), set Output Format to Magnitude/Phase, and set Component to Y, Phase.Frequency Math Function TypeAppears when Response Type is set to Frequency Response Displacement (FRDISP), Frequency Response Velocity (FRVELO), Frequency Response Acceleration (FRACCL), Frequency Response Force (FRFORC), Frequency Response SPCForce (FRSPCF), or Frequency Response Stress (FRSTRE).Specifies how to determine the frequency response value to minimize or maximize.You can either select Value and then specify the value, or you can select a math function to compute the frequency response value across multiple frequencies:SUM—Uses the sum of the response values.AVG—Uses the average response value.SSQ—Uses the sum of the squares of the response values.RSS—Uses the square root of the sum of the squares of the response values.MAX—Uses the maximum response value.MIN—Uses the minimum response value.Frequency ValueAppears when Frequency Math Function Type is set to Value.Sets the frequency response value.
Node Selection	Appears when Response Type is set to Displacement (DISP), SPCForce (SPCFORCE), Frequency Response Displacement (FRDISP), Frequency Response Velocity (FRVELO), Frequency Response Acceleration (FRACCL), or Frequency Response SPCForce (FRSPCF). Group ReferenceLets you select nodes by selecting a group.For more information, see Group Reference options.Select Node Available when the Group Reference check box is cleared.Lets you select nodes in the graphics window.ExcludedLets you exclude certain nodes from selection.
Element Selection	Appears when Element Specification Method is set to Element Selection. Group ReferenceLets you select elements by selecting a group.For more information, see Group Reference options.Select 0D Element Appears when Element Dimension is set to 0D. Available when the Group Reference check box is cleared.Lets you select 0D elements in the graphics window.Select 1D Element Appears when Element Dimension is set to 1D. Available when the Group Reference check box is cleared.Lets you select 1D elements in the graphics window.Select 2D Element Appears when Element Dimension is set to 2D Shell or 2D Shear. Available when the Group Reference check box is cleared.Lets you select 2D elements in the graphics window.Select 3D Element Appears when Element Dimension is set to 3D. Available when the Group Reference check box is cleared.Lets you select 3D elements in the graphics window.ExcludedLets you exclude certain elements from selection.Note: If you select elements in the graphics window, be sure to select only elements of the appropriate type. For example, if Element Dimension is set to 1D and Element Type is set to CBEAM, you can select any 1D element, even if it is not a CBEAM element.If you select elements that are not the appropriate type, Simcenter Nastran might use unintended responses from other elements for which the response item code is still valid.
Subcase Internal Combination Method	Appears when Response Type is set to Displacement (DISP), Strain (STRAIN), Strain Energy (ESE), Stress (STRESS), Force (FORCE), SPCForce (SPCFORCE), Composite Strain (CSTRAIN), Composite Stress (CSTRESS), or Composite Failure (CFAILURE).Specifies how to determine the response value to use for each individual subcase.For example, with a displacement response, you might select multiple nodes, and indicate that you want to use the average response for all the selected nodes.For information about the math functions, see Frequency Math Function Type above.
Across Subcase Combination Method	Appears when Response Type is set to Compliance (CMPLNCE), Displacement (DISP), Strain (STRAIN), Strain Energy (ESE), Stress (STRESS), Force (FORCE), SPCForce (SPCFORCE), Composite Strain (CSTRAIN), Composite Stress (CSTRESS), Composite Failure (CFAILURE), Eigenvalue Modes (EIGN), Normal Modes (FREQ), or Buckling Modes (LAMA).Specifies how to determine the response value to use from multiple subcases.For information about the math functions, see Frequency Math Function Type above.
Optimization Method	Specifies the goal of the design objective.MAXMaximizes the selected response.MINMinimizes the selected response.
Card Name	Displays the names of the Simcenter Nastran bulk entries that will be generated when you solve the solution: DESOBJ and DRESP1.

How do I

Create the design objective for topology optimization

Learn more

Design objectives in topology optimization

Working with nodal coordinate systems

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Design Objective - Global 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 } });