Responses

The following responses can be found in this section:

OptiStruct allows the use of numerous structural responses, calculated in a finite element analysis, or combinations of these responses to be used as objective and constraint functions in a structural optimization.

Responses are defined using DRESP1 bulk data entries. Combinations of responses are defined using either DRESP2 entries, which reference an equation defined by a DEQATN bulk data entry, or DRESP3 entries, which make use of user-defined external routines identified by the LOADLIB I/O option. Responses are either global or subcase (loadstep, load case) related. The character of a response determines whether or not a constraint or objective referencing that particular response needs to be referenced within a subcase.

Subcase Independent

Mass and Volume

Both are global responses that can be defined for the whole structure, for individual properties (components) and materials, or for groups of properties (components) and materials.

It is not recommended to use mass and volume as constraints or objectives in a topography optimization. Neither is very sensitive towards design modifications made in a topography optimization.

In order to constrain the mass or volume for a region containing a number of properties (components), the SUM function can be used to sum the mass or volume of the selected properties (components), otherwise, the constraint is assumed to apply to each individual property (component) within the region. Alternatively, a DRESP2 equation needs to be defined to sum the mass or volume of these properties (components). This can be avoided by having all properties (components) use the same material and applying the mass or volume constraint to that material.

RTYPE=VOLUME and ATTA=ENCLOSED can be used to create an enclosed volume response for Shape, Free-Shape, and Topography optimization. The ENCLOSED option indicates that this response is an enclosed volume defined by a closed 2D mesh (free-edges are not supported). For this enclosed volume response type, ATTI field(s) should be set to PID. Multiple ATTi are allowed, as long as the mesh defined by the PID’s is fully enclosed. The property type should be PSHELL, PCOMP, or PSHEAR only. The normals of the 2D mesh should be oriented consistently and the mesh should be sufficiently fine to capture the volume data. The volume is calculated based on the mesh and it is not recommended to use a coarse mesh.

Fraction of Mass and Fraction of Design Volume

Both are global responses with values between 0.0 and 1.0. They describe a fraction of the initial design space in a topology optimization. They can be defined for the whole structure, for individual properties (components) and materials, or for groups of properties (components) and materials.

The difference between the mass fraction and the volume fraction is that the mass fraction includes the non-design mass in the fraction calculation, whereas the volume fraction only considers the design volume.

Formulation for volume fraction:
Volume fraction = (total volume at current iteration – initial non-design volume)/initial design volume

Formulation for mass fraction:
Mass fraction = total mass at current iteration/initial total mass

If, in addition to the topology optimization, a size and shape optimization is performed, the reference value for the volume fraction (the initial design volume) is not altered by size and shape changes. This can, on occasion, lead to negative values for this response. Therefore, if size and shape optimization is involved, it is recommended to use the Volume responses instead of the Volume Fraction response.

These responses can only be applied to topology design domains. OptiStruct will terminate with an error if this is not the case.

Center of Gravity

This is a global response that may be defined for the whole structure, for individual properties (components) and materials, or for groups of properties (components) and materials.

Moments of Inertia

This is a global response that may be defined for the whole structure, for individual properties (components) and materials, or for groups of properties (components) and materials.

Weighted Compliance

The weighted compliance is a method used to consider multiple subcases (loadsteps, load cases) in a classical topology optimization. The response is the weighted sum of the compliance of each individual subcase (loadstep, load case).

This is a global response that is defined for the whole structure.

Weighted Reciprocal Eigenvalue (Frequency)

The weighted reciprocal eigenvalue is a method to consider multiple frequencies in a classical topology optimization. The response is the weighted sum of the reciprocal eigenvalues of each individual mode considered in the optimization.

This is done so that increasing the frequencies of the lower modes will have a larger effect on the objective function than increasing the frequencies of the higher modes. If the frequencies of all modes were simply added together, OptiStruct would put more effort into increasing the higher modes than the lower modes. This is a global response that is defined for the whole structure.

Combined Compliance Index

The combined compliance index is a method to consider multiple frequencies and static subcases (loadsteps, load cases) combined in a classical topology optimization. The index is defined as follows:

This is a global response that is defined for the whole structure.

The normalization factor, NORM, is used to normalize the contributions of compliances and eigenvalues. A typical structural compliance value is of the order of 1.0e4 to 1.0e6. However, a typical inverse eigenvalue is on the order of 1.0e-5. If NORM is not used, the linear static compliance requirements dominate the solution.

The quantity NORM is typically computed using the formula:

Where, Cmax is the highest compliance value in all subcases (loadsteps, load cases) and is the lowest eigenvalue included in the index.

In a new design problem, you may not have a close estimate for NORM. If this happens, OptiStruct automatically computes the NORM value based on compliances and eigenvalues computed in the first iteration step.

Stress Responses for Topology and Free-Size Optimization

Actual Stress Responses for Topology and Free-Size Optimization are available through corresponding Stress response RTYPE’s on the DRESP1 Bulk Data Entry. The Stress-NORM aggregation is internally used to calculate the Stress Responses for groups of elements in the model.

von Mises Stress in a Topology or Free-Size Optimization

Additionally, von Mises stress constraints may be defined for topology and free-size optimization through the STRESS optional continuation line on the DTPL or the DSIZE card. There are a number of restrictions with this constraint:

•

The definition of stress constraints is limited to a single von Mises permissible stress. The phenomenon of singular topology is pronounced when different materials with different permissible stresses exist in a structure. Singular topology refers to the problem associated with the conditional nature of stress constraints, i.e. the stress constraint of an element disappears when the element vanishes. This creates another problem in that a huge number of reduced problems exist with solutions that cannot usually be found by a gradient-based optimizer in the full design space.

•

Stress constraints for a partial domain of the structure are not allowed because they often create an ill-posed optimization problem since elimination of the partial domain would remove all stress constraints. Consequently, the stress constraint applies to the entire model when active, including both design and non-design regions, and stress constraint settings must be identical for all DSIZE and DTPL cards.

•	The capability has built-in intelligence to filter out artificial stress concentrations around point loads and point boundary conditions. Stress concentrations due to boundary geometry are also filtered to some extent as they can be improved more effectively with local shape optimization.

•	Due to the large number of elements with active stress constraints, no element stress report is given in the table of retained constraints in the .out file. The iterative history of the stress state of the model can be viewed in HyperView or HyperMesh.

•	Stress constraints do not apply to 1D elements.

•	Stress constraints may not be used when enforced displacements are present in the model.

Bead Discreteness Fraction

This is a global response for topography design domains. This response indicates the amount of shape variation for one or more topography design domains. The response varies in the range 0.0 to 1.0 (0.0 < BEADFRAC < 1.0), where 0.0 indicates that no shape variation has occurred, and 1.0 indicates that the entire topography design domain has assumed the maximum allowed shape variation.

Random Response Analysis

PSD and RMS Responses

PSD displacement, PSD velocity, PSD acceleration, PSD acoustic pressure, PSD stress, PSD strain, RMS displacement, RMS velocity, RMS acceleration, RMS acoustic pressure, RMS stress, and RMS strain responses are available as global, as well as subcase-dependent responses (this information is also available in the Subcase Dependent responses section below).

Subcase Dependent

Linear Static Analysis

Static Compliance

The compliance C is calculated using the following relationship:

where

For a structure with an applied forces f subcase, the compliance C can be considered a reciprocal measure of the stiffness K:

Where, is constant.

For maximum stiffness K, the compliance C can be minimized.

For a structure with an applied displacements u subcase, the compliance C can be considered a direct measure of the stiffness K:

Where, is constant.

Elements in the Compliance

Compliance can be defined for the whole structure, for individual properties (components) and materials, or for groups of properties (components) and materials. The compliance must be assigned to a linear static subcase (loadstep, load case).

In order to constrain the compliance for a region containing a number of properties (components), the SUM function can be used to sum the compliance of the selected properties (components), otherwise, the constraint is assumed to apply to each individual property (component) within the region. Alternatively, a DRESP2 equation needs to be defined to sum the compliance of these properties (components). This can be avoided by having all properties (components) use the same material and applying the compliance constraint to that material.

Static Displacement

Displacements are the result of a linear static analysis. Nodal displacements can be selected as a response. They can be selected as vector components or as absolute measures. They must be assigned to a linear static subcase.

Static Stress of Homogeneous Material

Different stress types can be defined as responses. They are defined for components, properties, or elements. Element stresses are used, and constraint screening is applied. It is also not possible to define static stress constraints in a topology design space (see above). This is a linear static subcase (loadstep, load case) related response.

Static Strain of Homogeneous Material

Different strain types can be defined as responses. They are defined for components, properties, or elements. Element strains are used, and constraint screening is applied. It is also not possible to define strain constraints in a topology design space. This is a linear static subcase (loadstep, load case) related response.

Static Stress of Composite Lay-up

Different composite stress types can be defined as responses. They are defined for PCOMP(G) components or elements, or PLY type properties. Ply level results are used, and constraint screening is applied. It is also not possible to define composite stress constraints in a topology design space. This is a linear static subcase (loadstep, load case) related response.

Static Strain of Composite Lay-up

Different composite strain types can be defined as responses. They are defined for PCOMP(G) components or elements, or PLY type properties. Ply level results are used, and constraint screening is applied. It is also not possible to define composite strain constraints in a topology design space. This is a linear static subcase (loadstep, load case) related response.

Static Failure in a Composite Lay-up

Different composite failure criterion can be defined as responses. They are defined for PCOMP(G) components or elements, or PLY type properties. Ply level results are used, and constraint screening is applied. It is also not possible to define composite failure criterion constraints in a topology design space. This is a linear static subcase (loadstep, load case) related response.

Static Force

Different force types can be defined as responses. They are defined for components, properties, or elements. Constraint screening is applied. It is also not possible to define force constraints in a topology design space. This is a linear static subcase (loadstep, load case) related response.

Single Point Force at a constrained grid point

This response can be defined using the DRESP1 bulk data entry (RTYPE=SPCFORCE). This response is defined for constrained grid points. Constraint screening is applied to this response. This is a linear static subcase (loadstep, load case) related response.

Grid Point Force

This response can be defined using the DRESP1 bulk data entry (RTYPE=GPFORCE). This response defines the contribution to a specific grid point force component from a non-rigid element (which is connected to that grid). Constraint screening is applied to this response. If ATTi specify multiple elements, then multiple responses will be generated; where, each response calculates a specified element’s contribution to the grid point force component at the specified grid. This is a linear static subcase (loadstep, load case) related response.

Heat Transfer Analysis

Temperature

Temperatures are the result of a heat transfer analysis, and must be assigned to a heat transfer subcase (loadstep, load case). Temperature response cannot be used in composite topology and free-size optimization.

Thermal Compliance

Thermal compliance C is calculated using:

Where, T is the temperature vector, f is the power vector, KC is the conduction matrix, and H is the convection matrix. Thermal compliance is a global measure for structural heat transfer problem. It is calculated for the entire structure. Thermal compliance must be assigned to a linear steady state heat transfer subcase (loadstep, load case).

When minimizing thermal compliance, temperatures at grids of flux input are minimized. The optimum structure provides maximum conduction of thermal energy. Since thermal compliance is a smooth convex function, it is typically more efficient to minimize thermal compliance than to perform a min-max of the temperature of the entire structure. During thermal-structural optimization, the temperature field is updated for each iteration. Additionally, for thermal-structural topology optimization, the density design variable affects the conductivity, and the conductivity is also penalized.

Thermal Compliance Response can only be used in Sizing, Shape, Topology, and Free-Size Optimization.

Normal Modes Analysis

Frequency

Natural frequencies are the result of a normal modes analysis, and must be assigned to the normal modes subcase (loadstep, load case). It is recommended to constrain the frequency for several of the lower modes, not just of the first mode.

There are two ways to use Normal Mode response in an Optimization run:

1.	Set the ATTA field on DRESP1 entry equal to the Normal Mode number(s) that you want to use as a response. In this process, you will identify and provide the mode number(s) that are to be optimized.

You can also source the mode number of the mode with largest modal participation at the peak loading frequency by adding a separate Modal Frequency Response Subcase, in addition to the existing Normal Modes subcase. The ATTA field should be left blank and the ATTi field should be set equal to the subcase ID of the Modal Frequency Response subcase. The Modal Frequency Response Analysis subcase should contain a PEAKOUT entry that identifies peak identification criteria. OptiStruct will internally identify the mode that is to be optimized based on Modal Frequency Response Analysis.

Mode Shape

Mode shapes are the result of a normal modes analysis. Mode shapes can be selected as a response. They can be selected as vector components or as absolute measures. They must be assigned to a normal modes subcase.

Linear Buckling Analysis

Buckling Factor

The buckling factor is the result of a buckling analysis, and must be assigned to a buckling subcase (loadstep, load case). A typical buckling constraint is a lower bound of 1.0, indicating that the structure is not to buckle with the given static load. It is recommended to constrain the buckling factor for several of the lower modes, not just of the first mode.

Frequency Response Function (FRF Analysis)

Frequency Response Displacement

Displacements are the result of a frequency response analysis. Nodal displacements, i.e. translational, rotational and normal*, can be selected as a response. They can be selected as vector components in real/imaginary or magnitude/phase form. They must be assigned to a frequency response subcase (loadstep, load case).

*The normal at a grid point is calculated based on the normals of the surrounding elements. The normal frequency response displacement at a grid point can be selected as a response and it is the displacement in the normal’s direction. The normals are also updated when shape changes occur during shape optimization.

Frequency Response Velocity

Velocities are the result of a frequency response analysis. Nodal velocities, i.e. translational, rotational and normal*, can be selected as a response. They can be selected as vector components in real/imaginary or magnitude/phase form. They must be assigned to a frequency response subcase (loadstep, load case).

*The normal at a grid point is calculated based on the normals of the surrounding elements. The normal frequency response velocity at a grid point can be selected as a response and it is the velocity in the normal’s direction. The normals are also updated when shape changes occur during shape optimization.

Frequency Response Acceleration

Accelerations are the result of a frequency response analysis. Nodal accelerations, i.e. translational, rotational and normal*, can be selected as a response. They can be selected as vector components in real/imaginary or magnitude/phase form. They must be assigned to a frequency response subcase (loadstep, load case).

*The normal at a grid point is calculated based on the normals of the surrounding elements. The normal frequency response acceleration at a grid point can be selected as a response and it is the acceleration in the normal’s direction. The normals are also updated when shape changes occur during shape optimization.

Frequency Response Stress

Different stress types can be defined as responses. They are defined for components, properties, or elements. Element stresses are not used in real/imaginary or magnitude/phase form, and constraint screening is applied. The von Mises stress for solids and shells can also be defined as direct responses. It is not possible to define stress constraints in a topology design space. This is a frequency response subcase (loadstep, load case) related response.

Frequency Response Strain

Different strain types can be defined as responses. They are defined for components, properties, or elements. Element strains are used in real/imaginary or magnitude/phase form, and constraint screening is applied. The von Mises strain for solids and shells can also be defined as direct responses. It is not possible to define strain constraints in a topology design space. This is a frequency response subcase (loadstep, load case) related response.

Frequency Response Force

Different force types can be defined as responses. They are defined for components, properties, or elements in real/imaginary or magnitude/phase form. Constraint screening is applied. It is also not possible to define force constraints in a topology design space. This is a frequency response subcase (loadstep, load case) related response.

Random Response Analysis

PSD and RMS Responses

PSD displacement, PSD velocity, PSD acceleration, PSD acoustic pressure, PSD stress, PSD strain, RMS displacement, RMS velocity, RMS acceleration, RMS acoustic pressure, RMS stress and RMS strain responses are available as global as well as subcase-dependent responses (this information is also available in the Subcase Independent responses section above).

Coupled FRF Analysis on a Fluid-structure Model (Acoustic Analysis)

Acoustic Pressure

Acoustic pressures are the result of a coupled frequency response analysis on a fluid-structure model. This response is available for fluid grids. It must be assigned to a coupled frequency response subcase (loadstep, load case) on a fluid-structure model.

Multi-body Dynamics Analysis

Flexible Body Responses

For Multi-body Dynamics problems, the Mass, Center of gravity, and Moment of Inertia of one or more flexible bodies are available as responses. This is in addition to other usual structural responses.

MBD Displacement

MBD displacements are the result of a multi-body dynamics analysis. They must be assigned to a multi-body dynamics subcase (loadstep, load case).

MBD Velocity

MBD velocities are the result of a multi-body dynamics analysis. They must be assigned to a multi-body dynamics subcase (loadstep, load case).

MBD Acceleration

MBD acceleration are the result of a multi-body dynamics analysis. They must be assigned to a multi-body dynamics subcase (loadstep, load case).

MBD Force

MBD forces are the result of a multi-body dynamics analysis. They must be assigned to a multi-body dynamics subcase (loadstep, load case).

MBD Expression

MBD expression responses are the result of a multi-body dynamics analysis. They are the result of the evaluation of an expression. They must be assigned to a multi-body dynamics subcase (loadstep, load case).

Fatigue

Life/Damage

Life and Damage are results of a fatigue analysis. They must be assigned to a Fatigue subcase.

Dynamic/Nonlinear Analysis

Equivalent Plastic Strain

Equivalent plastic strain can be used as an internal response when a nonlinear response optimization is run using the equivalent static load method. This is made possible through the use of an approximated correlation between linear strain and plastic strain, which are calculated in the inner and outer loops respectively, of the ESL method.

ESL Velocity

ESL velocity can be used as an internal response, when a nonlinear response optimization is run, using the equivalent static load method. The RTYPE=ESLV option can be used in conjunction with the velocity component value and a GRID ID specification.

User Responses

Function

A function response is one that uses a mathematical expression to combine design variables, grid point locations, responses, and/or table entries. Whether the function is subcase (loadstep, load case) related or global, is dependent on the response types used in the equation.

External

An external response is one that uses an external user-defined routine to combine design variables, grid point locations, eigenvectors, responses, and/or table entries. Whether the function is subcase (loadstep, load case) related or global is dependent on the response types used in the routine. Refer to External Responses below for more information.

The DRESP3 bulk data entry, in combination with the LOADLIB I/O option entry, allows for the definition of responses through user-defined external functions. The external functions may be written in HyperMath Language (HML), FORTRAN, C or a Microsoft Excel workbook. The resulting libraries and files should be accessible by OptiStruct regardless of the coding language, providing that consistent function prototyping is respected, and adequate compiling and linking options are used.

Writing External Functions

The OptiStruct installation provides "barebone" functions for FORTRAN (dresp3_barebone.F) and for C (dresp3_barebone.c) with proper function definition, arguments, and compilation directives. These files can be used as starting points to write your own functions. Refer to Referencing External Files for information on response definition through a user-defined Microsoft Excel workbook.

HyperMath Language (HML) functions are defined as follows:

integer function myfunct(iparam, rparam, iresp, rresp, userdata)

If sensitivities need to be requested, then the following external function can be used.

integer function myfunct(iparam, rparam, iresp, rresp, dresp, isens

userdata)

FORTRAN functions are defined as follows:

integer function myfunct(iparam, rparam, nparam,

iresp, rresp, nresp,

userdata)

If sensitivities need to be requested, then the following external function can be used.

integer function myfunct(iparam, rparam, nparam,

iresp, rresp, dresp, nresp, isens

userdata)

character*32000 userdata

integer nparam, nresp

integer iparam(nparam), iresp(nresp)

double precision param(nparam), rresp(nresp), dresp(nparam,nresp)

C functions are defined as follows:

int myfunct(int* iparam, double* rparam, int* nparam,

int* iresp, double* rresp, int* nresp,

char* userdata)

If sensitivities need to be requested, then the following external function can be used.

int myfunct(int* iparam, double* rparam, int* nparam,

int* iresp, double* rresp, double* dresp, int* nresp, int*

isens, char* userdata)

Note that the functions' arguments are identical in both languages so as to preserve compatibility. However, since FORTRAN always passes arguments by address, it is important to understand that external C functions receive pointers instead of variables.

In order to ensure portability, the following must be adhered to:

•	Function names should be written using either all lower-case or all upper-case characters

•	Only alphanumeric characters should be used

•	Underscore characters are prohibited

•	Names cannot be longer than eight characters

Regarding implementing of external, user-defined routines using HyperMath, refer to the online documentation for writing scripts in HyperMath. HyperMath is supported on the Windows and Linux operating systems only.

Function Return Values

External functions should return 0 or 1 for successful completion, where 1 indicates that a user-defined information message should be output by OptiStruct. External functions should return -1 in case of fatal error, in which case OptiStruct will terminate after outputting a user-defined error message. See below for more information about error and information messages.

Function Arguments

The following table briefly describes the arguments which are passed from OptiStruct to the external functions.

Argument	Type	Input/Output	Description
iparam	integer (table)	Input	Input parameters types (optional use)
rparam	double (table)	Input	Input parameters values
nparam	integer	Input	Number of parameters
iresp	integer (table)	Input	Output responses requests (optional use)
rresp	double (table)	Output	Output responses values
dresp	double (table)	Output	Output sensitivity values
nresp	integer	Input	Number of responses
isens	integer	Input	Sensitivity output flag
userdata	string	Input/Output	User data/Error or information message

Parameters:

•	nparam is the number of input parameters that were defined on the DRESP3 card.

•	rparam(nparam) contains the values of the input parameters as evaluated by OptiStruct.

•	iparam(nparam) indicates the types of the input parameters as described below.

Parameter values are passed in the exact order in which they were defined on the DRESP3 card, regardless of their type. Using the parameter types table is optional, for instance to perform verifications or code-branching.

The following types are currently supported:

Parameter type	iparam value
DESVAR	1
DTABLE	2
DGRID/DGRIDB	3
DRESP1	4
DRESP2	5
DRESP1L	6
DRESP2L	7
DVPREL1	8
DVPREL2	9
DVMREL1	10
DVMREL2	11
DVCREL1	12
DVCREL2	13
DVMBRL1	14
DVMBRL2	15
DEIGV	16
DGRIDB	18

Responses:

•	nresp is the maximum number of responses which the function is able to compute, as defined on the MAXRESP field of the DRESP3 card.

•	rresp(nresp) returns the values of the responses as evaluated by the external function.

•	iresp(nresp) contains the responses requests as described below.

The responses requests table indicates which of the available responses are actually needed by OptiStruct. Entries in iresp(nresp) are flagged as 1 for requested responses and as 0 otherwise. Using that information is optional, and allows for saving computational effort by not evaluating responses which OptiStruct does not need.

Userdata String

Upon entering the function, the userdata string contains data as defined in the USRDATA field of the DRESP3 card. It provides a convenient mechanism to pass constants or any other relevant information to the function. There are no restrictions regarding the contents of the string, but its length must not exceed 32,000 characters.

Upon exiting the function, the string may contain a user-defined error or information message. The updated string is then returned to OptiStruct, where it is printed to the standard output (.out file and/or screen). Here again, the contents of the string are not restricted as long as its length does not exceed 32,000 characters.

The error or information messages may be formatted by using the character "|" as a line-break indicator. Standard C escape sequences are supported, as well. It is advised, but not necessary, to format messages in such a way that each line does not exceed 80 characters, since the same convention is used in OptiStruct's output files.

Sensitivity Flag

•	isens indicates whether sensitivities are requested in the code. It is recommended to skip the calculation of sensitivities when isens is turned off. This will avoid unnecessary computations.

Building External Libraries

Windows Systems with Microsoft Developer Studio

Creating dynamic libraries under Windows with Microsoft Developer Studio is an extremely easy task. Simply start a new project and select either "FORTRAN Dynamic Link Library" for FORTRAN, or "Win32 Dynamic-Link Library" for C.

For FORTRAN libraries, you need to change the argument passing conventions in the project settings. Under the "FORTRAN" tab, select the category "External Procedures" and then change the "Argument Passing Conventions" to "C, By Reference".

On Windows systems, %PATH% must be set correctly to ensure that the right compiler DLLs are picked up at runtime.

UNIX Systems

Under UNIX, the general syntax to build a shared library starting from a FORTRAN or C file is:

FC [options] -c myfile.F -o myfile.o	(for FORTRAN)
CC [options] -c myfile.c -o myfile.o	(for C)
LD [options] myfile.o -o mylib.so

Where, FC refers to the FORTRAN compiler (for instance f77), CC refers to the C compiler (for instance cc or gcc), and LD refers to the linker (for instance ld) installed on your computer. Refer to your system's manuals for more information.

The compiler and linker options provide information about the platform you are building the library for. The linker options also specify that you are building a shared library. Other options, such as code optimization parameters, are left to your discretion and should not usually affect the compatibility with OptiStruct.

The following table defines options for each of OptiStruct's release platforms, which have been verified to work correctly on various systems. Keep in mind that these options might change depending on the compilers and linker installed on your computer, so refer to your operating system manual for further information. In most cases GNU compilers can be used in place of Intel compilers. Use the appropriate compiler and linker options to create a shared library with the compiler of your choice. The compilers and versions in the following table are the ones used to build OptiStruct.

Platform	FORTRAN Compiler Version	FORTRAN Compiler Options	C Compiler Version	C Compiler Options	Linker Options
Win32	Intel FORTRAN 12.1	/iface:default /libs:dll /threads	Intel C++ 12.1	/MD	/LD
Win64	Intel FORTRAN 12.1	/iface:default /libs:dll /threads	Intel C++ 12.1	/MD	/LD
Macosx64	Intel FORTRAN 10.1.006	-fPIC	Intel C++ 10.1.006	-fPIC	-dynamiclib
Linux64	Intel FORTRAN 12.1	–fPIC	Intel C++ 12.1	-fPIC	-shared

If Compaq Visual Fortran is used to build the external response functions called by DRESP3, the following compiler directive is required to export the functions appropriately:

For a function – “myfunc”

integer function myfunc (iparam, rparam, nparam,

iresp, rresp, dresp, nresp, isens, userdata)

cDEC$ ATTRIBUTES DLLEXPORT, C, REFERENCE :: myfunc

Compiler and linker options for Compaq Visual Fortran, similar to those given in the above table, will be required to build and use multithreaded dynamic runtime libraries.

Once your library is built, you can verify that the functions have been exported correctly by using nm mylib.so on UNIX systems and dumpbin /exports mylib.dll on Windows systems with Microsoft Developer Studio. This command will display the list of symbols found in the library, among which you should recognize the function(s) which you have written.

Note that some FORTRAN compilers convert function names to lower-case or upper-case symbols, and some compilers also append an underscore to these names. However, in your input decks, you do not have to worry about the exact symbol name. Simply use the function name as it is defined in your code, and OptiStruct will automatically locate the appropriate symbol.

Using External Libraries

All files referenced here are located in the HyperWorks installation directory under <install_directory>/demos/os/manual/.

To locate the HyperWorks installation directory, <install_directory>, use the following approach:

From the permanent menu, select the global panel and review the path next to template file: <install_directory> is the portion of the path preceding the templates/ directory on PC, and the hm/ directory on UNIX.

HyperMath Example

Refer to the OptiStruct tutorial, OS-4095 (Size Optimization using External Responses (DRESP3) through HyperMath), for information on using DRESP3 with HyperMath to implement external, user-defined routines.

Simple Example

The files dresp3_simple.F and dresp3_simple.c contain source code for simple examples of external functions written in FORTRAN and C, respectively. Both functions are named mysum and compute two responses – the sum of the parameters and the averaged sum of the parameters.

The input deck dresp3_simple.fem contains an example problem calling both of these external functions. Two LOADLIB cards referring to the FORTRAN and C libraries are defined:

LOADLIB DRESP3 FLIB dresp3_simple_f.dll
LOADLIB DRESP3 CLIB dresp3_simple_c.dll

You have created four DRESP3 cards, which are pointing to the FORTRAN and C functions and requesting the first and second responses in each of those functions. Two DRESP1 responses are used as parameters:

DRESP3 6 SUMF FLIB MYSUM 1 2
+ DRESP1 2 3
DRESP3 7 AVGF FLIB MYSUM 2 2
+ DRESP1 2 3
DRESP3 8 SUMC CLIB MYSUM 1 2
+ DRESP1 2 3
DRESP3 9 AVGC CLIB MYSUM 2 2
+ DRESP1 2 3

For verification purposes, you have also defined two DRESP2 cards that are pointing to two simple equations which evaluate the sum and the averaged sum of their parameters:

DEQATN 1 F(x,y) = x+y
DEQATN 2 F(x,y) = avg(x,y)

DRESP2 4 SUME 1
+ DRESP1 2 3
DRESP2 5 AVGE 2
+ DRESP1 2 3

Running this input deck through OptiStruct shows that the FORTRAN external functions, the C external functions and the internal equations always return the same values, and are updated simultaneously throughout the optimization process.

Advanced Example

The file dresp3_advanced.F contains the FORTRAN source code of the second example, in which you are making use of advanced features of the DRESP3 functionality.

The external function is able to compute the von Mises and maximum principal stresses (strains) of an element based on its stress (strains) components. Either 3 or 6 components can be passed as parameters – 3 components for a shell element and 6 components for a solid element. The following features are used:

•	The USRDATA string is parsed to determine whether stresses or strains are requested, and an error message is returned otherwise.

•	The number of parameters is used to determine whether a shell or solid element is treated, and an error message is returned if that number is not equal to 3 or 6.

•	An error message is returned if the parameters are not of type DRESP1 or DRESP1L, since stress or strain components are expected.

•	Even though the function is able to compute two different responses, only the response(s) actually requested by OptiStruct are computed when the function is called.

•	An information message is returned indicating which responses were evaluated.

The input deck dresp3_advanced.fem gives a simple example of problem making use of this external function, for analysis only.

The DRESP1 responses 10-12 and 13-18 correspond to the stress components of a 2D and a 3D element, respectively. The DRESP1 responses 20-23 evaluate the von Mises stress and the maximum principal stress of the same two elements:

DRESP1 10 SXX2D STRESS ELEM SX1 100
DRESP1 11 SYY2D STRESS ELEM SY1 100
DRESP1 12 SXY2D STRESS ELEM SXY1 100
DRESP1 13 SXX3D STRESS ELEM SXX 50
DRESP1 14 SYY3D STRESS ELEM SYY 50
DRESP1 15 SZZ3D STRESS ELEM SZZ 50
DRESP1 16 SXY3D STRESS ELEM SXY 50
DRESP1 17 SXZ3D STRESS ELEM SXZ 50
DRESP1 18 SYZ3D STRESS ELEM SYZ 50

DRESP1 20 SVM2D-1 STRESS ELEM SVM1 100
DRESP1 21 SMP2D-1 STRESS ELEM SMP1 100
DRESP1 22 SVM3D-1 STRESS ELEM SVM 50
DRESP1 23 SMP3D-1 STRESS ELEM SMP 50

In addition, you have defined DRESP3 cards which compute the same stress results through our external library. You are also using the SLAVE feature to clone the parameters of similar cards:

DRESP3 30 SVM2D-3 STRLIB GETSTR 1 2
+ DRESP1 10 11 12
+ USRDATA STRESS
DRESP3 31 SMP2D-3 STRLIB GETSTR 2 2
+ SLAVE 30
DRESP3 32 SVM3D-3 STRLIB GETSTR 1 2
+ DRESP1 13 14 15 16 17 18
+ USRDATA STRESS
DRESP3 33 SMP3D-3 STRLIB GETSTR 2 2
+ SLAVE 32

Referencing External Files

Microsoft Excel workbooks can be referenced via the LOADLIB entry to define user-defined responses. Both Implicit and Explicit options are available and are defined as follows:

Implicit definition

This is a simple implementation wherein two columns in an Excel worksheet are used to define the input and output parameters. Column 1 can be used to list input parameters and Column 2 can be used to list output parameters.

LOADLIB DRESP3 ELIB dresp3_excel.xlsx

DRESP3 10 SUM ELIB MYSUM

+ DRESP1 5 6

response_implicit

Explicit definition

In this advanced implementation, the cell input number is specified. Cells for input and output data are listed.

LOADLIB DRESP3 ELIB dresp3_excel.xlsx

DRESP3 20 FUNC ELIB MYFUNC

+ DRESP1 5 6 7 8

+ DESVAR 1

+ CELLIN B3 through B6

+ CELLIN C10

+ CELLOUT E10

response_explicit