01. Function Description and Limitation 02. Fortran File Preparation 03. DLL File Preparation 04. Using the USSR material model in midas FEA

Transcription

1 midas FEA User Supplied Subroutine User Manual 01. Function Description and Limitation 02. Fortran File Preparation 03. DLL File Preparation 04. Using the USSR material model in midas FEA MIDAS Information Technology Co. Ltd, Copyrights SINCE 1989 All rights reserved

2 01. Function Description and Limitation The user supplied material function allows users to customize their own material nonlinear model in conjunction with existing Pre/Post processing features in midas FEA. Nonlinear elastic material and Nonlinear elasto-plastic material can be defined in the user supplied material function, and support elements that are Plane strain (3, 4, 6, 8 node element), Axisymmetric (3, 4, 6, 8 node element) and Solid (4, 6, 8, 10, 15, 20 node element). Stress components for each element type are defined as follows. Table 1. Stress component of element Element Stress Strain Truss σ xx ε xx Axisymmetirc σ xx, σ yy, σ xy, σ zz ε xx, ε yy, γ xy, ε zz Plane strain σ xx, σ yy, σ xy, σ zz ε xx, ε yy, γ xy, 0 Plane stress σ xx, σ yy, σ xy, 0 ε xx, ε yy, γ xy, ε zz Solid σ xx σ yy, σ zz, σ xy, σ yz, σ zx ε xx, ε yy, ε zz, γ xy, γ yz, γ, zx Requirements for midas FEA user supplied material function are listed below: - Preparing a FORTRAN File - Compiling and making a DLL File - Using the user supplied material model in midas FEA. 1

3 02. Fortran File Preparation User supplied material functions either can be created using a Fortran 77 or Fortran 90 programming language; however, since midas FEA solver uses Fortran 90, users are encouraged to follow the same language. In order for midas FEA solver to recognize Fortran files, the programming code, which is provided below, is required at the beginning of the user supplied material program.!***************************************************************************! USER SUPPLIED MATERIAL SUBROUTINE!*************************************************************************** SUBROUTINE USRMAT(EPS0, DEPS, EPSP, NS, INFM_STEP, COORD, SE, USRVAL, NUV, USRSTA, NUS, IUSRIND, NUI, SIG, STIFF,ID, DETJ, DTIME) IMPLICIT NONE &!DEC$ ATTRIBUTES DLLEXPORT::USRMAT INTEGER, INTENT(IN) :: NS! NUMBER OF STRESS COMPONENT INTEGER, INTENT(IN) :: INFM_STEP(5)! STEP INFORMATION FOR STAGE, INCREMENT, ITERATION, ELEMENT, INTEGRATION POINT! INFM_STEP(1) : STAGE ID! INFM_STEP(2) : LOAD INCREMENTAL STEP ID! INFM_STEP(3) : ITERATION STEP ID! INFM_STEP(4) : ELEMENT ID! INFM_STEP(5) : INTEGRATION POINT ID INTEGER, INTENT(IN) :: ID! MATERIAL ID OF CURRENT ELEMENT INTEGER, INTENT(IN) :: NUV! NUMBER OF PARAMETERS INTEGER, INTENT(IN) :: NUS! NUMBER OF INTERNAL STATE VARIABLES INTEGER, INTENT(IN) :: NUI! NUMBER OF INTEGER INDICATOR VARIABLES REAL*8, INTENT(IN) :: DETJ! DETERMINENT VALUE AT CURRENT INTEGRATION POINT REAL*8, INTENT(IN) :: DTIME! TIME INCREMENT AT CURRENT STAGE REAL*8, INTENT(IN) :: EPS0(NS)! TOTAL STRAIN AT PREVIOUS STEP REAL*8, INTENT(IN) :: DEPS(NS)! INCREMENTAL STRAIN REAL*8, INTENT(IN) :: COORD(3)! COORDINATE OF INTEGRATION POINT REAL*8, INTENT(IN) :: SE(NS, NS)! ELASTIC CONSTITUTIVE MATRIX REAL*8, INTENT(INOUT) :: SIG(NS)! TOTAL STRESS AT PREVIOUS(IN) & CURRENT(OUT) STEP REAL*8, INTENT(INOUT) :: STIFF(NS, NS)! TANGENT STIFFNESS AT CURRENT STEP (OUT) REAL*8, INTENT(INOUT) :: EPSP(NS)! TOTAL PLASTIC STRAIN AT PREVIOUS STEP REAL*8, INTENT(INOUT) :: USRSTA(NUS)! INTERNAL STATE VARIABLES REAL*8, INTENT(IN) :: USRVAL(NUV)! PARAMETERS INTEGER, INTENT(INOUT) :: IUSRIND(NUI)! INTEGER INDICATOR VARIABLES User Supplied Subroutine RETURN END SUBROUTINE USRMAT!*************************************************************************** NS : Number of stress component. INFM_STEP : Step Information INFM_STEP(1) : Current stage number INFM_STEP(2) : Current load increment step INFM_STEP(3) : Current iteration number INFM_STEP(4) : Current element number INFM_STEP(5) : Current integration point number ID NUV : Material ID of current element. : Number of parameters. 2

4 NUS NUI EPS0 DEPS COORD SE SIG STIFF EPSP USRSTA USRVAL IUSRIND DETJ DTIME : Number of internal state valuables. : Number of integer indicator valuables. : Total strain of previous step. : Incremental strain. : Coordinate of integration point. : Elastic constitutive matrix. : Total stress of previous step. : Tangent stiffness of current step. : Total plastic strain of previous step. : Internal state variables. : User defined parameters. : Integer indicator valuables. : Determinant of Jacobian matrix at current integration point. : Time increment at current stage.( only used in construction stage analysis) The following three examples: linear elastic material model for 3D solid elements; simple nonlinear elastic constitutive model for 2D plane strain elements; and the final example shows how to define two different nonlinear elastic material models for 3D solid elements. [EXAMPLE 1] Linear elastic constitutive model for 3D solid element:!***************************************************************************! USER SUPPLIED MATERIAL SUBROUTINE!*************************************************************************** SUBROUTINE USRMAT( EPS0, DEPS, EPSP, NS, INFM_STEP, COORD, SE, USRVAL, NUV, USRSTA, NUS, IUSRIND, NUI, SIG, STIFF,ID, DETJ, DTIME) & IMPLICIT NONE!DEC$ ATTRIBUTES DLLEXPORT::USRMAT INTEGER, INTENT(IN) :: NS! NUMBER OF STRESS COMPONENT INTEGER, INTENT(IN) :: INFM_STEP(5)! STEP INFORMATION FOR STAGE, INCREMENT, ITERATION,! ELEMENT, INTEGRATION POINT! INFM_STEP(1) : STAGE ID! INFM_STEP(2) : LOAD INCREMENTAL STEP ID! INFM_STEP(3) : ITERATION STEP ID! INFM_STEP(4) : ELEMENT ID! INFM_STEP(5) : INTEGRATION POINT ID INTEGER, INTENT(IN) :: ID! MATERIAL ID OF CURRENT ELEMENT INTEGER, INTENT(IN) :: NUV! NUMBER OF PARAMETERS INTEGER, INTENT(IN) :: NUS! NUMBER OF INTERNAL STATE VARIABLES INTEGER, INTENT(IN) :: NUI! NUMBER OF INTEGER INDICATOR VARIABLES REAL*8, INTENT(IN) :: DETJ! DETERMINENT VALUE AT CURRENT INTEGRATION POINT REAL*8, INTENT(IN) :: DTIME! TIME INCREMENT AT CURRENT STAGE REAL*8, INTENT(IN) :: EPS0(NS)! TOTAL STRAIN AT PREVIOUS STEP REAL*8, INTENT(IN) :: DEPS(NS)! INCREMENTAL STRAIN REAL*8, INTENT(IN) :: COORD(3)! COORDINATE OF INTEGRATION POINT REAL*8, INTENT(IN) :: SE(NS, NS)! ELASTIC CONSTITUTIVE MATRIX REAL*8, INTENT(INOUT) :: SIG(NS)! TOTAL STRESS AT PREVIOUS(IN) & CURRENT(OUT) STEP REAL*8, INTENT(INOUT) :: STIFF(NS, NS)! TANGENT STIFFNESS AT CURRENT STEP (OUT) REAL*8, INTENT(INOUT) :: EPSP(NS)! TOTAL PLASTIC STRAIN AT PREVIOUS STEP REAL*8, INTENT(INOUT) :: USRSTA(NUS)! INTERNAL STATE VARIABLES REAL*8, INTENT(IN) :: USRVAL(NUV)! PARAMETERS INTEGER, INTENT(INOUT) :: IUSRIND(NUI)! INTEGER INDICATOR VARIABLES 3

5 INTEGER :: I, J REAL*8 :: TEMP REAL*8, ALLOCATABLE :: DSIG(:) IF(ALLOCATED(DSIG)) DEALLOCATE(DSIG) ALLOCATE(DSIG(NS)) DO I = 1, NS TEMP = 0.D0 DO J = 1, NS TEMP = TEMP + SE(I, J) * DEPS(J) STIFF(I, J) = SE(I, J) ENDDO DSIG(I) = TEMP SIG(I) = SIG(I) + DSIG(I) ENDDO RETURN END!*************************************************************************** [EXAMPLE 2] Simple nonlinear elastic constitutive model for 2D plane strain element!***************************************************************************! USER SUPPLIED MATERIAL SUBROUTINE!*************************************************************************** SUBROUTINE USRMAT( EPS0, DEPS, EPSP, NS, INFM_STEP, COORD, SE, USRVAL, NUV, USRSTA, NUS, IUSRIND, NUI, SIG, STIFF,ID, DETJ, DTIME) & IMPLICIT NONE!DEC$ ATTRIBUTES DLLEXPORT::USRMAT INTEGER, INTENT(IN) :: NS! NUMBER OF STRESS COMPONENT INTEGER, INTENT(IN) :: INFM_STEP(5)! STEP INFORMATION FOR STAGE, INCREMENT, ITERATION, ELEMENT, INTEGRATION POINT! INFM_STEP(1) : STAGE ID! INFM_STEP(2) : LOAD INCREMENTAL STEP ID! INFM_STEP(3) : ITERATION STEP ID! INFM_STEP(4) : ELEMENT ID! INFM_STEP(5) : INTEGRATION POINT ID INTEGER, INTENT(IN) :: ID! MATERIAL ID OF CURRENT ELEMENT INTEGER, INTENT(IN) :: NUV! NUMBER OF PARAMETERS INTEGER, INTENT(IN) :: NUS! NUMBER OF INTERNAL STATE VARIABLES INTEGER, INTENT(IN) :: NUI! NUMBER OF INTEGER INDICATOR VARIABLES REAL*8, INTENT(IN) :: DETJ! DETERMINENT VALUE AT CURRENT INTEGRATION POINT REAL*8, INTENT(IN) :: DTIME! TIME INCREMENT AT CURRENT STAGE REAL*8, INTENT(IN) :: EPS0(NS)! TOTAL STRAIN AT PREVIOUS STEP REAL*8, INTENT(IN) :: DEPS(NS)! INCREMENTAL STRAIN REAL*8, INTENT(IN) :: COORD(3)! COORDINATE OF INTEGRATION POINT REAL*8, INTENT(IN) :: SE(NS, NS)! ELASTIC CONSTITUTIVE MATRIX REAL*8, INTENT(INOUT) :: SIG(NS)! TOTAL STRESS AT PREVIOUS(IN) & CURRENT(OUT) STEP REAL*8, INTENT(INOUT) :: STIFF(NS, NS)! TANGENT STIFFNESS AT CURRENT STEP (OUT) REAL*8, INTENT(INOUT) :: EPSP(NS)! TOTAL PLASTIC STRAIN AT PREVIOUS STEP REAL*8, INTENT(INOUT) :: USRSTA(NUS)! INTERNAL STATE VARIABLES REAL*8, INTENT(IN) :: USRVAL(NUV)! PARAMETERS INTEGER, INTENT(INOUT) :: IUSRIND(NUI)! INTEGER INDICATOR VARIABLES 4

6 INTEGER :: I, J REAL*8 :: EMOD REAL*8, ALLOCATABLE :: EPS(:) IF(ALLOCATED(EPS)) DEALLOCATE(EPS) ALLOCATE(EPS(NS)) EMOD = USRVAL(1) EPS(1:NS) = EPS0(1:NS) + DEPS(1:NS)! ! TOTAL STRESS! SIG(1) = EMOD * EPS(1) D0 * EMOD * EPS(1)**2 SIG(2) = EMOD * EPS(2) D0 * EMOD * EPS(2)**2 SIG(4) = EMOD * EPS(4) D0 * EMOD * EPS(4)**2 SIG(3) = (EMOD * EPS(3)) / 2.D0! ! MATERIAL STIFFNESS MATRIX! STIFF(1,1) = EMOD D0 * EMOD * EPS(1) STIFF(2,2) = EMOD D0 * EMOD * EPS(2) STIFF(4,4) = EMOD D0 * EMOD * EPS(4) STIFF(3,3) = 0.5D0 * EMOD RETURN END!*************************************************************************** [EXAMPLE 3] defines two different nonlinear elastic material models for 3D solid elements. It makes use of variable ID, which helps easily define multiple material models simultaneously.!***************************************************************************! USER SUPPLIED MATERIAL SUBROUTINE!*************************************************************************** SUBROUTINE USRMAT( EPS0, DEPS, EPSP, NS, INFM_STEP, COORD, SE, USRVAL, NUV, USRSTA, NUS, IUSRIND, NUI, SIG, STIFF,ID, DETJ, DTIME) & IMPLICIT NONE!DEC$ ATTRIBUTES DLLEXPORT::USRMAT INTEGER, INTENT(IN) :: NS! NUMBER OF STRESS COMPONENT INTEGER, INTENT(IN) :: INFM_STEP(5)! STEP INFORMATION FOR STAGE, INCREMENT, ITERATION, ELEMENT, INTEGRATION POINT! INFM_STEP(1) : STAGE ID! INFM_STEP(2) : LOAD INCREMENTAL STEP ID! INFM_STEP(3) : ITERATION STEP ID! INFM_STEP(4) : ELEMENT ID! INFM_STEP(5) : INTEGRATION POINT ID INTEGER, INTENT(IN) :: ID! MATERIAL ID OF CURRENT ELEMENT INTEGER, INTENT(IN) :: NUV! NUMBER OF PARAMETERS 5

7 INTEGER, INTENT(IN) :: NUS! NUMBER OF INTERNAL STATE VARIABLES INTEGER, INTENT(IN) :: NUI! NUMBER OF INTEGER INDICATOR VARIABLES REAL*8, INTENT(IN) :: DETJ! DETERMINENT VALUE AT CURRENT INTEGRATION POINT REAL*8, INTENT(IN) :: DTIME! TIME INCREMENT AT CURRENT STAGE REAL*8, INTENT(IN) :: EPS0(NS)! TOTAL STRAIN AT PREVIOUS STEP REAL*8, INTENT(IN) :: DEPS(NS)! INCREMENTAL STRAIN REAL*8, INTENT(IN) :: COORD(3)! COORDINATE OF INTEGRATION POINT REAL*8, INTENT(IN) :: SE(NS, NS)! ELASTIC CONSTITUTIVE MATRIX REAL*8, INTENT(INOUT) :: SIG(NS)! TOTAL STRESS AT PREVIOUS(IN) & CURRENT(OUT) STEP REAL*8, INTENT(INOUT) :: STIFF(NS, NS)! TANGENT STIFFNESS AT CURRENT STEP (OUT) REAL*8, INTENT(INOUT) :: EPSP(NS)! TOTAL PLASTIC STRAIN AT PREVIOUS STEP REAL*8, INTENT(INOUT) :: USRSTA(NUS)! INTERNAL STATE VARIABLES REAL*8, INTENT(IN) :: USRVAL(NUV)! PARAMETERS INTEGER, INTENT(INOUT) :: IUSRIND(NUI)! INTEGER INDICATOR VARIABLES INTEGER :: I, J REAL*8 :: EMOD REAL*8, ALLOCATABLE :: EPS(:) IF(ALLOCATED(EPS)) DEALLOCATE(EPS) ALLOCATE(EPS(NS)) IF(ID == 1)THEN SIG(1:NS) = 0.D0 EMOD = USRVAL(1) EPS(1:NS) = EPS0(1:NS) + DEPS(1:NS)! ! TOTAL STRESS! SIG(1) = EMOD * EPS(1) D0 * EMOD * EPS(1)**2 SIG(2) = EMOD * EPS(2) D0 * EMOD * EPS(2)**2 SIG(3) = EMOD * EPS(3) D0 * EMOD * EPS(3)**2 SIG(4) = (EMOD * EPS(4)) / 2.D0 SIG(5) = (EMOD * EPS(5)) / 2.D0 SIG(6) = (EMOD * EPS(6)) / 2.D0! ! MATERIAL STIFFNESS MATRIX! STIFF(1,1) = EMOD D0 * EMOD * EPS(1) STIFF(2,2) = EMOD D0 * EMOD * EPS(2) STIFF(3,3) = EMOD D0 * EMOD * EPS(3) STIFF(4,4) = 0.5D0 * EMOD STIFF(5,5) = 0.5D0 * EMOD STIFF(6,6) = 0.5D0 * EMOD ELSEIF(ID == 2) THEN SIG(1:NS) = 0.D0 EMOD = USRVAL(1) EPS(1:NS) = EPS0(1:NS) + DEPS(1:NS)! ! TOTAL STRESS! SIG(1) = EMOD * EPS(1) D0 * EMOD * EPS(1)**2 6

8 SIG(2) = EMOD * EPS(2) D0 * EMOD * EPS(2)**2 SIG(3) = EMOD * EPS(3) D0 * EMOD * EPS(3)**2 SIG(4) = (EMOD * EPS(4)) / 2.D0 SIG(5) = (EMOD * EPS(5)) / 2.D0 SIG(6) = (EMOD * EPS(6)) / 2.D0! ! MATERIAL STIFFNESS MATRIX! STIFF(1,1) = EMOD D0 * EMOD * EPS(1) STIFF(2,2) = EMOD D0 * EMOD * EPS(2) STIFF(3,3) = EMOD D0 * EMOD * EPS(3) STIFF(4,4) = 0.5D0 * EMOD STIFF(5,5) = 0.5D0 * EMOD STIFF(6,6) = 0.5D0 * EMOD ENDIF RETURN END!*************************************************************************** Note: Internal subroutine or internal function variables used in the user supplied material subroutine must begin with XX to avoid conflict with midas FEA solver subroutine variables. 7

9 03. DLL File Preparation Adding user supplied material model in midas FEA can be created by a DLL (Dynamic Link Library) material model file using Compaq Visual Fortran 6.6 or an Intel Fortran 8.0 compiler. 3.1 Compaq 6.6 This section explains how to create a DLL file using Compaq Visual Fortran 6.6. Figure 1 shows an example interface of Compaq Visual Fortran 6.6. Figure 1. Initial window of Compaq Fortran 6.6 8

10 Procedure: 1) First click on File > New from the menu bar. (see Figure 2) 2) Click on [Projects] tab 3) Select Fortran Dynamic Link Library. Project name must use USERMAT. 4) Click OK Figure 2. New window 5) Select An empty DLL application and click Finish (see Figure 3). Figure 3. Fortran Dynamic Link Library Step 1 of 1 window 9

11 6) Click OK in New Project Information to create a new project, see Figure 4. Figure 4. New Project Information 7) Click FileView at the bottom of the workspace (Figure 5). 8) Select Project > Add to Project > Files. Figure 5. Add Files to Project 9) Select previously made Fortran file (Figure 6). 10

12 Figure 6. Insert Files into Project window 10) Click on OK button. 11) Verify that the Fortran file appears in the project (Figure 7). Figure 7. Workspace 11

13 12) Select Win32 Release in Configuration window (Figure 8) 13) Click [Build\Build FILENAME.dll] menu (Figure 9). Figure 8. Selection of Win32 Release Figure 9. Build 14) DLL file created successfully should print out the following information in the message (Figure 10). Figure 10. Message window 12

14 15) Verify the path of the DLL file, select [Project\Settings ]. 16) Open Project Settings window. 17) Select Link tab, see the Output file name input window. Where Release/ is the name of the of the Project folder. Figure 11. Project Settings window 13

15 3.2 Intel Fortran 9.0 Creating DLL file using Intel Fortran 9.0. Figure 12. Intel Fortran 9.0 Initial execution screen 1) Execute.Net based Intel Fortran 9.0. The window as shown in Figure 12 should be activated. 2) Select File > New > Project (Figure 13). Figure 13. Selection of project menu 14

16 3) A new project window is opened. (Figure 14) Figure 14. Input window of new project 4) For Intel (R) Fortran Projects, select the Dynamic-Link Library icon from New Project Template window. 5) Enter the name USRMAT. 6) Enter the path destination or use the Browse button. 7) Verify correct path destination is displayed in [Project will be created at] 8) Click on [OK]. 9) Confirmation window Figure 15 will be displayed. 10) Click [Finish]. Figure 15. Confirmation window of creating a project 15

17 After completing the following the steps, users can verify if USRMAT has been created by using the solution explorer displayed on the right side of the page. Intel Fortran 9.0 can verify that USRMAT.f90 has been automatically created. Note, this feature cannot be done in Compaq Fortran 6.6. If users double click on USRMAT.f90 then users can verify whether the subroutine has been created automatically as shown in Figure 17. Figure 16. Initial window for creating a project The following example explains how to create a DLL file with a simple nonlinear elastic model. 1) Enter the argument for the name to be defined on the subroutine (Figure 18). 2) Input! Variables and! Body of USRMAT according to Figure 19 and 20. 3) Input the Function as shown in Figure 21 after End subroutine USRMAT. Then all the coding required for this example and for a basic example ends. 16

18 Figure Initial construction of subroutine Figure 18. Argument input code Figure 19. Variable input code 17

19 Figure 20. Execution part input code Figure 21. Function input code 3.2 Compaq Visual Fortran 6.6 The following explains how to create a DLL file using Compaq Visual Fortran 6.6. midas solver requires the DLL files be compiled under a Compaq Visual Fortran 6.6 Compiler, As shown in Figure 22, if users select Project > USRMAT Properties option then the Project Property Window appears as shown in Figure 23. To select the default calling convention for an application, the steps are as follow: 1) Select External Procedures from the Fortran Menu at the Component Property Menu. 2) Calling Convention is set to default. 3) Change Calling Convention to CVF (Compaq Visual Fortran) 4) Click OK. 18

20 Figure 22. Project property menu Figure 23. Project property page As shown in Figure 24, select Release from [Select active configuration window] which is at the top part of Intel Fortran window. As shown in Figure 25, Build > Solution Build function will start building a solution. If the [Output] appears as Figure 26, then build is completed. If there is no extra setting for the created DLL file, then USRMAT.dll will be created in a subfolder called Release of the project. 19

21 Figure 24. Select active configuration window Figure 25. Solution build Figure 26. Output message. 20

22 04. Using the user-defined material model in midas FEA The Create/Modify Material dialog box contains constitutive models in midas FEA Solver as shown in Figure 27. By selecting the constitutive model as User-Supplied material, the Parameters subsequently are enabled: Number of Parameters (NUV), Number of Internal State Variables (NUS), and Number of Indicator Variables. This section provides a description about the parameters and required procedures. Figure 27. Create/Modify Material dialog box Elastic Modulus, Poisson s Ratio and Shear Modulus: This is used for Linear Elastic Constitutive matrix. Therefore this should be entered as an initial value for nonlinear analysis. Weight density can be set to any arbitrary value. Expansion Coefficient cannot be applied. Seepage Parameters and Drainage Parameters cannot be applied while using user supplied material function. 21

23 1. User Supplied Material Library File By clicking on, as shown in Figure 27, users can select existing DLL files from a library. Figure 28. DLL file open window 2. Number of Parameters (NUV) NUV indicates the number of parameters which are user-defined constant coefficients. By clicking on the adjacent icon 2, as shown in Figure 27, the USRVAL can be viewed. Generally this includes the coefficients defining the Constitutive model, for instance, if Mohr-Coulomb model were used, then coefficients such as Cohesion and Friction angle will be displayed. Parameters can only be defined in the Add/Modify User-defined value. Parameters cannot be defined in a FORTRAN code. If is selected, as shown in Figure 27, then the parameters can be entered by following the procedure outlined below: Procedure: 1) Input the coefficients into the corresponding row Figure 29. 2) Click Enter Key after inputting each value. *Note: If users do not press the Enter Key then the value will be set to 0. Users can input up to data parameters. Figure 29. User-defined values input window 22

24 3. Number of Internal State Variables (NUS) Number of Internal State Variables NUS is a value for each step in the inelastic routine for example plastic strain. Unlike NUV, NUS can be modified in a FORTRAN routine. If selected, as shown in Figure 30, then the parameters can be entered by following the procedure outlined below: Procedure: 1) Input the coefficients for each corresponding row Figure 30. 2) Click Enter Key after inputting each value. Note: If users do not press the Enter Key then the value will be considered as 0. Users can input up to data parameters. Figure 30. Internal State Variables input window 4. Number of Integer Indicator Valuables (NUI) Internal Integer variables indicates the divergence term or number of iterations. Unlike the NUV, NUI can be modified in a FORTRAN routine. If is selected, as shown in Figure 27, then the parameters can be entered by following the procedure outlined below: Procedure: 1) Input the Integer Indicator Variable for each corresponding row Figure 31. 2) Press Enter Key after entering each value. Note: If users do not press the Enter Key then the value will be set to 0. Users can input up to data parameters. Figure 31. User-defined Integer Indicator Variable input window 23