ML22356A140

Caice Users Manual v21 Final Tlr 2022-Post Qte Clean

ML22356A140
Person / Time
Issue date:	12/21/2022
From:	Jing Y, Huan Li, Madhumita Sircar, Xi Y NRC/RES/DE/SGSEB, Univ of Colorado
To:
Shared Package
ML22356A138:ml22356A138	List: ML22356A140
References
Download: ML22356A140 (1)

Text

Users Manuals for Coupled Analysis of Irradiated ConcretE (CAICE)

Manuscript Completed: December 4, 2022 Date Published: December 21, 2022 Prepared by:

Yunping Xi Yuxiang Jing Department of Civil, Environmental and Architectural Engineering University of Colorado Boulder, CO 80309-0428 Madhumita Sircar, NRC Technical Lead and Project Manager Huan Li, NRC Structural Engineer Technical Letter Report Office of Nuclear Regulatory Research

Disclaimer This report was prepared as an account of work sponsored by an agency of the U.S.

Government. Neither the U.S. Government nor any agency thereof, nor any employee, makes any warranty, expressed or implied, or assumes any legal liability or responsibility for any third party's use, or the results of such use, of any information, apparatus, product, or process disclosed in this publication, or represents that its use by such third party complies with applicable law.

This report does not contain or imply legally binding requirements. Nor does this report establish or modify any regulatory guidance or positions of the U.S. Nuclear Regulatory Commission and is not binding on the Commission.

2

Table of Contents 1 Introduction ........................................................................................................ 5 2 The Users Manual for the Multiscale and Multiphase Model for Concrete .. 6 2.1 Introduction............................................................................................................................ 6 2.1.1 Features and Capabilities ........................................................................................... 6 2.1.2 Structure of the Codes................................................................................................. 6 2.2 Getting Started...................................................................................................................... 9 2.3 Inputs...................................................................................................................................... 9 2.4 Executing the Program ...................................................................................................... 10 2.5 Results and Visualization .................................................................................................. 11 3 The Users Manual for Radiation Transport Modeling.................................. 12 3.1 Introduction.......................................................................................................................... 12 3.1.1 Features and Capabilities ......................................................................................... 12 3.1.2 Structure of the Codes............................................................................................... 12 3.2 Getting Started.................................................................................................................... 13 3.3 Executing the Program ...................................................................................................... 14 3.4 Inputs.................................................................................................................................... 14 3.5 Results and Visualization .................................................................................................. 15 4 The Users Manual for Coupled Damage-Creep Modeling ........................... 17 4.1 Introduction.......................................................................................................................... 17 4.1.1 Features and Capabilities ......................................................................................... 17 4.1.2 Structure of the Codes............................................................................................... 17 4.2 Getting Started.................................................................................................................... 27 4.3 Inputs.................................................................................................................................... 28 4.4 Executing the Program ...................................................................................................... 29 4.5 Results and Visualization .................................................................................................. 29 Appendix ................................................................................................................. 30 A.1 Demonstrations ....................................................................................................................... 30 A.1.1 Validation of the Composite Model ............................................................................... 30 A.1.2 Parametric Analyses of the Composite Model Input Parameters............................. 31 A.1.3 Radiation Transport Modeling for a Simplified Example ............................................ 32 A.1.4 Analysis of an Example Using the Coupled Damage-Creep Model......................... 34 A.1.5 A Comprehensive Case Study: A Coupled Radio-Thermo-Mechanical Analysis for a Section of a Concrete Biological Shielding Wall in a Nuclear Power Plant ................... 39 A.2 Warnings and Limitations....................................................................................................... 43 3

A.3 Units .......................................................................................................................................... 43 A.4 Program Diagram .................................................................................................................... 43 4

1 Introduction As documented in the U.S. Nuclear Regulatory Commissions (NRCs) Research Information Letter (RIL) 2021-07, Radiation Effects on ConcreteAn Approach for Modeling Degradation of Concrete Properties, issued August 2021 (Agencywide Documents Access and Management System Accession No. ML21238A064), theoretical and numerical models, called Coupled Analysis of Irradiated ConcretE (CAICE), were developed to predict the long-term performance of mechanical and transport responses of concrete structures used in nuclear power plants. The CAICE models were implemented using MATLAB and ABAQUS through a custom subroutine. The codes use the finite element and finite difference computational methods. The results of the completed project represent a computational framework consisting of a combination of user-defined materials models (in-house code) and available commercial finite element software such as ABAQUS.

The CAICE models were initially implemented for research purposes. The objective of this new project is to make the CAICE computer codes and framework user-friendly, paving the way for future applications and developments. Therefore, this project focuses on knowledge transfer and the development of detailed documentation to make the CAICE program more accessible to the NRC staff. The developers added comments to all the written codes, delineated their structure and sequence, developed an extensive users manual, built detailed structural models for demonstration purposes, established training sessions, and developed some of the relevant documentation that will be necessary for the NRC staff to fully understand and use the CAICE computer codes in future applications.

This report includes three users manuals. Chapter 2 is the users manual for the multiscale and multiphase model for concrete. Chapter 3 is the users manual for radiation transport modeling. Chapter 4 is the users manual for coupled damage-creep modeling. The appendix includes necessary examples for demonstration purposes.

5

2 The Users Manual for the Multiscale and Multiphase Model for Concrete 2.1 Introduction The multiscale and multiphase model for concrete (the composite model) was implemented using MATLAB. RIL 2021-07 chapter 2, Multiscale and Multiphase Model for Concrete, gives the theories involved in this part of the CAICE codes. To help potential users better understand and use the codes for future applications and developments, this users manual contains an overview for this part of the codes, including capabilities and program flow, defining the problem, obtaining inputs, how to run the codes, and how to obtain the results.

Appendix sections A.1.1 and A.1.2 include two examples for demonstration purposes.

Appendix section A.2 lists the limitations of the program.

2.1.1 Features and Capabilities In the program developed in MATLAB, the internal structure of concrete was modeled at four different scale levels with different constituent phases using the Mori-Tanaka model and the generalized self-consistent (GSC) model. The overall stiffness (elastic modulus) and strain of the concrete can be calculated based on the properties and behavior of the constituent phases at the scale levels. The damage to concrete due to irradiation was estimated using a composite damage mechanics model. The developed program can be applied to various concrete materials with different mix designs used in different nuclear power plants to estimate the reduction of the modulus of elasticity and deformation of and damage to nuclear-irradiated concrete.

2.1.2 Structure of the Codes This part of the program is in the Composite model folder, which contains the series of files listed in Table 2-1. Table 2-1 also lists their types and descriptions. The Composite model folder contains a subfolder called MK, which stands for the Mori-Tanaka model. Readers interested in the background theories in the composite model may refer to the RIL 2021-07 section numbers given in table 2-1.

6

Table 2-1 Program Files in the Composite model Folder File name Type Description Folder The main script for the theoretical modeling of neutron irradiated concrete Composite Main.m script (see RIL 2021-07 sections 2.1, 2.2.2, and model 2.5 and appendix sections A.3 and A.4)

Calculation of the strain of cement paste Composite cp.m function (see RIL 2021-07 section 2.3.2 and model appendix section A.2)

Calculation of Youngs modulus based on Composite elastic_modulus.m function Hookes Law model Radiation-induced deformation of different Composite irradiation.m function constituent phases (see RIL 2021-07 model section 2.5.1)

Modification of the Bogue calculation (to determine the approximate proportions of Composite MBC.m function the four main minerals in Portland cement model clinker)

Calculation of the bulk and shear modulus based on the GSC model (see Composite modulus.m function RIL 2021-07 section 2.2.1 and appendix model section A.1)

Calculation of the bulk and shear modulus Composite modulus_convert.m function based on Hookes Law model Calculation of the shear modulus based Composite shear_modulus.m function on Hookes Law model Calculation of strain based on the GSC Composite strain.m function model (see RIL 2021-07 section 2.2.1 and model appendix section A.1)

Thermal expansion of different constituent Composite Thermal.m function phases (see RIL 2021-07 section 2.5.1.3) model The main function file for the Mori-Tanaka Model.m function model of cement paste (see RIL 2021-07 MK section 2.3) deter.m function Calculation of the determinant of a matrix MK Dimq.m function Writing order 4 tensor MK Determination of the stiffness matrix Elas.m function MK based on Hookes Law 7

File name Type Description Folder The general method for determining the Eshelby.m function MK Eshelby tensor Determination of the Eshelby tensor for an Eshelcy.m function MK infinite elliptic cylinder Determination of the Eshelby tensor for an Eshobsp.m function MK oblate spheroid Determination of the Eshelby tensor for a Eshpesh.m function MK penny shape Determination of the Eshelby tensor for a Eshprsp.m function MK prolate spheroid Determination of the Eshelby tensor for a Eshsph.m function MK spherical shape Euler.m function Conversion of Euler coordinates MK Determination of the inverse of a 3*3 inverse.m function MK matrix legendre_dd.m function 2D Gauss Legendre integration MK lengfdre_ud.m function 1D Gauss Legendre integration MK Modification of the Bogue calculation (to determine the approximate proportions of MBC.m function MK the four main minerals in Portland cement clinker)

Calculation of a modified Eshelby Modeshqu.m function inclusion tensor for an ellipsoidal inclusion MK with a slightly weakened interface Function to sort the axis values of the Sort.m function different phases and determine the MK associated Eshelby tensor Determination of the volume fractions of constituents in cement paste and concrete Vol.m function MK (see RIL 2021-07 section 2.4 and appendix section A.2)

Volume fractions and properties of the Volc.m function MK clinker (see RIL 2021-07 section 2.3.3)

Volume fractions and properties of the Voli.m function intermediate inclusion MK Note: 1D: one-dimensional; 2D: two-dimensional 8

2.2 Getting Started Users should have a release of MATLAB installed on their computers and a working knowledge of the program, including but not limited to matrices/arrays and their operations, array indexing, workspace variables, statements, programming scripts and functions, debugging, and plotting functions. Users can refer to the documentation for their version of MATLAB to better understand the programming.

Users set up their models by creating and modifying the necessary m files used by this program. The files contain information about the problem to be solved, such as the following:

• the description of the problem

• the geometry specification

• the description of material properties

• the environmental conditions

• the types of prediction desired The sections below discuss each area. Table A-1 in appendix section A.3 shows the units used, and they are also mentioned in comments in the codes.

2.3 Inputs This part of the codes has no separate input file. Most of the inputs are listed in the main.m and model.m. Table 2-2 summarizes the input items. Users make necessary changes for these inputs based on the definition of their problem.

Table 2-2 Input Parameters for the Composite Model Concrete Material Environmental Aggregate (fine and coarse Information Cement aggregate)

• Neutron flux

• Cement type (chemical

• Aggregate fractions in the

• Temperature composition) concrete

• Water-to-cement ratio

• Aggregate type

• Density

• Density

• Compressive strength of

• Elastic modulus hardened cement paste

• Poissons ratio

• Tensile strength of

• Coefficient of thermal expansion hardened cement paste 9

Concrete Material Environmental Aggregate (fine and coarse Information Cement aggregate)

• Ed/E0 (ratio of fully

• Expansion of aggregate under distressed material neutron radiation stiffness to instantaneous

• Degradation of elastic modulus stiffness) under neutron radiation

• Curing time

• Properties of constituent phases in hardened cement paste 2.4 Executing the Program First, open MATLAB (figure 2-1 shows the interface). To run the program, users need to add the folder Composite model and its subfolder MK to the current working folder in MATLAB. Type main in the command window or open main.m in the script editor and click the green Run button on the top.

Figure 2-1 How to run the script 10

Figure 2-2 shows the sequence in which the program files should be run. Table 2-1 describes each program file.

Figure 2-2 Sequence of the program files 2.5 Results and Visualization This part of the code has three outputs: fraction of damaged cement paste (fv), Youngs modulus (E_eff), and dimensional change (e_eff). These three arrays contain material properties that change with neutron levels. They can be plotted versus neutron fluence using the MATLAB plot function. E_eff and e_eff will be exported and stored in two files:

damage.txt and DC.txt. The data in these two files will be used later in the MATLAB code for the transport model of neutron and gamma rays shown in chapter 3. The two examples presented in appendix sections A.1.1 and A.1.2 give more details.

11

3 The Users Manual for Radiation Transport Modeling 3.1 Introduction The radiation transport model was implemented using MATLAB. Users can refer to RIL 2021-07 chapter 4, long-term neutron radiation levels in distressed concrete, and chapter 5, long-term gamma-ray radiation levels in distressed concrete, for the theories involved in this part of the CAICE codes. To help potential users better understand and use the codes for future applications and developments, this users manual contains an overview for this part of the codes, including capabilities and program flow, defining the problem, obtaining inputs, how to run the codes, and how to obtain results. Appendix section A.1.3 includes an example using this part of the codes for demonstration purposes. Appendix section A.2 lists the limitations of the program.

3.1.1 Features and Capabilities A coupled radio-thermo model was developed and added to the MATLAB program based on one-dimensional (1D) two-group neutron diffusion equations, multigroup photon diffusion equations, and the heat conduction equation with heat sources considering neutron and gamma ray heating. The variations of transport properties of distressed concrete due to nuclear irradiation were estimated by cross-property correlation theories, together with the multiphase and multiscale model developed for distressed mechanical properties. The program can calculate the fast and thermal neutron fields, gamma ray photon fields of all photon groups, and the thermal field in concrete.

3.1.2 Structure of the Codes This part of the program is in the N&P folder, which contains the series of files listed in table 3-1. Table 3-1 also lists their types and descriptions. Table 3-1 gives the section numbers of RIL 2021-07 for readers interested in the background theories in the transport analysis.

Table 3-1 Program Files in the Folder N&P File name Type Description The main script for the 1D neutron and photon main_Nng.m script diffusion modeling in concrete (see RIL 2021-07 section 4.1 and appendix sections A.5-A.8) 12

File name Type Description The 1D neutron and photon diffusion modeling in concrete without considering radiation main_Nng_withoutRT.m script heating, radiation, and thermal damage (see RIL 2021-07 section 4.1 and appendix sections A.5-A.8)

Inputs needed for the model, including information about environment, material, Inputs.m script geometry, initial conditions, and boundary conditions (see RIL 2021-07 sections 4.3.2 and 4.3.3)

Calculation of damage parameters and diffusion coefficient matrix using the cross-property damage.m function correlation* between mechanical and transport properties (see RIL 2021-07 section 4.2)

Generation of plots based on the results Plot.m script obtained through this part of the program Damage to concrete at different neutron fluence damage.txt Text doc. levels using the composite model described in chapter 2 Dimensional changes at different neutron DC.txt Text doc. fluence levels using the composite model described in chapter 2

• Different properties of the material can be linked to one another in rigorous ways. Cross-property correlations are useful when some properties can be measured/obtained more easily than others. In this case, the mechanical properties of irradiated concrete were obtained, and transport properties of the concrete are unknown that can be obtained using cross-property correlation and previously obtained mechanical properties (see RIL 2021-07 section 4.2.1 for more details).

3.2 Getting Started Users should have a release of MATLAB installed on their computers and a working knowledge of the program, including but not limited to matrices/arrays and their operations, array indexing, workspace variables, statements, programming scripts and functions, debugging, and plotting functions. Users can refer to the documentation for their version of MATLAB to better understand the programming.

Users set up a model by creating or modifying the necessary m files used by this program.

The files contain information about the problem to be solved, such as the following:

• the description of the problem 13

• the geometry specification

• the description of materials properties

• the environmental conditions

• the types of prediction desired The sections below discuss each area. Table A-1 in appendix section A.3 shows the units used, and they are also mentioned in comments in the codes.

3.3 Executing the Program First, open MATLAB. To run the program, add the folder N&P to the current working folder in MATLAB. Type main_Nng in the command window or open main_Nng.m in the script editor and click the green Run button on the top. Figure 3-1 shows the sequence of running of the program files. Tables 2-1 and 3-1 describe the program files.

Figure 3-1 Sequence of the program files 3.4 Inputs The inputs include all the information needed to describe the problem, as summarized in tables 2-2 and 3-2. A separate input file (Inputs.m) in this part of the codes contains most of the input parameters needed. Some of the inputs needed may be listed in other files. Make the necessary changes to these inputs based on their problems.

14

Table 3-2 Additional Input Parameters for Radiation Transport Modeling Neutrons and Gamma Ray Concrete

• Density

• Neutron diffusion coefficients

• Neutron source (boundary conditions)

• Neutron cross sections

• Photon source (boundary conditions)

• Photon diffusion coefficients

• Photon energy

• Photon coefficients and cross

• Neutron speed sections

• Specific heat capacity

• Thermal conductivity 3.5 Results and Visualization For this part of the codes, outputs are mainly divided into two categories: concrete properties and environmental variables. Concrete properties include damage parameter (di), diffusion coefficients (neutron and photon), thermal conductivity (ki), and dimensional change (DCi);

environmental variables include temperature (T_nn), neutron flux/fluence, and photon flux/fluence. All outputs are in a matrix form because these variables are time dependent and location dependent. This part of the program includes a script called plot.m, which is used to plot the results in MATLAB. Appendix section A.1.3 demonstrates a sample case.

Figure 3-2 1D finite difference mesh along the depth In the analysis performed using the ABAQUS code discussed in chapter 4, two of the output files obtained in matrix form were damage parameter (di) and dimensional change (DCi) related to radiation induced volume expansion (RIVE). For the 1D finite difference mesh used in this chapter (shown in figure 3-2), each value in the two matrices indicates the damage level or RIVE at a specific location and time. The parameters of di and the last column of DCi are saved as two separate data files, 1.dat and 2.dat. For the first case study, another datafile, 3.dat, was generated for coupled creep and damage analysis for one location at various times. The data structures in the three output files are described below.

1.dat: Each row in 1.dat stores the damage values for each time step. Each column in 1.dat stores the damage values at each location (node), shown in appendix section A.1.5. The time steps and locations (grid size) are not stored in 1.dat, so the user needs to go to the 15

subroutine files to obtain information on each time increment and grid size (see figure 4-11 for an example).

2.dat: This file has one column of data, the last column of the DCi matrix (the last time step) shown in appendix section A.1.5. Each value is the dimension change related to RIVE at each specific location (node).

3.dat: This file was generated specifically as the input file for the first case study using the ABAQUS code (CoupDamagCreep_Chapt3_1), as shown in appendix section A.1.4 for the coupled damage-creep study. The first column gives the time, and the second column shows the damage value. The second column of 3.dat is one row in 1.dat, and the selection of the row depends on the location of the material selected.

16

4 The Users Manual for Coupled Damage-Creep Modeling 4.1 Introduction The model was implemented using ABAQUS. RIL 2021-07 chapter 3, Creep of Nuclear Irradiated Concrete, and chapter 6, Coupled Radio-Thermo-Mechanical Analysis, discuss this part of the CAICE codes. To help potential users better understand and use the codes for future applications and developments, this users manual contains an overview of the theories involved in this part of the codes, including capabilities and program flow, defining the problem, obtaining inputs, how to run the codes, and how to obtain results. Appendix sections A.1.4 and A.1.5 present two examples for demonstration purposes, and appendix section A.2 lists the limitations of the program.

4.1.1 Features and Capabilities For concrete material under long-term nuclear irradiation, damage and creep occur concurrently, but ABAQUS cannot handle coupled damage-creep analysis through built-in viscoelastic and damage models. A coupled damage-creep model of nuclear-irradiated concrete was developed based on the generalized Maxwell model for creep development and Mazars damage model for damage evolution. The coupled model was then implemented using ABAQUS through the subroutine UMAT. The constitutive model implemented uses the isotropic scalar damage model (with scalar damage parameter D).

The damage factor (1-D), which characterizes the stiffness reduction of the material, includes two independent damage processes in the program: the mechanical damage obtained through Mazars damage model and the nuclear irradiation damage estimated based on the multiphase and multiscale model and the transport model implemented in the MATLAB code.

4.1.2 Structure of the Codes This part of the program is in the ABAQUS folder, which contains the series of files listed in table 4-1. Table 4-1 also lists their types and descriptions.

17

Table 4-1 Program Files in the Folder ABAQUS File name Type Description Nuclear irradiation damage obtained using the 1.dat Data file multiscale and multiphase models developed in MATLAB (Composite model described in chapter 2)

Strain of the concrete obtained using the multiscale 2.dat Data file and multiphase models developed in MATLAB (Composite model described in chapter 2)

Calculation of damage parameter and diffusion Fortran CoupDamagCreep.f coefficient matrix using cross-property relations source between mechanical and transport properties The structure of CoupDamagCreep.f is explained below. Some important equations in RIL 2021-07 are mentioned for clarity.

1) Subroutine UEXTERNALDB Figure 4-1 Lines of code for the subroutine UEXTERNALDB Figure 4-1 shows the subroutine UEXTERNALDB. It is used to call each data file once at the beginning of the analysis. The two data files from chapter 3, 1.dat and 2.dat, are read and stored as pp1 and pp2 in ABABQUS analysis. The data in these files are used by subroutine UMAT.

18

1) Subroutine UMAT The subroutine UMAT was developed to provide material models that are not available in ABAQUS. Figure 4-2 shows the header, followed by dimensioning of local arrays.

Figure 4-2 Lines of code for the header of the subroutine UMAT

• Inputs This part of the codes, shown in figure 4-3, read inputs provided by users through the ABAQUS interface; these inputs are only used in the subroutine UMAT.

19

Figure 4-3 Lines of code for the inputs of the subroutine UMAT

• Check damage The part of the codes shown in figure 4-4 is the damage evolution algorithm developed in Mazars damage model. Users can refer to equations 3-29 and 3-30 in RIL 2021-07.

Figure 4-4 Lines of code for damage initialization and damage threshold update

• Add strain The part of the codes shown in figure 4-5 adds a radiation-induced strain (pp2) at the end of the analysis at each integration point. The algorithm will be explained in detail later in the instructions for Introduce radiation damage below.

20

Use the correct grid size Figure 4-5 Lines of code for radiation-induced strain

• Linear elasticity The part of the codes shown in figure 4-6 is used to calculate the parameters for the linear elasticity theory for continuous media.

Figure 4-6 Lines of code for the linear elasticity model

• Generalized Maxwell model The lines of code shown in figures 4-7 and 4-8 describe a generalized Maxwell model with seven Maxwell elements. Figure 4-7 shows the calculation process used to obtain internal state variables (ISVs) (refer to equation 3-26 in RIL 2021-07). Figure 4-8 shows the 21

calculation process used to obtain the strain and stress values (refer to equations 3-24 and 3-25 in RIL 2021-07).

Figure 4-7 Lines of codes for the calculation of ISVs in the generalized Maxwell model Figure 4-8 Lines of the codes for the calculation of creep strain, elastic strain, and effective stress in the generalized Maxwell model 22

• Mazars damage model The lines of codes shown in figure 4--9 and figure 4-10 describe Mazars damage model.

Figure 4-9 shows how to obtain the equivalent strain; users can refer to equations 3-28, 3-32, 3-33, and 3-34 in NRC RIL 2021-07. Figure 4-10 shows the calculation process to obtain the mechanical damage; users can refer to equations 3-31, 3-35, and 3-36 in NRC RIL 2021-07.

Figure 4-9 Lines of code for the calculation of equivalent strain in Mazars damage model 23

Figure 4-10 Lines of the codes for the calculation of mechanical damage in Mazars damage model

• Introduce radiation damage The lines of code shown in figure 4-11 introduces the radiation damage (pp2) obtained through the MATLAB models in the ABAQUS analysis using linear interpolation. The time and space domain synchronizations between the MATLAB code and ABAQUS UMAT are explained below.

Use the correct grid size and time step Figure 4-11 Lines of the codes for the introduction of radiation damage 24

• Time domain synchronization To obtain the correct values at current locations from the data imported through data files, such as strain or radiation damage, the time domains used in MATLAB and ABAQUS should be synchronized first. As shown in figure 4-12, different time steps are used in the MATLAB and ABAQUS codes. In MATLAB, the size of the time step is defined as uniform, which means that the time step is fixed and will not change along with the analysis. However, the time step is usually set to automatic for highly nonlinear problems in ABAQUS, which means that the time step is dynamic and will change along with the analysis. As illustrated in figure 4-12, the linear interpolation method is used to calculate the value in order to obtain the correct value of imported data at a specific time at a fixed location.

Figure 4-12 Time domain synchronization between MATLAB and ABAQUS UMAT

• Space domain synchronization At present, MATLAB is only capable of modeling 1D problems, while the modeling in ABAQUS is three dimensional (3D) and so can handle more complicated structures. To obtain the correct values at a specific location in a 3D finite element model, based on the data from the 1D MATLAB model, a synchronization process is needed. Figure 4-13 shows the approach adopted. For radiation damage modeling, a 3D finite element model of a biological shielding wall is converted into multiple finite element bars along the z direction (the depth in the wall), and each bar can be considered as a 1D problem in MATLAB. In this way, 3D modeling considering radiation damage can be simplified by assembling multiple 1D models. It should be noted that, using this method, only the radiation transport along the z direction is considered. The spatial distribution of the radiation level on the surface of the wall can be considered by assigning different boundary conditions to different finite element 25

bars. This 1D approach is only a simplification; a 3D model for nuclear damage and transport analysis needs to be developed in the future based on the 1D model.

A similar linear interpolation method used for time domain synchronization can then be used, as shown in figure 4-14. Different meshes were used in MATLAB and ABAQUS. In MATLAB, the mesh size is uniform in 1D, while a different meshing strategy is used in ABAQUS.

Figure 4-13 Convert a 3D problem into multiple 1D problems Figure 4-14 Space domain synchronization between MATLAB and ABAQUS UMAT

• Total damage As shown in figure 4-11, the total damage is the combination of mechanical damage and radiation-induced damage in a multiplying format. The mechanical damage is estimated based on Mazars damage model using ABAQUS UMAT, and the radiation-induced damage is in (?) the outputs of MATLAB (in the folders Composite model and N&P).

26

• Storage of ISVs The lines of code shown in figure 4-15 are intended to store the ISVs required during the analysis.

Figure 4-15 Lines of the codes for the storage of ISVs and some results 4.2 Getting Started Users should have a release of ABAQUS with user subroutines capability installed on their computers. Users should also have a working knowledge of ABAQUS/CAE (complete ABAQUS environment), including how to create and analyze finite element models using ABAQUS modules, how to customize ABAQUS functionality using UMAT, and how to evaluate and visualize results. Users can refer to the documentation for their version of ABAQUS to better understand the programming. A brief guide introducing the modeling process is provided below.

27

Users should set up their models by themselves based on their problem definitions.

Necessary modifications should be made in some parts of the program files, and certain information should be collected before modeling, including the following:

• the description of the problem

• the geometry specification

• the description of materials properties

• the environmental conditions

• the types of prediction desired In general, use the modules in ABAQUS/CAE to define a models geometry and other physical properties, submit the model for analysis, and view the results of the analysis. The Part, Property, Assembly, Step, Interaction, Load, Mesh, Job, and Visualization modules are needed. Users should refer to demonstrations presented in appendix sections A.1.4 and A.1.5 during the modeling.

Table A-1 in appendix section A.3 shows the units used, which are also mentioned in comments in the codes.

4.3 Inputs The inputs include all the information needed to describe the problem and are summarized in tables 2-2, 3-2, and 4-2. Users can make the necessary changes to these inputs based on their problems.

Table 4-2 Additional Input Parameters for Coupled Damage-Creep Modeling Concrete Other

• Instantaneous Youngs modulus

• Poissons ratio

• Mechanical

• Prony series parameters ( , pm) loadings

• Parameters for Mazars damage model (0, At, Bt, Ac, Bc) 28

4.4 Executing the Program Once the preprocessing stage of the model is complete, users can either use the convenient ABAQUS/CAE user interface or the command line interface to submit an ABAQUS analysis.

The analysis parameters, such as user subroutines, should be set when a job is submitted.

Figure 4-16 shows the sequence of all the program files. Tables 2-1, 3-1, and 4-1 describe each program file.

Figure 4-16 Sequence of all the program files 4.5 Results and Visualization In addition to the results obtained in chapters 2 and 3, the output results can be configured in the field output requests in the Step module in ABAQUS/CAE, such as stresses, strains, displacements, and state variables. Users can employ the Visualization module to view the model and the results of the analysis. Appendix sections A.1.4 and A.1.5 present two examples for demonstration purposes.

29

Appendix A.1 Demonstrations The case studies shown in the U.S. Nuclear Regulatory Commissions (NRCs) Research Information Letter (RIL) 2021-07, Radiation Effects on ConcreteAn Approach for Modeling Degradation of Concrete Properties, issued August 2021 (Agencywide Documents Access and Management System Accession No. ML21238A064), are explained in the following step-by-step demonstrations.

A.1.1 Validation of the Composite Model

• The code for the multiscale and multiphase model (the composite model) are in the Composite model folder. Open the folder Composite model and add the folder and its subfolder MK to the current working folder in MATLAB.

• In the Composite model folder, open main.m.

• In the MATLAB script editor, obtain the inputs from the literature. RIL 2021-07 section 2.7 lists the inputs for this case study. The inputs are specific to each problem, so the inputs in main.m need to be revised based on the information of the problem, such as neutron radiation levels, aggregate RIVE, concrete mix design information, and others, as shown below.

• For each neutron fluence level, multiple steps should be taken to reach the final value. Modify the code as shown below.

30

• Execute the code by clicking Run in MATLAB

• The results of Youngs modulus are stored in the array E_eff and the results of dimensional change are stored in the array e_eff.

A.1.2 Parametric Analyses of the Composite Model Input Parameters

• Parameters including the water-cement ratio, aggregate fraction, and aggregate expansion

• Steps similar to those shown in section A.1.1 are used here. The multiscale and multiphase model is used for the parametric analysis, so the current working folder remains the same. Open main.m in the MATLAB script editor, obtain the input parameters listed in RIL 2021-07 section 2.8, and modify the inputs in main.m.

• A certain number of steps should be used to achieve convergence and accuracy (e.g., 10,000), as shown below.

31

• Execute the code by clicking Run.

• The results of Youngs modulus are stored in the array E_eff and the results of dimensional change are stored in the array e_eff.

• Compare the results obtained using different input parameters. For example, comparing the results of different water-to-cement ratios reveals the effect of this concrete design parameter on the properties of neutron-irradiated concrete.

Note: In the above code, the tic function at the beginning records the current time while the toc function at the end (not shown in the figure above) uses the recorded value to calculate the elapsed time. They are used together to estimate running time and have no effect on the results.

A.1.3 Radiation Transport Modeling for a Simplified Example

• The code for radiation transport modeling is in the N&P folder. In this case, evaluate the radiation-induced damage first using the composite model, then use the results in the transport model to consider the effect of radiation-induced damage on the transport properties of the concrete.

32

• Run main.m in the Composite model folder. Appendix sections A.1.1 and A.1.2 show the process. RIL 2021-07 section 5.2 lists the inputs used in this case. The results are stored in two files, named damage.txt and DC.txt, and are used for the degradation of Youngs modulus and dimensional changes at different neutron fluence levels, respectively.

• Change the current working folder in MATLAB to the folder N&P for radiation transport analysis.

• Open input.m and main_Nng.m in the MATLAB script editor, as shown below. Make the necessary changes according to the inputs listed in RIL 2021-07 section 5.2.

input.m 33

main_Nng.m

• Execute the code main_Nng.m by clicking Run.

• The result of damage is in the matrix di and the result of dimensional change is in the matrix DCi. These two matrices store all the data at different locations and different times, and are saved as 1.dat and 2.dat, respectively. These two data files will be used in the case study shown in appendix section A.1.5.

• Other results are also available in other arrays: n1 is for fast neutron fluence, T_nn is for temperature, and Dose is for gamma ray dose. These are the neutron, temperature, and gamma ray distributions in concrete that take into account the effects of radiation-induced damage.

A.1.4 Analysis of an Example Using the Coupled Damage-Creep Model

• This example is for a coupled damage-creep analysis of concrete at a fixed location.

• Run main.m in Composite model (appendix section A.1.1 shows the process).

RIL 2021-07 section 3.6.3 lists the inputs. The damage is obtained based on the degradation of Youngs modulus, stored in array E_eff. A data file called 3.dat is generated for this case study, as shown below. The first column is the time, and the second column is the damage parameter. Section 3.5 describes the detail of the 3.dat file.

34

• For this case study, a finite element model in ABAQUS is created for the concrete at a fixed location, as shown below.

a. Create model

b. Set material 35

c. Set time step

d. Define boundary conditions

e. Generate mesh

• Go to the Job module and create a job. In Edit Job, go to tab General, select the correct user subroutine file (for this case study, the ABAQUS code CoupDamagCreep_Chapt3_1 should be selected; click OK and Job manager, then submit the job created. The figures below show the process.

36

• Note that the code (CoupDamagCreep_Chapt3_1) and the input file (3.dat) are specifically designed for this case study, not for general structural analysis. The general approach is shown in the next case study, presented in appendix section A.1.5.

a. Create a job based on the model

b. User subroutine file selection 37

c. Job submission

• Once the job is completed, click the results button; the Visualization module will then appear.

• For this case study, the results are the strain-stress curve under irradiation and creep. As shown below, click Create XY Data, select ODB field output, then click Continue.

38

• Check the variables (S33 and E33), go to tab Elements/Nodes, select the element targeted, and then click Plot to plot the results. The process is shown below.

• Go to XY Data Manager, select the data to be checked, and click Edit, which will give you access to the actual data points.

A.1.5 A Comprehensive Case Study: A Coupled Radio-Thermo-Mechanical Analysis for a Section of a Concrete Biological Shielding Wall in a Nuclear Power Plant

• This case study focuses on the coupled radio-thermo-mechanical damage in a concrete wall, so the MATLAB code in the two folders Composite model and N&P is used to obtain the damage distribution of concrete at different locations and different times.

39

• RIL 2021-07 section 6.2 lists the inputs. As mentioned at the end of appendix section A.1.3, the data about damage and dimensional change should be obtained first using the MATLAB code in the Composite model and N&P folders. The results needed here are saved as 1.dat and 2.dat files as shown below. Section 3.5 describes the details of the 1.dat and 2.dat files.

1.dat 2.dat

• The ABAQUS code CoupDamagCreep is used for this case study.

• The similar process shown in appendix section A.1.4 is used for the finite element analysis of this case study; however, only the visualization of the results is shown here.

• Once the job is completed, click results to reveal the Visualization module.

• Click Tools to go to the tool menu, then create a path as shown in the figure below.

• Select all the nodes along the path you want to plot data and click OK.

40

• Click Create XY Data, select Path, and click Continue.

• Select the path and field output variable you want to plot, then click Plot.

41

• Similarly, go to XY Data Manager to view the data.

42

Note: The ABAQUS code (CoupDamagCreep) and the input files (1.dat and 2.dat) used in this case study can be used for general structural analysis.

A.2 Warnings and Limitations

• The MATLAB code covered in these users manuals was written in MATLAB R2018a in Windows 10. In very rare cases, this may cause issues when the code is run using different MATLAB versions.

• Users must have access to ABAQUS or the complete ABAQUS environment with user subroutine capability to run some parts of the program. This usually requires installing additional software.

• This program is not foolproof. Error messages may appear due to parameters changes.

• The benchmarking done by code developers for the program may or may not be adequate for a users particular requirements.

A.3 Units Table A-1 shows the units used. The units used are also shown in the codes.

Table A-1 Units Quantity Unit Length cm Density kg/cm3 Pressure Pa Temperature ºC Elastic modulus Pa Time Sec Thermal conductivity W/(cm*K)

Energy MeV A.4 Program Diagram Table A-2 gives the structure of the program listing the modeling methods, file names, and folder names. The diagram of the program shows the various parts of the program with associated folders and files.

43

Table A-2 Structure of the Program Folder Modeling File Name Name Generalized self-consistent Composite model/composite damage mechanics of All files model concrete Mori-Tanaka model of cement paste All files MK Radiation transport (neutrons and photons) main_Nng.m N&P Heat conduction Cross-property correlation damage.m N&P Coupled damage-creep model CoupDamagCreep.f ABAQUS 44

Diagram of the program with file names 45