JAEA-Research2024-001
DOI:10.11484/jaea-research-2024-001

Standard Guideline for the Seismic Response Analysis Method Using
Three-Dimensional Finite Element Modelof Reactor Buildings (Contract Research)(Translated Document)
Byunghyun CHOI, Akemi NISHIDA, Manabu KAWATA, Tadahiko SHIOMI
and Yinsheng LI

Materials and Structural Integrity Research Division
Nuclear Safety Research Center
Sector of Nuclear Safety Research and Emergency Preparedness

March 2024
Japan Atomic Energy Agency

日本原子力研究開発機構

本レポートは国立研究開発法人日本原子力研究開発機構が不定期に発行する成果報告書です。
本レポートはクリエイティブ・コモンズ 表示 4.0 国際 ライセンスの下に提供されています。
本レポートの成果（データを含む）に著作権が発生しない場合でも、同ライセンスと同様の条件で利用してください。（https://creativecommons.org/licenses/by/4.0/deed.ja）
なお、本レポートの全文は日本原子力研究開発機構ウェブサイト（https://www.jaea.go.jp）
より発信されています。本レポートに関しては下記までお問合せください。
国立研究開発法人日本原子力研究開発機構〒 319-1112

JAEA イノベーションハブ

研究成果利活用課

茨城県那珂郡東海村大字村松 4 番地 49

E-mail: ird-support@jaea.go.jp
This report is issued irregularly by Japan Atomic Energy Agency.
This work is licensed under a Creative Commons Attribution 4.0 International License(https://creativecommons.org/licenses/by/4.0/deed.en).
Even if the results of this report (including data) are not copyrighted, they must be used under
the same terms and conditions as CC-BY.
For inquiries regarding this report, please contact Institutional Repository and Utilization Section,
JAEA Innovation Hub, Japan Atomic Energy Agency.
4-49 Muramatsu, Tokai-mura, Naka-gun, Ibaraki-ken 319-1112, Japan
E-mail: ird-support@jaea.go.jp© Japan Atomic Energy Agency, 2024

JAEA-Research 2024-001

Standard Guideline for the Seismic Response Analysis Method Using ThreeDimensional Finite Element Model of Reactor Buildings(Contract Research)(Translated Document)
Byunghyun CHOI, Akemi NISHIDA, Manabu KAWATA, Tadahiko SHIOMI and Yinsheng LI
Materials and Structural Integrity Research Division, Nuclear Safety Research Center
Sector of Nuclear Safety Research and Emergency Preparedness
Japan Atomic Energy Agency
Tokai-mura, Naka-gun, Ibaraki-ken(Received January 4, 2024)
In the assessment of seismic safety and the design of building structures in nuclear facilities , lumped
mass models have been used as standard methods. Recent advances in computer capabilities allow theuse of three-dimensional finite element (3D FE) models to account for the 3D behavior of buildings,
material nonlinearity, and the nonlinear soil-structure interaction effect. While 3D analysis method has
many advantages, it is necessary to ensure its reliability as a new approach. The International Atomic
Energy Agency performed an international benchmark study using the 3D FE analysis model for reactor
building of Unit 7 at TEPCO's Kashiwazaki-Kariwa Nuclear Power Station based on recordings from the
Niigataken Chuetsu-oki Earthquake in 2007. Multiple organizations from different countries participatedin this study and the variation in their analytical results was significant, indicating an urgent need to
improve the reliability of the analytical results by standardization of the analytical methods using 3D FE
models. Additionally, it has been pointed out that it is necessary to understand the 3D behavior in theseismic fragility assessment of buildings and equipment, using realistic seismic response analysis method
based on 3D FE models. In view of these considerations, a guideline for the seismic response analysis
method using a 3D FE model was developed by incorporating the latest knowledge and findings in thisarea. The purpose of the guideline is to improve the reliability of the seismic response analysis method
using 3D FE model of reactor buildings. The guideline consists of a main body, commentaries, andappendixes. The standard procedures, recommendations, key points to note, and technological bases for
conducting seismic response analysis on reactor buildings using 3D FE models are provided in theguideline. In addition, the guideline will be revised reflecting the latest knowledge.
Keywords: 3D FEM, Seismic Response Analysis, Reactor Building, Guideline
This report includes a part of the results obtained in the contract research entrusted from Secretariat of
Nuclear Regulation Authority of Japan.
This document is the English translation of “Standard Guideline for the Seismic Response Analysis
Method Using 3D Finite Element Model of Reactor Buildings” (JAEA-Research 2021-017).

i

JAEA-Research 2024-001

原子炉建屋の 3 次元有限要素モデルを用いた
地震応答解析手法に関わる標準的解析要領（受託研究）（翻訳資料）
日本原子力研究開発機構 安全研究・防災支援部門
安全研究センター 材料・構造安全研究ディビジョン
崔

炳賢、西田

明美、川田

学、塩見

忠彦、李

銀生

（2024 年 1 月 4 日受理）
原子力発電施設における建物・構築物の地震応答解析においては、我が国では、従来より質点系モデルが用いられてきたが、近年の解析技術の発展により、立体的な建物を 3 次元的にモデル化し、建物の 3 次元挙動、建物材料の非線形性、建物及び地盤間の非線形性等を考慮した有限要素法による地震応答解析が実施されるようになってきた。3 次元モデルによる有限要素
解析（3 次元 FEM）は，複雑で高度な技術が用いられる一方、汎用性があるために広く利用され、原子力分野以外では構造物のモデル化、材料物性の非線形特性の信頼性を確保するためのガイドラインの策定や技術認定などがなされるようになってきた。原子力分野においては、
IAEA により平成 19 年（2007 年）新潟県中越沖地震における質点系モデル、3 次元 FEM モデルによる観測記録の再現解析が KARISMA ベンチマークプロジェクトとして実施され、複数の解析者の解析結果が報告された。その報告によると、解析者により解析結果にばらつきが大きいということが判明され、解析手法の標準化による解析結果の信頼性の確保が急務となっている。また、原子力発電施設の強非線形領域の現実的な挙動の評価が必要となる建物・構築物・機器のフラジリティ評価においても詳細な 3 次元挙動把握の必要性が指摘されている。こうした背景を踏まえ、原子炉建屋を対象とした地震応答解析に用いられる 3 次元 FEM モデルの作成及び解析にあたって必要となる一般的・基本的な手法や考え方を取りまとめて標準的解析要領を整備した。これにより原子炉建屋の 3 次元 FEM モデルによる地震応答解析手法の信頼性向上につながることが期待される。本標準的解析要領は、本文、解説、及び解析事例で構成されており、原子炉建屋 3 次元 FEM モデルを用いた地震応答解析の実施手順、推奨事項、留意事
項、技術的根拠等が含まれている。また、本標準的解析要領は、最新知見を反映し、適宜改訂する。
本報告書は、原子力規制委員会原子力規制庁からの受託事業「原子力施設等防災対策等委託費（高経年化を考慮した建屋・機器・構造物の耐震安全評価手法の高度化）」の成果の一部である。
本報告書は、JAEA-Research 2021-017 を英訳したものである。
原子力科学研究所：〒319-1195

茨城県那珂郡東海村大字白方 2-4ii

JAEA-Research 2024-001

Table of Contents
I.

Position of the guideline ................................................................................................................... 1
1. Background and purpose .................................................................................................................. 1
2. Trend in the 3D FEM model analysis methods application guide .................................................... 4
3. Basic policy of the guideline ............................................................................................................ 7

II. Main body ........................................................................................................................................... 8
1. General information ......................................................................................................................... 8
2. Purpose and object of analysis ....................................................................................................... 17
3. Analysis domain ............................................................................................................................. 22
4. Creation of the geometric model .................................................................................................... 29
5. Creation of the structural model ..................................................................................................... 37
6. Mass model .................................................................................................................................... 47
7. Material model ............................................................................................................................... 49
8. Mathematical model of damping .................................................................................................... 56
9. Boundary joint model ..................................................................................................................... 60
10. Input seismic motion ...................................................................................................................... 67
11. Initial state model ........................................................................................................................... 69
12. Condition setting for mathematical analysis ................................................................................... 71
13. Examination and validation of analysis results .............................................................................. 77
14. Utilization of analysis result ........................................................................................................... 83
15. Documentation ............................................................................................................................... 86
Acknowledgment ................................................................................................................................... 87
References ............................................................................................................................................. 88
Appendix ............................................................................................................................................... 93
Attachment 1

Sensitivity analysis results of the influential factors ............................................. 93

Annex 1Modeling by solid element and shell element ............................................................... 95

Annex 2

Effect of different damping modeling ........................................................................... 99

Annex 3

Accuracy of vertical response of reactor building ...................................................... 105

Annex 4

Effect of nonlinear soil-structure interaction .............................................................. 112

Annex 5

Effect of nonlinear constitutive model of reinforced concrete .................................... 126

Annex 6

Effect of finite element program ................................................................................. 139

Annex 7

Effect of mesh sizes of finite elements ....................................................................... 144

Attachment 2

Analysis example ................................................................................................ 151

iii

JAEA-Research 2024-001

目
I.

次

本解析要領の位置づけ .................................................................................................................. 1
1. 背景及び目的 .................................................................................................................................. 1
2. 3 次元 FEM 解析の適用ガイドの動向 ......................................................................................... 43. 本解析要領の基本方針 .................................................................................................................. 7

II. 本編 ................................................................................................................................................... 8
1. 一般事項 .......................................................................................................................................... 8
2. 解析の目的及び対象 .................................................................................................................... 17
3. 解析領域 ........................................................................................................................................ 22
4. 形状モデルの作成 ........................................................................................................................ 29
5. 構造モデルの作成 ........................................................................................................................ 37
6. 質量モデル .................................................................................................................................... 47
7. 材料モデル .................................................................................................................................... 49
8. 減衰の数理モデル ........................................................................................................................ 56
9. 境界接合部モデル ........................................................................................................................ 60
10. 入力地震動 .................................................................................................................................... 67
11. 初期状態モデル ............................................................................................................................ 69
12. 数値解析に関する条件設定 ........................................................................................................ 71
13. 解析結果の照査と妥当性確認 .................................................................................................... 77
14. 解析結果利用 ................................................................................................................................ 83
15. 文書化 ........................................................................................................................................... 86
謝辞 ....................................................................................................................................................... 87
参考文献 ............................................................................................................................................... 88
付録 ....................................................................................................................................................... 93
別紙 1

影響因子の感度解析結果 ............................................................................................. 93

附属書 1

異なるタイプの有限要素によるモデル化の違いによる影響 ............................... 95

附属書 2

減衰のモデル化の違いによる影響 .......................................................................... 99

附属書 3

建物地盤連成における水平動－上下動の影響 .................................................... 105

附属書 4

側面剥離・滑りの考慮の有無による影響 ............................................................ 112

附属書 5

鉄筋コンクリート非線形の地震応答への影響 .................................................... 126

附属書 6

有限要素の精度の違いによる影響 ........................................................................ 139

附属書 7

有限要素のメッシュサイズの違いによる影響 .................................................... 144

別紙 2

適用事例 ....................................................................................................................... 151

iv

JAEA-Research 2024-001

List of Tables
Table II-2-1

Combinations of SI units used in seismic response analysis ................................... 20

Table II-3-1

Selection conditions of the walls considered in the simulation analysis of the

Niigataken Chuetsu-oki Earthquake in 2007 .......................................................................... 24
Table II-5-1

Comparison of natural frequencies of beam/shell structural model and solid structuralmodel between the building basemat and B2F ....................................................................... 41
Table II-7-1

Viscous damping constants of materials (ASCE/SEI 4-16)..................................... 54

Table II-7-2

Viscous damping constants of materials (JEAG 4601-1987) .................................. 55

Table II-9-1

Constitutive law of joint element ............................................................................ 62
List of Figures

Fig.I-1-1

Example of a 3D FEM model analysis in the KARISMA benchmark project ................ 3

Fig.II-1-1

Analysis flow ................................................................................................................ 9

Fig.II-3-1

Examples of seismic walls and auxiliary walls ........................................................... 24

Fig.II-3-2

Diagram of the structure and the surrounding ground................................................. 28

Fig.II-4-1

Examples of creating geometric and structural models ............................................... 31

Fig.II-4-2

Coupling of the vertical deformation of the roof and the horizontal deformation of thestructure ................................................................................................................................. 33
Fig.II-4-3

Diagram of a geometric model consisting of solid elements....................................... 34

Fig.II-4-4

Visualization of modeling that takes strata into account ............................................. 36

Fig.II-5-1

Modeling of a corner .................................................................................................. 38

Fig.II-5-2

Example of member joint between a plane element and beam element ...................... 39

Fig.II-5-3

Analysis of a cantilever beam with isoparametric quadratic element ......................... 43

Fig.II-5-4

Example of mesh in JEAG4601-1987 ......................................................................... 45

Fig.II-7-1

Relationship between the size of shear strain and the ground constitutive law ........... 53

Fig.II-7-2

Equivalent stiffness and equivalent damping in equivalent linearization analysis ...... 53

Fig.II-9-1

Constitutive law of joint elements (Axial direction component) ................................ 62

Fig.II-9-2

Constitutive law of joint elements (Shear direction component) ................................ 62

Fig.II-9-3

Modeling of analysis ground area ............................................................................... 65

Fig.II-10-1

Overview of input seismic motion preparation ......................................................... 68

Fig.II-12-1

Diagram of the interpolation of transfer function in frequency response analysis .... 73

Fig.II-13-1

Examples of warning and error messages (MSC Nastran 2019） ............................ 79

Fig.II-13-2

Example of input text echo back (MSC Nastran 2019） .......................................... 80

Fig.II-13-3

Example of abnormal mode shapes caused by data error .......................................... 80v

This is a blank page.

JAEA-Research 2024-001

I. Position of the guideline
1. Background and purpose
In seismic response analysis of building structures in nuclear power facilities, in Japan,
the traditional mass-spring model has historically been used. However, with the advancementof recent analytical techniques, three -dimensional modeling of complex structures has
become feasible. Simultaneously, seismic response analyses utilizing the finite element
method, which considers the three -dimensional behavior of buildings, the nonlinear
characteristics of building materials, and the nonlinear interaction between buildings and thefoundation soil, has started to be conducted.
Three-dimensional finite element analysis, often referred to as 3D FEM analysis, i nvolves
using detailed three-dimensional models and employs more advanced techniques comparedwith conventional methods. It is not limited to the nuclear field but has been found in various
other fields, such as architectural buildings and civil engineerin g structures. These
applications come with established guidelines to ensure the reliability of nonlinear material
properties and also have been implemented technical certifications. Notable examples ofthese applications include:

The Japan Society of Civil Engineers' Concrete Standard Specifications



Guidelines related to Verification and Validation (V&V) by the Japan Society for
Computational Engineering and the Atomic Energy Society of Japan

Professional certifications offered by the Japan Society of Mecha nical EngineersTechnical certifications related to numerical analysis by the Japan Society of Civil
Engineers
In the nuclear field, the International Atomic Energy Agency (IAEA) conducted abenchmark project called the KARISMA in 2007 to simulate observed records using massspring models and 3D FEM models for reactor building of Unit 7 at TEPCO's Kashiwazaki Kariwa Nuclear Power Station based on recordings from the Niigataken Chuetsu-oki
Earthquake in 2007 1 . Multiple analysts reported their results by 3D FEM. Fig. I-1-1(a) shows
an example of the acceleration response spectrum at observation positions (on the basemat)
and the 3D FEM model used in the analysis. The thick red line represents the observed record.
The results of the analysis showed significant variation among different analysts. Given thisbackground, ensuring the reliability of analysis results through standardization of analysis
methods has become a pressing need 2 . Additionally, for the seismic fragility assessment ofbuildings, structures, and equipment that require an evaluation of realistic behavior instrongly nonlinear regions of nuclear power facilities, the necessity of detailed understandingof three-dimensional behavior has been emphasized.
These guidelines serve as compilation of general and fundamental procedures andapproaches essential for developing and analyzing 3D Finite Element Models (FEM) used in-1-

JAEA-Research 2024-001

seismic response analysis for nuclear reactor buildings. Its primary purpose is to improve
the reliability of seismic response analysis methods for nuclear reactor buildings whenemploying 3D FEM models. Additionally, it offers a comprehensive reference for thecreation and analyzing such models, aiding in their development and examination.

-2-

Acceleration (cm/s 2 )JAEA-Research 2024-001

Frequency (Hz)

Acceleration (cm/s 2 )NS (X) direction

Frequency (Hz)UD (Z) direction(a) Acceleration response spectra (h = 5%) (basemat)(b) Examples of a 3D FEM model of a reactor building
Fig.I-1-1

Example of a 3D FEM model analysis in the KARISMA benchmark project 1-3-

JAEA-Research 2024-001

2. Trend in the 3D FEM model analysis methods application guide
The following presents the trend related to analysis methods, validity of analysis methods,
and ensuring reliability in 3D FE M analysis are positioned within the guidelines andstandards of major organizations.
2.1 Nuclear Regulation Authority in Japan
In the “Examination Guide for Standard Seismic Motion and Seismic Design Policy 3 ”, theevaluation of input seismic motion is specified to be considered using a three -dimensional
subsurface structure model. In the “Examination Guide for Structural Certification Related
to Seismic Design” 4 , in cases where the simultaneity of responses ne eds to be consideredbased on the phase characteristics of input seismic motion in each direction or the three dimensional response characteristics of buildings/structures, a method such as sequentiallysuperimposing response values at each response time history for each direction is describedto account for simultaneity. In the “Operational Guide for Enhancing Safety Assessment ofPractical Power Generating Nuclear Reactors 5 ”, evaluation of realistic responses up to thedamage limit considering three -dimensional response characteristics (floor deformations,torsion, etc.) for fragility assessment is described to be suitable using 3D FEM analysis.
Additionally, according to NTEC -2021-4002 6 , new considerations for the seismic safety ofbuildings were discussed in reviews involving the seismic response analysis results of soilstructure interaction by 3D FEM models. Furthermore, in the same document, it isexamined the validity of seismic response analysis methods using 3D FEM models and themodeling of influential factors that are likely to affect the response characteristics of thebuilding.
2.2 Japan Electric Association
The “Technical Guidelines for Seismic Design of Nuclear Power Plants, JEAG46011984/1991/2015 7 , 8 , 9 ” discusses the necessity of 3D-FEM model analysis capable ofconsidering deformation of the basemat, irregularity of the ground, deep embedding ofstructures, and neighboring buildings, a nd so on, in particular, in the dynamic soil-structureinteraction.
2.3 Atomic Energy Society of Japan
Following on the Niigata ken Chuetsu-oki Earthquake in 2007, a “Seismic Safety Roadmap ”
was formulated in collaboration with the Japan Association for Earthquake Engineering.
Furthermore, considering the Fukushima Daiichi Nuclear Power Station accident caused by
the 2011 off the Pacific Coast of Tohoku Earthquake, the “Roadmap for Light Water Reactor
Safety Technology and Human Resources at the Atomic Energy Society of Japan – Rolling-4-

JAEA-Research 2024-001

Response – Final Report” 1 0 was compiled in the fiscal yea r 2013 and revised in 2017. In
these roadmaps, the necessity for response analysis and systematized evaluation based on 3D
FEM for seismic response of buildings and structures is highlighted.
Essentially, the Atomic Energy Society of Japan's standard “A Standard for Procedure ofSeismic Probabilistic Risk Assessment for Nuclear Power Plants: 2015 1 1 ” emphasizes thenecessity of 3D FEM for realistic response evaluation of buildings and structures.
Additionally, in the “Guidelines for Ensuring Reliability in S imulations: 2015 1 2 ” theSubcommittee on Simulation Reliability within the Standardization Committee Infrastructure
and Applied Technology Division, after deliberations within the division, outlines a sharedapproach across a wide range of technical fields to ensure the relia bility of simulations
related to nuclear power.
2.4 Japan Society of Mechanical Engineers
In the “Codes for Nuclear Power Generation Facilities – Rules on Design and Construction
for Nuclear Power Plant: Alternative Design for Seismic Design of Seismic S Class Steel
Piping Based on Elastic-Plastic Response Analysis (2019) 1 3 ” of the Japan Society of
Mechanical Engineers, which is one of the standards of power generation nuclear energy
facilities, 3D FEM modeling is the premise.
Moreover, the Japan Society of Mechanical Engineers provides computational dynamics
technician certification to ensure a high technological proficiency level in analysis
technicians.
2.5 Architectural Institute of JapanFor nuclear power facilities, the “ AIJ Standard for Structural Calculation of Reinforced
Concrete Structures for Nuclear Power Facilities (2013) 1 4 ” has been compiled. Moreover,the “Guidebook for Numerical Analysis of Spatial Structure (2017) 1 5 ” contains a detailed
explanation of issues, basic theory of the ir analysis, and basis for selecting modeling andanalysis methods regarding the numerical analysis used for the structural design of spatial
structures; it includes the basic points of caution in 3D -FEM model analysis.
2.6 Japan Society of Civil Engineers
The nonlinear analysis method for reinforced concrete structures using 3D FEM model s is
discussed in detail in the Japan Society of Civil Engineers’ “Standard Specifications forConcrete Structures -2017, Design 1 6 ”. They also authorize numerical analysis certification
based on their technical evaluation system.
Moreover, regarding important outdoor structures and underground structures, the Japan
Society of Civil Engineers published the “Seismic Performance Verification Guidelines,
Manuals and Examples for Underground RC Structures in Nuclear Power Plants (2018) 1 7 ” to-5-

JAEA-Research 2024-001

advance and systematize methods for the examination of the seismic performance ofreinforced concrete structures that are important outdoor structures for nuclear power plants.
2.7 Japan Society for Computational Engineering and Science“Quality Management of Engineering Simulation (2017) 2 ” was prepared by the Japan
Society for Computational Engineering and Science as the guidelines for V&V during theapplication of numerical analysis methods including 3D FEM modeling in the fi eld ofengineering. It defines both the management method of the analysis process and the skill ofanalysts who perform important analyses.
2.8 International Atomic Energy Agency (IAEA )The IAEA Safety Guide (2003) 1 8 indicates that methods of modeling of nuclear power
facilities range from the lumped mass model to 3D FEM model; one of these should beselected to minimize the effect of differences in the methodologies used in the analysis
results. Moreover, it is suggested that, in the issue of soil-structure interaction analysis,modeling methods such as a more detailed 3D FEM model are recommended rather than arigid model with soil springs and the lumped mass model. It mentions the issue of soil structure interaction addressed through the nonlinear 3D FEM model.
2.9 American Society of Civil Engineers (ASCE )ASCE/SEI 4-16 (2017) 1 9 requires 3D FE analysis for seismic examination in some cases.
For example, soil-structure interaction analysis using a 3D FEM model is recommended
instead of a 2D FEM model (3-directional input and response). However, detailed modelingof buildings is regarded as necessary only when considering nonlinearity such as the issue
of uplift.
2.10 The U.S. Nuclear Regulatory Commission (US NRC )NUREG-0800 (2007) 2 0 states that while the 3D FEM model should be used as the
structural model for nuclear power facilities for their seismic response analysis, simpler
models can be used if there is no interaction between vibration directions .

-6-

JAEA-Research 2024-001

3. Basic policy of the guideline
The basic policy for the guideline is as follows.
(1) The guideline summarizes common methods and the way of thinking necessary forseismic response analysis for reactor buildings using 3D FEM model s. The main text
will contain the basic analysis policy, and the commentaries will contain thecorresponding modeling methods, the conceptual basis of each analysis method, andthe technical backgrounds of each analysis method.
(2) The target structures of the guideline are the nuclear reac tor buildings of both the
BWR type and PWR type reactors, and they are applied to the seismic response
analysis of reactor buildings during fragility evaluation.
(3) The appendix of the guideline includes examples of various analyses.

-7-

JAEA-Research 2024-001

II. Main body
1. General information
1.1 Introduction
The guideline summarizes the standard modeling methods and criteria for selecting
analysis techniques in the seismic response analysis of nuclear reactor buildings using a 3D
FEM model.
[Commentary]
The guideline illustrates the outline of standard modeling methods and analysis methods(e.g., analysis conditions, procedures, result evaluation, etc.), as well as their points ofcaution, used for seismic response analysis of reactor buildings using a 3D FEM model toensure that analysts with a certain skill level will obtain result s at the same degree of
accuracy.
It's important to note that when analyzing reactor buildings using 3D FEM models, themodel's scale and numerical calculation complexity increase significantly. This means thatthe choice of calculation method, along with the modeling method for the reactor building
and its surrounding ground, plays a crucial role in determining the accuracy of the solution.
Therefore, the guideline encompasses the calculation methods as well.
1.2 Composition of analysis procedures of the guideline
Following the analysis flow show n in Fig.II-1-1, the standard analysis procedure s at eachstage are presented.

-8-

JAEA-Research 2024-001

1. Analysis purpose/object[Chapter 2]

2. Defining analysis domain[Chapter 3]
3. Setting geometric model[Chapter 4]
4. Setting analysis model
5. Setting numerical analysis

4-1 Structural model[Chapter 5]
4-2 Mass model[Chapter 6]
4-3 Material model[Chapter 7]

4-4 Mathematical modelof damping [Chapter 8]4-5-1 Joint condition

conditions[Chapter 12]
6. Analysis
7. Verifying validity[Chapter 13]
8. Analysis result evaluation[Chapter 14]

model

4-5 Boundary joint model[9.2, 9.3]

[Chapter 9]

4-6 Input seismic motion[Chapter 10]

4-7 Initial state model[Chapter 11]

9. Documentation[Chapter 15]

Fig.II-1-1

Analysis flow

-9-

4-5-2 Boundary modelsof the bottom and theside of the analy sis
ground area [9.4]JAEA-Research 2024-001

1.3 Application scope
The guideline is intended to cover seismic response analysis including seismic safety
evaluations using 3D FEM model analysis of nuclear reactor buildings, as well as simulation
analysis of experiments or seismic observation records, etc.
[Commentary]
The guideline primarily focuses on the reactor building, encompassing its frame structure,
wall structure, dome structure, and various other structural elements, including shield walls
and large equipment. The analysis scope covers seismic safety assessment, simulation
analysis of experimental data and earthquake observation records, as well as seismic response
prediction for the entire structure or its individual components. Additionally, it extends tothe evaluation of fragility for buildings, structures, and equipment in probabilistic risk
analysis (PRA) related to earthquake events.
In the seismic safety evaluation of reactor buildings, the purpose of seismic response
analysis is the calculation of the seismic load, strain, etc. Additionally, the guideline
considers the detailed analysis of responses in deformation, load, strain, etc., through 3D
seismic response analysis. In the guideline, the application scope of the seismic load, strain,etc., is from elasticity to around weak nonlinearity. However, it is possible to consider thematerial nonlinearity of buildings or nonlinearity of soil -structure interaction using joint
elements.
An advantage of 3D FEM modeling of reactor buildings is that it is possible to perform
superimposition of generated stresses and strains under different loads with high accuracy
using the same model, even under different load conditions. Note that the guideline assumes
seismic motion as the external force and do not consider extraordinary temperature, external
impact force, etc. However, they do consider normal loads such as the dead load, live load,and ordinary temperature load. Furthermore, detailed parts, such as non -structural parts,
equipment, piping, welded parts, and joints, are also not considered.
1.4 Main terminologies
The symbols and terminologies used in the guideline are explained below.
[Commentary]
1.4.1 SymbolE𝜎𝜎dYoung’s modulus
Stress
Displacementv

Velocity

Vs

Shear wave velocity- 10 -

JAEA-Research 2024-001

a
𝜌𝜌
𝛾𝛾
𝜀𝜀
ν (nu)

Acceleration
Mass density
Shear strain
Strain vector/tensor
Poisson’s ratio

1.4.2 Terminology
3D CAD software

CAD software used in the production of 3D models of structures
Many of these also function as BIM software.

3D FEM model

3D model of finite element method

3D FEM model analysis Analysis that uses a 3D model of the finite element method
Adhesion

Indicates the tensile strength between the bottom of the structure
basemat and the supporting ground.

Analysis model

It indicates everything in the finite element analysis including thegeometric model, structural model (mesh model), constitutive law,and boundary condition including external force.

Analysis model center

Position of the neutral line of the beam cross section in beam theory,or the neutral plane in the shell theory.

Analysis object

Buildings and soils whose response to be obtained through seismic
response analysis.

Bar element

Line element that has freedom in tension, compression, and torsion

Basemat uplift

Separation of basemat that detaches from the ground and is uplifted
because of an earthquake, etc.

Beam element

Most universally applicable line element with freedom in tension,
compression, twisting, and bending .

Building/Structure

General term for structures such as reactor buildings and structures
such as exhaust towers among nuclear reactor facilities

Consistent mass matrix It is a mass matrix used in the finite element method, and values are
assignedtooff-diagonalterms.

Itisoccasionally

used

in

conjunction with the lumped mass matrix. Therefore, it is known as
the consistent mass matrix.
Constitutive law

It mathematically describes the mechanical properties of a substancethat is in continuum and is one of the fundamental equations of acontinuum. It is commonly expressed as a relational expression ofstress and strain.

Contact ratio

Ratio of the area of the bottom of the basemat that is in contact withthe ground in relation to the entirety of the bottom of the basemat.

Dynamic analysis

A type of analysis that identifies changes in the response ofstructures through solving equations of motion. In the guideline, it- 11 -

JAEA-Research 2024-001

is used in the same sense as seismic response analysis.
Dynamic deformation characteristic
Relationship between secant shear stiffness G v.s. shear strain 𝛾𝛾
and damping h v.s. shear strain 𝛾𝛾. It is obtained through the dynamic

deformation test of soil specimen.

Earthquake-resistant wall, load -bearing wall

Walls that can bear seismic force. In the “AIJ Standard for Structural
Calculation of Reinforced Concrete Structures for Nuclear Power
Facilities” 1 4 by the Architectural Institute of Japan, the term
earthquake-resistant wall is used, and the term load-bearing wall isused in the Building Standards Act.
Effective strain

Strain for setting the equivalent stiffness to obtain the effective
response of the main vibration in equivalent linearization analysis;
it is the maximum strain multiplied by the coefficient values from
0.6 to 0.7.

Element integration point
Also known as the Gauss point, it is a point for element integrity
when guiding the stiffness matrix, etc., of finite elements. Normally,
it is used as the evaluation point of stress and strain among finite
elements.
Equipment/piping system
General terms for vessels, piping, pumps, electric instruments, etc.,
as well as their supporting structures, in nuclear reactor facilities.
Equivalent linearization analysis
A type of analysis of nonlinear problems through linear analysis
using secant stiffness (equivalent stiffness) in relation to theeffective strain.
Evaluation guide“Inspection Guide for Certification of Earthquake -resistant Design
Construction” (2013) 4 , published by the Nuclear Regulation
Authority of Japan

Finite element model

A model that sets mass, material, boundary conditions, damping, andinitial conditions as its finite element mesh. (In the guideline, it isused in the same sense as the structural m odel.)Finite element type

Types of finite element mesh. For instance, there are bar elements,
beam elements, shell elements, and solid elements such as
tetrahedral

elements,

elements.

- 12 -

pentahedron

elements,andhexahedron

JAEA-Research 2024-001

Floor response spectrum
Response spectrum at a floor position during an earthquake, and it
is used for designing equipment installed on the floor. Floor
response spectrum (FRS) is also known as in -structure response
spectrum (ISRS).
Fragility evaluation

Using the realistic response and realistic yield strength ofbuildings/equipment to probabilistically obtain conditioned damage
probability.

Geometric model

Geometric data consisting of line parts, plane parts, and solid parts(also known as geometry data).

Gravitational acceleration
9.80665 m/s 2 is the SI standard.
Hour glass mode

State (mode) in the finite element method where strain is zero
although there is deformation. It is a mathematically stable state that
does not occur physically. It is also known as the zero-energy mode .
It occurs in elements that use a reduced integral. It is known as thehourglass mode as the shape of deformation is hour glass shaped.

Induced vertical motion
Vertical response of a structure induced when the horizontal
response of the structure become s large and an uplift of the basemat
occurs.
Joint element

Element that models contact, separation, and sliding of twomaterials of different shapes. It was used for the first time byGoodman et al. 2 1 , for their analysis of the natural behavior of
bedrock. In the guideline, this element indicates the finite elementsthat modeled the behavior of the exterior walls of the undergroundparts of the structure or between the bottom of the basemat slabs andthe ground.

Linear analysis

Analysis where the relationship between displacement and force is
proportional. Here, it indicates analysis of material under thecondition without side separation and sliding and without uplift.

Line element

Element of a geometric model that is represented by lines .

Lumped mass matrix

Mass matrix where only diagonal terms are assigned value. There
are several methods to set it. If the finite element is a primaryelement, this is the method to obtain it from the gove rning volumeof the node. Further, there are other methods such as obtaining it bydiagonalizing the consistent mass matrix. Therefore, it is known as
the lumped mass matrix.

- 13 -

JAEA-Research 2024-001

Mesh model

Model consisting of finite elements.

Modeling factors

Factors in 3D-FEM model analysis that influence the analysis result .
It includes the analysis method containing the analysis theory thatis its basis, the analysis condition, and constitutive law.

Nonlinear analysis

A type of analysis that takes nonlinearity into accoun t.

Nonlinearity

A term that includes material nonlinearity (elasto -plasticity),geometric nonlinearity (formulation of the case where deformationis large in relation to the scale of the structure), and boundary
nonlinearity (separation/sliding of side, up lift of the bottom of thebasemat).

Non-structural members
Members that are not expected to bear stress, such as partitions andceilings.
One-dimensional wave theory
Wave theory that limits propagation direction to the verticaldirection 2 2 .
Peer check

Check by a specialist of a third-party. The purpose of it is the sameas the structural calculation legality evaluation in the BuildingStandards Act.

Performance verification
Action tojudge whether a structure satisfies

the required

performance by comparing it to reference data and documents.
Plane element

Element of a geometric model represented by planes .

Pressure bulb

Curve created by connecting points with equal vertical stress that
occur in the ground toward the depth direction.

Probabilistic risk assessment
Quantitative evaluation of the probability of occurrence of
undesirable phenomena such as accidents and the extent of damage
caused by them.
Pullback wave

Input seismic motion used for dynamic analysis . A type of seismic
motion that was pulled down or pulled up to the seismic motions
defined on the free rock surface, such as the basic earthquake groundmotion, to the bottom end of the analysis model, based on one dimensional wave theory, to take the grou nd structure within the site
into account.

Response

Acceleration, velocity, displacement, stress (stress intensity), strain,etc., of the analysis result obtained from disturbance.

Response spectrum

The maximum responses of a one-lumped mass model with several- 14 -

JAEA-Research 2024-001

naturalfrequencies

that

receive

the

same

input

earthquake

connected by the frequency axis.
Secondary member

Members placed for purposes such as transmitting force to the main
frame that do not bear vertical force and seismic force. They include
members such as joists and studs and are normally not considered tobe earthquake-resistant members.

Seismic force

Inertia force applied on an object by seismic motion . In earthquake
resistant design, it indicates the inertia force applied on structures.
It includes dynamic seismic force and static seismic force.

Seismic response analysis
Time history response analysis of seismic motion
Separation

Separation between the surface of exterior walls of the undergroundparts of a structure and the ground

Shell element

Finite element that can represent in -plane deformation and out-ofplane bending deformation of curved surface .

Sliding

The guideline refer to the sliding on the surface where the structureand ground come into contact and include the sliding on the side andat the bottom of a structure.

Solid element

Solid elements for the finite element method .

Solid shapeThree-dimensional geometric data produced with 3D CAD .

Solid shape element

A type of element for a geometric model with three -dimensional
shapes such as rectangular parallelepiped, cylinder, and cone.

Static analysis

A type of analysis for obtaining displacement, deformation, stress,
strain, etc., on a structure in relation to load or displacement thatis not dependent on time. It is used for the analysis of permanentloads such as the dead load.

StressForce applied to unit area. In th e guideline, it is used in the same
sense as stress intensity.

Stress–strain relationship
Relationship between stress and strain when loading and unloading
are repeated.
Structural damage

Damage to structural members such as cracks in reinforced concreteand buckling of steel frames.

Structural model

A model where the mass, material, boundary condition, damping,and initial condition is set in a finite element mesh .

Structure

Same as architectural structure. “Reactor building” is referred to as
structure.

Sub-shear wall

Walls with thickness over 30 cm other than earthquake-resistant- 15 -

JAEA-Research 2024-001

walls (shear wall), that also resist seismic force.
Time history response analysis
Response analysis that obtains response at each moment using time
history wave as its input. There is a method to analyze in the time
domain and a method to analyze in the frequency domain.
Transmission frequency
Maximum frequency to be considered in the seismic response
analysis of soil-structure interaction.
1.4.3 Abbreviation
BIM

Building Information Modeling

CAD

Computer Aided Design

FEM

Finite Element Method

FRS

Floor Response Spectrum

JEAG

Japan Electric Association Guide

KARISMA

Kashiwazaki-Kariwa

Research

Initiativefor

Seismic

MarginAssessment
NAFEMS

National Agency for Finite Elemen t Methods and Standards. The
International Association for the Engineering modelling, Analysis
and Simulation Community

PRA

Probabilistic Risk Assessment

SSI

Soil–Structure Interaction

V&V

Verification and Validation- 16 -

JAEA-Research 2024-001

2. Purpose and object of analysis
2.1 Introduction
In seismic response analysis of nuclear reactor buildings using a 3D FEM model, it isessential to first define the analysis objectives and scope, and then select appropriate
analysis conditions, methods, and result evaluation procedure s in accordance with thoseobjectives.
[Commentary]
For the seismic response analysis of reactor buildings using the 3D FEM model, it isnecessary to clearly define the analysis object. For this reason, the analysis purpose should
be clarified at the beginning of the analysis process, and the analysis object and its scope are
set according to this purpose.
Note that the basic principle of the guideline can be also applied to the seismic response
analysis of structures in nuclear power plants other than reactor buildings.
2.2 Analysis purpose
Clearly define the objectives and scope of seismic response analysis using a 3D FEM
model.
[Commentary]
The purposes of seismic response analysis encompass several objectives, including
understanding the effects of earthquakes on structures, the nonlinear behavior of materials,
the impact of embedment, and the potential for local damage to structural components.
Specifically, the analysis serves the following purposes and focuses on the following objects:(1) Verification of the performance of structural components within reactor buildings
during seismic safety evaluations(2) Calculation of responses for individual portions of structures to serve as seismic input
for piping and equipment systems(3) Simulation analysis of records from observations of reactor buildings, thesurrounding ground, and other relevant areas(4) Preliminary analysis and simulation of model experimen ts on various structuralelements(5) Evaluation of the fragility of structural components within reactor buildings(6) Assessment of structural responses to evaluate the fragility of piping and equipment
Prepare an appropriate analysis plan for each analysis purpose using the right analysis
method, analysis conditions, and evaluation method for the analysis results. For making thisplan, it is necessary to take the s ize of the analysis model, calculation t ime, analysis- 17 -

JAEA-Research 2024-001

capability, etc., into account. Whether the prepared analysis model is suitable for the analysis
purpose must be properly examined by those who planned the analysis, those who conducted
it, the users, and the reviewers.
Notably, when the abovementioned fragility evaluation is the purpose of analysis, theresponse of each member is expected to be highly nonlinear; therefore, appropriate modelingand analysis methods will be required for the corresponding nonlinear regions.

- 18 -

JAEA-Research 2024-001

2.3 Analysis method
Depending on the analysis objectives, select the appropriate analysis method. The
chosen analysis method should be validated through either similar analyses, thesimulation analysis of experiments or seismic observation records, etc.
[Commentary]
There are a variety of seismic response analysis methods, including the time integration
method, the finite element method, and the material nonlinearity. Select an analysis methodthat appropriately combines these and analysis software with reasonable usage. If selecting
other analysis methods and analysis software, the validity of such methods must be
demonstrated through analyses that verify the same through comparison with similar
problems or simulation analyses of experiment/earthqua ke observation records.
Note that the methods to demonstrate the validity of analysis software include the analysis
of benchmark problems provided by trusted organizations such as scientific societies or
NAFEMS 2 3 , in addition to the simulation analyses of experiments and earthquake
observations.
The time integration method for seismic response analysis includes the direct time
integration method and the frequency response analysis method. In the linear analysis of
lumped mass system models, the frequency re sponse analysis method is capable of doing acalculation using hysteresis damping (complex damping); however, it has issues including
not being capable of conducting an elasto-plastic analysis following hyster ic behavior.
For finite elements, there is the option to model earthquake -resistant walls with shellelements or solid elements.
If the nonlinearity of materials needs to be considered, select an appropriate constitutive
law for each material and use reliable analysis software. On this subject, “ Codes for Nuclear
Power Generation Facilities – Rules on Design and Construction for Nuclear Power Plant:
Alternative Design for Seismic Design of Seismic S Class Steel Piping Based on Elastic Plastic Response Analysis 1 3 ” by the Japan Society of Mechanical Engineers, one of thestandards for nuclear energy facility standards, stipulates the analysis methods and analysis
software. The analysis method indicates the modeling method of analysis. For the analysis
software, Abaqus, Ansys, FINAS, FINAS/STAR, MSC Marc, and their versions aredesignated. Moreover, the guideline state s that other analysis softwares can be used as longas benchmark analyses in SEGP are conducted.
For the KARISMA benchmark project, N astran, Abaqus, Ansys, SAP2000/SUPER,
CAST3M, and COSMOS/M were used.
ASCE/SEI 4-16 1 9 presents LS-DYNA, Abaqus, and Ansys as commercial analysis- 19 -

JAEA-Research 2024-001

software; the NRC ESSI Simulator i as licensed software; and O penSees and Mastodon as
open-source software for nonlinear analysis of ground.
2.4 Unit used
In 3D FEM model analysis, SI units are used. It is important to ensure the consistency of
the units used in input data combinations.
[Commentary]
SI units are used as the units in analysis model, material constants, etc. (Table II-2-1).
Moreover, one must pay attention to the consistency of the combination of all input data. Be
aware that units used in the list of report of analysis conditions could differ from the unit
system used in the analysis data for representing material constants, and this can easily cause
mistakes.

Table II-2-1 Combinations of SI units used in seismic response analysis
SI unit (System 1)

SI unit (System 2)

m

m

Mass

kg

Mg (t (ton))

Velocitym/s

m/s

Acceleration

m/s 2

m/s 2

Force

N (kg・ m/s 2 )kNStressPa (N/m 2 )kPa (kN/m 2 )

Time

s

s

Length (Coordinate,
Displacement)

Note: t (ton) is officially used together with SI units. This is also the case with Mg.
Gal (cm/s 2 ) is a non-SI unit in the CGS units, and it is not officially used.
In material property lists and others, N/mm 2 is used for material strength and kN/m 3 is used forweight density. These must occasionally be converted when entering data into some analysis
software and unit systems. Be aware that this can easily cause mistakes .

2.5 Analysis plan
Create a specific analysis plan in accordance with the analysis objectives.
[Commentary]
When conducting an analysis, confirm the application scope of the analysis method,i Programs, manuals, exercises, and post -processing tools are published in the website ofReal ESSI Simulator (http://www.real -essi.us).

- 20 -

JAEA-Research 2024-001

examine the guarantee of the analysis result validity, and prepare an analysis plan. Further,
prepare an analysis plan for how to improve analysis models in which the validity is
insufficient.
Prepare an analysis plan that is sufficiently accurate, where calculation can be conductedfrom 2 to 8 shown in the analysis flow (Fig.II-1-1).
Analysis planning is an important process for quality control in analysis. Make a plan toselect and set the analysis method for analysis evaluation, and conduct analysis according tothis plan. Specifically, clarify the selection of the governing equation, model form, finite
element, and material model (constitutive law) for the analysis method appropriate for the
analysis purpose, analysis object, and phenomenon to be analyzed. Further, if material
nonlinearity is to be considered, select an appropriate constitutive law and demonstrate its
validity.
Preparation of an appropriate analysis plan is an important step for V&V. Here, it isdesirable that factors relevant to the abovementioned analysis purpose, analysis object,modeling method, and analysis method are documented in text, and its content is verified by
all personnel involved in the analysis, including the person who planned the analysis, theone who conducted the analysis, users, and reviewers (analysis evaluator s). The person who
conducted the analysis must present the basis for the background of the analysis plan in theanalysis report.

- 21 -

JAEA-Research 2024-001

3. Analysis domain
3.1 Introduction
Consider the analysis objectives and scope to appropriately set the level of detail forthe building model and define the analysis domain.
[Commentary]
Set the level of detail of the structure model and its constituent members to be analyzed,
as well as the analysis domain of its surrounding ground. Ensure that difference in analy sis
domain should not influence the analysis result.
3.2 Level of detail of building structural model
Consider the analysis objectives and appropriately define the modeling extent ofbuilding components (level of detail of the building structural model) within the building
structure.
[Commentary]
Set the scope for constituent elements, such as basemat/columns, floors/walls/roof,
secondary members, heavy equipment, and facilities, that can potentially influence theanalysis result as the level of detail of the modeling of the constituent members of thestructure. Components that can influence the seismic response include the pressure vessel
and its related components, cranes, secondary walls other than the earthquake -resistant walls,
joist, small openings, roof slabs, shielding walls, and stairs.
Consider the installation positions of equipment and their supporting points whenobtaining the floor response to piping and equipment. Moreover, regarding vertical motion,
take the width of the floor (depe ndent on the positions of the walls in the floor below) andthe influence of the support members into account when modeling.
In 3D FEM model analysis, a more detailed response can be obtained when modeling ismore detailed (e.g., local floor response, in-plane deformation of floor, out-of-plane
deformation of floor and wall, building torsion, members response). However, because
analysis requires significant amount of resources, it is necessary to be efficient in modeling(preparing an analysis model that can be calculated) for each purpose. Be aware that theanalysis method and the level of detail for the analysis model may differ depending on the
purpose of analysis.
When obtaining the seismic force applied on a structure, 3D -FEM model analysis may bebased on a model that only considers the main structural members. However, for simulation
analysis of observation records or calculation of input seismic motion to piping/equipment,
it is necessary to take the difference depending on the positions in the structure into account;- 22 -

JAEA-Research 2024-001

it is possible that more detailed modeling may be required.
Further, when evaluating damage of structure members, it is necessary to appropriately
model in detail the parts where damage is expected and the parts where stress may
concentrate.
3.2.1 Modeling range of constituent members of structure
In principle, constituent members are modeled according to the plan that matches theanalysis object. However, modeling structural members exactly as they are shown in the plan
could be difficult; therefore, simplification rules for modeling (of the parts that do not affectthe analysis result that satisfies the analysis purpose) must be set. For instance, the omissionof factors that have a minimal effect on the analysis purpose, such as level differences on
the floor, drainage slope, and small openings, can be considered if the reasoning for doing
so can be justified. Moreover, non-structural components such as stairs, bay windows,
balconies, parapets, and additionally placed concrete portions are often omitted in modelingas they do not influence the analysis result. However, it may not be possible to ignore themwhen considering local vibrations.
Therefore, the inspection guide 4 requires setting of members that influence verticalresponse for vertical analysis models of buildings/structures.

Therefore, it is also necessary

to consider the influence of secondary walls and weight distribution on the floor on thevertical vibration of the floor for 3D FEM models. Conduct modeling of secondar y walls andeach equipment, and detailed modeling of weight, etc., if necessary.
Furthermore, in 3D FEM models of reactor buildings, it is sometimes necessary to perform
modeling that includes walls other than earthquake -resistant walls for seismic respons e
analysis. For instance, in the simulation analysis of the observation record (horizontal
direction) from the Kashiwazaki-Kariwa Nuclear Power Plant building during the 2007
Chuetsu offshore earthquake, walls thinner than earthquake -resistant walls were modeled as
supporting walls. By obtaining the response spectrum through usage of the actual stiffness(real stiffness), better agreement between the analysis result and the observation result isachieved 2 4 , 2 5 (Table II-3-1 and See Fig.II-3-1). Though a sufficient result to the verticalresponse was not obtained in this example, the possibility that there are issues in the accuracyof the wall layout and weight distribution has been suggested.

- 23 -

JAEA-Research 2024-001

Table II-3-1 Selection conditions of the walls considered in the simulation analysis of the
Niigataken Chuetsu-oki Earthquake in 2007 2 4
Seismic wall

Auxiliary wall

The thickness of the wall must be 300 mm

Same as details provided in the left side.

or more, and 1/30 or more of the door frame
reveal height.
Shear reinforcement ratio of a wall is 0.6%

Shear reinforcement ratio of a wall is 0.25%

or more for each orthogonally intersecting

or more for each orthogonally intersecting

direction.

direction.

A wall that continuously rises from the

A wall that is continuing to the floor below

basemat slabs.

or a wall that can transmit the shear force
occurring in it via floor slabs to theearthquake-resistant wall of the floor below.

A

wall

insideframe

structure(between columns or beams)

plane

A wall that satisfies the above even if it isoutside the frame structure plane

Seismic wall
Auxiliary wall

Fig.II-3-1 Examples of seismic walls and auxiliary walls 2 4(Left: NS direction, Right: EW direction)
Modeling of roof: Roof truss and roof slabs must be modeled to consider the in -plane/outof-plane deformations of the roof floor. For roof truss, th e main members, diagonal members,
bundled members, etc., are modeled. Perform modeling that is appropriate to each situation
for roof slabs and roof trusses by taking the influence of mode shape into account.
Modeling scopes of secondary members: Consider a model that is closer to reality if not- 24 -

JAEA-Research 2024-001

modeling non-structural walls and joists results in a longer span that supports the floor,
which may result in the coupling of the vertical natural frequency that corresponds to thevertical stiffness of the floor, and the vertical natural frequency of the structure.
Modeling scope of large equipment: Determine the modeling scope of large equipment
such as the pressure vessel and its support structure by considering their influence on thevibration characteristics of the building. The possibility that it can affect vertical vibrationand deformation of basemat slabs has been suggested.
In-plane shear deformation occurring in wall and floor due to horizontal vibration isresisted mostly by the exterior walls, and the in-plane displacement at each floor slab is kept
small by the in-plane stiffness of the floor.
During vertical vibration, for each reference line, exterior walls and main columns areconstrained by adjacent walls, and the whole building vibrates as though it is a single rod.
Note that if a wall is not connected vertically from the upper floors to lower floors, thedifference of displacement at each column position becomes larger.
In Annex 3 of Appendix 1, one can observe how the vertical response s of the exterior andinterior walls, which located inward from the exterior walls, are different. The interior wallsin the analysis model ha ve much fewer walls at the lower part of the building than that ofexterior walls and supported by columns. For this reason, the vertical stiffness of the exterior
walls and that of the interior walls are different. Moreover, while the earthquake observation
instrument is located on the reference line of interior walls, its vertical response is closer tothat of the exterior walls in the analysis. These facts suggest that in reality, the vertical
stiffness of the interior walls is in unison with that of the exterior walls; therefore, it issuggested that the scope of the analysis model was insufficie nt.
3.2.2 Examples of selecting the scope of the analysis object according to analysis purpose
The following are the examples of selecting analysis object scopes that correspond with (1)to (6) in section 2.2.
(1) For performance verification of structural members of the reactor building in seismic
safety evaluation, set the modeling scope according to the importance of members.
(2) For floor response calculation, which will be used as the input to piping, equipment, et c.,model the relevant members while taking the equipment/piping system into consideration.
For instance, in addition to equipment, it is necessary to model the parts where
equipment/piping systems couple or interfere with the building, such as support
structures, diaphragm, stabilizer, and shear lag, to obtain the responses related topressure vessel. Moreover, when focusing on equipment to be installed on the floor, thefloor and the walls of the floor below, which support the equipment, also must be
considered. Their modeling may influence the vertical response of the building.
(3) For the simulation analysis of the observation record, model the position of the- 25 -

JAEA-Research 2024-001

seismometer, members that may affect the vibration characteristics of the analysis object,
and the surrounding ground.
(4) For pre-analysis and simulation analysis of the model experiment, model the membersthat may influence the experiment result.
(5) For fragility evaluation of a structure against seismic motion, it is inferred that a rationalmodel that takes damage modes into account is necessary as analysis of many cases is tobe performed. Moreover, because it requires strong nonlinear analysis tha t takes material
nonlinearity into account, the application scope (capability) of analysis software also
must be considered. Furthermore, the un certainty of the ground, the soil-structureinteraction, and building characteristics (e.g., stiffness, damping, various nonlinearities)
must be modeled appropriately.
(6) For the structural response to be used for fragility evaluation of piping/equipment,
modeling must consider the position/stiffness/mass of the piping/equipment in addition
to the above.
3.3 Analysis domain of the surrounding ground
Depending on the analysis objectives, define the analysis domain appropriately,
including the surrounding ground and buildings/structures, etc.
[Commentary]
For the seismic response analysis of a structure, set an analysis area that can take soilstructure interaction into account. Moreover, if they can potentially affect the response,neighboring structures and their surrounding grounds must be included in the scope of theanalysis object.
The analysis area of the ground must, based on the strata type and characteristics , be set
within the region where its influence on the response result of the analysis object structure
is sufficiently small.
Note that in addition to the one -dimensional wave propagation within the ground, it isdesirable to set the ground analysis area that takes the underground stress distribution (strain
distribution), etc., into account so that the 1st mode of soil–structure interaction (horizontal
and vertical) within the support ground should be included.
Furthermore, if the free rock or ground surface is inclined or irregular, this must be
examined in advance to the modeling of the ground to consider its effect.
3.3.1 Object scope of ground analysis area in horizontal direction
According to JEAG4601-1987 2 6 , the horizontal length of the ground of the analysis areais the length that includes the wavelength 𝜆𝜆 = 𝑉𝑉𝑠𝑠 ⁄𝑓𝑓𝐿𝐿 being studied and is not dependent on

the structure width if a viscous boundary is being used. (Here, 𝑉𝑉𝑠𝑠 : Shear wave velocity of- 26 -

JAEA-Research 2024-001

the ground, 𝑓𝑓𝐿𝐿 : Minimum frequency of the analysis.) For instance, if the frequency for theexamination is set at 1 Hz, the length of the side boundary for the analysis becomes 500 m
at the ground where the shear wave velocity is 500 m/s. If the structure width B is about 80
m, it is approximately 6 B.
If the ground displays elasto-plastic behavior and the radiation waves due to the structure
vibration dissipate within a short distance, it could result in a narrow area.
3.3.2 Object scope of ground analysis area in depth-direction
If the bottom of the analysis area is set as viscous boundary and an incident wave is being
entered, the depth must be set at a level where the influence of the vibration of the structureon the bottom of analysis area is sufficiently small.
If the free rock surface is sufficiently deeper than the basemat of the structure, set thedepth of the analysis area at the free rock surface. If it is shallower than the basemat of thestructure, determine the depth of the analysis area by considering the influence of thedominant frequency of the sup porting ground and the dissipation of structural vibration into
the ground. It is sometimes necessary to set the bottom of the analysis model in the middleof the basemat and the free rock surface.
According to JEAG4601-1987 2 6 , it is set at the depth until the bottom of the analysis areaof the ground, 𝐻𝐻 = 𝑉𝑉𝑠𝑠 ⁄(𝑎𝑎 ∙ 𝑓𝑓𝐿𝐿 ); if it is a viscous boundary, it is 1/10 of wavelength ( a = 10),and if it is a fixed boundary, it is 1/2 of wavelength ( a = 2). When securing accuracy at Vs =500 m/s ground and within a frequ ency region that is 1 Hz or more, H = 50 m if it is a viscousboundary.
Meanwhile, if the vibration character due to the building basemat vibration is to beconsidered, it is desirable also to take the influence range of the vertical stress within the
ground into account. Considering a range in which the pressure bulb at the supporting groundof a square basemat is 1/10 of support pressure, it is inferred that a height that is about
double the width of the basemat of the structure will be necessary.
Note that NUREG/CR-7230 2 7 demonstrates that when the supporting ground is extremely
hard, a structure placed on the ground whose Vs is 2438 m/s (8000 ft/s) or more can be
regarded as a fixed basemat model. In addition, NUREG/CR -6896 2 8 and ASCE SE 4-16 1 9 are
also useful to refer to.
3.4 Neighboring structure included in the scope of the analysis object
If the analysis object building and its neighboring structure are nearly equal to each other(either same level of mass or approximate natural frequencies) and if the ground is relatively
soft, the neighboring structure is expected to have a large influence on the analysis object
structure, and it is desirable to include it in the scope of the analysis object.

- 27 -

JAEA-Research 2024-001

Fig.II-3-2 shows the diagram of the structure and the surrounding ground .

Fig.II-3-2 Diagram of the structure and the surrounding ground- 28 -

JAEA-Research 2024-001

4. Creation of the geometric model
4.1 Introduction
Create a geometric model appropriately according to the analysis objectives.
[Commentary]
In a finite element analysis, it is necessary to prepare the geometric shapes of thestructure/ground to be analyzed using finite element meshes. To achieve this, geometricmodel data is first prepared using 3D CAD software and then structural model data (FEM
analysis data) is produced based on this. Here, geometric model data indicates geometricdata (geometry data) consisting of line parts, plane parts, and solid parts, and structuralmodel data indicates a type of model data where mass, material, boundary con ditions,
damping, input seismic motion, initial conditions, etc., are added to the finite element meshdata produced from this geometric data.
Creation of geometric model data refers to preparing a three -dimensional model on acomputer. Commonly, geometric model data is produced with 3D CAD software or FEM pre software and consists of columns, beams, floors, walls, etc., with line parts, planer parts, andthree-dimensional parts (e.g., rectangular parallelepipeds, cylinders , and cones). Data
formats such as ACIS, Parasolid, STEP, dwg, and IGES are used to convert these data.
Conventionally, finite element mesh data was sometimes produced directly without
producing geometric model data. However, the creation of complex models required vast
amounts of labor, and it was difficult to add/change shapes or to verify the correctness ofthe models. Therefore, the method of preparing geometric model data through 3D CAD andbuilding information modeling (BIM) first and then generating finite element mesh data
based on it is becoming more common.
Creating structural model data from the geometric model data prepared through 3D CAD
data has become common in the analysis of mechanical systems. Architectural systems areexperiencing the same trend with the development of BIM software.
4.2 Creation of a geometric structural model
Construct a geometric model of the building, taking into account their construction
methods and relying on the reference documents that specify their shapes and materials.
[Commentary]Prepare a geometric model for each structural member based on the structure plan. Set anappropriate modeling rule according to the finite elements used in the modeling and member
material types (e.g., reinforced material, steel frame, steel reinforced con crete, etc.) andperform modeling of structural members according to the rule.

- 29 -

JAEA-Research 2024-001

For instance, when verifying the performance of an existing structure during an earthquake,check if the geometric model matches the drawing and the actual structure through an onsite study (plant walkdown) when necessary. Moreover, when performing a seismic response
analysis for seismic safety verification following a large earthquake, the damage level of thestructure, such as cracks, is occasionally investigated in detail in addition to the observation
record to reflect it on the geometric model.
Because it is difficult to create a geometric model that is exactly like the drawing (i.e.,
exactly like the real building), misalignment of columns/beams/walls from the center line,
inclination, floors with different levels, etc., can be simplified if it is possible to demonstratethat such simplification will have little impact on the analysis result.
Although 3D FEM models are often regarded as equivalent to real structures, it is d ifficult
to reproduce a real structure perfectly in a geometric model, and some degree ofsimplification is inevitable. One must conduct modeling in such a way as to ensure thissimplification does not affect the response of the analysis object, and theref ore, anappropriate modeling rule is necessary.
There are different methods of creating geometric models, depending on the type ofstructural model to be produced. Two examples are discussed below.
• When a beam/shell element model is used for the structur al model (beam/shell structuralmodel)• When a solid element model is used for the structural model (solid structural model)
When using a solid structural model, creation of the geometric model involves modelingof structural components with solid shapes such as cubes, cylinders, and spheres using 3D
CAD software. When using a beam/shell structural model, model the columns and beams inlinear shape with section information and model the floors and walls in planer shape withthickness information using pre - or post-processing coordinated with the finite element mesh,and attach these section information as attribute data. In either case, the analysis must selectthe structural model creation method at the point of starting to prepare the geometric model.
When using 3D-FEM model analysis for stress analysis in cross-sectional design, abeam/shell structural model, which enables one to obtain the stress resultants of members
directly, is commonly used.
Fig.II-4-1 shows the difference between geometric models and structural models- 30 -

JAEA-Research 2024-001

Geometric model

Structural model(Finite element mesh)

Beam/shell structural model

Solid structural model

Fig.II-4-1 Examples of creating geometric and structural models 2 9

When creating a structural model with beam/shell elements, the geometric model consistsof preparing planes with the roughest mesh model. The structural model generates meshes
by subdividing it into appropriate sizes.
When creating a structural model with solid elements , columns, beams, floors, walls, etc.,
are modeled with rectangular parallelepipeds, and shell walls are modeled with cylinders,etc., which are then divided into meshes.
4.2.1 Example of modeling with beam/shell elements
When modeling a structural model with beam/shell elements, an appropriate modeling rule
must be set for each member and modeling be performed according to this rule.
For instance, the setting of the analysis model center of columns, beams, floors, and walls
must match at the end of columns; the setting of the height of the analysis model centers ofbeams and floors must match at the floor surface of each level; and the setting of the analysis
model centers of columns and beams must match in the plan. In this case, there will be
misalignment between the component centers and analysis model centers, and it will benecessary to consider the regions of joints within, for instance, a rigid zone, to model
accurately.
Examples of creating geometric models of representative members and sections are shown
below.

- 31 -

JAEA-Research 2024-001• Reinforced concrete column/beam
The height of the beam center is set at the height of the upper surface of each reference
floor, the column center is set at the base line position, and the end of the beam is connectedto the column center. The analysis model center of the beam in the plane direction is alignedwith the reference line. If this is significantly misaligned with the column center, set anappropriate node for joining the beam.
• Steel reinforced concrete colu mn/beam
The positions of the column and beam, as well as their analysis model cores, are the sameas those of reinforced concrete members. As the steel frame and reinforced concrete part
have different elastic constants, one can either model them as a beam element synthesizing
the two or model them individually and then share the node.
• Reinforced concrete wall
The position of a reinforced concrete wall is, in principle, the center of the wall in the
thickness direction. However, if this is misaligned with the analysis model center of a beam
or a column, it is often adjusted to the beam center or the column center. Moreover, forexterior walls, it is occasionally aligned to the exterior wall surface.
A wall with a long span, such as the upper wall of the operation floor (OF), must undergo
high-precision mesh division against out-of-plane vibration.
• Reinforced concrete floor
It is modeled at the position of the analysis model core of the beam that is to be joined. If
there is a large difference of level, its effect must be taken into account. Commonly, a frame
structure building is modeled with beam cores. However, the modeling of a nuclear power
facility is often conducted with the height of reference floor .
• Steel beam
Model it in the same way as a reinforced concrete beam and set appropriate cross section
information as attribute data. When modeling steel beams, take their joints with steel
columns and steel reinforced concrete columns into account.
• Steel truss
The steel truss of a reactor building is modeled with the intersection of member centers as
the node. However, because of its large beam height, gaps may occur between the roof slabs
and the steel truss. This must be considered in relation to th e analysis purpose, for instance,
by offsetting the misalignment between the analysis model centers of the roof slabs and thoseof the upper chord members of the steel truss.

- 32 -

JAEA-Research 2024-001• Roof slab
Model the joints with roof trusses appropriately as the roof is thin and, therefore, out-ofplane deformation can easily occur. This modeling can influence the dominant natural
frequencies of the structure. In the first mode of the analysis model of Fig.II-4-2, the verticaldeformation of the roof and the out -of-plane deformation of the exterior walls that support
it are coupled, and when an exterior wall is warping outward, the roof is warping inwar d.
The vertical deformation of the roofslabs supported by the truss influences
the deformation of the roof truss,
which in turn interferes with thedeformation

of

the

structurethat

supports

resulting

in

the

roof

peripheral
thetruss,

warping

downward when the exterior walls are
warping outward.

Fig.II-4-2 Coupling of the vertical deformation of the roof and the horizontal deformationof the structure 2 9• Pool water
Pool water is generally modeled as an additional mass and considered when creating a
structural model.
• Pressure vessel and its support
Regarding the pressure vessel and its support, it is desirable to create a simplified modelusing beam and shell elements and consider them as a structural model. When only its mass
is considered and when it is supported by the surrounding members, ensure that it does notaffect the analysis purpose when preparing the structural model.
4.2.2 Example of rule for modeling with solid elements
When modeling a structural model with solid elements, ensure that the boundaries ofmember joints are modeled accordin g to certain rules.
• Reinforced concrete column/beam/floor/wall/roof
Columns, beams, floors, and walls made of reinforced concrete are modeled with solid
shapes (e.g., rectangular parallelepipeds, cylinders, etc.) . For instance, columns and walls
are divided into each level by the upper side of the floor surface, girders are divided by the- 33 -

JAEA-Research 2024-001

column surface, joists are divided by the girder surface, floors are divided by the surfaces ofcolumns and beams, and walls are divided by column surfaces and beam bot tom surfaces.
These are then modeled with solid shapes such as cubes. Fig.II -4-3 shows the diagram of ageometric model consisting of solid elements.

Columns are divided
by upper surfaces ofthe floor.

Beams are divided bycolumn surfaces.

Wall under the beam.

Fig.II-4-3 Diagram of a geometric model consisting of solid elements• Steel column/beam
Steel columns and beams are modeled with solid shapes. Certain rules are necessary forthe modeling of joints between steel frames. In reality, these are joined, for instance, withjoint plates. However, if these are to be simplified, it is desirable to conduct an examinationof the simplified method in advance at the member level.
• Steel reinforced concrete column/beam
Steel reinforced concrete columns and beams are modeled with solid shapes, andequivalent physical properties are assigned or modeled individually.
• Steel truss
Steel trusses are modeled with solid shapes. Include the joint between the roof and trusses
to create a model that matches the real structure. Note that, if everything, including the jointof each member of the truss, is modeled with solid finite elements, the number of elements
would be enormous. Thus, prepare a geometric model by considering that in the structuralmodel, beam elements and shell elements will be used.
• Pool water
Modeling of pool water is dependent on the modeling method of dynamic water pressure.
However, if it is analyzed through fluid elements, use geometric modeling. If it is modeled
as additional mass, consider it during the creation of the structural model.

- 34 -

JAEA-Research 2024-001• Pressure vessel and its support
There is a research example where the pressure vessel and all its supports were modeledwith solid elements. However, in a general calculation environment, modeling is conducted
through a combination of solid elements and shell elements.

- 35 -

JAEA-Research 2024-001

4.3 Creation of geometric model of the ground
Create a model of the ground based on topographical data, surveys, or geological reports.
Ensure that the ground model accurately represents the site's terrain, including any slopes,
irregularities, or other features that may affect the analysis.
[Commentary]
For the modeling of the ground of the analysis object area, consider the stratigraphic
classification (ground material) based on ground investigation documents, etc., and model itwith three-dimensional shapes. Fig.II-4-4 shows a visualization of modelling that takes strata
into account.
Verify that the prepared model matches the investigation documents in both geometry andmaterial constants.
If a ground model is created based on the finite ground information of a limited area, use
an appropriate interpolation/extrapolation method.

Ground surface

Ground surface

Stratum section

Strata boundary

Fig.II-4-4 Visualization of modeling that takes strata into accountIf the input seismic motion is horizontal 1 direction + vertical direction, the structure ismodeled with a 3D FEM model and the ground is modeled with springs. However, setting ofground springs with simultaneous input of three directions is difficult.

- 36 -

JAEA-Research 2024-001

Creation of the structural model
5.1 Introduction
Based on the geometric model, create a structural model that is appropriately meshedusing suitable finite element types.
[Commentary]
Create a structural model using finite elements (finite element model). As the setting ofelements affects the analysis result, set them appropriately according to the analysis purpose.
For the generation of meshes, verify the finite element ty pes and the fineness and accuracyof the meshes in advance through sensitivity analysis.
Verify the quality ind icators of meshes such as their distortion and aspect ratios tomaintain their quality.
When member joints are modeled with glue elements during a mesh generation with solid
elements, verify that it has little effect on the analysis result.
5.2 Difference in finite element types
Create a mesh appropriately using suitable finite element types based on the geometricmodel. Pay attention to quality indicators of the mesh, such as misalignment of member
cores, mesh distortion, aspect ratio, etc.
[Commentary]
A structural model is a model consisting of finite elements. Finite elements include barelements, beam elements, shell elements, and solid elements such as tetrahedral elements,
pentahedron elements, and hexahedron elements. Moreover, there are several formulas foreach element depending on accuracy, consideration of nonlinearity, etc.
As explained in the previous section, the structura l model includes cases where, as finite
element types, columns and beams are modeled with beam elements, and walls and floors aremodeled with shell elements and cases where these are modeled with solid elements. The
benefit of the former is that one can o btain the stress resultants of each member directly, andthe benefit of the latter is that it enables modeling of component joints that is closer to thereal shape and, therefore, capable of more accurate evaluation of structural deformation andthe mode shape.
5.2.1 Example of modeling with beam/shell structural model
In the case of a beam/shell structural model, each component can be modeled as follows.
• Column and beam members
Model them with beam elements and generate meshes that share nodes with the shell- 37 -

JAEA-Research 2024-001

elements of floors and walls. Both members made of reinforced concrete and of steel frames
are modeled with beam elements and differences in members are considered in terms of cross sectional property. Members made of steel reinforced concrete are regarded as a synthesis ofreinforced concrete and steel frames.
• Floor and wall members
Model them with shell elements, and generate meshes that share nodes with the beam
elements that modeled columns/beams that are connected to floor and wall members.
• Corners between walls
For the member joints between thick walls, evaluate corners appropriately. Fig.II -5-1
shows an example of the method to be considered.
Shell element

Shell element

Rigid body(a) Corner with shell elements(b) Corner with solid elements

Fig.II-5-1 Modeling of a corner 1 5• Floor and beam (wall and column) members
There are misalignments between the analysis model center of the floors and those of thebeams. If it can make a difference in the analysis result, consider these distances whenmodeling. Fig.II-5-2 shows an example of a member joint between a plane element and beam
element.

- 38 -

JAEA-Research 2024-001

Shell element

Rigid connection

Beam element

Fig.II-5-2 Example of member joint between a plane element and beam element 15• Roof slabs and roof truss members
Join the mesh of roof slabs with their support members appropriately.
• Steel truss member
Consider the joining conditions of the truss members at both ends. There are pin joints andrigid joints.

- 39 -

JAEA-Research 2024-001• Pool water
If using additional mass for modeling, obtain the additional mass of the pool water andadd that to the nodes around the pool.
• Pressure vessel and its support
If creating a model with beam elements and shell elements, create a model where mass isappropriately distributed and join it appropriately with the mesh of the support on thebuilding side. When performing a modeling by using additional mass, obtain the mass added
to both the pressure vessel and its support and add the m to the nodes that correspond withthe supports on each floor.
5.2.2 An example of modeling with solid elements• Columns, beams, floors, and walls
Model column, beam, floor, and wall members with solid elements (e.g., tetrahedral,pentahedron, hexahedro n, etc.) If using linear tetrahedral elements, analyze with quadraticelements before turning into a mesh to ensure accuracy.
• Pool water
Model pool water either with fluid elements using the structure –fluid coupling function orwith additional mass. Moreover, if the object is the sloshing phenomenon, use the elementsthat correspond with it.
• Steel truss member
Model it with beam elements or shell elements. Although there are examples where it wasmodeled with solid elements for research purposes, it is difficult to conduct them in normal
calculation environments.
In Annex 1 of Appendix 1 of the guideline, the part extracted from the basemat to B2F ofthe structure model used in the KARISMA project was used to perform analyses with abeam/shell structural model and solid structural model to demonstrate the difference in theirresults (Table II-5-1). In the analysis where horizontal inertia fo rce was applied to NS
direction, bigger deformation was generally observed in the beam/shell structural model, andits displacement at the part where there was the largest deformation was about 20% larger.
The result of comparing the 1st to 3rd natural frequencies of the same analysis model undera fixed basemat condition shows that those of the beam/shell structural model wereapproximately 15% lower.

These differences are due to the difference in the modeling of

the rigid zone of the joints of the beam/ shell structural model.

- 40 -

JAEA-Research 2024-001

Table II-5-1 Comparison of natural frequencies of beam/shell structural model and solid
structural model between the building basemat and B2F (Fixed basemat)

Ratio of beam/shell structural

Beam/Shell

Solid

Structural

Structural

model

model

1st

27.8 Hz33.8 Hz0.82

2nd34.7 Hz40.7 Hz0.85

3rd38.9 Hz44.5 Hz

0.87

Mode

model
in relation to solid structuralmodel

In addition, there is a report on the comparison of the beam/shell structural model andsolid structural model of a three -story building with wide columns and tall beams

30, and theresult also showed that the solid structural model had a higher natural frequency. Meanwhile,
although there is a report on the comparison of natural frequencies of two models of a simple
reactor building model mostly with walls 2 9 , their difference was small.
It is predicted that the difference between two models will be large when column width,beam width, and beam height are large compared to wall thickness. Thus, verify thedifference in advance.
5.3 Accuracy of finite element mesh
The size of the finite element mesh is set to satisfy the accuracy required for the analysis
objectives. Additionally, the model is created with a sufficiently small mesh to ensure thatthe analysis results are not dependent on the mesh. Furthermore, it is important to verify
that the mesh quality is appropriate.
[Explanation]
The mesh size of the finite element must be set at an appropriate size to ensure sufficient
analysis accuracy in both static and dynamic analysis. Obtain an appropriate size fromsensitivity analysis or similar past analysis examples.
5.3.1 Mesh size of static analysis
In static analysis, the mesh size must be set to a size where there is hardly any influenceon the strain and stress of members, even if the mesh size is made smaller. Referring toMartin and Ostadan 3 1 , ASCE/SEI 4-16 1 9 offers rules for the bending evaluation of slabs andunderground exterior walls, such that it must be set at six elements or more in the short side
direction. For the bending evaluation of other walls, it must be set at four elements or more

- 41 -

JAEA-Research 2024-001

in the vertical direction, and the areas around the opening must be further divided.
Generally, a large number of meshes are required to solve a bending problem with linear
isoparametric 4-node elements. According to the analysis example 3 2 of the Japan Concrete
Institute, to obtain 98.9% accuracy in relation to the theoretic al solution in the analysis of along cantilever beam with sections of 10 cm x 10 cm and 2 cm x 2 cm square meshes, 50
meshes in the length direction and 5 meshes in the width direction are required (Fig.II -5-3).
At the same time, according to CQUAD4 of N astran (see Annex 6 of Appendix 1), the samelevel of accuracy is obtained with 5 cm x 5 cm square meshes (10 meshes in the length
direction, 2 meshes in the width direction).

Note that accuracy could differ depending on

the finite element type.

- 42 -

JAEA-Research 2024-001

Analysis model

Ratio of be nding
momentcalculated f rom
the stress
distribution of
the element to
the theoreticalvalue (%)

Second order First order
8-noded
4-nodedquadrilateral quadrilateralb (width) = 10cm

Ratio ofdi s p l a c em en t
at the load
point to thet h eo r et i c a lvalue (%)

Fig.II-5-3 Analysis of a cantilever beam with isoparametric quadratic element 3 2
5.3.2 Mesh size of dynamic analysis
The mesh size of dynamic analysis must be less than the size of Equation (5 -1) obtained
from the transmission frequency 𝑓𝑓max . While in JEAG4601-1987 2 6 , the coefficient 𝑎𝑎 of
Equation (5-1) is set between 8 and 12 following the proposal by Lysemer 3 3 ; this shows that

5 is used as the standard according to the conventional empirical value. In section 5.34 of
ASCE/SEI 4-16 1 9 , the mesh size of the one-dimensional ground is set at a = 5.

∆ℎ <

𝑉𝑉s
𝑎𝑎 ∙ 𝑓𝑓max(5-1)

Here, Δh is the length of the long side of the mesh. According to ASCE/SEI 4 -16, Δh must
be set to a length that does not exceed 1/10 of the wavelength in nonlinear soil -structureinteraction analysis 1 9 . Moreover, f ma x is required to be 50 Hz or more according to the NRC
staff guidelines 3 4 , and in Seismic Design Bases of US -APWR standard plants by MHI 3 5 ,examination is conducted at 70 Hz.
Regardless of the above, the time step size of seismic motion in seismic response analysis
is generally 0.01 seconds and the Nyquist frequency is 50 Hz. This is the case when one
cycle is represented with two points and, physically, about 4 points; in other words, about
0.04 seconds (25 Hz), are necessary, so it is meaningless to increase only the transmission
frequency of the structure in elasticity analysis. If the focus of nonlinear analysis is on thehigh frequency component caused by failure, fine meshes may become necessary.
Structure mesh size
When obtaining stress that is necessary to evaluate cracking in earthquake-resistant walls- 43 -

JAEA-Research 2024-001

or local damage, finer mesh division may become necessary. For instance, in simulation
analysis for the loading test for seismic walls, a sample approximately 2 m in height (where
the top and bottom are constrained by the beam and the basemat) was divided by about 10 toevaluate associated cracks and damage 3 6 .
Examples from the 1990s include those with one mesh/floor for the structure height
direction used in 3D FEM model analysis, partly due to the limit of computational capacity 2 6(Fig.II-5-4). If a wall opening wherein each side is about 2 m is considered, the structureheight direction mesh would be about 4 meshes/floor 3 7 . When the mesh size is obtained fromthe equation below with reinforced concrete with a concrete strength Fc of about 40 ( V s ≒2500 m/s) and a transmission frequency f c = 50 Hz, it is L ≒ 10 m. Thus, 4 meshes/floor canbe regarded as a sufficient fineness to obtain the structural deformation within the elastic region. When performing elasto -plastic analysis, obtain the stress occurring locally throughelasticity analysis and refine meshes appropriately based on its result.

𝐿𝐿 =

𝑉𝑉𝑠𝑠
5 ∙ 𝑓𝑓𝑐𝑐

Here, V s is the shear wave velocity of reinforced concrete (m/s).

- 44 -(5-2)

JAEA-Research 2024-001(a) 3D model of reactor building(b) 3D model of arbitrary shape shell(1/4 partial model)(c) Externally shielded building/neighboring building model

Fig.II-5-4 Example of mesh in JEAG4601-1987 2 6- 45 -

JAEA-Research 2024-001

Comparison example of meshes of reactor building: According to the analysis example(Annex 7 of Appendix 1), there was hardly any difference in the natural frequency andresponse quantities in seismic response analysis for the model that increased the mesh sizesof the walls and floors of the structure in KARISMA 1 by 4 times (16 times in terms of area).
This is because the major vibration mode of the reactor building was the shear behavior of
the exterior walls, and the mesh size was sufficiently detailed for this type of behavior.
At the same time, though the floor level slabs of the crane floor of KARISMA (4F roofslabs) were modeled with MITC (tensor component) shell element, when the natural
frequency was obtained as the fix ed condition of the four sides, the difference of 12.6 Hzwith division by 4 of the short side and difference of 11.0 Hz with division by 16 of the shortside were observed. This indicates that division by 4 is insufficient and too inaccurate forconsidering out-of-plane deformation with MITC shell elements (See Annex 6 of Appendix
1).
Mesh size of the groundFor ground mesh, using surface contact elements, glue elements, et c., can be considered
because it is possible that the mesh quality could worsen because of the limitation in theconsistency with the strata forms and the finite element mesh of the structure.
The mesh of the ground under the structural basemat must be able to allow high precisionevaluation of the ground reaction. Moreover, use detailed meshes to consider the stressconcentration at the edge of the basemat.
5.3.3 Mesh quality
The quality indexes of the mesh of the FEM include the Jacobian and aspect rati os (ratioof the sides of elements). As many commercial finite element method pre -software provide
these indexes and guidelines, verify whether these indexes are appropriate by utilizing such
software. For indexes, these include software offering classific ations such as invalid (unable
to analyze), error, insufficient, and satisfactory. For the aspect ratio, 5 or less is desirable.
More detailed meshes are occasionally necessary to understand the stress concentration
state around the openings of walls and floors. If stress concentration becomes a problem, set
sufficiently small and appropriate meshes based on sensitivity analysis and similar past
analysis examples.
5.3.4 Glue conditions
If modeling the connections between the column/beam/floor/wall members with glue
elements, perform a sensitivity analysis of the mesh sizes of these members to verify that
their effect on the response is sufficiently small.

- 46 -

JAEA-Research 2024-001

6. Mass model
6.1 Introduction
Mass models consist of various components, including the structural elements,
architectural features, equipment, and more. While the structural mass can be determinedfrom the geometry, for non-structural components not defined by the building's shape, it isessential to rely on credible data and report the materials used as part of the analysis dataset.
[Commentary]
If the mass is modeled in detail, including the secondary members, and stiffness evaluationis performed only on earthquake -resistant walls, it is possible that natural frequency isevaluated to be lower.
6.2 Scope of mass to be considered
In the analysis, all mass components are considered in the assumed analysis s tate. In
seismic response analysis, various scenarios need to be considered.
[Commentary]
Ensure that the modeling scope of the mass of the 3D FEM matches the scope of theanalysis model. If only mass is added for a specific purpose, verify its effect. These masses
include the mass of the structure itself containing secondary members and non-structuralmembers, the mass of facilities/equipment, and the live load.
The equipment load is either presented as the equipment load distributed across the total
floor of each level, distributed across the individual floor, or that presented with the weights
and positions of separate heavy equipment on the layout in addition t o the distributed
equipment load. In the latter case, model the mass at each position.
In 3D-FEM model analysis, equipment load, etc., are to be considered at their installation
positions to understand three-dimensional behaviors such as the torsion of structure, andmodeling is conducted by including them in the masses of the rooms or the floors of theirinstallation locations.
6.3 Finite element model of mass
Set lumped mass and consistent mass appropriately for the finite element mass model.
[Commentary]
For setting the mass of a structure itself, one only needs to set the mass density of thegeometric model if one uses a solid structural model. However, when using a beam/shellstructural model, set the mass density while considering the occurrence o f overlapping parts- 47 -

JAEA-Research 2024-001

between elements at joints and set the mass of each level so that each matches the reality.
As an example, comparing the mass of each level obtained by using the geometric model,
etc., and volume multiplied by mass density of the beam/shell structural model and adjusting
their difference with the mass of the floor can be considered.
For the calculation of lumped mass of beam elements and shell elements, consider theinertial mass associated with three-axial translations and three axial rotations.

- 48 -

JAEA-Research 2024-001

7. Material model
7.1 Introduction
The material model used for 3D -FEM model analysis must be set appropriately according
to its analysis purpose, and its validity must be confirmed. When considering material
nonlinear behavior, clarify the definition of the material model (constitutive law) to be usedand set the required material parameters.
[Commentary]
A material model indicates a mathematical model of the stress and strain relationship(constitutive law), and the specified parameters are material parameters related to stiffness,
strength, damping, and plasticity. For these material parameters, the fluct uation range due tovariability in material must be considered according to the purpose of analysis.
In the inspection guide for certification of earthquake -resistant design construction 4 , it isnecessary to “understand the influence of realistic stiffness evaluations on the vibration andresponse properties.” Moreover, the Safety Guide 1 8 of IAEA includes design guidelines 1 6
and guidelines for existing facilities 3 8 , and settings appropriate to each purpose are required
for each of them.
Analyses using the values based on relevant standards/guidelines, such as the structural
calculation standard, are conducted during the design, and the model is updated when a large
earthquake is experienced or there are changes in the structure.
For PRA examination or performance verificat ion through material nonlinearity analysis,
set the necessary material parameters through material tests.
Analysis that considers the elast o-plasticity of reinforced concrete and steel frames has
become possible with seismic response analysis of reactor bu ildings using the 3D FEM model.
In such elasto-plastic analysis, constitutive law and its parameters of individual material andmember influence the analysis accuracy, and it is important to verify the validity of theconstitutive laws used in the analysis . When applying it to the seismic response analysis ofa reactor building, it is necessary to verify the validity and setting method of the constitutive
law in advance through, for example, the simulation analysis of the member test.
Moreover, with elasto-plastic analysis, parameters could differ even with the same
constitutive law depending on the analysis software being used. Refer to existing simulation
analyses such as the element test and member test to set these. Record the applied constitutive
law including contents such as specific parameters.

- 49 -

JAEA-Research 2024-001

7.2 Reinforced concreteUse the constitutive law and material constant of reinforced concrete based on clear
evidence such as valid standard, regulations, experiments, etc.
[Commentary]
In the inspection guidelines 4 , it is stated that as the structural response is used as the input
seismic motion to equipment and piping system, one mus t conduct realistic stiffness
evaluations and pay attention to the relationship between the design strength and real strength.
One can refer to the guidelines related to nuclear reactor facilities for power generation,such as the “AIJ Standard for Structural Calculation of Reinforced Concrete Structures for
Nuclear Power Facilities 1 4 ” by the Architectural Institute of Japan for the material constants
and allowable stress of concrete and steel in 3D -FEM model analysis.
For the constitutive law of elasto-plasticity, one can use the constitutive laws that havebeen employed in the past such as those listed in the “Guidebook for Numerical Analysis of
Spatial Structure 1 5 ” by the Architectural Institute of Japan or “ Standard Specifications forConcrete Structures -2017 1 6 ” by the Japan Society of Civil Engineers.
For the constitutive law of the reinforced concrete model, many proposals have been madethus far, such as the cracking model, model of the interactio n between concrete andreinforcement after the occurrence of cracks, model of stress transmission on the cracked
surface, and the elasto-plasticity hysteretic model of steel, and one must select an appropriate
model for the analysis object 1 4 .
The model 3 9 proposed by Maekawa et al. is often applied in the analysis of structures innuclear facilities. However, the details of its formulation can differ depending on the analysis
software. Moreover, there is an example of applying the constitutive law proposed by
Hong/Noguchi et al. 4 0 to member analysis and an example of applying the constitutive law
proposed by Naganuma et al. 4 1 to experiments with a three -dimensional structure.
When conducting an analysis that takes the nonlinearity of reinforced concrete int oaccount, verify the validity of the constitutive law being used in advance through simulation
analysis of the material test.
When applying the nonlinear constitutive law to the 3D FEM model of a building, theconstitutive laws of reinforced concrete need to be considered only for the floors and walls.
However, when examining the final state, the constitutive laws of reinforced concrete alsoneed to be considered for the columns and beams, as the bending deformation of the building
will become large in add ition to its shear deformation.

- 50 -

JAEA-Research 2024-001

7.3 Steel
The constitutive equations and material constants for steel materials shall be based on
valid standards, regulations, etc.
[Commentary]
Based on “Design Standard for Steel Structures 4 2 ” by the Architectural Institute of Japanand “Codes for Nuclear Power Generation Facilities -Rules on Design and Construction of
Nuclear Power Plants 4 3 ” by the Japan Society of Mechanical Engineers, it is possible to usematerial constants such as mill test reports for simulation analysis.
7.4 Steel reinforced concrete
The constitutive equations and material constants for steel -reinforced concrete materials
shall be based on valid standards, regulations, etc.
[Commentary]
The material constants of steel reinforced concrete can be obtained from the “AIJ Standard
for Structural Calculation of Steel Reinforced Concrete Structures 4 4 ” by the Architectural
Institute of Japan. If one has already obtained a measured value, use that instead.

- 51 -

JAEA-Research 2024-001

7.5 Ground
The material constants of the ground shall be determined based on ground investigationand indoor testing results. Additionally, for m aterial nonlinearity, appropriate constitutive
equations and analysis methods shall be used depending on the level of strain response.
[Commentary]
Set the mass density used for the analysis from the physical test based on the standard,and set the strength and nonlinear material properties from the laboratory test of the sampling
specimen. Set the initial stiffness based on the elastic wave velocity logging (PS logging)test. Depending on the type of constitutive law, other material constants may become
necessary.
The following relationships exist between the Young’s modulus E(N/m 2 ), shear modulus
G(N/m 2 ), mass density ρ(kg/m 3 ), and Poisson’s ratio ν of the ground and the compressional
wave velocity Vp(m/s) and shear wave velocity of the ground Vs(m/s).

(7-1)
,

,

7.5.1 Elasto-plastic behavior of the ground
There have been many proposals on the constitutive laws of elasto -plastic behaviors of theground, such as its strain dependence and liquefaction, and there are some material constants
that are unique to each constitutive law. Some of these unique material constants are difficult
to obtain through normal testing and are occasionally set based on the existing validity
analyses of similar grounds. In such cases, one must thoroughly verify the influence of thosematerial constants through sensitivity analysis.
In addition to the classic Mohr-Coulomb model and Dracker-Prager model, elasto plasticity constitutive laws of the ground include more advanced constitutive law by
Hashiguchi (subloading surface model) 4 5 , Asaoka et al. (SYS Cam-clay Model) 4 6 , Oka et
al 4 7 ., and Iai et al. 4 8 , just to list those from Japan. OpenSees 4 9 , discussed in ASCE/SEI section
4-16 1 9 , provides several constitutive laws.
Fig.II-7-1 shows the relationship between the size of shear strain and the groundconstitutive law. Advanced knowledge and experience are required to perfo rm seismic
response analysis of real ground using these constitutive laws.
At the same time, there is a method to perform linear analysis using the secant stiffness(equivalent stiffness) during the effective shear strain (equivalent linearization analysi s) asa method to easily consider the elasto -plastic behavior of the ground (Fig.II -7-2). However,note that there is a scope within which this method can be applied. Ishihara presented a table- 52 -

JAEA-Research 2024-001

that set around 0.2% to 0.8% to be its limit 5 0 .

Fig.II-7-1 Relationship between the size of shear strain and the ground constitutive law(Revision of K. Ishihara 5 0 )γmax
γ eff =Cγ max

Effective strain (C = 0.65)

D y n a m ic d e f o r m a tio n
c h a ra c te ris t ic

G eq
St if fn e s s

time

h

G
Eq u iv a le n t

γ

γeff

heq

Eq u iv a le n t d a m p in g

Fig.II-7-2 Equivalent stiffness and equivalent damping in equivalent linearization analysis

Effective strain in equivalent linearization analysis
Schnabel et al. 2 2 set the effective shear strain γ e ff at 0.5 to 0.7 times that of the maximum
shear strain γ ma x based on measured values. However, in common surface subsoil, 0.65 times
is often used, and for analyses at nuclear facilities, 0.7 times is often used.
7.6 Material damping
The material damping constants shall be determined using valid values obtained frommaterial test data.

- 53 -

JAEA-Research 2024-001[Commentary]
Causes of damping include the viscosity of member materials during micro strain, friction
at joints, dissipation into the ground, and friction between secondary members and finishingmaterials. For these material damping constants, damping unique to each material isevaluated as viscous damping (damping that is proportional to velocity).
When the material damping constant becomes larger, the dynamic response becomes
smaller. Therefore, be aware that underestimating the damping constant means designing on
the safe side, and setting an excessively large dam ping factor underestimates the response
value of the structure, which is a more dangerous evaluation.
7.6.1 Structure damping
For earthquake-resistant design, viscous damping constants are provided in several
guidelines.
Table II-7-1 lists the ASCE standard values for elasticity response analysis 1 9 . The reason
why damping becomes larger when the response level becomes larger is because the influenceof material nonlinearity is more significant in larger responses.

Table II-7-1 Viscous damping constants of materials (ASCE/SEI 4-16) 1 9
Response level

Response level

Response level

1

2

3

Reinforced concrete

4%

7%

10%

Prestressed concrete

2%

5%

7%

Steel structure welded

2%

4%

7%

4%

7%

10%

or joined with frictionbolts.
Steel structure joinedwith bearing bolts.
Here, response levels 1, 2, and 3 indicate the state where cracks are not occurring, the state where
cracks occurred, and the state where permanent strain occurred on reinforced concrete walls, beams, andcolumns, respectively.

While the following material damping values of structures in relation to the SSE groundmotion (safe shutdown earthquake ground motion) are included in NRC:RG1.61 Revision 1,
2007, it does not contain classifications according to the response level.
• Reinforced concrete: 7%• Prestressed concrete: 5%• Welded or shear friction bolt joints of steel framework: 4%- 54 -

JAEA-Research 2024-001• Steel container vessel: 4%• Steel frame building: 4% to 7%• Structure joined with bolts or rivet: 4% to 7%
JEAG4601-1987 2 6 defines damping in elastic response analysis as given in Table II -7-2.

Table II-7-2 Viscous damping constants of materials (JEAG 4601-1987) 2 6
Structure type

Damping constant

RC structure

5%

PCCV

3%

Steel container

1%

Steel structure

2%

Nakamura et al. 5 1 organized the values used for vibration experiments and simulation
analysis of earthquake observation records, and around 3% is appropriate as a more realistic
damping constant of reinforced concrete earthquake -resistant walls of nuclear facilities
within the linear region for seismic response analysis.
7.6.2 Damping of the groundThe ground displays elasto-plastic behavior from micro strain, and the stress –strain
relationship draws a hysteresis loop. The energy consumption in this hysteresis loop is
evaluated as damping. Damping depends on the size of strain and not on its velocity. The
relationship between damping and strain is commonly obtained through a dynamic
deformation test.

- 55 -

JAEA-Research 2024-001

8. Mathematical model of damping
8.1 Introduction
The internal damping of the structure and ground shall be set using an appropriate
mathematical model.
[Commentary]
The mathematical models of damping are divided into two types according to the time
integration method. For the method that performs iterated integration in the time domain,
several models have been proposed, including those with Rayleigh damping, hybrid damping,and hybrid mode damping. Hybrid damping includes elemental Rayleigh damping andelemental mode damping.
Furthermore, while complex damping is often used for the time integration method in thefrequency domain, it is also possible to use the abovementioned damping.
8.2 Mathematical models in the time domain
In time-domain response analysis, there are mult iple mathematical models available,
so it is important to consider their differences and choose the appropriate one.
[Commentary]
In time history response analysis, it is often approximated with stiffness proportional
damping or Rayleigh damping. In this case, the damping constant is set at one or two natural
frequencies. However, note that because 3D analyses focus on horizontal beh avior andvertical behavior simultaneously, their natural frequencies are different when determining
the setting.
Further, their validity is to be verified through the simulation analysis of the observation
record. It is also necessary to verify that the effect of the difference in settings is small
through sensitivity analysis or that the value of complex damping and the analysis result are
the same through linear calculation.
Moreover, the damping effect from nonlinear hysteresis is added to nonlinear mat erials.
However, when using Rayleigh damping in the region where the damping effect fromhysteresis is not added, be aware that its parameter setting could result in excessive damping
in the nonlinear region. Furthermore, when considering visco us damping in addition to thedamping effect from hysteresis, there is a method to use either the initial stiffness or the
momentary tangential stiffness, wherein the validity of damping must be verified throughsensitivity analysis.
Additionally, when using viscous damping for the stability of numerical analysis stability,
verify that its impact on the response of the structure is sufficiently small in advance.

- 56 -

JAEA-Research 2024-001

The formulations of representative damping are shown as follows. Among them, Rayleighdamping could use f 1 of Equation (8-1) as the natural frequency of horizontal motion and f 2
as the natural frequency of vertical motion. As modeling is conducted so as to make thedamping constants of the two frequencies those that were set, damping is estimated to besmaller between these frequencies and is estimated to be larger at the frequencies that aresmaller than f 1 and those that are larger than f 2 . Therefore, the setting should ensure that all
the frequencies to be considered in response analysis (primary natural frequency of eachcomponent of the three directions of soil -structure interactiob and the 1st natural frequencyof each component of the three directions of the structure) are within the range between these
two frequencies.
In simulation analysis of the observation record, the damping on the main vibration modes
is sometimes set to approximate material damping.
8.2.1 Damping matrix(1) Rayleigh damping
Rayleigh damping is a mathematical model that sets the coefficient of velocity to Equation(8-1) 1 9 . It is used when there is only one material. If the analysis object consists of materials
with different damping such as ground and concrete, elemental damping of (2) hybrid
damping is often used.
(8-1)

𝑪𝑪 = 𝛼𝛼𝑴𝑴 + 𝛽𝛽𝑲𝑲
Here,2ℎ𝜔𝜔 𝜔𝜔1 2𝛼𝛼 = 𝜔𝜔 +𝜔𝜔
1

2

𝛽𝛽 =

2ℎ

𝜔𝜔1 +𝜔𝜔2

M is the mass matrix, K is the stiffness matrix, h is the damping constant, 𝜔𝜔 is the angularfrequency, 𝜔𝜔1 = 𝑓𝑓1 ⁄2𝜋𝜋, 𝜔𝜔2 = 𝑓𝑓2 ⁄2𝜋𝜋; here, f 1 and f 2 are the main natural frequencies.

When the natural frequency is reduced because of becoming nonlinear, damping could beoverestimated.

The analysis example (Annex 2 of Appendix 1) shows an example of the Rayleigh damping
setting. When the results of seismic response analysis with Rayleigh damping and complex
damping under the analysis model/conditions of KARISMA were compared, the respons ewith Rayleigh damping was larger. (Note that f 1 = horizontal primary natural frequency ofsoil–structure interaction and f 2 = 20 Hz [setting made following the description “if the 1stnatural frequency is 20 Hz or more, it can be regarded as a stiff stru cture” in the earthquakeresistant design of equipment/piping systems in JEAC4601 while focusing on the dominantfrequency of the equipment]). This is inferred to be because of the damping between f 1 andf 2 being smaller than complex damping. However, it i s conceivable that this tendency may
change depending on the setting of f 2 . Thus, when a vibration mode whose frequency is larger- 57 -

JAEA-Research 2024-001

than f 2 affects seismic response, this must be verified with sensitivity analysis.
(2) Hybrid damping
When damping differs among finite elements or among domains, damping must be set foreach element or for each domain, and it must be in corporated into the overall matrix. Suchdamping is called the hybrid damping 1 9 .
𝑪𝑪 = ∑𝑁𝑁𝑁𝑁
𝑖𝑖=1 𝑪𝑪𝑖𝑖(8-2)

NS: Number of elements or domains
C i : Damping matrix of each element or each domain• Elemental damping
If damping is different for each element, Rayleigh damping must be set for each element.
Elemental damping can be obtained from Equation (8 -3).
(8-3)

𝑪𝑪𝒊𝒊 = 𝛼𝛼𝑖𝑖 𝑴𝑴𝒊𝒊 + 𝛽𝛽𝑖𝑖 𝑲𝑲𝒊𝒊
• Damping by domain

If damping is different for each domain, it must be set for each domain. Damping by domain
is a mathematical model of damping where mode damping of each domain with a structure is
obtained through boundary-free mode and then added rigid body mode.
𝑪𝑪𝐹𝐹𝐹𝐹𝑖𝑖
𝑪𝑪i = [ 𝑟𝑟 𝑇𝑇 𝐹𝐹𝐹𝐹
−𝑻𝑻𝑖𝑖 𝑪𝑪𝑖𝑖
Here,

𝑟𝑟
−𝑪𝑪𝐹𝐹𝐹𝐹𝑖𝑖 𝑻𝑻𝑖𝑖𝑇𝑇

𝑟𝑟−𝑻𝑻𝑟𝑟𝑖𝑖 𝑪𝑪𝐹𝐹𝐹𝐹
𝑖𝑖 𝑻𝑻𝑖𝑖(8-4)]

𝑪𝑪𝐹𝐹𝐹𝐹𝑖𝑖 : Damping matrix where the boundary condition of each domain was obtained

through fixed conditions.

𝑻𝑻𝑟𝑟𝑖𝑖 : Rigid body deformation mode matrix at the interface of each domain.

8.2.2 Hybrid mode damping

It is a mathematical model of damping obtained through Equation (8-5) using damping
matrix C of hybrid damping calculated in 8.2.1(2) and the mode shape 1 9 .

ℎ𝑗𝑗 =

𝑇𝑇

{𝜑𝜑𝑗𝑗 } 𝑪𝑪 {𝜑𝜑𝑗𝑗 }

(8-5)

2𝜔𝜔𝑗𝑗

- 58 -

JAEA-Research 2024-001{𝜑𝜑𝑗𝑗 } is the mode shape.

8.3 Mathematical model in the frequency domain
Complex damping can be used for frequency response analysis in addition to thedamping models in the previous section.
[Commentary]
For frequency response analysis, complex damping is commonly used. However,mathematical models such as the Rayleigh damping used in the previous section can also be
used.
8.3.1 Complex damping[Commentary]Complex damping is the term related to h of Equation (8-6) expressed using complex
numbers. This damping is often used in frequency response analysis.
Moreover, in frequency response analysis, the upper limit of the analysis frequency is
occasionally set above the Nyquist frequency. Note that this regards the response of thefrequency component above the limit as zero.

𝐾𝐾 ∗ = 𝐾𝐾(1 − 2ℎ2 + 2𝑖𝑖ℎ√1 − ℎ2 ) or 𝐾𝐾 ∗ = 𝐾𝐾 (1 + 2𝑖𝑖ℎ)(8-6)

K* is complex stiffness, K is stiffness, and i is the imaginary unit. h is the damping constant.
While the early equivalent linearizing method was the latter, the former is being used after
SHAKE-91 5 2 . The effect of this difference in formulation on the response is small.

- 59 -

JAEA-Research 2024-001

9. Boundary joint model
9.1 Introduction
For the boundaries or connections between the interior and exterior of the building, useappropriate structure models.
[Commentary]
The main joints include those between the bottom of the building basemat and supporting
ground, the underground exterior walls of the building and the side ground, and the member
joints of the structure.
9.2 Modeling of the joint between an underground structure and the groundIn cases where the building response becomes s ignificant with large amplitudes, the soil structure interaction between the embedded building and the ground is modeled using finite
elements, such as joint elements, that can consider detachment, re -contact, and sliding.
[Commentary]
For a 3D FEM model of a reactor building buried underground, perform modeling by taking
soil-structure interaction (i.e., separation, recon tact, and sliding) into account. Use joint
elements (here, a general term including gap elements) for modeling. Joint elements include
those that model the area between the building node and the ground node and those thatmodel the area between the structure and the ground as a solid element without thickness.
The former formulates the constitutive law with the relative displacement and st ress between
nodes and the latter with element strain and element stress.
The distribution of the initial stress of the joint elements must be consistent with thereaction distribution in dynamic analysis. Ensure that this initial stress is evaluated as areleased force against the separation surface when separation occurs.
The constitutive laws of separation and sliding in joint elements are defined as the axial
direction component and shear direction component of stress (or force) in the verticaldirection and horizontal direction, respectively, regardless of the finite element type. The
axial direction component models the separation/recon tact phenomenon and the shear
direction component models sliding. Table II -9-1, Fig.II-9-1, and Fig.II-9-2(a) show theconstitutive laws of the joint elements.
Vertical force and friction proportional to adhesion are used for modeling of the joint
between the underground structure and the ground. Both of these are to be set according to
the material tests that are suitable to the actual construction situation. Re garding the friction
coefficient considering the waterproof layer between the underground exterior walls of thestructure and the side ground, there was an experiment that reported that the dynamic friction- 60 -

JAEA-Research 2024-001

coefficient between the underground walls and the ground was 0.35 5 3 . The static friction
coefficient is larger than this; however, it is between 0.5 and 1.0, showing a large variability.
Considering this information, it is desirable to verify the shear force caused by therotational vibration of the stru cture applied on the boundary between the undergroundexterior walls and the side ground in relation to the seismic force, friction coefficient, etc.,
through sensitivity analysis. Fig.II -9-2(b) shows the relationship between the adherence
strength of the friction on the joint and the shear strength.

- 61 -

JAEA-Research 2024-001

Table II-9-1 Constitutive law of joint element
Axial direction

Shear direction component

component
Compression side
Tension side

Elasticity

Friction law

Elasticity until

Friction law untiladhesion strength,

adhesion strength, zerothen separation

after separation

Force/Stress(Tensile side force/stress)
Adhesion strength

Relative displacement/strain

A x ia l d i re c tio n s t i f fn e s s(Compression side force/stress)

Fig.II-9-1 Constitutive law of joint elements (Axial direction component)

Shear/stress

Shear strength
Compression
side

Relative displacement/strain

Adhesionstrength(a) Relative displacement/strain is the value after(b) Friction law

Fig.II-9-2 Constitutive law of joint elements (Shear direction component)

Seismic response analysis with joint elements considers separation, displacement, andreaction change suddenly at the moment of recon tact; therefore, the acceleration of thecontact point (twice differentiated displacement) becomes extremely large, which appears asa spike-shaped acceleration in the time history. Regarding the acceleration of the contact
point, including this spike-shaped acceleration, obtain a realistic acceleration by devising anonlinear analysis algorithm or by using an appropriate value for the axis -direction stiffness- 62 -

JAEA-Research 2024-001

of the joint elements.
If avoiding it through axis-direction stiffness, an appropriate stiffness must be usedthrough sensitivity analysis to ensure that the analysis result will not change. In general, thevalue obtained by multiplying the stiffness per unit area taken from the vertical ground springobtained through the vibration admittance theory by 50 –1000 is used 5 4 .

- 63 -

JAEA-Research 2024-001

9.3 Connections between building members
Use appropriate modeling method considering the influence of modeling of the connection
between building members to the analytical results.
[Commentary]
Utilize an appropriate modeling approach that minimizes the impact on the analysis results,
particularly at the intersections of building members, including columns and beams orcolumn-beam junctions. Be cautious when dealing with overlapping regions in cases whereshell and beam elements are employed. When working with a solid structural model, be
mindful of potential stress concentrations at member interfaces and joints.
9.4 Bottom and side boundaries of the analysis ground area
The modeling of the side and bottom boundaries of the analysis ground area should enable
the accurate assessment of wave dissipation for both internal and external vibration issues
within the half-infinite space.
[Commentary]
In a 3D FEM model, the bottom and side of the ground are regarded as stratified gro unds
that are semi-infinite (hereinafter referred to as “semi -infinite ground”). The validity ofmodeling for real ground is discussed in the section on the analysis object area. Here, theanalysis method for semi-infinite ground is discussed.
The effect that semi-infinite ground has on the structural response include internal
vibration problems and external vibration problems. The internal vibration problem is where
waves occurring in the ground because of structural response dissipates into the semi -infinite
ground. The external vibration problem is a problem where the vibration within the analysis
ground area may not match the free ground even when the input from the side free ground isconsidered. Analysis methods for the soil -structure interaction problem that considers thesemi-infinite boundary include the direct and the substructure methods.
The calculation models that are able to consider these problems include the non-reflection
boundary [Cundall] 5 7 , propagation boundary [Lysmer] 5 5 , viscous boundary [Lysmer] 5 5 , andnotch force. Use these suitably to model semi-infinite ground appropriately and evaluate thestructure response.

- 64 -

JAEA-Research 2024-001(a) Bottom ground
Corner free ground
Side free ground
Corner free ground

Side free ground

Building

Side free ground

Analysis ground

Corner free ground

Corner free ground

Side free ground(b) Side ground 3 7
Fig.II-9-3 Modeling of analysis ground area

- 65 -

JAEA-Research 2024-001

Commonly, the bottom of the analysis ground area is modeled with a viscous damper as
the viscous boundary.
When the ground is stratified ground, for the side of analysis ground area side, thefollowing have been proposed:(1) Periodic boundary model(2) Viscous boundary that regards far ground as one-directional free ground 5 5 , notch force
model(3) Frequency domain propagation boundary 5 5(4) Paraxial model 5 6(5) Non-reflection boundary 5 7(6) Infinite boundary model 5 8(7) Time domain energy propagation boundary 5 9
However, (4) to (7) are rarely used in actual analysis.
If the ground is stratified, in (1), the free side ground shown in Fig.II -9-3(b) is often
represented by a “periodic boundary model”. In (2), the model where the far ground isrepresented by the free side ground and free corner ground and then both are connected witha “viscous damper” and “notch force” is more accurate. However, it has the problem of alarger calculation load.
The periodic condition is a condition where the displacements of the points of a given sideground and its corresponding opposite side ground are the same when the ground is stratified
ground.

- 66 -

JAEA-Research 2024-001

10. Input seismic motion
10.1 Introduction
Apply the relevant seismic motion input to the bottom of the analysis ground area, inalignment with the specific analysis objectives.
[Commentary]
While the seismic motion used in seismic response analysis is set according to the analysis
purpose, in 3D analysis, the seismic motion is first converted into the seismic motion input
to the bottom of the analysis ground area.
For the seismic response analysis for seismic safety evaluation, use the input seismic
motion that matches the motion that was set as t he basic earthquake ground motion. For
simulation analysis of the observation record or experiment, set the input seismic motionthat is close to the actual circumstance.
10.2 Seismic motion set at the bed rock
When establishing seismic motion at the bedrock surface, the input seismic motion
should be adjusted relative to the bottom of the analysis ground area using an appropriate
method.
[Commentary]
For the input seismic motion in the seismic safety evaluation, the seismic response at thebottom of the analysis ground area calculated through one -dimensional wave theory, two dimensional analysis, etc., derived from the basic earthquake ground motion is set at the freerock surface. Fig.II-10-1 shows the overview of input seismic motion preparation. This basic
earthquake ground motion must be the one where two horizontal directions and the verticaldirection are appropriately combined.
In 3D-FEM model elasticity analysis, it is possible to perform an analysis where eachcomponent of an input seismic motion with three directiona l components is independently
applied and their solution is then superimposed. However, in elasto-plasticity analysis, thesethree directions are applied simultaneously.
One can also refer to the earthquake observation records from the analysis object site to
set an input seismic motion with three directional components. When setting simulated
seismic motion, it is necessary to consider the correlation of the three directions and thecharacteristics of the observed seismic motions.
As the methods to simulate input seismic motion assuming simultaneous input from three
directions are still in their research phase, perform the evaluation of the analysis result byreflecting the latest knowledge in setting the three directions of input seismic motion and the- 67 -

JAEA-Research 2024-001

spatial distribution of seismic motion characteristics such as the phase difference in the input
seismic motions at the bottom of the analysis ground area.
One can use a 2D or 3D ground model for evaluating pullback waves.

Ground surface

Free ground
Free rock surface

Ground model

Bottom of the ground model

Input ground motion U

Groundresponse

Free rock surface

Fixed boundary

Upgoing wave

Viscous boundary

Downgoing wave

When the free rock surface is deeper than the

When the free rock surface is shallower
than the bottom of the ground model.

bottom of the ground model.
Fig.II-10-1

Overview of input seismic motion preparation

In simulation analysis using the earthquake observation records of a structure, the validityof the analysis conditions is examined by obtaining the wave input into the bottom of theanalysis ground area so as to ensure that it is consistent with the obser vation record at thebasemat position, and then attempting to simulate the records from other observation
positions through seismic response analysis using this seismic motion.

- 68 -

JAEA-Research 2024-001

11. Initial state model
11.1 Introduction
Set the appropriate stress as the initial value corresponding to self -weight and temperature
distribution.
[Commentary]
As the difference in the initial stress for the constitutive law of reinforced concrete, theuplift of the “structural basemat bottom and supporting ground” and “underground exterior
walls of the structure and side ground” and the joint elements for consid ering separation andsliding occasionally influence the response result; thus, one must pay attention to the settingof initial values.
Set appropriate initial conditions in response to the changes in the structure after its
construction.
11.2 Self weight model
When accounting for the elasto -plastic behavior of reinforced concrete members, theground, and the uplift of the structure's basemat, ensure that the initial conditions for eachmember and the ground are set appropriately.
[Commentary]
The calculation model of the initial stress caused by the dead weight affect the elastoplasticity of reinforced concrete, the uplift caused by joint elements, and the responses ofseparation and sliding.
A combination of the consistent mass matrix and lumped mass matrix is sometimes usedas the mass matrix of dynamic analysis. Ensure that the dead weight calculated from these isconsistent with static analysis.
For the setting of initial conditions, use dead weight analysis with a 3D FEM model or theearth pressure at rest. For dead weight analysis, fixed conditions are often used for the bottomof the analysis model, and horizontal constraints are often used for the sides. However, beaware that when performing dynamic analysis, boundary conditions may differ. For instance,
the periodic boundary is used for these.
11.3 Thermal stress model
If the temperature of the analysis object has an impact on seismic response, be sure toinclude it in the analysis.

- 69 -

JAEA-Research 2024-001[Commentary]
As the temperature is inferred to be in a steady state during a short phenomenon like anearthquake, regard this as the initial condition.

- 70 -

JAEA-Research 2024-001

12. Condition setting for mathematical analysis
12.1 Introduction
Choose the analysis method and conditions so that the errors due to the numerical anal ysis
technique do not affect the intended analysis results.
[Commentary]
One must ensure that in analysis with the finite element method, the influences of thefinite element, time integration method, nonlinear analysis algorithm, etc., are sufficiently
small.
12.2 Accuracy of the finite elements
Considering the accuracy of the element formulation of FEM supported by the analysis
software select appropriate element formulation depend on the analysis purpose.
[Commentary]Among finite elements, there are beam elements, shell elements, and solid elements, andeach includes various types of elements. Verify the formulation and validity of the elements
provided by the analysis software and select the appropriate element for the anal ysis purpose.
Moreover, be aware that depending on the type of finite element, it might display uniquedeformation behaviors such as shear locking and hourglass mode.
These element accuracies are occasionally presented in papers on element development or
through comparison with the examples provided by NAFEMS 2 3 . The analyst must verify theiraccuracy in advance. However, if there are ex isting verification results, they can be referred
to instead.
12.2.1 Beam element
Representative beam elements are elements derived from theoretical solutions andisoparametric elements. As the former cannot be used for elasto -plastic analysis, if elastic
analysis and elasto-plastic analysis are to be performed, the difference in accuracy andvalidity must be verified prior to the main analysis.
12.2.2 Shell element
As shown in “Table 3.2.1 Concept of elements used in analysis of plate and shell structure”
of the “Guidebook for Numerical Analysis of Spatial Structure 1 5 ”, there are various finite
elements for plate and shell structures. One must understand what type of formulation is
employed by the analysis software being used.

- 71 -

JAEA-Research 2024-001

12.2.3 Solid element
For 3D-FEM model analysis, tetrahedral elements are often used because they simplify theautomatic generation of mesh models. F or 3D analysis of mechanical systems, second -ordertetrahedral elements are often used. Note that analysis models that use first-order tetrahedral
elements are generally inaccurate. Thus, caution should be exercised when using them.
First-order hexahedron elements are not generally used because mesh generation withthese is difficult. However, in recent years, a mesh model where the analysis object structure
is divided into many partial structures, generating meshes from them and linking them withglue elements, has been used. Research and verify its formulation and accuracy in advancein this case as well.
12.3 Seismic response analysis method
Seismic response analysis methods include the time domain and the frequency domain
methods. Set an appropriate method and parameters by considering their respective features.
[Commentary]
Seismic response analysis methods include the linear analysis method, the nonlinear
analysis method, and equivalent linearization analysis. These methods are obtained throughtime domain or frequency domain integration of the response of the analysis objec t to the
input seismic motion at each moment.
In the case of linear analysis, time integration methods include those of the time andfrequency domains, and each are divided into time history response analysis and thefrequency response analysis methods. Th e time history response analysis method includes
the direct integration and mode analysis methods. The mode analysis method is rarely usedin 3D-FEM model analysis. Moreover, though there is also the spectrum mode analysis
method, it is rarely used in conjunction with 3D FEM model analysis.
In the case of nonlinear analysis, the method that in corporates the nonlinear analysis
method into the time history response analysis method using the direct integration method isused.
Equivalent linearization analysis is often combined with the frequency response analysis
method through the method to obtain nonlinear behavior using linear analysis with secant
stiffness corresponding to response strain.
12.3.1 Direct integration method
The common response analysis metho ds with respect to direct time integration are theNewmark-β method and the Wilson-θ method, which are implicit methods of unconditional
stability in relation to calculation time step size. Further, there is central difference method,which is an explicit method, as well as the Runge–Kutta method and the Houbolt method,- 72 -

JAEA-Research 2024-001

which are both conditional stability methods 6 0 , 6 1 .
As K.J. Bathe 6 0 and O.C. Ziewiewicz 6 1 have pointed out, when using direct integrationof iterated integrals, one must pay attention to numerical stabilization and numerical damping.
3D FEM model analysis tends to have an extremely large maximum natural frequency. At
the same time, the direct integration method results in a less accurate response to highfrequencies because of its time step size. Generally, in the case of 0.01 seconds, as used inlinear calculation, the accuracy worsens when it exceeds 10 Hz. Attention also needs to be
paid to the integration method and numerical damping due to the calculation time step size.
ΔhIn ASCE/SEI4-16 1 9 , the time step size is set as Δt ≤ v . Here, Δh is the minimum lengthof finite elements, and Vs is the shear wave velocity.

sMoreover, in nonlinear analysis, the calculation time step size must be made smaller thanthat in linear analysis depending on the nonlinear analysis algorithm. The degree depe nds on
the nonlinear analysis algorithm.
12.3.2 Frequency response analysis method
When using the frequency response analysis, ensure that the increment frequency(interpolation of the transfer function) and cut -off frequency do not influence the result
intended for analysis.
Specifically, Fig.II-12-1 shows the diagram of the interpolation of the transfer function in
frequency response analysis.

In frequency response analysis, there are cases where thetransfer function is sometimes calculated wit h jumping increment frequency and otherfrequencies are calculated through the interpolated transfer function. However, in 3D -FEM
model analysis, it is necessary to use an appropriate increment al frequency as many vibration
modes are included.

Transferfunction

Calculate by interpolating transfer
functions of other frequencies fromthe calculation points f a and f b .
Accurate interpolation of the 3D
transfer function is required.

fa

fb

Fig.II-12-1 Diagram of the interpolation of transfer function in frequency response analysis- 73 -

JAEA-Research 2024-001

12.4 Nonlinear analysis method
For analysis with the implicit method in nonlinear analysis, verify the convergence of
iterative calculations performed at each step.
[Commentary]
Nonlinear analysis methods include the implicit and explicit methods. The implicit method
is often used in seismic response analysis, and the explicit method is often used in collision
or fall analysis. Further, nonlinear calculation algorithms for the imp licit method include theinitial stiffness method, Newton’s method, and the modified Newton’s method. Thesemethods obtain the solution through iterations at each calculation step. At this time, theresidual at each step must converge below the acceptable value.
In dynamic analysis, if the residual is not fully converged at the step where the directionof the external force is inverted, there is a possibility that the correct solution cannot be
obtained. Therefore, the iteration number, residual, and conver gence at each calculation step
must be checked to verify that their influence on the analysis result is small.
In many nonlinear analysis algorithms, if the solution does not converge during theiterative calculation at a given step, its residual is transf erred to the next step. However,depending on the stiffness for obtaining the solution at each iteration (i.e., tangential
stiffness, secant stiffness, analogical stiffness, etc.), numerical vibration could occur. Thus,
pay attention to the applicability o f the analysis algorithm that contains these types of
stiffness.

- 74 -

JAEA-Research 2024-001

12.4.1 Features of nonlinear analysis of reinforced concrete
There are two features of nonlinearity for reinforced concrete. It is a composite ofreinforcement and concrete, and they both di splay nonlinear behaviors. Because of thecracking of concrete, the isotropy of the material disappears. While there are diverse
modeling methods, it is difficult to represent every crack and stress state. It is desirable toconduct sensitivity analyses with several constitutive laws to verify the validity of theanalysis solution.
Moreover, as nonlinear analysis with a 3D FEM model of reactor building can potentiallydisplay strong local nonlinear behavior because of influences from the existence of openin gs,
layout of walls, and modeling of the joints of the SRC structure, it is desirable to examine itwith partial models in advance.
12.4.2 Features of nonlinear analysis related to basemat uplift
A collision occurs when the basemat bottom and the support ground recon tact after
separation. At this time, the ground shows the same deformation behavior corresponding to
the rotational deformation of the structure. Depending on the deformation state of the ground,
it is possible that the separated basemat bottom recontacts almost at the same time. In thiscase, large vertical acceleration (induced vertical motion) can occur throughout the whole
structure. In the analysis, the large force from the moment of collision is received by thejoint elements. If the stiffness of these joint elements is extremely large, unrealistic, spike shaped acceleration occurs unless the calculation time step size is sufficiently small. In
general, the energy from this spike is small, and its influence on the st ructure response isoften small. However, it can potentially affect the stress in the underground structure walls.
Thus, the analysis result must be investigated, and if it affects the stress in the undergroundstructure walls and other factors, one must p erform more accurate calculations by, forexample, shortening the time interval.
With nonlinear analysis using a 3D FEM model of reactor building that takes basemat
uplift into account, there are reports stating that the influence of whether there is basemat
uplift on the maximum acceleration of the building is about 10% up to the minimum groundcontact ratio of about 50% 6 2 . Furthermore, if damping is considered for the joint elements
during numerical analysis, be aware of the fact that it can potentially u nderestimate the uplift(separation) state.
12.4.3 Features of nonlinear analysis of separation/recon tact of underground exterior wallsof a structure and the side ground
When the structure and the ground recon tact after separation, large acceleration occ urs
because of collision, as in basemat uplift; however, when the surface subsoil is softer than
the support ground, the structure and the side ground vibrate independently, resulting in the- 75 -

JAEA-Research 2024-001

nonlinearity of the vibration type at the moment of recon tact becoming stronger.
12.4.4 Features of nonlinear analysis of sliding of underground exterior walls of a structure
and the side ground
When sliding stiffness is extremely large, the stiffness during the sliding is set as zero
inclination, and it is solved with the tangential stiffness method, it is necessary to make thecalculation time step size small enough such that the sliding inclination contains the response
value. When this is ignored, numerical vibration occurs. Thus, as sliding stiffness can not be
excessively large, appropriate stiffness and damping must be obtained through sensitivity
analysis.
While it is possible to consider damping in a sliding state to stabilize numerical analysis,
it is desirable to verify its effect through sensitivity analysis as it can change the amount ofsliding.

- 76 -

JAEA-Research 2024-001

13. Examination and validation of analysis results
13.1 Introduction
Before verifying the validity of the analysis results, one must ensure that the analysis has
been completed successfully. Then, check the input data and subsequently inspect thecontent of the analysis from a macroscopic perspective, such as the load -displacement
relationship, deformation diagrams, internal force diagrams, etc. Here, by 'inspection,' inthe case of material nonlinear analysis, it means ensuring that the analysis conditions andsolutions fall within the application range of the analytical method, and that they havephysical significance. It also includes comparisons with solutions from similar analyses. If
necessary, improvements to the analytical model and re -analysis should be performed before
confirming the validity of the analysis results.
[Commentary]
The following items can be used to confirm that the analysis has been completed correctly.
•

Calculation error record•

Analysis software (version), Computer (calculation environment): Comparison
with the plan•Calculation time: Comparison with the expected time•

Input file name, Output file name: Check whether the cases were mixed up•

Date, Person responsible: Check whether processed files were mixed up

Perform input data checks on the following items:•

Element division diagram (structural diagram), Member list: Verify shapes•

Constraint diagram : Verify the constraint conditions•

Seismic motion wave diagram: Verify the input seismic motion•

Material distribution diagram: Verify the material setting•

Natural frequency and mode shape: Verify whether they match the predicted natural
frequency and mode shape. Verification of the natural frequency of the structureor the soil-structure interaction model and the state of vibration model using themode shape is an effective method to verify the accuracy of the analysis model, as
well as its geometric model, structural model, materials, boundary conditions, etc.

Verification of the validity of the analysis result ensures that the following variables areboth within the application scope of the analysis software and physically meaningful and thatthey are consistent with similar analyses.
•

Node variables (e.g., acceleration, velocity, displacement)•

Response spectrum- 77 -

JAEA-Research 2024-001•

Stress resultants: Strength evaluation•

Element variables (stress, strain): Strength evaluation•

Reaction force- 78 -

JAEA-Research 2024-001

13.2 Confirmation of normal completion of the analysis result
Confirm that the analysis has been successfully completed .
[Commentary]
Confirm that there are no errors in the calculation result. Also, verify the contents ofwarnings. First, check the calculation log file in relation to one’s experience to see if there
are any irregularities. Fig.II-13-1 shows examples of warning and error messages.
Moreover, refer to the records from similar analyses as empirical values with regard to theanalysis scale, calculation time, and calculation environment to confirm that the analysis has
been completed normally.

*** USER WARNI NG MESS AGE 8152 (M3DCNT1B)
BOTH BCTABL1 AND BCONECT HAVE THE SAME ID = 1. BCTABL1 WILL BE USED INSTEAD OF BCONECT.
User Information: BCT ABL1 and BCONECT can have the same ID. In t his case, BCTABL1 will be used instead of BCONECT.
*** USER FATAL MESS AGE 8146 ( MCN1DATS)
For BCBODY1 ID = 1044, either no supported elements have been found in the deformable contact body or all elements have been
specified in the contact body of another contact pair.
User Information: Every deformable conta ct body must contain some elements, supported by 3D contact capability .
User Action: Check contact modeling for errors i n the input dat a entries, such as BCTABL, BCONECT, BCBODY1, and so on .

Fig.II-13-1 Examples of warning and error message s (MSC Nastran 2019)13.3 Examination of input data
For the input data, confirm that there are no differences from the original data before
the analysis.
[Commentary]
The input data that can be output from analysis data such as mesh diagrams (structural
diagrams), member lists, constraint diagrams, seismic motion wave diagrams, and material
diagrams can be checked through comparisons with the original data. Compare nume ricallywhen possible.
Among echo backs, there are those that are simple outputs of the letters of the input text
and those that are outputs of the same but read as numbers. Verify that the input values ofthe latter are correct.
With the former, it is dif ficult to check whether the digit separators are misaligned or notin the case of fixed format. The sixth data in Fig.II -13-2 is 18.5. However, it is continuouswith the previous number and, therefore, errors are easy to miss.

- 79 -

JAEA-Research 2024-001

COUNT
660511 660512 660513 -

.
1
GRID
GRID
GRID

..
2 ..
328594328595328596

3

..

4 ..
5 ..
6 ..
-27.55 15.8455218.5-27.55 15.0481818.5-27.55 14.2508418.5

7

..

8

..

9

..

10

.

Fig.II-13-2 Example of input text echo back ( MSC Nastran 2019)
By turning it into a diagram, one can identify major errors in the coordinate input data.
Regarding the structural model data, one must ensure that there are no abnormal values
among natural frequencies and mode shapes before the main analysis through eigenvalue
analysis to ensure there are no errors in the shape, constraint, and joint conditions.
Regarding the boundary conditions, input seismic motion, and initial conditions, each of
their conditions and states should be plotted to ensure that there are no errors. Fig.II -13-3
shows an example of abnormal mode shapes caused by data errors.

By making a comparison with the mesh diagram on the right, one can recognize that
deformation occurs only in the cylindrical part of the container vessel as the primary
vibration mode.
Fig.II-13-3 Example of abnormal mode shapes caused by data error 6 3
13.4 Examination of analysis contents
Examine whether the analysis contents are within the application range of the analysis
method.
[Commentary]
After verifying that there are no problems with the calculation processing information,
calculation errors, or calculation time, confirm the following items for the analysis content.
The use of video is effective for these checks.
•

Correspondence between acceleration/deformation, displacement distribution, and load•

Ratio of acceleration/displacement and stress and simple calculation or theo reticalsolution- 80 -

JAEA-Research 2024-001•

Positive/negative, symmetry, and over/underestimation of acceleration/displacement•

Balance of acceleration/stress and displacement•

Tendency of acceleration/displacement and stress•

Locations of tension/compression occurrences•

Reaction at the position to prevent a rigid body motion•

Reaction at the constraint position and consistency with the load•

Strain and stress distribution at joints•

Stress and yield strength- 81 -

JAEA-Research 2024-001

13.5 Validation of analysis results
In validating the analysi s results, compare the results of simulations using the targeted
analysis model and method with actual experiments, observations, or real damage
situations. Ensure that the reproducibility and predictive performance align with theintended objectives.
[Commentary]
Verify the validity of the analysis result by matching with similar analyses and experimentand observation records. For this, quantitative evaluation of accuracy using an appropriate
evaluation standard is necessary. Evaluation standards used for the vali dity evaluation
include M S R Q of ASME 6 4 (Measurement standard of system response quantity and anevaluation standard that can represent the relative error of the average. Here, SRQ stands for
SystemResponse

Quality)andstatisticalcharacteristics

such

as

the

calculation

value/experiment value ratio (e.g. , average, coefficient of variation).
Moreover, as a validity verification of the analysis result, comparison with a simpl ified
model is effective. For a simpler analysis model, analysis can be conducted us ing the lumped
mass model 6 5 . In terms of 3D analysis, analysis using a lumped mass model is equivalent to“one-dimensional analysis”, and it plays an important role in understanding the overallbehaviors and verifying the validity of the analysis result. F or instance, the characteristics
and accuracy of the overall behaviors can be verified by comparing the average of the 3D
analysis results with the analysis result using a lumped mass model.

- 82 -

JAEA-Research 2024-001

14. Utilization of analysis result14.1 Introduction
When using analysis results that have been validated, pay attention to errors in processingof those results.
[Commentary]
The analysis results include the following variables. Pay attention to the errors when
outputting the necessary variables for each analysis purpose.
The node variables are the values that were directly calculated through the finite element
method, and the only error caused by result processing is the number of output digits.
Variables include acceleration, velocity, an d displacement.
•

Time history: Pay attention to the output time step size.

•

Maximum value: Pay attention to the fact that the time step size for obtaining the
maximum value is occasionally different from the calculation.

•

Maximum value contour diagram: Pay attention to the fact that it interpolates node values
and draws an isopleth.
Element variables include strain and stress. Additionally, nonlinear calculations include

nonlinear state variables. While the element variables are calculated through the Gauss point,
the output may be the average at the center of the element.
•

Time history: Check whether the output is the calculation or average value within anelement and the difference. Regarding time, pay attention to the time interval.

•

Maximum value: Pay attention to the fact that the time step size for obtaining the
maximum value is occasionally set longer than the calculation time step size.

•

Contour diagram: Pay attention to the calculation method for the contour value.

•

Crack condition diagram: Pay atte ntion to the output method for closed cracks.

•

Contact/Separation: Check the stress of joint elements and the time history of relative
displacement. Regarding the maximum value of acceleration, obtain a realistic value by
referring to the sensitivity analys is. The application of a low -pass filter to the result canalso be considered (see 14.2).

•

Induced vertical motion: During uplift, a large induced vertical motion (acceleration)
occurs. Thus, obtain a realistic value by referring to the sensitivity analysis.

14.2 Utilization of nonlinear analysis result
For the analysis results in nonlinear analysis, thorough consideration is necessary forpost-processing.

- 83 -

JAEA-Research 2024-001[Commentary]
In the analysis of material nonlinearity, the basemat uplift, and separation and recontactof the structure’s underground exterior walls and the side ground, the nonlinearity ofmaterials becomes stronger and a sudden change in the external force occurs at the momentof reconnection. This results in a significant chang e in acceleration; however, the common
time interval of seismic response analysis is not capable of correctly analyzing these sudden
and rapid changes, which may result in vibrations with unrealistically high er modes.
Unrealistic high-frequency waveforms are associated with spike -shaped acceleration. As thisfrequency requires four points for each cycle, it can result in a frequency that is four times
larger than the calculation time step size. In such a case, t his frequency can be removed witha low-pass filter.
Annex 4 of Appendix 1 contains an example where a high -frequency waveform caused byside separation/recontact was removed. At a calculation time step size of 1/1000 sec, thewave centered on the 4/1000 s ec cycle (250 Hz) is included in the analysis result, causing
the maximum response acceleration of the basement of the structure to be unrealisticallylarge. While the maximum response acceleration distribution comes closer to a realistic
number when the components above 100 Hz are cut from it, the response spectrum at the
separation/recontact position has a large high-frequency domain response. This is because of
the recontact. While further investigation is needed to determine the accuracy of this value,
the results that have been obtained thus far show that the influence of this spike -shaped
acceleration on the center or the upper part of the reactor building is small.
Annex 5 of Appendix 1 shows that high -frequency waveforms caused by cracks are also
contained in the analysis that considers the nonlinearity of reinforced concrete.
14.3 Accounting for variation in the analysis results
Depending on the analysis objective, consider deviation using factors such as structural
analysis coefficients.
[Commentary]
When using the result of a seismic response analysis for performance inspection, take thestructural analysis factor into account. The structural analysis factor is set by assessing theanalysis basis documents, the accuracy of analysis conditions, and the knowledge andexperience of the analyst in the analysis method according to the utilization purpose of theanalysis result.
If the purpose of analysis is simula tion analysis of experiment or observation records,
consider the variability in material constants, etc.
For performance inspection of the analysis, the Japan Society of Civil Engineers 1 6 set thestructural analysis factor 𝛾𝛾𝐴𝐴 , one of the safety factors, by taking the uncertainty of structural- 84 -

JAEA-Research 2024-001

analysis when calculating the response into account. In general, it is set at 1.0; h owever, fornonlinear analysis, the structural analysis factor, which includes the member factor, is set
between 1.1 and 1.5. Regarding the safety factor, refer to the publication 6 6 by the Japan
Society of Civil Engineers.
Moreover, in the Japan Society of Civil Engineers 6 7 , errors in the numerical analysis using
𝛾𝛾𝐴𝐴 of Equation (14-1) in relation to the response of the real structure.
S ≤ 𝑅𝑅𝑎𝑎 =

Here,

1

𝛾𝛾𝐴𝐴 𝛾𝛾𝐵𝐵 𝛾𝛾𝑖𝑖

𝑅𝑅

(14-1)

S: Response value (Stress, strain and displacement calculated through analysis)
R a : Limit value (Limit of stress, strain and displacement that takes material characteristics
into account)𝛾𝛾𝐴𝐴 : Structural analysis factor (1.0 to 1.1)𝛾𝛾𝐹𝐹 : Member factor (1.1 to 1.3)

𝛾𝛾𝑖𝑖 : Structure factor (Importance of a structure 1.0 to 1.2)
14.4 Peer check

To ensure the validity and reliability of analysis results, it is desirable to have themchecked by a third party.
[Commentary]
Perform a peer check to evaluate the analysis results. The Standard Specifications forConcrete 1 6 encourage third-party evaluation to ensure the validity of reinforced co ncrete
structures. Additionally, the Japan Society of Civil Engineers conducts numerical analysis
certification evaluations 6 8 .

- 85 -

JAEA-Research 2024-001

15. Documentation
15.1 Introduction
For the effective implementation of th e guideline, it is essential to document the inputs,
outputs, and execution contents of each analysis process from Chapter 2 to Chapter 14.
[Commentary]
Appropriate documentation is an important step in V&V. All of the items relevant to theanalysis purpose, analysis object, modelin g method, analysis method, etc., must be notatedin text, and the contents should be verified by every person involved, including the person
who planned the analysis, the analyst, the users, and the reviewers (analysis reviewer). When
preparing documentation, the compatibilityof theimplemented

documentation object and its equivalent situation must be traceable.

- 86 -

process with theJAEA-Research 2024-001

Acknowledgment
This report is a part of results obtained from the Nuclear Regulation Authority consignment
project “Consignment Expenses for Disaster Prevention Measures for Nuclear Facilities(Advancement of Seismic Safety Evaluation Methods for Buildings, Equipment, andStructures that Consider their Aging).”

Additionally, parts of the published data from the

Review of Seismic Evaluation Methodologies for Nuclear Power Plants Based on a
Benchmark Exercise, IAEA TECDOC No. 1722, IAEA, Vienna ( 2014) have been used withthe permission of the IAEA. Furthermore, these guidelines were developed in considerationof the discussions held in the Expert Committee on Nuclear Reactor Building integrity
Research. We would like to express our gratitude to each person involved.

- 87 -

JAEA-Research 2024-001

References
1 IAEA, Review of Seismic Evaluation Methodologies for Nuclear Power Plants Based on a
Benchmark Exercise, IAEA-TECDOC-1722, 2013, 156p.
2 Japan Society for Computational Engineering, Quality Management of Engineering
Simulation, 3rd Edition, JSCE S -HQC001:2017, 2017, 20p.
3 Nuclear Regulation Authority of Japan, Inspection Guide for Basic Earthquake Ground
Motion and Earthquake-resistant Design, June 19, 2013.
4 Nuclear Regulation Authority of Japan, Inspection
Guide
for
CertificationofEarthquake-resistant Design Construction, June 19, 2013.
5 Nuclear Regulation Authority of Japan, Operation Guide for Safety Improvement
Evaluation of Commercial Nuclear Power Reactor, Revised on March 20, 2017.
6 Nuclear Regulation Authority of Japan, Ana lysis of influence factors that contribute todetailed estimation of three-dimensional earthquake behavior of buildings of nuclear
reactor facilities and examination of its modeling, NTEC -2021-4002, 2021.
7 Japan Electric Association, Technical Guidelines for Seismic Design of Nuclear Power
Plants, Chapter on importance classification/Allowable stress, JEAG4601, Revision -1984,
1984.
8 Japan Electric Association, Technical Guidelines for Seismic Design of Nuclear Power
Plants, Expanded edition, JEAG4601 -1991, 1991.
9 Japan Electric Association, Technical Guidelines for Seismic Design of Nuclear Power
Plants, 3rd edition, JEAG4601-2015, 2015.
10 Final Report on the Light Water Reactor Safety Technology/Human Resource
Roadmap/Rolling Response at the Atomic Energy Society of Japan March 2017,https://www.aesj.net/document/com-r_lwrroadmap20170322.pdf(Referred
toon
February 8, 2024).
11 Atomic Energy Society of Japan, A Standard for Procedure of Seismic Probabilistic Risk
Assessment for Nuclear Power Plants : 2015, AESJ-SC-P006:2015, 2015, 1012p.
12 Atomic Energy Society of Japan, Guidelines for securing reliability of simulations: 2015,
AESJ-SC-A008:2015, 2015, 110p.
13 Japan Society of Mechanical Engineers, Codes for Nuclear Power Generation Facilities– Rules on Design and Construction for Nuclear Power Plant: Alternative Design for
Seismic Design of Seismic S Class Steel Piping Based on Elastic-Plastic Response
Analysis, JSME S NC-CC-008, 2019.
14 Architectural Institute of Japan, AIJ Standard for Structural Calculation of Reinforced
Concrete Structures for Nuclear Power Facilities , 2013, 221p.
15 Architectural Institute of Japan, Guideboo k for numerical analysis of spatial structure,
2017, 407p.
16 Japan Society of Civil Engineers, Standard Specifications for Concrete Structures -2017,
Design, 2018, 679p.
17 Japan Society of Civil Engineers, Seismic Performance Verification Guidelines, Manuals
and Examples for Underground RC Structures in Nuclear Power Plants, 2018.
18 IAEA, Safety Guide Seismic Design and Qualification for Nuclear Power Plants, IAEA
Safety Standard Series No. NS -G-1.6, STI/PUB/1158, 2003.
19 American Society of Civil Engineering, Seismic Analysis of Safety -Related Nuclear
Structures, ASCE/SEI 4-16, 2017, 171p.
20 U.S.NRC, Standard Review Plan for the Review of Safety Analysis Reports for Nuclear
Power Plants, NUREG-0800, 2007.
21 Goodman, R. E., et al., A model for the Mechanics of Jointed Rock, Proc. ASCE, 94 SM3,
1968, pp.637-659.
22 Schnabel, P. B., et al., SHAKE -A computer program for earthquake response analysis ofhorizontally layered sites, Report No. EERC 72 -12, 1972.
23 NAFEMS, The International Association for the Engineering modelling, Analysis andSimulation Community, https://www.nafems.org/ (Referred to on February 8, 2024).
24 Tokyo Electric Power Company, Inspection/evaluation report on the facility health of- 88 -

JAEA-Research 2024-001

Reactor 7 of Kashiwazaki-Kariwa Nuclear Power Plant after the 2007 Chuetsu offshore
earthquake (Chapter on Building/Strucutre) (Revised edition 1), Reference 2 on theevaluation of the supporting walls of the building (Reactor 7 building), 2008,https://www.tepco.co.jp/cc/press/betu08_j/images/080925f.pdf (Referred to on February
8, 2024).
25 Japan Nuclear Energy Safety Organization, An Incorporated Administrative Agency,
Analysis of ground -building analysis model of the 2007 Chuetsu offshore earthquake(Analysis of this observation record and seismic response analysis mode), 2008.
26 Japan Electric Association, Technical Guidelines for Seismic Design of Nuclear Power
Plants, JEAG4601-1987, 1987.
27 U.S.NRC, Seismic Design Standards and Calculational Methods in the United States andJapan, NUREG/CR-7230, 2017.
28 U.S.NRC, Assessment of Seismic Analysis Methodologies for Deep ly Embedded Nuclear
Power Plant Structure, NUREG/CR -6896, 2006.
29 Tadahiko Shiomi, First step of Verification and Validation for seismic response analysis
of Nuclear Reactor Building, Proceedings of the Conference on Computational
Engineering and Science, Vol.18, 2013, 4p.
30 Hiroyuki Yoshida et al., Study on building modeling using 3D FEM, Summaries oftechnical papers of annual meeting of the Architectural Institute of Japan, 2019, pp.281 282.
31 Martin, D. S. and Ostadan, F., Summary structural report, HLW vitrification building,24590-WTP-RPT-ST-03-001, Bechtel, 2004.
32 Japan Concrete Institute, Guideline for application of FEM analysis on concrete structure
design, 1989, 134p.
33 Lysmer, J., et al., Finite dynamic model for infinite media, J. of the Engineering
Mechanics Division, Vol.95, No.4, 1969.
34 U.S.NRC, NRC Interim Staff Guidance Associated with Combined License Application
and Design Certification for New Reactor Applicants, COL/DC -ISG-1, 2008.
35 Mitsubishi Heavy Industries Ltd., Seismic Design Bases of the US -APWR Standard Plant,
2011, https://www.nrc.gov/docs/ML1104/ML110470431.pdf (Referred to on February 8,2024).
36 OECD, Seismic shear wall ISP NUPEC’s seismic ultimate dynamic respons e test;comparison report, NEA/CSNI/R(1996)10, 1996.
37 Katsuichiro Hijikata et al., Three dimensional response behavior of unit No.5 reactor
building subjected to the Niigataken Chuetsu -Oki Earthquake in 2007, Journal of
Structural and Construction Enginee ring, Architectural Institute of Japan, Vol.75, Issue
658, 2010, pp.2179-2187.
38 IAEA, Evaluation of Seismic Safety for Existing Nuclear Installations, IAEA Safety
Standard Series No. NS-G-2.13, STI/PUB/1379, 2009, 84p.
39 Koichi Maekawa, Naoyuki Fukuura, R e-formulation of spatially averaged RC
constitutive model with quasi-orthogonal bi-directional cracking, Collected papers of theJapan Society of Civil Engineers, Vol.634, 1999, pp.157 -176.
40 Hong Jie, Study on shear strength of RC beam -column joint by 3D FEM analysis,
Doctoral dissertation, Graduate School of Chiba University, 2009.
41 Kazuhiro Naganuma, An analytical model for reinforced concrete panels under cyclic
stresses, Journal of Structural and Construction Engineering, Architectural Institute ofJapan, Issue 536, 2000, pp.135 -142.
42 Architectural Institute of Japan, AIJ Standard for Allowable Stress Design of Steel
Structures, 2005.
43 Japan Society of Mechanical Engineers, Power generation nuclear energy facility
standard Design/construction standar d, JSME SNC2-2016, 2016.
44 Architectural Institute of Japan, AIJ Standard for Structural Calculation of Steel
Reinforced Concrete Structures, 2014, 395p.
45 Koichi Hashiguchi, Latest Theory on Elasto -Plasticity, Asakura Shoten 1990, 205p.

- 89 -

JAEA-Research 2024-001

46 Asaoka A., et al., AN ELASTO -PLASTIC DESCRIPTION OF TWO DISTINCTVOLUME CHANGE MECHANISMS OF SOILS, Soils and Foundations, Vol.42, no.5,
2002, pp.47-57.
47 Oka, F., et al., A cyclic viscoelastic–viscoplastic constitutive model for clay andliquefaction analysis of multi‐layered ground, International Journal for Numerical andAnalytical Methods in Geomechanics, Vol.28, no.2, 2004, pp.131 -179.
48 Iai, S., Ozutsumi, O., Yield and cyclic behaviour of a strain space multiple mechanism
model for granular materials, International Journal for Numerical and Analytical Methods
in Geomechanics, Vol.29, no.4, 2005, pp.417 -442.
49 Mazzoni, S., et al., OpenSee s Command Language Manual, 2006, 465p.
50 Ishihara, K., Soil Behaviour in Earthquake Geotechnics, Oxford, Clarendon Press, 2003,
350p.
51 Naohiro Nakamura, et al., Study on modeling error in strong nonlinear area of structure
in fragility evaluation of NPP b uildings, AIJ Journal of Technology and Design,
Architectural Institute of Japan , Vol.13, Issue 26, 2007, pp.499 -504.
52 Schnabel, P. B., et al., SHAKE -91: Equivalent linear seismic response analysis ofhorizontally layered soil deposits, the earthquake en gineering online archive NISEE e library, 1992.
53 Tokyo Electric Power Company Holdings, On prevention of earthquake damage on
Reactor 6 and Reactor 7 of Kashiwazaki -Kariwa Nuclear Power Plant 2016,
https://www.tepco.co.jp/about/power_station/disaster_prev ention/pdf/nuclear_power_16
1129_03.pdf (Referred to on October 15, 2021).
54 Naohiro Nakamura, et al., Response behavior of nuclear power plant building for
simultaneous horizontal and vertical motions using 3D FEM model considering basement
uplift, Journal of structural engineering, Vol.54B, 2008, pp.581 -589.
55 Lysmer, J, et al., FLUSH- A computer program for approximate 3 -D analysis of soilstructure interaction problems, EERC -75-30, 1975.
56 Kim, H.S., Finite Element Analysis with Paraxial & Viscous Bounda ry Conditions for
Elastic Wave Propagation, Engineering, Vol.4, no.12, 2012, pp.843 -849.
57 Cundall, P.A., et al., Solution of infinite dynamic problems by finite modelling in thetime domain, Second International Conference on Applied Numerical modeling, M adrid,
Spain, 1978.
58 Bettess, P., Infinite elements, Int. J. for Num. Methods in Engineering, Vol.11, 1977,
pp.53-64.
59 Shodo Akita, et al., A study on time domain energy transmitting boundary for improving
efficiency of calculation and application to de tail soil-structure interaction system,
Journal of Structural and Construction Engineering, Architectural Institute of Japan, Issue
689, 2013, pp.1263-1272.
60 Bathe, K.J., Finite Element Procedures in Engineering Analysis, Prentice-Hall, 1982,
736p.
61 Ziewiewicz, O.C., and Taylor, R., The Finite Element Method, Vol.2, McGraw -Hill Book
Company, 1989.
62 Nuclear Regulation Authority, Project progress report for 2020 consignment expenses
for disaster prevention measures for nuclear facilities (Advancement of seismic safety
evaluation methods for buildings, equipment, and structures that consider their aging),
2021.
63 Japan Society for Computational Engineering Standard, Academic Society Standard(HQWC001&002) Collected Examples, 2015.
64 ASME, An Illustration of the Concepts of Verification and Validation in Computational
Solid Mechanics, ASME V&V 10.1 -2012, 2012, 32p.
65 Abell, J.A., et al., Earthquake soil‐structure interaction of nuclear power plants,
differences in response to 3-D, 3×1-D, and 1-D excitations, Earthquake Engineering andStructural Dynamics, Vol.47, no.6, 2018, pp.1478 -1495.
66 Japan Society of Civil Engineers, Seismic Performance Verification
Guidelines,- 90 -

JAEA-Research 2024-001

Manuals for Important Outdoor RC Structures of Nuclear Power Plants, 2005, 150p.
67 Japan Society of Civil Engineers, Standard Specifications for Steel and Composite
Structures -2018, IV Seismic Design, Maruzen Publishing, 2018, 321p.
68
Japan
Societyof
Civil
Engineers
Technology
Evaluation
System,http://committees.jsce.or.jp/opcet/hyoka (Referred to on February 8, 2024).

- 91 -

This is a blank page.

JAEA-Research 2024-001

Appendix
Attachment 1

Sensitivity Analysis Results of the Influential Factors

In this appendix, we performed sensitivity analyses on key factors to quantitatively
assess their impact on the response results in the 3D Finite Element Method (FEM) modelof the reactor building. The results are presented to provide a clearer understandi ng of
how these factors influence the response outcomes in terms of both methods and content.
Annex 1 Modeling by Solid Element and Shell Element
Annex 2 Effect of Different Damping Modeling
Annex 3 Accuracy of Vertical Response of Reactor Building
Annex 4 Effect of Nonlinear Soil -structure Interaction
Annex 5 Effect of Nonlinear Constitutive Model of Reinforced Concrete
Annex 6 Effect of Finite Element Program
Annex 7 Effect of Mesh sizes of Finite Elements
References- 93 -

This is a blank page.

JAEA-Research 2024-001

Annex 1 Modeling by Solid Element and Shell Element
The following are the results of sensitivity analyses utilizing shell element and solid
element models. These findings are presented to validate the influence of employing
various types of finite elements in the modeling process on the building response.
1.1. Analysis model and analysis condition
In this example, the basemat to the B2F floor of a reactor building were modeled usingshell and solid elements, which are different types of finite elements (hereinafter referred
to as the shell model and solid model). Eigenvalue analysis and static analysis were
performed, and the difference in modeling according to the finite elements used wasevaluated. For the static analysis, the method where uniform body force in one horizontal
direction is applied on the entire model was employed. Fig.1 -1 shows the shell model andthe solid model that were analyzed. The basemats of both were modeled with solid
elements. The shell model uses laminated shell elements, and the solid model uses
hexahedral primary elements. The loading is applied in the +X direction (NS direction).

Elevation(1) Shell model(2) Solid modelFig.1-1 Bird's-eye view (B2F floor slabs not displayed)
1.2. Eigenvalue analysis result
1.2.1 Natural frequency
First, the natural frequency of each model was verified. Table 1 -1 shows up to the 3rdnatural frequencies in the NS direction . The main natural frequencies were determined by
the effective mass ratio. The 1st natural frequency in the NS direction of the shell model
was 27.8 Hz (natural period: 0.036 s) and that of the solid model was 33.8 Hz (natural
period: 0.030 s). Thus, the natural frequency of the shell model was about 20% lower thanthat of the solid model. This is because in the solid model, the hei ght of the walls arelowered by the height of the beams and the width of the walls are narrowed by the width ofthe columns because of the modeling process. Further, the wall thickness es of these parts
are evaluated through the beam width and column width; therefore, their stiffness ishigher than that of the walls.

- 95 -

JAEA-Research 2024-001

Table 1-1 Natural frequency (NS direction)
Shell model
Mode

Frequency

order

(Hz)

Period (s)Solid model
Effective

Frequency

PeriodEffective

mass ratio

(Hz)

(s)

mass ratio

1st

27.8

0.036

0.267

33.8

0.030

0.229

2nd

34.7

0.029

0.040

40.7

0.025

0.023

3rd

38.9

0.026

0.022

44.5

0.022

0.030

1.2.2 Mode shape
The mode shapes of the shell model and solid model are shown in Fig.1 -2. Here, thepart with the largest displacement is indicated by red, and the part with the smallest
displacement is indicated by deep blue. While there are some discrepancies in the locationof the maximum value, the overall mode shapes are largely similar.

(a)1st mode(a) 1st mode(b) 2nd mode(b) 2nd mode(c) 3rd mode(c) 3rd mode

(1) Shell model(2) Solid modelFig.1-2 Comparison of mode shapes- 96 -

JAEA-Research 2024-001

1.3. Analysis result
1.3.1 Maximum displacement
Fig.1-3 shows the height–direction distributions of the maximum displacements of theshell and solid models when an uniform body force is applied to the entire model. Overall,
the result of the shell model tended to have larger displacement than that of the solid
model, and it was about 20% larger at the upper end. Moreover, the basemats of both theshell model and the solid model (elevation between −13.7 m and −8.2 m) were modeledwith solid elements, and their maximum displacements were nearly identical.

A

difference in displacement was observed in B3F, where different element types were used
(elevation between −8.2 m and −1.7 m), and it is inferred that the difference in themodeling method using finite elements affected their difference in displacement.

B3F
A b o v e b a s e ma t

B3F
Above basemat

All nodes
Repr esentative nodes

B e lo w b a s e ma t

All nodes
Repr esentative nodes

B e lo w b a s e m a t(1) Shell model(2) Solid modelFig.1-3 Comparison of maximum displacement distribution(RA center (R1A and R7A are the corners of the building, while R4A is the center of theexternal wall))- 97 -

JAEA-Research 2024-001

1.3.2 Deformation and shear strain distribution
Similarly, Fig.1-4 shows the deformations, while Fig. 1-5 shows the shear strain
distributions of the shell and solid models when uniform body force is applied to theentire model. The deformations and shear strain distributions of the two models match
well overall. In both, the maximum value of the shell mod el was about 20% larger thanthat of the solid model, demonstrating larger stiffness in the sold model.
This is also inferred to be due to the difference in the modeling method using finite
elements affecting difference in displacement.

(1) Shell model(2) Solid modelFig.1-4 Comparison of deformation (m)(1) Shell model(2) Solid modelFig.1-5 Comparison of shear strain distribution- 98 -

JAEA-Research 2024-001

Annex 2 Effect of Different Damping Modeling
A sensitivity analysis was performed by employing both Rayleigh damping and complex
damping, and the results were scrutinized to assess the implications of variations in
damping modeling on the building response. This analysis involved conducting a time
history response analysis with a soil-structure interaction model utilizing Rayleighdamping and a frequency response analysis employing complex damping to evaluate theirrespective impacts on the building response.
2.1. Analysis model and analysis conditions
2.1.1 Analysis conditions
For the 3D FEM model of the reactor building, the element used in the analysis modelof the KARISMA benchmark model 1 was used in principle. The surrounding ground was
produced as a 3D FEM model, and the physical properties of the surface ground andsupporting ground were set to be uniform. Fig.2 -1 shows the overview of the 3D FEM
model.
Elevation

Fig.2-1 Overview of the 3D FEM model
The seismic waves used in this analysis were simulated seismic waves (one horizontal
motion wave and one vertical motion wave), with a maximum horizontal motion
acceleration of 600 cm/s 2 and a maximum vertical motion acceleration of 400 cm/s 2 . The
horizontal motion was exited into the NS direction and the EW direction, and the verticalmotion was exited into the UD direction.

- 99 -

JAEA-Research 2024-001

2.1.2 Damping model
2.1.2.1 Rayleigh damping
Rayleigh damping (Rayleigh damping for each element) was used for the time history
response analysis of this example. Table 2 -1 shows the eigenvalue analysis result, andFig.2-2 shows the horizontal 1st mode of the building with fixed basemat. When setting
Rayleigh damping, it is necessary to determine the main natural frequencies. They wereset as
・ f 1 : From the eigenvalue result, the natural frequency of horizontal 1st mode・ f 2 : 20 Hzin this analysis. Regarding the damping ratio, h was set as the damping ratio in relation tovarious materials. For example, this was 5.0% for RC and 2.0% for steel. The eigenvalue
analysis for obtaining f 1 was conducted with the independent building model with fixedbasemat, and the 1st mode in the NS direction, 3.99 Hz, was set as f 1 . To obtain f 2 , wefocused on the dominant frequency of the equipment, and following the description in theearthquake-resistant design of the equipment/piping system section in the Regulations for
Earthquake-Resistant Design Technology for Nuclear Power Stations, JEAC4601 2 , whichstated that “when the 1st frequency is 20 Hz or more, the structure can be regarded as arigid structure,” it was set as f 2 = 20 Hz.
Fig.2-3 shows the relationship between Rayleigh damping and frequency. In this setting,the damping ratio in relation to the main natural frequencies of the building model is lessthan 5.0% and is around 4.0% near 9.0 Hz, where the damping is the smallest (with theexample of RC). Compared to damping models with a constant frequency, such as mode
damping, this damping model is smaller. However, we empl oyed this setting to avoid theunderestimation of the response value by setting excessive damping.
The parameters of Rayleigh damping of the ground were set through the same approachas that for the building.
2.1.2.2 Complex damping
Complex damping is used for frequency response analysis. Regarding the damping
constant h, set as the damping constant in relation to various materials, it was set as RC =5.0% and steel = 2.0%. In this example, the upper limit of frequency was set to 30 Hz.

- 100 -

JAEA-Research 2024-001

Table 2-1 Eigenvalue analysis result
Modes
モード

1
2
3
4
5
6
7
8
9
10

F re q.
振動数
Hz
3.99
4.75
5.60
6.47
6.57
6.64
7.34
7.52
7.86
8.15

P周期
er i o d

s
0.25
0.21
0.18
0.15
0.15
0.15
0.14
0.13
0.13
0.12

S t i m ul刺激係数
us c o eff i c i e nt

X(NS)
4.01
0.06
-4.23
0.37
-0.62
0.25
0.01
0.13
-0.14
1.64

Y(EW)
-0.03
3.87
0.14
1.76
-0.67
-3.34
-0.14
0.13
-0.13
-0.11

Z(UD)
-0.05
-0.01
-0.02
0.55
0.37
0.08
0.38
0.17
4.50
0.24

N S di r ec t i on

Mo d es

E ff ect i v e m as s r a ti o
有効質量比

X(NS)
0.44
0.00
0.15
0.00
0.00
0.00
0.00
0.00
0.00
0.04

Y(EW)
0.00
0.54
0.00
0.01
0.00
0.07
0.00
0.00
0.00
0.00

Z(UD)
0.00
0.00
0.00
0.00
0.00
0.00
0.00
0.00
0.01
0.00

E W di r ec ti on

1st

Fig.2-2 Horizontal 1st mode of the building (fixed basemat)
S oi l ( h = 3% )
R C (h = 5% )D am pi n g ( -)S te el ( h = 2% )F re q ue nc y (H z )Fig.2-3 Relationship between Rayleigh damping and frequency- 101 -

R em
ar k s
備考
st
1NS1次
(NS)
st
1EW1次
(E W )nd
2NS2次(N S )nd
2EW2次(E W )

JAEA-Research 2024-001

2.2. Analysis result
2.2.1 Maximum response acceleration and maximum response displacement
Fig.2-4 shows the representative nodes of each floor in this analysis.
Corner of exterior wall
corner
Midpoint of exterior wall(a) B3F (Elevation −8.2 m)(b) B2F (Elevation −1.7 m)(c) B1F (Elevation +4.8 m)(d) 1F (Elevation +12.3 m)(e) 2F (Elevation +18.1 m)(f) 3F (Elevation +23.5 m)(g) 4F (Elevation +31.7 m)

Fig.2-4 Representative nodes of each floor in this analysis (plan view)- 102 -

JAEA-Research 2024-001

Fig.2-5 and Fig.2-6 show the comparisons of height direction distributions of the
maximum response acceleration and maximum response displacement obtained throughtime history response analysis and frequency response analysis. The solid line in the
figure indicates the average of all the nodes at each floor in the building model. The
broken line indicates the average of the representative nodes of the building model (seeFig.2-4). The black line indicates the result of time history response analysis. The red line
indicates the result of frequency response analysis. In this example, the results of thefrequency response analysis were all about 10% smaller than that of time history response
analysis.
E l ev at i o n
60

GLAll nodes(Time hist ory)
Rep. nodes(Time hist ory)
All nodes(Frequency)
Rep. nodes(Frequency)

(m)

60

50

50

40

40

30

30

20

20

10

10

0

0

-10

-10

-20

(a) X(NS) direction

0

500

1000

1500

2000
(cm/s2)-20(b) Y(EW) direction

(m)

0

500

1000

1500

2000
(cm/s2)(c) Z(UD) direction

Fig.2-5 Comparison of maximum response acceleration distributions (Average)
E l ev at i o n
60

GLAll nodes(Time hist ory)
Rep. nodes(Time hist ory)
All nodes(Frequency)
Rep. nodes(Frequency)(a) X(NS) direction

(m)

60

50

50

40

40

30

30

20

20

10

10

0

0

-10

-10

-20

0

5

10

15

20

25
(mm)

(b) Y(EW) direction

-20

(m)

0

5

10

15

20

25
(mm)

(c) Z(UD) direction

Fig.2-6 Comparison of maximum response displacement distributions (Average)- 103 -

JAEA-Research 2024-001

2.2.2 Floor response spectrum
Fig.2-7 and Fig.2-8 show the comparisons of floor response spectrums at B3F and 3F
through the time history response analysis and frequency response analysis.

It wasverified that the results of the frequency response analysis tended to be slightly smaller
than those of the time history response analysis, and they were up to 10% smaller.
Fig.2-5 to Fig.2-8 show that the results of the frequency response analysis tend to besmaller than the results of the time history response analysis.

The reason for this is thefact that while they have the same damping for the 1st natural frequency, the damping at
the 2nd and 3rd mode shapes are underestimated.

(cm/s2)Average of Rep. (Time history)(cm/s2)

2500

2500

2000

2000

1500

1500

1000

1000

500

500

Average of Rep. (Frequency)

Period (sec)(a) X(NS) direction

0
0.01

0.1

1
10
Period (sec)(b) Y(EW) direction

0
0.01

0.1

1
10
Period (sec)(c) Z(UD) direction

Fig.2-7 Comparison of floor response spectrums h = 5% (B3F, elevation −8.2 m)(cm/s2)Average of Rep. (Time history)(cm/s2)

5000

5000

4000

4000

3000

3000

2000

2000

1000

1000

Average of Rep. (Frequency)

Period (sec)(a) X(NS) direction

0
0.01

0.1

1
10
Period (sec)(b) Y(EW) direction

0
0.01

0.1

1
10
Period (sec)(c) Z(UD) direction

Fig.2-8 Comparison of floor response spectrums h = 5% (3F, elevation 23.5 m)- 104 -

JAEA-Research 2024-001

Annex 3 Accuracy of Vertical Response of Reactor Building
The inspection guide for earthquake -resistant design and construction certification
stipulates the need to ensure the appropriate verification of stress resulting from seismic
forces in both horizontal and vertical directions . Furthermore, the guide emphas izes theconsideration of simultaneity of responses, especially when accounting for the phasecharacteristics of seismic motion in each direction or the three-dimensional response
characteristics of buildings and structures . Methods such as maintaining consistent
response values across each direction in each time history are recommended for
addressing simultaneity of responses . Hence, we assess the precision of each responsecomponent by comparing the results of the analysis with the observed data.
Here, we show the examination result of the effect of ground coupling between
horizontal and vertical motion on the response during a simulation analysis of anearthquake observation record. The simulation analysis used the main shock record fromthe Reactor 7 building of the Kashiwazaki -Kariwa Nuclear Power Station of the Tokyo
Electric Power Company Holdings during the Niigataken Chuetsu-oki Earthquake in 2007.
3.1. Analysis model and analysis conditions
A seismic response analysis through time history response analysis was conductedbased on the analysis conditions listed in Appendix 1, 2.1.1. Fig.3 -1 shows the overview
of the analysis model.
Fig.3-2 shows the earthquake observation record from above the building basemat. The
input seismic motion was prepared by pulling down this observation record from above thebasemat to the bottom of the analysis model to enter it from the bottom of the analysis
model shown in Fig.3-1.

Fig.3-1 Analysis model overview- 105 -

JAEA-Research 2024-001

Obs erv ation rec ord abov e bas emat (NS)F ou ri er s pe c t r um (c m / s )A c c el e r ati o n (c m / s 2 )Observation record
above basemat (NS)T i m e (s ec )P er i o d (s ec )P er i o d (s ec )A c c el e r ati o n (c m / s 2 )Observation record
above basemat (UD)T i m e (s ec )F ou ri er s pe c t r um (c m / s )A c c el e r ati o n (c m / s 2 )T i m e (s ec )F ou ri er s pe c t r um (c m / s )Obs erv ation record abov e bas emat (EW)

Observation record
above basemat (EW)

Obs erv ation record abov e bas emat (UD )P er i o d (s ec )Fig.3-2 Earthquake observation record from above the basemat(Left: Acceleration waveform, Right: Fourier spectrum)- 106 -

JAEA-Research 2024-001

3.2. Characteristics of input seismic motion
Fig.3-3 shows the input seismic motion to the analysis model. A large peak occurred
near 11–12 Hz in the input seismic motion in the EW and UD directions. Though small,the same peak was observed in the NS direction. As no peak is observed near thisfrequency in the observation records for the structure basemat, there are several possible
explanations, including the wave of this frequency significantly damping in the ground,the vertical movement at the basemat observation position being canceled by therotational motion accompanying the horizontal motion of the structure, or the existence ofa vibration mode wherein the structure basemat is the node.

In any case, the structure

vibration in the EW direction suggests the occurrence of the influence of couplingA c c el e r ati o n (c m / s 2 )F ou ri er s pe c t r um (c m / s )between the horizontal and vertical motions near 11 –12 Hz.

A c c el e r ati o n (c m / s 2 )T i m e (s ec )T i m e (s ec )F ou ri er s pe c t r um (c m / s ) F ou ri er s pe c t r um (c m / s )A c c el e r ati o n (c m / s 2 )T i m e (s ec )F re q ue nc y (H z )F re q ue nc y (H z )F re q ue nc y (H z )Fig.3-3 Input seismic motion to the analysis model(Left: Acceleration waveform, Right: Fourier spectrum)3.3. Discussion of the response result
3.3.1 Discussion considering the floor response spectrum
Fig.3-4 shows the observation records at the above basemat and 3 rd floor as well as thecomparison of the acceleration response spectrum of the elastic analysis result. While theresponse spectrums at the above basemat almost identical, but the analytical results of thevertical response spectra at 3rd floor are larger than the observation records of the 3 rdfloor. The observed discrepancy may stem from the horizontal response, specifically the- 107 -

JAEA-Research 2024-001

peak at the period of 0.08 seconds (12.5 Hz). Given the absence of this peak in theobservation record, it suggests that it may be an artifact introduced during the numericalcalculation. This occurrence is likely influenced by the coupling mode near the verticalnatural frequency of 11–12.5 Hz between the ground and the building, as depicted in
Fig.3-5.
Further, other possible reasons for the large discrepancy between the observation record
and the analysis result at 3F include the difference between the analysis model and thereal structure, an example of which is the effect of the fact that the partition walls, etc.,
other than the earthquake resistance walls, or secondary members such as joists, were notmodeled, or the effect of the nonlinear behavior of the ground not being considered. To
improve the reproducibility of vertical response, it is conside red necessary to verify these
possible influences and create a more realistic model. However, because the model was
produced based on published information, further refinement would be difficult at thistime. Therefore, the acceleration time history wavefo rms of the exterior walls near theobservation position in 3F, which is inferred to have large vertical stiffness of the floor
surface, were similarly compared. Fig.3 -6 shows the floor response spectrum at theexterior wall part of 3F. The horizontal respo nse largely matches the result from theobservation point, and the vertical response was still somewhat larger than the observation
point. However, it shows that the peak near the period of 0.08 seconds was significantly
lower than the result from the obse rvation point.

From these findings, it is inferred that,in reality, the vertical stiffness of the center of interior walls in a state that is unified withthe exterior walls.

- 108 -

Ob s .

NS

A na l y s i sA c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )JAEA-Research 2024-001

A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )Ob s .
A na l y s i s

A na l y s i s

P er i o d (s ec )Ob s .
A na l y s i sA c c el e r at i o n re s p o ns e s p ec t rum (c m /s 2 )A c c el e r at i o n re s p o ns e s p ec t rum (c m /s 2 )

Obs.

EW

P er i o d (s ec )UD

A na l y s i s

P er i o d (s ec )P er i o d (s ec )

EW

Obs.

NS

Obs.

UD

A na l y s i s

P er i o d (s ec )P er i o d (s ec )(1) Above basemat(2) 3F (Observation position)

Fig.3-4 Comparison of floor response spectrums (h = 5%)- 109 -

JAEA-Research 2024-001

11 Hz

12 Hz

12.5 Hz
Fig.3-5 Coupling mode between the ground and the building- 110 -

A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )JAEA-Research 2024-001

Ob s .

NS

A na l y s i s

E x t eri o r w al lA c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )P er i o d (s ec )Ob s .

EW

A na l y s i sA c c el e r at i o n re s p o ns e s p ec t rum (c m /s 2 )P er i o d (s ec )Ob s .

UD

A na l y s i s

P er i o d (s ec )Fig.3-6 Comparison of floor response spectrums ( h = 5%) (Exterior wall part of 3F)- 111 -

JAEA-Research 2024-001

Annex 4 Effect of Nonlinear Soil-structure Interaction
In this sensitivity analysis, we performed an elastic time history response analysis on
the reactor building, incorporating side separation and sliding (excluding bottom uplift),using the main shock record from the Reactor 7 bui lding of the Kashiwazaki-Kariwa
Nuclear Power Station during the Niigataken Chuetsu-oki Earthquake in 2007. The
examination results, specifically addressing the impact of whether side separation or
sliding was considered, are presented herein.
4.1. Analysis model and analysis conditions
A seismic response analysis was conducted based on the analysis conditions listed inAppendix 1, 2.1.1. Fig.4-1 shows the overview of the analysis model. The aspects thatdiffer from the analysis conditions in 2.1.1 are as follows: Side separation and sliding is
considered by inserting a non-linear joint into the interface between the building and theground. In this example, the stiffness of the nonlinear joint when compressed is 1,000
times that of the ground that is in contact with the side of the building.

For the sliding

on the side, a dynamic friction coefficient 0.35 was set. The time interval of the time
history response analysis was set to 1/1000 second(s) for nonlinear analysis.

Fig.4-1 Overview of the analysis model- 112 -

JAEA-Research 2024-001

4.2. Analysis result
The subsequent discussion will concentrate on the distinctions arising from theconsideration of side separation or sliding. The key representative nodes and each centerof the building are identical to those illustrated in Fig.2-4. Specifically, the RA center
denotes the midpoint along the western exterior wall, where R4A corresponds to thecentral node, and R1A and R7A correspond to the node s at each respective end (seeFig.2-4).
Comparison of the observation record and the analysis result
4.2.1.1 Comparison of maximum response acceleration distributions
Figure 4-2 shows the maximum response acceleration distributions. Unlike the resultthat did not take side separation or sliding into consideration, the result that did consider
it shows extremely high discrepancies in the maximum acceleration below the groundsurface (elevation +12 m). This is because of the occurrence of an underground recon tact
phenomenon between the building and the ground when side separation or sliding wereconsidered, resulting in spike-shaped acceleration.

Therefore, high frequencies above

100 Hz were regarded as vibrations in numerical analysis, and Fig.4 -3 shows the result
after applying a low-pass filter.

Thus, it can be confirmed that the maximum response

acceleration distribution is an approximate match to that of the elastic analysis.
Fig.4-4 shows examples of the acceleration time history and Fourier spectrum for the
representative node. The folding frequency was 500 Hz. In the analysis results that tookside separation or sliding into account, a peak occurred at 250 Hz, and that peak can be
confirmed to have been removed with the application of a low -pass filter. The acceleration
time history and Fourier spectrum after applying the filter show nearly the same results as
those of the case where side separation and sliding were not considered. Thus, in thisexample, whether or not side separation or sliding were considered, either had little
influence on the building response.

- 113 -

JAEA-Research 2024-001

E l ev at i o nGLObservation

Rep. nodes

Rep. nodes(a) X(NS) direction(b) Y(EW) direction

Rep. nodes(c) Z(UD) direction(1) Separation and sliding on the side not consideredE l ev at i o n

Rep. nodes

Rep. nodes

Rep. nodes

GL(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(2) Separation and sliding on side considered
Fig.4-2 Maximum response acceleration distribution (RA center)- 114 -

JAEA-Research 2024-001

E l ev at i o nGLObservation

Rep. nodes

Rep. nodes(a) X(NS) direction(b) Y(EW) direction

Rep. nodes(c) Z(UD) direction(1) Separation and sliding on the side not consideredE l ev at i o nGLObservation
Rep. nodes

Rep. nodes(a) X(NS) direction(b) Y(EW) direction

Rep. nodes(c) Z(UD) direction(2) Separation and sliding on the side considered (with 100 Hz low -pass filter)
Fig.4-3 Maximum response acceleration distribution (RA center)- 115 -

JAEA-Research 2024-001

Acceleration (cm/s 2 )Without filter
With filter

Time (sec)(1) Acceleration time history of the representative node
Fourier spectrum (cm/s)

Without filter
With filter

Frequ ency (Hz)(2) Fourier spectrum of the representative nodeFig.4-4 Comparison example of applying and not applying a 100 Hz low -pass filter
4.2.1.2 Comparison of floor response spectrum
Fig.4-5 and Fig.4-6 show the observation records from above the basemat and 3F aswell as the comparison of the acceleration response s pectrum from the analysis result. The
response spectrum that takes side separation and sliding into account above the basemat is
an approximate match with the observation record at periods that are longer than 0.1
second(s). However, because of the influence of the spike -shaped acceleration, verticalamplitude was large during the periods that are shorter than 0.1 second(s).

Th e cause of

the peak near the 0.1-second period is inferred to be the effect of taking side separationand sliding into account.
Meanwhile, the response spectrum of 3F is almost the same as that of the analysis result
where side separation or sliding were not considered, and the horizontal response largely
matches the observation record. However, the vertical response was larger than theobservation record overall.

- 116 -

Ob s .
A na l y s i sA c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )JAEA-Research 2024-001

P er i o d (s ec )Ob s .
A na l y s i s

Obs.
A na l y s i s

P er i o d (s ec )Ob s .
A na l y s i sA c c el e r ati o n re s p o ns e s p ec t rum (c m /s 2 )P er i o d (s ec )A c c el e r at i o n re s p o ns e s p ec t rum (c m /s 2 )A na l y s i sA c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )P er i o d (s ec )Obs.

P er i o d (s ec )Obs.
A na l y s i s

P er i o d (s ec )Fig.4-5 Comparison of floor response spectrum ( h = 5% (Above the basemat)(Left: Side separation/sliding not considered; Right: Side separation/sliding considered)- 117 -

Ob s .
A na l y s i sA c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )JAEA-Research 2024-001

P er i o d (s ec )Ob s .
A na l y s i s

Obs.
A na l y s i s

P er i o d (s ec )Ob s .
A na l y s i sA c c el e r ati o n re s p o ns e s p ec t rum (c m /s 2 )P er i o d (s ec )A c c el e r at i o n re s p o ns e s p ec t rum (c m /s 2 )A na l y s i sA c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )A c c el e r ati o n re s p o ns e s p ec t rum (c m / s 2 )P er i o d (s ec )Obs.

P er i o d (s ec )Obs.
A na l y s i s

P er i o d (s ec )Fig.4-6 Comparison of floor response spectrum ( h = 5%) (Exterior wall of 3F)(Left: Side separation/sliding not considered; Right: Side separation/sliding considered)- 118 -

JAEA-Research 2024-001

4.2.2 Maximum response acceleration distribution diagram
Fig.4-7 and Fig.4-8 show distribution diagrams for the maximum response acceleration.
In the contour where the low -pass filter was not applied, an extremely large maximum
response acceleration was observed at the outer periphery of B1F because of theunderground recontact phenomenon of the building and the ground due to side separationand sliding. However, when the 100 Hz low -pass filter was applied, the result was almost
the same as that of the case where side separation and sliding was not considered.
Meanwhile, the result from 3F was almost the same as that of the case where side
separation and sliding was not considered, regardless of whether the low -pass filter wasapplied.

- 119 -

JAEA-Research 2024-001(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(1) Separation and sliding on the side not considered(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(2) Separation and sliding on the side considered (without filter)(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(3) Separation and sliding on the side considered (with 100 Hz low -pass filter)
Fig.4-7 Maximum response acceleration distribution diagram: B1F ( Elevation +4.8 m)- 120 -

JAEA-Research 2024-001(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(1) Separation and sliding on the side not considered(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(2) Separation and sliding on the side considered (without filter)(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(3) Separation and sliding on the side considered (with 100 Hz low -pass filter)
Fig.4-8 Maximum response acceleration distribution diagram: 3F ( Elevation +23.5 m)- 121 -

JAEA-Research 2024-001

4.2.3 Maximum response displacement
4.2.3.1 Height direction distribution diagram
Fig.4-9 shows the height direction distribution diagram of the maximum response
displacement. Here, the average of the representative nodes (12 nodes) and that of every
node are shown. Further, the maximum and minimum values of the representative nodes
and every node at each floor are shown with blue bars and red bars, respectively. The
result was almost the same as that of the case in which side separation and sliding were
not taken into consideration, and no influence of side separation and sliding was observed.
E l ev at i o n

GLAll nodes

All nodes

All nodes

Rep. nodes

Rep. nodes

Rep. nodes(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(1) Separation and sliding on the side not consideredE l ev at i o n

GLAll nodes

All nodes

All nodes

Rep. nodes

Rep. nodes

Rep. nodes(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction(2) Separation and sliding on side considered
Fig.4-9 Maximum response displacement distribution (RA center)- 122 -

JAEA-Research 2024-001

4.2.4 Separation and sliding of the side of the basement of the building and the ground
The ratio of axial direction maximum stress distribution and maximum vertical shear
stress of the side(s) are shown in Fig.4 -10 and Fig.4-11.

According to the result of the

maximum stress distribution in the axial direction of the side when side separation andsliding were considered, the maximum tensile stress from the elevation 6.8 m to theground surface (elevation 12.3 m) was almost 0, suggesting that separation was occurring.
The maximum vertical shear stress ratio of the side separation was 0.35 at every position,
indicating that sliding was occurring.
Thus, as described above, the influence on the building response was analyzed in termsof whether side separation and sliding were considered; in this example, it was verified
that taking side separation and sliding into account does not make a significant difference
to the overall building response in comparison to not taking them into account. However,it was verified that on the underground floors, spike -shaped acceleration occurs becauseof the recontact phenomenon caused by side separation and sliding. Thus, precautions
must be taken to obtain realistic responses, such as the application of an appropriate
low-pass filter.

- 123 -

Ho ri z o n t a l c o o r di n a t es ( m )

South
side

H o ri z o nt al c o o rd i n at es (m )Ea s t s i d e
Ho ri z o n t a l c o o r di n a t es ( m )

Wes t
side
H o ri z o nt al c o o rd i n at es (m )Ma x . t en s i l e s t re s s ( k N / m 2 ) Ma x . t en s i l e s t re s s ( k N / m 2 ) Ma x . t en s i l e s t re s s ( k N / m 2 )No rt h s i d e

E l ev at i o n

No rt h s i d e
Ho ri z o n t a l c o o r d i n a t es ( m )

South
side

H o ri z o nt al c o o rd i n at es (m )Ea s t s i deHo ri z o n t a l c o o r d i n a t es ( m )Ma x . t en s i l e s t re s s ( k N /m 2 )Ma x . t en s i l e s t re s s ( k N /m 2 )Ma x . t en s i l e s t re s s ( k N / m 2 ) Ma x . t en s i l e s t re s s ( k N / m 2 ) Ma x . t en s i l e s t re s s ( k N / m 2 )JAEA-Research 2024-001

Wes t
side
H o ri z o nt al c o o rd i n at es (m )(1) Separation and sliding on the(2) Separation and sliding on side

side not considered

considered

Fig.4-10 Maximum axial direction stress distribution on the side

- 124 -

JAEA-Research 2024-001

Max. vertical shear stressratio (τ /σ )No rt h s i d e

No rt h s i d e

Ho ri z o n t a l c o o r d i n a t es ( m )Ho ri z o n t a l c o o r d i n a t es ( m )

South
side

Max. vertical shear stressratio (τ /σ )Max. vertical shear stressratio (τ /σ )Max. vertical shear stressratio (τ /σ )E l ev at i o n

South
side

H o ri z o nt al c o o rd i n at es (m )Ea s t s i d eMax. vertical shear stressratio (τ /σ )Max. vertical shear stressratio (τ /σ )H o ri z o nt al c o o rd i n at es (m )Ea s t s i deHo ri z o n t a l c o o r d i n a t es ( m )

Wes t
side

Max. vertical shear stressratio (τ /σ )Max. vertical shear stressratio (τ /σ )Ho ri z o n t a l c o o r d i n a t es ( m )

Wes t
side

H o ri z o nt al c o o rd i n at es (m )H o ri z o nt al c o o rd i n at es (m )(1) Separation and sliding on the(2) Separation and sliding on side

side not considered

considered

Fig.4-11 Maximum vertical shear stress ratio distribution on the side

- 125 -

JAEA-Research 2024-001

Annex 5 Effect of Nonlinear Constitutive Model of Reinforced Concrete
In this sensitivity analysis, we concentrated on evaluating the effects of constitutive
models implemented in analysis codes. To identify this, simulation analyses of theshaking table test for the reinforced concrete earthquake -resistant wall (NUPEC) 3 wereconducted using two finite element analysis codes, namely FINAS/STAR (F/S) andFINAL.
5.1. Analysis modelThis

experimentwasconducted

toverifythedynamic

elasto -plasticityofearthquake-resistant walls. The specimen consists of web walls and flange walls. The web
walls and flange walls were modeled with shell elements, and the nonlinearity of thereinforced concrete wall material was taken into account. The upper slabs and the basemat
slabs were modeled with solid elements and were regarded as elastic bodies. A full model
was used for FINAS/STAR, and a half model was used for FINAL to conduct the analysis.
Fig.5-1 and Fig.5-2 show the analysis models for FINAS/STAR and FINAL,
respectively.

- 126 -

JAEA-Research 2024-001

Added mass
(Solid element)

Upper slab
(Solid element)

Flange seismic wall
(Shell element)

Web seismic wall
(Shell element)

Base slab(Solid element)

Excitation direction

Orthogonal directionof excitation

Upper slab

Upper slab

Web seismic
Wall (t=75mm)

Flange seismic
Wall (t=100mm)

Ba s e s l a b

Ba s e s l a b

Ad d ed m a s s
Web wall
Fl a n g e w a l l

Fig.5-1 Analysis model FINAS/STAR

Fig.5-2 Analysis model FINAL- 127 -

JAEA-Research 2024-001

5.2. Analysis conditions
5.2.1 Analysis parameters
Table 5-1 shows the material parameters used in the analysis with FINAS/STAR andFINAL. Fig.5-3 shows the stress–strain relationship used for the analysis, and Fig.5 -4
shows the stress–strain relationship of the test results.
Table 5-1 Material parameters

Analysiscode
F INAS/STARF INAL

Concrete
Peak
Poisson’s
strainratio
εcν

Young’s
Modulus E c
N/mm 2

Densityγ
N/mm 2Yield
stress σ y
N/mm 2

Rebar
Young’smodulus E s
N/mm 22.24

0.00220.2

2.60E+04

24.0

383.4

1.85E+05

2.23

0.00250.2

2.29E+04

23.0

383.2

1.84E+05

Compressive
strength F c
N/mm 2Tensilestress σ c r
N/mm 2

28.6
28.6*Tensile characteristics

F/S: Izumo et al. model 4 C = 2.0, FINAL: Naganuma/Yamaguchi model 5

Compression characteristics

F/S: Maekawa model 6 , 7 , FINAL: Revised Ahmad model 83530

S tr応力(MPa)es s ( MP a )

25
20
15
10
前川モデル
Ma e k a w a m o de l
50

修正Ahmadモデル
R ev i s ed
A hm a dm od el

0

0.001

0.002

0.003

Sひずみ(-)
tr ai n( - )

0.004

0.005

0.006

Fig.5-3 Stress-strain relationship used for the
analysis- 128 -

JAEA-Research 2024-001(C i rc um f er e nt i al s t r ai n)

Lo n gi t u di n al ( ax i al ) s t r ai n

Fig.5-4 Stress-strain relationship of the test result 3- 129 -

JAEA-Research 2024-001

5.2.2 Analysis conditions of seismic response analysis
Table 5-2 shows the dynamic analysis conditions of FINAS/STAR and FINAL.
Table 5-2 Analysis conditions
FINAS/STAR

FINAL

Direct integral method

Direct integral method

Numerical

Newmark-β method

Newmark-β method

integration(β = 1/4, γ = 1/2)

(β = 1/4, γ = 1/2)

Nonlinear

Tangential stiffness method

Tangential stiffness method

analysis(tangential stiffness method is

methodpartially used within the

Analysis
methodmethodconstitutive law)
Repetition

Maximum 3 times

None

How to treat

Add residual to the load term of

Add residual to the load term of

residual

the next step.

the next step.

Integral time

See the analysis case table.

See the analysis case table.

Initial stiffness proportional type

Initial stiffness proportional

dampingtype damping

β = 0.000193

β = 0.000261(h = 0.8% in relation to the 1st(h = 1.1% in relation to the 1st

frequency 13.2 Hz)

frequency 13.4 Hz)

numberintervalDamping

5.2.3 Analysis
The analyses are conducted in the format shown in the right column of Table 5 -3.
Perform integrated structural analysis where RUN2d to RUN5 are entered in order after
conducting a dead load analysis. (As RUN1 is an elastic behavior, it is analyzed
separately.)
Integral time interval is changed for each input according to the size of the input motion,
as shown in Table 5-4.

- 130 -

JAEA-Research 2024-001

Table 5-3 Analysis cases
RUN1

Self-weight → RUN1

RUN2d

Self-weight

RUN3→ RUN2d→ RUN3RUN4→ RUN4RUN5→ RUN5

Table 5-4 Integral time interval
FINAS/STAR

FINAL

RUN1

0.002 s0.0005 s

RUN2d0.0005 s

0.0005 s

RUN30.0005 s

0.0005 s

RUN40.0002 s

0.005~0.0001 s ※RUN50.0002 s

0.005~0.0001 s ※※ FINAL is automatically adjusted by its program to ensure that the increase by one (1) stepof the input acceleration is 10 Ga l or less. The minimum is 0.0001 s.

- 131 -

JAEA-Research 2024-001

5.2.4 Input seismic motion
Fig.5-5 shows the input seismic motion into the analysis model and inertia force –horizontal displacement relationship diagram. The basemat slab response acceleration
obtained from the test result is entered into the bottom of the model as the input seismic

Acceleration (cm/s 2)

Acceleration (cm/s2)

motion. The boundary condition of the bottom of the model is fixed.

Time (s)Acceleration (cm/s2)

Acceleration (cm/s2)

Time (s)Time (s)Inertia force (kN)

Experiment

Displacement (mm)Time (s)Acceleration (cm/s2)

Acceleration (cm/s2)

Time (s)Inertia force (kN)Time (s)Inertia force (kN)

Experiment

Displacement (mm)Experiment

Displacement (mm)

Inertia force (kN)

Inertia force (kN)

Experiment

Displacement (mm)Experiment

Displacement (mm)Fig.5-5 Comparison of input seismic motion waveforms and inertia force -horizontal
displacement relationship- 132 -

JAEA-Research 2024-001

5.3. Analysis result
5.3.1 Analysis result of each case
The time history acceleration waveforms of the upper slabs, acceleration response
spectrum (h = 5%), and acceleration -displacement relationships shown in Fig.5 -6 wereobtained and compared to the experiment results. The results are shown in Fig.5-7 to
Fig.5-11.
・ Time history acceleration waveform
The results of FINAS/STAR and FINAL between RUN1 and RUN3 were consistent withthe experiment results. In RUN4, some discrepancies with the experiment results begin
to appear between 4 and 5 seconds in the period and amplitude, but the tendencies
generally match. In RUN5, the results were mostly reproduced until around 4 seconds,
when the specimen was destroyed.
• Acceleration response spectrum (h = 5%)
The results between RUN1 and RUN3 matched the experiment results well. After RUN4,
the result of FINAS/STAR was smaller than the experiment result at the 0.1 second
period and larger at the 0.13 second period. Thus, it is inferred that the decrease instiffness was smaller than the experiment result. RUN5 was almost completely
reproduced. Thus, the results of both programs mostly match and correspond well withthe experiment.

Fig.5-6 Input seismic motion output position- 133 -

Acceleration (cm/s 2)

JAEA-Research 2024-001

E x p e ri m e nt

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)Time (sec)Full range

Enlargement (2–6 s)Acceleration (cm/s 2)

Transfer function (-)

Response acceleration waveform

Frequency (Hz)Period (sec)Transfer function
Acceleration (cm/s 2)

Acceleration (cm/s 2)

Acceleration response spectrum (h = 5%)

Displacement (mm)Displacement (mm)Acceleration–displacement relationshipFig.5-7 Result of RUN1 (Upper slab)- 134 -

Acceleration (cm/s 2)

JAEA-Research 2024-001

E x p e ri m e nt

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)
Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)Time (sec)Full range

Enlargement (2–6 s)2Acceleration (cm/s )Transfer function (-)

Response acceleration waveform

Period (sec)Frequency (Hz)Transfer function

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Acceleration response spectrum (h = 5%)

Displacement (mm)Displacement (mm)Acceleration–displacement relationshipFig.5-8 Result of RUN2d (Upper slab)- 135 -

Acceleration (cm/s 2)

JAEA-Research 2024-001

E x p e ri m e nt

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)Time (sec)Full range

Enlargement (2–6 s)Acceleration (cm/s 2)

Transfer function (-)

Response acceleration waveform

Frequency (Hz)Period (sec)Transfer function

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Acceleration response spectrum (h = 5%)

Displacement (mm)Displacement (mm)Acceleration–displacement relationshipFig.5-9 Result of RUN3 (Upper slab)- 136 -

Acceleration (cm/s 2)

JAEA-Research 2024-001

E x p e ri m e nt

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)Time (sec)Full range

Enlargement (2–6 s)Acceleration (cm/s 2)

Transfer function (-)

Response acceleration waveform

Frequency (Hz)Period (sec)Transfer function

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Acceleration response spectrum (h = 5%)

Displacement (mm)Displacement (mm)Acceleration–displacement relationshipFig.5-10 Result of RUN4 (Upper slab)- 137 -

Acceleration (cm/s 2)

JAEA-Research 2024-001

E x p e ri m e nt

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Time (sec)Time (sec)Time (sec)Full range

Enlargement (2–6 s)Acceleration (cm/s 2)

Transfer function (-)

Response acceleration waveform

Frequency (Hz)Period (sec)Transfer function

Acceleration (cm/s 2)

Acceleration (cm/s 2)

Acceleration response spectrum (h = 5%)

Displacement (mm)Displacement (mm)Acceleration–displacement relationshipFig.5-11 Result of RUN5 (Upper slab)- 138 -

JAEA-Research 2024-001

Annex 6

Effect of Finite Element Program

In this sensitivity analysis, we explored the influence of the finite element type
implemented in the analysis codes. The element type under examination is a shell element,
and the comparison was made between two analysis codes, namely FINAS/STAR and MSC
Nastran.
6.1. Analysis model and analysis conditions
There are many types of finite elements, including beam elements, shell elements, andsolid elements, and the same element type can have different characteristics and accuracy
depending on the formulation. Regarding accuracy, the mor e detailed the mesh, the moreaccurate the result. Here, an example where the difference in the accuracy of plane shapeelements was examined is discussed.
Two element types based on different formulations ( linear quadrilateral (MITC) andlinear quadrilateral (CQUAD4)) were examined. Table 6 -1 shows the list of analysis cases,
and Fig.6-1 shows an overview of the analysis model.
Table 6-1 Analysis case list
No.

Element type

SolverAnalysis model

Boundary condition

Case01

Linear

FINAS/STAR

Mesh division 1

Constrain thequadrilateral

peripheral nodes(MITC)
Case02

LinearMSC NastranMesh division 1

quadrilateral

Constrain the
peripheral nodes(CQUAD4)
Case03

Linear

FINAS/STARquadrilateral

Mesh division 2

Constrain the
peripheral nodes(MITC)- 139 -

JAEA-Research 2024-001

N um be r of n o de s : 1 4 5N um be r of e l em en ts : 11 2

(1) Mesh division 1

N um be r of n o de s : 4 9 3
N um be r of e l em en ts : 44 8(2) Mesh division 2
Fig.6-1 Overview of the analysis model- 140 -

JAEA-Research 2024-001

6.2. Analysis result
6.2.1 Influence of difference in finite element formulation on eigenvalue analysis result
Fig.6-2 shows the comparison of mode shapes based on the MITC element (division 1)
and CQUAD4 element (division 1), and Table 6 -2 shows the comparison of their 1st
frequencies to verify the influence of the differences in finite element formulations on the
eigenvalue analysis result. According to Fig.6-2, the mode shapes of the MITC element(division 1) and CQUAD4 element (division 1) were largely the same. According to thecomparison of the 1st natural frequencies in Table 6-2, there was about a 15% difference
between the 1st natural frequency of the MITC element (division 1) and that of the
CQUAD4 element (division 1).
1st mode

2nd mode(1) Mode shape of MITC element (division 1)(2) Mode shape of CQUAD4 element (division 1)
Fig.6-2 Comparison of mode shapes with different finite element formulations

Table 6-2 Comparison of 1st natural frequencies with different finite element formulations
Freq.

PeriodStimulus coefficient

Effective mass ratio

No.

Hz

s

X

Y

Z

X

Y

Z

Case01

12.634

0.079

0.000

0.000

33.689

0.000

0.000

0.704

Case02

10.881

0.092

0.000

0.000

-34.153

0.000

0.000

0.723

- 141 -

JAEA-Research 2024-001

6.2.2 Influence of mesh division on eigenvalue analysis result
Eigenvalue analysis using linear quadrilateral element type (MITC), whose meshdivision is 1, as well as the element that divided it by 4 in its short side direction (MITC
element (division 2)), was conducted to verify the influence of mesh division. Fig.6 -3
shows the comparison of mode shapes, and Table 6-3 shows the comparison of 1st natural
frequencies. The comparison of mode shapes in Fig.6-3 shows that the mode shape of the
MITC element (division 1) and that of the MITC element (division 2) were almost thesame. The comparison of 1st natural frequencies in Table 6-3 shows that the result of the
MITC element (division 2), which is a finer mesh, had 13% less 1st natural frequency than
the result of the MITC element (division 1). It was verified that its difference with the 1stnatural frequency of CQUAD4 element (division 1), which is 10.881 Hz, is about 1%.
While further verification of its convergence is necessary, thi s examination verified thatfor the accuracy of out-of-plane bending, CQUAD4 is better than MITC.
In finite element analysis, it is necessary to understand and utilize an appropriate meshfor each element through sensitivity analysis.
1st mode

2nd mode(1) Mode shape of MITC element (division 1)(2) Mode shape of MITC element (division 2)
Fig.6-3 Comparison of mode shapes with different mesh divisions- 142 -

JAEA-Research 2024-001

Table 6-3 Comparison of 1st natural frequencies with different mesh divisions
Freq.

PeriodStimulus coefficient

Effective mass ratio

No.

Hz

s

X

Y

Z

X

Y

Z

Case01

12.634

0.079

0.000

0.000

33.689

0.000

0.000

0.704

Case0311.011

0.091

0.000

0.000

34.289

0.000

0.000

0.583

- 143 -

JAEA-Research 2024-001

Annex 7 Effect of Mesh sizes of Finite Elements
In this sensitivity analysis, we investigated the impact of mesh size on seismic response
analysis. To accomplish this, we examined two models with varying mesh sizes in
response analysis of the Reactor 7 building of the Kashiwazaki-Kariwa Nuclear Power
Station subjected to the Niigataken Chuetsu-oki Earthquake in 2007.
7.1. Analysis model and analysis conditions
Fig.7-1 shows two types of analysis models, namely, the standard model and detailed
mesh model.
The standard model divides the span between reference lines by 4 or 5, and the floor
height direction is divided by 4 or 5 with 2 m as the baseline. The detailed mesh mode l
was created as an analysis model with each side of the element further divided by four
(4x4 division in length and breadth). Other analysis conditions were the same as those inAppendix 1, section 2.1.1.

- 144 -

JAEA-Research 2024-001

Standard model

Detailed mesh model(1) Bird’s-eye view

Standard model

Detailed mesh model(2) 1F Plan

Fig.7-1 Analysis model diagram- 145 -

JAEA-Research 2024-001

7.2. Analysis result
7.2.1 Maximum response acceleration and maximum response displacement
Fig.7-2 and Fig.7-3 show the comparisons of the height direction distributions of the
maximum response acceleration and maximum response displacement. The solid line in
the figure indicates the average of every node in the building model. The broken line
indicates the average of the representative nodes of the building model. The black line
indicates the analysis result with the st andard model. The red line indicates the analysis
result with the detailed mesh model. Overall, they correspond with each other well.
However, some difference with the standard model was observed at 4F ( elevation +31.7m) and beyond. This is inferred to be caused by the change in the natural frequency
outside the wall with the mesh becoming finer, resulting in the changes in response
characteristics.
E l ev at i o nGLStandard(All nodes)
Standard(Rep. nodes)
Detailed(All nodes)
Detailed(Rep. nodes)(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction

Fig.7-2 Comparison of maximum response acceleration distributions- 146 -

JAEA-Research 2024-001

E l ev at i o nGLStandard(All nodes)
Standard(Rep. nodes)
Detailed(All nodes)
Detailed(Rep. nodes)(a) X(NS) direction(b) Y(EW) direction(c) Z(UD) direction

Fig.7-3 Comparison of maximum response displacement distribution s- 147 -

JAEA-Research 2024-001

7.2.2 Floor response spectrum
Fig.7-4 and Fig.7-5 show the comparisons between floor response spectra using thestandard model and the detailed mesh model from B3F and 3F. Based on the fact that theresults of the standard model and the detailed mesh model are not significantly different,
it can be understood that, with only this degree of differen ce in the mesh size, the impact
on the floor spectrum in 3F is small.

Standard(Rep. nodes)
Detailed(Rep. nodes)

P er i o d (s ec )P er i o d (s ec )(a) X(NS) direction
Fig.7-4(b) Y(EW) direction

P er i o d (s ec )(c) Z(UD) direction

Comparison of floor response spectrum h = 5% ( B3F, elevation −8.2 m)

Standard(Rep. nodes)
Detailed(Rep. nodes)

P er i o d (s ec )P er i o d (s ec )(a) X(NS) direction
Fig.7-5(b) Y(EW) direction

P er i o d (s ec )(c) Z(UD) direction

Comparison of floor response spectrum h = 5% ( 3F, elevation +23.5 m)- 148 -

JAEA-Research 2024-001

References
1 IAEA, Review of Seismic Evaluation Methodologies for Nuclear Power Plants Based on
a Benchmark Exercise, IAEA -TECDOC-1722, 2013.
2 Japan Electric Association, Regulations for Earthquake -Resistant Design Technology
for Nuclear Power Stations, JEAC4601 -2008, 2009.
3 Nuclear Engineering Test Center, Elasto‐plasticity test of reactor building, Tests
related to dynamic restoring force, 1992, 385p.
4 Junichi Izumo, et al., Analytical model for reinforced concrete panel elements
subjected to in-plane forces, Concrete Journal, Vol.25, No.9, 1987, pp.107-120.
5 Kazuhiro Naganuma, Tsuneo Yamaguchi, Tension Stiffening Model under In -plane
Shear Stress, Summaries of technical papers of annual meeting, Architectural Instituteof Japan, Structure Ⅱ, 1990, pp.649 -650.
6 Koichi Maekawa, Naoyuki Fukuura, Reconstruction of a spatial average composition
model of flat RC elements with pseudo orthogonal bidirectional cracks, Proceedings of
JSCE, No.634/V-45, 1999, pp.157-176.
7 Naoyuki Fukuura, Koichi Maekawa, Constitutive law o f spacial averaging of flat RC
elements with non‐orthogonal crack groups, Proceedings of JSCE, No.634/V -45, 1999,
pp.177-195.
8 Kazuhiro Naganuma, Stress–strain relationship for concrete under triaxial compression,
The Architectural Institute of Japan’s Jo urnal of Structural and Construction
Engineering, Issue 474, 1995, pp.163 -170.

- 149 -

This is a blank page.

JAEA-Research 2024-001

Attachment 2 Analysis Example
This appendix illustrates the application of the “Standard Guidelines” for the Simulation
Analysis of the Observation Records of Reactor Buildings at the Kashiwazaki -Kariwa
Nuclear Power Station. The particulars of this example are expounded upon in accordancewith the items outlined in the standard guidelines listed below.
1. Purpose and object of analysis
2. Analysis domain
3. Creation of the geometric model
4. Creation of the structural model
5. Mass model
6. Material model
7. Mathematical model of damping
8. Boundary joint model
9. Input seismic motion
10. Initial state model
11. Condition setting for numerical analysis
12. Examination and validation of analysis results
13. Documentation
References- 151 -

This is a blank page.

JAEA-Research 2024-001

1.

Purpose and object of analysis

1.1

Purpose of Analysis

The purpose of analyzing this example is to v alidate the seismic response analysis of thereactor buildings using a 3D FEM model (soil -structure interaction) through the simulation
analysis of an observation record. We used the main shock record from the Reactor 7 buildingof the Kashiwazaki-Kariwa Nuclear Power Station (above the basemat and 3F) during the
Niigataken Chuetsu-oki Earthquake in 2007.
1.2

Analysis method

The analysis to be validated involves the seismic response analysis code utilizing a directtime integration method within a Finite Element code, specifically FINAS/STAR version
2019r190925 1 .
1.3Units used

The unit systems used for analysis are as follows: m for length, ton for mass, kN for force,s for time, m/s 2 for acceleration, and m/s for velocity. Gravitational acceleration was set at
g = 9.80665 m/s 2 .
1.4

Analysis plan

Upon embarking on the analysis, an analysis plan was prepared by checking the application
area of the analysis method and examining the validity of the analysis result. This example
is presented in accordance with the analysis plan.
Below is an overview of the observation record used in this analysis example.
1.4.1

Overview of observation record(1)

Arrangement of seismometers

Fig.1-1 shows the arrangement of seismometers.

- 153 -

JAEA-Research 2024-001

Elevation

Cross section
Seismometer

Basemat (B3F)

Fig.1-1 Arrangement of seismometers 2- 154 -

JAEA-Research 2024-001(2)

Observation record

Fig.1-2 and Fig.1-3 show the observation records from above the basemat (B3F) and 3F,
respectively.
Acceleration (cm/s2)

Observation
NS (B3F)

Acceleration (cm/s2)

Time (s)Observation
EW (B3F)

Acceleration (cm/s2)

Time (s)Observation
UD (B3F)

NS (B3F)

Period (s)Acceleration (cm/s2)

Acceleration (cm/s2)

Time (s)EW (B3F)

Acceleration (cm/s2)

Period (s)UD (B3F)

Period (s)Fig.1-2 Observation record from above the basemat (B3F).
(Above: Acceleration time history; Below: Acceleration response spectrum (h = 5 %))- 155 -

JAEA-Research 2024-001

Acceleration (cm/s2)

Observation
NS (3F)

Acceleration (cm/s2)

Time (s)Observation
EW (3F)Time (s)Acceleration (cm/s2)

Observation
UD (3F)NS (3F)

Period (s)Acceleration (cm/s2)

Acceleration (cm/s2)

Time (s)EW (3F)

Acceleration (cm/s2)

Period (s)UD (3F)

Period (s)Fig.1-3 Observation record from 3F(Above: Acceleration time history; Below: Acceleration response spectrum (h = 5 %))1.5 Documentary evidence
The report from the international benchmark project KARISMA ( IAEA-TECDOC-1722) 2
by the IAEA was used as the documentary evidence forming the basis of this report.

- 156 -

JAEA-Research 2024-001

2.

Analysis domain

2.1

Building

The Reactor 7 building of the Kashiwazaki -Kariwa Nuclear Power Station was the objectof analysis. Time history seismic response analysis was performed using the input seismic
wave based on the observation record from the Niigataken Chuetsu-oki Earthquake in 2007.
For the parameters used in the analysis, the data used in the IAEA’s KARISMA report 2 wasused, in principle, for both the ground and the building.
The size of the Kashiwazaki -Kariwa Nuclear Power Station Reactor 7 building is 56.6 m(NS) × 59.6 m (EW); its height is 63.4 m, and it is 37.7 m above ground level. The thicknessof its basemat is 5.5 m, and it is structurally separated from adjacent buildings. Its section
and plan are shown in Fig.2 -1 and Fig.2-2, respectively. In the plan, B3F and B1F are shownas the representative planes, and the sign of reference lines are also shown.
Other setting characteristics are shown below.
 Wall: Supporting wall and earthquake resistant wall (There are no documents for othercomponents).
 Column, beam, floor: Everything in the component list
 Opening: As far as one can understand from the diagrams of the crack occurred
immediately after the earthquake Roof slabs: As their thickness and specifications are unknown, these were assumed tobe 100 cm flat slabs.
 Pressure vessels, etc.: The total mass, including the pedestal, was distributed across thejoined floor. (It may not be suitable with regard to floor vibrations.)- 157 -

JAEA-Research 2024-001

Elevation (m)Fig.2-1 Building section (Left: NS section, Right: EW section) 2

Fig.2-2 Building section (Left: B3F, Right: B1F) 2- 158 -

Elevation (m)JAEA-Research 2024-001

2.2

GroundThe data from KARISMA report 2 is used for the initial physical properties of the ground.
In the simulation analysis of the Reactor 7 building of the Kashiwazaki -Kariwa Nuclear
Power Station, conducted by Hijikata et al. 3 , manmade rock (MMR) was modeled on the
supporting ground and the side ground. However, in this analysis, it was deemed to besupported by the Nishiyama Formation.
In this analysis, the size of ground model in the horizontal direction was set toapproximately six times the width of the building, with reference to the existing analysis
examples. Moreover, the bottom boundary surface of the analysis model was set at Vs = −720m, and the Elevation of the lower layer of the Nishiyama format ion was set at −155 m. Notethat Hijikata et al. set −90 m from the ground surface as the bottom analysis surface.

- 159 -

JAEA-Research 2024-001

3.

Creation of the geometric model

3.1

Building

The details of the structural members (columns, beams, floors and walls) being analyzed
are as follows. Regarding the size of members, the member list in KARISMA report 2 wasreferred to for columns and beams, while the values listed in the plan in the KARISMA
report 2 were referred to for floors and walls. Moreover, regarding the coordinates, the levelof each floor was set at the top end of the floor, those of the columns were set at theintersection of the reference lines in principle, those of the exterior wall were set at the outersurface, and those of the interior walls were based on the reference lines.
3.1.1

Columns and Beams

The positions and shapes used for the columns and beams are those in the KARISMA
report.
The lower part of the middle column of the plans (Fig.3-1 to Fig.3-7) show the analysis
modeling area of the columns and beams for each floor. The length of the flange of the steel
beams on the crane floor was set to 525 mm (average of 600 and 450 mm).
3.1.2

Floors and Walls

Regarding the floors and the walls, the earthquake -resistant wall and supporting walls in
the KARISMA report are the objects of analysis.
The analysis area of the walls and floor of each floor are shown in the plans (Fig.3 -1 toFig.3-7) . The figure on the left shows the earthquake -resistant wall on each floor; the figureon the right shows the earthquake -resistant walls and supporting walls; and the central figure
shows their models. The walls were modeled with shell elements, and their thicknesses areshown.
Further, Fig.3-8 shows a cross-sectional view of the building model.

- 160 -

JAEA-Research 2024-001

E L.
Plan view

FE m o del(A b o v e : hi de c ol um ns an d b eam s )S ei s m i c w al l s a nd a u x i l i ar y w al l s(A b o v e : N S di r ., B el o w : E W di r. )S ei s m i c w al l s
A ux i l i a ry w al l s

Fig.3-1

Plan 2 B3F

E L.
Plan view

FE m o del(A b o v e : hi de c ol um ns an d b eam s )S ei s m i c w al l s a nd a u x i l i ar y w al l s(A b o v e : N S di r ., B el o w : E W di r. )S ei s m i c w al l s
A ux i l i a ry w al l s

Fig.3-2

Plan 2 B2F- 161 -

JAEA-Research 2024-001

E L.
Plan view

FE m o del(A b o v e : hi de c ol um ns an d b eam s )S ei s m i c w al l s a nd a u x i l i ar y w al l s(A b o v e : N S di r ., B el o w : E W di r. )S ei s m i c w al l s
A ux i l i a ry w al l s

Fig.3-3

Plan 2 B1F

E L.
Plan view

FE m o del(A b o v e : hi de c ol um ns an d b eam s )S ei s m i c w al l s a nd a u x i l i ar y w al l s(A b o v e : N S di r ., B el o w : E W di r. )S ei s m i c w al l s
A ux i l i a ry w al l s

Fig.3-4

Plan 2 1F- 162 -

JAEA-Research 2024-001

E L.
Plan view

FE m o del(A b o v e : hi de c ol um ns an d b eam s )S ei s m i c w al l s a nd a u x i l i ar y w al l s(A b o v e : N S di r ., B el o w : E W di r. )S ei s m i c w al l s
A ux i l i a ry w al l s

Fig.3-5

Plan 2 2F

E L.
Plan view

FE m o del(A b o v e : hi de c ol um ns an d b eam s )S ei s m i c w al l s a nd a u x i l i ar y w al l s(A b o v e : N S di r ., B el o w : E W di r. )S ei s m i c w al l s
A ux i l i a ry w al l s

Fig.3-6

Plan 2 3F- 163 -

JAEA-Research 2024-001

E L.
FE m o del(A b o v e : hi de c ol um ns an d b eam s )Plan view

S ei s m i c w al l s a nd a u x i l i ar y w al l s(A b o v e : N S di r ., B el o w : E W di r. )S ei s m i c w al l s
A ux i l i a ry w al l s

Fig.3-7

Plan 2 4F

Elevation (m)Fig.3-8

Analysis model section (NS section)- 164 -

JAEA-Research 2024-001

3.1.3

Roof

The data from the KARISMA report is used for the roof truss. Fig.3 -9 shows the plan viewfor the roof truss.

Fig.3-9 Plan view of the roof truss (Roof, Elevation +49.7 m)- 165 -

JAEA-Research 2024-001

As there was no data regarding the roof slab in the KARISMA report, modeling was donewith a 100 mm thick RC in consideration of the common roof slab thickness used for lightwater reactors, deck plates, etc. Fig.3-10 shows the overview of the roof model.

Roofslab ( She ll element)
屋根スラブ（シェル要素）
Rooftruss ( Be am element )屋根トラス（ビーム要素）
Roof truss ( Tru ss element)

屋根トラス（トラス要素）

Fig.3-10 Roof model (Above: The entire roof, Lower left: Roof truss, Lower right: Roofslab)

- 166 -

JAEA-Research 2024-001

3.2

GroundThe ground area is the same as that in the KARISMA report 2 . Table 3-1 shows the groundarea.
Table 3-1 Ground area
Elevation

GL

(m)

(m)

12.0

0.0

8.0

−4.0

4.0

−8.0

−6.0

−18.0

−33.0

−45.0

−90.0

−102.0−136.0−148.0−155.0−167.0Classification

Sand
YasudaGeologicalfeatures
Sand
Sand
Clay
Rock

Nishiyama

Rock
Rock

Nishiyama- 167 -

JAEA-Research 2024-001

4.

Creation of the structural modelFig.4-1 and Fig.4-2 show the 3D FEM model (soil-structure interaction). The details aredescribed in sections 4.1 and 4.2.

Fig.4-1 View of the building buried in the groundFig.4-2 General view of the 3D FEM model (soil -building coupling)- 168 -

JAEA-Research 2024-001

4.1

Building

The basemat slab is modeled with solid elements; the building wall and floor are modeledwith shell elements; and the column, beam, and roof truss are modeled with beam elements.
Only the weights of the pedestal and pressure vessel are considered, and they are treate d as
the unit volume weight at each floor.
In this analysis, the mesh size was set to divide the floor height into about four parts toobtain the building response of the elastic region.
Fig.4-3 shows the overview of the analysis mode l, and Fig.4-4 to Fig.4-12 show the plans.
In the plans, gray indicates walls, blue indicates beams, and blanks indicate columns. The
walls of the fuel pool and the exterior walls of RF in 3F and 4F are arranged toward the east
and west.

Number of nodes: 14540
Number of elements: 18493

Thickness ofplan elements(m)

Fig.4-3 3D FEM model of the building- 169 -

JAEA-Research 2024-001

Fig.4-4

Plan B3F

Fig.4-5

Plan B2F- 170 -

JAEA-Research 2024-001

Fig.4-6

Plan B1F

Fig.4-7

Plan 1F- 171 -

JAEA-Research 2024-001

Fig.4-8

Plan 2F

Fig.4-9

Plan 3F- 172 -

JAEA-Research 2024-001

Fig.4-10

Plan 4F

Fig.4-11

Plan CRF- 173 -

JAEA-Research 2024-001

Fig.4-12

Plan Roof slab

- 174 -

JAEA-Research 2024-001

The joint conditions for the roof trusses, the roof truss and exterior wall, and roof truss
and roof slab are shown below.
(1)

Roof truss

The edges of both the upper and lower chord members have the same displacement androtation as their neighboring beams (rigid joint ) at every degree of freedom. The diagonal
and struts are connected with pin joints.
(2)

Roof truss and exterior wall

The nodes of the supporting parts of the upper chord members and the lower chordmembers of the roof truss have the same displacement and rot ation for all degrees of freedom
as the nodes of the peripheral columns and beams (rigid joint). The edges of the horizontal
brace are connected with pin joints.
(3)

Roof truss and roof slab

The upper chord members of the roof truss, horizontal brace, and roo f slab are connectedwith pin joints, as indicated by the red circles in Fig.4 -13.

Main truss: Intersection of struts
and diagonal member(s)Sub-truss:Intersection

with

Y-

direction bundled truss
members*Pin joint (x, y, z joint)

Fig.4-13 Example of the joint position of roof slab and roof truss (red circle)- 175 -

JAEA-Research 2024-001

4.2

GroundAs in Hijikata et al. 3 , the transmission frequency was set to approximately 17 Hz, which
exceeds the vertical dominant frequency of 10 Hz in the upper and lower parts of the building.
Moreover, the ground mesh from the ground surface to the bottom of the basemat was set
after taking the matching mesh of the building model into consideration. While the equivalentfrequency would be less than 17 Hz, it was assumed that the effect of the high frequency
behavior of the surface ground on the response of the structure would be small. Note that theequivalent properties used here are the average of the equivalent property values at eachlayer obtained from the KARISMA report. These will be discussed in the section on thematerial model.

- 176 -

JAEA-Research 2024-001

5.

Mass model
The mass of the building model was set in a way so that the mass of each floor of thebuilding matched the weight of the lumped mass model in the KARISMA report, shown in
Table 5-1 below is an example of the way of thinking when adjusting the weight of the
lumped mass model into the floor mass density of the building 3D FEM model.
• Regarding the mass of the columns and walls, the total mass between two floors was firstobtained, and then half of each was allocated to the u pper and lower floors.
• The mass of the beams was distributed to each floor.
• The mass density was set by adding the difference between the lumped mass and the massof the floor.

Table 5-1 Parameters of the lumped mass model 2- 177 -

JAEA-Research 2024-001

6.

Material model

6.1

Physical properties of the building

The value calculated based on the actual strength of the concrete is used as its stiffness.
Table 6-1 shows the actual strength of concrete in the KARISMA report. With this value, use
Equation (6.1) to obtain Young's modulus. For reinforcing steel, the values listed in Table
6-2 are used, and for steel, the values listed in Table 6 -3 are used.

These are summarizedin Table 6-4. Note that, in this report, it was determined to be unnecessary to consider the
RC nonlinear character from the field investigation of the Niigataken Chuetsu-oki
Earthquake in 2007.
1

𝛾𝛾 2
𝐹𝐹c 3
𝐸𝐸 = 3.35 × 10 × ( ) × ( ) , (normal concrete： 18 ≤ 𝐹𝐹c ≤ 60)
24
60
4( 6.1 )

Here, E: Young’s modulus (N/mm 2 ), Fc: Design strength (N/mm 2 ), γ: Air drying unit weight(kN/m 3 )- 178 -

JAEA-Research 2024-001

Table 6-1 Real strength in the KARISMA report 2

Table 6-2 Material constant of reinforcing steel 2

Table 6-3 Material constant of steel 2

Table 6-4 Strength and elastic constants of reinforced concrete
Young’s modulus

Shear modulus

E(N/mm 2 )G(N/mm 2 )Poisson’s ratio ν

Unit volume
weightγ(kN/m 3 )Concrete

3.13×10 4

1.21×10 4

0.20

24.0※

Reinforced

2.05×10 5

－

0.30

77.0

Steel frame

2.05×10 57.90×10 4

0.30

77.0

*γ is set at the value obtained by subtracting 1.0 from the unit volume weight of reinforced
concrete.

- 179 -

JAEA-Research 2024-001

6.2

Ground properties

The equivalent physical properties (average of each stratum) used in the simulation
analysis of the Niigataken Chuetsu-oki Earthquake in 2007 in the KARISMA report were
employed as the ground properties in this application example. The ground equivalent
properties were calculated using the initial stiffness and G-γ curve based on one-dimensional
wave theory while taking the two horizontal directions into account.
Table 6-5 shows the initial stiffness ground properties, and Tables 6-6 and 6-7 show theground equivalent properties for detailed and average ground based on one -dimensional wave
theory.

Table 6-5 Initial stiffness ground properties 2- 180 -

JAEA-Research 2024-001

Table 6-6 Ground equivalent properties based on one -dimensional wave theory(Detailed ground)
G.L.
(m)
0.5
1.5
2.5
3.5
4.5
5.5
6.5
7.5
9.0
11.0
13.0
15.0
17.0
19.5
22.5
25.5
28.5
31.5
34.5
37.5
40.5
43.5
47.0
51.0
55.0
59.0
63.0
67.0
71.0
75.0
79.0
83.0
87.0
91.0
95.0
99.5
104.5
109.5
114.5
119.5
124.5
129.5
134.5
139.5
145.0
150.5
155.5
160.5
167.0

G/Go

h(%)

Max. shear strain

X-DIR Y-DIR X-DIR Y-DIR X-DIR
0.647
0.283
0.141
0.084
0.19
0.159
0.132
0.11
0.742
0.682
0.642
0.606
0.586
0.964
0.961
0.957
0.954
0.952
0.95
0.95
0.949
0.95
0.956
0.958
0.958
0.956
0.954
0.953
0.952
0.952
0.951
0.95
0.948
0.947
0.946
0.945
0.954
0.953
0.952
0.951
0.95
0.95
0.949
0.948
0.948
0.959
0.958
0.957
0.957

0.58
0.19
0.084
0.084
0.178
0.149
0.112
0.084
0.724
0.669
0.619
0.573
0.549
0.959
0.957
0.953
0.951
0.948
0.947
0.946
0.946
0.946
0.952
0.953
0.953
0.953
0.95
0.946
0.944
0.941
0.939
0.938
0.934
0.933
0.931
0.932
0.946
0.946
0.946
0.946
0.943
0.941
0.938
0.932
0.926
0.944
0.943
0.942
0.941

10.7
21.7
26
27.8
24.5
25.5
26.3
27
3.9
4.8
5.4
5.9
6.2
1.6
1.7
1.8
1.9
1.9
1.9
2
2
1.9
1.8
1.8
1.8
1.8
1.9
1.9
1.9
1.9
1.9
1.9
2
2
2
2
1.9
1.9
1.9
1.9
1.9
1.9
2
2
2
1.8
1.8
1.8
1.8

- 181 -

12.7
24.6
27.8
27.8
24.9
25.8
26.9
27.8
4.1
5
5.7
6.4
6.8
1.8
1.8
1.9
1.9
2
2
2
2
2
1.9
1.9
1.9
1.9
2
2
2.1
2.1
2.2
2.2
2.3
2.3
2.3
2.3
2
2
2
2
2.1
2.1
2.2
2.3
2.4
2.1
2.1
2.1
2.1

0.01368
0.09769
0.31049
0.648080.180120.253170.344290.44387
0.0281
0.04408
0.05865
0.07101
0.079280.02303
0.02538
0.028420.031410.033470.035150.03552
0.03592
0.03525
0.029650.02775
0.02769
0.02974
0.03126
0.032220.032850.033430.03410.03475
0.03697
0.03835
0.039490.040190.03149
0.032280.03287
0.033930.03469
0.03525
0.03599
0.03679
0.037290.027430.02786
0.028390.02888

Y-DIR
0.01988
0.18264
0.63103
0.721210.20184
0.27989
0.428850.629140.032240.04851
0.065960.084420.096440.027
0.02867
0.031830.03462
0.037
0.03889
0.03979
0.03967
0.038960.03276
0.032190.03252
0.03253
0.03557
0.039070.04246
0.04553
0.048070.050050.05163
0.05230.05277
0.05275
0.03979
0.039160.039030.04003
0.04276
0.046240.04955
0.05251
0.055390.04182
0.04332
0.04460.04545

JAEA-Research 2024-001

Table 6-7 Ground equivalent properties based on one -dimensional wave theory(Average ground)

G.L.
(m)

Vs
(m/s)

0.0
-4.0
-8.0
-18.0
-45.0
-102.0-148.0-167.0
6.3

G/Go

150
200
330
490
530
590
650

h(%)

0.262 22.39
0.139 26.09
0.639 5.42
0.952 1.89
0.947 2.00
0.946 2.03
0.950 1.95

Material damping

The values from the KARISMA report were used for the material damping of eachcomponent, which are listed in Table 6 -8. Moreover, Rayleigh damping was used for the time
history response analysis.

Table 6-8 Material damping
Material Type

Damping
Constant

Reinforced concrete

5%

Steel truss

2%

GroundEquivalent
damping(See Table 6-7)

- 182 -

JAEA-Research 2024-001

7.

Mathematical model of damping

7.1

Rayleigh damping

For time history response analysis of the 3D FEM model, Rayleigh damping (Rayleighdamping of each element) is used. When setting Rayleigh damping, it is necessary to
determine the main natural frequencies. In this verification, they were set as follows:・ f 1 : Average of the 1st mode natural frequencies in the NS and EW directions
・ f 2 : The 1st mode natural frequency in the UD direction based on the eigenvalue analysis
resultRayleigh damping f 1 and f 2 , as used for the building, were set according to the eigenvalue
analysis of the independent building model under the fixed conditions of the building
basemat. However, note that Rayleigh damping f 1 used for the ground was set according to
the eigenvalue analysis of the soil -building coupling model. Table 7 -1 shows the frequencies
used to set Rayleigh damping. Table 7 -2 and Fig.7-1 show the eigenvalue analysis result and1st mode diagram of the independent building model under the building basemat fixed
conditions, and Table 7 -3 and Fig.7-2 show the eigenvalue analysis result and 1st mode
diagram of the 3D FEM model (soil -structure interaction). Moreover, the relationships
between the Rayleigh damping of the building and ground and the frequencies are shown in
Table 7-4, Fig.7-3, Table 7-5, and Fig.7-4, respectively.
Table 7-1
Building

Frequencies used to set Rayleigh damping
f1

f2

Reinforced concrete

Average of the 1st natural

Natural frequency in the(RC)frequencies
direction

in

the

NS

UD direction when the

and

the

EW

building basemat is fixed

direction when the building
basemat is fixed
Steel truss
GroundSame as RCSame as RC

Average of the 1st natural

Natural frequency in thefrequencies in the NS and

UD direction when the

EW directions when thebuilding basemat is fixedbuilding and the ground arecoupled(Reference) While it is possible to regard f 2 of the steel truss as the 1st natural frequency of
the roof slab, it was considered to be the same as that of RC because its difference with the
1st natural frequency in the UD direction when the building basemat is fixed as small.

- 183 -

JAEA-Research 2024-001

Table 7-2 Eigenvalue analysis result of the independent building model under thebuilding basemat fixed conditions
モード
Mo
d es

F re q.
振動数

P周期
er i o d

次数

Hz

sec

刺激係数
S t i m ul us
c o eff i c i e nt
NS(X)

EW(Y)

E ff ec有効質量比t i v e m as s r a ti oNS(Z)UD(Z )

NS(X)

EW(Y)

R em
ar k s
備考

NS(Z))
UD(Z

1

4.187

0.239

318.138-1.278-3.409

0.538

0.000

0.000

t
1 sNS1次
(NS)

2

4.791

0.209

-2.756-329.092

1.687

0.000

0.576

0.000

t
1 sEW1次(E W )

3

5.080

0.197

-1.0645.740

31.756

0.000

0.000

o of t ru s s
0.005 R
屋根トラス

6

7.109

0.141

126.755-8.574

4.846

0.085

0.000

0.000

nd
2NS2次
(N S )

9

7.661

0.131

2.324

-63.656-2.863

0.000

0.022

0.000

nd
2 EW2次(E W )

36

10.5170.095-10.248-69.891-23.860

0.001

0.026

0.003

rd
3 EW3次(E W )

43

11.001

0.091

0.251

1.449

278.942

0.000

0.000

0.414

st
1UD1次
(UD)

47

11.3970.088-78.1729.830-14.563

0.032

0.001

0.001

rd
3NS3次
(N S )(a) NS direction(b) EW direction(c) UD direction

Fig.7-1 1st mode diagram of the independent building model ( basemat fixed)- 184 -

JAEA-Research 2024-001

Table 7-3 Eigenvalue analysis result of 3D FEM model (soil -structure interaction) using
equivalent properties in the KARISMA report 2
Mode

Frequency

Cycle

Mode participation factor

order

Hz

Sec

NS(X)

EW(Y)

UD(Z)

Effective Mass Ratio
NS(X)

EW(Y)

Note

UD(Z)
NS

1

0.846

1.183

−4293.6

−66.2

0.0

0.768

0.000

0.000

direction
primary
EW

2

0.846

1.182

68.2

−4293.7

0.0

0.000

0.768

0.000

direction
primary*Excerpt of the main modes of simulation analysis(a) NS direction (Bird’s-eye view)(b) EW direction (Bird’s-eye view)(c) NS direction(d) EW direction

Fig.7-2 1st mode diagram of the 3D FEM model (soil -structure interaction)- 185 -

JAEA-Research 2024-001

Table 7-4 Relationship between the Rayleigh damping of the building and frequencies
F re q ue nc y

D am pi n g r ati o

R ay l ei g h d am pi n g

ｆ1

ｆ2

h1

h2

α

β

(Hz)

(Hz)

(-)

(-)

(-)

(-)

RC

4.49

11.00

0.050

0.050

2.003 1.028E-03

S鉄骨
teel

4.49

11.00

0.020

0.020

0.801 4.110E-04

ターゲット2点をプロット

D am pin g r ati o
減衰比

0.20

S t鉄骨
eel

RC

0.10

0.00

0

5

10

15

20

F re q振動数(Hz)ue nc y (H z )RC:Walls,
slab, and roof are shell elements;
RC： floor
壁、床スラブ及び屋根スラブのシェル要素
columns andbeams are beam elements; and柱及び梁のビーム要素
基礎スラブのソリッド要素
the basemat
slab is the solid element.
Steel frame: The
rooftruss is a beam and truss element, and鉄骨：
屋根トラスのビーム、トラス要素
the steel girder
is a beam element.
鋼材ガーダーのビーム要素

Fig.7-3 Relationship between the Rayleigh damping of the building and frequencies
Table 7-5 Relationship between the Rayleigh damping of the ground and frequencies
F re q ue nc y

D am pi n g r ati o

R ay l ei g h d am pi n g

ｆ1

ｆ2

h1

h2

α

β

(Hz)

(Hz)

(-)

(-)

(-)

(-)

S砂層1
and1

0.846

11.001

0.206

0.206

2.034 5.535E-03

S砂層2
and2

0.846

11.001

0.254

0.254

2.507 6.825E-03

Y a安田層suda

0.846

11.001

0.047

0.047

0.464 1.263E-03

N i西山層1
shiyama1

0.846

11.001

0.018

0.018

0.178 4.837E-04

Nishiyama2

0.846

11.001

0.022

0.022

0.217 5.911E-04

N i西山層3
shiyama3

0.846

11.001

0.021

0.021

0.207 5.643E-04

N i西山層4
shiyama4

0.846

11.001

0.018

0.018

0.178 4.837E-04

0.50

S砂層1
and1
S
and2
砂層2

D am 減衰比
pi n g r at i o

0.40

Y安田層
asuda

0.30

Nis hiy ama1

西山層1

Nis hiy ama2

西山層2

0.20

Nis hiy ama3

西山層3

N i 西山層4s hiy ama4

0.10

0.00

0

5

10

15

20

F re q振動数(Hz)ue nc y (H z )Fig.7-4 Relationship between the Rayleigh damping of the ground and frequencies- 186 -

JAEA-Research 2024-001

8.

Boundary joint model

8.1

Modeling of the joint of the buried building and the groundIn the report after the Niigataken Chuetsu-oki Earthquake in 2007, a gap of about a few tensof centimeters was observed between the building and the ground surface. However, it wasdeemed to have little influence on the building response. Therefore, the separation and contact
between the building and the ground were no t considered.
8.2

Joining of structure components

There is overlapping in the joints between members, such as the columns and beams orcolumns/beams and walls, and the center line in the beams/shell structure model, but this was
ignored. This is because a lthough they affect the underground part, they have little effect on
the overall building, including the third floor.
8.3

Bottom and side boundaries of the ground analysis region

The bottom boundary was set as a viscous boundary (Vs = 720 m/s, Vp = 1,898 m/s).
The side boundary was set as a periodic boundary (repeating boundary), where thetranslational displacement of nodes of corresponding sides are the same.

- 187 -

JAEA-Research 2024-001

9.

Input seismic motion
The free rock wave (pullback wave), which was set to ensure that the seismic response

analysis result and the observation record at the observation position above the basemat of thereactor building match, was used as the input seismic motion.
9.1

Pullback wave

The 3 directional components of 2E wave at the bottom of the analysis model obtained fromthe observation record were entered into the bottom of the analysis model. The input seismic
motion (pullback wave) at the bottom of the analysis model was prepared according to thefollowing procedure using the transfer functions of the observation position above the basemat
and at the bottom of the analysis model so as to ensure that the response acceleration at theobservation position above the basemat of the reactor building matches that of the observation
record.
• Seismic response analysis was conducted using a 3D FEM model. The observation record
from above the basemat was used as the input seismic motion.
• Using the transfer functions obtained from the time history response analysis result above thebasemat of the aforementioned seismic response analysis and the input wave at the bottomof the analysis model (observation record above the basemat), the seismic motion input into
the bottom of the analysis model was calculated so as to ensure that the response acce leration
spectrum above the basemat matches that of the observation record. However, the input
motion in each direction was calculated individually on each occasion.
Fig.9-1 shows the observation point above the basemat, and Fig.9-2 shows the calculation
procedure.

- 188 -

JAEA-Research 2024-001

Fig.9-1 Observation point above the basemat and its correspondence with the 3D FEM model- 189 -

JAEA-Research 2024-001

S ei s m i c r es p o n s e a n a l y s i s fo r ea c h d i r ec t i o n( a n a l y z e NS , E W, U D d i r ec t i o n i n d i v i d u a l l y )Temporary input wave (components indirections other than β direction ar e zero)Ti m e -h i s t o r y res p o n s e w a v e fo r m s o n t h e
b a s e m a t f o r ea c h d i r ec t i o n

α d i r ec t i o n r es p o n s e c o m p o n en t t o β d i re c t i o n i n p u t
fr eq u en c y c o m p o n en t o f F o u ri er t ra n s f o r m a t i o n

Fo u ri er t ra n s f o rm a t i o n
Fo u ri er t ra n s fo rm a t i o n o f t h e t i m e - h i s t o r yres p o n s e w a v e fo rm

Tra n s f er fu n c t i o n s fo r t h r ee d i r e c t i o n s

Calculation of the input wave at the bottom
o f t h e m o de l

Fo u ri er t ra n s fo rm a t i o n o f t h e o b s e rv ed w a v efo rm o n t h e b a s em a t

Fo u ri er t ra n s fo rm a t i o n o f t h e i n p u t w a v e a tt h e b o t t o m o f t h e m o d el
In v ers e Fo u ri e r t ra n s f o rm
Ti m e -h i s t o r y res p o n s e w a v e fo r m s a t t h ebottom of the modelUsing

as the input,s ei s m i c
r es p on s e
a nal y s i s
w i ths i m ul t a n eo us e x c i t at i o n i n t h r ee di r ec t i o ns

Was the observed
record rep roduce d?

FinishC o rr ec t th e i n p ut w a v e f o r ea c h di r ec t i o n.

R es p on s e w a v e o f t heob s e rv a ti o n r ec or d

Fig.9-2 Input seismic motion calculation procedure (pullback wave)- 190 -

JAEA-Research 2024-001

Fig.9-3 shows the acceleration time history waveform of the prepared input seismic motion

A c c el e r ati o n (c m / s 2 )(pullback wave).

T i m e (s ec )A c c el e r ati o n (c m / s 2 )(a) NS direction

T i m e (s ec )A c c el e r ati o n (c m / s 2 )(b) EW direction

T i m e (s ec )(c) UD direction
Fig.9-3 Acceleration time history waveform of the pullback wave (frequencies above 25 Hz
were cut)- 191 -

JAEA-Research 2024-001

Fig.9-4 shows the acceleration response spectrum and the Fourier spectrum of the pullback
wave. One possible reason why the amplitude around 11 –12 Hz in the UD direction became
larger is that the bottom of the analysis model became the node of the mode shape because
the vertical one-dimensional primary wave vibration mode of the analysis area below thebottom of the basemat was approx. 10.76 Hz and the building it self has an nearly equal

Acceleration (cm/s2)

Fourier spectrum (cm/s)

natural frequency.

Period (sec)

NS direction(d)

NS direction

Acceleration (cm/s2)

Fourier spectrum (cm/s)(a)Frequency (Hz)Period (sec)

EW direction(e)

EW direction

Acceleration (cm/s2)

Fourier spectrum (cm/s)(b)Frequency (Hz)Frequency (Hz)Period (sec)(c)

UD direction(f)Acceleration response spectrum

UD direction

Fourier spectrum

Fig.9-4 Acceleration response spectrum ( h = 5%) and Fourier spectrum.
(Frequencies above 25 Hz were cut.)- 192 -

JAEA-Research 2024-001

10. Initial state model
As this application example is an elastic analysis, it was not considered.

- 193 -

JAEA-Research 2024-001

11. Condition setting for numerical analysis
11.1 Parameters related to mass matrix
The mass matrix is set to be a consistent mass matrix.
11.2 Parameters related to time integration• Time integration method : Newmark-β (β = 1/4, γ = 1/2)
・ Duration : 40.96 seconds
・ Integration time interval: Elastic analysis 0.01 second

・ Parallel computation
Parallel number: 27
This analysis is conducted using the domain decomposition method (DDM).
• Convergence judgement value of the iteration method: 1.0E -8
The convergence judgement value mentioned here is the ratio between the two -dimensional
norm and the initial two -dimensional norm.
11.3 Analysis environment• Processor : Intel(R)Xeon(R) Platinum 8168 CPU @ 2.70GHz
・ RAM: 256 GB・ OS : Windows Server 2012 R2 Standard
11.4 Reference• Representative nodes
Fig.11-1 to Fig.11-3 show the representative node of each floor in this analysis.

- 194 -

JAEA-Research 2024-001

Corner of exterior wall
Midpoint of ex terior wall(a) B3F Plan (Elevation −8.2 m)(b) B2F Plan (Elevation −1.7 m)(c) B1F Plan (Elevation +4.8 m)
Fig.11-1 Positions of the representative nodes in this analysis (From above: B3F, B2F, and
B1F)- 195 -

JAEA-Research 2024-001

Corner of exterior wall
Midpoint of ex terior wall(a) 1F Plan (Elevation +12.3 m)(b) 2F Plan (Elevation +18.1 m)(c) 3F Plan (Elevation +23.5 m)
Fig.11-2 Positions of the representative nodes of this analysis (From above: 1F, 2F, and
3F)- 196 -

JAEA-Research 2024-001

Corner of exterior wall
Midpoint of ex terior wall

4F Plan (Elevation +31.7 m)
Fig.11-3 Positions of the representative nodes of this analysis (4F)

- 197 -

JAEA-Research 2024-001

12. Examination and validation of analysis results
12.1 Examination of successful termination of the analysis
The log file of the analysis code was checked to examine that the analysis terminatedsuccessfully.
12.2 Examination of Input data
Those that can be obtained as output from the analysis data, such as mesh diagrams(structural diagrams), member lists, constraint diagrams, seismic waveform diagrams, andmaterial diagrams, were compared and checked against the original data. The comparisonswere conducted numerically as much as possible.
For the structural model data, it was checked that there were no abnorma l values among
the eigenfrequencies and eigenmodes or mistakes in the geometric, constraint, or joint
conditions before this analysis.
The respective conditions and states of the boundary condition, seismic motion, initialstate, etc., were charted, and it was checked that there were no mistakes.
12.3 Examination of the analysis result
After confirming that there were no issues with the calculation processing information or
calculation time and that there had been no calculation errors, the following items wereconfirmed from the analysis results.


Correspondence between acceleration/deformation, displacement distribution, and load



Ratio

of

the

simplified

calculation

value

and

theoreticalsolutionacceleration/deformation and stress.


Polarity, symmetry, and over/under -estimation of acceleration/deformation.

The balance between acceleration/stress and displacement

Tendency in the distribution of acceleration/displacement and stress

Where pulling/compression occurs

Reaction force at the rigid body movement prevention position

Reaction force at the constraining position, matching with the loadStrain and stress distribution in the jointStress and yield strength- 198 -of

JAEA-Research 2024-001

12.4 Validation of analysis results
The validity of the analysis results was verified through its comparison with pastobservation records.
12.4.1 Time history acceleration waveform at each observation position
The comparisons of the observation records from observation positions (B3F and 3F) andthe acceleration time history waveform of the analysis result are shown in Fig.12 -1 to
Fig.12-6.

- 199 -

JAEA-Research 2024-001■NS
解析
Analysis2)
2)
Acceleration(cm/s
加速度(cm/s

600

観測記録
O
b s e rv at i o n

400
200
0
-200
-400
-600

0

10

20

30

40

時間(sec)Time(sec)

Fig.12-1 Acceleration time history waveform (Above the basemat (B3F) NS direction)2)
Acceleration
加速度(cm/s2(cm/s
)

■EW
解析
Analysis

600

O観測記録
b s e rv at i o n

400
200
0
-200
-400
-600

0

10

20

30

40

時間(sec)Time(sec)

Fig.12-2 Acceleration time history waveform (Above basemat (B3F), EW direction)

Acceleration(cm/s 2 )加速度(cm/s2)■UD
解析
Analysis

600

Observation
観測記録

400
200
0
-200
-400
-600

0

10

20

30

40

時間(sec)Time(sec)

Fig.12-3 Acceleration time history waveform (Above basemat (B3F), UD direction)- 200 -

JAEA-Research 2024-001

Acceleration(cm/s 2 )加速度(cm/s2)■NS
解析
Analysis

600

Observation
観測記録

400
200

0
-200
-400
-600

0

10

20

30

40

Time
(sec)
時間(sec)Fig.12-4 Acceleration time history waveform ( 3F, NS direction)2)
Acceleration
加速度(cm/s2(cm/s
)

■EW
解析
Analysis600

観測記録
Observation

400
200

0
-200
-400
-600

0

10

20

30

40

Time
(sec)
時間(sec)Fig.12-5 Acceleration time history waveform ( 3F, EW direction)

Acceleration(cm/s 2 )加速度(cm/s2)■UD
解析
Analysis

600

Observation
観測記録

400
200

0
-200
-400
-600

0

10

20

30

40

Time
(sec)
時間(sec)Fig.12-6 Acceleration time history waveform ( 3F, UD direction)- 201 -

JAEA-Research 2024-001

12.4.2 Acceleration response spectrum ( h = 5.0%) at the observation positions (B3F, 3F)
The comparisons of the observation records from observation positions (B3F and 3F) andthe acceleration response spectrum ( h = 5.0%) of the analysis result are shown in Fig.12 -7

2
2
Acceleration
response spectrum
加速度応答スペクトル(cm/s) (cm/s )

■NS
2000

Analysis
解析
Obs.
観測記録

1500

1000

500

0

0.01

0.1

Period(sec)
周期(sec)

(a)

■NS
2000

1

10

3F
Analysis
解析

Acceleration
response spectrum2) (cm/s 2 )加速度応答スペクトル(cm/s

to Fig.12-9.

Obs.
観測記録

1500

1000

500

0

0.01

0.1

Period(sec)
周期(sec)110(b) Above basemat (B3F)
Fig.12-7 Acceleration response spectrum (h = 5%) (NS direction)- 202 -

JAEA-Research 2024-001

2) (cm/s 2 )Acceleration
response spectrum
加速度応答スペクトル(cm/s

■EW
2000
Analysis
解析
Obs.
観測記録

1500

1000

500

0

0.01

Period(sec)
周期(sec)

(a)

■EW
2000
2)
Acceleration
response spectrum(cm/s 2 )加速度応答スペクトル(cm/s

0.1

1

10

3F
Analysis
解析

観測記録
Obs.

1500

1000

500

0

0.01

0.1

Period(sec)
周期(sec)110(b) Above basemat (B3F)
Fig.12-8 Acceleration response spectrum ( h = 5%) (EW direction)- 203 -

JAEA-Research 2024-001

2) (cm/s 2 )Acceleration
response spectrum
加速度応答スペクトル(cm/s

■UD
4000
Analysis
解析

3500

Obs.
観測記録

3000
2500
2000
1500
1000
500
0

0.01

Period(sec)
周期(sec)

(a)

■UD
2000
2)
Acceleration
response spectrum(cm/s 2 )加速度応答スペクトル(cm/s

0.1

1

10

3F
Analysis
解析
Obs.
観測記録

1500

1000

500

0

0.01

0.1

Period(sec)
周期(sec)110(b) Above basemat (B3F)
Fig.12-9 Acceleration response spectrum ( h = 5%) (UD direction)- 204 -

JAEA-Research 2024-001

13. Documentation
The implementation process of the simulation analysis of the observation record from thereactor building of Kashiwazaki -Kariwa Nuclear Power Station was documented to monitor
its compatibility and correspondence situation.

- 205 -

JAEA-Research 2024-001

References
1

ITOCHU Techno-Solutions Corporation, FINAS/STAR Version2015r170210, User
Manual, Tokyo, Japan, 2017.
2 IAEA, Review of Seismic Evaluation Methodologies for Nuclear Power Plants Based on
a Benchmark Exercise, IAEA -TECDOC-1722, 2013.
3 Katsuichiro Hijikata et al., Response performance of the Reactor 7 building of theKashiwazaki-Kariwa Nuclear Power Plant during the Chuetsu offshore earthquake,focusing on the nonlinearity of the ground, The Architectural Institute of Japan’s Journalof Structural and Constr uction Engineering, Vol.76, No.660, 2011, pp.319–327.

- 206 -