ISO/DIS 6023:2026(en)

ISO TC 10/SC 6/WG 23

Secretariat: SAC

Date: 2025-01-09

Technical product documentation (TPD) — General requirements of structural analysis for mechanical products based on the model of finite element analysis (FEA)

© ISO 2026

All rights reserved. Unless otherwise specified, or required in the context of its implementation, no part of this publication can be reproduced or utilized otherwise in any form or by any means, electronic or mechanical, including photocopying, or posting on the internet or an intranet, without prior written permission. Permission can be requested from either ISO at the address below or ISO’s member body in the country of the requester.

ISO copyright office

CP 401 • Ch. de Blandonnet 8

CH-1214 Vernier, Geneva

Phone: +41 22 749 01 11

Email: copyright@iso.org

Website: www.iso.org

Published in Switzerland

Contents

Foreword vi

Introduction vii

1 Scope 9

2 Normative references 9

3 Terms and definitions 9

4 Type of analysis 12

4.1 Structural statics analysis 12

4.2 Structural dynamics analysis 12

4.3 Linear analysis 12

4.4 Nonlinear analysis 12

5 General requirements 12

5.1 Plan of analysis 12

5.2 Model simplification 12

5.3 Element selection 12

5.4 Meshing 13

5.5 Calculation method selection 13

5.6 Dynamics analysis 13

5.7 Extraction of results 13

5.8 Coordinate system 13

5.9 Unit system 13

6 Analysis procedure 13

7 Requirements of FEA modelling 13

7.1 Geometric modelling 13

7.2 Model meshing 14

7.3 Define the material properties 15

7.4 Define boundary conditions 15

7.5 Pre-processing model check 15

8 Requirements for structural analysis using finite element method 16

8.1 Structural statics analysis 16

8.2 Structural dynamics analysis 16

9 Assessment and evaluation of results 17

9.1 Evaluation methods 17

9.2 Selection of the evaluation method 18

10 Results interpretation 18

10.1 Results for structural statics analysis 18

10.2 Results for structural dynamics analysis 18

10.3 Format of output 19

11 Requirements for the report of finite element analysis of structural analysis 19

11.1 Description of tasks 19

11.2 Normative references 19

11.3 Explanation of symbols 19

11.4 Analysis procedure 19

11.5 Results analysis and conclusion 19

11.6 Bibliography of references 19

12 Archiving requirements of FEA file 19

12.1 Finite element input management 19

12.2 Finite element model management 20

12.3 Analysis report management 20

12.4 Archived files management 20

12.5 Models and reports revision 20

12.6 Removing of models and reports 20

12.7 Statistics 20

Annex A (informative) A flowchart for the process of the FEA structural analysis for mechanical products 21

Annex B (informative) System of units and parameters for element properties check 22

B.1 SI unit system 22

B.2 Unit System 2 22

B.3 Unit quality checks 23

Annex C (informative) Use case 24

C.1 Statics analysis of U-groove 24

C.1.1 A U-groove example 24

C.1.2 Establish the finite element model 24

C.1.3 Apply load and set boundary conditions 25

C.1.4 Solve and submit the calculation 26

The calculation is solved and submitted. 26

C.1.5 Review and post-process the results 26

C.2 Modal analysis 27

C.2.1 A flat plane example 27

C.2.2 Material and unit 27

C.2.3 Material parameters setting 27

C.2.4 Element type 27

C.2.5 Constraints 27

C.2.6 Range of modal solution 27

C.2.7 Calculation 27

C.2.8 Result output 28

C.3 Nonlinear analysis of a clamp 29

C.3.1 Nonlinear structural assessment of a clamp loading then unloading 29

C.3.2 Establish the finite element model 29

C.3.3 Apply load, set boundary conditions and solver controls 29

C.3.4 Solve and submit the calculation 31

The calculation is solved and submitted. 31

C.3.5 Review and post process the results 31

C.4 Linear dynamic random vibration analysis 34

C.4.1 Linear dynamic random vibration assessment of an ultrasonic sensor PCB assembly 34

C.4.2 Establish the finite element model 34

C.4.3 Apply load, set boundary conditions and solver controls 34

C.4.4 Solve and submit the calculation 36

C.4.5 Review and post-processing the results 36

Annex D (informative) Template of the report of finite element analysis of mechanics 39

D.1 Object to be analysed 39

D.2 Problem to be solved 39

D.3 Reference files and symbols description 39

D.4 Simulation analysis process 39

D.5 Results analysis and conclusions 39

D.6 References 39

Bibliography 40

Foreword

ISO (the International Organization for Standardization) is a worldwide federation of national standards bodies (ISO member bodies). The work of preparing International Standards is normally carried out through ISO technical committees. Each member body interested in a subject for which a technical committee has been established has the right to be represented on that committee. International organizations, governmental and non-governmental, in liaison with ISO, also take part in the work. ISO collaborates closely with the International Electrotechnical Commission (IEC) on all matters of electrotechnical standardization.

The procedures used to develop this document and those intended for its further maintenance are described in the ISO/IEC Directives, Part 1. In particular, the different approval criteria needed for the different types of ISO documents should be noted. This document was drafted in accordance with the editorial rules of the ISO/IEC Directives, Part 2 (see www.iso.org/directives).

Attention is drawn to the possibility that some of the elements of this document can be the subject of patent rights. ISO shall not be held responsible for identifying any or all such patent rights. Details of any patent rights identified during the development of the document will be in the Introduction and/or on the ISO list of patent declarations received (see www.iso.org/patents).

Any trade name used in this document is information given for the convenience of users and does not constitute an endorsement.

For an explanation of the voluntary nature of standards, the meaning of ISO specific terms and expressions related to conformity assessment, as well as information about ISO's adherence to the World Trade Organization (WTO) principles in the Technical Barriers to Trade (TBT), see www.iso.org/iso/foreword.html.

This document was prepared by Technical Committee [or Project Committee, ISO/TC 10, Technical product documentation], Subcommittee SC 6, Mechanical Product Documentation.

Any feedback or questions on this document should be directed to the user’s national standards body. A complete listing of these bodies can be found at www.iso.org/members.html.

Introduction

The International Organization for Standardization (ISO) draws attention to the fact that it is claimed that compliance with this document can involve the use of a patent.

ISO takes no position concerning the evidence, validity and scope of this patent right.

The holder of this patent right has assured ISO that he/she is willing to negotiate licences under reasonable and non-discriminatory terms and conditions with applicants throughout the world. In this respect, the statement of the holder of this patent right is registered with ISO. Information can be obtained from the patent database available at www.iso.org/patents.

Attention is drawn to the possibility that some of the elements of this document can be the subject of patent rights other than those in the patent database. ISO shall not be held responsible for identifying any or all such patent rights.

Purpose

This document aims to provide comprehensive and detailed requirements for establishing a specification document for the finite element analysis (FEA) of mechanical products, covering various aspects such as analysis type, procedure, modelling principle, solution, analysis and evaluation of solution results, interpretation of solution results, solution results report, and documentary management.

Rationale

With the increasing complexity and diversification of mechanical products, accurate analysis of their structural performance has become increasingly crucial. Although the finite element analysis, as a powerful numerical analysis method, is widely used in the structural analysis of mechanical products, the lack of unified standards may lead to differences and unreliability in analysis results.

Technical product documentation (TPD) — General requirements of structural analysis for mechanical products based on the model of finite element analysis (FEA)

This document provides requirements for establishing a specification document for a finite element analysis (FEA) for a mechanical product, including type, procedure, modelling principle, solution, analysis and evaluation of the solution results, solution results interpretation, solution results report, and documentary management. It is applicable for FEA based structural analysis for mechanical products.

The following documents are referred to in the text in such a way that some or all their content constitutes requirements of this document. For dated references, only the edition cited applies. For undated references, the latest edition of the referenced document (including any amendments) applies.

ISO 17599:2015, Technical product documentation (TPD) — General requirements of digital mock-up for mechanical products

ISO/TS 18166:2016, Numerical welding simulation — Execution and documentation

ISO 10209:2012, Technical product documentation — Vocabulary — Terms relating to technical drawings, product definition and related documentation

For the purposes of this document, the following terms and definitions apply.

ISO and IEC maintain terminology databases for use in standardization at the following addresses:

— ISO Online browsing platform: available at https://www.iso.org/obp

— IEC Electropedia: available at https://www.iec.ch/electropedia

3.1

element

minimum discrete solution domain with nodes, filed variables, forces, interpolation functions, and physical and geometrical properties

3.2

finite element method

FEM

numerical analysis method to discretize a continuous domain under given constraints into finite pieces or elements

3.3

finite element analysis

FEA

analysis performed based on finite element method

Note 1 to entry: Typically, FEA is used to obtain an approximate solution of a real physical system.

3.4

finite element model

model to approximate mechanical product structure with a finite number of elements

3.5

node

spatial coordinate location where a degree of freedom is defined or calculated

3.6

mesh

set of the elements and nodes which defines the shape of the solution domain

3.7

analysis model

finite element model with material properties, boundary conditions applied and analysis type defined

EXAMPLE: Statics analysis model and dynamics analysis model, see Annex C for details.

3.8

pre-processing

activities where the analysis model is constructed

EXAMPLE: Geometry, mesh, loads, boundary conditions, materials, and solver setting.

3.9

post-processing

activities where the numerical solutions are processed and reviewed

3.10

material property

collection of data to describe the physical properties of materials used in mechanical product structures

3.11

field variables

dependent variables of interest governed by a differential equation

Note 1 to entry: In physical problems these are referred to displacement, temperature, etc.

3.12

boundary conditions

conditions imposed at the spatial boundary of a computational model that describe the interaction between the modelled and unmodelled domains

Note 1 to entry: Complete boundary conditions provide a unique solution to the specific mathematical problem being solved.

[SOURCE: ISO/TS 18166:2016,3.1]

3.13

stress concentration

phenomenon indicated by significant increase in stress value caused by the sharp change of stiffness in the local transition area of a mechanical structure

3.14

degree of freedom

the field variable defined at nodes

3.15

number of degrees of freedom

number of the field variables defined at nodes, at elements or at whole mesh

3.16

zero-dimensional element

element that takes the form of a point

EXAMPLE: A mass element or a rigid body among others.

3.17

one-dimensional element

element that takes the form of a segment

EXAMPLE: A rigid element, a rod element, a beam element.

3.18

two-dimensional element

element defined in a flat surface with arbitrary orientation

Note 1 to entry: With respect to an inertial frame and where the field variables and the loads are defined in the plane of this flat surface

EXAMPLE: A rectangular element, triangular element.

3.19

three-dimensional element

element that takes the form of solids

EXAMPLE: Tetrahedral elements, hexagonal elements, etc.

3.20

mass element

element to indicate mass attribute

3.21

constraints

various restrictions to reduce the freedom a system

3.22

plane

shell

structure feature that the thickness directional dimension is much smaller than the length and width directional dimensions

Note 1 to entry: Flat surfaces are defined as plane, and curved surfaces are defined as shells.

3.23

high order element

element with boundaries indicated by secondary or higher order functions

3.24

displacement

variable to indicate the distance of the position changing of an object to a reference

3.25

load

force to apply to an object or a system

3.26

strength

structural resistance to destruction or plastic deformation

3.27

structural statics analysis

analysis of structural response given static or approximate static load without time parameters involved

3.28

structural dynamics analysis

analysis of structural dynamics characteristics and response given a combination of time-dependent load, inertia, and damping

3.29

aspect ratio

amount of ratio to indicate the longest and shortest edges of a two-dimensional or three-dimensional element

3.30

slenderness ratio

amount of ratio to indicate the calculated length of the rod to the swing radius of the rod section

3.31

warpage

degree to indicate the deviation of an element from a plane

3.32

skew

amount to indicate the degree of distortion of an element

3.33

interior angle

value of the angle of a triangle element or a quadrangle element to indicate the maximum or minimum inner angle inside the element

When inertia and damping effects have no or very little influence on the mechanical properties of the structure, statics analysis shall be adopted.

When loads or prescribed displacement/rotations are time dependent but slowly enough in order to neglect the inertia and damping effects, quasi static analysis shall be adopted.

When the effects of inertia and damping on the mechanical properties of structures cannot be ignored, dynamic analysis shall be adopted, including modal analysis, harmonic response analysis, spectral analysis, buckling analysis and transient dynamic analysis.

When the material has a linear elastic behaviour, the structure is subjected to small displacement and there is no contact mechanics between bodies, linear analysis shall be adopted.

When the material has a nonlinear behaviour or the structure are subjected to large displacement or there are bodies in contact, or any combination before, nonlinear analysis shall be adopted. See Annex C for details.

Before establishing the finite element model, the finite element analysis scheme shall be formulated according to the structural characteristics, load, and constraint (or boundary condition) characteristics, simulation purpose, simulation cycle and computing resources of mechanical products.

During the simplification of the geometric model, the details of the geometric model such as edges, small grooves, bolt holes, process holes and fillet angles of the structure can be simplified as much as possible under the premise of ensuring the accuracy of the finite element analysis of the concerned parts.

When selecting elements, the type of elements shall be reasonably selected according to the geometric model of mechanical products, load and constraint characteristics, and the type and purpose of finite element analysis to ensure the calculation accuracy.

During meshing, areas with slow stress changes should be rough, and areas with sharp stress changes should be refined; areas of unconcern (areas built into the model only for pass-through) should be rough and areas of concern should be refined; the purpose of simulation as well as the availability of resources of computation should also be considered.

The selection of calculation method shall be determined according to the type of finite element analysis of mechanical product structure, the requirements of analysis results, the scope of application and advantages and disadvantages of the algorithm, the scale of finite element model and computer resources.

The analysis of model and the evaluation of calculation results shall be performed according to the analytical type and testing results.

The analysis results (list, contour map, curve map, etc.) shall be output according to the purpose and requirements of finite element analysis.

The coordinate system shall be determined by the right-hand rule, cartesian coordinate system should be selected, cylindrical coordinate system or spherical coordinate system can be selected if necessary. The global coordinate system shall be defined in finite element analysis modelling, and the local coordinate system can be added when the model loads, constraints or result display requirements are inconsistent with the global coordinate system.

The unit system shall be chosen according to the design unit of the mechanical product geometry model. Common units include M-KG-S SI system and MM-T-S system. See Tables B.1 and B.2 for details.

The finite element analysis procedure of mechanical product structure mainly includes following steps: finite element modelling (steps to composite a finite element model including geometric model construction and/or processing, material attribute definition, meshing, and boundary condition adoption, number, and type of elements), structural analysis via FEA model, results evaluation, results interpretation, FEA report, and archive. See Annex A for a complete flowchart.

Before establishing the finite element model, the finite element analysis scheme shall be formulated according to the structural characteristics, load, and constraint (or boundary condition) characteristics, simulation purpose, simulation cycle and computing resources of mechanical products.

The modelling principle is as follows:

a) Geometric models should express the structure design information of mechanical products in a concise and accurate manner.

b) The models should be as simplified as possible if fulfil the requirements.

c) If the geometric model and boundary conditions are symmetric, the symmetric structure model can be used.

The modelling requirements are as follows:

a) The geometric model shall be constructed in accordance with ISO 17599:2015, Clause 8.

b) The naming of geometric models shall adopt characters that can be recognized by software and should be kept unique.

c) The geometric model should be established in a 1:1 ratio.

d) For structures with slenderness ratio greater than 8, the middle axis should be selected for construction.

e) If the ratio of typical structure size to wall thickness is greater than 10, the middle plane should be selected for construction.

f) Solid construction shall be adopted for structures and key parts of structures that are not suitable for line, plane, or shell construction.

Before establishing the finite element model, the finite element analysis scheme shall be formulated according to the structural characteristics, load, and constraint (or boundary condition) characteristics, simulation purpose, simulation cycle and computing resources of mechanical products.

The selection of element types of mechanical products shall reflect the structural forms of different parts. Finite element types include zero-dimensional element (such as mass element), one-dimensional element (such as rigid element, bar element, beam element), two-dimensional element (such as shell element), and three-dimensional element (such as body element). During modelling, the element type shall be selected according to the geometric characteristics and requirements of the structure.

The modelling requirements are as follows:

a) High order element should be selected when the structure shape is irregular and the stress distribution is complex.

b) The high order element should be used in the area requiring high precision, and the low order element should be used in the area requiring low precision.

c) The connection positions of different order elements should use transition elements or multi-point constraints.

The definition of the density of elements is as follows:

a) Refinements shall be carried out for parts with large structural changes, surface curvature changes, load changes or connections of different materials.

b) The element size transition shall be smooth, and there shall be enough elements between the coarse and fine meshes to transition, to avoid the mass and stiffness difference between adjacent elements.

c) The mesh density of stress response area shall be greater than that of displacement response area.

d) The size of the unit in the direction of the main bearing force shall be small, and the unit perpendicular to the direction can be slightly enlarged to meet the quality requirements.

The meshing are as follows:

a) The main geometric outline shall be retained and the mesh shall be basically consistent with the geometric outline.

b) For solid meshing element, more than three layers shall be ensured in the direction of structural thickness.

c) Symmetrical mesh should be used for symmetrical structure.

d) For solid meshing element, hexahedral mesh should be used.

The unit system of material properties shall be consistent with that of geometric model.

The input information of material properties shall be accurate and complete for accurately expressing the stiffness, mass, and damping characteristics of the structure.

Material property information verified by experiments should be used as data accumulation for reference in material property setting.

The constraint is as follows:

a) The constraint of finite element model of mechanical products shall conform to the actual installation conditions.

b) Application mode shall be selected according to the constraint type.

NOTE All degree of freedom constraints shall be selected for a fixed support. Translational freedom constraints shall be selected for hinge support.

c) Symmetric or antisymmetric constraints shall be selected for symmetric structures or antisymmetric structures, respectively.

d) The constraint area shall be able to accurately reflect the actual constraints. Single point constraints shall be avoided to prevent stress concentration; If the actual constraint area is less than one element, more than four nodes shall be constrained or the mesh shall be refined.

The load is as follows:

a) The load type shall be selected according to the actual load. The loads commonly used in structural statics analysis include gravity load, acceleration load, ice and snow load, wind load, temperature load, displacement load, etc. The loads commonly used in structural dynamic analysis include impact loads, vibration loads and spectral loads.

b) The amount, direction and action area of the load shall conform to the actual load.

c) Load information verified by test can be used as data accumulation for reference of load application.

Prescribed displacements and rotations with specific value, including zero, can be applied to the structural analysis.

Before establishing the finite element model, the finite element analysis scheme shall be formulated according to the structural characteristics, load, and constraint (or boundary condition) characteristics, simulation purpose, simulation cycle and computing resources of mechanical products.

The geometry check is as follows:

a) When establishing the finite element model, the structure of the geometric model shall be checked, and the specific check contents are as follows.

b) Check geometry model integrity. According to the structural design requirements, check whether the geometric model has geometric feature loss, missing or deformity.

c) Check geometry model size. Check whether the feature size of the geometric model is consistent with the design size.

d) Parts check. Check geometry model for missing parts.

The meshing properties check is as follows:

a) When dividing the elements, the mesh shall be checked. The specific check contents and requirements are as follows.

b) There shall be no distorted mesh in the model. The main parameters of mesh check include element direction, aspect ratio, warpage, skew, and interior angle. In element division, the recommended quantization requirements of the above parameters are shown in Table B.3.

c) Ensure high quality of elements in key areas of the structure, while the quality of units in non-key areas can be appropriately reduced.

In finite element modelling, check shall be performed to the model mass distribution, total mass, centroid distribution, and other factors that affect the accuracy of calculation, and check whether the mass distribution and centroid distribution of each part of the model after counterweight are consistent with the actual state.

The engineering properties check is as follows:

a) After the completion of element division, the engineering characteristics of the finite element model shall be checked. The specific check contents and requirements are as follows.

b) Material parameter check. According to the material characteristics of mechanical product structure design, the material parameters are reviewed to check whether the material parameters are consistent with the design. Check whether the material parameter settings are complete and meet the analysis requirements according to the analysis type.

c) Element type check. According to the geometric characteristics of mechanical products, analysis requirements and assembly mode, the element type is checked to find out whether the selection of unit type is consistent with the structural form and connection mode.

d) Check the connection relationship. According to the installation and connection relation between the parts of the mechanical product structure, check whether the connection relation between the parts is established, and check and confirm the rationality and connection attribute of the connection relation.

e) Constraint check. According to the mechanical product structure installation interface, check the constraints, check whether the constraints are consistent with the installation conditions.

f) Load check. According to the working load condition of mechanical product structure, check the load, check the load type, load size, load object and area of action are consistent with the working load condition.

g) Displacement and/or rotation check. According to the working displacement condition of mechanical product structure, check the displacement, check the prescribed displacement/rotation type, prescribed displacement and/or rotation size, prescribed displacement/rotation object and area of action are consistent with the working condition.

Under the conditions of convergence, computing precision and computer resources, a reasonable computing time step should be set accordingly.

The model analysis is performed as follows, see Annex C for details.

a) A modal extraction linear method can be used for calculation of modes and natural frequencies (by e.g., Block Lanczos method) of structures under free vibration.

b) A reasonable modal order or modal upper limit shall be set according to the number of modes and modal calculation method.

c) The upper limit of the number of modes is the maximum number of degrees of freedom of the model.

Determine the dynamics response of a structure when loads are time dependent is obtained as a combination of the shape modes calculated from modal analysis. It is valid for linear structural analysis.

The geometry check is as follows:

a) Determine the response of a structure to a steady state at specific frequencies under sinusoidal excitation loading.

b) Direct integration method can be used in calculation, and modal superposition method can be used when calculation efficiency is low.

c) The modal superposition method shall not be used when applying non-zero displacement.

d) All modes that contribute to vibration response shall be extracted when modal superposition method is used to extract modes.

The spectrum analysis is as follows:

a) Estimate the structural dynamics response when non-deterministic transient dynamic events occur.

b) A modal extraction method can be used to extract the modes, e.g., Block Lanczos method.

c) The extracted modal number shall extract all modes in the concerned frequency band that contribute to the vibration response.

d) The excitation spectrum and direction shall be defined.

The transient dynamic analysis is as follows:

a) When a nonlinear dynamics analysis of structures subjected to arbitrary time dependent loads, a transient dynamic analysis shall be used. It is valid to linear analysis.

b) Direct integration method can be used in calculation, modal superposition method can be used when the calculation efficiency is low.

c) The modal superposition method shall not be chosen when applying non-zero displacement.

d) A constant time step shall be used for the modal superposition method.

The buckling analysis is as follows:

a) A modal method used to calculate how the critical load of the structure and the buckling shapes modes.

b) A modal extraction method can be used for eigenvalue buckling analysis, e.g., Block Lanczos method.

c) After eigenvalue buckling analysis is completed, nonlinear buckling analysis can be carried out.

The qualitative evaluation method is as follows:

a) Qualitative evaluation is carried out through the representation of results, and the specific principles are as follows.

b) Check the convergence of the mode.

c) Analyse the rationality of stress concentration position.

d) According to the structure vibration response curve and modal calculation results, the rationality of the generated wave peaks and troughs is analysed.

The displacement boundary and model parameters of the finite element model were modified several times, and the reliability of the analysis results was evaluated numerically.

Carry out physical prototype test and compare the finite element analysis results with the test results. If the deviation is large, revise the finite element analysis model and evaluate it after recalculation based on the test results.

Both representation and numerical methods shall be used to evaluate the analysis results. If necessary, physical prototype method should be used to evaluate the results. After the evaluation, if there is deviation between the analysis result and the actual state of the structure, the element type, order, mesh size, material attributes and boundary conditions of the finite element model shall be modified according to the situation, and recalculated and evaluated until the results meet the evaluation requirements. See Tables C.1 for details.

The concerned statics analysis results shall be read-in before displaying and/or outputting.

The output should contain parts of the stress, strain and deformation contour map of all or part of the content.

The results for modal analysis are as follows:

a) The concerned modal analysis results shall be read-in before displaying and/or outputting.

b) The output should contain all or part of the line chart that focuses on the inherent frequencies, modal vibration patterns, relative displacements, relative stresses, and relative strains within the frequency band.

The results for harmonic response analysis are as follows:

a) The concerned harmonic response analysis results shall be read-in before displaying and/or outputting.

b) According to the vibration response of a typical location node structure focus on regional (displacement, stress, strain, force, etc.), extreme of the spectrum curve to determine the frequency of vibration response of the distribution of value of demand.

c) To calculate the amplification coefficient, converting vibration displacement response for the same type of dimension according to the type of incentives (acceleration or velocity).

d) Harmonic response analysis in the output shall contain the result of the structure on band on the vibration of the measuring point displacement, velocity, acceleration, stress variables such as amplitude, phase, real or imaginary part and frequency curve, typical structure under the frequency excitation of the deformation, stress and strain contour and vector diagram or list. All or part of the relation curve between amplification coefficient and frequency of measuring points in frequency band.

The results for spectrum analysis are as follows:

a) The concerned spectrum analysis results shall be read-in before displaying and/or outputting.

b) Spectrum analysis results of output shall contain one sigma displacement, velocity, acceleration, stress, strain, force the equivalent figure and concerns of the power spectral density curve.

The results transient dynamic analysis are as follows:

a) The concerned transient dynamic analysis results shall be read-in before displaying and/or outputting.

b) According to the vibration response of a typical location node structure focus on regional (displacement, stress, strain, force, etc.), time history curve of extremum determine should focus on the vibration response of the critical point in time.

c) Transient dynamics analysis output shall contain the result of the structure on the measuring point displacement, velocity, acceleration and stress time history curve of the variable, the typical time points in the structure of the deformation, stress and strain contour and vector diagram or list.

The output should be presented in an appropriate format, such as in dynamic files, in written, as numerical, as a model.

There shall be a background introduction to the analysis and an explanation of the type of analysis taken in this report and the results of the analysis to be of concern.

When data or conclusions from other files are included, they shall be clearly stated in the appropriate section of the report and given the author, name, and time of the reference file.

Necessary explanations shall be given to the symbols that appear for the first time, and they can be directly quoted when continuing to be quoted below.

The analysis process includes model simplification, meshing, material model, boundary conditions, loads and solution methods, which shall be explained as necessary one by one.

Typical diagram results, such as stress and/or strain cloud, modal shapes, etc., shall be given. The chart shall be concise and easy to understand. There shall be no extraneous information in the chart. According to the results of the chart, the conclusions are summarized, such as strength characteristics, vibration characteristics, etc. See Annex D for details.

Relevant references, reports, etc. shall be indicated at the end of the report, including the author, full name and date of publication of the reference documents.

Archival files of finite element input shall meet at least the following requirements:

— Geometric model of mechanical product structure shall be archived and managed;

— Parameters and instructions of the structural design of mechanical products shall be archived and managed;

Archival files of finite element model shall meet at least the following requirements:

— Final model of finite element analysis model shall be archived;

— Finite element model shall be opened, run and output accurately by a computer normally.

Archival files of analysis report shall meet at least the following requirements:

— Analysis reports shall be archived in an un-editorial format such as PDF. If archive analysis reports are archived in an editorial format such as Word, the report content shall not be modified;

— Analysis report shall be opened and output accurately by a computer normally;

— The reference documents in the analysis report shall be archived properly so that they can be referred to as necessity.

Finite element model and analysis report to be archived shall meet at least the following requirements:

— Finite element model and analysis report library shall be established, and the management regulations of finite element model and analysis report library shall be formulated, and the storage, revision and removal of models and reports shall be strictly managed;

— The management department of the finite element model and analysis report database shall register and account the finite element model and analysis report in time;

— The finite element model and analysis report that has been archived shall be filled in the warehousing registration form, uploaded, and released.

Revision of models and reports shall meet at least the following requirements:

— When the finite element model and analysis report in storage needs to be revised due to the change of technical status or other circumstances, it shall go through a strict process of change;

— After obtaining the permission to make the change, mark the according finite element model and analysis report in the database as "Under Revision";

— After the revision is completed, fill in the revision registration form, re-store the new version model and analysis report, and release them.

Removing of models and reports shall meet at least the following requirements:

— The models and reports that have exceeded the storage period shall be identified;

— The models and reports that have no use or reference value after identification shall be filled in the removal registration form and removed from the database for destruction.

The management department of finite element model and analysis report database shall sort out the models and reports in the database regularly, and add, revise, utilize and remove statistical models and reports to form management status report.

1. 
   (informative)
   
   A flowchart for the process of the FEA structural analysis for mechanical products

Figure A.1 shows a common process of finite element analysis for mechanical products.

Figure A.1 — A common process of finite element analysis for mechanical product structure

1. 
   (informative)
   
   System of units and parameters for element properties check
   1. SI unit system

Table B.1 shows recommended SI unit system for modelling mechanical product analysis and modelling that is sensitive to quality is given.

Table B.1 — SI unit system

• 1. Unit System 2

Table B.2 shows unit system recommended for modelling mechanical product analysis and modelling that is not sensitive to quality is given.

Table B.2 — Unit system 2

• 1. Unit quality checks

Table B.3 shows unit quality check control parameters in the finite elements analysis modelling requirements are given.

Table B.3 — Unit quality check control parameters

1. 
   (informative)
   
   Use case
   1. Statics analysis of U-groove
      1. U-groove example

This example will create a finite element model of a given U-groove model, apply loads and set boundary conditions, perform finite element analysis, and observe the results of loaded U-groove deformation and stress.

This example includes the following steps:

— Establish the finite element model;

— Apply load, set boundary conditions and solver controls;

— Solve and submit the calculation;

— Review and post process the result.

• • 1. Establish the finite element model

The process are as follows:

a) Open or generate the model file and deal with the geometry, as shown in Figure C.1

Key

1 rib

2 bottom two surfaces, one with three interior fixed points

Figure C.1 — Loading the geometric model

b) The mesh was divided and the free edges of the mesh were checked. Use quadrilateral and triangle element type, and the generated mesh as shown in Figure C.2

c) Define material and geometric properties. The elastic modulus of the material is 2E+5 MPa, Poisson's ratio is 0,3, density is 7,9E-9 kg/m³, and material thickness is 3 mm. The unit system should be consistent if the software does not define any.

Figure C.2 — Creating a mesh

• • 1. Apply load and set boundary conditions

The process are as follows:

a) Create a set of loads (Single-point constraints and forces).

b) Create constraints, select the points need to be constrained, and create the constraints as shown in Figure C.3

Figure C.3 — Create constraints

c) Apply a load, select the point where the force needs to be applied, and apply the load as shown in Figure C.4

Figure C.4 — Applying load

d) Create a load condition (Load step). This example is linear solution.

• • 1. Solve and submit the calculation

The calculation is solved and submitted.

• • 1. Review and post-process the results

In this example, the process are as follows:

a) View the stress cloud, as shown in Figure C.5

Figure C.5 — Stress cloud diagram

b) View the displacement cloud map, as shown in Figure C.6

Figure C.6 — Displacement cloud diagram

• 1. Modal analysis
     1. A flat plane example

Modal analysis is the most basic and important analysis in dynamic analysis. Through modal analysis, modal frequency, vibration shape and damping of workpiece can be obtained, which provides reference for the design and structural optimization of workpiece. Figure C.7 shows a flat plane for modal analysis.

Figure C.7 — Creating a model for modal analysis

• • 1. Material and unit

In this example, aluminium alloy GE isotropic material and MM-T unit system are selected.

• • 1. Material parameters setting

Set material parameters, including elastic modulus, Poisson's Ratio and density.

• • 1. Element type

Use the 2D element and shell element, set the thickness.

• • 1. Constraints

Create constraints. Select the points need to be constrained, and create the constraints as shown in Figure C.8

Figure C.8 — Setting constraint 2

• • 1. Range of modal solution

Set the range of modal solution. In this example, the first six modes were solved.

• • 1. Calculation

Submit the calculation.

• • 1. Result output

Review and post process the results. In this example, the first-order modal shape is shown in Figure C.9

Figure C.9 — Result output

• 1. Nonlinear analysis of a clamp
     1. Nonlinear structural assessment of a clamp loading then unloading

This example will create a nonlinear (material model) finite element model of a given clamp, apply a load then unloading the load using a time curve load input, set suitable meshing parameters, and set boundary conditions, perform finite element analysis, and observe the results of loaded and unloaded deformation, stress, and total strain.

• • 1. Establish the finite element model

The process are as follows:

a) Open or generate the model file and deal with the geometry, as shown in Figure C.10

Figure C.10 — Loading the geometric model

b) The mesh was divided, and the free edges of the mesh and element size parameters were checked (aspect and Jacobian ratios). Tetrahedral element type was used, a finer mesh was defined by a mesh constraint on the lever arm clamping geometry and the generated mesh was shown in Figure C.10

c) Define the nonlinear material model (plasticity von Mises, stainless steel AISI 316) and geometric properties. The elastic modulus of the material is 1,93E+5 MPa, Poisson's ratio is 0,3, density is 8E-9 kg/m³, and the tangent modulus is 2,06E+4 MPa. The unit system should be consistent if the software does not define any unit set.

• • 1. Apply load, set boundary conditions and solver controls

The process are as follows:

a) Create constraints, select the points need to be constrained, and create the constraints as shown in Figure C.11

Figure C.11 — Create constraints

b) Set contact conditions on the contact surface sets, as shown in Figure C.12 Coefficient of friction setting is optional.

Figure C.12 — Create contact conditions

c) Create a load of 1 000 N on the split surface indicated in Figure C.13 and apply as time curve as indicated in Figure C.14 and Table C.1 Note this is to assess post-processing when loaded and after loading.

Figure C.13 — Applying load

Figure C.14 — Load curve

Table C.1 — Numerical value of load curve

d) Set solver settings as follows: end time 1 second, time step: automatic, solver type Fuzzy Front End (FFE) plus and use large displacement solver option. This example is a nonlinear time stepped solution.

• • 1. Solve and submit the calculation

The calculation is solved and submitted.

• • 1. Review and post process the results

In this example, the process are as follows:

a) View the stress plot at a time of 0,5 second (loaded), as shown in Figure C.15

Figure C.15 — Stress plot - loaded

b) View the stress plot at a time of 1 second (unloaded after loading), as shown in Figure C.16

Figure C.16 — Stress plot - unloaded after loading

c) View the displacement plot at a time of 0,5 second (loaded), as shown in Figure C.17

Figure C.17 — Displacement plot - loaded

d) View the displacement plot at a time of 1 second (unloaded after loading), as shown in Figure C.18

Figure C.18 — Displacement plot - unloaded after loading

e) View the total strain plot at a time of 0,5 second (loaded), as shown in Figure C.19

Figure C.19 — Total strain plot - loaded

f) View the total strain plot at a time of 1 second (unloaded after loading), as shown in Figure C.20

Figure C.20 — Total strain plot - unloaded after loading

• 1. Linear dynamic random vibration analysis
     1. Linear dynamic random vibration assessment of an ultrasonic sensor PCB assembly

This example will create a linear dynamic random vibration assessment of an Ultrasonic Sensor PCB assembly, apply an excitation to a frequency range using a time curve of frequency (in Hertz) against gravity acceleration (in m/s²), i.e. Hz vs g, set suitable meshing parameters, set suitable element types based on the geometry, set boundary conditions, perform finite element analysis, and observe the results of frequency response / natural frequency, mass participation factor, stress, and deformation acceleration.

• • 1. Establish the finite element model

The process are as follows:

a) Open or generate the model file and deal with the geometry, as shown in Figure C.21

Figure C.21 — Loading the geometric model

b) The mesh was divided, and the free edges of the mesh and element size parameters were checked (aspect and Jacobian ratios) were checked. Tetrahedral element type with a method of curvature based was used and the generated mesh as shown in Figure C.21

c) Define the linear material models and geometric properties for the parts as shown in Table C.2

Table C.2 — Material properties

• • 1. Apply load, set boundary conditions and solver controls

The process are as follows:

a) Create constraints, select the points need to be constrained, and create the constraints as shown in Figure C.22

Key

1 PCB

2 sensor

3 header

4 connector legs

Figure C.22 — Create constraints

b) Create a base excitation to the whole geometric model applied perpendicular to the PCB face as shown in Figure C.23 and apply as time curve as indicated in Figure C.24 and Table C.3

Figure C.23 — Create base excitation

Figure C.24 — Frequency curve

Table C.3 — Numerical value of frequency curve

c) Set solver settings as follows: number of frequencies to solve: 50, automatic, solver type FFE plus, soft springs option (to stabilize model frequency lower limit 20 Hz, upper lower limit 2 000 Hz and number of frequency points: 10. Set the results options based on hard drive space, required accuracy, and solve time across frequency sweep. This example is a linear dynamic time stepped solution.

• • 1. Solve and submit the calculation

The calculation is solved and submitted.

• • 1. Review and post-processing the results

In this example, the process are as follows:

a) Solve the frequency solver step and plot a table of resonant frequencies as shown in Figure C.25 and review modal plots as shown in Figure C.26 Then plot and review the table of the mass participation factor as shown in Figure C.27

Figure C.25 — Plot list of resonant frequencies

Figure C.26 — Mode shape plot

Figure C.27 — Table of mass participation factors

b) View the stress plot as shown in Figure C.28

Figure C.28 — Stress plot

c) View the displacement plot, as shown in Figure C.29

Figure C.29 — Displacement plot

d) View the acceleration plot, as shown in Figure C.30

Figure C.30 — Acceleration plot

1. 
   (informative)
   
   Template of the report of finite element analysis of mechanics
   1. Object to be analysed

This annex describes the analysis object and applicable environment scope of the analysis object.

• 1. Problem to be solved

To deal with the analysis of the problem of a certain background, explain the purpose of the analysis. The type of analysis adopted in this report and the analysis results to be focused on are also described.

• 1. Reference files and symbols description

The inclusion of data or conclusions from other documents should be clearly indicated in the corresponding section of the report, and the author, name and time of the reference should be given. Necessary explanations should be given to the symbols that appear for the first time, and they can be directly quoted when continuing to be quoted below.

• 1. Simulation analysis process

The analysis process includes model simplification, meshing, material model, boundary conditions, loads and solution methods, and the above should be explained one by one as necessary and illustrated with drawings.

• 1. Results analysis and conclusions

Typical diagram results should be given, such as stress or strain cloud diagram, modal shapes, etc. The chart should be concise and easy to understand. There should be no extraneous information in the chart. According to the results of the chart, the conclusions are summarized, such as strength characteristics, vibration characteristics, etc.

• 1. References

Relevant references, reports, etc. should be indicated at the end of the report, including the author, full name and date of publication of the reference documents.

Bibliography

[1] ISO 10303‑104:2000/Cor 2:2014, Industrial automation systems and integration—Product data representation and exchange—Part 104: Integrated application resource: Finite element analysis

[2] ISO 10303‑107:2019, Industrial automation systems and integration — Product data representation and exchange — Part 107: Integrated application resource: Finite element analysis definition relationships

[3] ISO 16792:2021, Technical product documentation — Digital product definition data practices

[4] ISO 18437‑5:2011, Mechanical vibration and shock — Characterization of the dynamic mechanical properties of visco-elastic materials — Part 5: Poisson ratio based on comparison between measurements and finite element analysis

[5] ISO 21143:2020, Technical product documentation — Requirements for digital mock-up virtual assembly test for mechanical products