ASTM F3161-2016 Standard Test Method for Finite Element Analysis (FEA) of Metallic Orthopaedic Total Knee Femoral Components under Closing Conditions《在封闭条件下对金属骨科全膝关节股骨组件进行有限元分析 (FE.pdf

《ASTM F3161-2016 Standard Test Method for Finite Element Analysis (FEA) of Metallic Orthopaedic Total Knee Femoral Components under Closing Conditions《在封闭条件下对金属骨科全膝关节股骨组件进行有限元分析 (FE.pdf》由会员分享，可在线阅读，更多相关《ASTM F3161-2016 Standard Test Method for Finite Element Analysis (FEA) of Metallic Orthopaedic Total Knee Femoral Components under Closing Conditions《在封闭条件下对金属骨科全膝关节股骨组件进行有限元分析 (FE.pdf（7页珍藏版）》请在麦多课文档分享上搜索。

1、Designation: F3161 16Standard Test Method forFinite Element Analysis (FEA) of Metallic Orthopaedic TotalKnee Femoral Components under Closing Conditions1This standard is issued under the fixed designation F3161; the number immediately following the designation indicates the year oforiginal adoption

2、or, in the case of revision, the year of last revision. A number in parentheses indicates the year of last reapproval. Asuperscript epsilon () indicates an editorial change since the last revision or reapproval.1. Scope1.1 This standard establishes requirements and consider-ations for the numerical

3、simulation of metallic orthopaediccemented and cementless total knee femoral components usingFinite ElementAnalysis (FEA) techniques for the estimation ofstresses and strains. This standard is only applicable to stressesbelow the yield strength, as provided in the material certifica-tion.1.2 Purpose

4、This test method establishes requirements andconsiderations for the development of finite element models tobe used in the evaluation of metallic orthopaedic total kneefemoral component designs for the purpose of prediction of thestatic implant stresses and strains. This procedure can be usedfor wors

5、t-case assessment within a family of implant sizes toprovide efficiencies in the amount of physical testing to beconducted. Recommended procedures for performing modelchecks and verification are provided to help determine if theanalysis follows recommended guidelines. Finally, the recom-mended conte

6、nt of an engineering report covering the mechani-cal simulation is presented.1.3 LimitsThis document is limited in discussion to thestatic structural analysis of metallic orthopaedic total kneefemoral components (which excludes the prediction of fatiguestrength).1.4 The values stated in SI units are

7、 to be regarded asstandard. No other units of measurement are included in thisstandard.1.5 This standard does not purport to address all of thesafety concerns, if any, associated with its use. It is theresponsibility of the user of this standard to establish appro-priate safety and health practices

8、and determine the applica-bility of regulatory limitations prior to use.2. Significance and Use2.1 This standard is applicable to the calculation of stressesseen on a knee femoral component when loaded in a mannerdescribed in this test method. This method can be used toestablish the worst-case size

9、for a particular implant family.When stresses calculated using this method were compared tothe stresses measured from physical strain gauging techniquesperformed at one laboratory, the results correlated to within9%.3. Geometric Data3.1 Finite element models are based on a geometric repre-sentation

10、of the device being studied. The source of thegeometric details can be obtained from drawings, solid models,preliminary sketches, or any other source consistent withdefining the model geometry. In building the finite elementmodel, certain geometric details may be omitted from theorthopaedic implant

11、geometry shown in the Computer AidedDesign (CAD) model if it is determined that they are notrelevant to the intended analysis. Engineering judgment shallbe exercised to establish the extent of model simplification andshall be justified.3.2 It is most appropriate to consider the worst-case stresscond

12、ition for the orthopaedic implant family being simulated.The worst-case shall be determined from all relevant engineer-ing considerations, such as femoral component geometry anddimensions. If finite element analysis is being used for deter-mining the worst-case, then the worst-case size may not bekn

13、own. It may be necessary to run several sizes in order todetermine the worst-case. If the FEA results do not conclu-sively determine the worst-case configuration, a rationaleshould be included (e.g., additional analysis or physical test-ing) to justify the worst-case size.4. Material Properties4.1 T

14、he required material properties for input into an FEAmodel for the calculation of strains and displacement aremodulus of elasticity (E) and Poissons ratio (). These valuescan typically be obtained from material certification data. Itshould be noted that the fatigue test is run under load control;the

15、 FEA should also be run under load control. When the FEAis run under load control, the modulus of elasticity will notaffect the stress calculations under small displacement theorybut will affect displacement and strain. The influence ofPoissons ratio on the stress calculations is negligible.1This te

16、st method is under the jurisdiction of ASTM Committee F04 on Medicaland Surgical Materials and Devices and is the direct responsibility of SubcommitteeF04.22 on Arthroplasty.Current edition approved Feb. 1, 2016. Published March 2016. DOI: 10.1520/F316116Copyright ASTM International, 100 Barr Harbor

17、 Drive, PO Box C700, West Conshohocken, PA 19428-2959. United States14.2 Ensure that material property units are consistent withgeometric units in the CAD model. SI units are the preferredunits of measurement.5. Loading5.1 The loading location and orientation of the knee femoralcomponent shall be gu

18、ided by the loading location andboundary conditions described below. The areas of particularinterest are the stresses at the posterior aspect of the condyle,anterior notch, and other design-specific critical regions.5.2 The worst-case condyle shall be loaded. If the weakercondyle cannot be justified

19、, each condyle shall be analyzedindividually. Centrally locate a 7.62 mm diameter projectedcircle over the apex of the posterior articulating surface withthe knee femoral component positioned in 90 degrees offlexion. Apply an anterior directed 1 N load uniformly over theface generated by the interse

20、ction of this projected circle withthe articulating surface. Refer to Fig. 1 and Fig. 2.NOTE 1Do not introduce additional solid material to the femoralcomponent model.NOTE 2It is recognized that the loading conditions in this test methodwill not be identical to those of a physical testing standard c

21、urrently underdevelopment. However, the differences in loading conditions (e.g., loadapplication differences; potting level differences; use of bone cementwhich is not modeled in FEA) do not significantly affect identification ofthe worst-case stress condition and construct for subsequent bench test

22、ing,which is the primary objective of this test method.5.3 Ensure that load units are consistent with materialproperty units.6. Boundary Conditions6.1 The prescribed boundary condition idealizes embeddingthe anterior flange within a potting medium. The femoralcomponent shall be fixed in all translat

23、ions on all “embedded”anterior flange surfaces. Refer to Fig. 1 and Fig. 3.Ahorizontalplane shall be constructed to define a closed perimeter aroundthe anterior flange periphery. Note that the horizontal planemay not be parallel to the anterior flange bone cut face. The useof other stress evaluation

24、 levels and/or constraint levels shallbe justified.7. Analysis7.1 The analysis and modeling system, programs or soft-ware used for the finite element model creation and analysisshould be capable of fully developing the geometric featuresand idealizing the loading and boundary condition environmentof

25、 the orthopaedic implant. An engineering justification shallbe provided to support any assumptions and/or simplifications.7.2 The finite element mesh can be created using automaticmeshing, manual meshing, or a combination of the twotechniques. The overriding consideration is that the type, thesize,

26、and the shape of the elements used must be able torepresent the expected behavior without significant numericallimitation or complication. Most FEA packages have a built-inprogram which checks the shape of the element for the type ofanalysis selected. If this tool is not available, then additionalch

27、ecks are needed.7.3 The number and spacing of nodes (i.e. mesh density)should be consistent with the type of element used and the typeof result desired. This may be demonstrated with a meshdensity study, whereby a series of models with increasing meshrefinement in the critical stress regions is used

28、 to demonstratesolution convergence. This allows the error associated withsubsequent models to be estimated. The method used todemonstrate mesh convergence, in analysis cases where it isnot performed directly onto the model being analyzed, shall bedocumented in the FEA report. It is recommended that

29、 aFIG. 1 Apex Location and Anterior Flange Constraint (lateralview)FIG. 2 Apply 1 N Load onto Load FootprintFIG. 3 Anterior Flange ConstraintF3161 162minimum of three mesh refinement levels be evaluated and amodel convergence of 5% be demonstrated on all measuresand regions of interest. If differenc

30、es in peak stresses betweentwo sizes in a product family are calculated to be less than 5%,a tightening of the model convergence is recommended toincrease the likelihood of establishing the worst-case sizewithin a product family. Reporting of the degrees of freedom isnot necessary if the model satis

31、fies the convergence criterion.7.4 The choice of element type is left to the analyst;however, it is recommended for analysis of a knee femoralcomponent that tetrahedral or hexahedral elements be used. Iftetrahedral elements are considered, use of 4-noded elementsshould be avoided to prevent stress a

32、nd strain incompatibilitiesacross elements. Additionally, the linear, 4-noded tetrahedronelement is a constant strain element. This means that displace-ment interpolation is linear and the corresponding stresses andstrains are constant within any element. Therefore, a veryrefined mesh is required ar

33、ound locations where high stress/strain gradients are present when utilizing these elements.When elements which are not directly identified in this testmethod are used, documentation which demonstrates theirvalidity shall be provided in the FEA report.7.5 The finite element results should be examine

34、d to ensurethat the geometrical models of the implant, boundary condi-tions and applied loads have been appropriately defined in theanalysis and properly represent the behavior being analyzed.Examples of model behavior which should be examinedinclude the reaction forces and moments as well as the ov

35、eralldeflected shape and deflection magnitude.7.6 The measure of interest is the Maximum (1st) PrincipalStress. Refer to Fig. 4. Stress concentrations near the boundarycondition regions are considered to be artifacts and shall not beconsidered to be regions of interest. If other stress values areuse

36、d, their validity for use should be documented.8. Report8.1 The finite element analysis for the evaluation of anorthopaedic implant should be fully documented in an engi-neering report. The actual format of the report should complywith any acceptable proprietary or non-proprietary engineeringreport

37、format; however, the report shall include, at a minimum,the following:8.1.1 A complete description of device being analyzedincluding detailed dimensions. The report should reference asource CAD geometry file by name and revision number. If theevaluation is not being performed on the final design of

38、thedevice or if there are other significant assumptions that maylimit the use of the results, this shall be clearly stated.8.1.2 A description of boundary constraints, loads, andmaterial properties. The source of the material property datautilized should be referenced.8.1.3 A summary of the finite e

39、lement modeling and analy-sis system used for the analysis. If current versions of widelyused, commercially available software are used, this summarycan be by name and reference to the version used. Fornon-commercially available proprietary tools, or custom usermodification of commercially available

40、 software, sufficienttechnical background and results of test problems should beprovided to demonstrate the utility, verification, applicabilityand limitations of the software tool.8.1.4 A description of the procedure used to convert thegeometric or CAD representation of the device to the finiteelem

41、ent model. Any geometry simplifications should be docu-mented.8.1.5 A description of the finite element model and itsrelation to the device being evaluated. The number of nodesand elements (or the degrees of freedom in the model), thefinite element type selected including its capabilities, and anysp

42、ecial considerations involved in the model should be in-cluded. For each region of interest, the maximum (1st) princi-pal stress and von Mises stress at the location of maximum(1st) principal stress shall be reported. Additional stress com-ponents can be included and their incorporation shall bejust

43、ified.8.1.6 Adescription of mesh convergence considerations andhow they were applied to the analysis.8.1.7 A description of any numerical considerations orconvergence criterion associated with the analysis.FIG. 4 Stress Plot (arrows point to regions of interest)F3161 1638.1.8 A summary of analysis r

44、esults using all appropriateforms of text, graphics and tabular representations of data tohighlight the key behavioral characteristics involved in theevaluation.8.1.9 Engineering conclusions or recommendations, as ap-propriate.8.1.10 Deviations from this standard.8.1.11 All relevant references and s

45、upporting documenta-tion and drawings.9. Precision and Bias9.1 The precision and bias of this test method has not beenestablished.10. Keywords10.1 computational simulation; displacement; FEA; finiteelement analysis; model calibration; model validation; modelverification; orthopaedic implants; soluti

46、on sensitivity; strain;stressAPPENDIXES(Nonmandatory Information)X1. FEA ROUND ROBIN STUDYX1.1 A round robin study was performed with 9 labs on arepresentative knee femoral component model (refer to Fig. 1and Fig. 2 for geometry) following the procedure in this testmethod. The stresses in the poster

47、ior aspect of the medialcondyle and anterior notch were evaluated (Fig. 4). Themaximum percent difference from the overall average was lessthan 1.0% (Table X1.1).TABLE X1.1 Round Robin FEA Model ResultsMaximum Principal Stress (MPa)A,B,CRound Robin ParticipantIdentifierCondyle Region MaxPrincipal St

48、ress (MPa)Notch Region MaxPrincipal Stress (MPa)% Condyle Stress FromAverage% Notch Stress fromAverage1A 0.1187 0.1026 -0.01 0.331B 0.1188 0.1019 0.07 -0.422B 0.1178 0.1018 -0.75 -0.453A 0.1189 0.1027 0.16 0.394A 0.1188 0.1023 0.03 0.034B 0.1190 0.1027 0.20 0.405A 0.1188 0.1026 0.10 0.326C 0.1189 0.

49、1026 0.16 0.327D 0.1190 0.1030 0.24 0.688A 0.1182 0.1016 -0.41 -0.698B 0.1186 0.1018 -0.09 -0.499A 0.1189 0.1020 0.16 -0.309B 0.1189 0.1022 0.16 -0.10Average 0.1187 0.1023Standard Deviation 0.0003 0.0004Range -0.75 to 0.24 -0.69 to 0.68AAll laboratories used 10-noded tetrahedral elements.BAll laboratories used the recommended convergence criterion of # 2%. However, also note that the 2% convergence criterion was not necessarily performed in bothregions of interest individually in the round robin. It is recommended that model convergence within each region of interest is # 2%