Patran / Nastran Lecture / Julien Le Fanic Tp ´nie Me ´canique Ge ´nierie des Syste `mes Inge February th Lectures Scope Lectures Scope 2/71 1. Lecture 1 deals with basics Finite Elements Method and introduces Nastran and Patran softwares. A cantilever beam is studied in linear elasticity and then with geometrical non linearity. If time left students can realize another exercise defined in appendixes §D. 2. Lecture 2 deals with plates and shells. A 2D plate with a hole is studied to assess a KT . Then buckling modes are computed for the same plate under compressive load. Finally a Guyan static reduction is performed. 3. Lecture 3 will let students finish Lecture 2 case studies before an assessment of a time dependent response for a beam and a contact 3D modelization. 4. Lecture 4 deals with Fsm idealization. Lecture 2/4 - Table of Contents Table of contents Lectures Scope Lecture 2/4 - Table of Contents The theory of Finite Elements Method Weak Form Simple axial element Simple bending element Extra case study Definition Case study # 3 - Plate with a hole Definition Meshing Technique KT assessment Closed form solution Nastran linear static run Results from Nastran linear static run from .op2 Conclusion & Outlook Case study # 4 - Buckling Analysis Theoretical Apart´ e Definition Mesh Nastran EIGRL Card Nastran buckling run Results from Nastran buckling run from .f06 Results from Nastran buckling run from .op2 Conclusion & Outlook Case study # 5 - Guyan Static Reduction Theoretical Apart´ e Definition Nastran ASET Card Nastran EXTOUT Parameter Nastran linear static run for reduction 3/71 Lecture 2/4 - Table of Contents Table of contents Results from Nastran linear static run from .pch Reading external element Nastran linear static run for residual structure Results from Nastran linear static run from .op2 Conclusion & Outlook References 4/71 The theory of Finite Elements Method Weak Form The theory of Finite Elements Method Weak form One solves −∆u = f u=0 in on Ω ∂Ω . . . . . . . . . . . . . . . . . . . . (17) It is considered f ∈ L2 (Ω). It is assumed u ∈ H 2 (Ω) . Thus by Green formula Z Z ∇u · ∇vdΩ = Ω ∂u Z f vdΩ + Ω . . . . . . . . . . . . . . . . . (18) , ∀v ∈ H0 (Ω) . . . . . . . . . . . . . . . . (19) ∂Ω ∂n vdΓ If it is chosen v ∈ H01 (Ω) one has Z Z ∇u · ∇vdΩ = Ω f vdΩ 1 Ω The equation (19) is called the variational formulation or the weak form of the differential equation (17). 5/71 The theory of Finite Elements Method Simple axial element The theory of Finite Elements Method Simple axial element N1 (x) N2 (x) y F1 ,u1 F2 ,u2 x l Figure 1: Simple axial element assumption sketch Linear form function N1 (x) = 1 l − x l 2 N2 (x) = 1 x + l l 2 . . . . . . . . . . . . . . u1 u2 . . . . . . . (20) . . . . . . . (21) Strain worth ε=B 6/71 u1 u2 = h ∂N1 ∂x , ∂N2 ∂x i u1 u2 = h − 1l , 1 l i The theory of Finite Elements Method Simple axial element The theory of Finite Elements Method Simple axial element Stiffness matrix is derived as l Z Z2 T K = E B EBdΩ = S Ω l2 −l 2 −1 1 1 −1 dx . . . . . . . . . . . . . . . (22) The simple bar element works merely as∗ F1 F2 = ES l −1 1 1 −1 u1 u2 . . . . . . . . . . . . . . . . . (23) with stiffness matrix K = ES l −1 1 1 −1 . . . . . . . . . . . . . . . . . . . . . . (24) . . . . . . . . . . . . . . . . . . . . . (25) Nota : Mass matrix is derived as M = ρSl 6 2 1 1 2 . . Nastran’s user can output K, M or any matrix in an .op2 or an .op4 file. ∗ 7/71 . . . a F = k u spring © The theory of Finite Elements Method Simple bending element The theory of Finite Elements Method Simple bending element M1 ,θ1 M2 ,θ2 l F1 ,v1 Figure 2: F2 ,v2 Simple bending element assumption sketch For a simple bending element one has the relationship 8/71 F1 M1 F M2 2 6 2EI −3l = −6 3 l −3l −3l 2l2 3l l2 −6 3l 6 3l −3l v 1 l2 θ1 v 3l 2 θ2 2l2 . . . . . . . . . . . (26) Extra case study Definition Extra case study - Clamped curved beam linear analysis Definition The framework is linear elasticity. F R 2R y x B $ A% A load F is applied in C. The beam is clamped in A and supported in B. The beam has a rectangular 3 . The beam is made of section S = b × h with b = h = 10 mm and R = 1000 mm. Inertia worth Iz = bh 12 steel E = 200 GPa and ν = 0.30. A 100 kg mass has been hung at C. Aim of Extra Case study : Students have to run a Nastran SOL 101 analysis and assess the deformation of the structure. Closed form solution : At C displacement worth 9/71 vC = − 2π F R3 5 EIz . . . . . . . . . . . . . . . . . . . . . . . . (27) Case study # 3 - Plate with a hole Definition Case study # 3 - Plate with a hole Definition The framework is linear elasticity. The plate is t = 5 mm thick, w = 50 mm wide and L = 100 mm long. Structure is clamped Lhs and a σ0 = 100 MPa tensile load is applied Rhs. Hole has a diameter D = 10 mm. The plate is made of aluminium E = 70 GPa and ν = 0.33. Aim of Case study # 3 : Students have to find the stress concentration factor KT associated to the hole. 10/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Meshing Technique A square patch is to be designed under Patran around the hole. This will basically allow to have a better assessment of stress around the hole. 11/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Meshing Technique Background : In order to mesh a surface the latter may be defined. But it does exist a more efficient solution. Technique : A surface may be meshed only drawing in Patran boundary curves and using the Mesh > 2 Curves menu form. Example : Consider the two arcs in next Patran snapshots. One realizes the mesh of the surface between the 2 curves without necessity of its definition. 12/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Meshing Technique The patch is to be split under Patran in 8 subdomains. The mesh is to be built with Nastran CQUAD4 elements. Nota : 2 circles are not shown in the above figure but do exist to build the mesh. 13/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Meshing Technique With Patran sketch the patches first. Assumptions are : 14/71 1. choose the number of square elements around the hole N with N ≡ 0 mod [6] and N ≡ 0 mod [4] e.g. N = 72 2. circular patch around the hole for a side length N square elements 3. circular patch around the hole for 3a × 2a rectangular elements to be broken for the transition mesh 4. 2 × R radius circular patch around the hole 5. square patch has a 6 × R = 3 × D side length Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh The plate contains coarse CQUAD4 5 × 5 mm2 elements. 15/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh 16/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh 17/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh 18/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh 19/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh The plate contains a disk of transition elements from 1 to 3 CQUAD4. The transition is done in Patran splitting 24 CQUAD4 with the Utilities menu. 20/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh Background : In order to refine a mesh one can shape every element. But it does exist a more efficient solution to derive the fine mesh from a coarse mesh. Technique : Enter the Utilities> Fem-Elements > Break Elements menu form. Example : Consider the mesh done between the two arcs. One splits each CQUAD4 in four smaller ones with the selection of the desired element and an edge. 21/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh The circular boundary of the structure contains 72 CQUAD4. Nota : Remove duplicate nodes with the Equivalence Patran function of the Mesh Menu form. 22/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole Mesh 23/71 Case study # 3 - Plate with a hole Meshing Technique Case study # 3 - Plate with a hole BCs & Loading 24/71 Case study # 3 - Plate with a hole KT assessment Case study # 3 - Plate with a hole KT assessment KT is defined as KT = σmax σ0 . . . . . . . . . . . . . . . . . . . . . . . . . (28) Nota : when the problem is easy KT definition is straightforward ; but for complex structure σ0 is usually particularly touchy to recover a universal definition. A reference textbook for KT definition is the Peterson [1]. 25/71 Case study # 3 - Plate with a hole Closed form solution Case study # 3 - Plate with a hole Closed form solution For a circular hole the mathematical theory of elasticity (refer e.g. to [2]) leads to 26/71 σxx (x = l 2 ( , y) = 1+ 1 R2 2 y2 + 3 R4 2 y4 ) σ0 . . . . . . . . . . . . . . . . (29) Case study # 3 - Plate with a hole Nastran linear static run Case study # 3 - Plate with a hole Nastran linear static run Nastran .dat is generated from Analysis menu Then run the analysis with Nastran $ nastran case study 3.dat news=n old=n scr=y User obtains as output to Nastran run ◦ case study 3.log : Control File ◦ case study 3.f04 : Execution Summary Table ◦ case study 3.f06 : ASCII Results file ◦ case study 3.op2 : Binary Results file 27/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Students have to plot the reacted force and the reacted moment in Patran after the import of the .op2. 28/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - u [mm] 29/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - σI [MPa] 30/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - σI [MPa] 31/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - σI [MPa] 32/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - freebody diagram form 33/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - elements and nodes for freebody diagram 34/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - freebody diagram 35/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - freebody diagram 36/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - σyy [MPa] vs. y [mm] The error to closed form solution of Nastran assessed from freebody results can be assessed through color spectrum : ◦ < 4.00 %≤◦ < 5.00 %≤◦ < 7.00 %≤◦< 8.00 %. 37/71 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 Case study # 3 - Plate with a hole Results from Nastran linear static run from .op2 - σyy [MPa] vs. y [mm] From freebody it is assessed KT = = = 2F . a × t × σ0 . N ×F π × R × t × σ0 2.99− . . . . . . . . . . . . . . . . . . . . . . . . (30) . . . . . . . . . . . . . . . . . . . . (31) . . . . . . . . . . . . . . . . . . . . (32) From GPSTRESS (grid point stress) in .f06 one derives 38/71 KT = = σ37 . . . . . . . . . . . . . . . . . . . . . . (33) 2.86 ± 3.45%− . . . . . . . . . . . . . . . . . . . . . (34) σ0 . . Case study # 3 - Plate with a hole Conclusion & Outlook Case study # 3 - Plate with a hole Conclusion & Outlook 39/71 ◦ One does not match the closed form solution because the studied plate is not an infinite continuum ◦ Error has been assessed after computation of a load F derived from a freebody and a surface computed from plate thickness × sum of mid adjacent quads heigth for comparison with a closed from solution ◦ Error in regard of closed form solution from theory of elasticty is under 3.00% but is highly mesh dependent ; stress results have been assessed on a single path at x = 0 in the range y ∈ [ D , w ] 2 2 ◦ A more generalized methodology to assess the convergence of a mesh under Nastran is to use the GPSTRESS (grid point stress : the extra/interpolation of σ recovery at Gauss points to nodes) output and the associated discontinuities the GPSDCON Case study # 3 - Plate with a hole Conclusion & Outlook Case study # 3 - Plate with a hole Conclusion & Outlook , 0) one For the mesh used for Case study # 3 illustration purpose at Node 37 whose coordinates are (0, D 2 has S T R E S S E S A T G R I D P O I N T S - S U R F A C E 10 SURFACE X-AXIS X NORMAL(Z-AXIS) Z REFERENCE COORDINATE SYSTEM FOR SURFACE DEFINITION CI GRID ELEMENT STRESSES IN SURFACE SYSTEM PRINCIPAL STRESSES MAX ID ID FIBER NORMAL-X NORMAL-Y SHEAR-XY ANGLE MAJOR MINOR SHEAR VON MISES 37 0 MID 2.860E+02 1.036E+01 -4.517E-03 -0.0009 2.860E+02 1.036E+01 1.378E+02 2.809E+02 and G R I D P O I N T S T R E S S D I S C O N T I N U I T I E S - S U R F A C E 10 SURFACE X-AXIS X NORMAL(Z-AXIS) Z REFERENCE COORDINATE SYSTEM FOR SURFACE DEFINITION CI GRID NORMAL STRESS DISCONTINUITY IN SURFACE SYSTEM PRINCIPAL STRESS DISCONTINUITY ERROR ID FIBER NORMAL-X NORMAL-Y SHEAR-XY MAJOR MINOR MAX SHEAR VON MISES EST. 37 MID 1.413E-03 7.667E-04 5.977E+00 1.831E-01 1.831E-01 1.831E-01 2.696E-01 3.451E+00 Error formula are quoted in Nastran Linear Static Guide [3] ; e.g. for a tensor component δg = 1 Ne 2 1 X 2 (σi − σg ) Ne . . . . . . . . . . . . i=1 then one derives a mean value depending upon tensor components number. 40/71 . . . . . . . . (35) Case study # 4 - Buckling Analysis Theoretical Apart´ e Case study # 4 - Buckling Analysis Theoretical Apart´e The buckling analysis is a bifurcation analysis. Start point is the functional W that describes the elastic energy of the solid with a parameter λ associated to the load. The eigenvalues stem from setting equal to 0 the second derivative of the functional W . 41/71 Case study # 4 - Buckling Analysis Definition Case study # 4 - Buckling Analysis Definition The framework is linear elasticity. The plate is t = 3 mm thick. A compressive load σ0 = −100 MPa is applied at one side. The beam is clamped at one side. The plate is made of aluminium E = 70 GPa and ν = 0.33. Aim of Case study # 4 : Students have to find the buckling modes associated to the compressive load and assess the critical load below which the structure remains stable. 42/71 Case study # 4 - Buckling Analysis Mesh Case study # 4 - Buckling Analysis Mesh The mesh of case study # 3 is suitable for the buckling analysis. The mesh is to be built with Nastran CQUAD4 elements. 43/71 Case study # 4 - Buckling Analysis Nastran EIGRL Card Case study # 4 - Buckling Analysis Nastran EIGRL Card Nastran SOL 105 is to be used.The Nastran EIGRL Card has to be called in Case Control Section after the linear SUBCASE associated to the compressive load by a Nastran METHOD Card. 44/71 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15 16 $ Case Control Section SUBCASE 1001 SUBTITLE = COMPRESSION LABEL = COMPRESSION LOAD = 2 $ SUBCASE 1002 SUBTITLE = COMPRESSION LABEL = COMPRESSION METHOD = 1 STATSUB ( BUCKLING )=1001 $ BEGIN BULK $ Bulk Section EIGRL 1 ... 10 Case study # 4 - Buckling Analysis Nastran buckling run Case study # 4 - Buckling Analysis Nastran buckling run Nastran .dat is generated from Analysis menu Then run the analysis with Nastran $ nastran case study 4.dat news=n old=n scr=y User obtains as output to Nastran run ◦ case study 4.log : Control File ◦ case study 4.f04 : Execution Summary Table ◦ case study 4.f06 : ASCII Results file ◦ case study 4.op2 : Binary Results file 45/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .f06 Case study # 3 - Plate with a hole Results from Nastran buckling run from .f06 Students have to find the eigenvalues associated to the computed modes in the .f06. 46/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .f06 Case study # 3 - Plate with a hole Results from Nastran buckling run from .f06 Students have to find the eigenvalues associated to the computed modes in the .f06. MODE NO. 1 2 3 4 5 6 7 8 9 10 46/71 EXTRACTION ORDER 1 2 3 4 5 6 7 8 9 10 EIGENVALUE 2.922786E+00 8.688133E+00 1.231678E+01 1.690665E+01 1.714466E+01 2.491786E+01 2.727503E+01 3.472403E+01 3.905111E+01 4.561754E+01 R E A L E I G E N V A L U E S RADIANS CYCLES 1.709616E+00 2.947564E+00 3.509528E+00 4.111770E+00 4.140611E+00 4.991779E+00 5.222550E+00 5.892710E+00 6.249089E+00 6.754076E+00 2.720938E-01 4.691193E-01 5.585586E-01 6.544085E-01 6.589987E-01 7.944663E-01 8.311947E-01 9.378539E-01 9.945734E-01 1.074944E+00 GENERALIZED MASS 1.147029E+03 2.579305E+03 4.383950E+02 3.473366E+03 8.870814E+02 1.714101E+03 6.138878E+03 2.523782E+03 8.644048E+03 3.599225E+03 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Students have to plot the buckling mode in Patran after the import of the .op2. 47/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 48/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 49/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 50/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 51/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 52/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 53/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 54/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 55/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 56/71 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 Case study # 4 - Buckling Analysis Results from Nastran buckling run from .op2 57/71 Case study # 4 - Buckling Analysis Conclusion & Outlook Case study # 4 - Buckling Conclusion & Outlook 58/71 ◦ Eigenmodes are particularly dependent upon boundary conditions applied at the loaded plate end : eigenvalues are different if rotations are clamped or not Case study # 5 - Guyan Static Reduction Theoretical Apart´ e Case study # 5 - Guyan Static Reduction Theoretical Apart´e The framework is linear elasticity. One solves K f f uf = Ff . . . . . . . . . . . . . . . . . . . . . . . . . (36) with o-set interior degrees of freedom and a-set exterior degrees of freedom one can split the equation (36) Koo K T oa K oa K aa uo ua = Fo Fa . . . . . . . . . . . . . . . . (37) . . . . . . . . . . . . . . . . (38) . . . . . . . . . . . . . . . . (39) whose first line of (37) means Koo uo + K oa ua = Fo −1 −1 ⇔ Koo (Koo uo + K oa ua ) = Koo Fo −1 −1 ⇔ uo = Koo Fo − Koo K oa ua −1 −1 ⇔ uo = Koo Fo − Koo K oa ua {z } | {z } | u0 o −Goa or 0 uo = uo + Goa ua . . . . . . . . with Goa boundary transformation and u0 o fixed boundary displacement. 59/71 Case study # 5 - Guyan Static Reduction Theoretical Apart´ e Case study # 5 - Guyan Static Reduction Theoretical Apart´e Thus the second line of (37) means with the definition (39) of uo K T oa uo + a K aa ua = F + K aa ua = Fa ⇔ K T oa u0 o + Goa ua . . . . . . . . . . . . . . T T 0 ⇔ K oa Goa +K aa ua = Fa − K oa uo | {z } | {z } Kaa Fa with Kaa boundary stiffness and Fa boundary load. Typically with a classical Nastran run one has Kaa ≡ KAAX and Fa ≡ PAX. Note that (40) defines the boundary displacement field associated to the ASET. 60/71 (40) Case study # 5 - Guyan Static Reduction Definition Case study # 5 - Guyan Static Reduction Definition The framework is linear elasticity. The residual structure is selected as the square structure 30 × 30 mm2 centered on the circular hole. Aim of Case study # 5 : Students have to realize a Guyan Static Reduction of structure associated to Case study # 2 and run SOL 101 the residual structure. The fill-in of KAAX is to be assessed by the students and compare to a classical finite elements matrix. 61/71 Case study # 5 - Guyan Static Reduction Nastran ASET Card Case study # 5 - Guyan Static Reduction Nastran ASET Card Nastran offers a card called ASET to define the degrees of freedom to be omitted in the reduction process. 62/71 Case study # 5 - Guyan Static Reduction Nastran EXTOUT Parameter Case study # 5 - Guyan Static Reduction Nastran EXTOUT Parameter In order to realize a Guyan Static Reduction one has to use EXTOUT parameter. 1 2 $ Case Control Parameters PARAM EXTOUT DMIGPCH Set equal to DMIGPCH the EXTOUT parameter means a .pch file creation for output of KAAX and PAX. 63/71 Case study # 5 - Guyan Static Reduction Nastran linear static run for reduction Case study # 5 - Guyan Static Reduction Nastran linear static run for reduction Nastran .dat is generated from Analysis menu Then run the analysis with Nastran $ nastran case study 5.dat news=n old=n scr=y User obtains as output to Nastran run ◦ case study 5.log : Control File ◦ case study 5.f04 : Execution Summary Table ◦ case study 5.f06 : ASCII Results file ◦ case study 5.op2 : Binary Results file ◦ case study 5.pch : PUNCH file 64/71 Case study # 5 - Guyan Static Reduction Results from Nastran linear static run from .pch Case study # 5 - Guyan Static Reduction Results from Nastran linear static run from .pch Students have to check .pch file contains a stiffness matrix and an interface load vector. The former is called KAAX and the latter PAX. 65/71 Case study # 5 - Guyan Static Reduction Reading external element Case study # 5 - Guyan Static Reduction Reading external element In order to read the result of a Guyan Static Reduction one has to use K2GG and P2G commands. 66/71 1 2 3 4 5 $ Case Control Section $ Command for reading boundary stiffness K2GG = ... $ Command for reading interface load P2G = ... Case study # 5 - Guyan Static Reduction Nastran linear static run for residual structure Case study # 5 - Guyan Static Reduction Nastran linear static run for residual structure Nastran .dat is generated from Analysis menu for the residual structure. Note the Selected Group Menu Form of the Analysis menu is particularly suitable to export a part of a previous model (here the central square of the plate). 67/71 Case study # 5 - Guyan Static Reduction Nastran linear static run for residual structure Case study # 5 - Guyan Static Reduction Nastran linear static run for residual structure The Nastran run case study 5 residual.dat has to call the result of the SOL 101 reduction run case study 5.dat. 1 2 3 4 5 6 $ Case Control Section INCLUDE ’ case_study_5 . pch ’ $ Command for reading boundary stiffness K2GG = ... $ Command for reading interface load P2G = ... Then run the analysis with Nastran $ nastran case study 5 residual.dat news=n old=n scr=y User obtains as output to Nastran run ◦ case study 5 residual.log : Control File ◦ case study 5 residual.f04 : Execution Summary Table ◦ case study 5 residual.f06 : ASCII Results file ◦ case study 5 residual.op2 : Binary Results file 68/71 Case study # 5 - Guyan Static Reduction Results from Nastran linear static run from .op2 Case study # 5 - Guyan Static Reduction Results from Nastran linear static run from .op2 Students have to check with Patran that for the residual structure the results from the run of case study #3 and case study #5 are in accordance. 69/71 Case study # 5 - Guyan Static Reduction Conclusion & Outlook Case study # 5 - Guyan Static Reduction Conclusion & Outlook 70/71 ◦ The analysis performed is particularly used in dynamic analyis to reduce the degrees of freedom of a model [4]. ◦ The Guyan Static Reduction was particularly used by the past to allow concurrent work between engineering teams. ◦ One can check that on the opposite of an assembly global finite elements stiffness matrix KAAX is not sparse. ◦ One can use a DMIGOP2 output for the matrix KAAX and the load vector PAX instead of the Ascii DMIGPCH output ; reading the binary format in Nastran to run the reduced structure is a little bit more touchy. Main outcome is the binary file size is significantly smaller than the Ascii one. References References [1] R.E. Peterson. Stress concentration factors: charts and relations useful in making strength calculations for machine parts and structural elements. Wiley-Interscience publication. Wiley, 1974. [2] B.F. De Veubeke. A Course in Elasticity. Number vol. 29 in Applied Mathematical Sciences. Springer-Verlag, 1979. [3] MSC Software. Linear Static Analysis User’s Guide: MSC Nastran 2012. MacNeal-Schwendler Corporation, 2011. [4] J.F. Imbert. Analyse des structures par ´ el´ ements finis. C´ epadu` es, 1991. 71/71
© Copyright 2024