Drinking Straw MSC Patran 2005 r 2 MSC

• Slides: 25

Drinking Straw MSC. Patran 2005 r 2 MSC. Marc 2005 r 2 Estimated Time for Completion: ~45 min Experience Level: Lower

Topics Covered • Topics covered in Modeling • Importing Geometry file with FEA data. • Neutral format (. out) • Creating controlling node and MPC • Multi-point Constraint element are created to connect the controlling node and the structure. • Creating Elastic-perfectly plastic material. • The material non-linearity is approximated by a constant. • Topic covered in Analysis • Applying Large Displacement/Small Strains Analysis. • Topics covered in Review • Creating XY plots and animations. 2

Problem Description • In this example, a bendable straw is fully stretched by applying displacement conditions at both ends. Plastic deformation occurs during the increments. Fmax=? 3

Problem Description • In this example problem, we apply Symmetric boundary conditions at the center of the pipe to reduce the number of elements and the analysis time. The following condition is applied at the boundary • uy=θx= θz=0 on the symmetric boundary. • The geometry and the Boundary conditions are axisymmetric. However there can be unsymmetric results due to the unstability. Instead fully axisymmetric conditions, only symmetric boundary conditions are applied to the half of the geometry. 4

Summary of Model • Straw • Dimensions: • Diameter=0. 016 m, • Total Length=0. 083 m, • Thickness=0. 0001 m • Material properties: Polystyrene • Young’s Modulus =1. 0 x 108 Pa, • Poisson’s ratio=0. 3, • Yield strength= 1. 0 x 106 Pa 0. 023 m t=0. 0001 m 0. 016 m 0. 083 m 5

Goal • We will determine the maximum stress in the structure. • We will determine the minimum load to extend the drinking straw. 6

Expected Results • Deformed Shape 7

Create Database and Import a Geometry File a f g h i c b j a. b. c. d. e. f. g. h. i. j. k. l. Click File menu / Select New In File Name enter bendablestraw. db Click OK Select Analysis Code to be MSC. Marc Click OK Click File menu / Select Import Select Object to be Model Select Source to be Neutral Select the model file, straw_geom. out Click Apply. Click Yes d k e l You will see elements and nodes in the current viewport. a b c d e f g h i j k l m n o p q r s t u 8 v w x y z

Create a Node Create a node to control the upper rigid surface a b c a. b. c. d. e. f. g. h. Click Element icon Select Action to be Create Select Object to be Node Select Method to be Edit In Node ID List, enter 15000 Uncheck Auto Execute In Node Location List, enter [0, 0, 0] Click Apply d This is the node created. e f g h You can visualize nodes by toggling this icon. 9

Create a MPC Create Multi-Point Constraints on the left end of the model. a. b. c. d. e. f. g. h. i. j. k. l. Select Action to be Create Select Object to be MPC Select Method to be Rigid(Fixed) Click Define Terms Select Create Dependent Uncheck Auto Execute In Node List, enter Node 2048: 2978: 31, or select all nodes on x=0 plane except Node 15000. Click Apply Select Create Independent In Node List, enter Node 15000, or select the node made in the previous slide. Click Apply a b c d l e i f g j k h Make sure that you do not select the centered node in the Dependent Terms m n o p q r s t u 10 v w x y z

Create Boundary Conditions Create the Boundary Conditions for the fixed end. a b c a. b. c. d. e. f. g. h. i. j. k. l. m. n. o. Click Loads/BCs icon Select Action to be Create Select Object to be Displacement Select Type to be Nodal In New Set Name, enter fixed Click Input Data In Translations, enter <0, 0, 0> In Rotations, enter <0, 0, 0> Click OK Click Select Application Region Select Geometry Filter to be FEM In Select Nodes, enter Node 11502: 12432: 31 or select the nodes on the right end of the model Click Add Click OK Click Apply d k g h l m n i e f j o l 11

Create Boundary Conditions Create the Boundary Conditions for the moving end. a b c a. b. c. d. e. f. g. h. i. j. k. l. m. n. o. Click Loads/BCs icon Select Action to be Create Select Object to be Displacement Select Type to be Nodal In New Set Name, enter disp_x Click Input Data In Translations, enter <-0. 03, 0, 0> In Rotations, enter <0, 0, 0> Click OK Click Select Application Region Select Geometry Filter to be FEM In Select Nodes, enter Node 15000 or select the centered node on the left end of the model Click Add Click OK Click Apply k d g h l m n i e f j o l 12

Create Boundary Conditions Create the Boundary Conditions for the symmetric boundary. a b c a. b. c. d. e. f. g. h. i. j. k. l. m. n. o. Click Loads/BCs icon Select Action to be Create Select Object to be Displacement Select Type to be Nodal In New Set Name, enter sym Click Input Data In Translations, enter < , , 0> In Rotations, enter <0, 0, > Click OK Click Select Application Region Select Geometry Filter to be FEM In Select Nodes, select the node on the symmetric boundary of the model Click Add Click OK Click Apply d k g h l m i n e f j o l 13

Create the Material Properties a a. b. c. d. e. f. g. h. i. j. k. l. m. n. o. p. q. Click Materials icon Select Action to be Create Select Object to be Isotropic Select Method to be Manual Input In Material Name, enter polystyrene Click Input Properties Select Constitutive Model to be Elastic In Elastic Modulus, enter 1 e 8 In Possion Ratio, enter 0. 3 Click OK Click Apply Click Input Properties again Select Constitutive Model to be Plastic Select Type to be Perfectly Plastic In Yield Stress, enter 1 e 6 Click OK Click Apply b g c d h i m e n j f o l k q p 14

Create the Element Properties a a. b. c. d. e. f. Click Properties icon Select Action to be Create Select Object to be 2 D Select Type to be Thin Shell In Property Set Name, enter prop 1 Select Options to be Homogeneous Click Input Properties Click Mat Prop Name icon Select polystyrene In [Thickness], enter 1 e-4 Click OK In Application Region, enter Elm 1: 10650 or select all elements Click Add Click Apply g. h. i. j. k. l. m. n. b c h d j i e f g k l m n l a 15

Run Analysis Options for the first load step a. b. c. d. e. f. g. h. i. j. k. l. m. n. o. p. q. r. s. t. a b Click Analysis icon c Select Action to be Analyze d Select Object to be Entire Model Select Method to be Full Run In Job Name, enter straw_ext Click Load Step Creation Click Solution Parameters Select Linearity to be Non. Linear Select Nonlinear Geometry Effects to be Large e Displacement(Updated Lagr. )/Small Strains Click Load Increment Parameters Select Increment Type to be Adaptive f In [Trial Time Step Size: ], enter 0. 01 t Click OK Click Iteration Parameters In Max # of Iterations per Increment, enter 100 Click OK Because of the structural unstability of Click OK the example, the results and the analysis Click Apply time are dependent on the analysis Click Cancel options. Click Apply h i j g r n q s k l o m p 16

Read Results File a. b. c. d. e. f. g. h. i. c In the Marc Job Monitoring window, if the Exit Number is 3004, the problem has been solved successfully. Click Cancel Select Action to be Read Results Select Object to be Result Entities Select Method to be Attach Click Select Results File Select straw_ext. t 16 Click OK Click Apply d e f i a g h b 17

Review and Display Results Plot the Displacement Result a a. b. c. d. e. f. g. h. i. j. k. l. m. n. Click Results icon Select Action to be Create Select Object to be Quick Plot In Select Results Cases, select the last result (Time=1. 00000) Click Fringe Attributes icon Click Spectrum, and select the one you want. Select Style to be Continuous Select Shading to be Shaded Click Deform Attributes icon Uncheck Show Undeformed Click Select Results icon In Select Fringe Result, select Displacement, Translation In Select Deformation Result, select Displacement, Translation Click Apply b c k i e f g d h l j m n 18

Review and Display Results Plot the Nodal Reaction Force at the Controlling Node (Load vs. Displacement Curve) a. b. c. d. e. f. g. h. i. j. k. l. m. n. o. p. q. r. s. Select Action to be Create Select Object to be Graph Select Method to be Y vs X In Select Result Case(s), select all cases Click Target Entity icon In Select Nodes, enter Node 1 or select the controlling node in the viewprot Click Select Results icon Click Display Attributes icon In XY Window Name, enter 5 or title number you want Click Select Results icon Select Y to be Result In Select Y Result, select Force, Nodal Reaction Select Quantity to be X Component Select X to be Result Click Select X Result In Select X Result, click Displacement, Translation Select Quantity to be X Component Click OK Click Apply a b c h g e j d f k l m p i n o s q r 19

Review and Display Results Plot the Elastic Strain Energy a. b. c. d. e. f. g. h. i. j. k. l. a b c Select Action to be Create Select Object to be Graph Select Method to be Y vs X In Select Result Case(s), select all cases Click Display Attributes icon In XY Window Name, enter 3 or title number you want Click Select Results icon Select Y to be Global Variable In Variable, select Elastic Strain Energy Select X to be Global Variable Select Variable to be Time Click Apply e g d h i j f k l 20

Results • Displacement Results At time=0. 0 At time=0. 2 At time=0. 4 At time=0. 6 At time=0. 8 At time=1. 0 a b c d e f g h i j k l m n o p q r s t u 21 v w x y z

Results • von-Mises at time=0. 15 Max=1. 62 E 6 MPa • von-Mises at time=0. 38 Max=1. 87 E 6 MPa 22

Results • Load vs. Displacement Max=0. 46 N • Strain Energy vs. Displacement (time=displacement factor) 23

Animation 24

Further Analysis (Optional) • Problem modification • Bending Straw: Rotate the one end of the straw 90°. Is the MPC still applicable? • Modeling • Modify the geometry to have axisymmetric conditions. Solve it and find the difference from the current results. 25