Drinking Straw Estimated Time for Completion: ~45min Experience Level: Lower MSC.Patran 2005 r2 MSC.Marc 2005 r2

2 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.

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

4 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 u y =θ x = θ z =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.

5 Summary of Model Straw Dimensions: Diameter=0.016m, Total Length=0.083m, Thickness=0.0001m Material properties: Polystyrene Young’s Modulus =1.0x10 8 Pa, Poisson’s ratio=0.3, Yield strength= 1.0x10 6 Pa 0.083m 0.016m 0.023m t=0.0001m

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

7 Expected Results Deformed Shape

8 Create Database and Import a Geometry File a.Click File menu / Select New b.In File Name enter bendablestraw.db c.Click OK d.Select Analysis Code to be MSC. Marc e.Click OK f.Click File menu / Select Import g.Select Object to be Model h.Select Source to be Neutral i.Select the model file, straw_geom.out j.Click Apply. k.Click Yes l.Click Yes def a bc gh i jabcdefghijklmnopqrstuvwxyz kl You will see elements and nodes in the current viewport.

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

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

11 Create Boundary Conditions a.Click Loads/BCs icon b.Select Action to be Create c.Select Object to be Displacement d.Select Type to be Nodal e.In New Set Name, enter fixed f.Click Input Data g.In Translations, enter h.In Rotations, enter i.Click OK j.Click Select Application Region k.Select Geometry Filter to be FEM l.In Select Nodes, enter Node 11502:12432:31 or select the nodes on the right end of the model m.Click Add n.Click OK o.Click Apply Create the Boundary Conditions for the fixed end. a b c d ef g ijk lm no h l

12 Create Boundary Conditions a.Click Loads/BCs icon b.Select Action to be Create c.Select Object to be Displacement d.Select Type to be Nodal e.In New Set Name, enter disp_x f.Click Input Data g.In Translations, enter h.In Rotations, enter i.Click OK j.Click Select Application Region k.Select Geometry Filter to be FEM l.In Select Nodes, enter Node or select the centered node on the left end of the model m.Click Add n.Click OK o.Click Apply Create the Boundary Conditions for the moving end. b c d ef g ijk lm no h la

13 Create Boundary Conditions a.Click Loads/BCs icon b.Select Action to be Create c.Select Object to be Displacement d.Select Type to be Nodal e.In New Set Name, enter sym f.Click Input Data g.In Translations, enter h.In Rotations, enter i.Click OK j.Click Select Application Region k.Select Geometry Filter to be FEM l.In Select Nodes, select the node on the symmetric boundary of the model m.Click Add n.Click OK o.Click Apply Create the Boundary Conditions for the symmetric boundary. b c d efgijk lm no h la

14 Create the Material Properties a.Click Materials icon b.Select Action to be Create c.Select Object to be Isotropic d.Select Method to be Manual Input e.In Material Name, enter polystyrene f.Click Input Properties g.Select Constitutive Model to be Elastic h.In Elastic Modulus, enter 1e8 i.In Possion Ratio, enter 0.3 j.Click OK k.Click Apply l.Click Input Properties again m.Select Constitutive Model to be Plastic n.Select Type to be Perfectly Plastic o.In Yield Stress, enter 1e6 p.Click OK q.Click Apply a bc d ef g h i jklmnopq

15 Create the Element Properties a.Click Properties icon b.Select Action to be Create c.Select Object to be 2D d.Select Type to be Thin Shell e.In Property Set Name, enter prop1 f.Select Options to be Homogeneous g.Click Input Properties h.Click Mat Prop Name icon i.Select polystyrene j.In [Thickness], enter 1e-4 k.Click OK l.In Application Region, enter Elm 1:10650 or select all elements m.Click Add n.Click Apply aab cdefgi j klmn h l

16 Run Analysis a.Click Analysis icon b.Select Action to be Analyze c.Select Object to be Entire Model d.Select Method to be Full Run e.In Job Name, enter straw_ext f.Click Load Step Creation g.Click Solution Parameters h.Select Linearity to be NonLinear i.Select Nonlinear Geometry Effects to be Large Displacement(Updated Lagr.)/Small Strains j.Click Load Increment Parameters k.Select Increment Type to be Adaptive l.In [Trial Time Step Size:], enter 0.01 m.Click OK n.Click Iteration Parameters o.In Max # of Iterations per Increment, enter 100 p.Click OK q.Click OK r.Click Apply s.Click Cancel t.Click Apply Analysis Options for the first load step ab c d e fgijklm n opqrsth Because of the structural unstability of the example, the results and the analysis time are dependent on the analysis options.

17 Read Results Read Results File a.In the Marc Job Monitoring window, if the Exit Number is 3004, the problem has been solved successfully. b.Click Cancel c.Select Action to be Read Results d.Select Object to be Result Entities e.Select Method to be Attach f.Click Select Results File g.Select straw_ext.t16 h.Click OK i.Click Apply abcdefghi

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

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

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

21 Displacement Results Results abcdefgijklmnopqrstuvwxyzh At time=0.0 At time=1.0 At time=0.2 At time=0.4 At time=0.6 At time=0.8

22 Results von-Mises at time=0.38 von-Mises at time=0.15 Max=1.87E6 MPa Max=1.62E6 MPa

23 Results Load vs. Displacement Strain Energy vs. Displacement (time=displacement factor) Max=0.46N

24 Animation

25 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.