MAR120, Workshop 1, December 2001 WORKSHOP 01 LINEAR AND NONLINEAR ANALYSIS OF A CANTILEVER BEAM

WS1-1 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001

WS1-2 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Problem Description  In this exercise, a cantilever beam is subjected to a static load. The beam is initially analyzed using small deformation theory. However, after reviewing the results, it becomes apparent that small deformation theory is not appropriate for this problem. Subsequently, a large deformation analysis is performed and its results are compared to the small deformation analysis. Section A-A b a (Data in next page)

WS1-3 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Length, L100.0 in2.54 m a1.0 in25.4 mm b2.0 in50.8 mm Young’s Modulus30.0 x 10 6 lb/in GPa Poisson’s Ratio0.3 P6000 lb27200 N Section A-A b a

WS1-4 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Problem Description (cont.)  The model is made using eight, 2D plane stress, incompatible mode elements. The elements are uniformly spaced along the length of the beam (i.e. a mesh eight elements wide and one element deep). The incompatible mode type element is designed specifically for in-plane bending and is well suited for this problem Objectives:  Small vs. large displacement analysis.  Linear elastic theory Required  No Supporting file is required

WS1-5 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Suggested Exercise Steps:  Create simple Cantilever model as illustrated  Use a simple, elastic steel material  Run a linear analysis with default setup  Run a nonlinear analysis with default setup.  Compare results.

WS1-6 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 1. Exercise Procedure a MSC.Marc  d f e Open a new database. Name it Tip_load.db a.File / New. b.Enter Tip_Load as the File name. c.Click OK. d.Wait a few seconds until the New Model Preference opens e.Select MSC.Marc as the Analysis Code. f.Click OK. Tip_load.db Tip_Load b c

WS1-7 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 2. Geometry: Create / Surface / XYZ b c The surface will be created when you apply and should look like the one here. Open a new database. Name it Tip_load.db a.Geometry: Create / Surface / XYZ. b.Enter as the Vector Coordinates List. c.Click –Apply-. a

WS1-8 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 After second -Apply- the mesh seeds will look like these: After first –Apply- the mesh seeds will look like these: i Step 3. Finite Elements: Create / Mesh Seed / Uniform d e 1 Surface 1.1 g j h Create the finite element mesh seeds. a.Elements: Create / Mesh Seed / Uniform. b.Enter 8 as the Number. c.Click on Curve List panel. d.Select Edge icon e.Pick bottom edge of surface f.Click –Apply- g.Enter 1 as the Number. h.Click on Curve List box i.Pick left edge of surface j.Click –Apply-. 8 Surface 1.4 f a b c

WS1-9 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 4. Finite Elements: Create / Mesh / Surface e The mesh will be created when you apply and should look like the one here. Create the finite element mesh. a.Create / Mesh / Surface. b.Select Quad 4. c.Click on Surface List panel. d.Select Surface or Solid Face Icon. e.Select Surface in view port. f.Uncheck Automatic Calculation. g.Enter 0.1 as the Value. h.Click –Apply-. Surface 1 h f c b a d g

WS1-10 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December e Step 5. Materials: Create / Isotropic / Manual Input d e g f Make sure that after you apply, that steel appears in the existing materials box Create the material property:steel a.Materials: Create / Isotropic / Manual Input. b.Enter steel as the Material Name. c.Click on Input Properties d.Enter 30e6 as the Elastic Modulus. e.Enter 0.30 as the Poisson Ratio. f.Enter as the Density. g.Click OK. h.Click –Apply-. steel a c h b

WS1-11 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 The test specimen is free to contract in the direction normal to its plane,thus developing normal strains; the stresses normal to the plane are nil. Why do we define this property as “Plane Stress” rather than “Plane Strain” ? Step 6. Properties: Create / 2D / 2D Solid beam a b c d e “Input Properties” form is on the next page Now create the properties of the beam a.Properties: Create / 2D / 2D Solid. b.Enter beam as the Property Set Name. c.Select Plane Stress. d.Select Reduced Integration. e.Click on Input Properties.

WS1-12 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 j beam i l m k f.Click on Material Name and Select Steel in Material Property Sets. g.Enter 1.0 as the Thickness. h.Click OK. i.Click on Select Members. j.Select Surface or Face icon. k.Select the Surface. l.Click Add. m.Click –Apply-. steel 1.0 steel f h g

WS1-13 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 7. Loads/BCs: Create / Displacement / Nodal d e Fix the left side by creating a displacement boundary. a.Loads/BCs: Create / Displacement / Nodal. b.Enter Fixed as the New Set Name. c.Click on Input Data. d.Enter for the Translations. e.Click OK. Fixed a b c

WS1-14 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 i j After you apply Fixed should appear in the “Existing Sets” box. f.Click on Select Application Region. g.Select Geometry as the Geometry Filter. h.Click in Select Geometry Entities panel. i.Select Edge icon j.Select Left edge of surface k.Click Add. l.Click OK m.Click –Apply-. l h g k Fixed m f

WS1-15 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 8. Loads/BCs: Create / Force / Nodal d e Create the load to be placed on the right tip. a.Create / Force / Nodal b.Enter Tip_Load as the New Set Name. c.Click on Input Data. d.Enter for the Force. e.Click OK. f.Click on Select Application Region. Tip_Load a b c f

WS1-16 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Tip_Load i n After you apply Tip_Load should appear in Existing Sets. k l h g g.Select FEM as the Geometry Filter. h.Click in Select Nodes Panel. i.Select Node icon. j.Select Nodes on Right Edge by clicking and dragging the mouse. k.Click Add. l.Click OK. m.Click –Apply-. m j

WS1-17 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 9. Analysis: Analyze / Entire Model / Full Run Linear_job1 a b c e d Running a linear analysis a.Analysis: Analyze / Entire Model / Full Run b.Enter Linear_job1 as the Job Name. c.Click on Translation Parameters. d.Check Assumed Strain. e.Click OK.

WS1-18 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 f.Click on Load Step Creation. g.Enter My Linear as the Job Step Name. h.Click on Solution Parameters. i.Select Linear as the Linearity. j.Click OK. k.Click Apply (the linear job step will be added to “Available Job Steps” box.) l.Click Cancel. Linear_job1 f My Linear i k l g Linear  i j h

WS1-19 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 My Linear Default Static Step Default Static Step My Linear My Linear o After you Select “Default Static Step” under Selected Job Steps It should disappear from Selected Job Steps. The final form should look like the one to the left. After you select “My Linear” in the “Existing Job Steps” box, it should appear in the “Selected Job Steps” box. After you apply “Linear_Job1” should appear in the “Available Jobs” box. m.Click on Load Step Selection. n.Select My Linear from the Existing Job Steps. o.Select Default Static Step from the Selected Job Steps. p.Click OK. q.Click Apply thus launching the MSC.Marc analysis. n Linear_job1 q m p

WS1-20 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 10. Analysis:Monitor / Job Linear_job1 a b c You can also view the log and output files by clicking on the other “View” buttons. Monitor the linear job. a.Monitor / Job. b.Select Linear_job1 as the Job Name. c.Click on View Status file. You can view the status of the analysis and check for Exit Code (3004 means Normal Termination).

WS1-21 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 11. Analysis: Read Results / Result Entities / Attach Linear_job1.t16 d c Linear_job1 a b e When the analysis is done read the results using PATRAN a.Read Results / Result Entities / Attach. b.Click on Select Results File. c.Select Linear_Job1.t16. d.Click OK. e.Click Apply. This action will actually make the results available for post-processing.

WS1-22 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 12. Results: Create / Quick Plot f g c d e b a Quick Plot is on next page When you select True Scale, the default Scale Factor is 1.0. (We want to see the “actual” deformed shape) Post-Processing linear job using Patran a.Results: Create / Quick Plot. b.Select Default A1: Incr =1, Time= from the Select Results Cases c.Select Displacement, Translation from the Select Fringe Result. d.Select Displacement, Translation from the Select Deformation Result. e.Click on the Deform Attributes Icon. f.Select True Scale. g.Click Apply.

WS1-23 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 After you apply your graph should look like this The maximum Y deflection of the beam can be taken directly off of the displayed spectrum/range. The largest value should correspond to a magnitude of 99.6, which is in fair agreement with our hand calculation of 100. You may still improve this by remeshing using two elements over the high of the section instead of just one as you have it now. (You will be asked to do this after your have ran nonlinear analysis of present mesh.) Linear beam theory assumes plane section remain plane and the deflection is small relative to length of the beam. As can be clearly seen by this analysis, the deflection is very large and this analysis is in violation of the underlying assumptions used for linear beam theory. These results match the linear hand calculations and also show that the small deformation assumption is not valid and therefore, a non-linear, large deformation analysis needs to be performed. In large deformation analysis, the bending and axial stiffness are coupled. Thus, as the cantilever beam deflects, a portion of the load P puts the beam in tension which tends to stiffen the beam in bending (i.e. “geometric stiffness”). Thus, one would expect to see a much smaller deformation in the large deformation analysis as compared to the small deformation analysis. To set up a large deformation analysis, one needs to change the analysis set-up and re-submit the job to MSC/ MARC Linear beam theory predicts the maximum beam deflection in the Y- direction and stress to be:

WS1-24 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 13: Analysis: Analyze / Entire Model / Method Nonlinear_job1 Linear_job1 a b c d e f Run a nonlinear analysis a.Analysis: Analyze / Entire Model / Full run. b.Enter Nonlinear_job1 as the Job Name. c.Click on Translation Parameters. d.Click on Solver Options. e.Check Non-Positive Definite (Without this option this analysis may exit prematurely with a numerical error code due to the coarse mesh.) f.Click OK.

WS1-25 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 My Nonlinear Nonlinear_job1 Linear_job1 g h j i g.Enter Nonlinear_job1 as the Job Name. h.Click on Load Step Creation. i.Enter My Nonlinear as the Job Step Name. j.Click on Solution Parameters.

WS1-26 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December o Nonlinear  k m n p Static Solution Parameters from previous page Notice: IF you are setting up the analysis to be run with the older MSC.Marc 2000 rather than for the default version 2001 (or newer), you must open the Criteria form, turn ON the “Use Criterion” toggle button and click “OK” k.Select Nonlinear as the Linearity. l.Select Large Displacement / Large Strain. m.Check Loads Follow Deformations. n.Click on Load Increment Parameters. o.Enter.04 as the Maximum Time Steps. p.Click OK. l

WS1-27 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 My Nonlinear q r After you Apply, the new My Nonlinear step should appear under the Available Job Steps box. q.Create the Job Step by clicking Apply. r.Click Cancel.

WS1-28 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Nonlinear_job1 Linear_job1 My Nonlinear My Linear MY Nonlinear After you Select My Linear under Selected Job Steps It should disappear under Selected Job Steps. The final form should look like the one to the left. After you select “My Nonlinear” under Existing Job Steps it should appear under Selected Job Steps. s.Click on Load Step Selection. t.Select My Nonlinear from the Existing Job Steps. u.Click on My linear Step to de- select it. v.Click OK. w.Click Apply. s t u v w

WS1-29 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Nonlinear_job1 Linear_job1 Nonlinear_job1 Step 14. Analysis: Monitor / Job a b c You can view the status of the analysis and check for Exit Code (3004 means Normal Termination). You can also view the log and output files by clicking on the other “View” buttons. Monitor the nonlinear job. a.Monitor / Job. b.Select Nonlinear_job1 as the Job Name. c.Click on View Status File.

WS1-30 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 15. Analysis: Read Results / Result Entries / Attach Nonlinear_job1 nonlinear Linear_job1 Nonlinear_job1 a b Nonlinear_job1.t16 c d e Read Results from the nonlinear analysis a.Read Results / Result Entities / Attach. b.Click on Select Results File. c.Select Nonlinear_job1.t16. d.Click OK e.Click Apply.

WS1-31 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 16. Results: Create / Quick Plot After you apply your screen should look like this. If need be use the Deform Attributes form to set the scale to True (1.0). Post-Processing nonlinear job using Patran a.Results: Create / Quick Plot. b.Click on Select Results. c.Select the last increment. c.Select Displacement, Translation from the Select Fringe Result. d.Select Y Component. e.Select Displacement, Translation from the Select Deformation Result. f.Click Apply. a c d f g e b

WS1-32 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Step 17. Compare Your Results n Compare the results u Finally get the maximum Y deflection from the fringe spectrum/range. Enter that value into the table below. Another interesting post-processing technique is to create an animation by selecting the Animate Results Icon in the Results form. u Also compare the quickplots obtained with both jobs. (Below.) MSC/MARC Small DeflectionLarge Deflection Enter your new results (2x8 mesh) MSC/MARC Theory Small DeflectionLarge Deflection Compare with these (1x8 mesh)

WS1-33 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Nonlinear_job1 Linear_job1 Notice the horizontal displacement in the nonlinear solution As shown in the results obtained, inclusion of large deformation effects are very important in realistically modeling the physical behavior of the cantilever model.

WS1-34 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 Why do we ask you to have half the load on the center node and a quarter of the load on each corner node ? Each of the two elements connected to the center node contribute the same stiffness to the center node that each contribute to the corner node each is attached to. Step 18. Improve your Results n As a final step, do the following: 1. Detach both result files (use Analysis, Delete Result Attachment) 2. Delete the existing mesh 3. Create a new mesh that has the same number of elements lengthwise but has two elements over the height of the beam. 4. Modify the tip load so that the load in the center node is still 3000 while the load on each corner node is 1500 (for the same total of 6000 you had before). 5. Run both linear and nonlinear jobs again.

WS1-35 PAT328, Workshop 10, March 2001MAR120, Workshop 1, September 2001 MAR120, Workshop 1, December 2001 MSC/MARC Small DeflectionLarge Deflection Enter your new results (2x8 mesh) MSC/MARC Theory Small DeflectionLarge Deflection Compare with these results(2x8 mesh) 6. Attach the result files and make quick plots as before. Compare the Y- displacements with the ones obtained before and the theoretical values (previous page). Notice how much the results improved with the finer mesh.