WORKSHOP 1 COMPOSITE MODEL OF LOADED FLAT PLATE WS1-1 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation. - презентация

1 WORKSHOP 1 COMPOSITE MODEL OF LOADED FLAT PLATE WS1-1 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation

2 Mar120, Workshop 10, March 2001 WS1-2 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation

3 Mar120, Workshop 10, March 2001 WS1-3 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Problem Description Model a 1x1 meter plate. Use millimeters as units of length. The plate is 4 mm thick and is a laminate made up of 16 plies with equal thickness. The laminate is uniform. The plies have two orientations, 0 and 90 degrees, i.e. parallel to the plate edges. The material properties of the lamina are E-modulus: E 11 = 181 GPa, E 22 = 10.3 GPa Shear modulus: G 12 = 7.17 GPa, G 23 = 5.00 GPa, G 13 = 7.17 GPa Poisson Ratio: 0.28 Density: 1.6E-9 The plate is fixed along one edge, and supported laterally at one of the two opposite corners. The plate is loaded with a uniform pressure of 0.1 KPa, giving a total force acting on the plate of 100 Newtons. We want to investigate the occurring stresses in the layers and the maximum deflection of the plate.

4 Mar120, Workshop 10, March 2001 WS1-4 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Suggested Exercise Steps 1. Create a new database 2. Create the model surface 3. Mesh the surface to create the model elements 4. Constrain an edge and an opposite point 5. Create pressure loading for the plate 6. Create 2D orthotropic material for lamina 7. Create composite laminate from 2D orthotropic material 8. Define 2D shell elements 9. Determine direction of element normals 10. Verify orientation angle of laminate 11. Run analysis using MSC.Nastran 12. Attach.XDB results file to MSC.Patran database 13. Look at stresses and displacements

5 Mar120, Workshop 10, March 2001 WS1-5 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation d e f b c Open a new database. Name it Flatplate.db. a.File / New. b.Enter Flatplate as the file name. c.Click OK. d.Select MSC.Nastran as the Analysis Code. e.Select Structural as the Analysis Type. f.Click OK. a Step 1. Create a New Database

6 Mar120, Workshop 10, March 2001 WS1-6 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Create the flatplate geometry. a.Geometry: Create / Surface / XYZ b.Enter as the Vector Coordinates List. c.Enter [0 0 0] as the Origin Coordinates List. d.Click –Apply-. e.Click Iso 3 View. Step 2. Create the Model Surface e b c d a

7 Mar120, Workshop 10, March 2001 WS1-7 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 3. Mesh the Surface to Create the Model Elements Create a mesh for the model. a.Elements: Create / Mesh / Surface. b.Select IsoMesh as the Mesher. c.Select Quad4 as the Topology. d.Uncheck the Automatic Calculation. e.Enter 125 as the Global Edge Length Value. f.Select Surface 1 for the Surface List. g.Click –Apply-. d e c b a f g

8 Mar120, Workshop 10, March 2001 WS1-8 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 4. Constrain an Edge and an Opposite Point Define constraints. a.Loads/BCs: Create / Displacement / Nodal. b.Enter Fixed Edge as the New Set Name. c.Click Input Data. d.Enter as the Translations. e.Click OK. f.Click Select Application Region. g.Select Edge Icon. h.Select Surface 1.4 for Select Geometry Entities. i.Click Add. j.Click OK k.Click –Apply-. d e g h i j b c a f k

9 Mar120, Workshop 10, March 2001 WS1-9 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Define constraints. a.Loads/BCs: Create / Displacement / Nodal. b.Enter Supported Point as the New Set Name. c.Click Input Data. d.Enter as the Translations. e.Click OK. f.Click Select Application Region. g.Select Point Icon. h.Select Point 2 for Select Geometry Entities. i.Click Add. j.Click OK k.Click –Apply-. b c d e a f g h i j k Step 4. Constrain an Edge and an Opposite Point (Cont.)

10 Mar120, Workshop 10, March 2001 WS1-10 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Define Loading. a.Loads/BCs: Create / Pressure / Element Uniform. b.Enter Pressure Load as the New Set Name. c.Click Input Data. d.Enter as the Top Surf Pressure. e.Click OK. f.Click Select Application Region. g.Select Surface Icon. h.Select Surface 1 for Select Surface or Edges. i.Click Add. j.Click OK k.Click –Apply-. Step 5. Create Pressure Loading for the Plate b c d e a f g h i j k

11 Mar120, Workshop 10, March 2001 WS1-11 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Note that the pressure is in MegaPascals. Until now this exercise has been quite straight forward, but the next step is to define the laminate. The model should look like this after clicking –Apply-. Step 5. Create Pressure Loading for the Plate (Cont.)

12 Mar120, Workshop 10, March 2001 WS1-12 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 6. Create 2D Orthotropic Material for Lamina Define lamina material properties. a.Materials: Create / 2D Orthotropic / Manual Input. b.Enter ud_t300_n5208 as the Material Name. c.Click Input Properties. d.Select Linear Elastic as the Constitutive Model. e.Enter as the Elastic Modulus 11. f.Enter as the Elastic Modulus 22. g.Enter 0.28 as the Poisson Ratio 12. h.Enter 7170 as the Shear Modulus 12. i.Enter 5000 as the Shear Modulus 23. j.Enter 7170 as the Shear Modulus 13. k.Enter 1.6E-9 as the Density. l.Click OK. m.Click Apply. b c d e a f g h i j k l m These material properties will be used later for other workshops. Thus, a session file, material.ses, is provided with the workshop files. This can be played into MSC.Patran creating the properties quickly and easily.

13 Mar120, Workshop 10, March 2001 WS1-13 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 7. Create Composite Laminate From 2D Orthotropic Material Define laminate properties. a.Materials: Create / Composite / Laminate. b.Enter My first laminate as the Material Name. c.Select Insert as the Text Entry Mode. d.Select Material Names. e.Input 16(ud_t300_n5208) as the Insert Material Names. f.Click Load Text Into Spreadsheet. 16 rows corresponding to plies are created. Also, need to fill in thickness and orientations. Now build the laminate out of the lamina just defined. Take notice of how the laminate is defined in the spreadsheet. b c d e a f

14 Mar120, Workshop 10, March 2001 WS1-14 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation a.Select Overwrite as the Text Entry Mode. b.Select Thickness. c.Enter 16(0.25) as the Overwrite Thicknesses. d.Click Load Text Into Spreadsheet. a b c d Step 7. Create Composite Laminate (Cont.)

15 Mar120, Workshop 10, March 2001 WS1-15 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation a.Select Overwrite as the Text Entry Mode. b.Select Orientations. c.Enter 4(90/0) as the Overwrite Orientations. d.Click Load Text Into Spreadsheet. e.Enter 4(0/90) in Overwrite Orientations. f.Click Load Text Into Spreadsheet. g.Click –Apply-. (4 pairs of 90 degrees and 0 degrees) (4 pairs of 0 degree and 90 degrees) a b c d e f g Step 7. Create Composite Laminate (Cont.)

16 Mar120, Workshop 10, March 2001 WS1-16 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 8. Define 2D Shell Elements Define 2D element properties. The composite laminate material property is to be used. a.Properties: Create / 2D / Shell. b.Enter Plate as the Property Set Name. c.Select Laminate as the Options. d.Select Standard Formulation as the Options. e.Click Input Properties. f.Select My First Laminate as the Material Name. g.Select Vector. h.Enter as the Material Orientations. i.Click OK. j.Select Surface1 as the Select Members. k.Click Add. l.Click Apply. f g h i Now the fiber directions have been related to the MSC.Patran global X direction. Half of the fibres are rotated 90 degrees relative to this direction. b c d e a j k l

17 Mar120, Workshop 10, March 2001 WS1-17 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 9. Determine Direction of Element Normals Verify laminate direction. a.Elements: Verify / Element / Normals. b.Select Draw Normal Vectors as the Display Control. c.Click Apply. Verify that all vectors are pointing in the positive z-axis direction b c a It is best to check a model before running an analysis, especially when the materials are laminates. Remember that layer 1 is at the bottom of the stack of plies. First, check the direction of the element normals to determine what direction is up.

18 Mar120, Workshop 10, March 2001 WS1-18 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Verify Laminate Direction. a.Properties: Show. b.Select Orientation Angle as the Existing Properties. c.Select Vector Plot as the Display Method. d.Click –Apply-. The initial reference direction is shown. Note that the individual fibre directions cannot be seen. They can only be checked in the laminate spreadsheet. The total laminate thickness can be checked, but this is of little interest in this case. It is necessary to verify that all the layers are defined correctly, and there are several tools that can be used to do this task. Step 10. Verify Orientation Angle of Laminate b c a d

19 Mar120, Workshop 10, March 2001 WS1-19 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 11. Run Analysis Using MSC.Nastran Set up and run the analysis. a.Analysis: Analyze / Entire Model / Full Run b.Click Subcases. c.Select Default as an Available Subcases. d.Click Output Requests. b a c d

20 Mar120, Workshop 10, March 2001 WS1-20 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation a.Select Advanced as the Form Type. b.Select STRESS as the Output Requests. c.Select Ply Stresses as the Composite Plate Opt. d.Click OK. a b c d Step 11. Run Analysis Using MSC.Nastran (Cont.)

21 Mar120, Workshop 10, March 2001 WS1-21 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation a.Click Apply in the Subcase Menu. b.Click Cancel. c.Click Apply in the Analysis menu. a b c Step 11. Run Analysis Using MSC.Nastran (Cont.)

22 Mar120, Workshop 10, March 2001 WS1-22 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 12. Attach.XDB Results File to MSC.Patran Database Create a link to the MSC.Nastran analysis results file a.Analysis: Access Results / Attach XDB / Result Entities. b.Click Select Results Files. c.Select Flatplate.xdb. d.Click OK. e.Click Apply. c d b e a

23 Mar120, Workshop 10, March 2001 WS1-23 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation View the results a.Results: Create / Quick Plot. b.Select Default, Static Subcases as the Select Result Cases. c.Select Stress Tensor as the Select Fringe Result. d.Select Layer 12 as the Position. e.Click Close. f.Select X Component as the Quality. g.Select Displacements, Translational as the Select Deformation Result. h.Click Apply. Step 13. Look at Stresses and Displacements d e First look at the stresses in one of the layers. Choose layer 12, and plot stresses in the X- direction. b c a f g h d

24 Mar120, Workshop 10, March 2001 WS1-24 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Step 13. Look at Stresses and Displacements (Cont.)

25 Mar120, Workshop 10, March 2001 WS1-25 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation Also, investigate the deflection of the plate. a.Select Displacements, Translational as the Select Fringe Result. b.Click Apply. b a Step 13. Look at Stresses and Displacements (Cont.)

26 Mar120, Workshop 10, March 2001 WS1-26 PAT325, Workshop 1, February 2004 Copyright 2004 MSC.Software Corporation If extra time Another laminate builder tool can be found in the Utilities menu: Materials/Laminate Builder Tool. Check it out. If you have any questions, please do not hesitate to ask. Do not delete this database, it will be used later.