Using MSC SimXpert, create, verify, and post-process a composite layup model using the following statements and properties: Problem Description: a 1 in. x 1 in. composite plate is loaded with 2000 lb/in. in the Y direction on the top edge, 1000 lb/in. in both the X direction and Y direction on the right hand side edge. Composite Description: The left side reacts the loads with X, Y, Z, and Ry constraints. The layup is made of graphite/epoxy tape and is shown to the right. The angles shown are relative to the global axis shown. Thus, the 0 degree ply 1 has its fibers running along the Y direction, and 90 degree ply 4 has its fibers running along the X direction Note that while the positive sense of the angles are right hand rule around the Z global axis in this layup definition, in the Nastran definition, it is around the element Z axis and thus dependent on the element node order. Material Description: The composite plies are graphite/epoxy tape with a thickness of 0.0054 in. The elastic and strength properties are shown on the right. The failure theorem to be used is Hill.

1) Click Structures.

1) Check in the lower right-hand corner for the current system of units.

2) If the current system of units is not English units (in, lb, s), click on the box to bring up the User Options form.

3) Click on Standard Units.

4) Scroll down and select the line with units in, lb, s,…

5) Click OK and OK.

1) Under the Geometry tab, click Filler in the Surface group.

2) Select Points.

3) Click in the Points text box and enter 0, 0, 0;1,0,0; 1,1,0; 0,1,0.

4) Press Enter then click OK.

5) Change the view to Top.

1) Under the Meshing tab, click Surface in the Automesh group.

2) Select the surface.

3) Enter 0.5 for Size.

4) Click OK.

1) Under the Geometry tab, pull down Coord and and then Cartesian in the Construction Geom group.

2) Select 3 Points for Method and enter 0, 0, 0 for Location, enter 0, 0, 1 for Point on Axis, and select Z for Axis. Enter 0, 1, 0 for Point on Plane, and select XZ.

3) Click the Visualization tab.

4) Change the Color to Blue and click OK.

1) Under the Nodes/Elements tab, click Assign LCS in the Modify group.

2) Select To Shell Element for Assign LCS.

3) Select the local coordinate system.

4) Click in the Shell element text box and select Select All on the Pick Filter.

5) Click OK.

1) Under the LBCs tab, click General in the Constraints group.

2) Enter X Z Ry Constraints for Name.

3) Click in the Entities text box and deselect all filters except Curves from the Pick Filter.

4) Select the left vertical edge of the surface.

5) Uncheck T2, R1, and R3 and click Apply.

6) Change the Name to Y Constraint.

7) Pull down the down arrow to the right of the Entities text box and select Clear.

8) Select only Nodes from the Pick Filter.

9) Select the node at the bottom left corner of the surface.

10) Check only T2; uncheck all others. Click OK.

1) Click Force in the LBCs group.

2) Enter Y_load_(top) for force Name.

3) Click in the Entities text box.

4) Select the middle node on the top edge.

5) Enter 1000 for Scale Factor.

6) Enter 0 1 0 for the Direction and click Apply.

7) Turn On Detailed Rendering.

8) Display the geometry in Geometry Wireframe. You may want to rotate your model slightly in order to see the LBC vectors.

1) Enter force Name, X load (ends).

2) Pull down the down arrow to the right of the Entities text box and select Clear.

3) Select the top and bottom nodes on the right edge.

4) Enter 250 for Scale Factor.

5) Enter 1 0 0 for the Direction and click Apply.

2) Pull down the down arrow to the right of the Entities text box and select Clear.

3) Select the top and bottom nodes on the right edge.

4) Enter 250 for Scale Factor.

5) Enter 1 0 0 for the Direction and click Apply.

2) Pull down the down arrow to the right of the Entities text box and select Clear.

3) Select the middle node on the right edge.

4) Enter 500 for Scale Factor.

5) Enter 1 0 0 for the Direction and click Apply.

2) Pull down the down arrow to the right of the Entities text box and select Clear.

3) Select the middle node on the right edge.

4) Enter 500 for Scale Factor.

5) Enter 0 1 0 for the Direction and click Apply.

1) Enter force Name, Y_load_(right ends).

2) Pull down the down arrow to the right of the Entities text box and select Clear.

3) Select the two corner nodes on the right edge.

4) Enter 250 for Scale Factor.

5) Enter 0 1 0 for the Direction and click Apply.

1)Under the Materials and Properties tab, click Orthotropic 2D in the Materials group.

2) Enter graphite_epoxy_tape for the Name.

3) Enter 20e6, 2e6, 0.35, 1e6 for the Moduli and Poisson’s Ratio as shown and click Advanced.

4) Enter 1e6 for the shear moduli as shown.

5) Check the Specify failure limits check box.

6) Select Stress for Failure Limits.

7) Enter the following stress limits as shown: 130e3, 120e3, 11e3, 12e3, 12.5e3 and click OK.

1) Click Layered composite in the 2D Properties group.

2) Enter 8_ply_symmetric for Name.

3) Click in the Entities text box and deselect Elements, Parts, and Sheet Features in the Pick Filter.

4) Select the surface.

5) Click Laminate Editor.

6) Highlight graphite epoxy tape in the Ply Source list box.

7) Enter the following: Multiplier: 1, Thickness: 0.0054, Orientation: 0, Stress Output: YES.

9) Repeat steps b and c entering the following orientations in this order: 45, -45, 90. The other parameters remain constant.

10) Click the Create Symmetric button to complete the stacking sequence. Click Apply.

12) Enter 5000 for the Bonding material shear stress.

13) Select HILL for Failure theory. Click OK.

1) Under the Quality tab, pull down Misc. > Laminate Verification in the Edit/Fix Elements group.

2) Select Element for Verify By.

3) Pull down Ply Angles for By Element Type.

4) Check Fringe for Method and click Apply.

5) Hide the display of Coordinate Frames and LBC Symbols.

6) Orient the model to Isometric View.

7) Check Arrow and Label for Method. Choose a color that will clearly show on the screen and click Apply.

8) Pull down Thicknesses (Laminates) for By Element Type.

9) Check Fringe for Method. Click Apply.

10) Pull down Element Normal for By Element Type.

11) Check Arrow for Method. Click Apply.

12) Pull down Material Coordinate System for By Element Type.

13) Check Fringe and Arrow for Method and click Apply and then Cancel.

14) Select to return to the Previous View to return the model to plan view.

1) Right-click FileSet, and select Create new Nastran job.

2) Change the Job Name to Composite.

3) Select Linear static Analysis (SOL 101) for the Solution Type.

4) If desired, click the folder icon for Solver Input File and select the file path location. Click OK.

5) Right-click Composite under Simulations and select Run.

6) Go to File and Attach Results.

7) Under File Path, locate the composite.xdb file and click OK.

1) Under the Results tab, click Deformation in the Results group.

2) Select the Result case.

3) Highlight Displacements, Translational for Result type. Click Update.

4) Select Fringe for Plot type.

5) Highlight Stress Tensor for Result type.

6) Highlight Stress Tensor for Result type.

7) Highlight Stress Tensor for Result type.

8) Highlight Stress Tensor for Result type.

9) Highlight Stress Tensor for Result type.

1) Click Hide.

2) Select Vector for Plot type.

3) Highlight Stress Tensor for Result type

4) Highlight Max Principal for Derivation.

5) Highlight Layer 1. Click Update.

5) Repeat steps e and f for each layer.