1. Define a Composite Material
WORKSHOP
Define a Composite Material
NAS121, Workshop , May 6, 2002
WS-1

2. Problem Description
A 1 in. x 1 in. composite plate is loaded with 2000 #/in. in the Y direction on the top edge, 1000 #/in. in both the X direction and Y direction on the right hand side edge.
The left side reacts the loads with X, Y, Z, and Ry constraints.

3. Problem Description
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 it’s fibers coming out of the page in the Y 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 Z element axis and thus dependent on the element GRID order.

4. Problem Description (cont.)
U12
.35
G12
1e6
G13
G23 Xt
120 ksi Xc
110 ksi Yt
13 ksi Yc
16 ksi S
14 ksi Sb
5 ksi
Problem Description (cont.)
The composite plies are graphite/epoxy tape with a thickness of in.
The elastic and strength properties are shown on the right.
The failure theorem to be used is Hill.

5. Suggested Exercise Steps
Create a geometry model.
Use mesh seeds to define the mesh density.
Create a finite element mesh.
Apply boundary conditions to the model.
Apply loads to the model.
Define ply material properties.
Check element normals
Define composite material properties.
Define a material coordinate system
Apply the material coordinate system to the elements.
Submit the model to MSC.Nastran for analysis.
Attach xdb Results File
Display ply stresses using MSC.Patran.
View ply failure indices in MSC.Nastran
Change layup to make failure indices below 1.0.
Analyze the model with the new composite layup
View the changed ply failure indices

6. CREATE NEW DATABASE a d e f c g b
Create a new database called composite1.db:
In File select New
Enter composite1 as the file name
Click OK
Choose Default Tolerance
Select MSC.Nastran as the Analysis Code
Select Structural as the Analysis Type e f b c g

7. Step 1. Create a geometry model
In Geometry create the first curve.
Select Create / Surface / Vertex
On the Surface Vertex “n” Lists enter [0 0 0], [1 0 0], [1 1 0], [0 1 0]
Click Apply
Click the Show Label icon b c

8. Step 2. Use mesh seeds to define the mesh densitya b
In Elements, create mesh seeds.
Select Create / Mesh Seed / Uniform
Click on the top edge of the plate to create a mesh seed
Then click on the right edge c

9. Step 3. Create a finite element meshb
In the Elements menu create surface mesh based on the mesh seeds assigned in the previous steps.
Select Create / Mesh / Surface
Select Quad as the Elem Shape
Click on surface 1
Click Apply c d

10. Step 4. Apply boundary conditions to the model
In Loads/BCs
Select Create / Displacement / Nodal
For New Set Name enter “constraints”
In Input Data, enter <0,0,0> for Translations, <,0,> for Rotations then OK
On the top menu click on the Curve or Edge icon
In Select Application Region click lefthand edge of the surface
Click Add and OK
Click Apply e c b f g

11. Step 5. Apply loads to the model
On the top menu click Reset Graphics
Select Create / Distributed Loads / Element Uniform
Enter “Dist. Load Y” for New Set Name
In Input Data, Enter <0 –2000 0> for Edge Distr Load <f1 f2 f3>, then OK
In Select Application Region, click on the top curve of the surface
Click Add then OK
Click Apply b e d c f g

12. Step 5a. Apply loads to the model (cont.)
In a similar way create Dist. Load X:
Enter “Dist. Load X” for New Set Name.
In Input Data, Enter <0 –1000 0>, then OK
In Select Application Region, click on the right hand side curve of the surface, then Add, then OK.
Click Apply
And then create Dist. Load XY:
Enter “Dist. Load XY” for New Set Name.
In Input Data, Enter <– >, then OK
In Select Application Region, again click on the right hand side curve of the surface, then Add, then OK.
Click Apply
Note that since the same edge was picked, the loads are combined a e b c d

13. Step 6. Define ply material properties
Go to Material menu
Select Create / 2d Orthotropic / Manual Input
For Material Name enter “graphite-epoxy_tape”
Click Input Properties, Select Linear Elastic, enter 20e6, 2e6, .35, 1e6, 1e6, 1e6
Click OK
Click Apply
Click Input Properties again, Select Failure / Stress / Hill and enter 120e3, 13e3, 110e3, 16e3, 13e3, 5000.
Click Apply again c f b g e h d

14. Step 7. Check Element Normalsb
Check element normals to determine the location of ply 1.
Select the Element menu:
At the top menu click Reset Graphics
At the top menu click Hide Labels
Select Verify / Element / Normals
Click Draw Normal Vectors
Click Apply c d e

15. Step 8. Define composite material properties
Go to Materials:
Select Create/ Composite/ Laminate
At Material Name enter 8_ply_symmetric_quasi
Click tape property name (graphite-epoxy_tape) slowly 8 times to make 8 plies
At Thickness for all layers enter .0054<cr>
Click on ply 1’s empty Orientation cell
Enter the following into the Insert Orientations box: Note that the +-45 degree plies have changed sign due to the element Z axis being in the opposite direction to the global Z axis.
Click Load Text Into Spreadsheet
Click Apply e c b f d g h

16. Step 9. Define a material coordinate system
Go to Geometry:
Select Create / Coord / 3Point
Enter Coord ID (99 in this case) you want at Coord ID list
At Origin enter [0 0 0]
At Point on Axis 3 enter [0 0 1]
At Point on Plane 1-3 enter [0 1 0]
Click Apply a b c d e f

17. Step 10. Apply the material coordinate system to the elements
Go to Properties:
Select Create / 2D / Shell
Enter “composite1” at Property Set Name
At Options select Laminate
In Input Properties click on the composite material name (8_ply_symmetric_quasi)
At Material Orientation select CID and then click the material coordinate system 99 on the screen
Click OK
Click Application Region and click on Surface 1
Click Add
Click Apply a e b c d g f g h

18. Step 11. Submit the model to MSC.Nastran for analysis
Go to Analysis:
Select Analyze / Entire Model / Full Run
Click Subcases
At Available Subcases click Default
Click Output Requests
At Form Type select Advanced
At Output Requests, click twice STRESS(SORT1,REAL,VONMISES,BINLIN)=ALL;PARAM,NOCOMPS,-1
At Composite Plate Opt: select Ply Stresses. Note that PARAM, NOCOMPS,-1 has now changed to 1.
Click OK
Click Apply at Subcases and then Cancel
And click Apply at the Analyze menu a e c g f b h d j i

19. Step 12. Attach xdb Results File
Go to Analysis:
Select Attach XDB / Result Entities / Local
Click Select Results File
Use the Select File tool to find your xdb file in your local Patran directory and click it, in this case, “composite1.xdb”
Click OK
Click Apply a c d b e

20. Step 13. Display ply stresses using MSC.Patranb
To display the ply 8’s 1 direction stresses:
go to the Results menu:
First turn off the geometry in Plot/Erase Geometry Erase
Select Create / Quick Plot
Click Stress Tensor
Click Position then select Layer 8 and click Close
Click Quantity and select X Component
Click Displacements Translational
Click Apply d c e f g

21. Step 14. View ply failure indices in MSC.Nastran
To view the failure indices, open the composite1.f06 file in an editor and search for the following section. It is organized as follows:
Element number
Ply number
Ply failure index
Ply interlaminar failure index
Highest failure index in element
Flag if highest failure index is greater than 1.0 (indicating ply failure)
F A I L U R E I N D I C E S F O R L A Y E R E D C O M P O S I T E E L E M E N T S ( Q U A D 4 )
ELEMENT FAILURE PLY FP=FAILURE INDEX FOR PLY FB=FAILURE INDEX FOR BONDING FAILURE INDEX FOR ELEMENT FLAG
ID THEORY ID (DIRECT STRESSES/STRAINS) (INTER-LAMINAR STRESSES) MAX OF FP,FB FOR ALL PLIES
1 HILL
0.0000
*** . c d a b e f
Note that Patran does not display composite failure indices.

22. Step 15. Change layup to make failure indices below 1.0
Hand calculations
Element 1, ply 2, a –45 degree ply, has the highest failure index of 7.72 but all of the plies have similar values, thus it is difficult to determine which direction to add plies. However, looking at the terms of Hill’s theorem may tell us:
Substituting values:
Shows that the 1 direction is the largest contributor to the failure and thus the composite needs more -45 degree plies.
Using this same method, it was found that a 20 ply symmetric layup will give failure indices less than The layup is a 0 ply, 4 45 plies, 2 –45 plies, and 3 90 plies and then a symmetric layup for the other 10 plies.

23. Step 15a. Change layup to make failure indices below 1.0
To change to a new layup:
go to Materials:
Select Modify / Composite / Laminate
In Laminated Comp. To Modify click 8_ply_symmetric_quasi
At New Material Name enter 0_4x45_2x-45_3x90_sym
In the Laminated Composite popup click on ply 1 and then shift click on ply 8 to select all the plies
Click on Delete Selected Rows
Select Text Entry Mode Insert.
In the Modify Menu on the right, click slowly on graphite-epoxy_tape 10 times, once for each ply
On Stacking Sequence Convention select Symmetric
At Thickness For All Layers enter .0054<cr>
Click on the empty ply 1 Orientation cell
Select Text Entry Mode Overwrite
In Overwrite Orientations enter
Click Load Text Into Spreadsheet
Click Apply h d j g b f k e l c i m n

24. Step 16. Analyze the model with the new composite layup
Go to Analysis:
Select Analyze / Entire Model / Full Run
Click Apply
Click Yes on both overwrite messages. a c c b

25. Step 17. View the changed ply failure indices
To view the changed failure indices, again open the composite1.f06 file. Note that the failure indices are all below 1.0.
F A I L U R E I N D I C E S F O R L A Y E R E D C O M P O S I T E E L E M E N T S ( Q U A D 4 )
ELEMENT FAILURE PLY FP=FAILURE INDEX FOR PLY FB=FAILURE INDEX FOR BONDING FAILURE INDEX FOR ELEMENT FLAG
ID THEORY ID (DIRECT STRESSES/STRAINS) (INTER-LAMINAR STRESSES) MAX OF FP,FB FOR ALL PLIES
1 HILL
0.0000
0.7709