WS- 1

1 / 25

# WS- 1 - PowerPoint PPT Presentation

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

I am the owner, or an agent authorized to act on behalf of the owner, of the copyrighted work described.

## PowerPoint Slideshow about 'WS- 1' - arich

Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author.While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server.

- - - - - - - - - - - - - - - - - - - - - - - - - - E N D - - - - - - - - - - - - - - - - - - - - - - - - - -
Presentation Transcript

WORKSHOP

Define a Composite Material

WS-1

NAS121, Workshop , May 6, 2002

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.
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.
Problem Description (cont.)
• 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.
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
CREATE NEW DATABASE

a

• 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
• Click OK

d

e

f

g

c

b

Step 1. Create a geometry model

d

a

• 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

Step 2. Use mesh seeds to define the mesh density

a

• In Elements, create mesh seeds.
• Select Create / Mesh Seed / Uniform
• Click on the top edgeof the plate to create a mesh seed
• Then click on the right edge

b

c

Step 3. Create a finite element mesh

a

• 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

b

c

d

Step 4. Apply boundary conditions to the model

d

a

• 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 Apply

e

c

b

f

g

Step 5. Apply loads to the model

a

b

e

• 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 Apply

d

c

f

g

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 <–1000 0 0>, then OK
• In Select Application Region, again click on the right hand side curveof 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

Step 6. Define ply material properties

a

c

• 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 OK
• Click Apply again

f

b

g

h

e

d

Step 7. Check Element Normals

b

a

c

• Check element normals to determine the location of ply 1.
• At the top menu click Reset Graphics
• At the top menu click Hide Labels
• Select Verify / Element / Normals
• Click Draw Normal Vectors
• Click Apply

d

e

Step 8. Define composite material properties

a

• 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: 0 -45 45 90 90 45 -45 0 . 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 Apply

e

c

b

f

d

h

g

Step 9. Define a material coordinate system

a

• 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

b

c

d

e

f

a

• 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 Apply

e

b

c

d

g

f

g

h

Step 11. Submit the model to MSC.Nastran for analysis

a

e

• 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

c

g

f

b

d

h

j

i

Step 12. Attach xdb Results File

a

• 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

c

d

b

e

Step 13. Display ply stresses using MSC.Patran

a

b

• 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

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 1 6.1711

0.0000

2 7.7170

0.0000

3 6.4169

0.0000

4 7.3154

0.0000

5 7.3154

0.0000

6 6.4169

0.0000

7 7.7170

0.0000

8 6.1711

7.7170 ***

.

.

.

c

d

a

b

e

f

Note that Patran does not display composite failure indices.

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 1.0. 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.
Step 15a. Change layup to make failure indices below 1.0

a

h

• 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 0 45 45 45 45 -45 -45 90 90 90
• Click Apply

d

j

g

b

f

k

e

c

l

i

m

n

Step 16. Analyze the model with the new composite layup

a

• Go to Analysis:
• Select Analyze / Entire Model / Full Run
• Click Apply
• Click Yes on both overwrite messages.

c

c

b

Step 17. View the changed ply failure indices

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 1 0.6422

0.0000

2 0.7709

0.0000

3 0.7709

0.0000

4 0.7709

0.0000

5 0.7709

0.0000

6 0.6580

0.0000

7 0.6580

0.0000

8 0.7494

0.0000

9 0.7494

0.0000

10 0.7494

0.0000

11 0.7494

0.0000

12 0.7494

0.0000

13 0.7494

0.0000

14 0.6580

0.0000

15 0.6580

0.0000

16 0.7709

0.0000

17 0.7709

0.0000

18 0.7709

0.0000

19 0.7709

0.0000

20 0.6422

0.7709

• To view the changed failure indices, again open the composite1.f06 file. Note that the failure indices are all below 1.0.