Ae 569 - Project for Graduate Students

AE 569 - PROJECT FOR GRADUATE STUDENTS

(due January 26th, Thursday until 17:00 PM)

FINITE ELEMENT ANALYSIS BASED PROGRESSIVE FAILURE ANALYSIS OF LAMINATED COMPOSITE STRUCTURES

1. INTRODUCTION AND GENERAL DESCRIPTION OF THE FINITE ELEMENT BASED PROGRESSIVE FAILURE ANALYSIS

In this project groups (2 student per group) are expected to perform progressive failure analysis of a composite laminate with a central hole by finite element analysis. Students are expected to use a commercial finite element program as a solver, and write a code which will perform failure analysis and progress failure by employing sudden and gradual material property degradation. Students should not use the progressive failure analysis modules of certain commercial codes such as Abaqus, MD Nastran 2010 etc. The idea is to write a progressive failure analysis code and employ a commercial finite element code as a solver. This way, failure analysis code can be expanded by employing different failure and material property degradation schemes.

Two flowcharts of the progressive failure analysis were discussed in class. Flowcharts are linked in the course web site. These flowcharts are specific for hand calculation. In this project, finite element based progressive failure analysis will be performed by editing the input file of the finite element code which includes all the model information. This process is summarized below in Fig.1.

Fig. 1 Simplified flowchart of finite element analysis based progressive failure analysis

NOTE: Students who find it hard to fully automate the failure progression, via an external code, which does everything (runs FE code, reads output file, calculates failure indices based on the failure criterion used, performs material property degradation and modifes the input file), can have a separate code calculating failure indices and execute FE runs separately. This way, the process will not be automatic, and the user has to intervene at every step of the failure progression.

In order to effectively allow material property degradation at the ply level, for each element in the finite element mesh distinct composite laminate properties with distinct two dimensional orthotropic materials has to be generated. Stiffness reduction scheme can then be implemented easily for the failed ply by referencing the element property identification and material identification numbers of the ply.

A typical input file (.bdf) of Nastran is shown below. In this file PCOMP refers to the composite property identification cards. In order to progress failure at the ply level, distinct composite property identification has to be assigned for each element. These are given by the red numbers in the PCOMP cards. The blue numbers in the PCOMP cards refer to the layer materials. Thus, for each layer we define a new material. CQUAD4 cards refer to elements. The green numbers, in the CQUAD4 cards, refer to the element numbers and the red numbers in the CQUAD4 cards refer to the composite property cards PCOMP. MAT8 cards define the 2D orthotropic materials. Thus, in the example .bdf file given below, we have N*L number of layer materials defined (L: # of layers in an element, N: # of elements in the model). During material property degradation, all we have to identify is the number of the MAT8 cards that we should modify depending on whether failure is predicted or not. Once the related MAT8 card is modified, composite properties (PCOMP cards) will be automatically updated since PCOMP cards reference material MAT8 cards, as indicated by the blue numbers shown in the PCOMP cards.

An example output file is given after the input file. In this example, it is assumed that laminate has two plies. After the output file is created (following a Nastran run), the lines giving the stress results should be read. While reading the lines, element IDs and ply IDs should also be read and recorded. If failure of any particular layer is predicted, element ID and ply ID will be used to find the ID number of the MAT8 cards. Once the IDs of the failed plies are identified, these MAT8 cards should be modified in the input file. After the modification of the MAT8 cards, the code has to call for another FE run and the whole process will start all over again.

NOTE: Students who want to use other FE codes such as Abaqus, Ansys can do so. In that case, they have to use the input and output files of those programs, and carry out the reading and editing operations accordingly.

The main code that will perform progessive failure analysis can be written in FORTRAN, PYTHON, PERL (Ansys uses this script language), MATLAB, VISUAL BASIC etc. Remember that you have to read and edit text files many times during the progressive failure analysis. Therefore, you should use the code that you are most comfortable with.

------

EXAMPLE INPUT FILE OF NASTRAN

RED: PCOMP PROPERTY NUMBERS-PCOMP NO.

BLUE: LAYER MATERIAL NUMBERS - MID MO. and MAT8 numbers

GREEN: ELEMENT NUMBERS - CQUAD4 NO.

$ NASTRAN input file created by the MSC MSC.Nastran input file

$ translator ( MSC.Patran 13.1.116 ) on October 24, 2009 at 11:13:35.

$ Direct Text Input for Bulk Data

$ Elements and Element Properties for region : shell

$ Composite Property Record created from P3/PATRAN composite material

$ record : lam

$ Composite Material Description :

PCOMP 1 50. TSAI 0. 0.

1 .25 0. YES

2 .25 10. YES

3 .25 20. YES

. . . . .

L .25 20. YES

PCOMP 2 50. TSAI 0. 0.

L+1 .25 0. YES

L+2 .25 10. YES

L+3 .25 20. YES

. . . . .

2L .25 20. YES

. . . . .

PCOMP N 50. TSAI 0. 0.

(N-1)L+1 .25 0. YES

(N-1)L+2 .25 20. YES

NL .25 40. YES 1 .25 50. YES

CQUAD4 1 1 1 2 11 10 0.

CQUAD4 2 2 2 3 12 11 0.

CQUAD4 3 3 3 4 13 12 0.

......

CQUAD4 N N 71 72 81 80 0.

$ Referenced Material Records

$ Material Record : ortho

$ Description of Material : Date: 27-Dec-08 Time: 16:36:32

MAT8 1 181000. 10300. .28 7170. 7170. 5000. 1.6-9

1500. 1500. 40. 246. 68.

-.5

MAT8 2 181000. 10300. .28 7170. 7170. 5000. 1.6-9

1500. 1500. 40. 246. 68.

-.5

MAT8 3 181000. 10300. .28 7170. 7170. 5000. 1.6-9

1500. 1500. 40. 246. 68.

-.5

......

MAT8 N*L 181000. 10300. .28 7170. 7170. 5000. 1.6-9

1500. 1500. 40. 246. 68.

-.5

$ Nodes of the Entire Model

GRID 1 0. 0. 0.

GRID 2 125. 0. 0.

GRID 3 250. 0. 0.

GRID 4 375. 0. 0.

GRID 5 500. 0. 0.

GRID 6 625. 0. 0.

GRID 7 750. 0. 0.

GRID 8 875. 0. 0.

GRID 9 1000. 0. 0.

GRID 10 0. 125. 0.

GRID 11 125. 125. 0.

GRID 12 250. 125. 0.

GRID 13 375. 125. 0.

GRID 14 500. 125. 0.

GRID 15 625. 125. 0.

GRID 16 750. 125. 0.

$ Loads for Load Case : Default

$ Displacement Constraints of Load Set : n

SPC1 1 123 1 THRU 9

$ Displacement Constraints of Load Set : n1

SPC1 3 3 73

$ Pressure Loads of Load Set : p

PLOAD4 1 1 -1.-4 THRU 64

------

EXAMPLE OUTPUT FILE OF NASTRAN

ELEMENT PLY STRESSES IN FIBER AND MATRIX DIRECTIONS

ID ID NORMAL-1 NORMAL-2 SHEAR-12

1 1 3.00725E+04 -4.84032E+03 4.64574E+03

1 2 8.26329E+04 7.01767E+02 -8.22791E+03

2 1 3.85178E+04 -1.02513E+04 3.31139E+03

2 2 4.51463E+04 -5.88696E+02 -1.19184E+04

3 1 4.05495E+04 -1.06741E+04 2.74296E+03

3 2 4.54650E+04 -6.57785E+02 -1.21436E+04

. . . . .

------

2. MODEL DESCRIPTION

The model which will be used in the progressive failure analysis is a square composite laminate with a central hole, as shown in Fig. 2 below. The material properties of the ply material (T300/N5208) is given by:

=132.38GPa,=10.76 GPa, =0.24 5.66 GPa, 3.38 GPa,

Xt=1513.4 MPa, Xc=1696 MPa, Yt=44 MPa, Yc=44MPa, S=86.87 MPa

Ply thickness: 0.25 mm ( note that this thickness is larger than the prepreg thickness)

Laminate configurations to be investigated: [0/90/0], [90/0/90]

NOTE: In order to make a simple model, in this project only three plies are used in the laminate.

Fig. 2 Square composite laminate with a central hole

Laminates with the central holes will be investigated under uniaxial loading. Load case is shown in Fig. 3. Uniaxial loading is assumed to be applied in a displacement controlled fashion. That is, the end displacements are assumed to be controlled by the tensile test machine. The resulting constraint forces in the direction of the end displacement u can be determined from the output file of Nastran. Thus, you can draw the load displacement curve. Incremental load, given in the flowchart in Fig.1, corresponds to incremental displacement. Therefore, before you start progressive failure analysis, decide on an appropriate incremental displacement. Incremental displacement must be neither too small nor too large. You can decide on the appropriate incremental displacement by calculating the x-direction constraint forces at the right edge in sample runs before you start progressive failure analyis. The magnitude of the constraint force will give you a clue about the appropriatenes of the incremental displacement.

Fig. 3 Uniaxial tensile loading

During the finite element analysis, due to symmetry only quarter laminate will be modeled. Finite element model to be used is shown in Fig. 4 for the uniaxial tensile loading. In order to keep the model size small, finite element models are made coarse on purpose. This way students, who can not automate the progressive failure process, can make input file modifications in a short time. Each FE model has 12 elements and 3 plies per element. Thus, total number of 2D orthotropic materials to be defined, is 36.

It is assumed that the tests are carried on a uniaxial test machine. Therefore, boundary conditions are defined accordingly.

1: x disp. , 2: y disp. , 3: z displ. , 4: x-axis rot. , 5: y-axis rot. , 6: z-axis rot.

Fig. 4 Finite element model for the uniaxial tensile loading

3. FAILURE CRITERIA AND STIFFNESS DEGRADATION METHOD

Failure Criteria

Two dimensional Tsai-Wu failure criteria will be implemented in the progressive failure analysis code.

References:

Tsai-Wu

S.W. Tsai, “A General theory of strength for anisotropic materials”, Journal of Composite Materials, 5(1), 58-80 (1971).

Stiffness Degradation

Sudden degradation

For sudden degradation use a stiffness reduction factor of 0.001. Once failure is predicted, degrade all properties at once. This is the so-called complete ply failure method which is the conservative approach. Degrade E1,E2,G12,G13,G23,v12 by the reduction factor of 0.001. Once a property is degraded, make sure that you do not degrade it again during failure progression or load increase. So, you should have appropriate control statements in your code to prevent further degradation of elastic properties.

Gradual degradation

For gradual degradation use a stiffness reduction factor of 0.25. In case of gradual degradation, allow plies to fail repeatedly until the degradation factor reaches 0.001, which is assumed to indicate complete failure. In gradual degradation, since degradation factor is large your run will take longer to time to reach to ultimate failure. Again, as in sudden, upon the prediction of a failure degrade all material properties (E1,E2,G12,G13,G23,v12) by the stiffness reduction factor of 0.25. However, this time you have to allow repeated failures until the overall stiffness reduction factor becomes less than 0.001.

4. PROJECT REQUIREMENTS

(a) For the uniaxial tensile load case, students are expected to determine first ply load, failure progression and ultimate failure loads for both sudden and gradual degradation. For failure progression prepare simple plots such as shown below.

90 deg. layer 0 deg. layer

Load level: Nx = XXX

where shows failed layer.

Decision on ultimate failure:

Decide on the ultimate failure by making use of the following arguments:

i) Ultimate failure can be assumed to have occured, if in the FE model, all three layers of the three elements along a line fail. So, you should have three red dots on all 0 deg. and 90 deg. layers along a line such as the one shown in the figure below. (Note: In reality ultimate failure can occur before the failure of all layers, so use the second check in combination to make a better prediction about the ultiamte failure load)

0 and 90 deg. layers

ii) As a second check of the ultimate failure you can use the load displacement curve. Since you input is displacement, when you degrade a ply or plies, then the stiffness of the plate will be reduced, and therefore you will see drops in the total constraint force (total x-direction constraint forces) at the input displacement edge. Small drops may indicate single ply failures. For ultimate failure, you must observe a sharp drop in the total constraint force as shown in the Fig.5. However, in your models since you have 3 layers with either 0o or 90o fiber orientations, it is very likely that more than one layer may fail simultaneously. So, you have to be careful in deciding on the ultimate failure point.

Fig. 5 Typical load displacement curve during progressive failure analysis

(b) Write an project report which has the following sub-sections:

- Title page, group members

- Introduction: Give a brief introduction

- Description of your code (your methodology)

- Verification of your code (present a verification for the no hole case. And compare first ply load with the hand calculation)