User login

You are here

modelling

Hi

i have to model a graphite/epoxy [0/+-45/90]2s composite laminate using ansys. can anyone please help me how to model it, as i m using ansys 4 the 1st time and dont know how to model a composite.

waiting 4 an early response

regards

Khan

Comments

Engr. Adeela Khan

ramdas chennamsetti's picture

You may choose SHELL99 element. This is a layered shell element. Define the fiber orientation, material properties and thickness for each lamina in Real constants. Go through element library (help) before using this element.

I don't know whether this element is available in ANSYS 4 or not??? You may check in higher versions.

- Ramdas

thanks for ur suggestions. i will try and hope it works

Octavio A. González Estrada's picture

Ramdas is right, the SHELL99 element allows you to model composite materials. Before meshing you have to pay special attention to the element coordinate system been used. Normally for simple problems, using mesh attributes you can set an ESYS that is in conformity with the layer orientation. You can check the link here for more info.

hi,

i followed shell99 element 4 my graphite/epoxy composite laminate, but the problem i m having is how to provide these given values in ansys,

my data is

Typical properties for unidirectional graphit/epoxy [0/+-45/90]2s  system at room temp.

longitudinal tensile modulus(ksi)     20300,

transverse tensile modulus(ksi)        1490,

shear modulus (ksi)                        830,

poisson's ratio (major)                    0.3,

fiber volume fraction                       0.74,

average thickness (in)                    0.005,

can u plz guide me towards this,

waiting for an early response

regards

Khan

 

Octavio A. González Estrada's picture

Check this layer definition for a  [90 0 90]s laminate, though one can define a symmetry option I think is better to define the whole set of layers. Tensile and shear modulus are defined in material properties, fiber volume fraction is not introduced as it is a parameter related to these tensile modulus. Thickness can be set for each different layer in RMODIF.

 

 /PREP7  
!PLATE UNDER UNIAXIAL LOAD

!Element definition: layers and materials
ET,1,SHELL99
KEYOPT,1,8,1
 
!Real Constants: Layers
R,1
RMODIF,1,1,6,0,0,0,0,0      !6 layers
RMODIF,1,13,    1,90,0.5e-3,    !set table_position 1 layer_angle layer_thickness
RMODIF,1,16,    1,0,0.5e-3,
RMODIF,1,19,    1,90,0.5e-3,    
RMODIF,1,22,    1,90,0.5e-3,
RMODIF,1,25,    1,0,0.5e-3,    
RMODIF,1,28,    1,90,0.5e-3,

!Materials
MPTEMP,,,,,,,,  
MPTEMP,1,0  
MPDATA,EX,1,,200e9          !longitudinal tensile modulus
MPDATA,EY,1,,5.2e9          !transverse tensile modulus
MPDATA,EZ,1,,5.2e9          !EY=EZ plane stress
MPDATA,PRXY,1,,0.26         !Major Poisson's ratios
MPDATA,PRYZ,1,,0.26
MPDATA,PRXZ,1,,0.26
MPDATA,GXY,1,,3e9           !Shear modulus
MPDATA,GYZ,1,,3e9   
MPDATA,GXZ,1,,3e9   
MPTEMP,,,,,,,,  
MPTEMP,1,0 

Engr. Adeela Khan

hi,

when we create a model for composite laminate, do we have to create each layer separately and then glue it together, or simply we just define the thickness and angles in real constant and model a simple one layer model having all the properties of layers. if so, how we can check the behavior of individual layers.

waiting for an early response

regards

Khan

Octavio A. González Estrada's picture

Hi Adeela,

You don't have to create each layer separately since you are already defining them within the SHELL99 properties using real constants. This definition would be the one that characterizes laminate's response. Afterwards, you can use the command LAYPLOT to check visually the layer setting. Further postprocessing includes choosing a layer to display results with the command LAYER,n. You can choose if you want results in the top of that layer: SHELL, Top, or in the bottom: SHELL, Bot. It's recommended at this point to display results  using the coordinate system of the active layer: RSYS, Solu.

Cheers, 

 

Thanks alot.

It has really helped me alot.

Regards

Khan

hi,

can u plz tell me how to apply a tensile load of 20 lb/sec with a total range of load 10,000 lbs on a bar end in ansys, i have chosen shell99 element and i have to find the point of failure in the notched bar and the maximum stress induced at that point.

waiting 4 an early response

regards

Khan

I am working on FE Modelling of Composite (graphite-epoxy) hollow rectangular section
beam in Ansys. When I select beam 188 element, there is no need of
inputting real constants. Where do i put the initial values in
pre-processing????Pls do help me,,I am new to applying Composite
material in Ansys.....pls...

Hamid Keshavarzi's picture

Hi friends,

I want to apply some number of unidirectional CFRP lamina with different orientations and make a laminate plate.  I have the in-plane properties of lamina only and in ANSYS I have to define other out-of-plane properties which I don’t have.

Can anyone help me to solve the problem?

 Thank you in advance.

ramdas chennamsetti's picture

Hi,

In general, lamina is assumed to be transversely isotropic. Number of independent constants required becomes five, because of the following relations.

E22 = E33

G12 = G13

E22 = 2G23(1+nu23)

nu12 = nu13

Since E22, G12 and nu12 are in-plane properties. Use above relations to get unknown properties. Only nu23 is not known. This is value is very close to matrix Poisson ratio. Use that value (=nu23).

With regards,

- Ramadas

Hamid Keshavarzi's picture

 

Thank you Ramadas. It was functional.

Hamid

Hamid Keshavarzi's picture

 

Hi all,

I have to model a 3d layup composite rather than a shell type with ABAQUS.

I have difficulty assigning appropriat material properties to a 3d stress element.

Is there anyone who can help me?

Thank you in advance.

Hamid

Subscribe to Comments for "modelling"

Recent comments

More comments

Syndicate

Subscribe to Syndicate