Graded materials finite element modeling 2

[dankoonFANTOMAS]

Hello the community,

I want to make a simple example of FGM (functionally graded materials) finite element model but with continuous variation in elements. Not by modeling each layer with a different property buy by displaying the continuous transition between MAT A and MAT B in an element. See as below:

I am used using OPTISTRUCT and ABAQUS for FEA so I had a look to the subroutine options for user material definitions.

In ABAQUS I saw subroutine UMAT written in FORTRAN modeling a variation of the young modulus E with an exponential function through the length of the model using uni axial coordinates of the integration points. If MAT A has Ea as young modulus and MAT B has Eb and L as the length of model we have:

A=(1/L)Ln(Eb/Ea)
E(x)=(Ea)exp(Ax)

The Jacobian matrix is calculated using E(x) (by calculating Lame's constants)and then the stress and strain. But does this will affect different properties for eache element or does ABAQUS will interpolate the material properties between each integration point? Because I saw that some people used USDFLD for spatial variation of parameters but I am not familiar with that I do not kknow if it's better or worst for FGM transition modeling.

There is an equivalent in OPTISTRUCT using USRMAT in the version 2017. But there are less arguments than in ABAQUS subroutines, for example the variable COORDS that are the X coordinates of the integration points is not available so I cannot reproduce the same subroutine.

Does someone has experience with modeling FGM elements? And can tell me how to model the sooth material transition?

Thks

 

[Mustaine3]

You've already named two options in Abaqus. Programming a USDFLD, where the the youngs modulus is dependend of field variable, is definitely easier than a UMAT.

But there is another method, than does not require programming a subroutine, as long as you don't do a thermal analysis. Make your material properties depended of the temperature and then define the value of the temperature with a formula in A/CAE depended of the position (=Analytical Field). With that you also get a spatial variation of the material property.

 

[dankoonFANTOMAS]

Thk you for your advice.

For the USDFLD program I came across a subroutine written by Emilio Martinez-Paneda for parameter transition between integration points. Here is the program:

SUBROUTINE USDFLD(FIELD,STATEV,PNEWDT,DIRECT,T,CELENT,
1 TIME,DTIME,CMNAME,ORNAME,NFIELD,NSTATV,NOEL,NPT,LAYER,
2 KSPT,KSTEP,KINC,NDI,NSHR,COORD,JMAC,JMATYP,MATLAYO,LACCFLA)
C
INCLUDE 'aba_param.inc'
C
CHARACTER*80 CMNAME,ORNAME
CHARACTER*3 FLGRAY(15)
DIMENSION FIELD(NFIELD),STATEV(NSTATV),DIRECT(3,3),
1 T(3,3),TIME(2)
DIMENSION ARRAY(15),JARRAY(15),JMAC(*),JMATYP(*),COORD(*)
C DIMENSION INTV(1),REALV(1)


X=COORD(1)
Y=COORD(2)

FIELD(1)=dexp(2.07944154168*X)



RETURN
END

I have difficulties understanding the program is doing with "FIELDS".. Can someone help me?

 

[Mustaine3]

In the model you make the material properties dependent of a field variable. With a subroutine you can define the values of this field variable with you own function. The value of FIELD(1) is reported back to Abaqus for each integration point individually.

 

[dankoonFANTOMAS]

Ok and I make the link with material properties in the input file with dependencies right?

*Material, name=MAT
*Depvar
1,
*Elastic, dependencies=1
210000., 0.45, , 1.
1e+06, 0.45, , 10.
*User Defined Field

By a way it controls the interpolations in an element?

 

[Mustaine3]

Looks right. In the manuals are multiple examples.

Interpolation is done linearly between data lines. Spatial interpolation in an elements is not necessary, since the field variable is defined at an integration point, like the material data.

 

[dankoonFANTOMAS]

Alright thank you very much for your help

Have a nice day