Varying Yield Strength through depth in Abaqus

Hello,





below is a collection of discussion threads that have appeared in the Yahoo ABAQUS list.



Also:



1) get this PhD thesis:



DYNAMIC STRESS INTENSITY FACTORS

FOR HOMOGENEOUS AND NONHOMOGENEOUS MATERIALS

USING THE INTERACTION INTEGRAL METHOD

BY

SEONG HYEOK SONG

THESIS

Submitted in partial fulfillment of the requirements

for the degree of Master of Science in Civil Engineering

in the Graduate College of the

University of Illinois at Urbana-Champaign, 2003





The code appears also in

Buttlar, W., Paulino, G., and Song, S. (2006). ”Application of Graded Finite Elements for Asphalt Pavements.” J. Eng. Mech., 132(3), 240–249.

Application of Graded Finite Elements for Asphalt Pavements



2) http://www.imechanica.org/node/9485



Regards



Frank



###########################################################################################################################



Hi All

 

As a first time to apply user subroutines, I wrote a user subroutine UMAT to define Young's modulus as a function of the vertical coordinate. , The subroutine is attached and also enclosed below. I tried to run a job and use it but I got a linking error. The error message is as follows:

 

Error in job Job-1: Problem during linking - Abaqus/Standard User Subroutines.   This error may be due to a mismatch in the Abaqus user subroutine arguments.   These arguments sometimes change from release to release, so user subroutines   used with a previous version of Abaqus may need to be adjusted.

 

Do you have some idea about how can I overcome that linking error? Is there any error in the subroutine?

 

Best wishes

Yasser

======================

 

SUBROUTINE UMAT(STRESS,STATEV,DDSDDE,SSE,SPD,SCD,

1 RPL,DDSDDT,DRPLDE,DRPLDT,

2 STRAN,DSTRAN,TIME,DTIME,TEMP,DTEMP,PREDEF,DPRED,CMNAME,

3 NDI,NSHR,NTENS,NSTATV,PROPS,NPROPS,COORDS,DROT,PNEWDT,

4 CELENT,DFGRD0,DFGRD1,NOEL,NPT,LAYER,KSPT,KSTEP,KINC)

C

INCLUDE 'ABA_PARAM.INC'

C

CHARACTER*80 CMNAME

DIMENSION STRESS(NTENS),STATEV(NSTATV),

1 DDSDDE(NTENS,NTENS),DDSDDT(NTENS),DRPLDE(NTENS),

2 STRAN(NTENS),DSTRAN(NTENS),TIME(2),PREDEF(1),DPRED(1),

3 PROPS(NPROPS),COORDS(3),DROT(3,3),DFGRD0(3,3),DFGRD1(3,3)



 

PROPS(1) = 100.*COORD(2)

PROPS(2) = .3



DO K1=1,NTENS

DO K2=1,NTENS

DDSDDE(K2,K1) = 0.

END DO

END DO

C

young = PROPS(1)

poiss = PROPS(2)

c

c elasticity matrix for plane stress case

c

const = young/(1.-poiss*poiss)

DDSDDE(1,1) = const

DDSDDE(2,2) = const

DDSDDE(1,2) = const*poiss

DDSDDE(2,1) = const*poiss

DDSDDE(3,3) = (1.-poiss)*const/2.

RETURN

END

 



----------



SUBROUTINE UMAT(STRESS,STATEV,DDSDDE,SSE,SPD,SCD,

1 RPL,DDSDDT,DRPLDE,DRPLDT,

2 STRAN,DSTRAN,TIME,DTIME,TEMP,DTEMP,PREDEF,DPRED,CMNAME,

3 NDI,NSHR,NTENS,NSTATV,PROPS,NPROPS,COORDS,DROT,PNEWDT,

4 CELENT,DFGRD0,DFGRD1,NOEL,NPT,LAYER,KSPT,KSTEP,KINC)

C

INCLUDE 'ABA_PARAM.INC'

C

CHARACTER*80 CMNAME

DIMENSION STRESS(NTENS),STATEV(NSTATV),

1 DDSDDE(NTENS,NTENS),DDSDDT(NTENS),DRPLDE(NTENS),

2 STRAN(NTENS),DSTRAN(NTENS),TIME(2),PREDEF(1),DPRED(1),

3 PROPS(NPROPS),COORDS(3),DROT(3,3),DFGRD0(3,3),DFGRD1(3,3)





C open (unit=1, form='unformatted')



C DIMENSION DSTRES(6),D(3,3)



PROPS(1) = 100.*COORD(2)

PROPS(2) = .3





DO K1=1,NTENS

DO K2=1,NTENS

DDSDDE(K2,K1) = 0.

END DO

END DO

C

young = PROPS(1)

poiss = PROPS(2)

c

c elasticity matrix for plane stress case

c

const = young/(1.-poiss*poiss)

DDSDDE(1,1) = const

DDSDDE(2,2) = const

DDSDDE(1,2) = const*poiss

DDSDDE(2,1) = const*poiss

DDSDDE(3,3) = (1.-poiss)*const/2.



C WRITE(1,*) NOEL,NPT,PROPS(1),PROPS(2)



C CLOSE(1)



RETURN

END



########################################################################################################



Changing material property over coordinates



You should be able to define your elastic modulus values as a tabular

function of a field variable (set the number of field variables to "1"

when defining an elastic material in the "Edit Material" dialog box).

In this case, the field variable value will correspond to your

Y-coordinate. Unfortunately, ABAQUS/CAE doesn't currently support the

definition of predefined field variables (even though it has tools to

define discrete and analytical fields which can be used in interaction

and load definitions). So, you'll need to edit the input file to add a

*INITIAL CONDITIONS,TYPE=FIELD,VARIABLE=1 section and/or a

*FIELD,VARIABLE=1 section to actually define the field variable values.

Alternatively, you can use the UFIELD subroutine (this might actually

be easier, since the coordinates of the nodes are passed into the

subroutine, and all you'll have to do is set FIELD(NSECPT,1) = COORDS(2)).



Regards,

Dave



-------------------------

Dave Lindeman

Lead Research Specialist

3M Company

3M Center 235-3F-08

St. Paul, MN 55144

651-733-6383



S.M.Ali Tasaloti wrote:

>

>

> Hello to all,

> Maybe my question is easy but I didn't find any answer for it. I want

> for example to change the young modulus of material linearly over

> y-coordinate of the 2D model. My specific question is about clay

> plasticity which I want to change the intercept over y-coordinate.

> How can I do so?

>

> Your help is kindly appreciatd.

>

> tnx

>

> S.M.Ali Tasalloti

>



###############################################################################################





------------------------------------------
Ruhr-University
Bochum
Germany