Hello Cathal,

Though you have made a mention of USDFLD in your message, I just wanted to check if you have tried to employ them as mentioned below. 

1) Define a dummy USDFLD subroutine and associate it with state variables.

2) From a USDFLD subroutine make a call to utility routine GETVRM to retrieve the desired stress values.

3) Store the stress values in state variables.

4) State variables are shared between USDFLD and creep user subroutines.

The stored stress values in USDFLD can be retrieved in the CREEP user subroutine.

This is the only approach I can think of. 

Hi Rajas,

Firstly, thank you for your reply. I have set up my subroutine .for file so that the USDFLD subroutine calls 'SP' using the GETVRM command and writes it to Field(1) and then sets Statev(2) =Field(1) . Once this section of the code completes, the CREEP subroutine begins where it calls in the Statev(2) which at this point should contain the required value of 'SP' (namely in this case the maximum principal stress). 

The analysis completes without any errors, however my Statev(2) has a value of 0 for the entire analysis. May I send you a copy of the subroutine for you to better understand the layout? 

Kind Regards

Cathal

You could try to exchange information between the routines using common blocks instead.

Hi all,

I've since discovered that when density is defined as part of the material properties in Abaqus, this error does not occur and the principal stress is defined correctly in the statev(2). Density isn't called in either of the subroutines in use, and I've never had to define it with any other job I've run.

The question now becomes: why does the inclusion of a mass density dependency effect the correct extraction of a principal stress within a user subroutine?

Martin, I have never used a set of common blocks but I will investigate the possibilities. Thank you for your response.

Dear Cathal,

If I understood well you are modeling creep damage using the *CREEP subroutine and you need principal stress to use it in the calculation of rupture stress, which is function of principal stress and von Mises stress. I attach here part of my script:

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

IF (KINC.EQ.1) THEN

FIELD(1) = 0.0

ELSEIF(STATEV(1)>=0.0) THEN

FIELD(1) = STATEV(1)

ELSE

FIELD(1) = 0.0

END IF

C --- get the maximum principal stress

CALL GETVRM('SP',ARRAY,JARRAY,FLGRAY,JRCD,JMAC,JMATYP,

1 MATLAYO,LACCFLA)

STATEV(2) = ( ABS( ARRAY(3) )+ ARRAY(3) ) / 2

C

RETURN

END

Hi all,

This issue has been resolved, the ordering of the subroutines within the .for file is extremely important. The USDFLD subroutine needed to be called prior to the creep subroutine.

Once the order of the subroutines was changed, the correct principal stress values were fed to the creep subroutine and the damage was calculated accurately.

Thanks to all who replied.