Out put variables while using VUSDFLD

[Davidz]

Hi,

I am studying the sample of VUSDFLD of ABAQUS user subroutine reference manual.
I tried to output variables like props and stateNew while debugging using "ABAQUS job=sample user=vusdfld.for interactive" in ABAQUS command.
But the output is weird. For example, "props" which indicates modulus in the sample, constantly equals zero.

Thanks!
DavidZ



Output:

.................
 nprops=   173011416
 stateNew=  3.9973736E-02
 props=  0.0000000E+00
 nprops=   173112296
 stateNew=  3.9980490E-02
 props=  0.0000000E+00
 nprops=   173011416
 stateNew=  3.9987233E-02
 props=  0.0000000E+00
...............

altered sample subroutine:

      subroutine vusdfld(
c Read only -
     *   nblock, nstatev, nfieldv, nprops, ndir, nshr, 
     *   jElem, kIntPt, kLayer, kSecPt, 
     *   stepTime, totalTime, dt, cmname, 
     *   coordMp, direct, T, charLength, props, 
     *   stateOld, 
c Write only -
     *   stateNew, field )
c
      include 'vaba_param.inc'
c
      dimension jElem(nblock), coordMp(nblock,*), 
     *          direct(nblock,3,3), T(nblock,3,3), 
     *          charLength(nblock), props(nprops), 
     *          stateOld(nblock,nstatev), 
     *          stateNew(nblock,nstatev),
     *          field(nblock,nfieldv)
      character*80 cmname
c
c     Local arrays from vgetvrm are dimensioned to 
c     maximum block size (maxblk)
c
      parameter( nrData=6 )
      character*3 cData(maxblk*nrData)
      dimension rData(maxblk*nrData), jData(maxblk*nrData)
c      READ(*,*), rData
c
      jStatus = 1
      call vgetvrm( 'LE', rData, jData, cData, jStatus )
c
      if( jStatus .ne. 0 ) then
         call xplb_abqerr(-2,'Utility routine VGETVRM '//
     *      'failed to get variable.',0,zero,' ')
         call xplb_exit
      end if
c
      call setField( nblock, nstatev, nfieldv, nrData, 
     *   rData, stateOld, stateNew, field)
c
      return
      end
      subroutine setField( nblock, nstatev, nfieldv, nrData, 
     *   strain, stateOld, stateNew, field )
c
      include 'vaba_param.inc'
c
      dimension stateOld(nblock,nstatev), 
     *   stateNew(nblock,nstatev),
     *   field(nblock,nfieldv), strain(nblock,nrData)
c      Read(*,*), stateOld 
c
      do k = 1, nblock
c
c     Absolute value of current strain:
         eps = abs( strain(k,1) )
c
c     Maximum value of strain up to this point in time:
         epsmax = stateOld(k,1)
c
c     Use the maximum strain as a field variable
         field(k,1) = max( eps, epsmax )
c
c     Store the maximum strain as a solution dependent state 
         stateNew(k,1) = field(k,1)
      print *,'nprops=', nprops 
      print *,'stateNew=', stateNew(k,1)
      print *,'props=', props
      end do
c
      return
      end

INP

*HEADING
 Damaged elasticity model with user subroutine vusdfld
*ELEMENT, TYPE=T2D2, ELSET=ONE
1, 1, 2
*NODE, NSET=NALL
   1,  0., 0.
   2, 10., 0.
*SOLID SECTION, ELSET=ONE, MATERIAL=ELASTIC
1.
*MATERIAL, NAME=ELASTIC
*ELASTIC, DEPENDENCIES=1
** Table of modulus values decreasing as a function
** of field variable 1.
2000., 0.3, 0., 0.00
1500., 0.3, 0., 0.01
1200., 0.3, 0., 0.02
1000., 0.3, 0., 0.04
*DENSITY
1.0e-6
*USER DEFINED FIELD
*DEPVAR
1
1,EPSMAX,"Maximum strain value"
*BOUNDARY
1, 1, 2
2, 2
*AMPLITUDE, NAME=LOAD1
0.0, 0.0, 1.0, 1.0
*AMPLITUDE, NAME=LOAD2
0.0, 0.0, 2.0, 1.0
*AMPLITUDE, NAME=UNLOAD
0.0, 1.0, 1.0, 0.0
*STEP, NLGEOM=NO
*DYNAMIC, EXPLICIT
 , 1.0
*CLOAD, AMPLITUDE=LOAD1
2, 1, 20.
*OUTPUT, FIELD, VARIABLE=PRESELECT
*OUTPUT, HISTORY, VARIABLE=PRESELECT
*ELEMENT OUTPUT, ELSET=ONE
S, E, SDV
*NODE OUTPUT, NSET=NALL
RF, CF, U
*END STEP
*STEP, NLGEOM=NO
*DYNAMIC, EXPLICIT
, 1.0
*CLOAD, AMPLITUDE=UNLOAD
2, 1, 20.
*END STEP
*STEP, NLGEOM=NO
*DYNAMIC, EXPLICIT
 , 2.0
*CLOAD, AMPLITUDE=LOAD2
2, 1, 40.
*END STEP

[lumpwood]

You have two problems here. First, props isn't your value of Young's Modulus from the INP file. It is an array of material constants that is used with the VUMAT subroutine.

Second, you aren't passing nprop or the props array into the subroutine where your print statements are so naturally they will have no set value in there.

[Davidz]

You have two problems here. First, props isn't your value of Young's Modulus from the INP file. It is an array of material constants that is used with the VUMAT subroutine.

Second, you aren't passing nprop or the props array into the subroutine where your print statements are so naturally they will have no set value in there.

Thank you! Lumpwood.
Is there any way that I can output or check modulus for this sample?
(modulus decreases as a function of the maximum tensile strain)

[lumpwood]

Thank you! Lumpwood.
Is there any way that I can output or check modulus for this sample?
(modulus decreases as a function of the maximum tensile strain)

Yes, but not directly that I know of. You will know the field variable value, which can be requested as output for the ODB file and viewed as a contour plot. Abaqus will linearly interpolate the value of E based on the table of field variable dependencies in your INP file so you can use a simple interpolation to get E based on the field variable value.

[Davidz]

Thank you.
Modulus can be tracked by stress/strain. Curve of modulus consistent with the table of field variable dependencies in INP file.

Redards,
Davidz