Abaqus Subroutine to remove element after each increment 1

[iamoxygen]

Hello everyone,
I am writing a user subroutine in Abaqus to remove element that has reached damage criteria ( as a function of max principal stress and strain ). I knew how to use URDFIL to read data (stress/strain) in integration points of C3D element so I am wondering if there would be a way/routine to set state or status of failed elements in next increment to be deleted/deactivated. I am working with Abaqus/Standard.
Thank you very much.

 

[FEA way]

Element deletion can be controlled via UMAT subroutine. You just have to specify the number of state variable controlling this:
*DEPVAR, DELETE=variable_number

This is described in the "User-defined mechanical material behavior" chapter of the documentation (paragraph titled "Deleting elements from a mesh using state variables").

 

[iamoxygen]

Thank you. I found the tutorial to delete element using state variables with Abaqus/Explicit only. I want to remove element in the same way it does with *Model change option in the input file without developing material model by UMAT.

 

[FEA way]

If you don’t want to create UMAT there’s still an option to specify your own criterion for element deletion using (V)USDFLD subroutine. I know that VUSDFLD (Explicit) can do it (there’s even an example on github) but I think that USDFLD (Standard) will also work. At least in newer versions of Abaqus.

 

[iamoxygen]

I did a code with USDFLD and DEPVAR. I set state variable to control element deletion as 2. If criterion has reached, I set STATEV(2) as 0 to flag the material point to be deleted. But somehow the values of STATE(2) in my ODB file are not only "0" and "1".

 

[iamoxygen]

I want to get maximum principal strain, from Abaqus Document, which LEP. When I used GETVRM to get that value, I am not sure whether ARRAY(1)is the value I want.

 

[FEA way]

When it comes to the first issue (values of STATEV other than 0 and 1), I guess that you have something like that at the end of your code:

if (calculated_value > admissible_value) then
STATEV(2) = 0
end if

In such case you can try this:

if (calculated_value > admissible_value) then
STATEV(2) = 0
else
STATEV(2) = 1
end if

For the second problem (with GETVRM), if you request LEP in this utility routine you will get 3 values out of which ARRAY(3) will contain maximum principal stress (LEP3).

Could you share your subroutine’s code here ? It would be easier to provide further help.

 

[iamoxygen]

I am so thankful to your instant help. I alse found ordering of LE variables.
Here is my code
SUBROUTINE USDFLD(FIELD,STATEV,PNEWDT,DIRECT,T,CELENT,
* TIME,DTIME,CMNAME,ORNAME,NFIELD,NSTATV,NOEL,NPT,LAYER,
* 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),
* T(3,3),TIME(2)
DIMENSION ARRAY(15),JARRAY(15),JMAC(*),JMATYP(*),
* COORD(*)
open(unit=16,file='pvalue.dat',status='old')
!write(*,*) 'called now'
!write(6,*) 'called now'
!write(16,*) 'CALLED NOW'
C
! Absolute value of current strain:
CALL GETVRM('LEP',ARRAY,JARRAY,FLGRAY,JRCD,JMAC,JMATYP,MATLAYO,LACCFLA)
EPS = ABS(ARRAY(3))
! Maximum value of strain up to this point in time:
! CALL GETVRM('SDV',ARRAY,JARRAY,FLGRAY,JRCD,JMAC,JMATYP,MATLAYO,LACCFLA)
! EPSMAX = ARRAY(1)
! ! Use the maximum strain as a field variable
! FIELD(1) = MAX( EPS , EPSMAX )
! Store the maximum strain as a solution dependent state
! variable
FIELD(1)=EPS
STATEV(1) = FIELD(1)
IF (field(1). gt. 0.0195) THEN
IF (STATEV(2).NE.0) THEN
STATEV(2)=0
WRITE(16,*) 'ELEMENT ', NOEL, 'DELETED AFTER INCREMENT', KINC, '.'
END IF
END IF

! If error, write comment to .DAT file:
IF(JRCD.NE.0)THEN
WRITE(6,*) 'REQUEST ERROR IN USDFLD FOR ELEMENT NUMBER ',NOEL,'INTEGRATION POINT NUMBER ',NPT
END IF
C
RETURN
END

 

[FEA way]

I’m glad that I can help. And thanks for sharing your code. Does it work as expected after the changes ? Are elements properly deleted ?

 

[iamoxygen]

Yes, the elements has been deleted. I am simulating a tensile test of a specimen with Abaqus Standard. But when it has broken into 2 pieces, the solver cannot continue the next increment.

 

[FEA way]

Convergence difficulties might occur in Abaqus/Standard once the sample is broken into two pieces. Is it necessary for you to continue the analysis after it happens ? If it’s static analysis you can try with automatic stabilization in step settings. This may help.

 

[iamoxygen]

Even when a few elements have been deleted like this picture, the solver cannot continue. The plastic property of material is:
*Plastic
100.012, 0.
110.061, 0.00032
120.788, 0.00058
130.379, 0.00091
140.082, 0.00133
150.12, 0.00188
160.26, 0.00262
170.217, 0.00356
180.139, 0.00486
190.043, 0.00667
194.299, 0.00804
195, 0.3

 

[FEA way]

I’ve seen a similar issue in tensile test simulation with built-in damage criterion. Adding automatic stabilization in step settings helped the analysis go further, up to the point where fracture propagated through the entire cross-section. This I think that this is the best option in your case as well. Just make sure that it doesn’t affect the results significantly.

 

[iamoxygen]

I am quite new to that option. I see 2 sub-options (energy fraction, damping ratio) in Step Edit Dialog. Can you suggest me which option I should use?

 

[FEA way]

In most cases I use the default one:

Specify dissipated energy fraction: 0.0002
Use adaptive stabilization with max. ratio of stabilization to strain energy: 0.05

In keywords this is:

*Static, stabilize=0.0002, allsdtol=0.05

But *Static, stabilize will provide the same effect.

You can adjust the parameters if it turns out that the default ones are not sufficient but it’s rarely necessary to do it.

 

[iamoxygen]

Oh yes, thank you so much. I've got this after adding the keyword. You can see in picture focusing on blue mark, 2 brick elements now sharing one node so they will be highly distorted in next increment.