@ Qingqing Zhao:

Yeah. It seems that the "Recomputation Part" must be included. (See the comments above). However, there is a numerical instability in this code due to the instant reduction of the elastic modulus which can be solved by doing a gradual reduction of the elastic modulus in 10 steps. I strongly recommend to read the following reference completely. There are valuable comments in it which may be helpful for you.

Knight, N. F., Jr., User-Defined Material Model for Progressive Failure Analysis, NASA CR-2006-214526,December 2006.

I have checked the code for simple cases and it is working properly. No covergency issues are seen; however, in the case of notched plated the code diverges exactly before damage initiation!

The error is :

"Time increment required is less than minimum specified."

The minimum time increment is: 1e-8

when I remove the recomputation of the stiffness matrix and stress after damage initiation check in the code, everything seems fine and abaqus/standard converges!

(Please take a look at the "3DIsotropicElasticityVonMisesDamage, ImplicitNone.for".

Here is the part I meant:

C RECOMPUTE COMPONENTS OF STIFFNESS TENSOR

E=E*(1.D0-D)

LAMBDA=E*NU/((1.D0+NU)*(1.D0-2.D0*NU))

MU=E/(2.D0*(1.D0+NU))

CALL STIFFMAT(LAMBDA,MU,NTENS,DDSDDE)

C RECOMPUTE THE STRESS TENSOR

DO I=1, NTENS

STRESS(I)=0.D0

DO J=1, NTENS

STRESS(I)=STRESS(I)+DDSDDE(I,J)*UPSTRAN(J)

END DO

END DO

when I remove this part everthing is working, but I know that the recomputation is required, as it has been mentioned in the following reference:

Knight, N. F., Jr., User-Defined Material Model for Progressive Failure Analysis, NASA CR-2006-214526,

December 2006.

What is the correct definition of DDSDDE for the damaged material? Is it equal to the damaged stiffness matrix?

Do we have any UMAT code in ABAQUS relating to Progressive Failure Analysis on the net?

I recommend you to see, Abaqus documentation==>Examples book, 1.4.6 Failure of blunt notched fiber metal laminates. in this example you can find a .FOR file that can help you.

If you mean the attached file to this message, I have seen that before! :)

The code is too long and cumbersome! Also the criterion used there, is based on strains not stresses! :)

Hi Hosein, have you solved your problem?

@ Qingqing Zhao:

Yeah. It seems that the "Recomputation Part" must be included. (See the comments above). However, there is a numerical instability in this code due to the instant reduction of the elastic modulus which can be solved by doing a gradual reduction of the elastic modulus in 10 steps. I strongly recommend to read the following reference completely. There are valuable comments in it which may be helpful for you.

Knight, N. F., Jr., User-Defined Material Model for Progressive Failure Analysis, NASA CR-2006-214526,December 2006.

Hi Hosein, would you mind I ask you one question relating to UMAT validation. What validation tests have you performed? Just incorporated into your model and plot the curves to compare with experimental results or you first test on single element model. Thanks. 

You should do them both! :)

At the first step you may run the code with single element model for axial tension and pure shear. For these cases it is easy to predict the response so you can compare the response from the code with what is in your mind. In the next step you can increase the number of elements in the aforementioned cases to be sure about the code working correctly. The last step is the model verification which is implemented in the code . It can be achieved by comparing with experimental results.

Hi Hosein,

you should recovery the stresses for previous increment and update them with the increment strain of current increment with degraded stiffness matrix.

REPLACE:

DO I=1, NTENS

   STRESS(I)=0.D0

   DO J=1, NTENS

         STRESS(I)=STRESS(I)+DDSDDE(I,J)*UPSTRAN(J)

   END DO

END DO

with:

 DO K1=1,NTENS

        DO K2=1,NTENS

              STRESS(K2)= STRESS(K2)+DDSDDE(K2,K1)*DSTRAN(K1)

        ENDDO

ENDDO

Regards

I think the original code is correct @ Domenico De Rosa, since the secant modulus is used to model progressive damage. In which case, DDSDDE is the secant modulus (which is decreased to model the progressive material degradation), therefore, the full-scale constitutive equation instead of the incremental constitutive equation should be used.

In this problem, the damage takes place in one increment, where the damage parameter D changes from 0 to 0.99999 abruptly, which will cause numerical instability. I would propose several approaches that might solve the difficulty:

1. If applicable, the most straightforward way is to decrease the damage parameter from 0.99999 to a smaller value (e.g., 0.9 or 0.95), which will greatly facilitate convergence.

2. Instead of modeling the damage in one step, try to use a "real" progressive damage process. A simple model would be linear degradation. See following for example codes. Note that D increases from 0 to DMAX, when Mises stress increases from STRESS_INI to STRESS_FAL.

• IF (SMISES .GT. STRESS_FAL) THEN
• D_temp = DMAX
• ELSE IF ( (SMISES .GT. STRESS_INI) .AND. (SMISES .LT. STRESS_FAL)) THEN
• D_temp = DMAX * (SMISES -STRESS_INI) / (STRESS_FAL-STRESS_INI)
• ELSE
• D_temp = 0
• END IF
• IF (D_temp .GT. D) D=D_temp

3. Element type also have great influence, based on my personal experience, 2nd order elements help in some cases.

4. As discussed in the previous answers, you should start from validating the umat on one element then to more complex problems. But sometimes umat codes work on one element but fail for complex models, just like in this problem.

When modeling damage, convergence is so annoying that it often makes graduate students Crazy. Hope these suggestion will be helpful~