Search
Close this search box.
Notifications
Clear all

Help on ABAQUS UMAT subroutine

21 Posts
10 Users
0 Reactions
2,276 Views
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

I also have above convergence. Tis kind of problem also occurs when I simulate contact between soft tissue and rigid body, such as cathater inserted into human body. My test showed that it was the low stiffness of tissue that cause divergence. The force equilibrium can not be reached, with increment decreasing to smaller and smaller....., not tolerable.

As you have noticed, contact is one of the most difficult aspects of finite element simulations, you often get convergence problems if you are not careful. There are some tricks that experienced simulators used to simplify contact. One approach that sometimes helps is to make sure the two bodies are in contact at the begining of the simulations, another approach is to use an explicit simulations.

Reply
Posts: 10
 Jay
(@Jay)
Active Member
Joined: 17 years ago

Jauman rate

Hi Jorgen, hi Emanuele,

could your convergence difficulties be an issue of using Jauman rates ❓

May be Im wrong, but as far as I remember the Jauman rate shows some kind of oscillating behavior for shear deformation. I think an analytical solution for a simple shear test exists which shows exactly this ❗ Could that be an issue ❓

I dont understand why ABAQUS uses this rates. I think there a better choices.

I would appreciate your comments..

Armin

Reply
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

I agree, the convergence problem can be caused by Jauman rates and large shear. To check this you can perform simulations of uniaxial loading, clearly there should be not issues with rotation in uniaxial loading. If you dont get good convergence in uniaxial loading then it is more likely that either the material model or the implementation of the model is unstable.

It is certainly not trivial to write a stable UMAT for any FE program 😕

Reply
Posts: 1
(@popsin)
New Member
Joined: 17 years ago

Convergence

Hello all,

I am new to the board and couldnt help post my 2 cents on this issue 🙂 ...actually I have asuggestion from my experiences and some questions too...I work on anisotropic hyper-visco-elasticity and have implemented a umat subroutine in ABAQUS. However I have the some problems with convergence in some modes.

From what I understand convergence problems arise mainly due to

1) Loss of ellipticity in some deformation states. As Jorgen pointed out the mooney rivlin is not unconditionally stable. For example for an invariant based anisotropic model if you contract it in the fiber directions the model may lose ellipticity. One way of overcoming this is by making sure that the anisotropic part model does not take load in compression.. however this is not very consistent with themodynamic assumptions. Another way is to construct polyconvex functions which are always stable(papers by Ball prove this..or ref to Marsden and Hughes or Antman). I do it the first way since construction of polyconvex functions with good initial conditions is not very simple (however there are papers by neff and schroeder which detail this construction for anisotropy)

2) Near incompressiblity has to be modelled thru a 3 feild variational principle like the Hu-Washizu principle(or use reduced integration techniques). Actually my question pertains to this since I have not worked in abaqus before. Does abaqus implement this well with their so called hybridelements? Or should I code the formulation explicitly in my umat subroutine?

3) Could anyone point me to the references on Jaumann rates and shear instability since I suspect that might be my problem?

Would be glad if someone could help me out on these.

Thanks

NV

Reply
Posts: 3998
(@jorgen)
Member
Joined: 5 years ago

Interesting comments. I am starting to work on anisotropic visco-hyperelasticity as well. Do you have any references to your own work? Also, how do you make sure the model does not take load in compression?

My experience is that the hybrid elements that are available in ABAQUS work well. I have not had any problems that would require a user element or other subroutine reformulation.

Finally, there is a good discussion about Jaumann rates and the shear instability in Kahn and Huangs book Continuum Theory of Plasticity on pages 242 - 244.

Thanks,

Jorgen

Reply
Posts: 8
 amar
(@amar)
Active Member
Joined: 17 years ago

Hi All:

Here is my 2 cents on the convergence issues:

1) As Stablguru mentioned, strain energy function needs to satisfy the ellipticity condition, it is essential for material stability.

2) Condition number of stiffness matrix, high condition number will cause difficulty in the inverse of stiffness matrix and I guess it will also lead to slower convergence rate, which may require more iterations than ABAQUS allows. For soft tissue, this may be more relevant as the bulk modulus is much higher than shear modulus due the incompressibility.

3) For low stiffness strain region for soft tissue, my understanding is:

Collagenous tissues usually exhibits strain-stiffnessing J-shaped stress-strain curves, ie., an initial large extension is achieved with relatively low levels of stress. This low stiffness of the material at the low strain region could cause convergence problems in the iterations. Say, for a given load increment dF(n+1) at increment step n+1, the predicted displacement increment is dU(n+1)=K{-1}dF(n+1) , where K is the stiffness matrix. dU(n+1) could be large due to the low stiffness, and thus the total displacement U(n)+ dU(n+1) may be out off the stress-strain range encompassed by J shape curve, this will lead to the difficulty in calculating F(U(n)+dU(n+1)) from the constitutive law and cause the convergence problems.

4) I doubt UMAT can handle the mixed formulation, wonder if anyone has successfully done it

5)To check if fiber is under compression, what I did is to see if I4 or I6<1, if so then set Sfiber=0. Physically it makes sense, however, I wonder if it will make energy discontinuity and cause numerical problems.

Thanks,

Wei

Reply
Posts: 10
(@stasseb)
Active Member
Joined: 15 years ago

Fortran Compiler for ABAQUS 6.4

Hi,

I wanted to run a UMAT with ABAQUS 6.4. Can you please let me know what compiler should I be using for the same.

Thanks

Reply
Page 2 / 3
Share: