Help on ABAQUS UMAT subroutine

[biomechanics]

Hi all,

I plan to use UMAT to do some simulations on soft tissue. Since I do not have experiences on this, I hope to find some example UMAT code to start with, especially on the typical hyperelastic models. I searched from google.com, but can not find useful information. Is there any resource on UMAT fortran code for downloading? Thank you very much.

SIncerely,
Derek

[Jorgen]

Hello Derek,

I agree, in order to accurately simulate a soft tissue using ABAQUS you probably want to use a UMAT. If you are only interested in using a hyperelastic model, and want to write your own, then you should not use a umat but a uhyper subroutine. Uhyper subroutines are much easier to write than umat subroutines, but at the same time are much less accurate for simulating soft tissue.

As you noticed, there are not many freely available UMATs that can be found on the web. I have published the code of a VUMAT for a hyperelastic material in the downloads section, but again, hyperelastic materials are typically not very accurate for soft tissue.

The first question that that I think you need to decide on is what material model that you want to use. What type of tissue are you interested in? What are the strain levels? Do you have experimental data for the tissue? How accurate do you need your simualtions to be? How much time and money are you willing to spend on getting accurate simulations? All of these questions will help you decide the best approach.

If you have any questions, I would be more than happy to help.
Jorgen

[Emanuele]

I'm a PhD student at the University of Padua (Itlay) and I'm interested in soft tissue mechanics.
I have developed some UMAT subroutines in order to simulate the instantaneous and time-delayed mechanical response of periodontal ligament and tendons. More precisely I have developed respectively an anisotropic hyperelasto-damage constitutive model and an anisotropic Visco-Hyperelastic constitutive model. The main difficulties I have encountered in order to obtain good convergence rate are many.
First of all I had problems with the tangent moduli matrix; finally I discovered that the correct one must be founded on the Jauman formulation (see Belytschko for more details or ask me for).
Anyway, now I have really big convergence problems in the case of big strains (50% or more), especially in the case of shear states. Probably, the problem is not due to my subroutines, because I have encountered the same problems using the Hyperelastic constitutive models pre-implemented in the ABQUS code and I think they are due to the really low stiffness which characterize soft tissues.

Can anyone help me with these convergence problems?

Thank You

Sincerely, Emanuele

P.S.: sorry for my really bad English!!!

[Jorgen]

It sounds like you are making good progress on developing models for ligaments and tendons. I am curious about your models, have they been published yet :?:

As you noticed, it can be very challenging to derive the Jacobian (tangent modulus matrix). I have had good experience using approximate Jacobians in implicit simulations.

You should be able to get reasonably good convergence properties also in simple shear. You can perhaps try your subroutines by using a higher shear modulus. That way you know if it is the low modulus that causes the problem. If that does not work, then you probably have not implemented the rotational aspects of the constitutive model correctly, or the model by design might be unstable. To test these things you might also want to create a 1-dimensional solution of your material model, implemented for example in matlab or mathematica.

[Emanuele]

I have made really a lot of tests, obtaining good convergence rate simply incrementing the extracellular-matrix stiffness.
With low stiffness moduli I have found convergence problems also with the Mooney-Rivlin Hyperelastic constitutive model pre-implemented in ABAQUS.

As Limbert underlined, the correct tangent moduli matrix would have to be based on the Jauman stress rate.

Yes, I have already published something about the Hyperelasto-damge constitutive model:

A.N. Natali, P.G. Pavan, E.L. Carniel, C. Dorow, "A Transversally Isotropic Elasto-damage Constitutive Model for the Periodontal Ligament", Computer Methods in Biomechanics and Biomedical Engineering, Vol. 6, pp. 329-336, 2003

Here you can find few mathematical aspects. A fully mathematical version of the model will be presented in a future paper (I'm writing it now).

A paper about the visco-hyperelastic constitutive model has been submitted to the Journal of Connective Tissue Research.

Bye, Emanuele

[Jorgen]

I am surprised by your convergence problems. I have done tons of UMAT simulations and very rarely get convergence problems. As you probably know, the Mooney-Rivlin model is not unconditionally stable. Depending on how you choose the material parameters you might get unstable behavior at large strains (i.e. the model is not drucker's stable).

[biomechanics]

Hi,

I am surprised there are already some replies followed my post. Glad to see you here.

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.

I am simulating human anorectal system, focusing the behavior of smooth and skeletal sphincters. UHYPER is not suitable for my case. My constitutive relations are based on my experimental data. Also, I need to include fiber-generated active contraction force, which is dependent on several factors.

Even though I already wrote my UMAT code, I still hope to see the code of others for comparison, to check whether my method, such as treating on incompressibility.

[Jorgen]

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.

[Armin]

Hi Jorgen, hi Emanuele,

could your convergence difficulties be an issue of using Jauman rates :?:
May be I'm 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 don't understand why ABAQUS uses this rates. I think there a better choices.
I would appreciate your comments..

Armin

[Jorgen]

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 don't 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 :?

[stableguru]

Hello all,

I am new to the board and couldn't 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 "hybrid"elements? 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

[Jorgen]

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 Huang's book "Continuum Theory of Plasticity" on pages 242 - 244.

Thanks,
Jorgen

[Wei]

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

[salamati]

Hi all
I am using ABAQUS UMAT subroutine for modelling plasticity, considering small strains but large rotations.
Now, my question is that in UMAT subroutine, which DDSDE I should report to the software, Since I have two options:
1- DDSDE as a tangent matrix between corotational stress and strain
2- DDSDE as a tangent matrix between Cauchy stress and Rate of deformation.
In reality my question is that, Does ABAQUS umat subroutines need spatial or corotational tangent matrix?
I'm using STRAn and DSTRAN as input to the subroutine and also I rotate the STATV by DROT, but finally I dont know that I should rotate my tangent matrix or not. Can somene help me to know that, which DDSDE I should report to ABAQUS?
1- d(sig)_corotational = DDSDE1 d(eps)_corotational
2- d(sig) = DDSDE d(eps).

As you know d(sig)_corotational = DROT d(sig) DROT';

Thanks in advance

Salamati

[Jorgen]

I typically don't use STRAN and DSTRAN in my UMATs, instead I use the deformation gradient.

I recommend that you simply try both for a case with large rotations and see which works better for your model implementation.

-Jorgen

[salamati]

Hi Jorgen
Thanks for your comment.
That's a good idea. I will check it and let you know the result.

Regards
salamati

[Hcham]

hello, Im implimenting a model of anisotropic damage, I made a success of the isotropic one, but does that it give me only zeros I do not know what the problem:confused:? I tried all that I could but not good news.and I obtain the same result if I consider only the elastic case
present I have ask of the assistance, and thank you in advance.

[Jorgen]

Do you have any specific questions??

-Jorgen

[ribh]

Hi, I am trying to model fracture behavior of NiTi, Shape Memory Alloy using UMAT subroutine. Can you please help me on this?

[Jorgen]

You should post your question in a new thread :eek:

Also, I am not sure what you are looking for. Can you explain more?

-Jorgen