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 :?