newbie question: strains in UMAT

[Ratatosk]

Hello,

I'm getting confused :? ..

What is the most convenient way to use strains ans strains increment in UMAT?

I'am modeling a large deformation biological tissue (intervertebral disc, annulus fibrosus for those who are bright in latin 8O ) and my material constitutive law is formulated in the Right Cauchy strain tensor, C. But for ABAQUS, I pushed it to the "true" Cauchy stress... and therefore my strain is the Left Cauchy strain tensor, B

Is it possible to have B from STRAN and the increment of B form DSTRAN, with this relation :

B=exp(2*STRAN) ? if STRAN is indeed the logarithmic strain, isn't it?

I have tried to formulate B with DEFGRD0 * DFGRD0^T but DFGRD0 is always nul?? :cry:

I use solid hybrid elements for a simple geometrie, and I believed that there was no problem in getting the deformation gradient? Am I doing something wrong?


Please Help!! :o

Arne

[Jorgen]

You should be able to calculate B from the deformation gradient. I do that in almost all my UMATs.

Your subroutine should never be fed a zero matrix for DFGRD0 or DFGRD1. If you get a zero matrix then something is very wrong, perhaps you are using wrong variable types (i.e. double precision instead of real, or vice versa)

I recommend that you print out the input variables that are fed into your UMAT and make sure that they are all OK.

Best of luck,
Jorgen

[Ratatosk]

Hello Jorgen,

As you suggested, I worked an empty UMAT with the header and footer of the file. The only commands was to print DFGRD0 and DFGRD1.

I found the bug. The mistake I did was to copy-paste the header ot a file which contained an O and not a 0 (zero) for DFGRD0!!! :lol:

So happy as ever, I continued my work.

but, it still doesn't work. I need some advices... :)

I am planning to implement a hyperviscous law for a soft tissu.

To simplify and to see if my potential converges to a solution, I wrote a UHYPER subroutine.. no problemo 8) , it converges!!!

Now, I want to implement the hyperelastic law in UMAT myself before integrating any viscous stuff :?

I need you to confirm my method.. as on paper I wrote in material configuration

S= 2*(W1 + I1*W2)* I - 2*W2*C

W1=W1(I1) and W2=cte

where W1 is dWdI1 and W2 is dWdI2, I suppose incompressibility.

Then the corresponding tangent tensor is

SS = 2*dSdC = 4*(W11 + W2)*[ I x I] - 4 * W2 * 1/2 *[ I _x I + I ^x I ]

where I is identity, W11 is dW1dI1 and the operators x , _x and ^x are diad, under diad and over diad.

then to spatialise it, I used the push-forward relation (J=1)

TT_ijkl = 1/J * F_ir *F_jm *F_kn *F_ls * SS_rmns

which gives, and now this is implemented :

:arrow: TT = 4*(W11 + W2) [ B x B] + 2*W2* [ invB _x invB + invB ^x invB]

where invB is the inverse matrice of B=DFGRD0*DFGRD0^T

:arrow: I convert this to a 6x6 symetric tensor => DDSDDE


Now for DSTRAN,

F0=DFGRD0
F1=DFGRD1

DF=F1 - F0

:arrow: DB=[ I _x F0 + F0 ^x I ] DF

:arrow: I convert this to a 6x1 vector => DSTRAN

then I update de STRESS with

:arrow: STRESS = STRESS + DDSDDE*DSTRAN

I hope I made my self clear enough, sorry if not :?

Do I have to include a lagrangian multiplier for the incompressibility, I did not since, at least I believe, the hybrid element adjust the principal values by themself...do they? Do I have to include J in the push-forward relation as it may numerically be not nul?

Thank you

Arne

P.S. sorry for my poor English

[Jorgen]

Hello Arne,

Your approach looks OK. I have two comments:

1. I would make the hyperelastic model compressible to avoid numerical problems.

2. If you still have problem making it work I would first add a bunch of print statements within your UMAT to make sure it works at you intendent. If that still does not solve your problem I would create a separate implementation of the UMAT in Matlab or some other mathematics software.

Best of luck,
Jorgen

[Ratatosk]

Hello Jorgen,

thank you for all your advices!! I found some errors, in the approach above. Infact I was surprised to find in an article of G. Limbert the term containing the inverse of B in the spatialised modulus.

I verified this and did not quite find the same terme, my modulus is

:arrow: T=2*(W11 + W2)*[ B x B ] + W2*[ B _x B + B ^x B ]

which appeared OK for me.

But this correction still didn't work, I then printed the original DSTRAN and the one calculated from DFGRD0 and DFGRD1

:arrow: mine is a factor of 2 greater !!! Do you know why?

:!: Dividing my calculated DSTRAN by 2 makes the solution to converge!!

This adaptation makes the calculated and the original DSTRAN equivelent wich is not so surprising.....:oops: why be so complicated..

But, it doesn't converge to the result using UHYPER which has the right solution!!

I may believe that this difference is due to the incompressibility...

What do you suggest? What kind of compressibility should I introduce? And how do I do this?

I have to give my final paper at the end of the week, so any suggestions would really be appreciated. Anyways I am very gratefull for your precious help as there is no information on the internet and even less in my school!!

lots of Thanks

Arne

[ashu28]

Hi!
I am realtively new to UMAT and am trying to write the file for a elastic-viscoplactic data. My model deals with the deformation gradient F but whatever UMAT files I have always take DSTRAN as the starting point. What I want is the F vector at any point of time from which I have to calculate F ealstic and F plastic. Can anyone please tell me whether ABAQUS gives deformation gradient vector and also whether the STRAN and DSTRAN are logarithmic strains or engineering strains?

Also I am a bit confused about when to use DROT or ROTSIG. My case deals with large deformations, so will i be required to rotate F using DROT before proceeding in the model calculations?

It would be great if someone can help me out in this.

Ashu

[hhspiny]

Abaqus only provides DSTRAIN/STRAIN into UMAT, since the rotation has already been processed before passed in, i.e., you don't need to do rotation yourself (double check manual please, it is just from my memory years back). large deformation STRAIN is always log strain in abaqus