View Full Version : deformation gradient vs stran
I am trying to write UMAT for BAP model and the model is in terms of F.
But what I observed was that DFGRD0 and DFGRD1 give an arbitraily high value (1072693248 0 0;0 0 0;0 0 1072693248) for every iteration. There seems to me no relation between DSTRAN values and DFGRD. Am I not using the correct command for obtaining deformation gradient? Can anyone help me out on this?
Thanks in advance
I have written many UMATS using DFGRD0 and DFGRD1 and you should not get those strange values.
Are you sure that you printed the values correctly? The values that you mentioned look like large integers, when in fact they should be floating point numbers.
I used CPE4 element for my purpose; could that be a problem as I just read
The deformation gradient is available for solid (continuum) elements, membranes, and finite-strain shells (S3/S3R, S4, S4R, SAXs, and SAXAs). It is not available for beams or small-strain shells.
And as you are the best person to answer this, is Boyce model available in ABAQUS by itself? I need to simulate 2d orthogonal cutting of Polycarbonate, and for that purpose I am following her 1988 paper. But just today I was told that a variation of Boyce model (Bergstrom and Boyce) is available in ABAQUS. I also need to use a simple elastic model in conjunction with this one as my job consists of teo types of materials. Do I need to write a separate UMAT for both or can I use some inbuilt
Oh yeah, you are right. The deformation gradients are not available for small strain shells.
The Boyce model from 1988 is not available in ABAQUS. The Bergstrom-Boyce model (1998, 2001) is available through the *Hysteresis command. The *Hysteresis model is mostly useful for elastomer-like materials. As an option, I have implemented the Boyce model and a number of other models for thermoplastics. These models are commercially available (http://www.polymerfem.com/modules.php?name=User_Subroutines).
I went through your papers and all other papers by Boyce as well, and what I think is perhaps your model is not best applicable to Polycarbonate. Am I correct in saying this, coz i see it being implemented for chloroprene rubber and similar elastomers.
One other question I had was, if I want to consider only sigma(11,12,21,22) in my implementation and still want to use Def. Grad., how to go about it? Which element to use keeping in mind that I have coded UMAT for these four stress components only and that stress is a function of ln(Fe).
One way out I could think of is by assuming STRAN=ln(F) and getting F in that way. Is this correct to any approximation??
I think in small strain, you can assume no rotation, therefore the relationship between F and strain would be straightforward. however, in large strain the strain abaqus gives to UMAT is already after rotation, thus you can not derive F from strain. you can search abaqus answers for how to use F in UMAT with hyperelastic materials.
:arrow: I agree with hhspiny that in general you cannot obtain the deformation gradient from the strain tensor.
:arrow: I would not use the Bergstrom-Boyce (1998, 2001) model for polycarbonate (PC). There are other much more accurate models for PC.
:arrow: You say that you are only interested in Sigma(11,12,21,22). Does that mean that you are simply interested in plane stress? or perhaps plane strain? I would use an element type that is consistent with the problem that you are working with (i.e. plane stress, plane stress, shell, etc.)
Powered by vBulletin® Version 4.2.0 Copyright © 2013 vBulletin Solutions, Inc. All rights reserved.