Symmetrical material and loading but shearing not zero?

[K.Li]

Dear FEAP users,

I am testing a new material model under uniaxial extension. My model geometry is 20 by 5 by 1 where 20 is the length in 1 (axial) direction, 5 being the width in 2 direction and 1 is the thickness in 3 direction. My material model and loading conditions are symmetric about 1-2 plane and 1-3 plane. So I don't expect any shearing on 1-3 plane. At the beginning of the analysis, all the non-diagonal terms of deformation gradient F is about 1E-15, then they increase gradually to 1E-14, 1E-13,......1E-8, 1E-3 ....  until I got a Residual norm error. I wonder if this is because something wrong with my material tangent stiffness matrix?  Or the material model itself could cause this non-stable behavior? Thank you!

[Prof. R.L. Taylor]

If the deformation is such that there is no shearing distortion anywhere then the off-diagonals should remain small.  What happens to the diagonal elements in your model? 

The issue is hard to diagnose from your verbal description. 

1. What is the convergence in each load step?  Does the residual converge to zero quickly?

2. Is the problem you are solving stable (are all rigid body modes restrained, is the element quadrature order high enough)?

3. Are the history variables updated correctly when the TIME command is issued?  Do a one element test and look at the values in the "H    " array (SHOW DICT will tell you how big the array is -- make sure you are storing all the values and they seem correct between each quadrature point).

We can test some if you post your input file and any material modules you developed.

[K.Li]

Thank you for your quick reply, Prof Taylor! At first, the diagonal terms of F are seems correct in the beginning. Then they got unreasonable towards the point when the analysis aborted. This might be caused by the non-diagonal terms.

1. At each step, it does converge to zero, but the convergence rate is linear. For example, after 7 Newton loops, the residual norm reaches to 1E-7, energy norm got to 1E-14.

2. The problem should be well-posed, and the element did work well with other material models. I am not sure about the details of the element. Can we check the order of the element?

3. For this material, we don't have any user-defined history variables. I used the "show dict" command after running a one element test with a set of material parameters which works (it does work with some parameters), and I found that the length of the "H" array is 4, and  parcn of "H" array is 2, array number is 49. I am not sure how to check the system history variables. I tried "show H", it outputs "Terms in array H     are zero". Does this mean no history variables were passed between the load steps? 
 

[Prof. R.L. Taylor]

If you do not have history variables then your model must be elastic(?) and depend only on the current deformation gradient F. 

If convergence is linear, your tangent is not consistent with your stress evaluation.  Be sure you are computing values related to Cauchy stress if you are using the FEAP standard elements.

Can you describe your model (or post your user function) so I have more information.

[K.Li]

Thank you, Prof Taylor! Yes, we assume the material is elastic. I am not sure why the material tangent is not consistent with the stress evaluation. Is there a way to check it? How could I make it consistent? I have computed Cauchy stress and material tangent tensors in a similar method as the micro-sphere model from Prof Govindjee 's website at http://www.ce.berkeley.edu/~sanjay/FEAP/Website/index.htm. 

We are using our own element. I tried to use the Solid element in FEAP with mixed and finite options, then all components of deformation gradient F become NaN after the initial step in which F is identity tensor.  I am not sure why?

Our material model is incompressible composite with a matrix material reinforced by fibers. Fibers are embedded in the matrix material. The fibers are not aligned in one direction, but they are distributed in planar fashion around a mean direction, for example, in 1-2 plane. Then we stretch the sample in 1 direction. The mean direction could be oriented in a general direction, not necessarily in the 1 direction. We do expect shearing in the 1-2 plane if mean fiber direction is not in the 1 direction. But if the mean fiber direction is in the 1-direction and all the fibers are distributed symmetrically on both sides of 1-direction (in-plane), then there should be no shearing in 1-2 plane, and the deformation is homogeneous. Our problem now is the case when the mean fiber direction is not aligned in the loading 1-direction. So the deformation becomes non-homogeneous.

[Prof. R.L. Taylor]

1. Please describe your formulation for the element -- when you say incompressible with fibers, how are you treating it?

2. You can use a "complex step" algorithm to compute the tangent matrix from the expression for stress -- Google to find references.

3. Adding fibers to an (or even nearly) incompressible matrix may require a very special element formulation -- I am not aware of any reference, but welcome one if you (or anyone) know of it.

[K.Li]

Thank you for your information, Prof Taylor!  I have switched to FEAP built-in 3D solid element (there was a interface problem, now I can use the built-in element). We used the decoupled form of strain energy, one for volumetric part, and  the other part is the isochoric contribution. I am using the augmented Lagrange method in FEAP to enforce incompressiblity. So after I calculate  the Cauchy stress and material tangent tensors, I think FEAP takes them and does further computation in fld3d1.f routine. But I am not sure which one is  the final material tangent matrix? Is  s(:,:) the final spatial tangent tensor?  If I have that, then can I validate my Cauchy stress calculation by using the final spatial tangent tensor and left Cauchy-Green deformation tensor  b = F F^{T}?