# How to Plot Stress Contours in Abaqus?

1) Under Visualization in Abaqus, contours for displacements-U1 and U2 are available. How could I generate contours for displacements in x-y direction, that is Ux and Uy? Similarly how can I get contours for stresses Sigma_x, Sigma_y and Sigma_xy?

2) To find homogenized elastic constants of a representative volume element of a fiber reinforced composite (that means to get homogenized E1,E2,E3,G12,G23,G13,v12,v23,v13), I need to find elastic constants of each element. I also need to get volume of each element. How can I get this two information (elastic constants and volume) for each element?

3) In Abaqus, in the representative volume element of fiber reinforced composite, fiber is aligned parallel to z axis. How could I rotate the axis so that the fiber would be aligned parallel to x axis? Noteworthy that I am modeling 2D planar problem.

(1) In Abaqus/CAE the stress at each integration point is given by the field variable $S$. Note that in Abaqus, like many or even most FE solvers, the stress computed is the Cauchy (true) stress. So, for a material with local material directions given by the Global basis: $\sigma_{x}=S_{11}$, $\sigma_{y}=S_{22}$, etc. You will need to make sure that stresses are being written to the ODB during the analysis to visualize them in CAE.

(2) This question is a bit more complicated. Generally, when talking about constitutive modeling the material parameters are independent of length scale. This is kinda the point of continuum scale modeling. If the material properties are varying spatially in your model you will need to either implement field variables or a user defined material (either a UMAT for Abaqus/Standard or a VUMAT for Abaqus/Explicit). I don't have any experience specifically with fiber reinforced composites in Abaqus, but the set of parameter you are describing in your question are for a general linear elastic, anisotropic material, which may or may not be able to describe the homogenized response of the material you are interested in. If that is the case, I know that it is possible to construct layered composites within Abaqus, but I can only point you to the Abaqus User Manual for more information. As for specific material constants, the best place to look is in the literature or, better yet, go run some experiments. This might not be the answer you are looking for, but each material is different. Given the anisotropy of the material you are going to want to look for data from multiple loading configurations.

I'm also not quite sure why you would need the volume for each element, but if your structure can be meshed uniformly them it might be possible to calculate element volumes prior to the analysis. If your mesh is irregular the answer is a bit more complicated. One possible solution I can think of is extracting integration point coordinates within the UMAT framework for each element, then based on all the integration points for the element determine the element nodal coordinates based on the associated quadrature rules. Another possibility is to look at the input file (.inp) and determine the nodal coordinates for each element, using them to calculate the element volumes.

(3) You can assign local material orientations in the Property menu of CAE. The symbol looks like a yellow L with red axes. Within the Material Orientation menu you can create local directions based on any coordinate system. In the Definition drop down select Coordinate system, then in the CSYS option create a new coordinate system. This can be down by clicking the coordinate system icon.

In a 2d abaqus analysis you can only rotate the material orientation in-plane, in other words you can not "transform" the material 3- direction into the plane of the analysis. (Which seems to be what you are asking in #3)

The only solution to this problem is to "manually" transform the material definition, i.e. reordering the values on the *Elastic,ENGINEERING CONSTANTS line. (and i'm sure you know the poisson ratios are not symmetric, so its not quite a trivial reordering)

to #2 You can request element volume as an output field variable, EVOL

• +1. As one of this site's top users in the Abaqus tag, I wonder if you've seen this question and/or if you might know the answer to it? mattermodeling.stackexchange.com/q/2055/5 Commented Nov 14, 2020 at 3:33