Hello,

Did you try to play with the different ANSYS plot options ? -> AVRES, AVPRIN commands for example.

In order to avoid side effects near material discontinuities, you can also use results on elements (PLESOL instead of PLNSOL).

Considering these discontinuities :

Let's consider a fixed-free beam, of constant section, made of two materials, with a traction displacement sollicitation.

First case, we have a "serial" mounting : the section is homogeneous, with one material on the first section, and a second material on the second section.

Second case, we have a "parallel" mounting" : the section is made of two materials, all along the beam length.

In the first case, you will have a continuous stress field (and even uniform) all along the beam structure. The strain field will be non continuous if the Young modulus are different in the tow materials.

In the second case, the strain field will be continuous (and even uniform) in the whole section, and all along the beam structure. And the stress field will be non continuous if the Young modulus are different in the tow materials.

You should think about this simple example in order to anticipate or to interpret correctly your results (with discontinuities or not, on stress or strain fields).

Your output is a result of FEM theory, which ensures only force equilibrium at nodes and displacement compatibility across adjacent elements, but not equilibrium of stress. Given a deformed mesh, the stress in a node changes depending on whether that node belongs to one element or to the adjacent one.

In addition, it seems that yor model has a geometrical singularity (zero notch radius), where the theoretical stress is clearly infinite (whilst the FE stress is finite, no matter how fine is the mesh).

Finally, it is not clear to me the purpose of your analysis and what result you expect from it.

Dear Timo, it depends of the stress component whether a discontinuity will appear or not. Consider two diffently stiff materials separated by a plane interface. Stress components perpendicluar to that plane must be continuous because of equilibrium. Stress components parallel to that plane must be discontinuous since the energetically conjugate strain components are equal on either side of the materials interface because of kinematics. The von Mises equivalent stresS is composed of all stress components so that the discontinuity of the perpendicular stress components shows in the equivalent stress. Thus, the discontinuity that you observe is real and not necessarily an artifact of the FEM or, particularly, ANSYS.

If the displacement vector is equal for both adjacent elements but the material not, each element will have a different Hook matrix [D], so the stress is different in each element

You can use subroutine in abaqus. it can be obtain. making stress linked with coords.