Below, I have shared pictures of a simple model in FEA. As it can be seen that the face onto which the fixed support is applied, there exists Von-Mises stresses. I cannot comprehend why. Since the nodal deformations are equal to zero there, but still there exists stresses. I am aware of the fact that there must be a transverse reaction force on that face due to poisson's ratio effect, but still why would I see stresses there. In reality, if a face of a solid body is extremely rigid because of how it is supported, should I still expect stresses on that face?
Deformations and stresses are different things. Stresses and strains are a function of the derivative of deformations, not the values. Consider a rod in tension, fixed at one end with a tension force applied to the other. The normal stress in every part of the rod is force over area. This is just as true for the fixed face as the other faces.
This has nothing to do with FEA implementation, or shape functions, or element types as the other answer says. You are getting stresses because the true elasticity answer has stresses in it.
Although the face of the element is rigid and does not move with respect to other points in the face, you are using a 3d element (a volumetric). Therefore while one face of the element is unstressed, the other faces are subjected to stresses. Therefore, the element is in a state of stress, despite one face of it being fixed and unstrained (like you've already mentioned you expect at least transverse stresses due to Poisson ratio).
Now there are two other things that are important.
- The representation you've chose is the Von Mises stress (the default)
Because the von Mises stress, considers the contribution of shear and normal stresses, you are expecting to see some non zero value of stress even if either the normal or the shear stresses are individually zero. If you select another representation (in this case radial/tangential stresses, then you would have a different picture).
- the way stress are interpolated in an element. (shape functions)
If you take a closer look at the image you uploaded, the shape of the contours is not the coincident with the element boundaries.
Essentially what happens (to spare details about an implementation I am not certain) is that in the most basic for FE, calculates properties for the element at the nodes, and then uses approximating functions (see shape functions) to interpolate what is happening in the other point. When you have a linear element (1d) things are relatively easy to grasp. However as you transverse the dimensions (2 and 3d) things can get difficult based on the element implementation you are using.
For example the simplest form of a 2d Element (used for shells) has a triangular form. In the simplest form (no intermediate integration points) the element has a constant strain (it is actually known as CST - Constant Strain Triangle). If you go to a 4-node surface element, then you can have a strain gradient. What is interesting to note, is that for those simple formulations the strain (and stress if you are using a linear solver) is not necessarily matching at the element boundaries with its adjacent elements (apart from the nodes).
Higher order elements use more sophisticated methods, and the result is the interpolating curves you see in the image above.
The elements with the fixed faces are stressed. The Von Mises stress is non zero when the element is in a state of stress. The software interpolates the values between the nodes with shape functions.