Bill Bulat
Ansys Employee

I tested adjusting number of cells used in the beam cross section with the SECDATA command in a command object under the line body and, like you see improper results displays. I think Mechanical expects 2 X 2 cell beam cross section, and it isn't written in such a way as to accomodate other possibilities.  One thing that might help is to set the display displacement scaling to zero:

You could also try a post processing command object - have MAPDL solver create static images of the beam results. First, before solving, request that the MAPDL db file be saved:

 

Next, insert a command object under the solution branch such as this one:

finish 
/clear 
resume 
 
/view,1,3,1,3
/graphics,power
/eshape,1
 
/post1 
set,last 
 
/show,png 
plns,s,x 
/show,close
 
 
You can access the image by clicking on "Post Output" under the command object in the tree:
 
 
Note that SX is the stress in the direction of the axis of the element (direct + bending stress) - even if the beam axis is not aligned with the global x axis. The appearance of the displayed stress distribution will be much like that you'd see if you were using solid elements.
 
Related to (though admittedly not directly addressing)  your question about shear stress output... one way to specify transverse shear stiffness is with the SECCONTROL command:
 
 
I hope this helps,
Bill