For some reason,my model's result have very high concetrated stress at the corner(s). Originally, I thought it's because I have nodal constraints that's fixed, I have changed it to no rotation, and still received the same problems in the results.
The model is parameter is only gravity and pressure (in a small area); with linear static analysis...
I have 2 forces applied, one's 63kips and the other is about 73kips; I do expect high stress near where I applied the load, but not at the boundary of the model about 10' away.
Does anyone have the similar problem? if so, how'd you solve it?
Solved! Go to Solution.
Welcome to the world of FEA (Finite Element Analysis).
I assume that you have a brick model, and by writing "I have changed it to no rotation", I assume you mean that you unchecked Rx Ry Rz for the constraints. In the real world, there is no such thing as a rotational constraint, and so brick elements ignore Rx Ry Rz constraints. "Fixed" constraints (Tx Ty Tz Rx Ry Rz all checked) and "No Translation" (Tx Ty Tz all checked) result in the same type of constraint. (If you literally used "No Rotation" (Rx Ry Rz all checked) and you have a brick model, then you have no support at those nodes!).
Regardless of the type of constraints you have, you do have forces or moments at the constraints: the reaction forces. So this is what is causing the high stresses. If you were to refine the mesh at the constraints, I think you would find that the stress concentration always occurs either at the constraint or 1 node away from the constraint. It is partly an artifact of the mathematical approach, so you can ignore the high stresses.
A realistic estimate of the stress can be obtained by extrapolating the stress using a couple of the nodes outside of the stress concentration zone. If you select a series of nodes along a line leading up to the constraint in the Results environment, then right-click and choose "Create Path Plot", you can do the extrapolation visually.
Simulation Mechanical user since Dec 1997
Thank you so much for your reply and help!! I checked Rx, Ry & Rz for my boundary condition, leaving the translations unchecked. The boundary condition is applied to the plate and beams only.. The brick elements have loads applied to simulate loading pattern. Stress value at that location is obviously expected
I will certainly refine my mesh a bit more at the edges and try again, if the values are still abnormally high, I'll write it up in the report as mathimatical approach of the program.
I really do appreciate your help!
Thanks so much!
Hard to say anything specific without screenshots , but in a linear static stress increase in concentrators (ie corners with fixing) is quite common. Reducing the elements size in the field of concentration can lead to even higher stresses.
If you want fix this abnormal situation, you can either change objectives formulation - for example boundary conditions, or by using nonlinear material.