Simulate Early, Simulate Often... In Rhino
I am trying to model a plate with uniform pressure and simply suppported at its four edges.
So I create the plate 2000x1000x25 mm, put the pressure load and restrain the two consecutive edges in x, y and z directions and the other two edges just in z direction.
I get a strange result in which the dflection is like the plate moves paralell in opposite direction to load pressure.
I tried different linear edge restrain arragemet and loads (pressure, scaler)
Does any one have an idea if I am using linear edge restrains incorrectly?
I am also seeing that behavior here. I don't have an explanation, but I suspect a bug. I will let you know what I find.
Thank you for pointing out this bug.
I found the source of the trouble and corrected it. Download the latest version (18.104.22.168) from here and let me know if it works better.
I can see that the wrong effect happens no more.
Solid 6016 Aluminium plate, 15 mm. 2000x1000 mm plate under 0.0132 MPa pressure. Supported on two linear edges X, Y, Z restricted and other two just Z restricted (four linear edges).
Two comments about results:
1- SnS Z displacement is 1,6 mm. I have checked this with analythics and FEA program and both values match on 6,2/6,4 mm
2- When I look at YY stress, the maximum value appears near the edges (happens the same with XX stress) which is not reasonable except the boundary condition would include some clamping effect, which would be in line with the reduced deflection. (checked maximium value for YY stress should be at the centre in the range of 32 MPa).
I would thank some explanation.
Edge restraints are inherently non-physical (stress= force/area, area=zero), so I'm always skeptical of the stress results in their neighborhood. That said, I too am also seeing the odd "clamping" behavior, which suggests a bug of some sort. I am looking into it.
A workaround would be to restrain the vertical faces in Z, which will allow small rotations. For numerical stability, you'll also need restraints in X and Y. Apply an X-restraint on one of the vertical faces running in the X-direction, and a Y-restraint on one of the faces running in the Y-direction. This is about as close as you can get, notwithstanding resolution limits inherent in such a thin part.
I have checked like you suggested and result are 5.2 mm for deflection and 25,6 MPa for sigma YY, which is in line with other calculations.
Nevertheless it might be a little bit tricky to predict when the boundary conditions are working correctly.
I encourage you to improve linear edges. Many boundary conditions in reality are simply supported.
Thank you anyway for your interest.