Hello everyone,

I am trying to calculate max Equilent Stress on my beam shape structual and for that i tried to used 2 diffrent methods. At first I deifne my structual as beam elemnt and fixed from one joint point and applied my force (4444 N) from other joint point. As you can see from the docs and screenshoots Equilent Stress was near 128 MPa which is very close wit analytical calculations (M*C/I)= 114 MPa. However if i try to simulate my strucatal as Solid , and give fixation and force to faces, Stress data changes dramticly and become 305 MPa and URES data changes too and this data depends of mesh's rate, it gets higher with mesh's rate gets higher. But Most importantly if I use Iso cliping and probe the locations of high stress areas, as shown at screenshot, I see that stress descress very fast and the stress over the yeild of stell (235 MPa) its continue only for 1-2 mm . not even thickness of plate.

So here is my question, which method i should depend and assume the right solition. or is there a problem with fixation corners, a numerical difficualty which makes stress values diverges . Is there a way i can make validation. I assume its a problem most of us dealing with. I am waiting your responds . Thanks.

But Most importantly if I use Iso cliping and probe the locations of high stress areas, as shown at screenshot, I see that stress descress very fast and the stress over the yeild of stell (235 MPa) its continue only for 1-2 mm . not even thickness of plate.

So here is my question, which method i should depend and assume the right solition. or is there a problem with fixation corners, a numerical difficualty which makes stress values diverges .

Yup, you are correct. Your peak stress of 305 MPa is due to numerical issues; more specifically, stress singularities. What is happening is that at the surface that you're applying your fixed constraint to, you have an infinite discontinuity in the stiffness of the structure. If you start from the free end of the beam and move towards the fixed end, the stiffness of the structure is defined by the Young's and Shear Modulus. However, once you get to the surface that your constraint is applied on, your structure is infinitely stiff. This issue is innate to the finite element method, and the best method of handling it is to increase the number of elements near the constraint and see what value the stresses converge to at locations just past the constraint (a distance about 2-3% of the total length of the beam). As you've already seen, as you decrease the size of your mesh, your stress values becomes higher. Some of these increases are real, and the refined mesh is converging to the "true" stresses. However, the stresses at the constraint (the singular locations) are not "true", and will increase to infinity if you were to continue to refine your mesh.

To answer another question of yours, beam elements are good if your structure is long and slender (like a beam! ) and give you an overall structural performance (displacement shape under load, modes of vibration, overall stress, etc.); they are also very efficient from a computations standpoint.. However, they won't give you the higher level of detail that you might need (stresses at joints, stresses around holes in your structure, etc.); for that you'll need solid elements (or potentially shell elements, depending on your geometry and analysis goals).