I am running a case on prepomax, using the geometry that was used in one off the tutorials for a simply supported beam by FEA Analyst on yt, with the following dimensions, the length is 2000mm, b = 140mm and t = 200mm. I am applying a UDL of w = 1000N/m on this and using steel with a Young’s Modulus of 190GPa.
Using the formula for maxiumum deflection in a UDL cantilever ( delta = -wL^4/8EI), I got a value of 0.11278mm, and when I did the same in prepomax, I got a value of 0.1027mm, which seems to be fine. What raises concern is that the maximum stress predicted by thhe simution in only 3.28Mpa, whereas using the classic beam theory, the maximum stress seems to be 2.14MPa.(not 4.28 as I had forgotten earlier to take distance as L/2 for moment)
I have attached my .pmx file below and was hoping if someone could take a look and tell me if i am doing something wrong. The file I have attached has very course mesh compared to what i used for it but the upload requirement made it coarse.
You should check the S33 stress (normal). Refine the mesh and take the boundary condition into account. To compare with the von Mises stress, you would have to calculate it for your analytical results too. There are simple formulas for this.
Hi, I have seen your private mail. I’m posting in the general so anyone could benefit if they find it usefull. FEAnalyst is completely right.
Note classical beam theory formulas do not consider Poisson ratio effects. It should be zero or BC should take care that no additional transverse compressive stresses are pressent. This is a common error when comparing with clasical formulas.
To check your BC are suitable for comparision, look at maximum and minimum longitudinal tensile and compressive stress at both ends of suporting area. They should be equal in absolute values. Ideally the same as maximum and minimum principal stresses (absolute values).
By other hand, you can reach an additional “pro” accuracy in the comparision by taking the Shear deflection into consideration. .
Edited:
This would be my set up using Plane Stress Compliant material model to get rid of szz and speed up the analisys.
Hi, can you elaborate on what you mean by taking boundary conditions into account? i am doing a cantilever, so does fixing a face and applying a surface traction not adequately represent the system?
edit: I want to ask regarding S33. I think of S33 as the stress normal with the plane being along z axis and the force being applied normally to it. Is this correct ? Like normally I would assume when I see S33, to be that the area vector of a plane would point in the z axis, and not the plane to be aligned with it, but since I am using bending formula which will calculate stress along the neutral axis, I get confused. Could you help clear this doubt?
Fixed BC is not very realistic and causes artificial stress concentrations. There are some blog posts that show this using cantilever beam example. It’s also discussed here: Cantilever beam with load at one end
Check the cross-section diagrams showing stresses in beams. They are common in books for strength of materials and represent this stress distribution pretty well.
I intend to measure strain on a beam by pasting a strain gauge on top of the beam. Now essentially that would mean calculating the strain along the red line right. So the red line is essentially the plane I want to calculate my strain on, from a vertical force downwards. so the strain value I should be looking at is E22 then right? since the normal vector of this plane points in y direction and the force is also in the y direction
.
