Stuck? 
support@mecway.com
support@mecway.com
Mecway
FEA
Top and bottom stresses comparison for a simply supported beam (1D, 2D & 3D)
Hello,
I am trying to understand how stresses work in Mecway ( I usually use only bending moment / shear forces & deflection information from a model ). My goal is to use tension stress information from a model in order to predict if a certain concrete zone is prone to cracking or not (disregarding reinforcement). Usually if the tensile stress is bigger than 3MPa ( let's assume it as tensile strength for concrete ), then that area might crack.
In order to understand how stresses develop, I assumed a concrete plank 5m long, simply supported each end and uniformly loaded. I used 3 models in order to analyze it: a linear member, a surface and a volume ( see attached files ). I used Euler - Bernoulli beam formula to derive the top and bottom stress ( maximum compression and tension ) in the middle of the plank, corresponding to the maximum bending moment. The analysis is only linear-elastic for all 3 cases.
The numbers are very close to the ones derived from the formulas for the 1D & 2D models. The problem is that I cannot get the same max/min stress in the third ( volumetric ) model. If the 1D & 2D models, the stress is around 9.399 MPa (almost matching the formula from the PDF) , I think I am doing something wrong in the third one, because the deflection is 4.2mm instead of 14mm and maximum stresses are very low. The plank looks like is deflecting correctly, but the values are way too different from the other 2 models and the ones generated by the classical formulas. I checked to have the same dimensions, loads, material properties between all three models and 'simply supported' behavior, but there is something that I probably missed in the volumetric one?!
Any idea what is wrong and how can I get the same min/max stress in the middle of the plank as predicted by Euler - Bernoulli formula for the third model?
Thank you.
I am trying to understand how stresses work in Mecway ( I usually use only bending moment / shear forces & deflection information from a model ). My goal is to use tension stress information from a model in order to predict if a certain concrete zone is prone to cracking or not (disregarding reinforcement). Usually if the tensile stress is bigger than 3MPa ( let's assume it as tensile strength for concrete ), then that area might crack.
In order to understand how stresses develop, I assumed a concrete plank 5m long, simply supported each end and uniformly loaded. I used 3 models in order to analyze it: a linear member, a surface and a volume ( see attached files ). I used Euler - Bernoulli beam formula to derive the top and bottom stress ( maximum compression and tension ) in the middle of the plank, corresponding to the maximum bending moment. The analysis is only linear-elastic for all 3 cases.
The numbers are very close to the ones derived from the formulas for the 1D & 2D models. The problem is that I cannot get the same max/min stress in the third ( volumetric ) model. If the 1D & 2D models, the stress is around 9.399 MPa (almost matching the formula from the PDF) , I think I am doing something wrong in the third one, because the deflection is 4.2mm instead of 14mm and maximum stresses are very low. The plank looks like is deflecting correctly, but the values are way too different from the other 2 models and the ones generated by the classical formulas. I checked to have the same dimensions, loads, material properties between all three models and 'simply supported' behavior, but there is something that I probably missed in the volumetric one?!
Any idea what is wrong and how can I get the same min/max stress in the middle of the plank as predicted by Euler - Bernoulli formula for the third model?
Thank you.
Howdy, Stranger!
It looks like you're new here. If you want to get involved, click one of these buttons!
Comments
The pivot point of the compression only support is not at the end of the beam where the other constraints are. You can see this in the deformed view. That makes it not really a simple support. To correct this, remove the X displacement constraint from one end so it's free to move longitudinally as it rotates. The effective length of the beam will still be slightly too short though.
The mesh is too coarse. Hex8 elements with the internal solver need a fine mesh because they are over-stiff in bending. They're so inefficient that you shouldn't really ever use them. Change to hex20 with Mesh tools -> Change element shape and add the new midside nodes to the constraints. Whatever elements you use, check for mesh convergence by solving at several different mesh densities to avoid such errors.
Not really a problem but compression only support isn't necessary here. It's slower to solve and makes it hard to predict where the support point will end up being. Use displacement in the Z direction instead.
Yes, you were right, it worked. My assumption was that using a simple-support on 'z' direction would restrict the corners of the blank from lifting 'naturally', so a 'compression-only' approach made more sense. Anyway, thank you for your time!