I am using Calculix to analyze a simple frame model with guided supports meshed with beam elements. I have access to Abaqus so I can check if both solutions are equal. Running the exact same input file, gives different results in abaqus and calculix. I solved the problem analytically and the correct solution is the one from Abaqus.
Is there anything that I need to add to the Calculix input file to get the same results?
beam element in CalculiX may differs with Abaqus since it expanded to solid element. your models are using two nodes B21 linear element which expanded to C3D8I and prone of locking (one element through thickness), try using three nodes B32 quadratic element to reduced large discrepancy compared to classical beams.
Thank you! I was not aware that the elements were expanded to solid elements. I scaled the pressure load to take into account that it is distributed through the solid face, and noth through the length. I tried changing the elements to B32 but the results still differ slightly.
You may need to refine the CCX mesh further the Abaqus to get convergence.
Beware there are various bugs/errors with beams, including external force output, section force output, non-homogenous boundary conditions, and point forces. You have to tip-toe around checking your results often. Sometimes one beam element type is OK but another is not.
I wouldn’t bother using the 2D B21 unless all your work is going to be 2D because you never know if the behavior is the same as the 3D beams or not and will have to start testing everything again from scratch. B32R seems to be generally the best beam element in both my experience and recommended in the manual.