Thanks again @FEAnalyst
I agree another test with reference results would help, but I really thought this tensile coupon (dog ears shape) was simple enough to start withā¦
I will check with a simple constant-section rectangular plate, and compare with analytical solution. But it would be good to fully understand why such large differences between Calculix and Abaqus, with very similar dimensions / mesh / load / BC.
when no reference solution available, usually solid element model is used since itās the most accurate ones. Iām only look based on several screenshot and results, Abaqus shell composite results are underestimate and CalculiX composite shell is overestimated, both are less accurate. However, refine the mesh in CalculiX composite shell result is closed to solid models. Some reason commonly from stress in thickness direction and shear transfer distribution in each layer.
Thatās why I propose another benchmark with a reference solution. Here, we donāt know the correct value and both Abaqus and CalculiX can be wrong due to insufficient discretization (likely in-plane since even if we add more integration points in the thickness direction, they can still be too far from the filletās surface). I can try different element types (including solids and continuum shells) and refined mesh in that area in Abaqus. I will also have a look at averaging.
We should use full integration second-order solids for that (while composites in CalculiX need S8R), but with the current mesh density, C3D20 elements in CalculiX donāt help.
@FEAnalyst
I followed your advice, and prepare a new test case to compare between ABQ and Calculix, using NAFEMS benchmarks (three-point bending test).
Problem is that my Abaqus model does not give the expected reference results. I should have something wrong in my model but do not see what.
I also followed this guide:
Could you please help me ?
Here are the ācaeā and āinpā files zip).
NAFEMS_three-point-bending_ABAQUS.zip (86.6 KB)
Here is the NAFEMS description :
(we should expect about 1mm of U3 deflection at max)
Try the input file provided in the Abaqus documentation for this benchmark: http://130.149.89.49:2080/v2016/books/bmk/default.htm?startat=ch04s09anf81.html
You could import it in Abaqus/CAE and then recreate it there (even including the geometry) if you want. Or convert the input deck for use in CalculiX if needed.
Many thanks.
I was then able to see my error (I did not applied Simpsonās distribution rule for load force values on nodes).