In this post I would like to share the modeling and analysis of a structural knee joint. This type of joint is common in column-girder connections. The hollow section I am using (S235 steel 250x100x5 mm) is commercially available.
I will use solid elements and hope to compare the results in a future post to what is obtained with shell elements. Of particular interest are the differences in FreeCAD modeling approach between solids and shells and the results in terms of von Mises stresses and Equivalent Plastic Strains.
The first figure show the mesh and boundary conditions for the knee joint. I will in a few steps explain how this model was set up.
As can be seen from the model panel to the left, the model is built up from 4 simple blocks. Both tubular sections are created by cutting 2000x240x90 mm blocks out of 2000x250x100 mm blocks. To create a continues hollow joint the side wall of the column is then cut with the inner block of the girder and the girder wall is cut with the inner block of the column. So the two internal blocks are used in four cutting operations. Finally all cuts are combined in a BooleanFragments object with mode set to CompSolid.
A mesh is created with min/max sizes of 5 and 100 mm, respectively. In addition I created 2 mesh regions (side faces of joint @ 50 mm and sharp corner edge + vertices @ 5 mm)
The bottom of the column is fully fixed and the girder is loaded by a force of 14 kN pointing at the column base. I chose this direction to make the knee joint the most heavily loaded part in bending.
Elastic Analysis Results
The tip deflection under the load is approximately 11 mm and the von Mises stress at the sharp corner is 656 MPa, which is much higher than the 235 MPa yield stress of the material. Later in this post I will show that IMHO this is of no great concern.
A cut view of the joint shows that the peak stress is caused by the girder bottom flange pressing up against the stiff web of the column.
Plastic Analysis Results
As discussed in another post (https://forum.freecadweb.org/viewtopic.php?f=24&t=26921
), a plastic analysis can be used to judge joint strength and ductility beyond first yield. For that purpose a non-linear material object is added with the following material properties:
Sig_yield = 235MPa @ Eps_plastic = 0.00
Sig_yield_2 = 238.4MPa @ Eps_plastic = 0.02
Sig_yield_ult = 360MPa @ Eps_plastic = 0.20
The results of the analysis shows that the peak von Mises stress has reduced from 656 MPa to 273 MPa at the expense of an increased yield area. This value is much lower than the ultimate stress of 360 MPa for S235 steel.
As mentioned in my other post, the result of the plastic analysis may be accepted if the plastic strains are relatively small, the joint is statically loaded and if no local buckling of the web occurs. Although this analysis includes full geometric non-linearity, I would still recommend a linear buckling analysis is performed to assess the buckling load.
I also reviewed the maximum von Mises stress and Equivalent Plastic strain in the DAT file. Again, significant differences are observed (273 MPa in the FRD file and 235.6 MPa in the DAT file). As explained before, this is due to the extrapolation and averaging that takes place in the FRD nodal results. In any event the integration point results in the DAT file are consistent (Sig_vM=235.6 MPa and PEEQ=0.00360 mm/mm) and well within acceptable levels.