FEM – Rectangular Hollow Section Knee Joint

Show off your FreeCAD projects here!
User avatar
HarryvL
Posts: 1042
Joined: Sat Jan 06, 2018 7:38 pm

FEM – Rectangular Hollow Section Knee Joint

Postby HarryvL » Mon Mar 12, 2018 10:14 pm

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.


RHS_Knee_Joint_Solid_1.png
RHS_Knee_Joint_Solid_1.png (228.15 KiB) Viewed 2961 times


Boolean Fragments

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.

FEMMeshGmsh

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)

Boundary conditions

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.


RHS_Knee_Joint_Elastic_Def_Mises.png
RHS_Knee_Joint_Elastic_Def_Mises.png (289.92 KiB) Viewed 2961 times


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.


RHS_Knee_Joint_Elastic_Mises_Cut_1.png
RHS_Knee_Joint_Elastic_Mises_Cut_1.png (306.86 KiB) Viewed 2961 times


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.


RHS_Knee_Joint_Plastic_Mises_Cut_1.png
RHS_Knee_Joint_Plastic_Mises_Cut_1.png (338.21 KiB) Viewed 2961 times


Further Discussion

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.
Last edited by HarryvL on Thu Mar 29, 2018 6:20 am, edited 1 time in total.
thschrader
Posts: 1407
Joined: Sat May 20, 2017 12:06 pm
Location: Germany

Re: FEM – Rectangular Hollow Section Knee Joint

Postby thschrader » Tue Mar 13, 2018 5:12 pm

Hi Harry,
thanks for the uge amount of work and the explanations you give.
I have problems to interpret the PEEQ-value. What does the PEEQ mean?
What is an acceptble value lets say for S235?
Thomas
User avatar
HarryvL
Posts: 1042
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM – Rectangular Hollow Section Knee Joint

Postby HarryvL » Tue Mar 13, 2018 6:23 pm

Hi Thomas,

PEEQ is Calculix (Abaqus) shorthand for Equivalent Plastic Strain. Like von Mises stress is a measure for stress intensity, so is the equivalent plastic strain a measure for plastic strain intensity. Both allow generalisation of the stress - (plastic) strain curve from a tensile test to general stress-strain conditions. In fact for the tensile test both quantities simplify to the uni-axial stress and (plastic) strain, respectively. The von Mises stress and Equivalent Plastic Strain are related by a (kinematic) hardening rule, i.e. Sig_vM = F (PEEQ). This function F is actually what you specify in the FreeCAD Nonlinear Material Object and that's why you can check if the output is in line with the input (which it is at integration points, but not at the nodes ... see my posts).

So what is an acceptable PEEQ? Well, there are many scientific papers on this, but for me the simple engineering answer is: stay really far away from the failure strain in an uni-axial tensile test, which is 0.1-0.2 mm/mm for ductile structural steel (the higher the steel grade, the lower the ultimate strain). I would not go higher than, say 0.05 mm/mm and only if the load is predominantly static.

I can recommend DNV-RP-C208 for guidance on the use of non-linear FEA in structural design.

Anyway, what I hope to demonstrate in the posts (apart from that FreeCAD is a great tool for conceptual design !!) is that elasto-plastic FEA gives a rational basis for structural design. For static loading, it does away with the debate about stress concentrations. In an elastic analysis mesh refinement gives ever growing stress concentrations and leads to a paradox in that the designer is punished for using a more accurate model. Not so in a elasto-plastic analysis.

Harry
User avatar
HarryvL
Posts: 1042
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM – Rectangular Hollow Section Knee Joint

Postby HarryvL » Wed Mar 14, 2018 5:21 am

... and here a picture to show that the spread of the plastic zone (PEEQ>0) is still quite limited

RHS_Knee_Joint_PEEQ.png
RHS_Knee_Joint_PEEQ.png (269.84 KiB) Viewed 2722 times
User avatar
HarryvL
Posts: 1042
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM – Rectangular Hollow Section Knee Joint

Postby HarryvL » Wed Mar 14, 2018 5:56 am

... and a linear buckling analysis shows that the buckling load is 30.2*14 kN = 423 kN, far in excess of the applied load.

RHS_Knee_Joint_Buckling.png
RHS_Knee_Joint_Buckling.png (43.38 KiB) Viewed 2691 times

I will do a non-linear buckling analysis next, taking into account initial deformations. factored from the linear buckling analysis. This to show the final step in a full set of design analyses.
Last edited by HarryvL on Mon Apr 02, 2018 9:00 am, edited 1 time in total.
User avatar
HarryvL
Posts: 1042
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM – Rectangular Hollow Section Knee Joint

Postby HarryvL » Thu Mar 15, 2018 12:25 am

To conclude this case study, I present here the results for a fully non-linear analysis with an initial imperfection based on the first linear buckling mode presented above. I very conservatively scaled the first buckling mode up to give a maximum of 17.5 mm "out-of-flatness" of the joint faces (i.e. the buckles shown above). Such a large initial imperfection would be very visible in the structure and most certainly not be accepted during construction.

The maximum tip displacements under a 14 kN load is up from the 11 mm we found in the original analysis (with perfectly flat joint faces) to approximately 13 mm. The maximum plastic strain has increased by a factor 3 to approximately 0.01.

RHS_Knee_Joint_NL_Buckling_14kN_(2).png
RHS_Knee_Joint_NL_Buckling_14kN_(2).png (70.64 KiB) Viewed 2547 times

When the load is further increased to 30 kN, the tip displacement increases to 32 mm and the plastic strain comes close to the 0.05 mm/mm limit I stated earlier.

RHS_Knee_Joint_NL_Buckling_30kN_(1).png
RHS_Knee_Joint_NL_Buckling_30kN_(1).png (75.06 KiB) Viewed 2547 times

IMHO the large deformations and large plastic strains indicate that the ultimate strength of the joint has been reached.
User avatar
HarryvL
Posts: 1042
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM – Rectangular Hollow Section Knee Joint

Postby HarryvL » Mon Apr 02, 2018 9:13 am

Please note that I updated the above posts to correct for an error in elastic buckling load. Also note that the lateral sway of the frame is prevented (like in a building frame). If this is not the case (like for a lifting davit), a lateral sway buckling mode would dominate.
User avatar
bernd
Posts: 8232
Joined: Sun Sep 08, 2013 8:07 pm
Location: Zürich, Switzerland

Re: FEM – Rectangular Hollow Section Knee Joint

Postby bernd » Tue Apr 03, 2018 5:06 am

All this is very cools stuff. You should make some tutorial out of this. Have you tried shell meshes too?
User avatar
HarryvL
Posts: 1042
Joined: Sat Jan 06, 2018 7:38 pm

Re: FEM – Rectangular Hollow Section Knee Joint

Postby HarryvL » Tue Apr 03, 2018 5:12 am

Thanks. Not yet. Next on the program :D

Happy to do a few tutorials, but guess I should focus more on the FC/CCX workflow than the "engineering physics".
Jee-Bee
Posts: 1942
Joined: Tue Jun 16, 2015 10:32 am
Location: Netherlands

Re: FEM – Rectangular Hollow Section Knee Joint

Postby Jee-Bee » Tue Apr 03, 2018 5:29 am

HarryvL wrote:
Tue Apr 03, 2018 5:12 am
Happy to do a few tutorials, but guess I should focus more on the FC/CCX workflow than the "engineering physics".
for me on both :D